Introduction
This manual describes how to carry out Mitsubishi Electric CNC programming. Supported models are as follows:
Abbreviations in this manual are as follows:
This manual describes programming, therefore, read this manual thoroughly before using this NC system. To ensure safe use of this NC system, thoroughly study the "Precautions for Safety" on the following page before using this NC system. Be sure to always keep this manual on hand so that users can refer to it at any time.
Details described in this manual
The description concerning "Signals" in the main text refers to information transmission between a machine and PLC or between NC and PLC. The method for controlling the signals (ON/OFF) differs depending on the machine. Refer to the manual issued by the machine tool builder (MTB). Some parameters can be used by end-users and some parameters are set by the MTB according to the specifications. End-users may not be able to set or change some of the parameters described as "... can be set with the parameter #XXXX" in the main text. Confirm the specifications for your machine with the manual issued by the MTB.
CAUTION
For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by the machine tool builder (MTB) takes precedence over this manual.
Items not described in this manual must be interpreted as "not possible".
This manual is written on the assumption that all the applicable functions are included. Some of them, however, may not be available for your NC system. Refer to the specifications issued by the machine tool builder before use.
Refer to the Instruction Manual issued by the MTB for details regarding each machine tool.
Some screens, functions, and the number of digits may differ depending on the NC system (or its version), and some functions may not be available. Please confirm the specifications before use.
To protect the availability, integrity and confidentiality of the NC system against cyber-attacks including unau- thorized access, denial-of-service (Dos) (*1) attack, and computer virus from external sources via a network, take security measures such as firewall, VPN, and anti-virus software. (*1) Denial-of-service (Dos) refers to a type of cyber-attack that disrupts services by overloading the system or
by exploiting a vulnerability of the system.
Mitsubishi Electric assumes no responsibility for any problems caused to the NC system by any type of cyber- attacks including DoS attack, unauthorized access and computer virus.
In this manual, the following abbreviations might be used. L system: Lathe system M system: Machining center system MTB: Machine tool builder
Also refer to the manuals on "Manual List" as necessary.
Supported models Details
M800W Series M850W, M830W M800S Series M850S, M830S M80W Series M80W M80 Series M80 TypeA, M80 TypeB E80 Series E80 TypeA, E80 TypeB C80 Series C80
Abbreviations Supported models
M800, M800 Series M800W Series/M800S Series M80, M80 Series M80 Series/M80W Series M800/M80, M800/M80 Series M800W Series/M800S Series/M80W Series/M80 Series M8, M8 Series M800W Series/M800S Series/M80W Series/M80 Series/E80 Series
Manual List
Manuals related to M800/M80/E80/C80 Series are listed as follows. These manuals are written on the assumption that all optional functions are added to the targeted model. Some functions or screens may not be available depending on the machine or specifications set by MTB. (Confirm the specifications before use.) The manuals issued by MTB take precedence over these manuals.
Manual IB No. Purpose and Contents M800/M80/E80 Series Instruction Manual IB-1501274
Operation guide for NC Explanation for screen operation, etc.
C80 Series Instruction Manual IB-1501453
Operation guide for NC Explanation for screen operation, etc.
M800/M80/E80/C80 Series Programming Manual (Lathe System) (1/2)
IB-1501275 G code programming for lathe system Basic functions, etc.
M800/M80/E80/C80 Series Programming Manual (Lathe System) (2/2)
IB-1501276 G code programming for lathe system Functions for multi-part system, high-accuracy function, etc.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
IB-1501277 G code programming for machining center system Basic functions, etc.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
IB-1501278 G code programming for machining center system Functions for multi-part system, high-accuracy function, etc.
M800/M80/E80 Series Alarm/Parameter Manual IB-1501279
Alarms Parameters
C80 Series Alarm/Parameter Manual IB-1501560
Alarms Parameters
Manuals for MTBs (NC)
Manuals for MTBs (drive section)
Manual IB No. Purpose and Contents M800/M80/E80/C80 Series Specifications Manual (Function) IB-1501505
Model selection Outline of various functions
M800/M80/E80/C80 Series Specifications Manual (Hardware) IB-1501506
Model selection Specifications of hardware unit
M800W/M80W Series Connection and Setup Manual IB-1501268
Detailed specifications of hardware unit Installation, connection, wiring, setup (startup/adjustment)
M800S/M80/E80 Series Connection and Setup Manual IB-1501269
Detailed specifications of hardware unit Installation, connection, wiring, setup (startup/adjustment)
C80 Series Connection and Setup Manual IB-1501452
Detailed specifications of hardware unit Installation, connection, wiring, setup (startup/adjustment)
M800/M80/E80 Series PLC Development Manual IB-1501270
Electrical design I/O relation (assignment, setting, connection), field network Development environment (PLC on-board, peripheral
development environment), etc.
M800/M80/E80 Series PLC Programming Manual IB-1501271
Electrical design Sequence programming PLC support functions, etc.
M800/M80/E80/C80 Series PLC Interface Manual IB-1501272
Electrical design Interface signals between NC and PLC
M800/M80/E80 Series Maintenance Manual IB-1501273
Cleaning and replacement for each unit Other items related to maintenance
C80 Series Maintenance Manual IB-1501454
Cleaning and replacement for each unit Other items related to maintenance
Manual IB No. Contents MDS-E/EH Series Specifications Manual IB-1501226 Specifications for power supply regeneration type
MDS-E/EH Series Instruction Manual IB-1501229 Instruction for power supply regeneration type
MDS-EJ/EJH Series Specifications Manual IB-1501232 Specifications for regenerative resistor type
MDS-EJ/EJH Series Instruction Manual IB-1501235 Instruction for regenerative resistor type
MDS-EM/EMH Series Specifications Manual IB-1501238 Specifications for multi-hybrid, power supply regeneration
type MDS-EM/EMH Series Instruction Manual IB-1501241 Instruction for multi-hybrid, power supply regeneration type
DATA BOOK IB-1501252 Specifications of servo drive unit, spindle drive unit, motor, etc.
Manuals for MTBs (Others)
For M800/M80/E80 Series
Manual No. Purpose and Contents GOT2000 Series Users Manual (Hardware) SH-081194 Outline of hardware such as part names, external dimensions,
installation, wiring, maintenance, etc. of GOTs GOT2000 Series Users Manual (Utility) SH-081195 Outline of utilities such as screen display setting, operation
method, etc. of GOTs GOT2000 Series Users Manual (Monitor) SH-081196 Outline of each monitor function of GOTs
GOT2000 Series Connection Manual (Mitsubishi Electric Products)
SH-081197 Outline of connection types and connection method between GOT and Mitsubishi Electric connection devices
GT Designer3 (GOT2000) Screen Design Manual SH-081220 Outline of screen design method using screen creation
software GT Designer3
Manual No. Purpose and Contents GOT2000/GOT1000 Series CC-Link Communication Unit User's Manual IB-0800351 Explanation for handling CC-Link communication unit (for
GOT2000 series/GOT1000 series) GX Developer Version 8 Operating Manual (Startup) SH-080372E Explanation for system configuration, installation, etc. of PLC
development tool GX Developer GX Developer Version 8 Operating Manual SH-080373E Explanation for operations using PLC development tool GX
Developer GX Converter Version 1 Operating Manual IB-0800004E Explanation for operations using data conversion tool GX
Converter
GX Works2 Installation Instructions BCN-P5999-0944 Explanation for the operating environment and installation method of GX Works2
GX Works2 Version 1 Operating Manual (Common) SH-080779ENG
Explanation for the system configuration of GX Works2 and the functions common to Simple project and Structured project such as parameter setting, operation method for the online function
GX Works2 Version 1 Operating Manual (Simple Project) SH-080780ENG Explanation for methods for such as creating and monitoring
programs in Simple project of GX Works2 GX Works2 Version 1 Operating Manual (Simple Project, Function Block)
SH-080984ENG Explanation for methods for such as creating function blocks,
pasting function blocks to sequence programs, and operating FB library in Simple project of GX Works2
GX Works2 Version 1 Operating Manual (Structured Project) SH-080781ENG Explanation for methods for such as creating and monitoring
programs in Structured project of GX Works2
GX Works3 Installation Instructions BCN-P5999-0391 Explanation for the operating environment and installation method of GX Works3
MELSEC-Q CC-Link System Master/ Local Module Users Manual SH-080394E Explanation for system configuration, installation, wiring, etc.
of master/local modules for CC-Link system GOT2000 Series Connection Manual (Non-Mitsubishi Electric Products 1)
SH-081198ENG Explanation for connection types and connection method
between GOT and other company's devicesGOT2000 Series Connection Manual (Non-Mitsubishi Electric Products 2)
SH-081199ENG
GOT2000 Series Connection Manual (Microcomputers, MODBUS/ Fieldbus Products, Peripherals)
SH-081200ENG Explanation for connection types and connection method
between GOT and microcomputers, MODBUS/fieldbus products, peripherals
GT SoftGOT2000 Version1 Operating Manual SH-081201ENG
Explanation for system configuration, screen configuration and operation method of monitoring software GT SoftGOT2000
For C80 Series
Reference Manual for MTBs
Manual No. Purpose and Contents MELSEC iQ-R Module Configuration Manual SH-081262 Outline of system configuration, specifications, installation,
wiring, maintenance, etc. MELSEC iQ-R CPU Module Users Manual (Startup) SH-081263 Outline of specifications, procedures before operation,
troubleshooting, etc. for CPU module MELSEC iQ-R CPU Module Users Manual (Application) SH-081264 Outline of memory, functions, devices, parameters, etc. for
CPU module MELSEC iQ-R CC-Link IE Field Network User's Manual (Application) SH-081259 Explanation for functions, parameter settings, programming,
troubleshooting, etc. of the CC-Link IE Field Network function QCPU Users Manual (Hardware Design, Maintenance and Inspection)
SH-080483 Outline of specifications, necessary knowledge to configure
the system and maintenance-related descriptions for Q series CPU module, etc.
GX Works3 Operating Manual SH-081215 Outline of functions, programming, etc.
Manual No. Purpose and Contents M800/M80 Series Smart safety observation Specification manual BNP-C3072-022
Explanation for smart safety observation function C80 Series Smart safety observation Specification manual BNP-C3077-022
M800/M80 Series CC-Link (Master/ Local) Specification manual BNP-C3072-089 Explanation for CC-Link
M800/M80 Series PROFIBUS-DP Specification manual BNP-C3072-118 Explanation for PROFIBUS-DP communication function
M800/M80 Series Interactive cycle insertion (Customization) Specification manual
BNP-C3072-121- 0003 Explanation for interactive cycle insertion
M800/M80 Series EtherNet/IP Specifications manual BNP-C3072-263 Explanation for EtherNet/IP
M800/M80 Series CC-Link IE Field (Master/local) Specifications manual BNP-C3072-283 Explanation for CC-Link IE Field
M800/M80 Series GOT Connection Specifications manual BNP-C3072-314 Explanation for GOT connection
M800/M80 Series CC-Link IE Field Basic Specifications manual BNP-C3072-337 Explanation for CC-Link IE Field Basic
M800/M80 Series FL-net Specifications manual BNP-C3072-368 Explanation for FL-net
M800/M80 Series Synchronous Control Specifications manual BNP-C3072-074 Explanation for synchronous control
M800/M80 Series Multiple-Axis Synchronization Control Specifications manual
BNP-C3072-339 Explanation for multiple-axis synchronization control
Precautions for Safety
Always read the specifications issued by the machine tool builder, this manual, related manuals and attached documents be- fore installation, operation, programming, maintenance or inspection to ensure correct use. Understand this numerical controller, safety items and cautions before using the unit. This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".
Note that even items ranked as " CAUTION", may lead to major results depending on the situation. In any case, important in- formation that must always be observed is described. The following signs indicate prohibition and compulsory.
The meaning of each pictorial sign is as follows.
Mitsubishi Electric CNC is designed and manufactured solely for applications to machine tools to be used for industrial purpos- es. Do not use this product in any applications other than those specified above, especially those which are substantially influential on the public interest or which are expected to have significant influence on human lives or properties.
Not applicable in this manual.
DANGER When the user may be subject to imminent fatalities or major injuries if handling is mistaken.
WARNING When the user may be subject to fatalities or major injuries if handling is mistaken.
CAUTION When the user may be subject to injuries or when physical damage may occur if handling is mistaken.
This sign indicates prohibited behavior (must not do). For example, indicates "Keep fire away".
This sign indicated a thing that is pompously (must do). For example, indicates "it must be grounded".
CAUTION
CAUTION
rotated object CAUTION HOT
Danger
Electric shock risk
Danger
explosive
Prohibited
Disassembly is
prohibited
KEEP FIRE AWAY
General instruction
Earth ground
For Safe Use
DANGER
1. Items related to operation If the operation start position is set in a block which is in the middle of the program and the program is started, the program before the set block is not executed. Please confirm that G and F modal and coordinate values are appropriate. If there are coordinate system shift commands or M, S, T and B commands before the block set as the start position, carry out the required commands using the MDI, etc. If the program is run from the set block without carrying out these operations, there is a danger of interference with the machine or of machine operation at an unexpected speed, which may result in breakage of tools or machine tool or may cause damage to the operators. Under the constant surface speed control (during G96 modal), if the axis targeted for the constant surface speed control (normally X axis for a lathe) moves toward the spindle center, the spindle rotation speed will increase and may exceed the allowable speed of the workpiece or chuck, etc. In this case, the workpiece, etc. may jump out during machining, which may result in breakage of tools or machine tool or may cause damage to the operators.
1. Items related to product and manual For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by the machine tool builder takes precedence over this manual. Items not described in this manual must be interpreted as "not possible". This manual is written on the assumption that all the applicable functions are included. Some of them, however, may not be available for your NC system. Refer to the specifications issued by the machine tool builder before use. Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool. Some screens and functions may differ depending on the NC system (or its version), and some functions may not be pos- sible. Please confirm the specifications before use. To protect the availability, integrity and confidentiality of the NC system against cyber-attacks including unauthorized ac- cess, denial-of-service (Dos) (*1) attack, and computer virus from external sources via a network, take security measures such as firewall, VPN, and anti-virus software. (*1) Denial-of-service (Dos) refers to a type of cyber-attack that disrupts services by overloading the system or by exploiting
a vulnerability of the system. Mitsubishi Electric assumes no responsibility for any problems caused to the NC system by any type of cyber-attacks in- cluding DoS attack, unauthorized access and computer virus.
2. Items related to operation Before starting actual machining, always carry out graphic check, dry run operation and single block operation to check the machining program, tool offset amount, workpiece compensation amount and etc. If the workpiece coordinate system offset amount is changed during single block stop, the new setting will be valid from the next block. Turn the mirror image ON and OFF at the mirror image center. If the tool offset amount is changed during automatic operation (including during single block stop), it will be validated from the next block or blocks onwards. Do not make the synchronized spindle rotation command OFF with one workpiece chucked by the reference spindle and synchronized spindle during the spindle synchronization. Failure to observe this may cause the synchronized spindle stop, and hazardous situation.
WARNING
CAUTION
3. Items related to programming The commands with "no value after G" will be handled as "G00". ";" "EOB" and "%" "EOR" are expressions used for explanation. The actual codes are: For ISO: "CR, LF", or "LF" and "%". Programs created on the Edit screen are stored in the NC memory in a "CR, LF" format, but programs created with external devices such as the FLD or RS-232C may be stored in an "LF" format. The actual codes for EIA are: "EOB (End of Block)" and "EOR (End of Record)". When creating the machining program, select the appropriate machining conditions, and make sure that the performance, capacity and limits of the machine and NC are not exceeded. The examples do not consider the machining conditions. Do not change fixed cycle programs without the prior approval of the machine tool builder. When programming the multi-part system, take special care to the movements of the programs for other part systems. The program including a character of any language other than the display language is not correctly displayed. Do not edit such a program. Any part of the program other than the comment part may also be changed if edited.
CAUTION
Disposal
(Note) This symbol mark is for EU countries only. This symbol mark is according to the directive 2006/66/EC Article 20 Information for end-users and Annex II.
Your MITSUBISHI ELECTRIC product is designed and manufactured with high quality materials and components which can be recycled and/or reused. This symbol means that batteries and accumulators, at their end-of-life, should be disposed of separately from your household waste. If a chemical symbol is printed beneath the symbol shown above, this chemical symbol means that the battery or accumulator contains a heavy metal at a certain concentration. This will be indicated as follows: Hg: mercury (0,0005%), Cd: cadmium (0,002%), Pb: lead (0,004%) In the European Union there are separate collection systems for used batteries and accumulators. Please, dispose of batteries and accumulators correctly at your local community waste collection/recycling centre.
Please, help us to conserve the environment we live in!
Trademarks
MELDAS, MELSEC, EZSocket, EZMotion, iQ Platform, MELSEC iQ-R, MELSOFT, GOT, CC-Link, CC-Link/LT, CC-Link IE, CC-Link IE/field, EcoMonitorLight and SLMP are either trademarks or registered trademarks of Mitsubishi Electric Corporation in Japan and/or other countries.
Ethernet is a registered trademark of Xerox Corporation in the United States and/or other countries. Microsoft, Windows, SQL Server and Access are either trademarks or registered trademarks of Microsoft Corporation in the United States and/or other countries. SD logo and SDHC logo are either registered trademarks or trademarks of LLC. UNIX is a registered trademark of The Open Group in the United States and/or other countries. Intel and Pentium are either trademarks or registered trademarks of Intel Corporation in the United States and/or other countries. MODBUS is either a trademark or a registered trademark of Schneider Electric USA, Inc. or the affiliated companies in Japan and/or other countries. EtherNet/IP is a trademark of Open DeviceNet Vendor Association,Inc. PROFIBUS-DP and PROFINET are either trademarks of Profibus International. Oracle is a registered trademark of Oracle Corporation, the subsidiaries, or the affiliated companies in the United States and /or other countries. VNC is a registered trademark of RealVNC Ltd. in the United States and other countries. Punchtap is licensed by EMUGE.
Other company and product names that appear in this manual are trademarks or registered trademarks of the respective companies.
( /Japanese)
( A)
Handling of our product
(English) This is a class A product. In a domestic environment this product may cause radio interference in which case the user may be required to take adequate measures.
( /Korean)
(A )
.
Contents
Chapter 1 - 14 : Refer to Programming Manual (Machining Center System) (1/2)
Chapter 15 and later : Refer to Programming Manual (Machining Center System) (2/2)
1 Control Axes................................................................................................................................................. 1 1.1 Coordinate Words and Control Axes ........................................................................................................................ 2 1.2 Coordinate Systems and Coordinate Zero Point Symbols ....................................................................................... 3
2 Minimum Command Unit............................................................................................................................. 5 2.1 Input Setting Unit and Program Command Unit ....................................................................................................... 6 2.2 Input Command Increment Tenfold .......................................................................................................................... 7 2.3 Indexing Increment ................................................................................................................................................... 8
3 Program Formats ......................................................................................................................................... 9 3.1 Program Format...................................................................................................................................................... 10 3.2 File Format.............................................................................................................................................................. 14 3.3 Optional Block Skip................................................................................................................................................. 17
3.3.1 Optional Block Skip; / ..................................................................................................................................... 17 3.3.2 Optional Block Skip Addition ; /n .................................................................................................................... 19
3.4 G Code ................................................................................................................................................................... 21 3.4.1 Modal, Unmodal ............................................................................................................................................. 21 3.4.2 G Code Lists .................................................................................................................................................. 21
3.5 Precautions before Starting Machining................................................................................................................... 26
4 Pre-read Buffer ........................................................................................................................................... 27 4.1 Pre-read Buffer ....................................................................................................................................................... 28
5 Position Commands .................................................................................................................................. 29 5.1 Position Command Methods ; G90,G91 ................................................................................................................. 30 5.2 Diameter Designation and Radius Designation ...................................................................................................... 32
5.2.1 Diameter/Radius Designation Switch; G10.9 ................................................................................................. 32 5.3 Inch/Metric Conversion; G20, G21 ......................................................................................................................... 35 5.4 Decimal Point Input................................................................................................................................................. 37
6 Interpolation Functions ............................................................................................................................. 45 6.1 Positioning (Rapid Traverse); G00 ......................................................................................................................... 46 6.2 Linear Interpolation; G01 ........................................................................................................................................ 49 6.3 Circular Interpolation; G02, G03 ............................................................................................................................. 51 6.4 R Specification Circular Interpolation; G02, G03 .................................................................................................... 57 6.5 Plane Selection; G17, G18, G19 ............................................................................................................................ 60 6.6 Thread Cutting ........................................................................................................................................................ 62
6.6.1 Constant Lead Thread Cutting; G33 .............................................................................................................. 62 6.6.2 Inch Thread Cutting; G33............................................................................................................................... 66
6.7 Helical Interpolation; G02, G03............................................................................................................................... 68 6.8 Unidirectional Positioning ....................................................................................................................................... 73
6.8.1 Unidirectional Positioning; G60 ...................................................................................................................... 73 6.8.2 Axis-based Unidirectional Positioning ............................................................................................................ 75
6.9 Cylindrical Interpolation; G07.1............................................................................................................................... 76 6.10 Circular Cutting; G12,G13 .................................................................................................................................... 83 6.11 Polar Coordinate Interpolation; G12.1, G13.1/G112, G113.................................................................................. 85 6.12 Exponential Interpolation; G02.3, G03.3............................................................................................................... 92 6.13 Polar Coordinate Command; G16 ........................................................................................................................ 99 6.14 Spiral/Conical Interpolation; G02.1/G03.1 (Type 1), G02/G03 (Type 2)............................................................. 106 6.15 3-dimensional Circular Interpolation; G02.4, G03.4............................................................................................ 110 6.16 NURBS Interpolation; G06.2............................................................................................................................... 116 6.17 Hypothetical Axis Interpolation; G07................................................................................................................... 122 6.18 Involute Interpolation; G02.2/G03.2.................................................................................................................... 124
7 Feed Functions......................................................................................................................................... 137 7.1 Rapid Traverse Rate............................................................................................................................................. 138
7.1.1 Rapid Traverse Rate .................................................................................................................................... 138 7.1.2 G00 Feedrate Command (,F Command) ..................................................................................................... 139
7.2 Cutting Feedrate ................................................................................................................................................... 143 7.3 F1-digit Feed......................................................................................................................................................... 144 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed); G94,G95 .............................. 146 7.5 Inverse Time Feed; G93 ....................................................................................................................................... 148 7.6 Feedrate Designation and Effects on Control Axes.............................................................................................. 153 7.7 Selection of Axis (Axes) for Feedrate Command; G130....................................................................................... 158 7.8 Rapid Traverse Constant-gradient Acceleration/Deceleration.............................................................................. 162 7.9 Rapid Traverse Constant-gradient Multi-step Acceleration/Deceleration ............................................................. 168 7.10 Cutting Feed Constant-gradient Acceleration/Deceleration................................................................................ 176 7.11 Exact Stop Check; G09 ...................................................................................................................................... 184 7.12 Exact Stop Check Mode; G61 ............................................................................................................................ 188 7.13 Deceleration Check ............................................................................................................................................ 189
7.13.1 Deceleration Check.................................................................................................................................... 189 7.13.2 Deceleration Check When Movement in the Opposite Direction Is Reversed ........................................... 197
7.14 Rapid Traverse Block Overlap; G0.5 P1............................................................................................................. 200 7.14.1 Rapid Traverse Block Overlap for G00; G0.5 ............................................................................................ 202 7.14.2 Rapid Traverse Block Overlap for G28 ...................................................................................................... 210
7.15 Automatic Corner Override ................................................................................................................................. 212 7.15.1 Automatic Corner Override ; G62............................................................................................................... 219 7.15.2 Inner Arc Override...................................................................................................................................... 220
7.16 Tapping Mode; G63 ............................................................................................................................................ 221 7.17 Cutting Mode; G64.............................................................................................................................................. 222
8 Dwell.......................................................................................................................................................... 223 8.1 Dwell (Time-based Designation); G04.................................................................................................................. 224
9 Miscellaneous Functions ........................................................................................................................ 227 9.1 Miscellaneous Functions (M8-digits) .................................................................................................................... 228 9.2 Second Miscellaneous Functions (A8-digits, B8-digits or C8-digits) .................................................................... 230 9.3 Index Table Indexing ............................................................................................................................................ 231
10 Spindle Functions .................................................................................................................................. 237 10.1 Spindle Functions ............................................................................................................................................... 238 10.2 Constant Surface Speed Control; G96, G97 ...................................................................................................... 239 10.3 Spindle Clamp Speed Setting; G92 .................................................................................................................... 246 10.4 Spindle Position Control (Spindle/C Axis Control) .............................................................................................. 248 10.5 Spindle Speed Fluctuation Detection; G162/G163 ............................................................................................. 256
11 Tool Functions (T command)................................................................................................................ 263 11.1 Tool Functions (T8-digit BCD) ............................................................................................................................ 264
12 Tool Compensation Functions ............................................................................................................. 265 12.1 Tool Compensation............................................................................................................................................. 266
12.1.1 Tool Compensation .................................................................................................................................... 266 12.1.2 Number of Tool Offset Sets Allocation to Part Systems............................................................................. 270
12.2 Tool Length Compensation/Cancel; G43, G44 / G49 ......................................................................................... 272 12.3 Tool Radius Compensation; G38,G39/G40/G41,G42 ........................................................................................ 280
12.3.1 Tool Radius Compensation Operation ....................................................................................................... 281 12.3.2 Other Commands and Operations during Tool Radius Compensation...................................................... 290 12.3.3 G41/G42 Commands and I, J, K Designation ............................................................................................ 300 12.3.4 Interrupts during Tool Radius Compensation............................................................................................. 306 12.3.5 General Precautions for Tool Radius Compensation................................................................................. 308 12.3.6 Changing of Compensation No. during Compensation Mode.................................................................... 309 12.3.7 Start of Tool Radius Compensation and Z Axis Cut in Operation .............................................................. 312 12.3.8 Interference Check..................................................................................................................................... 314 12.3.9 Diameter Designation of Compensation Amount ....................................................................................... 324 12.3.10 Workpiece Coordinate Changing during Radius Compensation.............................................................. 326
12.4 Tool Nose Radius Compensation (for Machining Center System) ..................................................................... 328 12.5 3-dimensional Tool Radius Compensation; G40/G41, G42................................................................................ 331 12.6 Tool Position Offset; G45 to G48........................................................................................................................ 343
13 Fixed Cycle ............................................................................................................................................. 351 13.1 Fixed Cycles ....................................................................................................................................................... 352
13.1.1 Drilling, Spot Drilling; G81 .......................................................................................................................... 356 13.1.2 Drilling, Counter Boring; G82 ..................................................................................................................... 357
13.1.3 Deep Hole Drilling Cycle; G83 ................................................................................................................... 358 13.1.3.1 Deep Hole Drilling Cycle ................................................................................................................... 358 13.1.3.2 Small Diameter Deep Hole Drilling Cycle.......................................................................................... 360
13.1.4 Tapping Cycle; G84 ................................................................................................................................... 363 13.1.5 Boring; G85................................................................................................................................................ 378 13.1.6 Boring; G86................................................................................................................................................ 379 13.1.7 Back Boring; G87....................................................................................................................................... 380 13.1.8 Boring; G88................................................................................................................................................ 384 13.1.9 Boring; G89................................................................................................................................................ 385 13.1.10 Stepping Cycle; G73 ................................................................................................................................ 386 13.1.11 Reverse Tapping Cycle; G74 ................................................................................................................... 388 13.1.12 Circular Cutting; G75................................................................................................................................ 390 13.1.13 Fine Boring; G76 ...................................................................................................................................... 392 13.1.14 Thread Milling Cycle; G187...................................................................................................................... 394 13.1.15 Punchtap Cycle ........................................................................................................................................ 398 13.1.16 Precautions for Using a Fixed Cycle ........................................................................................................ 411 13.1.17 Initial Point and R Point Level Return; G98, G99..................................................................................... 413 13.1.18 Setting of Workpiece Coordinates in Fixed Cycle Mode .......................................................................... 414 13.1.19 Drilling Cycle High-Speed Retract............................................................................................................ 415 13.1.20 Acceleration/Deceleration Mode Change in The Fixed Cycle for Drilling................................................. 419
13.2 Special Fixed Cycle ............................................................................................................................................ 421 13.2.1 Bolt Hole Cycle; G34.................................................................................................................................. 422 13.2.2 Line at Angle; G35 ..................................................................................................................................... 423 13.2.3 Arc; G36..................................................................................................................................................... 424 13.2.4 Grid; G37.1................................................................................................................................................. 425
13.3 Fixed Cycle for Turning Machining ..................................................................................................................... 427 13.3.1 Longitudinal Cutting Cycle; G174............................................................................................................... 428 13.3.2 Thread Cutting Cycle; G175....................................................................................................................... 431 13.3.3 Face Cutting Cycle; G176.......................................................................................................................... 435
14 Macro Functions .................................................................................................................................... 439 14.1 Subprogram Control; M98, M99, M198 .............................................................................................................. 440
14.1.1 Subprogram Call; M98, M99 ...................................................................................................................... 440 14.1.2 Subprogram Call; M198 ............................................................................................................................. 446 14.1.3 Figure Rotation; M98 I_J_K_ ..................................................................................................................... 447
14.2 Variable Commands ........................................................................................................................................... 450 14.3 User Macro ......................................................................................................................................................... 455 14.4 Macro Call Instructions ....................................................................................................................................... 456
14.4.1 Simple Macro Calls; G65 ........................................................................................................................... 456 14.4.2 Modal Call A (Movement Command Call) ; G66 ....................................................................................... 460 14.4.3 Modal Call B (for Each Block); G66.1 ........................................................................................................ 462 14.4.4 G Code Macro Call..................................................................................................................................... 464 14.4.5 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call) .................................................... 466 14.4.6 Detailed Description for Macro Call Instruction .......................................................................................... 468 14.4.7 ASCII Code Macro ..................................................................................................................................... 470
14.5 Variables Used in User Macros .......................................................................................................................... 474 14.5.1 Common Variables..................................................................................................................................... 476 14.5.2 Local Variables (#1 to #33) ........................................................................................................................ 477 14.5.3 System Variables ....................................................................................................................................... 480
14.6 User Macro Commands...................................................................................................................................... 481 14.6.1 Operation Commands ................................................................................................................................ 481 14.6.2 Control Commands .................................................................................................................................... 486 14.6.3 External Output Commands; POPEN, PCLOS, DPRNT............................................................................ 492 14.6.4 Precautions ................................................................................................................................................ 496 14.6.5 Actual Examples of Using User Macros..................................................................................................... 498
14.7 Macro Interruption; M96, M97............................................................................................................................. 502
15 Program Support Functions ................................................................................................................. 513 15.1 Corner Chamfering I/Corner Rounding I ............................................................................................................. 514
15.1.1 Corner Chamfering I ; G01 X_ Y_ ,C ......................................................................................................... 514 15.1.2 Corner Rounding I ; G01 X_ Y_ ,R_........................................................................................................... 516 15.1.3 Corner Chamfering Expansion/Corner Rounding Expansion..................................................................... 518 15.1.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ..................................................... 520
15.2 Corner Chamfering II/Corner Rounding II ........................................................................................................... 521 15.2.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_....................................................................................... 521 15.2.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_ .......................................................................................... 523 15.2.3 Corner Chamfering Expansion/Corner Rounding Expansion..................................................................... 524 15.2.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ..................................................... 524
15.3 Linear Angle Command; G01 X_/Y_ A_/,A_....................................................................................................... 525 15.4 Geometric I; G01 A_ ........................................................................................................................................... 526 15.5 Geometric IB....................................................................................................................................................... 528
15.5.1 Geometric IB (Automatic Calculation of Contact Point of Two Circular Arcs); G02/G03 P_Q_ /R_........... 529 15.5.2 Geometric IB (Automatic Calculation of Intersection Point between Line And Circular Arc) ;
G01 A_ , G02/G03 P_Q_H_ ...................................................................................................................... 531 15.5.3 Geometric IB (Automatic Calculation of Contact Point between Line And Circular Arc) ; G01 A_ , G02/G03 R_H_ ... 534
15.6 Mirror Image by G code ; G50.1,G51.1 .............................................................................................................. 536 15.7 Normal Line Control; G40.1/G41.1/G42.1 (G150/G151/G152)........................................................................... 540 15.8 Manual Arbitrary Reverse Run Prohibition ; G127.............................................................................................. 560 15.9 Data Input by Program........................................................................................................................................ 566
15.9.1 Parameter Input by Program; G10 L70, G11 ............................................................................................. 566 15.9.2 Compensation Data Input by Program (Tool Compensation Amount) ; G10 L10/L11/L12/L13, G11 ........ 568 15.9.3 Compensation Data Input by Program (Workpiece Offset Amount) ; G10 L2/L20, G11............................ 571 15.9.4 Compensation Data Input by Program (Turning Tool) ; G10 L12/L13, G11............................................... 575 15.9.5 Tool Shape Input by Program; G10 L100, G11.......................................................................................... 577 15.9.6 R-Navi Data Input by Program; G10 L110/L111, G11, G68.2, G69........................................................... 580
15.10 Tool Life Management ...................................................................................................................................... 584 15.10.1 Inputting the Tool Life Management Data by G10 L3 Command; G10 L3, G11 ...................................... 584 15.10.2 Inputting the Tool Life Management Data by G10 L30 Command; G10 L30, G11 .................................. 587 15.10.3 Precautions for Inputting the Tool Life Management Data....................................................................... 590 15.10.4 Allocation of the Number of Tool Life Management Sets to Part Systems .............................................. 591
15.11 Interactive Cycle Insertion; G180...................................................................................................................... 593 15.11.1 Interactive Cycle Insertion........................................................................................................................ 593 15.11.2 Interactive Macro...................................................................................................................................... 596
15.12 Axis Name Extension........................................................................................................................................ 597 15.13 Machining Interruption [C80]; G26.................................................................................................................... 603
16 Multi-part System Control ..................................................................................................................... 619 16.1 Timing Synchronization Operation...................................................................................................................... 620
16.1.1 Timing Synchronization Operation (! code) !n (!m ...) L ............................................................................. 620 16.1.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115 ...................................... 623 16.1.3 Timing Synchronization Operation with Start Point Designated (Type 2) ; G116 ...................................... 626 16.1.4 Timing Synchronization Operation Function Using M codes ; M*** ........................................................... 629 16.1.5 Timing Synchronization When Timing Synchronization Ignore Is Set........................................................ 633
16.2 Mixed Control...................................................................................................................................................... 636 16.2.1 Arbitrary Axis Exchange ; G140, G141, G142 ........................................................................................... 636
16.3 Sub Part System Control .................................................................................................................................... 639 16.3.1 Sub Part System Control I; G122.............................................................................................................. 639
17 High-speed High-accuracy Control ...................................................................................................... 655 17.1 High-speed Machining Mode .............................................................................................................................. 656
17.1.1 High-speed Machining Mode I, II; G05 P1, G05 P2................................................................................... 656 17.2 High-accuracy Control ........................................................................................................................................ 665
17.2.1 High-accuracy Control ; G61.1, G08 .......................................................................................................... 665 17.2.2 SSS Control ............................................................................................................................................... 686 17.2.3 Tolerance Control....................................................................................................................................... 690 17.2.4 Variable-acceleration Pre-interpolation Acceleration/Deceleration ............................................................ 694 17.2.5 Initial High-accuracy Control ...................................................................................................................... 697 17.2.6 Multi-part System Simultaneous High-accuracy ........................................................................................ 698
17.3 High-speed High-accuracy Control ..................................................................................................................... 700 17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0.................. 700 17.3.2 Fairing ........................................................................................................................................................ 717 17.3.3 Smooth Fairing........................................................................................................................................... 718 17.3.4 Cutting Speed Clamp with Acceleration Rate Judgment ........................................................................... 727 17.3.5 High-speed Mode Corner Deceleration...................................................................................................... 728 17.3.6 Precautions on High-speed High-accuracy Control ................................................................................... 729
17.4 Spline Interpolation ; G05.1 Q2/Q0..................................................................................................................... 732 17.5 Spline Interpolation 2; G61.4 .............................................................................................................................. 740 17.6 High-accuracy Spline Interpolation ; G61.2 ........................................................................................................ 749 17.7 Machining Condition Selection I ; G120.1, G121................................................................................................ 751
18 Advanced Multi-Spindle Control Function .......................................................................................... 755 18.1 Spindle Synchronization ..................................................................................................................................... 756
18.1.1 Spindle Synchronization I; G114.1............................................................................................................. 757 18.1.2 Spindle Position Control (Spindle/C Axis Control) under Spindle Synchronization Control ....................... 769
18.2 Tool Spindle Synchronization I ........................................................................................................................... 774 18.2.1 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon) ; G114.2, G113.1 ........................................ 774 18.2.2 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon) ; G51.2/G50.2 or G251/G250 ..................... 780 18.2.3 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon) ; G51.2/G50.2 or G251/G250 .................... 785
18.3 Tool Spindle Synchronization II .......................................................................................................................... 789 18.3.1 Tool Spindle Synchronization II (Hobbing) ; G114.3/G113 ........................................................................ 789
18.4 Multiple Spindle Synchronization Set Control [C80] ........................................................................................... 802
19 Advanced Machining Control ............................................................................................................... 807 19.1 Tool Position Compensation; G43.7/G49 ........................................................................................................... 808 19.2 Tool Length Compensation Along the Tool Axis; G43.1/G49 ............................................................................. 815 19.3 Tool Center Point Control; G43.4, G43.5/G49.................................................................................................... 822
19.3.1 Circular Command in Tool Center Point Control (G43.4/G43.5)................................................................ 854 19.4 Inclined Surface Machining; G68.2, G68.3/G69 ................................................................................................. 858
19.4.1 How to Define Feature Coordinate System Using Euler Angles ................................................................ 860 19.4.2 How to Define Feature Coordinate System Using Roll-Pitch-Yaw Angles................................................. 862 19.4.3 How to Define Feature Coordinate System Using Three Points in a Plane ............................................... 864 19.4.4 How to Define Feature Coordinate System Using Two Vectors ................................................................ 866 19.4.5 How to Define Feature Coordinate System Using Projection Angles ........................................................ 868 19.4.6 Define by Selecting the Registered Machining Surface ............................................................................. 870 19.4.7 How to Define Feature Coordinate System Using Tool Axis Direction ...................................................... 871 19.4.8 Tool Axis Direction Control; G53.1/G53.6 .................................................................................................. 873 19.4.9 Details of Inclined Surface Machining Operation ....................................................................................... 881 19.4.10 Rotary Axis Basic Position Selection ....................................................................................................... 886 19.4.11 Relationship between Inclined Surface Machining and Other Functions ................................................. 892 19.4.12 Precautions for Inclined Surface Machining............................................................................................. 897
19.5 3-dimensional Tool Radius Compensation (Tool's Vertical-direction Compensation); G40/G41.2, G42.2......... 900 19.6 Workpiece Installation Error Compensation; G54.4............................................................................................ 911 19.7 Rotation Center Error Compensation (Precautions for Creating a Machining Program) .................................... 924 19.8 Applicable Machines........................................................................................................................................... 928
20 Coordinate System Setting Functions ................................................................................................. 931 20.1 Coordinate Words and Control Axes .................................................................................................................. 932 20.2 Types of Coordinate Systems............................................................................................................................. 933
20.2.1 Basic Machine, Workpiece and Local Coordinate Systems....................................................................... 933 20.2.2 Machine Zero Point and 2nd, 3rd, 4th Reference Position (Zero Point) .................................................... 934 20.2.3 Automatic Coordinate System Setting ....................................................................................................... 935 20.2.4 Coordinate System for Rotary Axis ............................................................................................................ 936
20.3 Basic Machine Coordinate System Selection; G53 ............................................................................................ 939 20.4 Coordinate System Setting; G92 ........................................................................................................................ 942 20.5 Local Coordinate System Setting; G52............................................................................................................... 944 20.6 Workpiece Coordinate System Selection and Extended Workpiece Coordinate System Selection;
G54 to G59, G54.1 ............................................................................................................................................. 948 20.7 Workpiece Coordinate System Preset; G92.1 .................................................................................................... 956 20.8 Workpiece Position Offset for Rotary Axis ; G54.2 ............................................................................................. 961 20.9 3-dimensional Coordinate Conversion; G68/G69 ............................................................................................... 973 20.10 Coordinate Rotation by Program; G68/G69...................................................................................................... 991 20.11 Coordinate Rotation Input by Parameter; G10 I_ J_/K_ ................................................................................. 1000 20.12 Scaling; G50/G51 ........................................................................................................................................... 1017 20.13 Reference Position (Zero Point) Return; G28, G29 ........................................................................................ 1021 20.14 2nd, 3rd, and 4th Reference Position (Zero Point) Return ; G30.................................................................... 1025 20.15 Tool Change Position Return; G30.1 - G30.6................................................................................................. 1028 20.16 Reference Position Check; G27 ..................................................................................................................... 1031
21 Protection Function ............................................................................................................................. 1033 21.1 Stroke Check before Travel; G22/G23 ............................................................................................................. 1034
21.1.1 Stroke Check before Travel in Stored Stroke Limit Area ......................................................................... 1036 21.2 Enable Interfering Object Selection Data; G186............................................................................................... 1039
22 Measurement Support Functions ....................................................................................................... 1043 22.1 Automatic Tool Length Measurement; G37 ...................................................................................................... 1044 22.2 Skip Function; G31 ........................................................................................................................................... 1048 22.3 Multi-step Skip Function 1; G31.n, G04............................................................................................................ 1054 22.4 Multi-step Skip Function 2; G31 P .................................................................................................................... 1056 22.5 Speed Change Skip; G31 Fn............................................................................................................................ 1058 22.6 Torque Limitation Skip; G160 ........................................................................................................................... 1062 22.7 Programmable Current Limitation; G10 L14 ..................................................................................................... 1066
23 System Variables ................................................................................................................................. 1067 23.1 System Variables List ....................................................................................................................................... 1068 23.2 System Variables (G Command Modal) ........................................................................................................... 1070 23.3 System Variables (Non-G Command Modal) ................................................................................................... 1071 23.4 System Variables (Modal Information at Macro Interruption) ........................................................................... 1072 23.5 System Variables (Tool Information) ................................................................................................................ 1074 23.6 System Variables (Tool Compensation) ........................................................................................................... 1082 23.7 System Variables (Tool Life Management)....................................................................................................... 1083 23.8 System Variables (Workpiece Coordinate Offset) ............................................................................................ 1088 23.9 System Variables (Workpiece Position Offset Amount for Rotary Axis) ........................................................... 1089 23.10 System Variables (Extended Workpiece Coordinate Offset) .......................................................................... 1090 23.11 System Variables (External Workpiece Coordinate Offset) ............................................................................ 1091 23.12 System Variables (Position Information)......................................................................................................... 1092 23.13 System Variables (Alarm) ............................................................................................................................... 1096 23.14 System Variables (Message Display and Stop).............................................................................................. 1097 23.15 System Variables (Cumulative Time) ............................................................................................................. 1098 23.16 System Variables (Time Read Variables)....................................................................................................... 1099 23.17 System Variables (Machining Information) ..................................................................................................... 1101 23.18 System Variables (Reverse Run Information) ................................................................................................ 1102 23.19 System Variables (Number of Workpiece Machining Times) ......................................................................... 1102 23.20 System Variables (Mirror Image) .................................................................................................................... 1102 23.21 System Variables (Coordinate Rotation Parameter)....................................................................................... 1103 23.22 System Variables (Rotary Axis Configuration Parameter) .............................................................................. 1104 23.23 System Variables (Normal Line Control Parameter)....................................................................................... 1105 23.24 System Variables (Parameter Reading) ......................................................................................................... 1106 23.25 System Variables (Workpiece Installation Error Compensation Amount)....................................................... 1110 23.26 System Variables (Macro Interface Input (PLC -> NC)).................................................................................. 1111 23.27 System Variables (Macro Interface Output (NC -> PLC))............................................................................... 1117 23.28 System Variables (R Device Access Variables) ............................................................................................. 1123 23.29 System Variables (PLC Data Reading) .......................................................................................................... 1129 23.30 System Variables (Interfering Object Selection) ............................................................................................. 1133 23.31 System Variables (ZR Device Access Variables) [C80] ................................................................................. 1136 23.32 System Variables (NC Data Reading/Writing with API Section and Sub-section Nos. Input/Output by Program) [M8] ... 1138
24 Appx.1: Fixed Cycles ........................................................................................................................... 1141
25 Appx.2: Command Value Range Lists ............................................................................................... 1147
1
1 IB-1501277-P
Control Axes
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
1 Control Axes
2IB-1501277-P
1Control Axes 1.1 Coordinate Words and Control Axes
The number of control axes is set to "3" in the standard specifications; however, up to eight axes can be controlled if an additional axis is added. To specify each machining direction, use alphabetical coordinate words that are pre- defined appropriately.
Function and purpose
X-Y table
X-Y and rotating table
+Z
+Z
+Y
+Y
+X
+X
Program coordinates
Direction of table movement
Workpiece
Table
Bed
+Z +Y
+Y
+C
+C
+X +X Program coordinates
Direction of table movement Direction of table
revolution
Workpiece
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
1 Control Axes
3 IB-1501277-P
1.2 Coordinate Systems and Coordinate Zero Point Symbols
The basic machine coordinate system is the coordinate system that expresses the position (tool change position, stroke end position, etc.) that is specific to the machine. Workpiece coordinate systems are used for workpiece machining. Upon completion of the dog-type reference position return, the parameters are referred and the basic machine co- ordinate system and workpiece coordinate systems (G54 to G59) are automatically set. The offset of the basic machine coordinate zero point and reference position is set by a parameter. (Normally, set by MTB) Workpiece coordinate systems can be set with coordinate systems setting functions, workpiece coordinate offset measurement (additional specification), and etc.
Reference position: A specific position to establish coordinate systems and change tools
Basic machine coordinate zero point: A position specific to machine
Workpiece coordinate zero points (G54 to G59) A coordinate zero point used for workpiece machining
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
1 Control Axes
4IB-1501277-P
The local coordinate systems (G52) are valid on the coordinate systems designated by workpiece coordinate sys- tems 1 to 6. Using the G92 command, the basic machine coordinate system can be shifted and made into a hypothetical ma- chine coordinate system. At the same time, workpiece coordinate systems 1 to 6 are also shifted.
Reference position
Basic machine coordinate zero point
Workpiece coordinate zero points
Local coordinate zero point
Offset set by a parameter
Offset set by a program ("0" is set when turning the power ON)
G52 Local coordinate system offset (*1) G54 Workpiece coordinate (G54) system offset (*1) G55 Workpiece coordinate (G55) system offset G92 G92 Coordinate system shift EXT External workpiece coordinate offset
(*1) G52 offset is independently possessed by G54 to G59 respectively.
G52
G92
G55G54
EXT
G52
2
5 IB-1501277-P
Minimum Command Unit
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
2 Minimum Command Unit
6IB-1501277-P
2Minimum Command Unit 2.1 Input Setting Unit and Program Command Unit
The input setting units are the units of setting data including tool compensation amounts and workpiece coordinates compensation. The program command units are the units of movement amounts in programs. These are expressed with mm, inch or degree ().
Program command units for each axis and input setting units, common for all axes, are determined by the setting of parameters as follows. (This depends on the MTB specifications.)
(1) Inch/metric changeover can be handled by either a parameter screen (#1041 I_inch: valid only when the power is turned ON) or G commands (G20 or G21). However, the changeover by a G command applies only to the program command units, and not to the input setting units. Consequently, the tool offset amounts and other compensation amounts as well as the variable data should be preset in order to correspond to input setting units.
(2) The millimeter and inch systems cannot be used together. (3) When performing a circular interpolation between the axes whose program command units are different, the cen-
ter command (I, J, K) and the radius command (R) are designated by the input setting units. (Use a decimal point to avoid confusion.)
Function and purpose
Detailed description
Parameter Linear axis Rotary axis ()
Metric Inch
Input setting unit #1003 iunit = B 0.001 0.0001 0.001 = C 0.0001 0.00001 0.0001 = D 0.00001 0.000001 0.00001 = E 0.000001 0.0000001 0.000001
Program command unit (Input command unit)
#1015 cunit = 0 Follow #1003 iunit = 1 0.0001 0.00001 0.0001 = 10 0.001 0.0001 0.001 = 100 0.01 0.001 0.01 = 1000 0.1 0.01 0.1 = 10000 1.0 0.1 1.0
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
2 Minimum Command Unit
7 IB-1501277-P
2.2 Input Command Increment Tenfold
The program's command increment can be multiplied by an arbitrary scale with the parameter designation. This function is valid when a decimal point is not used for the command increment. The scale is set with the parameter "#8044 UNIT*10".
(1) When running a machining program already created with a 10m input command increment with a CNC unit for which the command increment is set to 1m and this function's parameter value is set to "10", this function en- ables the same machining as the original program.
(2) When running a machining program already created with a 1m input command increment with a CNC unit for which the command increment is set to 0.1m and this function's parameter value is set to "10", this function enables the same machining as the original program.
(3) This function cannot be used for the dwell function G04_X_(P_);.
(4) This function cannot be used for the compensation amount of the tool compensation input.
(5) This function can be used when decimal point type I is valid, but cannot be used when decimal point type II is valid.
(6) This function cannot be used for a tool shape setting command (in G10L100 format).
Function and purpose
Detailed description
Program example (Machining program : programmed with 1=10m)
(CNC unit is 1=1m system)
"UNIT*10" parameter
10 1
X Y X Y N1 G90 G00 X0 Y0; 0 0 0 0 N2 G91 X-10000 Y-15000; -100.000 -150.000 -10.000 -15.000 N3 G01 X-10000 Y-5000 F500; -200.000 -200.000 -20.000 -20.000 N4 G03 X-10000 Y-10000 J-10000; -300.000 -300.000 -30.000 -30.000 N5 X10000 Y-10000 R10000; -200.000 -400.000 -20.000 -40.000 N6 G01 X20.000 Y20.000 -180.000 -380.000 0.000 -20.000
UNIT*10 ON UNIT*10 OFF
N1
N2
N3
N4
N5
R
-400
-300
-200
-100
W
-100-200-300
N6
N1
N2
N3
N4
N5
R
-40
-30
-20
-10
W
-10-20-30
N6
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
2 Minimum Command Unit
8IB-1501277-P
2.3 Indexing Increment
This function limits the command value for the rotary axis. This can be used for indexing the rotary table, etc. It is possible to cause a program error with a program command other than an indexing increment (parameter setting value).
When the indexing increment (parameter) which limits the command value is set, the rotary axis can only be posi- tioned with that indexing increment. If a program other than the indexing increment setting value is commanded, a program error (P20) will occur. The indexing position will not be checked when the parameter is set to 0.
(Example) When the indexing increment setting value is 2 degrees, the machine coordinate position at the end point can only be commanded with the 2-degree increment.
The following axis specification parameter is used. (This depends on the MTB specifications.)
(1) When the indexing increment is set, positioning will be conducted in degree unit.
(2) The indexing position is checked with the rotary axis, and is not checked with other axes.
(3) When the indexing increment is set to 2 degrees, the rotary axis is set to the B axis, and the B axis is moved with JOG to the 1.234 position, an indexing error will occur if "G90B5." or "G91B2." is commanded.
Function and purpose
Detailed description
G90 G01 C102.000 ; Moves to the 102 degree angle. G90 G01 C101.000 ; Program error G90 G01 C102 ; Moves to the 102 degree angle. (Decimal point type II)
# Item Details Setting range (unit)
2106 Index unit Indexing incre- ment
Set the indexing increment with which the rotary axis can be positioned.
0 to 360()
Precautions
3
9 IB-1501277-P
Program Formats
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
10IB-1501277-P
3Program Formats 3.1 Program Format
A collection of commands assigned to an NC to move a machine is called "program". A program is a collection of units called "block" which specifies a sequence of machine tool operations. Blocks are written in the order of the actual movement of a tool. A block is a collection of units called "word" which constitutes a command to an operation. A word is a collection of characters (alphabets, numerals, signs) arranged in a specific sequence.
% Block Block Block Block Block Block Block Block Block
%
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
11 IB-1501277-P
A program format looks as follows.
(1) Program start Input an End Of Record (EOR, %) at the head of a program. It is automatically added when writing a program on an NC. When using an external device, do not forget to input it at the head of a program. For details, refer to the description of the file format.
(2) Program No. Program Nos. are used to classify programs by main program unit or subprogram unit. They are designated by the address "O" followed by numbers of up to 8 digits. Program Nos. must be written at the head of programs. A setting is available to prohibit O8000s and O9000s from editing (edit lock). Refer to the instruction manual for the edit lock.
(3) Comment Data between control out "(" and control in ")" is ignored. Information including program names and comments can be written in.
(4) Program section A program is a collection of several blocks.
(5) Program end Input an end of record (EOR, %) at the end of a program. It is automatically added when writing a program on an NC.
Detailed description
Program
% O (COMMENT) Block Block Block Block Block Block Block Block
%
(1)
(5)
(2)
(4)
(3)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
12IB-1501277-P
[Block]
A block is a least command increment, consisting of words. It contains the information which is required for a machine tool to execute a specific operation. One block unit con- stitutes a complete command. The end of each block is marked with an End of Block (EOB, expressed as ";" for the sake of convenience).
[Word]
A word consists of a set of an alphabet, which is called an address, and numerals (numerical information). Meanings of the numerical information and the number of significant digits of words differ according to an address.
(1) Leading zeros can be omitted from numerals.
The major contents of a word are described below.
(1) Sequence No. "Sequence No." consists of the address "N" followed by numbers up to 8 digits for M8 Series and 6 digits for C80 Series. It is used as an index when searching a necessary block in a program (as branch destination and etc.). It does not affect the operation of a tool machine.
(2) Preparatory function (G code, G function) "Preparatory function (G code, G function)" consists of the address G followed by numbers of 2 or 3 digits (it may include 1 digit after the decimal point). G codes are mainly used to designate functions, such as axis movements and setting of coordinate systems. For example, G00 executes a positioning and G01 executes a linear interpo- lation.
(3) Coordinate words "Coordinate words" specify the coordinate positions and movement amounts of machine tool axes. They consist of an address which indicates each axis of a tool machine followed by numerical information ("+" or "-" signs and numerals). X, Y, Z, U, V, W, A, B and C are used as address. Coordinate positions and movement amounts are specified by either "incremental commands" or "absolute commands". The axis name can be expanded to two letters depending on the MTB specifications. For details, refer to "15.12 Axis Name Extension".
(4) Feed functions (F functions) "Feed Functions (F functions)" designate the speed of a tool relative to a workpiece. They consist of the address F followed by numbers.
Block and word
(a) Alphabet (address) (n) Number
EOB
Word Word Word... ;Word
(a) (n)
Note
N___ G__ X__ Z__ F__ ;
( 1) ( 2) ( 3) ( 4) EOB
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
13 IB-1501277-P
Fixed sequences or repeatedly used parameters can be stored in the memory as subprograms which can then be called from the main program when required. If a command is issued to call a subprogram while a main program is being executed, the subprogram will be exe- cuted. And when the subprogram is completed, the main program will be resumed. Refer to "14.1 Subprogram Control; M98, M99, M198" for details of subprogram execution.
Main program and subprograms
O0010;
M98P1000;
M98P2000;
M02;
O1000;
M99;
O2000;
M99;
Main program Subprogram 1
Subprogram 2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
14IB-1501277-P
3.2 File Format
Program file can be created using NC edit screen and PC. It can be input/output between NC memory and an external I/O device. Hard discs stored in NC unit are regarded as an external I/O device. For the details of input/output method, refer to the instruction manual. Program file format differs depending on the device which creates the program.
Devices which can input/output program files are as follows.
(*1) GOT back-side SD card
(*2) GOT front-side USB memory
(*3) This function is valid only for M80 Series. The availability of the function depends on the MTB specifications. (parameter "#1760 cfgPR10/bit2" (Enable HD mode on IPC))
The file format for each external I/O device is as follows:
(1) NC memory (Creates program on NC)
Function and purpose
Detailed description
Devices available for input/output
External data input/output interface M800W/ M80W M800S/M80 C80 E80
NC memory Serial - SD card in control unit (HD) - - - Front-side SD card (*1) Ethernet Display unit-side data server (DS) - Front-side USB memory (*2) IPC (Industrial PC) - (*3) - -
Program file format
End of record (EOR, %) The end of record (EOR, %) is automatically added. It does not need to be input purposely.
Program No. (O No.) Not necessary. File transfer When multiple programs within the NC memory are transferred to an external
device as serial, they will be integrated into one file in the external device. When a file containing multiple programs in an external device is transferred to NC memory as serial, it will be divided into one file per one program.
(COMMENT) ; G28XYZ ;
M02 ; %
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
15 IB-1501277-P
(2) External device (except for serials such as SD card and USB memory)
(3) External device (serial)
[Single program] [Multiple programs]
End of record (EOR, %) The first line (from % to LF, or CR LF) will be skipped. Also, the content after the second % will not be transferred. "%" must be included in the first line because if not, the necessary information when transferring a file to an NC memory cannot be transferred.
Program No. (O No.) O No. before (COMMENT) will be ignored and the file name will be given the priority.
File transfer Multiple programs cannot be transfered or collated between the serial-con- nected device and the external devices except for the serial connection. When a file containing multiple programs in an external device is transferred to NC memory as serial, it will be divided into one file per one program. When transferring divided programs one by one from an external device, which is not serial, (multiple programs) to an NC memory, the head program name can be omitted like "(COMMENT)" only when the transferring destina- tion file name is designated to the file name field of device B.
Program name Program name should be designated with up to 32 alphanumeric characters (29 characters for a multi-part system program).
End of block (EOB, ;) When the I/O parameter "CR output" is set to "1", EOB becomes CRLF.
End of record (EOR, %) The first line (from % to LF, or CR LF) will be skipped. Also, the content after the second % will not be transferred. "%" must be included in the first line because if not, the necessary information when transferring a file to an NC memory cannot be transferred.
File transfer Multiple programs cannot be transfered or collated between the serial-con- nected device and the external devices except for the serial connection. When transferring a file as serial, the head program name can be omitted like "(COMMENT)" only when the transferring destination file name is designated to the file name field of device B.
Program name Program name should be designated with up to 32 alphanumeric characters (29 characters for a multi-part system program).
End of block (EOB, ;) When the I/O parameter "CR output" is set to "1", EOB becomes CRLF.
CRLF
(COMMENT) CRLF
G28 XYZ CRLF
: : M02 CRLF
% ^Z
CRLF
CRLF
G28 XYZ CRLF
: : M02 CRLF
O101(COMMENT1) CRLF
: M02 CRLF
% ^Z
O100(COMMENT)
LF
O100(COMMENT) LF
G28 XYZ LF
: : M02 LF
%
%
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
16IB-1501277-P
Chinese characters or the characters with umlaut symbol such as "" can be used in the messages of system vari- ables #3000 and #3006. Since it cannot be input on the NC edit screen, create it with a general text editor. Use the character code corresponding to the display language (parameter "#1043 lang"). Messages with character codes which do not correspond to the display language cause character corruption.
Character code of machining program
#1043 lang Character code
0 English Windows-1252 1 Japanese Shift-JIS
11 German Windows-1252 12 French Windows-1252 13 Italian Windows-1252 14 Spanish Windows-1252 15 Chinese (traditional) Big5 16 Korean (Hangeul) KS C 5601-1987 17 Portugese Windows-1252 18 Dutch Windows-1252 19 Swedish Windows-1252 20 Hungarian Windows-1250 21 Polish Windows-1250 22 Chinese (simplified) GB2312 23 Russian Windows-1251 24 Turkish CP1254 25 Czech Windows-1250 31 Indonesian Windows-1252
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
17 IB-1501277-P
3.3 Optional Block Skip
3.3.1 Optional Block Skip; /
This function selectively ignores a section of a machining program from a "/" (slash code) to the end of the block.
Provided that the optional block skip switch is ON, a section of a machining program from a "/" to the end of the block are ignored. They are executed if the switch is OFF. Parity check is valid regardless of whether the optional block skip switch is ON or OFF. When, for instance, all blocks are to be executed for one workpiece but specific blocks are not to be executed for another workpiece, one machining program can be used to machine different parts by inserting the "/" into those specific blocks.
(1) When the parameter "#1274 ext10/bit4" is set to "0" and the parameter "#1226 aux10/bit1" is set to "0": A "/" placed in the middle of a block is always interpreted as a division instruction regardless of whether or not the optional block skip signal state is ON or OFF.
(2) When the parameter "#1274 ext10/bit4" is set to "0" and the parameter "#1226 aux10/bit1" is set to "1": A "/" placed in a bracketed ("[ ]") expression is interpreted as a division instruction. As for a "/" that appears in any other contexts, the section of the block following the "/" will be skipped if the op- tional skip signal is ON, and the "/" itself will be ignored if the optional skip signal is OFF.
Function and purpose
Detailed description
Program example
G00 X0. Z0.; #101 = [ 100. / 4 ] ; Sets "25." to #101. (As the result of execution of a division instruction) G00 Z[ 100. / 4 ] ; Moves Z axis to "25.". (As the result of execution of a division instruction) #102 = 100. / #101 ; Sets "4." to #102. (As the result of execution of a division instruction) M30 ;
G00 X0. Z0.; #101 = [ 100. / 4 ] ; Sets "25." to #101. (As the result of execution of a division instruction) G00 X100. / Z200. ; Moves X axis to "100. No Z axis movements made. (As the result of skipping the
section of the block after "/") G00 Z[ 100. / 4 ] ; Moves Z axis to "25.". (As the result of execution of a division instruction) #102 = 100. / #101 ; Sets "100." to #102. (As the result of skipping the section of the block after "/") M30 ;
G00 X0. Z0.; #101 = [ 100. / 4 ] ; Sets "25." to #101. (As the result of execution of a division instruction) G00 X100. / Z200. ; Moves X axis to "100." and Z axis to "200.". (As the result of ignoring "/") G00 Z[ 100. / 4 ] ; Moves Z axis to "25.". (As the result of execution of a division instruction) #102 = 100. / #101 ; Program error (P242) occurs. (As the result of ignoring "/") M30 ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
18IB-1501277-P
(3) When the parameter "#1274 ext10/bit4" is set to "1" : When a "/" is placed in a bracketed expression or when an expression that includes a "/" is on the right side of an equation, the "/" is interpreted as a division instruction. As for a "/" that appears in any other contexts, the section of the block following the "/" will be skipped if the op- tional skip signal is ON, and the "/" itself will be ignored if the optional skip signal is OFF.
(1) When the parameter "#1274 ext10/bit4" is set to "0" and parameter "#1226 aux10/bit1" is set to "0", put the "/" code for optional block skip at the beginning of a block. If it is placed inside the block, it is assumed as a user macro, a division instruction. (Example) N20 G01 X25. /Z25. ; NG (User macro, a division instruction; a program error results.) /N20 G01 X25. Z25. ; OK When parameter "#1274 ext10/bit4" = "0" and parameter "#1226 aux10/bit1" = "1", a "/" placed in the middle of a block functions as a starting point of the optional skip. To use a "/" as a division instruction, bracket (enclose in square brackets) the formula containing a slash code.
(2) A space immediately followed by a "/" at the very beginning of a block is always regarded as equal to a "/" at the head of a block regardless of the value set in parameter "#1226 aux10/bit1".
(3) The optional block skip is processed immediately before the pre-read buffer. Consequently, it is not possible to skip up to the block which has been read into the pre-read buffer.
(4) This function is valid even during a sequence number search. (5) All blocks with the "/" code are also input and output during tape storage and tape output, regardless of the po-
sition of the optional block skip switch.
G00 X0. Z0.; #101 = [ 100. / 4 ] ; Sets "25." to #101. (As the result of execution of a division instruction) G00 X100. / Z200. ; Moves X axis to "100. No Z axis movements made. (As the result of skipping the
section of the block after "/") G00 Z[ 100. / 4 ] ; Moves Z axis to "25.". (As the result of execution of a division instruction) #102 = 100. / #101 ; Sets "4." to #102. (As the result of execution of a division instruction) M30 ;
G00 X0. Z0.; #101 = [ 100. / 4 ] ; Sets "25." to #101. (As the result of execution of a division instruction) G00 X100. / Z200. ; Moves X axis to "100." and Z axis to "200.". (As the result of ignoring "/") G00 Z[ 100. / 4 ] ; Moves Z axis to "25.". (As the result of execution of a division instruction) #102 = 100. / #101 ; Sets "4." to #102. (As the result of execution of a division instruction) M30 ;
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
19 IB-1501277-P
3.3.2 Optional Block Skip Addition ; /n
Whether the block with "/n (n:1 to 9)" (slash) is executed during automatic operation and searching is selected. By using the machining program with "/n" code, different parts can be machined by the same program.
The block with "/n" (slash) code is skipped when the "/n" is programmed to the head of the block and the optional block skip n signal is turned ON. For a block with the "/n" code inside the block (not at the head of the block), the program is operated according to the value of the parameter "#1226 aux10/bit1" setting. When the optional block skip n signal is OFF, the block with "/n" is executed.
(1) When the 2 parts like the figure below are machined, the following program is used. When the optional block skip 5 signal is ON, the part 1 is created. When the optional block skip 5 signal is OFF, the part 2 is created.
Function and purpose
Detailed description
Program example
N1 G54 ; N2 G90 G81 X50. Z-20. R3. F100 ;
/5 N3 X30. ; N4 X10. ; N5 G80 ; M02 ;
Part 1 Optional block skip 5 signal ON
Part 2 Optional block skip 5 signal OFF
N4 N2 N2N3N4
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
20IB-1501277-P
(2) When two or more "/n" codes are commanded at the head of the same block, the block will be ignored if either of the optional block skip n signals corresponding to the command is ON.
(3) When the parameter "#1226 aux10/bit1" is "1"and two or more "/n" are commanded inside the same block, the commands following "/n" in the block are ignored if either of the optional block skip n signals corresponding to the command is ON.
N01 G90 Z3. M03 S1000 ; (a) Optional block skip 1 signal ON (Optional block skip 2.3 signal OFF) N01 -> N08 -> N09 -> N10 -> N11 -> N12
/1/2 N02 G00 X50. ; /1/2 N03 G01 Z-20. F100 ; /1/2 N04 G00 Z3. ; /1 /3 N05 G00 X30. ; (b) Optional block skip 2 signal ON
(Optional block skip 1.3 signal OFF) N01 -> N05 -> N06 -> N07 -> N11 -> N12
/1 /3 N06 G01 Z-20. F100 ; /1 /3 N07 G00 Z3. ; /2/3 N08 G00 X10. ; (c) Optional block skip 3 signal ON
(Optional block skip 1.2 signal OFF) N01 -> N02 -> N03 -> N04 -> N11 -> N12
/2/3 N09 G01 Z-20. F100 ; /2/3 N10 G00 Z3. ;
N11 G28 X0 M05 ; N12 M02 ;
N01 G91 G28 X0.Y0.Z0.; N03 block will operate as follows. (a) Optional block skip 1 signal ON Optional block skip 2 signal OFF "Y1. Z1." is ignored. (b) Optional block skip 1 signal OFF Optional block skip 2 signal ON "Z1." is ignored.
N02 G01 F1000; N03 X1. /1 Y1. /2 Z1.; N04 M30;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
21 IB-1501277-P
3.4 G Code 3.4.1 Modal, Unmodal
G codes define the operation modes of each block in programs. G codes can be modal or unmodal command. Modal commands always designate one of the G codes in the group as the NC operation mode. The operation mode is maintained until a cancel command is issued or other G code among the same group is commanded. An unmodal command designates the NC operation mode only when it is issued. It is invalid for the next block.
3.4.2 G Code Lists
G code Group Function Section
00 01 Positioning 6.1 0.5 28 Rapid traverse block overlap 7.14.1 01 01 Linear interpolation 6.2 02 01 Circular interpolation CW 6.3
R-specified circular interpolation CW 6.4 Helical interpolation CW 6.7 Spiral/Conical interpolation CW (type2) 6.14
03 01 Circular interpolation CCW 6.3 R-specified circular interpolation CCW 6.4 Helical interpolation CCW 6.7 Spiral/Conical interpolation CCW (type2) 6.14
02.1 01 Spiral/Conical interpolation CW (type1) 6.14 03.1 01 Spiral/Conical interpolation CCW (type1) 6.14 02.2 01 Involute interpolation/Helical involute interpolation CW 6.18 03.2 01 Involute interpolation/Helical involute interpolation CCW 6.18 02.3 01 Exponential function interpolation positive rotation 6.12 03.3 01 Exponential function interpolation negative rotation 6.12 02.4 01 3-dimensional circular interpolation CW 6.15 03.4 01 3-dimensional circular interpolation CCW 6.15 04 00 Dwell (Time-based designation) 8.1 05 00 High-speed machining mode 17.1
High-speed high-accuracy control II/III 17.3 05.1 00 High-speed high-accuracy control I 17.3
Spline interpolation 17.4 06.2 01 NURBS interpolation 6.16 07 00 Hypothetical axis interpolation 6.17 07.1 107
19 Cylindrical interpolation 6.9
08 00 High-accuracy control 17.2 09 00 Exact stop check 7.11 10 00 Data input by program
(Parameter input, Compensation input, Tool shape input, R-Navi data in- put)
15.9
Tool life management data input 15.10 Coordinate rotation input by parameter 20.11
11 00 Data input by program cancel (Parameter input, Compensation input, Tool shape input, R-Navi data in- put)
15.9
Tool life management data input 15.10 10.9 00 Diameter/Radius designation switch 5.2.1 12 00 Circular cutting CW 6.10
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
22IB-1501277-P
13 00 Circular cutting CCW 6.10 12.1 112
21 Polar coordinate interpolation ON 6.11
* 13.1 113
21 Polar coordinate interpolation cancel 6.11
14 * 15 18 Polar coordinate command OFF 6.13 16 18 Polar coordinate command ON 6.13 17 02 X-Y plane selection 6.5 18 02 Z-X plane selection 6.5 19 02 Y-Z plane selection 6.5 20 06 Inch command 5.3 21 06 Metric command 5.3 22 04 Stroke check before travel ON 21.1 23 04 Stroke check before travel cancel 21.1 24 25 26 00 Return to the selected point/Tapping retract 15.13 27 00 Reference position check 20.16 28 00 Reference position return 20.13 29 00 Start position return 20.13 30 00 2nd to 4th reference position return 20.14 30.1 00 Tool change position return 1 20.15 30.2 00 Tool change position return 2 20.15 30.3 00 Tool change position return 3 20.15 30.4 00 Tool change position return 4 20.15 30.5 00 Tool change position return 5 20.15 30.6 00 Tool change position return 6 20.15 31 00 Skip/Speed change skip 22.2
Multi-step skip 2 22.4 31.1 00 Multi-step skip 1-1 22.3 31.2 00 Multi-step skip 1-2 22.3 31.3 00 Multi-step skip 1-3 22.3 32 33 01 Thread cutting 6.6 34 00 Special fixed cycle (bolt hole circle) 13.2.1 35 00 Special fixed cycle (line at angle) 13.2.2 36 00 Special fixed cycle (arc) 13.2.3 37 00 Automatic tool length measurement 22.1 37.1 00 Special fixed cycle (grid) 13.2.4 38 00 Tool radius compensation vector designation 12.3 39 00 Tool radius compensation corner arc 12.3 * 40 07 Tool radius compensation (tool nose radius compensation) cancel 12.3
3-dimensional tool radius compensation cancel 12.5 3-dimensional tool radius compensation (Tool's vertical-direction com- pensation) cancel
19.5
41 07 Tool radius compensation (tool nose radius compensation) left 12.3 3-dimensional tool radius compensation left 12.5
42 07 Tool radius compensation (tool nose radius compensation) right 12.3 3-dimensional tool radius compensation right 12.5
G code Group Function Section
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
23 IB-1501277-P
* 40.1 150
15 Normal line control cancel 15.7
41.1 151
15 Normal line control left ON 15.7
42.1 152
15 Normal line control right ON 15.7
41.2 07 3-dimensional tool radius compensation (Tool's vertical-direction com- pensation) (left)
19.5
42.2 07 3-dimensional tool radius compensation (Tool's vertical-direction com- pensation) (right)
19.5
43 08 Tool length compensation (+) 12.2 44 08 Tool length compensation (-) 12.2 43.1 08 Tool length compensation along the tool axis ON 19.2 43.4 08 Tool center point control type1 ON 19.3 43.5 08 Tool center point control type2 ON 19.3 43.7 08 Tool position compensation start 19.1 45 00 Tool position offset (extension) 12.6 46 00 Tool position offset (reduction) 12.6 47 00 Tool position offset (double elongation) 12.6 48 00 Tool position offset (double contraction) 12.6 * 49 08 Tool length compensation cancel 12.2
Tool length compensation along the tool axis cancel 19.2 Tool center point control cancel 19.3 Tool position compensation cancel 19.1
* 50 11 Scaling cancel 20.12 51 11 Scaling ON 20.12 * 50.1 19 Mirror image by G code cancel 15.6 51.1 19 Mirror image by G code ON 15.6 50.2 250
00 Tool spindle synchronization IB/IC cancel 18.2.2
18.2.3 51.2 251
00 Tool spindle synchronization IB/IC 18.2.2
18.2.3 52 00 Local coordinate system setting 20.5 53 00 Basic machine coordinate system selection 20.3 53.1 00 Tool axis direction control (type 1) 19.4.8 53.6 00 Tool axis direction control (type 2) 19.4.8 * 54 12 Workpiece coordinate system 1 selection 20.6 55 12 Workpiece coordinate system 2 selection 20.6 56 12 Workpiece coordinate system 3 selection 20.6 57 12 Workpiece coordinate system 4 selection 20.6 58 12 Workpiece coordinate system 5 selection 20.6 59 12 Workpiece coordinate system 6 selection 20.6 54.1 12 Extended workpiece coordinate system selection 20.6 54.2 23 Workpiece position offset for rotary axis 20.8 54.4 27 Workpiece installation error compensation - 60 00(01) Unidirectional positioning 6.8.1 61 13 Exact stop check mode 7.12 61.1 13 High-accuracy control ON 17.2 61.2 13 High-accuracy spline 17.6 61.4 13 Spline interpolation 2 17.5 62 13 Automatic corner override 7.15.1
G code Group Function Section
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
24IB-1501277-P
63 13 Tapping mode 7.16 * 64 13 Cutting mode 7.17 65 00 User macro simple call 14.4.1 66 14 User macro modal call A 14.4.2 66.1 14 User macro modal call B 14.4.3 * 67 14 User macro modal call cancel 14.3 68 16 Coordinate rotation by program ON 20.10
3-dimensional coordinate conversion mode ON 20.9 68.2 16 Inclined surface machining command 19.4
R-Navi data input (Selecting the registered machining surface) 15.9.6 68.3 16 Inclined surface machining command (Based on tool axis direction) 19.4 * 69 16 Coordinate rotation by program cancel 20.10
3-dimensional coordinate conversion mode OFF 20.9 Inclined surface machining cancel 19.4 R-Navi data input (Canceling the selected machining surface) 15.9.6
70 09 User fixed cycle 71 09 User fixed cycle 72 09 User fixed cycle 73 09 Fixed cycle (step) 13.1.10 74 09 Fixed cycle (reverse tap) 13.1.11 75 09 Fixed cycle (circle cutting cycle) 13.1.12 76 09 Fixed cycle (Fine boring) 13.1.13 77 09 User fixed cycle 78 09 User fixed cycle 79 09 User fixed cycle * 80 09 Fixed cycle cancel 13.1 81 09 Fixed cycle (drill/spot drill) 13.1.1 82 09 Fixed cycle (drill/counter boring) 13.1.2 83 09 Fixed cycle (deep drilling/small-diameter deep-hole drilling) 13.1.3 84 09 Fixed cycle (tapping) 13.1.4 85 09 Fixed cycle (boring) 13.1.5 86 09 Fixed cycle (boring) 13.1.6 87 09 Fixed cycle (back boring) 13.1.7 88 09 Fixed cycle (boring) 13.1.8 89 09 Fixed cycle (boring) 13.1.9 90 03 Absolute command 5.1 91 03 Incremental command 5.1 92 00 Coordinate system setting 20.4
Spindle clamp speed setting 10.3 92.1 00 Workpiece coordinate system preset 20.7 93 05 Inverse time feed 7.5 94 05 Feed per minute (asynchronous feed) 7.4 95 05 Feed per revolution (synchronous feed) 7.4 96 17 Constant surface speed control ON 10.2 97 17 Constant surface speed control OFF 10.2 * 98 10 Fixed cycle Initial level return 13.1.17 99 10 Fixed cycle (R point level return) 13.1.17 100-225 00 User macro (G code call) Max. 10 14.4.4 113.1 00 Spindle synchronization I/Tool spindle synchronization (IA/IB/II) cancel 18.1.1 114.1 00 Spindle synchronization I 18.1.1
G code Group Function Section
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
25 IB-1501277-P
(1) Codes marked with * are codes that must be or are selected in the initial state. The codes marked with are codes that should be or are selected in the initial state by the parameters.
(2) If two or more G codes from the same code are commanded, the latter G code will be valid. (3) This G code list is a list of conventional G codes. Depending on the machine, movements that differ from the
conventional G commands may be included when called by the G code macro. Refer to the Instruction Manual issued by the MTB.
(4) Whether the modal is initialized or not depends on each reset input. "Reset 1"
The modal is initialized when the reset initialization parameter (#1151 rstinit) is ON. (This depends on the MTB specifications.)
"Reset 2" and "Reset & rewind" The modal is initialized when the signal is input.
Reset at emergency stop release Conforms to "Reset 1".
When modal is automatically reset at the start of individual functions such as reference position return Conforms to "Reset & rewind".
114.2 00 Tool spindle synchronization IA 18.2.1 114.3 00 Tool spindle synchronization II 18.2.1 120.1 00 Machining condition selection I 17.7 121 00 Machining condition selection I cancel 17.7 122 00 Activate sub part system I 16.3.1 127 00 Prohibits the arbitrary reverse run in all part systems 15.8 130 00 Selection of axis (axes) for feedrate command 7.7 140 00 Arbitrary axis exchange command 16.2.1 141 00 Arbitrary axis exchange return command 16.2.1 142 00 Arbitrary axis exchange/reference axis arrange return command 16.2.1 145 00 Cancel sub part systems 16.3 160 00 Torque limitation skip 22.6 162 00 Spindle speed fluctuation detection 10.5 163 00 Spindle speed fluctuation detection cancel 10.5 180 00 Interactive cycle insertion program 15.11 186 00 Interference check III interfering object data enable command 21.2 187 09 Thread milling cycle 13.1.14
Precautions
CAUTION
The commands with "no value after G" will be handled as "G00".
G code Group Function Section
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
3 Program Formats
26IB-1501277-P
3.5 Precautions before Starting Machining
CAUTION
When creating the machining program, select the appropriate machining conditions, and make sure that the
performance, capacity and limits of the machine and NC are not exceeded. The examples do not take into ac-
count the machining conditions.
Before starting actual machining, always carry out a graphic check, a dry run operation, and a single block op-
eration to check the machining program, tool offset amount, workpiece offset amount, etc.
4
27 IB-1501277-P
Pre-read Buffer
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
4 Pre-read Buffer
28IB-1501277-P
4Pre-read Buffer 4.1 Pre-read Buffer
During automatic processing, the contents of one block ahead are normally pre-read so that program analysis pro- cessing is conducted smoothly. However, during tool radius compensation, a maximum of 5 blocks are pre-read for the intersection point calculation including interference check.
The specifications of pre-read buffers in 1 block are as follows:
(1) The data of 1 block is stored in this buffer. (2) When comments and the optional block skip function is ON, the data extending from the "/" (slash) code up to
the EOB code are not read into the pre-read buffer. (3) The pre-read buffer contents are cleared with resetting. (4) When the single block function is ON during continuous operation, the pre-read buffer stores the next block's
data and then stops operation. (5) The way to prohibit the M command which operates the external controls from pre-reading, and to make it to
recalculate, is as follows: Identify the M command which operates the external controls by a PLC, and turn on the "recalculation request" on PLC output signal. (When the "recalculation request" is turned ON, the program that has been pre-read is recalculated.) These operations depend on the MTB specifications.
(1) Depending on whether the program is executed continuously or by single blocks, the timing of the validation/ invalidation of the PLC signals, including optional block skip, will differ.
(2) If the PLC signal such as optional block skip is turned ON/OFF with the M command, the PLC control operation will not be effective for the program pre-read with the buffer register.
Function and purpose
Detailed description
Precautions
5
29 IB-1501277-P
Position Commands
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
30IB-1501277-P
5Position Commands 5.1 Position Command Methods ; G90,G91
By using the G90 and G91 commands, it is possible to execute the next coordinate commands using absolute com- mands or incremental commands. The R-designated circle radius and the center of the circle determined by I, J, K are always incremental commands.
Function and purpose
Command format
G90/G91 X__ Y__ Z__ __ ;
G90 Absolute command G91 Incremental command X,Y,Z, Coordinate values ( is the additional axis.)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
31 IB-1501277-P
(1) Regardless of the current position, in the absolute mode, it is possible to move to the position of the workpiece coordinate system that was designated in the program.
(2) For the next block, the last G90/G91 command that was given becomes the modal.
(3) Since multiple commands can be issued in the same block, it is possible to command specific addresses as ei- ther absolute positions or incremental positions.
(4) When the power is turned ON, it is possible to select whether you want absolute commands or incremental com- mands with the #1073 I_Absm parameter.
(5) Even when commanding with the manual data input (MDI), it will be treated as a modal from that block.
Detailed description
N1 G90 G00 X0 Y0 ;
In the incremental mode, the current position is the start point (0), and the movement is made only the value determined by the program, and is expressed as an incremental position.
N2 G90 G01 X200. Y50. F100 ; N2 G91 G01 X200. Y50. F100 ;
Using the command from the 0 point in the workpiece coordi- nate system, it becomes the same coordinate command value in either the absolute mode or the incremental mode.
Tool
(G90) N3 X100. Y100. ; The axis moves to the workpiece coordinate system X = 100.mm and Y = 100.mm position.
(G91) N3 X-100. Y50. ; The X axis moves to -100.mm and the Y axis to +50.0mm as an incremental position, and as a result X moves to 100.mm and Y to 100.mm.
N4 G90 X300. G91 Y100. ;
The X axis is treated in the absolute mode, and with G90 is moved to the workpiece coordinate system 300.mm position. The Y axis is moved +100.mm with G91. As a result, Y moves to the 200.mm position. In terms of the next block, G91 remains as the modal and becomes the incremental mode.
300.200.
200.
100 N1
100. N2
W X
Y
300.200.
200.
100.
N3
W
X
Y
100.
300.200.100.
N4
W
X
Y
100.
200.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
32IB-1501277-P
5.2 Diameter Designation and Radius Designation 5.2.1 Diameter/Radius Designation Switch; G10.9
The method of commanding a travel distance (command with a diameter dimension/command with a radius dimen- sion (as-is distance)) in a program is defined individually for each axis depending on MTB specifications (parameter "#1019 dia"). Diameter/Radius designation switch function, however, enables you to switch the diameter/radius designation of each axis using a G code at your desired timing. When you use the function to switch diameter/radius designation, it helps you create a program more flexibly according to each machining situation.
Diameter/Radius designation switch enables you to select any desired NC axis, excluding rotary axes, and switch the diameter/radius designation of the axis.
Function and purpose
Term
Diameter/Radius being switched
This refers to a condition where the diameter/radius selection of an axis is different from the power-ON state.
Command format
Diameter/Radius designation switch
G10.9 Axis name 1__ Axis name 2__ ... Axis name n__ ;
Axis name n Axis name for which diameter/radius designation is switched. Select radius or diameter designation with a value that follows the axis name. 0: Radius designation 1: Diameter designation If you do not command any axis name, the diameter/radius designation statuses of all the axes of the part system are returned to the initial power-ON state.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
33 IB-1501277-P
(1) G10.9 is a non-modal command that belongs to Group 0. (2) G10.9 is effective for all the G code lists. (3) If G10.9 is commanded together with any other G code in a block, the program error (P33) occurs. (4) For the axis name, specify the axis name that is set in "#1013 axname" or "#1014 incax" (*1). If the specified axis
name is not found, a program error (P33) will occur. (*1) The axis name set in "#1014 incax" can be specified only when the setting value of "#1076 AbsInc" is "1".
These settings depend on the MTB specifications.
(5) If a rotary axis is specified with "Axis name", a program error (P32) occurs. (6) If a number with a decimal point is specified with "Axis name", the fraction is ignored. If any value other than "0"
or "1" is specified, the program error (P35) occurs. If specified with a variable, the fraction is rounded to the clos- est whole number.
(7) G10.9 switches the diameter/radius designation for programmed coordinates command and coordinates of counter in Monitor screen. However, diameter/radius designation is not switched for data including parameters, workpiece offsets, tool data and tool offsets.
(8) The axis specified for diameter/radius designation switch by G10.9 is effective until G10.9 is given again for switching or until Reset or Emergency stop is input. After the Reset or Emergency stop, the diameter/radius des- ignation before G10.9 is restored. However, when "#1255 set27/bit3" is set to "1", the diameter/radius designation status is held even if resetting is performed. (This parameter setting depends on the MTB specifications.)
(9) If diameter/radius designation switch is not performed for an axis in the part system of G10.9 command, the axis behaves as follows: The axis behaves according to the setting of "#1019 dia" for L system. This setting depends on the MTB
specifications. The axis acts as radius-designation axis in the M system.
(10) Irrespective of the "#1019 dia" and "#1077 radius" settings, the designation selected by G10.9 has priority. (11) If you use G10.9 to switch diameter/radius designation for two axes (X axis and Z axis) at a time, program the
command as follows: G10.9 X1 Z0; In the example above, X axis is switched to diameter designation, and Z axis to radius designation.
(1) Restart search If you perform restart search after a G10.9 block, the diameter/radius designation switched by G10.9 is applied.
(2) Arbitrary reverse run If you perform reverse run for a G10.9 block, the reverse run stops at the G10.9 block, and is disabled for the prior blocks before the G10.9 block.
(3) Manual arbitrary reverse run If you perform forward run for G10.9 block, the diameter/radius designation switched by G10.9 is applied. If you perform reverse run for a G10.9 block, the reverse run stops at the G10.9 block, and is disabled for the prior blocks before the G10.9 block.
(4) Chopping G10.9 is unable to switch diameter/radius designation of a chopping axis. If G10.9 is given to an axis that is in chopping mode, or if you enable chopping mode for an axis for which diameter/radius designation is being switched by G10.9, the operation error (M01 0095) occurs. If the alarm above has been caused by giving G10.9 to an axis that is in chopping mode, the chopping axis keeps moving. Use the corresponding PLC signal or NC reset to stop the axis.
(5) Synchronous control For a master or slave axis that is in synchronous operation, you can switch diameter/radius designation using G10.9. Even when the diameter/radius designation status is different between master and slave axes, their synchroni- zation will not fail. The coordinates displayed on Monitor screen are dependent on the diameter/radius designa- tion of each axis.
Detailed description
Relationship with other functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
34IB-1501277-P
(6) Arbitrary axis exchange control The diameter/radius command switching for an axis in arbitrary axis exchange control mode depends on the MTB specifications(*1). (*1) Parameters of the command address: "#12071 adr_abs[1]" - "#12078 adr_abs[8]", "#12079 adr_inc[1]" -
"#12086 adr_inc[8]"
If an arbitrary axis exchange-related command (G140/G141/G142) has given in a part system, all the axes of the part system are returned to the initial status under the exchanged axis configuration after the axis exchange.
(7) Program format switch In M system, the setting of "#1019 dia" is disabled, thus all the axes are treated as radius-designation axis. How- ever, G10.9 enables a diameter-value command. When you switch the program format, the diameter/radius designation is returned to the default state for all the axes of the part system.
(8) Axis name extension Diameter/Radius designation switch with G10.9 is disabled for a name-extended axis.
(9) Manual arbitrary feed If a position command in manual arbitrary feed is given, the diameter/radius axis setting of each axis at power ON is applied. Therefore, even if a manual arbitrary feed command is given to an axis in diameter/radius desig- nation switch mode using the G10.9 command, the diameter/radius switch status is ignored.
(10) Cylindrical interpolation/Polar coordinate interpolation The diameter/radius designation of each axis at which these functions are being executed follows the setting of "#8111 Milling Radius" without being affected by the G10.9 command. When these functions are canceled, the setting returns to the diameter/radius axis designation that was valid before the functions are executed. If G10.9 is commanded while these functions are being executed, a program error (P481) will occur.
(11) Tool center point control If tool center point control is given to an axis for which diameter/radius designation is being switched by G10.9, a program error (P941) occurs. If G10.9 is given to an axis that is in tool center point control, the program error (P705) occurs.
(12) Graphic check (2D/3D), Graphic trace During graphic check or graphic trace, even if the diameter and radius are switched with G10.9, neither the draw- ing image nor coordinate value view is not switched.
(1) If diameter/radius designation is switched, the travel distance changes even though the command value is un- changed. Thus special care must be taken when creating or executing a machining program.
(2) Command the feedrate with the radius value regardless of whether the diameter designation or radius designa- tion is selected. (This is applied to both the movement amount per rotation and that per minute.)
(3) Diameter/Radius designation is not switched for a value that is read or written using PLC window or system vari- ables. For M system, it is treated as a radius value. For L system, the value follows the setting of "#1019 dia".
(4) When manual handle feed or incremental feed is performed at manual interruption, the switched diameter/radius designation is applied.
(5) In a G10.9 command block, the control confirms that all the axes of the part system are decelerated to a stop before switching the diameter/radius designation. If G10.9 is given between cutting blocks, it causes acceleration and deceleration, which may damage the workpiece. Thus make sure that the tool is away from the workpiece before giving G10.9.
(6) If a G10.9 command which has the same diameter/radius designation as the existing operation is given, the G10.9 command fails to be enabled. Thus if a G code that causes an error when combined with G10.9 is given together, no error occurs.
(7) Do not give "Start point designation timing synchronization" or "M code output during axis traveling" command to an axis for which diameter/radius designation is being switched. If commanded, it cannot be assured that the timing synchronization or the M code output is performed in the correct position.
(8) Do not perform manual tool length measurement I for an axis for which the diameter/radius designation is switched. The correct tool length cannot be measured for an axis for which the diameter/radius designation is switched.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
35 IB-1501277-P
5.3 Inch/Metric Conversion; G20, G21
The commands can be changed between inch and metric with the G20/G21 command.
The G20 and G21 commands merely select the command units. They do not select the Input units. G20 and G21 selection is meaningful only for linear axes. It is invalid for rotation axes.
The counter, parameter setting and display unit are determined by parameter "#1041 I_inch". The movement/speed command will be displayed as metric units when "#1041 I_inch" is ON during the G21 command mode. The internal unit metric data of the movement/speed command will be converted into an inch unit and displayed when "#1041 I_inch" is OFF during the G20 command mode. The command unit for when the power is turned ON and reset is decided by combining the parameters "#1041 I_inch", "#1151 rstint" and "#1210 RstGmd/bit5". These parameter settings depend on the MTB specifications.
NC axis
PLC axis
Function and purpose
Command format
Inch command
G20;
Metric command
G21;
Detailed description
Output unit, command unit and setting unit
Item Initial inch OFF Initial inch ON
(metric internal unit) (inch internal unit)
#1041 I_inch=0 #1041 I_inch=1
G21 G20 G21 G20
Movement/speed command Metric Inch Metric Inch Counter display Metric Metric Inch Inch Speed display Metric Metric Inch Inch User parameter setting/display Metric Metric Inch Inch Workpiece/tool offset setting/display Metric Metric Inch Inch Handle feed command Metric Metric Inch Inch
Item #1042 pcinch=0 (metric) #1042 pcinch=1 (inch)
Movement/speed command Metric Inch Counter display Metric Inch User parameter setting/display Metric Inch
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
36IB-1501277-P
(1) The parameter and tool data will be input/output with the unit set by "#1041 I_inch". If "#1041 I_inch" is not found in the parameter input data, the unit will follow the unit currently set to NC.
(2) The unit of read/write used in PLC window is fixed to metric unit regardless of a parameter and G20/G21 com- mand modal.
(3) A program error (P33) will occur if G20/G21 command is issued in the same block as following G codes. Com- mand in a separate block. G05 (High-speed machining mode) G7.1 (Cylindrical Interpolation) G12.1 (Polar coordinate interpolation)
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
37 IB-1501277-P
5.4 Decimal Point Input
This function enables to input decimal points. It assigns the decimal point in millimeter or inch units for the machining program input information that defines the tool paths, distances and speeds. Whether to apply minimum input command increment (type I) or zero point (type II) to the least significant digit of data without a decimal point depends on the MTB specifications (parameter "#1078 Decpt2").
(1) The decimal point command is valid for the distances, angles, times, speeds and scaling rate, in machining pro- grams. (Note, only after G51)
(2) In decimal point input type I and type II, the values of the data commands without the decimal points are shown in the table below.
(3) The valid addresses for the decimal points are X, Y, Z, U, V, W, A, B, C, I, J, K, E, F, P, Q, and R. However, P is valid only during scaling. For details, refer to the list.
(4) In decimal point command, the valid range of command value is as shown below. (When "#1015 cunit" (program input command) is "10".)
(5) The decimal point command is valid even for commands defining the variable data used in subprograms. (6) While the smallest decimal point command is validated, the smallest unit for a command without a decimal point
designation is the smallest command input unit set in the specifications (1 m, 10 m, etc.) or mm can be se- lected. This selection can be made with parameter "#1078 Decpt2".
(7) Decimal point commands for decimal point invalid addresses are processed as integer data only and everything after the decimal point is ignored. Decimal point invalid addresses include the followings; D,H,L,M,N,O,P,S,T. All variable commands, however, are treated as data with decimal points.
(8) "Input command increment tenfold" is applied in the decimal point type I mode, but not in the decimal point type II mode.
Function and purpose
Detailed description
Command Command unit Type I Type II
X1; #1015 = 10000 1000 (m, 10-4inch, 10-3)
1 (mm, inch, )
#1015 = 1000 100 1 #1015 = 100 10 1 #1015 = 10 1 1
Movement com- mand (linear)
Movement com- mand (rotary)
Feedrate Dwell
Input unit [mm] -99999.999 to 99999.999
-99999.999 to 99999.999
0.001 to 10000000.000
0 to 99999.999
Input unit [inch] -9999.9999 to 9999.9999
0.0001 to 1000000.0000
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
38IB-1501277-P
Decimal point input I and II will result as follows when decimal points are not used in an address which a decimal point command is valid. Both decimal point input I and II will produce the same result when a command uses a decimal point.
(1) Decimal point input I The least significant digit of command data matches the command unit. (Example) When "X1" is commanded in 1 m system, the same result occurs as for an "X0.001" command.
(2) Decimal point input II The least significant digit of command data matches the command unit. (Example) When "X1" is commanded in 1 m system, the same result occurs as for an "X1." command.
[Addresses used and validity of decimal point commands]
Decimal point input I, II and decimal point command validity
Address Decimal point command
Usage Remarks
A Valid Coordinate position data Invalid Revolving table Invalid Miscellaneous function codes Valid Angle data
Invalid Data settings, axis numbers (G10) Valid Spindle synchronization: Acceleration/deceleration time constant
Invalid Program No. Invalid R-Navi data input by program: Coordinate axis selection Invalid Interactive cycle insertion: Cycle ID
B Valid Coordinate position data Invalid Revolving table Invalid Miscellaneous function codes Invalid Sub part system I: Identification No. Invalid R-Navi data input by program: Coordinate axis direction setting
C Valid Coordinate position data Invalid Revolving table Invalid Miscellaneous function codes Valid Corner chamfering amount ,C
Invalid Target C axis in C axis mode for spindle position control (spindle/C axis control)
Invalid Tool shape input by program: Tool color Invalid R-Navi data input by program: Basic coordinate system Invalid R-Navi data input by program: Coordinate axis direction setting
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
39 IB-1501277-P
D Invalid Compensation numbers (tool position, tool radius) Valid Automatic tool length measurement: Deceleration distance d
Invalid Parameter input by program: Byte type data Invalid Spindle synchronization: Designation of synchronized spindle Invalid Subprogram storing device number ,D Invalid Sub part system I: Synchronous control designation Valid Droop skip value Valid Tool shape input by program: Shape data 1
Invalid R-Navi data input by program: Machining registration No. Invalid Rotation direction Invalid Subprogram device No. ,D Invalid Tool spindle synchronization IA: Workpiece axis selection (Synchro-
nized spindle) Invalid Tool spindle synchronization IB: Rotary tool axis selection (Synchro-
nized spindle) Invalid Tool spindle synchronization II: Hob axis selection
E Valid Inch thread: number of ridges, precision thread: lead Invalid R-Navi data input by program: Coordinate axis direction setting Valid Synchronous tap: Cutting feedrate (Number of screw threads)
Invalid Tool spindle synchronization IA: Rotary tool axis rotation ratio designa- tion
Invalid Tool spindle synchronization II: Rotation ratio designation (Hob axis) F Valid Cutting feedrate, automatic tool length measurement speed
Valid Thread lead Valid Number of Z axis pitch in synchronous tap Valid Rapid traverse rate ,F
Invalid R-Navi data input by program: Workpiece shape Invalid R-Navi data input by program: Coordinate axis direction setting Valid Involute interpolation: Feedrate (in involute curve tangent direction)
G Valid Preparatory function code H Invalid Tool length compensation No.
Invalid Sequence Nos. in subprograms Invalid Parameter input by program: Bit type data Invalid Tool spindle synchronization IA: Rotary tool axis selection (Reference
spindle) Invalid Tool spindle synchronization IB: Workpiece axis selection (Reference
spindle) Invalid Tool spindle synchronization II: Hob axis selection Invalid Sub part system I: Reset type Valid Tool shape input by program: Shape data 2
Invalid R-Navi data input by program: Coordinate axis direction setting Invalid Tool position compensation: Compensation No.
Address Decimal point command
Usage Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
40IB-1501277-P
I Valid Coordinates for arc center and center of figure rotation Valid Tool radius compensation vector components Valid Hole pitch in the special fixed cycle Valid Circle radius of cut circle (increase amount) Valid G0/G1 in-position width, Hole drilling cycle: G0 in-position width ,I Valid Stroke check before travel: Lower limit coordinates Valid Tool shape input by program: Shape data 3 Valid R-Navi data input by program: Workpiece shift
Invalid R-Navi data input by program: Coordinate axis direction setting Valid Arc radius and approach direction
Invalid Allowable fluctuation range of spindle speed Valid Involute interpolation: Distance to the center of base circle Valid Inclined surface machining: Rotation angle about the X axis (roll angle)
J Invalid Coordinates for arc center and center of figure rotation Valid Tool radius compensation vector components Valid Special fixed cycle's hole pitch or angle Valid G0/G1 in-position width, Hole drilling cycle: G1 in-position width ,J Valid Stroke check before travel: Lower limit coordinates Valid Tool shape input by program: Shape data 4 Valid R-Navi data input by program: Workpiece shift Valid Arc radius and approach direction Valid Involute interpolation: Distance to the center of base circle Valid Inclined surface machining: Rotation angle about the Y axis (pitch angle)
K Valid Coordinates for arc center and center of figure rotation Valid Tool radius compensation vector components
Invalid Number of holes of the special fixed cycle Invalid Hole drilling cycle, sub part system I: Number of repetitions Valid Stroke check before travel: Lower limit coordinates Valid Spline interpolation 2: Tolerance (Linear axis) ,K
Invalid Tool shape input by program: Tool type Valid R-Navi data input by program: Workpiece shift Valid Involute interpolation: Distance to the center of base circle Valid Inclined surface machining: Rotation angle about the Z axis (yaw angle)
L Invalid Number of fixed cycle and subprogram repetitions Invalid Tool compensation data input by program/workpiece offset input: type
selection L2, L20, L10, L11, L12, L13
Invalid Parameter input by program: data setting selection L70 Invalid Parameter input by program: 2-word type data 4 bytes Invalid R-Navi data input by program: Start setting workpiece data L110 Invalid R-Navi data input by program: Start setting machining surface data L111 Invalid Timing synchronization number Invalid Tool life data Invalid Tool spindle synchronization IA: Rotation ratio designation (Workpiece
axis) Invalid Tool spindle synchronization II: Rotation ratio designation (Workpiece
axis) M Invalid Miscellaneous function codes
Invalid R-Navi data input by program: Coordinate axis direction designation method
Address Decimal point command
Usage Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
41 IB-1501277-P
N Invalid Sequence No. Invalid Parameter input by program: data numbers
O Invalid Program No. P Invalid/Valid Dwell time Parameters
Invalid Subprogram program call: program No. Invalid/Valid Dwell at tap cycle hole base Parameters
Invalid Number of holes of the special fixed cycle Invalid Amount of helical pitch Valid Thread milling cycle: Pitch amount
Invalid Offset number (G10) Invalid Constant surface speed control axis number Invalid Parameter input by program: Broad classification number Invalid Tool compensation data input by program/workpiece offset input: Com-
pensation No. Invalid Tool shape input by program: Data numbers Invalid Multi-step skip function 2 signal command Invalid Subprogram return destination sequence No. Invalid 2nd, 3rd, 4th reference position return number Valid Scaling factor
Invalid High-speed mode type Invalid High-accuracy control mode: Start/End Invalid Extended workpiece coordinate system No, external workpiece coordi-
nate system offset compensation No. Invalid Tool life data: Group No. Invalid Machining purpose Invalid Sub part system I: Start sequence No. Invalid R-Navi data input by program: Machining surface registration Invalid R-Navi data input by program: Coordinate axis direction axis designation Valid Spindle speed fluctuation detection: Start delay time
Invalid Interactive cycle insertion: Cycle information identification number Invalid Tool center point control: G00 temporary cancel designation Invalid Tool spindle synchronization IB: Rotation ratio designation (Workpiece
axis) Invalid Tool spindle synchronization IC: Rotation ratio designation (Spindle) Valid Tool spindle synchronization II: Gear torsion angle designation
Address Decimal point command
Usage Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
42IB-1501277-P
Q Valid Cut amount of deep hole drill cycle Valid Shift amount of back boring Valid Shift amount of fine boring
Invalid Minimum spindle clamp speed Valid Thread cutting start shift angle
Invalid Tool life data management method Invalid Machining condition Invalid Sub part system I: End sequence No. Invalid Droop skip value Invalid R-Navi data input by program: Workpiece registration No. Valid Spindle up-to-speed detection width Valid Thread milling cycle: Dwell time
Invalid Inclined surface machining: Rotation order Invalid Machining interruption: Sequence No. [C80] ,Q Invalid Tool spindle synchronization IB/IC: Rotation ratio designation (Rotary
tool axis) Valid Tool spindle synchronization II: Module or diametral pitch designation
R Valid R-point in the fixed cycle Valid R-specified arc radius Valid Corner R arc radius ,R Valid Offset amount (G10)
Invalid Synchronous tap/asynchronous tap changeover ,R Valid Synchronous tap: Designation of R point position (absolute or incremen-
tal position) Valid Phase shift amount of synchronized spindle Valid Tool spindle synchronization II: Phase shift amount (Workpiece axis) Valid Automatic tool length measurement: Deceleration distance "r" Valid Rotation angle
Invalid Skip acceleration/deceleration time constant Valid Spline interpolation 2: Tolerance (Rotary axis) ,R Valid Tool compensation data input by program/workpiece offset input: Com-
pensation amount Invalid R-Navi data input by program: Marked point No. Valid Involute interpolation: Radius of base circle
Invalid Allowable fluctuation rate of spindle speed S Invalid Spindle function codes
Invalid Maximum spindle clamp speed Invalid Constant surface speed control or constant surface speed cancel: Sur-
face speed Invalid Parameter input by program: word type data 2 bytes Valid Synchronous tap: Designation of spindle rotation speed at the return
Invalid Spindle designation T Invalid Tool function codes U Valid Coordinate position data V Valid Coordinate position data W Valid Coordinate position data
Address Decimal point command
Usage Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
43 IB-1501277-P
(1) Decimal points are all valid in user macro arguments.
(1) Program example of decimal point valid address
(1) If an arithmetic operator is inserted, the data will be handled as data with a decimal point. (Example 1) G00 X123+0 ; This is the X axis 123mm command. It will not be 123 m.
X Valid Coordinate position data Valid Dwell time Valid R-Navi data input by program: Workpiece size Valid R-Navi data input by program/Inclined surface machining: Feature coor-
dinate zero point Y Valid Coordinate position data
Valid R-Navi data input by program: Workpiece size Valid R-Navi data input by program/Inclined surface machining: Feature coor-
dinate zero point Z Valid Coordinate position data
Valid R-Navi data input by program: Workpiece size Valid R-Navi data input by program/Inclined surface machining: Feature coor-
dinate zero point
Program example
Program example Decimal point command 1 Decimal point command 2
When 1 = 1 m When 1 = 10 m 1 = 1 mm
G00 X123.45 (decimal points are all mm points)
X123.450 mm X123.450 mm X123.450 mm
G00 X12345 X12.345 mm (last digit is 1 m unit)
X123.450 mm X12345.000 mm
#111=123 #112=5.55 X#111 Y#112
X123.000 mm Y5.550 mm
X123.000 mm Y5.550 mm
X123.000 mm Y5.550 mm
#113=#111+#112 (addition)
#113=128.550 #113=128.550 #113=128.550
#114=#111-#112 (subtraction)
#114=117.450 #114=117.450 #114=117.450
#115=#111*#112 (multiplication)
#115=682.650 #115=682.650 #115=682.650
#116=#111/#112 #117=#112/#111 (division)
#116=22.162 #117=0.045
#116=22.162 #117=0.045
#116=22.162 #117=0.045
Precautions
Address Decimal point command
Usage Remarks
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
5 Position Commands
44IB-1501277-P
6
45 IB-1501277-P
Interpolation Functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
46IB-1501277-P
6Interpolation Functions 6.1 Positioning (Rapid Traverse); G00
This command is accompanied by coordinate words and performs high-speed positioning of a tool, from the present point (start point) to the end point specified by the coordinate words.
The command addresses are valid for all additional axes.
(1) The rapid traverse speed varies depending on the MTB specifications (parameter "#2001 rapid"). When the "G00 feedrate designation (,F command)" function is enabled and an ",F" command is included in the same block as for the G00 command, positioning is carried out at the feedrate specified by the ",F" command. If this function is invalid or an ",F" command is not designated, positioning is carried out at the feedrate specified in parameter "#2001 rapid".
(2) G00 command belongs to the 01 group and is modal. When G00 command is successively issued, the following blocks can be specified only by the coordinate words.
(3) In the G00 mode, acceleration and deceleration are always carried out at the start point and end point of the block. Before advancing to the next block, a commanded deceleration or an in-position check is conducted at the end point to confirm that the movement is completed for all the moving axes in each part system.
(4) G functions (G72 to G89) in the 09 group are canceled (G80) by the G00 command.
Function and purpose
Command format
Positioning (Rapid Traverse)
G00 X__ Y__ Z____ ,I__ ,F__;
X, Y, Z, Coordinate values. ( is the additional axis.) An absolute position or incremental position is indicated based on the state of G90/ G91 at that time.
,I In-position width. (1 to 999999 ) This address is valid only in the commanded block. A block that does not contain this address will follow the parameter "#1193 inpos" settings. For details, refer to "7.13 Deceleration Check".
,F Specifies the rapid traverse rate of the movement initiated by a G00 command, the movement in the G00 mode, and the movement during the fixed cycle for drilling. The range is equal to the range of the feed per minute F command (mm/min, inch/ min) in the G01 mode. Switching inch/mm is invalid for rotary axes. For details, refer to "7.1.2 G00 Feedrate Command (,F Command)".
Detailed description
CAUTION
The commands with "no value after G" will be handled as "G00".
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
47 IB-1501277-P
Whether the tool moves along a linear or non-linear path varies depending on the MTB specifications (parameter "#1086 G0Intp"). The positioning time does not change according to the path.
(1) Linear path (When parameter "#1086 G0Intp" is set to "0") In the positioning process, a tool follows the shortest path that connects the start point and the end point. The positioning speed is automatically calculated so that the shortest distribution time is obtained in order that the commanded speeds for each axis do not exceed the rapid traverse rate. When, for instance, the X axis and Y axis rapid traverse rates are both 9600 mm/min and when programmed as follows, the tool will follow the path shown in the figure below. G91 G00 X-300000 Y200000; (With an input setting unit of 0.001 mm)
(2) Non-linear path (When parameter "#1086 G0Intp" is set to "1") In positioning, the tool will move along the path from the start point to the end point at the rapid traverse rate of each axis. When, for instance, the X axis and Y axis rapid traverse rates are both 9600 mm/min and when programmed as follows, the tool will follow the path shown in the figure below. G91 G00 X-300000 Y200000; (With an input setting unit of 0.001 mm)
Tool path
(S) Start point (E) End point (fx) Actual X axis rate (fy) Actual Y axis rate
(S) Start point (E) End point (fx) Actual X axis rate (fy) Actual Y axis rate
300
(mm)
(E)
(S)
fy=6400mm/min
Y
X
20 0
fx=9600mm/min
300
(mm)
(E)
(S)
fy=9600mm/min
Y
X
20 0
fx=9600mm/min
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
48IB-1501277-P
There are three methods of carrying out a deceleration check: the command deceleration check method, the smoothing check method, and the in-position check method. The method used for rapid traverse or cutting feed var- ies depends on the MTB specification (combination of parameters "#1306 InpsTyp", "#1389 G1SmthChk", "#1223 aux07/bit1", and "#1193 inpos"). A block with an in-position width command performs an in-position check with a temporarily changed in-position width. (Programmable in-position width command) A block without an in-position width command is processed using the deceleration check method based on the MTB specifications (parameter "#1193 inpos"). During cutting feed and when the error detection is ON, the in-position check is forcibly carried out.
Refer to "7.13 Deceleration Check" for the deceleration check method.
Program example
(S) Start point (E) End point
G91 G00 X-270. Y300. Z150. ;
Precautions for deceleration check
Rapid traverse (G00)
#1193 inpos
0 1
,I com- mand
No Commanded deceleration method (Command- ed deceleration check that varies according to the type of acceleration/deceleration, set in "#2003 smgst" bit3-0)
In-position check method (In-position check by "#2077 G0inps", "#2224 SV024")
Yes In-position check method (In-position check by ",I", "#2077 G0inps", "#2224 SV024")
Cutting feedrate (G01)
#1193 inpos
0 1
,I com- mand
No Commanded deceleration method (Command- ed deceleration check that varies according to the type of acceleration/deceleration, set in "#2003 smgst" bit7-4)
In-position check method (In-position check by "#2078 G1inps", "#2224 SV024")
Yes In-position check method (In-position check by ",I", "#2078 G1inps", "#2224 SV024")
(-120,+200,+300) (E)
(S) (+150,-100,+150)
Y
Z
X
+150
+300
-100
+150
-120
+200
mm
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
49 IB-1501277-P
6.2 Linear Interpolation; G01
This command is accompanied by coordinate words and a feedrate command. It makes the tool move (interpolate) linearly from its current position to the end point specified by the coordinate words at the speed specified by address F. In this case, the feedrate specified by address F always acts as a linear speed in the tool nose center advance direction.
(1) G01 command is a modal command in the 01 group. When G01 command is successively issued, the following blocks can be specified only by the coordinate words. If there is no command, a program error (P62) will occur.
(2) The feedrate for a rotary axis is commanded by /min (decimal point position unit). (F300=300/min) (3) The G functions (G72 to G89) in the 09 group are cancelled (G80) by the G01 command.
This command commands the in-position width for the linear interpolation command from the machining program.
The commanded in-position width is valid in the linear interpolation command only when carrying out deceleration check.
When the error detection switch is ON. When G09 (exact stop check) is commanded in the same block. When G61 (exact stop check mode) is selected.
(1) Refer to section "6.1 Positioning (Rapid Traverse); G00" for details on the in-position check operation.
Function and purpose
Command format
Linear interpolation
G01 X__ Y__ Z__ __ F__ ,I__ ;
X,Y,Z, Coordinate values. ( is the additional axis.) An absolute position or incremental position is indicated based on the state of G90/ G91 at that time.
F Feedrate (mm/min or /min) ,I In-position width. (1 to 999999)
This address is valid only in the commanded block. A block that does not contain this address will follow the parameter "#1193 inpos" settings.
Detailed description
Programmable in-position width command for linear interpolation
G01 X_ Y_ Z_ F_ ,I_ ;
X,Y,Z Linear interpolation coordinate value of each axis F Feedrate ,I In-position width
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
50IB-1501277-P
(Example) Cutting in the sequence of P1 -> P2 -> P3 -> P4 -> P1 at 300mm/min feedrate. However, P0 -> P1 is for tool positioning.
Program example
G91 G00 X20. Y20. ; P0 -> P1 G01 X20. Y30. F300 ; P1 -> P2 X30. ; P2 -> P3 X-20. Y-30. ; P3 -> P4 X-30. ; P4 -> P1
P4 P1
P0
P3P2
20
30
20 20 30
Y
X
(mm)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
51 IB-1501277-P
6.3 Circular Interpolation; G02, G03
These commands serve to move the tool along a circular.
Function and purpose
Command format
Circular interpolation : Clockwise (CW)
G02 X__ Y__ I__ J__ F__ ;
Circular interpolation : Counterclockwise (CCW)
G03 X__ Y__ I__ J__ F__ ;
X,Y Arc end point coordinates I,J Arc center coordinates F Feedrate
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
52IB-1501277-P
(1) For the arc command, the arc end point coordinates are assigned with addresses X, Y (or Z, or parallel axis X, Y, Z), and the arc center coordinate value is assigned with addresses I, J (or K). Either an absolute position or incremental position can be used for the arc end point coordinate value command, but the arc center coordinate value must always be commanded with an incremental position from the start point. The arc center coordinate must be commanded in the input setting unit. Caution is required for the arc command of an axis for which the program command unit differs. Command with a decimal point to avoid confusion.
(2) G02 (G03) is a modal command of the 01 group. When G02 (G03) command is issued continuously, the next block and after can be commanded with only coordinate words. The circular rotation direction is distinguished by G02 and G03. G02 CW (Clockwise) G03 CCW (Counterclockwise)
(3) Select the XY plane, ZX plane or YZ plane to draw an arc on it, using the plane selection G code.
(4) An arc which extends for more than one quadrant can be executed with a single block command. (5) The following information is needed for circular interpolation.
(6) If an R specification and I, K specification are given at the same time in the same block, the circular command with the R specification takes precedence.
Detailed description
G17(X-Y) plane G18(Z-X) plane G19(Y-Z) plane
(a) Plane selection Is there an arc parallel to one of the XY, ZX or YZ planes? (b) Rotation direction Clockwise (G02) or counterclockwise (G03) (c) Arc end point coordi- nates
Set by addresses X, Y, Z.
(d) Arc center coordinates Set by addresses I, J, K. (incremental commands) (e) Feedrate Set by address F
X
Z
Y G03
G03
G03
G02 G02
G02
Y
X
G02
G03
G02
G03
X
Z
G02
G03
Y
Z
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
53 IB-1501277-P
Program error (P33) will occur in general use when the center and radius are not designated at circular command. Depending on the MTB specifications, the linear interpolation can be carried out up to the end point coordinates only in a block with no center coordinates or radius specified (parameter "#11029 Arc to G1 no Cent"). However, a modal is the circular modal. This function is not applied to a circular command by a geometric function.
(Example) #11029 = "1"
Change into linear interpolation command
G90 X0 Y0 ; N1 G02 X20. I10. F500 ; ... (a) N2 G00 X0 ; N3 G02 X20. F500 ; ... (b) M02 ;
(a) The circular interpolation (G02) is executed because there is a center command. (b) The linear interpolation (G01) is executed because there is no center and radius command.
Y
X
N1
N3
200
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
54IB-1501277-P
(Example 1)
(Example 2)
Program example
(S) Start point (E) End point (J) Circle center
G02 J50. F500; Circle command
(S) Start point (E) End point (J) Arc center
G91 G02 X50. Y50. J50. F500; 3/4 command
F = 500mm/min
+Y
+X
J = 50mm
Y
X
(S) / (E)
(J)
F = 500mm/min
+Y
+X
J = 50mm X50Y50mm
(J)
Y
X
(E)
(S)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
55 IB-1501277-P
(1) The terms "clockwise" (G02) and "counterclockwise" (G03) used for circular operations are defined as a case where, in a right-hand coordinate system, the negative direction is viewed from the positive direction of the co- ordinate axis which is at right angles to the plane in question.
(2) If all the end point coordinates are omitted or the end point is at the same position as the start point, commanding the center using I, J and K is the same as commanding a 360arc (perfect circle).
(3) The following occurs when the start and end point radius do not match in a circular command : (a) Program error (P70) results at the circular start point when error R is greater than parameter "#1084 Rad-
Err".
(b) Spiral interpolation in the direction of the commanded end point will be conducted when error R is less than the parameter value.
Also, if "#1084 RadErr" is set to "0", "0.1" is assumed to set.
Precautions
#1084 RadErr parameter value 0.100 Start point radius=5.000 End point radius=4.899 Error R =0.101
(S) Start point (CP) Center point (E) End point (SR) Start point radius (ER) End point radius (AL) Alarm stop
#1084 RadErr parameter value 0.100 Start point radius=5.000 End point radius=4.900 Error R =0.100
(S) Start point (CP) Center point (E) End point (SR) Start point radius (ER) End point radius (SI) Spiral interpolation
(G91) G02 X9.899 I5. ;
R (S)
(AL)
(SR) (ER)
(CP) (E)
(G91) G02 X9.9 I5. ;
R
(SI)
(E)(CP) (S)
(SR) (ER)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
56IB-1501277-P
(c) If the start point radius differs from the end point radius but if the start point angle does not differ from the end point angle, the linear interpolation or spiral interpolation is selected depending on the MTB specifications (pa- rameter "#1278 ext14/bit7").
#1278 ext14/bit7 = 0 Linear interpolation
#1278 ext14/bit7 = 1 Spiral interpolation
G90 G00 X10. Y0.; G02 X10.01 Y0. I-10.01;
G90 G00 X10. Y0.; G02 X10.01 Y0. I-10.01;
(CP) Center point (S) Start point (E) End point
(SR) Start point radius (ER) End point radius (LI) Linear interpolation (SI) Spiral interpolation
(CP) (E)(S)
(SR)
(ER)
(LI)
R
X
Y
(CP) (E)(S)
(SR)
(ER)
R
(SI)
X
Y
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
57 IB-1501277-P
6.4 R Specification Circular Interpolation; G02, G03
Along with the conventional circular interpolation commands based on the circular center coordinate (I, J, K) desig- nation, these commands can also be issued by directly designating the circular radius R.
The arc radius must be commanded in the input setting unit. Caution is required for the arc command of an axis for which the program command unit differs. Command with a decimal point to avoid confusion. A maximum of 6 digits before decimal point can be specified for the radius.
The circular center is on the bisector line which is perpendicular to the line connecting the start and end points of the circular. The point, where the circular with the specified radius whose start point is the center intersects the per- pendicular bisector line, serves as the center coordinates of the circular command. If the R sign of the commanded program is plus, the circular is smaller than a semicircular; if it is minus, the circular is larger than a semicircular.
Function and purpose
Command format
R specification circular interpolation Clockwise (CW)
G02 X__ Y__ R__ F__ ;
R specification circular interpolation Counterclockwise (CCW)
G03 X__ Y__ R__ F__ ;
X X axis end point coordinate Y Y axis end point coordinate R Circular radius F Feedrate
Detailed description
(S) Start point (E) End point (C1): Arc center if R<0 (C2): Arc center if R>0
R < 0
R > 0
(E)
(S)
L
r
(C1)
(C2)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
58IB-1501277-P
The following condition must be met with an R-specified arc interpolation command:
Where L is the line from the start point to the end point. If an R specification and I, J, (K) specification are given at the same time in the same block, the circular command with the R specification takes precedence. In the case of a full-circle command (where the start and end points coincide), an R specification circular command will be completed immediately even if it is issued and no operation will be executed. An I, J, (K) specification circular command should therefore be used in such a case. The plane selection command is the same as the I, J, or K specification circular command.
When "the error margin between the segment connecting the start and end points" and "the commanded radius 2" is less than the setting value because the required semicircle is not obtained by calculation error in R specification circular interpolation, "the midpoint of the segment connecting the start and end points" is compensated for as the circular center. The setting value depends on the MTB specifications (parameter "#11028 Tolerance Arc Cent" (Tolerable correction value of arc center error)).
(Example) #11028 = "0.000 (mm)"
Calculation error margin compensation allowance value: 0.002 mm Segment connecting the start and end points: 10.000 N3: Radius 2 = 10.002 "Error 0.002 -> Compensate" N5: Radius 2 = 10.004 "Error 0.004 -> Do not compensate"
When (L/2 - r) > (parameter : #1084 RadErr), an alarm will occur.
Circular center coordinate compensation
Setting value Tolerance value
Setting value < 0 0 (Center error will not be interpolated) Setting value = 0 2minimum setting increment Setting value > 0 Setting value
G90 X0 Y0 ; N1 G02 X10. R5.000; N2 G00 X0; N3 G02 X10. R5.001; ...(a) N4 G00 X0; N5 G02 X10. R5.002; ...(b) N6 G00 X0; M02 ;
(a) Compensate the center coordinate: Same as N1 path (b) Do not compensate the center coordinate: Inside path a little than N1
L 12 r
N1, N3
N5
100 X
Y
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
59 IB-1501277-P
(Example 1)
(Example 2)
(Example 3)
(Example 4)
(1) In the case of a full-circle command (where the start and end points coincide), an R specification circular com- mand will be completed immediately even if it is issued and no operation will be executed. An I, J, K specification circular command should therefore be used in such a case.
(2) If an R specification and I, K specification are given at the same time in the same block, the circular command with the R specification takes precedence.
Program example
G02 Xx1 Yy1 Rr1 Ff1 ; XY plane R-specified arc
G03 Zz1 Xx1 Rr1 Ff1 ; R specification circular on Z-X plane
G02 Xx1 Yy1 Ii1 Jj1 Rr1 Ff1 ; XY plane R-specified arc (When the R specification and I, J, (K) specification are contained in the same block, the circular command with the R specification takes precedence.)
G17 G02 Ii1 Jj1 Rr1 Ff1 ; XY plane This is an R-specified arc, but as this is a circle command, it will be completed immediately.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
60IB-1501277-P
6.5 Plane Selection; G17, G18, G19
The plane to which the movement of the tool during the circle interpolation (including helical cutting) and tool radius compensation command belongs is selected. If the 3 basic axes and the parallel axes corresponding to these basic axes are entered as parameters, the com- mands can select the plane composed of any 2 axes which are not parallel axes. If a rotary axis is entered as a parallel axis, the commands can select the plane containing the rotary axis. These commands are used to select following planes:
Plane that executes circular interpolation (including helical cutting) Plane that executes tool radius compensation Used to select a plane that executes fixed cycle positioning.
X, Y and Z indicate each coordinate axis or the parallel axis.
Table 1 Examples of plane selection parameter entry
As shown in the above example, the basic axis and its parallel axis can be registered. The basic axis can be an axis other than X, Y and Z. Axes that are not registered are irrelevant to the plane selection.
Function and purpose
Command format
G17 ; X-Y plane selection
G18 ; Z-X plane selection
G19 ; Y-Z plane selection
Detailed description
Parameter entry
#1026-1028 #1029-1031
Basic axis I, J, K Flat axis I, J, K
I X U J Y K Z V
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
61 IB-1501277-P
In Table 1, characters I, J, K represent the following axes. I: Horizontal axis for the G17 plane or the vertical axis for the G18 plane J: Vertical axis for the G17 plane or horizontal axis for the G19 plane K: Horizontal axis for the G18 plane or vertical axis for the G19 plane Therefore, the G17, G18 and G19 commands select the following planes. G17: I-J plane G18: K-I plane G19: J-K plane
(1) Axis addresses assigned in the same block as the plane selection (G17, G18, G19) command determine which of the basic axes or parallel axes are to be in the actual plane selected. For the parameter entry example in Table 1
(2) Plane selection is not performed with blocks in which the plane selection G code (G17, G18, G19) is not as- signed.
(3) If the axis address is omitted in the block where the plane selection G code (G17, G18, G19) is commanded, it is assumed that the axis addresses of the 3 basic axes have been omitted. For the parameter entry example in Table 1
(4) When the axis addresses are commanded to the same block as the plane selection G code (G17, G18, G19), the commanded axes will travel.
(5) The axis command that does not exist in the plane determined by the plane selection G code (G17, G18, G19) is irrelevant to the plane selection. For the parameter entry example in Table 1, if the command is issued as below, the U-Y plane will be selected and "Z" will move regardless of the plane.
(6) When the basic axes or their parallel axes are duplicated and assigned in the same block as the plane selection G code (G17, G18, G19), the plane is determined in the order of basic axes, and then parallel axes. For the parameter entry example in Table 1, if the command is issued as below, the U-Y plane will be selected and "W" will move regardless of the plane.
When the power is turned ON or when the system is reset, the plane set by the parameter "#1025 Initial plane selection" is selected.
Plane selection system
G17 X__ Y__ ; X-Y plane G18 X__ V__ ; V-X plane G18 U__ V__ ; V-U plane G19 Y__ Z__ ; Y-Z plane G19 Y__ V__ ; Y-V plane
G17 X__ Y__ ; X-Y plane Y__ Z__ ; X-Y plane (No plane change)
G17 ; X-Y plane G17 U__ ; U-Y plane G18 U__ ; Z-U plane G18 V__ ; V-X plane G19 Y__ ; Y-Z plane G19 V__ ; Y-V plane
G17 U__Z__ ;
G17 U__Y__W__ ;
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
62IB-1501277-P
6.6 Thread Cutting
6.6.1 Constant Lead Thread Cutting; G33
The G33 command exercises feed control over the tool which is synchronized with the spindle rotation and so this makes it possible to conduct constant-lead straight thread-cutting, and tapered thread-cutting. Multiple thread screws, etc., can also be machined by designating the thread cutting angle.
(1) The E command is also used for the number of ridges in inch thread cutting, and whether the number of ridges or precision lead is to be designated can be selected by parameter setting. (Parameter "#8156 Fine thread cut E" is set to "1" for precision lead designation.)
(2) The lead in the long axis direction is commanded for the taper thread lead.
Function and purpose
Command format
Normal lead thread cutting
G33 Z__(X__ Y__ __) F__ Q__ ;
Z (X Y ) End point of thread cutting F Lead of long axis (axis which moves most) direction Q Thread cutting start shift angle (0.001 - 360.000)
Precision lead thread cutting
G33 Z__(X__ Y__ __) E__ Q__ ;
Z (X Y ) End point of thread cutting E Lead of long axis (axis which moves most) direction Q Thread cutting start shift angle (0.001 - 360.000)
Detailed description
(t) Tapered thread section
When a < 45, lead is in LZ direction. When a > 45, lead is in LX direction. When a = 45, lead can be in either LZ or LX direc- tion.
LZ
Z
XLX
a
(t)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
63 IB-1501277-P
Thread cutting metric input
Thread cutting inch input
imum cutting feedrate. (3) The constant surface speed control function should not be used for taper thread cutting commands or scrolled
thread cutting commands. (4) The spindle rotation speed should be kept constant throughout from the rough cutting until the finishing. (5) If the feed hold function is employed during thread cutting to stop the feed, the thread ridges will lose their shape.
For this reason, feed hold does not function during thread cutting. Note that this is valid from the time the thread cutting command is executed to the time the axis moves. If the feed hold switch is pressed during thread cutting, block stop will occur at the end point of the block following the block in which thread cutting is completed (no longer G33 mode).
Input Setting unit
B (0.001 mm) C (0.0001 mm)
Command address
F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)
Minimum command unit
1 (=0.001) (1.=1.000)
1 (=0.0001) (1.=1.0000)
1 (=1.00) (1.=1.00)
1 (=0.0001) (1.=1.0000)
1 (=0.00001) (1.=1.00000)
1 (=1.000) (1.=1.000)
Range 0.001 - 999.999
0.0001 - 999.9999
0.03 - 999.99
0.0001 - 999.9999
0.00001 - 999.99999
0.026 - 222807.017
Input Setting unit
D (0.00001 mm) E (0.000001 mm)
Command address
F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)
Minimum command unit
1 (=0.00001) (1.=1.00000)
1 (=0.000001) (1.=1.000000)
1 (=1.0000) (1.=1.0000)
1 (=0.000001) (1.=1.000000)
1 (=0.0000001) (1.=1.0000000)
1 (=1.00000) (1.=1.00000)
Range 0.00001 - 999.99999
0.000001 - 999.999999
0.0255 - 224580.0000
0.000001 - 999.999999
0.0000001 - 999.9999999
0.02541 - 224719.00000
Input Setting unit
B (0.0001 inch) C (0.00001 inch)
Command address
F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)
Minimum command unit
1 (=0.0001) (1.=1.0000)
1 (=0.00001) (1.=1.00000)
1 (=1.000) (1.=1.000)
1 (=0.00001) (1.=1.00000)
1 (=0.000001) (1.=1.000000)
1 (=1.0000) (1.=1.0000)
Range 0.0001 - 39.3700
0.00001 - 39.37007
0.025 - 9999.999
0.00001 - 39.37007
0.000001 - 39.370078
0.0255 - 9999.9999
Input Setting unit
D (0.000001 inch) E (0.0000001 inch)
Command address
F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)
Minimum command unit
1 (=0.000001) (1.=1.000000)
1 (=0.0000001) (1.=1.0000000)
1 (=1.00000) (1.=1.00000)
1 (=0.0000001) (1.=1.0000000)
1 (=0.00000001) (1.=1.00000000)
1 (=1.000000) (1.=1.000000)
Range 0.000001 - 39.370078
0.0000001 - 39.3700787
0.02541 - 9999.99999
0.0000001 - 39.3700787
0.00000001 - 39.37007873
0.025401 - 9999.999999
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
64IB-1501277-P
(6) The converted cutting feedrate is compared with the cutting feed clamp rate when thread cutting starts, and if it is found to exceed the clamp rate, an operation error will occur.
(7) In order to protect the lead during thread cutting, a cutting feedrate which has been converted may sometimes exceed the cutting feed clamp rate.
(8) An illegal lead is normally produced at the start of the thread and at the end of the cutting because of servo sys- tem delay and other such factors. Therefore, it is necessary to command a thread length which is determined by adding the illegal lead lengths to the required thread length.
(9) The spindle rotation speed is subject to the following restriction: 1 <= R <= Maximum feedrate/Thread lead
Where R <= Tolerable speed of encoder (r/min) R: Spindle rotation speed (r/min) Thread lead = mm or inches Maximum feedrate= mm/min or inch/mim (this is subject to the restrictions imposed by the machine specifica- tions.)
(10) A program error (P93) may occur when the result of the expression (9) is R<1 because the thread lead is very large to the highest cutting feedrate.
(11) Dry run is valid for thread cutting but the feedrate based on dry run is not synchronized with the spindle rotation. The dry run signal is checked at the start of thread cutting and any switching during thread cutting is ignored.
(12) Synchronous feed applies for the thread cutting commands even with an asynchronous feed command (G94). (13) Spindle override and cutting feed override are invalid and the speeds are fixed to 100% during thread cutting. (14) When a thread cutting is commanded during tool radius compensation, the compensation is temporarily can-
celed and the thread cutting is executed. (15) When the mode is switched to another automatic mode while G33 is executed, the following block which does
not contain a thread cutting command is first executed and then the automatic operation stops. (16) When the mode is switched to the manual mode while G33 is executed, the following block which does not con-
tain a thread cutting command is first executed and then the automatic operation stops. In the case of a single block, the following block which does not contain a thread cutting command (G33 mode is canceled) is first ex- ecuted and then the automatic operation stops. Note that automatic operation is stopped until the G33 command axis starts moving.
(17) The thread cutting command waits for the single rotation synchronization signal of the rotary encoder and starts movement. Make sure to carry out timing synchronization operation between part systems before issuing a thread cutting command with multiple part systems. For example, when using the 1-spindle specifications with two part sys- tems, if one part system issues a thread cutting command during ongoing thread cutting by another part system, the movement will start without waiting for the rotary encoder single rotation synchronization signal causing an illegal operation.
(18) The thread cutting start shift angle is not modal. If there is no Q command with G33, this will be handled as "Q0". (19) The automatic handle interrupt/interruption is valid during thread cutting. (20) If a value exceeding 360.000 is command in G33 Q, a program error (P35) will occur. (21) G33 cuts one row with one cycle. To cut two rows, change the Q value, and issue the same command.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
65 IB-1501277-P
Program example
N110 G90 G00 X-200. Y-200. S50 M3 ; The spindle center is positioned to the workpiece center, and the spin- dle rotates in the forward direction.N111 Z110 ;
N112 G33; Z40 F6.0; The first thread cutting is executed. Thread lead = 6.0mm N113 M19 ; Spindle orientation is executed with the M19 command. N114 G00 X-210.; The tool is evaded in the X axis direction. N115 Z110. M0 ; The tool rises to the top of the workpiece, and the program stops with
M00. Adjust the tool if required.
N116 X-200. ; M3 ;
Preparation for second thread cutting is done.
N117 G04 X5.0 ; Command dwell to stabilize the spindle rotation if necessary. N118 G33 Z40.; The second thread cutting is executed.
Z
X Y
X
10
50
10
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
66IB-1501277-P
6.6.2 Inch Thread Cutting; G33
If the number of ridges per inch in the long axis direction is assigned in the G33 command, the feed of the tool syn- chronized with the spindle rotation will be controlled, which means that constant-lead straight thread-cutting and ta- pered thread-cutting can be performed.
(1) The number of ridges in the long axis direction is assigned as the number of ridges per inch. (2) The E code is also used to assign the precision lead length, and whether the number of ridges or precision lead
length is to be designated can be selected by parameter setting. (The number of ridges is designated by setting the parameter "#8156 Fine thread cut E" to "0".)
(3) The E command value should be set within the lead value range when converted to lead. (4) See Section "Constant lead thread cutting" for other details.
Function and purpose
Command format
Inch thread cutting
G33 Z__ (X_ Y_ _) E__ Q__ ;
Z (X Y ) End point of thread cutting E Number of ridges per inch in direction of long axis (axis which moves most) (decimal
point command can also be assigned) Q Thread cutting start shift angle, 0.001 to 360.000
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
67 IB-1501277-P
Thread lead: 3 threads/inch (= about 8.4666)
When programmed with 1= 10 mm, 2=10 mm using metric input
Program example
N210 G90 G00 X-200. Y-200. S50 M3 ; N211 Z110. ; N212 G91 G33 Z-70. E3.0 ; (First thread cutting) N213 M19; N214 G90 G00 X-210. ; N215 Z110. M0 ; N216 X-200. ;
M3 ; N217 G04 X2.0 ; N218 G91 G33 Z-70. ; (Second thread cutting)
Z
XY
X
1 50.0mm
2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
68IB-1501277-P
6.7 Helical Interpolation; G02, G03
When this interpolation is performed with 3 orthogonal axes, the tool will travel helically when circular interpolation is executed for any 2 axes and, at the same time, when another 1 axis is synchronized with the rotation of the circular and linear interpolation is executed synchronously with the rotation of the circular arc. This command must be issued as the combination of the circular interpolation command with the height axis.
Function and purpose
Program command path XY plane projection path
(S) Start point (E) End point
Program command path
Circular interpolation components
Linear interpolation components
Z
Y(S)
(E)
X
Y
X
(E)
(S)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
69 IB-1501277-P
(1) In this manual, the following setting descriptions are used. I axis: X; J axis: Y; K axis: Z (2) The arc center coordinates and arc radius value must be commanded in the input setting unit. Caution is required
for the helical interpolation command of an axis for which the program command unit differs. Command with a decimal point to avoid confusion.
(3) Either an absolute command or incremental command can be used for the arc end point coordinate value com- mand and the linear axis end point coordinate value command, but the arc center coordinates must always be designated with an incremental position from the start point.
(4) If a pitch command is issued with the ",P" address, a program error (P33) occurs. (5) If the number of pitches is "0", address P can be omitted. (6) If the radius (R) is designated, the number of pitches is ignored even when it is commanded. (7) Two or more axes can be designated for the linear interpolation axis.
Command format
Helical interpolation command (Specify arc center)
G17 G02/G03 X_ Y_ Z_ I_ J_ P_ F_ ;
G18 G02/G03 Z_ X_ Y_ K_ I_ P_ F_ ;
G19 G02/G03 Y_ Z_ X_ J_ K_ P_ F_ ;
Helical interpolation command (Specify radius (R))
G17 G02/G03 X_ Y_ Z_ R_ F_ ;
G18 G02/G03 Z_ X_ Y_ R_ F_ ;
G19 G02/G03 Y_ Z_ X_ R_ F_ ;
G17, G18, G19 Arc plane G17: XY plane G18: ZX plane G19: YZ plane
G02/G03 Arc rotation direction G02: Clockwise G03: Counterclockwise
X, Y, Z Arc end point coordinates: (X, Y) is set in G17, (Z, X) in G18, and (Y, Z) in G19. Linear axis end point coordinates: Z is set in G17, Y in G18, and X in G19.
I, J, K Arc center coordinates: (I, J) is set in G17, (K, I) in G18, and (J, K) in G19.
P Number of pitches R Circular arc radius F Feedrate
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
70IB-1501277-P
Speed designation "F" during the helical interpolation has the following types. The available type depends on the MTB specifications.
Command the feedrate F as the resultant speed for each axis.
If speed designation by the arc plane component is selected, the F command will be handled as modal data in the same manner as the normal F command. This will also apply to the following G01, G02 and G03 commands. For example, the program will be as follows.
When the speed designation by the arc plane component is selected, only the helical interpolation speed command is converted to the speed commanded with the arc plane component and operates. The other linear and arc com- mands operate as normal speed commands.
(1) The actual feedrate display (Fc) indicates the tangent component of the helical interpolation. (2) The modal value speed display (FA) indicates the command speed. (3) This function is valid only when feed per minute (asynchronous feed: G94) is selected. If feed per revolution (syn-
chronous feed: G95) is selected, the arc plane component speed will not be designated.
Detailed description
Speed designation during the helical interpolation
Parameter #1235/bit0 Tangent speed (command value of address "F")
0 Speed designation for normal helical interpolation Commands the tangent speed (equivalent to "fb" in the lower-right figure) in- cluding interpolation component of the 3rd axis.
1 Speed designation by the arc plane component Commands the tangent speed (equivalent to "fa" in the lower-left figure) in the arc plane. At this time, the NC automatically calculates the helical interpolation tangent speed "fb" so that the tangent speed on the arc plane is "fa".
(S) Start point (E) End point fa: Tangent speed in arc plane fb: Helical interpolation tangent speed
Speed designation by the arc plane component
G17 G91 G02 X10. Y10. Z-4. I10. F100 ; Helical interpolation is performed with such speed that arc plane component is F100.
G01 X20. ; Linear interpolation is performed at the speed of F100. G02 X10. Y-10. Z4. J10. ; Helical interpolation is performed with such speed that arc plane
component is F100. G01 Y-40. F120 ; Linear interpolation is performed at the speed of F120. G02 X-10. Y-10. Z-4. I-10. ; Helical interpolation is performed with such speed that arc plane
component is F120. G01 X-20. ; Linear interpolation is performed at the speed of F120.
fa
Y
X (S)
(E)
Y
Z
X
fb
(S)
(E)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
71 IB-1501277-P
(1) Pitch "L" is obtained with the following expression.
xs, ys: Distance from the arc center to the start point (each of X and Y axes)
xe, ye: Distance from the arc center to the end point (each of X and Y axes)
(2) If pitch No. is "0", address "P" can be omitted.
The pitch No. designation ("P" command) cannot be made with the R-specified arc.
The helical interpolation arc plane selection is determined with the plane selection mode and axis address in the same manner as the circular interpolation. For the helical interpolation command, the plane where circular interpo- lation is executed is required to be commanded with the plane selection G code (G17, G18, G19), and two circular interpolation axes and three linear interpolation axes (axes which perpendicular to the arc plane) are required to be commanded.
X-Y plane circular, Z axis linear Command the X, Y and Z axis addresses in the G02 (G03) and G17 (plane selection G code) mode.
Z-X plane circular, Y axis linear Command the Z, X and Y axis addresses in the G02 (G03) and G18 (plane selection G code) mode.
Y-Z plane circular, X axis linear Command the Y, Z and X axis addresses in the G02 (G03) and G19 (plane selection G code) mode.
The plane for an additional axis can be selected as with circular interpolation.
Number of pitches
(S) Start point (E) End point
Plane selection
Z
Y
X
L
P
Z
Y
X
(E)
(S)
e
s2
1
L =
= e - s = tan - 1 - tan - 1 ( )0 < 2 ysye
xsxe
P + /2 Z
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
72IB-1501277-P
(1) When executing helical interpolation, issue the circular interpolation command and another linear axis command (several axes can be commanded) that does not contain the arc axis.
(2) The number of axes that can be commanded simultaneously is less than or equal to the number of simultaneous contouring control axes.
(3) With helical interpolation, the axes that configure the plane are the circular interpolation axes, and the other axis is the linear interpolation axis.
(4) The movement of the linear interpolation axis is stopped and only the circular interpolation axes operate during the corner chamfering or corner rounding commands.
(5) Refer to description of "6.3 Circular Interpolation; G02, G03" for other precautions.
Precautions and restrictions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
73 IB-1501277-P
6.8 Unidirectional Positioning
The unidirectional positioning function positions the tool at a high degree of precision without backlash error by lo- cating the final tool position from a constant direction. There are two types of positioning methods: G command method (G60 use method) and axis-based unidirectional positioning method (in which the axis specified by the MTB is always targeted for unidirectional positioning). For the specifications of the machine you are using, see the specifications or Instruction Manual issued by the MTB.
6.8.1 Unidirectional Positioning; G60
The G60 command can position the tool at a high degree of precision without backlash error by locating the final tool position from a constant direction.
(1) The creep distance for the final positioning as well as the final positioning direction is set by parameter.
(2) After the tool has moved at the rapid traverse rate to the position separated from the final position by an amount equivalent to the creep distance, it moves to the final position in accordance with the rapid traverse setting where its positioning is completed.
(3) The above positioning operation is performed even when Z axis commands have been assigned for Z axis cancel and machine lock. (Display only)
(4) When the mirror image function is ON, the tool will move in the opposite direction as far as the intermediate po- sition due to the mirror image function but the operation within the creep distance during its final advance will not be affected by a mirror image.
(5) The tool moves to the end point at the dry run speed during dry run when the G00 dry run function is valid.
Function and purpose
Command format
G60 X__ Y__ Z__ __; ... Unidirectional positioning
Additional axis
Detailed description
- +
G60a
G60 - a
End point Start point
Start point
Final advance direction
G60 creep distance
Positioning position
Stop once
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
74IB-1501277-P
(6) Feed during creep distance movement with final positioning can be stopped by resetting, emergency stop, inter- lock, feed hold and rapid traverse override zero. The tool moves over the creep distance at the rapid traverse setting. Rapid traverse override is valid.
(7) Unidirectional positioning is not performed for the drilling axis during fixed cycle for drilling.
(8) Unidirectional positioning is not performed for shift amount movements during the fine boring or back boring fixed cycle.
(9) Normal positioning is performed for axes whose creep distance has not been set by parameter.
(10) Unidirectional positioning is always a non-interpolation type of positioning.
(11) When the same position (movement amount of zero) has been commanded, the tool moves back and forth over the creep distance and is positioned at its original position from the final advance direction.
(12) Program error (P61) will occur when the G60 command is assigned with an NC system which has not been provided with this particular specification.
(13) The G60 command is assigned to group 00 (unmodal) in the previous versions; however, it can be operated as the modal G code of group 01 depending on the MTB specifications (parameter "#1271 ext07/bit3"). This omits a step to command G60 for each block. This G60 command is the same as the previous unmodal G60 command, except it handles the G60 command as a modal.
(14) If the G code of group 01 is commanded in the same block when the G60 command is handled as a modal, the G code commanded next becomes valid.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
75 IB-1501277-P
6.8.2 Axis-based Unidirectional Positioning
This function carries out unidirectional positioning for each axis for G00 positioning. The target axis is determined in the MTB specifications (parameter "#2084 G60_ax"). When the unidirectional positioning is commanded, set the last positioning direction and distance to parameter "#8209 G60 shift amount" for each axis. The example below shows a case in which axis B is set as the unidirectional positioning axis.
The axis-based unidirectional positioning is the same as for the G60 command. Refer to "6.8.1 Unidirectional Posi- tioning; G60".
Function and purpose
G00 X100.; Normal positioning G00 B100.; Unidirectional positioning G00X200.B200.; Axis X: Normal positioning, Axis B: Unidirectional positioning
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
76IB-1501277-P
6.9 Cylindrical Interpolation; G07.1
This function develops a shape on the side of a cylinder (shape in a cylindrical coordinate system) into a plane. When the developed shape is programmed as the plane coordinates, it will be converted into a linear axis movement and rotation axis (temporarily, "B axis") movement in the original cylindrical coordinates to conduct contour control when machining.
As programming can be carried out to the developed shape of the side of the cylinder, this is effective for machining cylindrical cams, etc. When programmed with the rotary axis and its orthogonal axis, grooves and other shapes can be machined on the side of the cylinder.
Function and purpose
Command format
Cylindrical interpolation mode start
G07.1 Rotary axis name, rotation radius value;
G107 Rotary axis name, rotation radius value;
Rotary axis name Axis name assigned to rotary axis Rotation radius value Command a value other than "0".
When a value other than "0" is commanded, the cylindrical interpolation mode starts.
Cylindrical interpolation mode cancel
G07.1 Rotary axis name 0;
G107 Rotary axis name 0;
r
B
Z
X
Y
0
360
2 r
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
77 IB-1501277-P
(1) The cylindrical interpolation is carried out between the rotary axis designated in the G07.1 block and another linear axis. (The following example shows a case in which the rotary axis name is set to "C".)
(2) G107 can be used instead of G07.1. (3) Command G07.1 alone in a block. If it is commanded in the same block with other G code, a program error (P33)
will occur. (4) The cylindrical interpolation mode is canceled when the power is turned ON or at resetting. (5) Linear interpolation or circular interpolation can be commanded during the cylindrical interpolation mode. Note
that the plane selection command must be issued just before or after the G07.1 block. (6) The coordinate commands can be both an absolute command or incremental command. (7) Tool radius compensation can be applied on the program command. Cylindrical interpolation will be executed to
the path after it has gone through a tool radius compensation. (8) Command the tangent speed on the developed cylinder by F. F is in mm/min or inch/min unit. (9) A program error (P484) will occur if any axis commanded during cylindrical interpolation has not completed the
reference position return. (10) The deceleration check is made for the cylindrical interpolation start command block.
In the cylindrical interpolation mode, the movement amount of the rotary axis commanded with an angle is converted into distance on a circle periphery, and after calculating the linear and circular interpolation between the other axes, the amount is converted into an angle again. Thus, the actual movement amount may differ from the commanded value such as when the cylinder radius is small. Note that the gap generated by this will not be cumulated.
(1) To cancel the cylindrical interpolation mode, the following condition must be satisfied. Tool radius compensation is canceled.
(2) When the cylindrical interpolation mode is canceled, the plane selected before the cylindrical interpolation will be restored.
(3) The deceleration check is made for the cylindrical interpolation cancel command block.
Detailed description
G19 ; Plane selection G07.1 C20. ; Cylindrical interpolation mode start (Cylindrical interpolation will start.)
: (The coordinate commands in this interval will be the cylindrical coordinate system) G07.1 C0 ; Cylindrical interpolation mode cancel (Cylindrical interpolation will be canceled.)
Cylindrical interpolation accuracy
Cylindrical interpolation mode cancel
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
78IB-1501277-P
The axis used for cylindrical interpolation must be set with the plane selection command.
Use parameters (#1029, #1030 and #1031) to set which parallel axis corresponds to the rotary axis. The circular interpolation and tool radius compensation, etc., can be designated on that plane. The plane selection command is set immediately before or after the G07.1 command. If a movement command is issued without this command, a program error (P485) will occur.
(Example)
Plane selection
G19 Z0. C0. ; Plane selection command for cylindrical interpolation, and 2-axis com- mand of Z axis and C axis for interpolation
G07.1 C100. ; Cylindrical interpolation start :
G07.1 C0 ; Cylindrical interpolation cancel
Basic coordinate system X,Y,Z
Cylindrical coordinate system C , Y , Z (Rotary axis is X axis' par- allel axis) #1029
Cylindrical coordinate system X , C , Z (Rotary axis is Y axis' par- allel axis) #1030
Cylindrical coordinate system X , Y , C (Rotary axis is Z axis' par- allel axis) #1031
G17
Y
X
G18
Z
X
G19
Y
Z
G18
Z
C
G17
C
Y
G19
C
Z
G17
X
C
G18
C
X
G19
Y
C
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
79 IB-1501277-P
Program example
N01 G28 XZC ; N02 T0202 F500 ; N03 G97 S100 M23 ; N04 G00 X50. Z0. ; N05 G94 G01 X40. F100. ; N06 G19 C0 Z0 ; Plane selection command for cylindrical interpolation and two axes
command for interpolation N07 G07.1 C20. ; Cylindrical interpolation start N08 G41 ; N09 G01 Z-10. C80. F150 ; N10 Z-25. C90. ; N11 Z-80. C225. ; N12 G03 Z-75.C270. R55. ; N13 G01 Z-25. ; N14 G02 Z-20.C280. R80. ; N15 G01 C360. ; N16 G40 ; N17 G07.1 C0 ; Cylindrical interpolation cancel N18 G01 X50. ; N19 G00 X100. Z100. ; N20 M25 ; N21 M30 ;
#1029 aux_I #1030 aux_J C #1031 aux_K
50
100
150
200
250
300
350
-20-40-60-80
C
Z
N09N10
N11
N12 N13
N14
N15
(mm)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
80IB-1501277-P
(1) Circular interpolation between the rotary axis and linear axis is possible during the cylindrical interpolation mode. (2) Only the R specification command (mm/inch) is available for circular interpolation. (I, J and K cannot be desig-
nated.)
The tool radius can be compensated during the cylindrical interpolation mode.
(1) Command the plane selection in the same manner as circular interpolation. When using tool radius compensation, start up/cancel the compensation in the cylindrical interpolation mode.
(2) A program error (P485) will occur if G07.1 is commanded during tool radius compensation. (3) If the G07.1 command is issued with no movement command after the tool radius compensation has been can-
celed by commanding G40 alone, the position of the axis in the G07.1 command block is interpreted as the po- sition applied after the tool radius compensation has been canceled and the following operations are performed.
(1) The miscellaneous functions (M) and 2nd miscellaneous functions (B) can be issued in the cylindrical interpola- tion mode.
(2) The S command in the cylindrical interpolation mode specifies the rotary tool's rotation speed instead of the spin- dle rotation speed.
(1) Program error (P481) will occur if tool length compensation is performed in the cylindrical interpolation mode.
(2) Complete the tool compensation operation (movement of tool length and wear compensation amount) before executing the cylindrical interpolation. If the tool compensation operation is not completed when the cylindrical interpolation start command is issued, the followings will occur: The workpiece coordinate system shifts so that the relationship between the machine coordinate position and workpiece coordinate position matches the "positional relationship after the tool compensation has been com- pleted" without actually moving the axis. The workpiece coordinate system shifted here is not reset even if the cylindrical interpolation is canceled. The subsequent operations are performed, assuming that the tool compensation operation has been completed.
Relationship with other functions
Circular interpolation
Tool radius compensation/tool nose radius compensation
Miscellaneous functions
Tool length compensation
: G43 H12 ; G00 X100. Z0. ; G19 Z C ; G07.1 C100. ;
Tool length compensation before cylindrical interpolation -> Valid
: G43 H11 ; Tool length compensation in cylindrical interpolation mode -> Program error
: G07.1 C0 ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
81 IB-1501277-P
The operation varies depending on whether the synchronous feed is valid or invalid during cylindrical interpolation. Whether the synchronous feed is valid or invalid depends on the MTB specifications (parameter "#1293 ext29"/bit0).
(1) When the synchronous feed is invalid (#1293 ext29/bit0 = 0): Only the asynchronous feed is valid during the cylindrical interpolation mode. If the synchronous feed command (G95) is issued during the cylindrical interpolation mode, a program error (P481) will occur. The operation to be performed when the cylindrical interpolation mode is started or canceled varies depending on the feed mode that is specified before the cylindrical interpolation mode is started.
(2) When the synchronous feed is valid (#1293 ext29/bit0 = 1): Both the synchronous feed and asynchronous feed are valid during the cylindrical interpolation mode. The feed mode and feedrate remain unchanged and take over the previous state when the cylindrical interpola- tion mode is started or canceled.
In the cylindrical coordinate system of the rotary axis for cylindrical interpolation, the coordinate positions depend on the MTB specifications (#1270 ext06/bit7).
Feed mode and F command before and after cylindrical interpolation mode
Feed mode before start
Operation in cylindrical interpolation mode (At start/cancel)
Asynchronous feed (G94)
The previous feed mode (asynchronous feed) and the feedrate designated with the F command are inherited when the cylindrical interpolation mode is started or canceled.
Synchronous feed (G95)
When the cylindrical interpolation mode is started, the asynchronous mode is enabled forcibly, and the feedrate is canceled. After the cylindrical interpolation mode has been started, designate the feedrate using the F command. A program error (P62) will occur if the F command is not designated. When the cylindrical interpolation mode is canceled, the setting returns to the feed mode (synchronous feed) and feedrate before the cylindrical interpolation mode starts.
Synchronous feed function valid/invalid (#1293 bit0)
Change of feed mode and feedrate
Before the cylindrical in- terpolation mode starts
When the cylindrical inter- polation mode starts
When the cylindrical interpo- lation mode is canceled
Invalid Asynchronous feed Asynchronous feed Asynchronous feed Feedrate just before start Feedrate just before cancel
Synchronous feed Asynchronous feed Synchronous feed Feedrate = 0 (Cancel) Feedrate before cylindrical in-
terpolation starts Valid Asynchronous feed Asynchronous feed Feed mode just before the
mode is canceled Feedrate just before start Feedrate just before cancel
Synchronous feed Synchronous feed Feedrate just before start
Cylindrical interpolation coordinate system
Parameter set- ting
(#1270 bit7)
Coordinate position of rotary axis in cylindrical coordinate system
0 In this coordinate system, the rotary axis position is set to "0" when the cylindrical interpo- lation start command is issued.
1 The workpiece coordinate positions just before the cylindrical interpolation starts are also continued to be used during cylindrical interpolation.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
82IB-1501277-P
The following G code commands can be used during the cylindrical interpolation mode.
A program error will occur if a G code other than those listed above is commanded during cylindrical interpolation.
[Combination of cylindrical interpolation and high-accuracy control function]
To enable the G08P1 or G61.1 (high-accuracy control) mode during the G07.1 (cylindrical interpolation) or G12.1 (polar coordinate interpolation) mode or to enable the G07.1 (cylindrical interpolation) or G12.1 (polar coordinate interpolation) mode during the G08P1 or G61.1 (high-accuracy control) mode, you need to enable the axis-spe- cific acceleration tolerance control (optimum acceleration control) or variable-acceleration pre-interpolation ac- celeration/deceleration. (The validity of these functions depends on the MTB specifications.) If the cylindrical interpolation or polar coordinate interpolation command is issued during the high-accuracy con- trol mode while the functions above are invalid, a program error (P126) will occur. Also, if the high-accuracy control command is issued during the cylindrical interpolation or polar coordinate in- terpolation mode, a program error (P481) will occur.
(1) The cylindrical interpolation mode is canceled when the power is turned ON or reset. (2) Program cannot be restarted (program restart) when the block is in the cylindrical interpolation. (3) The cylindrical interpolation command cannot be issued in mirror image (parameter/external input ON). If the
command is issued, a program error (P486) will occur. (4) A program error (P481) will occur if the cylindrical interpolation command (G07.1), the polar coordinate interpo-
lation command (G12.1), or the milling interpolation command (G12.1) is issued again during the cylindrical in- terpolation mode.
Cylindrical interpolation function: Combinations of G code commands
G code Description
G00 Positioning G01 Linear interpolation G02 Circular interpolation (CW) G03 Circular interpolation (CCW) G04 Dwell G09 Exact stop check G40 - G42 Tool radius compensation G61 Exact stop mode G64 Cutting mode G65 Macro call (simple call) G66 Macro modal call (modal call) G66.1 Macro modal call (block call per macro) G67 Macro modal call cancel (modal call cancel) G80 - G89 Fixed cycle for drilling G90/G91 Absolute/incremental command G94 Asynchronous feed G98 Hole drilling cycle initial return G99 Hole drilling cycle R point return
Restrictions and precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
83 IB-1501277-P
6.10 Circular Cutting; G12,G13
Circular cutting starts the tool from the center of the circle, and cuts the inner circumference of the circle. The tool continues cutting while drawing a circle and returns to the center position.
(1) The sign + for the offset amount indicates reduction, and - indicates enlargement. (2) The circle cutting is executed on the plane G17, G18 or G19 currently selected.
For G12 (tool center path) 0->1->2->3->4->5->6->7->0
For G13 (tool center path) 0->7->6->5->4->3->2->1->0
Function and purpose
Command format
Circular cutting Clockwise (CW)
G12 I__ D__ F__ ;
Circular cutting Counterclockwise (CCW)
G13 I__ D__ F__ ;
I Radius of circle (incremental position), the sign is ignored D Offset No. (The offset No. and offset data are not displayed on the setting and display unit.) F Feedrate
Detailed description
Compensation amount sign + Compensation amount sign - (a) Circle radius (b) d1 offset amount + (c) d1 offset amount -
0
1 2
3
4
5
6 7
(a)
i 1
(b)
(c) X
Y
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
84IB-1501277-P
(Example 1) G12 I50.000 D01 F100 ; When compensation amount is +10.000mm
(1) If the offset No. "D" is not issued or if the offset No. is illegal, the program error (P170) will occur. (2) If [Radius (I) - offset amount] is 0 or negative, the program error (P223) will occur. (3) If G12 or G13 is commanded during radius compensation (G41, G42), the radius compensation will be validated
on the path after compensated with the D, commanded with G12 or G13. (4) If an address not included in the format is commanded in the same block as G12 and G13, the program error
(P32) will occur. But when the parameter "#11034 Circular cutting command address check type" is set to "1", it operates as fol- lows; (a) Program error will not occur except for an "H" command. (b) Only "D","F","I" and "M","S","T","B" will be valid.
Program example
Tool
Compensation amount
Radius
Precautions
50.000
10.000
X
Y
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
85 IB-1501277-P
6.11 Polar Coordinate Interpolation; G12.1, G13.1/G112, G113
This function converts the commands programmed with the orthogonal coordinate axis into linear axis movement (tool movement) and rotary axis movement (workpiece rotation), and controls the contour. The plane that uses the linear axis as the plane's 1st orthogonal axis, and the intersecting hypothetical axis as the plane's 2nd axis (hereafter "polar coordinate interpolation plane") is selected. Polar coordinate interpolation is car- ried out on this plane. The workpiece coordinate system zero point is used as the coordinate system zero point during polar coordinate interpolation.
This is effective for cutting a notch in a linear line to the external diameter of the workpiece, for cutting cam shafts, etc.
Function and purpose
Linear axis
Rotary axis (Hypothetical axis)
Polar coordinate interpo- lation plane (G17 plane)
Command format
Polar coordinate interpolation mode start
G12.1 ;
Polar coordinate interpolation mode cancel
G13.1 ;
X
Z
C
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
86IB-1501277-P
(1) The coordinate commands in the interval from the start to cancellation of the polar coordinate interpolation mode will be polar coordinate interpolation.
(2) G112 and G113 can be used instead of G12.1 and G13.1. (3) G12.1 must be commanded alone in a block, which also applies to G13.1. If it is commanded in the same block
with other G code, a program error (P33) will occur. (4) Linear interpolation or circular interpolation can be commanded during the polar coordinate interpolation mode. (5) The coordinate commands can be both an absolute command or incremental command. (6) Tool radius compensation can be applied on the program command. Polar coordinate interpolation will be exe-
cuted to the path after it has gone through a tool radius compensation. (7) Command the tangent speed in the polar coordinate interpolation plane (orthogonal coordinate system) by F. F
is in mm/min or inch/min unit. (8) When the G12.1/G13.1 command is issued, the deceleration check is executed.
The linear axis and rotary axis used for polar coordinate interpolation depend on the MTB specifications (parameter #1533).
(1) Determine the deemed plane for carrying out polar coordinate interpolation with the parameter (#1533) of the linear axis used for polar coordinate interpolation.
(2) A program error (P485) will occur if the plane selection command (G17 to G19) is issued during the polar coor- dinate interpolation mode.
will be the same as when the parameter (#1533) is blank (no setting).
#1516 mill_ax (Milling axis name)
#1517 mill_c (Milling interpolation hypothetical axis name)
#8111 Milling Radius
#1533 mill_Pax (Polar coordinate linear axis name)
Detailed description
G12.1 ; Polar coordinate interpolation mode start (Polar coordinate interpolation will start.) (The coordinate commands in this interval will be the polar coordinate interpolation.)
: G13.1 ; Polar coordinate interpolation mode cancel (Polar coordinate interpolation is canceled.)
Plane selection
Setting for #1533 Deemed plane
X G17 (XY plane) Y G19 (YZ plane) Z G18 (ZX plane)
Blank (no setting) G17 (XY plane)
Related parameter
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
87 IB-1501277-P
Program example
Hypothetical C axis
Hypothetical C axis
Tool
Path after tool radius compensation Programmed path
: N01 G17 G90 G00 X40.0 C0 Z0; Setting of start position N02 G12.1 ; Polar coordinate interpolation mode: Start N03 G01 G42 X20.0 F2000; Actual machining start N04 C10.0; N05 G03 X10.0 C20.0 R10.0; N06 G01 X-20.0; Shape program N07 C-10.0; N08 G03 X-10.0 C-20.0 I10.0 J0; (Follows orthogonal coordinate positions on X-C hypothetical axis
plane.) N09 G01 X20.0; N10 C00; N11 G40 X40.0; N12 G13.1 ; Polar coordinate interpolation mode: Cancel : M30 ;
X C
Z
C
X
N06 N05
N04 N03
N10
N09N08
N07 N11
N01 N02
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
88IB-1501277-P
(1) The program commands in the polar coordinate interpolation mode are issued by the orthogonal coordinate val- ue of the linear axis and rotary axis (hypothetical axis) on the polar coordinate interpolation plane. The axis address of the rotary axis (C) is specified as the axis address for the plane's 2nd axis (hypothetical axis) command. The command unit is not deg (degree). The same unit (mm or inch) as used for the command by the axis address of the plane's 1st axis (linear axis) will be used.
(2) The hypothetical axis coordinate value will be set to "0" when G12.1 is commanded. In other words, the position where G12.1 is commanded will be interpreted as angle = 0, and the polar coordinate interpolation will start.
The arc radius address for carrying out circular interpolation during the polar coordinate interpolation mode is deter- mined with the linear axis parameter (#1533).
The arc radius can also be designated with the R command.
(1) Depending on the model or version, parameter (#1533) may not be provided. In this case, the operation will be the same as when the parameter (#1533) is blank (no setting).
The tool radius can be compensated during the cylindrical interpolation mode.
(1) Command the plane selection in the same manner as polar coordinate interpolation. When conducting tool radius compensation, it must be started up and canceled during the polar coordinate in- terpolation mode.
(2) A program error (P485) will occur if polar coordinate interpolation is executed during tool radius compensation. (3) If the G12.1 and G13.1 commands are issued with no movement command after the tool radius compensation
is canceled, the position of the axis in the G12.1 and G13.1 commands block is interpreted as the position ap- plied after the tool radius compensation is canceled and the following operations are performed.
(1) The asynchronous mode is forcibly set when the polar coordinate interpolation mode is started. (2) When the polar coordinate interpolation mode is canceled, the synchronous mode will return to the state before
the polar coordinate interpolation mode was started. (3) A program error (P485) will occur if G12.1 is commanded in the constant surface speed control mode (G96).
(1) The miscellaneous function (M) and 2nd miscellaneous function can be issued in the polar coordinate interpola- tion mode.
(2) The S command in the polar coordinate interpolation mode specifies the rotary tool's rotation speed instead of the spindle rotation speed.
Relationship with Other Functions
Program commands during polar coordinate interpolation
Circular interpolation on polar coordinate plane
Setting for #1533 Center designation command
X I, J (polar coordinate plane is interpreted as XY plane) Y J, K (polar coordinate plane is interpreted as YZ plane) Z K, I (polar coordinate plane is interpreted as ZX plane)
Blank (no setting) I, J (polar coordinate plane is interpreted as XY plane)
Tool radius compensation
Cutting asynchronous feed
Miscellaneous function
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
89 IB-1501277-P
(1) Program error (P481) will occur if tool length compensation is performed in the polar coordinate interpolation mode.
(2) Complete the tool compensation operation (movement of tool length and wear compensation amount) before executing the polar coordinate interpolation. If the tool compensation operation is not completed when the polar coordinate interpolation start command has been issued, the followings will occur: Machine coordinate will not change even if G12.1 is executed. When G12.1 is executed, the workpiece coordinate will change to that of the post tool length compensation. (Even if polar coordinate interpolation is canceled, this workpiece coordinate will not be canceled.)
As for the F command during polar coordinate interpolation mode, whether to use the previous F command depends on the previous mode of the feed per minute command (G94/G98) or feed per rotation command (G95/G99).
(1) When G94 (G98) is commanded just before G12.1 If there is no F command in the polar coordinate interpolation, the previous F command feedrate will be used. After the polar coordinate interpolation mode is canceled, the F command feedrate set at the start of the polar coordinate interpolation mode or the last F command feedrate set during polar coordinate interpolation will con- tinue to be the feedrate.
(2) When G95 (G99) is commanded just before G12.1 The previous F command feedrate cannot be used during polar coordinate interpolation. A new F command must be issued. The feedrate after the polar coordinate interpolation mode is canceled will return to the state before the polar coordinate interpolation mode was started. [When there is no F command in G12.1]
[When F is commanded in G12.1]
Hole drilling axis in the fixed cycle for drilling command during the polar coordinate interpolation is determined with the linear axis parameter (# 1533).
Tool length compensation
: G43 H12 ; Tool length compensation before polar coordinate interpolation -> Valid G00 X100. Z0. ; G12.1 ; : G43 H11 ; Tool length compensation in polar coordinate interpolation mode -> Pro-
gram error : G13.1 ;
F command during polar coordinate interpolation
Previous mode No F command After G13.1
G94 (G98) Previous F is used (Same as on the left) G95 (G99) Program error (P62) F just before G12.1 is used
Previous mode With F command After G13.1
G94 (G98) Commanded F is used (Same as on the left) G95 (G99) Commanded F is used (*1) F just before G12.1 is used (*1) Moves with the feed per minute command during G12.1.
Hole drilling axis in the fixed cycle for drilling command
Setting for #1533 Hole drilling axis
X Z (polar coordinate plane is interpreted as XY plane) Y X (polar coordinate plane is interpreted as YZ plane) Z Y (polar coordinate plane is interpreted as ZX plane)
Blank (no setting) Z (polar coordinate plane is interpreted as XY plane)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
90IB-1501277-P
Shift amount in the G76 (fine boring) or G87 (back boring) command during the polar coordinate interpolation is de- termined with the linear axis parameter (#1533).
In circular interpolation that passes through the center of the workpiece, a large movement occurs on the C axis when the axis passes through the center of the workpiece. By using the parameter "#19104 G12.1 no reversal", you can switch whether the rotation direction of the C axis at that time to be a short rotation or the previous rotation di- rection to be maintained. Set "0" to make a short turn, and set "1" to maintain the rotation direction up to that point. The parameter "#19104 G12.1 no reversal" can be switched only for the movement of the timing when the axis pass- es through the center of the workpiece. Specify the range to be judged as the center of the workpiece using the parameter "#19105 G12.1 zero range". If one axis on the polar coordinate plane crosses the quadrant and the other axis is within the range of the parameter "#19105 G12.1 zero range", it is assumed that the axis have passed through the center of the workpiece. The rotation direction of the C axis that is used immediately before the position of the axis on the polar coordinate plane enters the range specified with the parameter "#19105 G12.1 zero range" is set as the rotation direction of the C axis used when the quadrant is switched.
[Timing to acquire the rotation direction of the C axis used when the quadrant is switched]
When the parameter #19104 is set to "1", adjust the setting value of the parameter #19105. The movement of the C axis becomes unstable near the center of the workpiece; therefore, set the parameter #19105 to a value larger than "0.0". Execute the machining program including the target circular interpolation and check the rotation direction of the C axis at the center of the workpiece. If there is no problem, the setting is com- pleted. If the rotation direction of the C axis that passes through the center of the workpiece is not improved, change the setting value of the parameter #19105 to a larger value.
(1) If the arc does not pass through the center of the workpiece, the direction does not change suddenly when the quadrant is switched, so set the parameter #19104 to "0".
(2) In the case of an arc of which the start point is near the center of rotation (the start point is within the range spec- ified with the parameter #19105), the rotation direction of the C axis used at the time of quadrant switching is shortcut regardless of the setting of the parameter #19104. Therefore, set the start point of the arc away from the center of the workpiece (outside the range specified with the parameter #19105).
Shift amount in the G76 (fine boring) or G87 (back boring) command
Setting for #1533 Center designation command
X I, J (polar coordinate plane is interpreted as XY plane) Y J, K (polar coordinate plane is interpreted as YZ plane) Z K, I (polar coordinate plane is interpreted as ZX plane)
Blank (no setting) I, J (polar coordinate plane is interpreted as XY plane)
Operation switching for circular interpolation in the center of a workpiece
(1) Circular command direction (2) Timing to acquire the movement direction of the C axis (3) Range specified with the parameter #19105 (4) Timing at which the C axis rotates in the same direction as (2)
(When the parameter #19104 is set to "1")
Y
X
(3)
(4)
(1)
(2)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
91 IB-1501277-P
(1) The following G code commands can be used during the polar coordinate interpolation mode.
A program error (P481) may occur if a G code other than those listed above is commanded during polar coordi- nate interpolation.
(2) Program cannot be restarted (program restart) when the block is in the polar coordinate interpolation. (3) Before commanding polar coordinate interpolation, set the workpiece coordinate system so that the center of the
rotary axis is at the coordinate system zero point. Do not change the coordinate system during the polar coordi- nate interpolation mode. (G50, G52, G53, relative coordinate reset, G54 to G59, etc.)
(4) The feedrate during polar coordinate interpolation will be the interpolation speed on the polar coordinate inter- polation plane (orthogonal coordinate system). (The relative speed with the tool will vary according to the polar coordinate conversion.) When passing near the center of the rotary axis on the polar coordinate interpolation plane (orthogonal coordi- nate system), the rotary axis side feedrate after polar coordinate interpolation will be very high.
(5) The axis movement command outside of the plane during polar coordinate interpolation will move unrelated to the polar coordinate interpolation.
(6) The current position displays during polar coordinate interpolation will all indicate the actual coordinate value. However, the "remaining movement amount" indicates the movement amount on the polar coordinate input plane.
(7) The polar coordinate interpolation mode is canceled when the power is turned ON or reset. (8) A program error (P484) will occur if any axis commanded during polar coordinate interpolation has not completed
the reference position return. (9) Tool radius compensation must be canceled before canceling the polar coordinate interpolation mode. (10) When the polar coordinate interpolation mode is canceled and switched to the cutting mode, the plane selected
before the polar coordinate interpolation will be restored. (11) A program error (P486) will occur if the polar coordinate interpolation command is issued during the mirror im-
age. (12) A program error (P481) will occur if the cylindrical interpolation or the polar coordinate interpolation is command-
ed during the polar coordinate interpolation mode. (13) During polar coordinate interpolation, if X axis moveable range is controlled in the plus side, X axis has to be
moved to the plus area that includes "0" and above before issuing the polar coordinate interpolation command. If X axis moveable range is controlled in the minus side, X axis has to be moved to the minus area that does not include "0" before issuing the polar coordinate interpolation command.
Restrictions and precautions
G code Details
G00 Positioning G01 Linear interpolation G02 Circular interpolation (CW) G03 Circular interpolation (CCW) G04 Dwell G09 Exact stop check G40 - G42 Tool radius compensation G61 Exact stop mode G64 Cutting mode G65 Macro call (simple call) G66 Macro modal call (modal call) G66.1 Macro modal call (block call per macro) G67 Macro modal call cancel (modal call cancel) G80 - G89 Fixed cycle for drilling G90/G91 Absolute/incremental command G94 Asynchronous feed G98 Hole drilling cycle initial return G99 Hole drilling cycle R point return
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
92IB-1501277-P
6.12 Exponential Interpolation; G02.3, G03.3
Exponential function interpolation changes the rotary axis into an exponential function shape in respect to the linear axis movement. At this time, the other axes carry out linear interpolation between the linear axis. This allows a machining of a taper groove with constant torsion angle (helix angle) (uniform helix machining of taper shape). This function can be used for slotting or grinding a tool for use in an end mill, etc.
Uniform helix machining of taper shape
Relation of linear axis and rotary axis
Function and purpose
A: A axis (rotation ax- is) X: X axis (linear axis)
Torsion angle: J1 = J2 = J3
A: A axis (rotation axis) X: X axis (linear axis) * : {B, C... constant}
(G02.3/G03.3)(G01)
Z
A J1 J2 J3
X
(G01)
(G00)
X=B(eCA-1)
A
X *
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
93 IB-1501277-P
(*1) Designate the end point of the linear axis specified by parameter "#1514 expLinax" and the axis that carries out linear interpolation between that axis. If the end point on of the rotary axis designated with parameter "#1515 expRotax" is specified, linear interpola- tion without exponential function interpolation will take place. These parameter settings depend on the MTB specifications.
(*2) The command unit is as follows.
The command range is -89 to +89. A program error (P33) will occur if there is no address I or J command. A program error (P35) will occur if the address I or J command value is 0.
(*3) The command unit is as follows.
The command range is a positive value that does not include 0. A program error (P33) will occur if there is no address R command. A program error (P35) will occur if the address R command value is 0.
(*4) The command unit and command range is the same as the normal F code. (Command as per minute feed.) Command the composite feedrate that includes the rotary axis. The normal F modal value will not change by the address F command. A program error (P33) will occur if there is no address F command. A program error (P35) will occur if the address F command value is 0.
Command format
Forward rotation interpolation (Modal)
G02.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ;
Backward rotation interpolation (Modal)
G03.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ;
X X axis end point (*1) Y Y axis end point (*1) Z Z axis end point (*1) I Angle i1 (*2) J Angle j1 (*2) R Constant value r1 (*3) F Initial feedrate (*4) Q Feedrate at end point (*5) K Command will be ignored.
Setting unit #1003=B #1003=C #1003=D #1003=E (Unit = ) 0.001 0.0001 0.00001 0.000001
Setting unit #1003=B #1003=C #1003=D #1003=E Unit Millimeter system 0.001 0.0001 0.00001 0.000001 mm Inch system 0.0001 0.00001 0.000001 0.0000001 inch
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
94IB-1501277-P
(*5) The command unit is as follows.
The command unit and command range is the same as the normal F code. Command the composite feedrate that includes the rotary axis. The normal F modal value will not change by the address Q command. The axis will interpolate between the initial speed (F) and end speed (Q) in the CNC according to the linear axis. If there is no address Q command, interpolation will take place with the same value as the initial feedrate (ad- dress F command). (The start point and end point feedrates will be the same.) A program error (P35) will occur if the address Q command value is 0.
[Example of uniform helix machining of taper shape]
The exponential function relational expression of the linear axis (X) and rotary axis (A) in the G02.3/G03.3 command is defined in the following manner.
where, "D" is as follows. D = tan(j1) / tan(i1) During forward rotation (G02.3): = 0 During backward rotation (G03.3): = 1 is the rotation angle (radian) from the rotary axis' start point. The rotary axis' rotation angle () is as follows ac- cording to expression (1). = D * 1n{(X * tan(i1) / r1) + 1}
Setting unit #1003 = B #1003=C #1003=D #1003=E Unit Millimeter system 0.001 0.0001 0.00001 0.000001 mm Inch system 0.0001 0.00001 0.000001 0.0000001 inch
X : X axis (linear axis) A : A axis (rotation axis) x0 : linear axis (X axis) start point
Detailed description
Relational expression of exponential function
X() = r1 * (e/D - 1) / tan(i1) Linear axis (X) movement (1)
A() = (-1) * 360 * / (2) Rotary axis (A) movement
i1
j1 x1x0
r1
ZZ
A X
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
95 IB-1501277-P
[Uniform helix machining of taper shape]
where, "D" is as follows. D = tan(j1) / tan(i1)
Machining example
Z() = r1 *(e/D-1)* tan(p1) / tan(i1) + z0 (1)
X() = r1 *(e/D-1)/ tan(i1) (2)
A() = (-1) * 360 * / (2)
Z() Absolute position from zero point of Z axis (axis that linearly interpolates with linear axis (X axis)) X() Absolute position from X axis (linear axis) start point A() Absolute position from A axis (rotary axis) start point r1 Exponential function interpolation constant value (address R command) r2 Workpiece left edge radius x2 X axis (linear axis) position at the left edge of the workpiece x1 X axis (linear axis) end point (address X command) x0 X axis (linear axis) start point (Set as "x0 x1" so that workpiece does not interfere with the tool) z1 End point of Z axis (axis that linearly interpolates between interval with linear axis (X axis)) (address Z
command) z0 Start point of Z axis (axis that linearly interpolates between interval with linear axis (X axis)) i1 Taper gradient angle (address I command) p1 Slot base gradient angle j1 Torsion angle (helix angle) (address J command) Torsion direction (0: Forward rotation, 1: reverse direction) Workpiece rotation angle (radian) f1 Initial feedrate (address F command) q1 Feedrate at end point (address Q command) k1 Insignificant data (address K command)
i1
j1 x1x0 x2
p1
r1r2
z1
z2 z0 A
X
Z
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
96IB-1501277-P
According to expressions (1) and (2), expression (3) is obtained. Z() = X() * tan(p1) + z0 ...(3) According to expression (3), the slot base gradient angle (p1) is set from the X axis and Z axis end point positions (x1, z1). The Z axis movement amount is determined by the slot base gradient angle (p1) and X axis position. In the above diagram, the exponential function interpolation's constant value (r1) is determined with the following expression using the workpiece left edge radius (r2), X axis start point (x0), X axis position at workpiece left edge (x2) and taper gradient angle (i1). r1 = r2 -{(x2 - x0) * tan(i1)} The taper gradient angle (i1) and torsion angle (j1) are set by the command address I and J, respectively. Note that if the shape is a reverse taper shape, the taper gradient angle (i1) is issued as a negative value. The torsion direction () is changed by the G code. (Forward rotation when G02.3 is commanded, negative rotation when G03.3 is commanded) The above settings allow uniform helix machining of a taper shape (or reverse taper shape).
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
97 IB-1501277-P
(1) G2.3 (equivalent to G3.3 if j1 < 0) In the conditional figure below, the upper side shows a command, and the lower side shows an operation.
(S) Start point, (E) End point
(2) G3.3 (equivalent to G2.3 if j1 < 0) In the conditional figure below, the upper side shows a command, and the lower side shows an operation.
(S) Start point, (E) End point
Command and operation
X movement direction > 0 X movement direction < 0
i1 > 0 i1 < 0 i1 > 0 i1 < 0
N10 G28XYZC; N20 G91G0 X100. Z100.; N30 G2.3 X100. Z100. I50. J80. R105. F500.; N40 M30;
N10 G28XYZC; N20 G91G0 X100. Z200.; N30 G2.3 X100. Z-100. I- 50. J80. R105. F500.; N40 M30;
N10 G28XYZC; N20 G91G0 X-100. Z100.; N30 G2.3 X-100. Z100. I50. J80. R105. F500.; N40 M30;
N10 G28XYZC; N20 G91G0 X-100. Z200.; N30 G2.3 X-100. Z-100. I-50. J80. R105. F500.; N40 M30;
X movement direction > 0 X movement direction < 0
i1 > 0 i1 < 0 i1 > 0 i1 < 0
N10 G28XYZC; N20 G91G0 X100. Z100.; N30 G3.3 X100. Z100. I50. J80. R105. F500.; N40 M30;
N10 G28XYZC; N20 G91G0 X100. Z200.; N30 G3.3 X100. Z-100. I- 50. J80. R105. F500.; N40 M30;
N10 G28XYZC; N20 G91G0 X-100. Z100.; N30 G3.3 X-100. Z100. I50. J80. R105. F500.; N40 M30;
N10 G28XYZC; N20 G91G0 X-100. Z200.; N30 G3.3 X-100. Z-100. I-50. J80. R105. F500.; N40 M30;
(S)
r1
Z
j1
i1 (E)
X
Z
(S)
j1
i1
(E)
Xr1
Z
(S)
Xr1
j1
i1(E) (S)
X
Z i1
j1 (E)
r1
A
X
A
X
A
X
A
X
Z
(S)
r1 X
j1
(E)i1 Z
(S)
j1
i1
(E)
Xr1
Z
(S)
Xr1
j1
i1(E) (S)
X
Z i1
j1 (E)
r1
A
X
A
X
A
X
A
X
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
98IB-1501277-P
(1) When G02.3/G03.3 is commanded, interpolation takes place with the exponential function relational expression using the start position of the linear axis and rotary axis as 0.
(2) Linear interpolation will take place in the following cases, even if in the G02.3/G03.3 mode. The feedrate for linear interpolation will be the F command in that block. (Note that the normal F modal is not updated.) The linear axis designated with the parameter (#1514 expLinax) is not commanded, or the movement
amount for that axis is 0. The rotary axis designated with the parameter (#1515 expRotax) is commanded.
(3) A program error will occur if the following commands are issued during the G02.3/G03.3 mode. A program error will also occur if G02.3 or G03.3 command is issued in the following modes. Tool length compensation (A program error will occur only when the compensation starts at the same time
as the movement by exponential function interpolation. The tool length compensation will operate normally if it has started before the G02.3/G03.3 mode starts.) Tool radius compensation High-speed High-accuracy Control High-speed machining Scaling Tool length compensation along the tool axis Figure rotation Coordinate rotation by program Coordinate rotation by parameter 3-dimensional coordinate conversion
(4) A program error (P481) will occur if commands are issued during the pole coordinate interpolation, cylindrical interpolation or milling interpolation modes.
(5) Program error (P612) will occur if commands are issued during the scaling or mirror image. (6) Program error (P34) will occur if commands are issued during the high-speed high-accuracy control II. (7) G02.3/G03.3 will function with asynchronous feed even during the synchronous feed mode, and the synchronous
feed mode will be canceled. (8) If the parameter "#1515 expRota" setting is the same axis name as the initial C axis, the axis selected with the
C axis selection signal will interpolate as the rotary axis.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
99 IB-1501277-P
6.13 Polar Coordinate Command; G16
With this function, the end point coordinate value is commanded with the polar coordinate of the radius and angle.
Function and purpose
Command format
Polar coordinate command mode ON
G16 ;
Polar coordinate command mode OFF
G15 ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
100IB-1501277-P
(1) The polar coordinate command is applied in the interval from turning ON to OFF of the polar coordinate command mode
(2) The plane selection during the polar coordinate command mode is carried out with G17, G18 and G19. (3) The polar coordinate command is a modal. The polar coordinate command mode when the power is turned ON
is off (G15). Whether to initialize the modal at reset or not can be selected with the parameter (#1210 RstGmd/ bit 11) setting.
(4) During polar coordinate command mode, command the radius with the 1st axis for the selected plane, and the angle with the 2nd axis. For example, when the X-Y plane is selected, command the radius with the address "X", and the angle with the address "Y".
(5) For the angle, the counterclockwise direction of the selected plane is positive and the clockwise direction is neg- ative.
(6) The radius and angle can be commanded with both the absolute command (G90) and incremental command (G91).
(7) When the radius is commanded with the absolute position, command the distance from the zero point in the work- piece coordinate system (note that when the local coordinate system is set, command the distance in the local coordinate system).
(8) When the radius is commanded with the incremental command, considering the end point of the previous block as the polar coordinate center, command the incremental position from that end point. The angle is commanded with the incremental position of the angle from the previous block.
(9) When the radius is commanded with the negative value, the same operation as the command that the radius command value is changed to the absolute position and 180 is added to the angle command value.
Detailed description
G1x ; Plane selection for polar coordinate command (G17/G18/G19) G16 ; Polar coordinate command mode ON G9x G01 Xx1 Yy1 F2000 ; :
Polar coordinate command G9x: Center selection for polar coordinate command (G90/G91) G90: The workpiece coordinate system zero point is the polar coordinate center. G91: The current position is the polar coordinate center. x1: 1st axis for the plane: The radius of the polar coordinate commanded y1: 2nd axis for the plane: The angle of the polar coordinate commanded
G15 ; Polar coordinate command mode OFF
(CP) Current position (IP) Commanded position
For G90/G17 (X-Y plane)
y1
x1
X
Y
(IP)
(CP)
+
-
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
101 IB-1501277-P
(1) When the zero point in the workpiece coordinate system is applied to the polar coordinate center The zero point in the workpiece coordinate system is applied to the polar coordinate center by commanding the radius value with the absolute position.
Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coor- dinate system (G52) is used.
(2) When the present position is applied to the polar coordinate center The present position is applied to the polar coordinate center by commanding the radius value with the incre- mental position.
Commanded position
When the angle is the absolute command When the angle is the incremental command
When the angle is the absolute command When the angle is the incremental command
(CP) Current position (IP) Command position (a) Angle (r) Radius
(IP)
(CP)
(r)
(a)
(IP)
(CP)
(r)
(a)
(IP)
(CP)
(r)
(a)
(IP)
(CP)
(r) (a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
102IB-1501277-P
(3) When the radius value command is omitted When the radius value command is omitted, the zero point in the workpiece coordinate system is applied to the polar coordinate center, and the distance between the polar coordinate center and current position is regarded as the radius. Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coordinate system (G52) is used.
(4) When the angle command is omitted When the angle command is omitted, the angle of the present position in the workpiece coordinate system is applied to the angle command. The zero point in the workpiece coordinate system is applied to the polar coordinate center by commanding the radius value with the absolute position. Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coordinate system (G52) is used.
If the radius value is commanded with the incremental position, the current position is applied to the polar coor- dinate center.
When the angle is the absolute command When the angle is the incremental command
When the angle is the absolute command When the angle is the incremental command
(CP) Current position (IP) Command position (a) Angle (r) Radius
(IP)
(CP)
(r)
(a)
(IP)
(CP)
(r) (a)
(IP)
(CP)
(r)
(a)
(IP)
(CP)
(r)
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
103 IB-1501277-P
The axis command with the following command is not interpreted as the polar coordinate command during the polar coordinate command mode. The movement command that has no axes commands for the 1st axis and 2nd axis in the selected plane mode is also not interpreted as polar coordinate command during the polar coordinate command mode.
Axis command not interpreted as polar coordinate command
Function G code
Dwell G04 Parameter input by program/Compensation data input G10 Local coordinate system setting G52 Machine coordinate system setting G92 Machine coordinate system selection G53 Coordinate rotation by program G68 Scaling G51 G command mirror image G51.1 Reference position check G27 Reference position return G28 Start position return G29 2nd, 3rd, 4th reference position return G30 Tool change position return 1 G30.1 Tool change position return 2 G30.2 Tool change position return 3 G30.3 Tool change position return 4 G30.4 Tool change position return 5 G30.5 Tool change position return 6 G30.6 Automatic tool length measurement G37 Skip G31 Multi-step skip 1-1 G31.1 Multi-step skip 1-2 G31.2 Multi-step skip 1-3 G31.3 Linear angle command G01 Aa1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
104IB-1501277-P
When the zero point in the workpiece coordinate system is the polar coordinate zero point
The polar coordinate zero point is the zero point in the workpiece coordinate system. The plane is the X-Y plane. (1) When the radius and angle are the absolute command
(2) When the radius is the absolute command and the angle is the incremental command
Program example
N1 G17 G90 G16 ; Polar coordinate command, X-Y plane selection The polar coordinate zero point is the zero point in the work- piece coordinate system.
N2 G85 X200. Y30. Z-20. F200. Radius 200mm, angle 30 N3 Y120. Radius 200mm, angle 120 N4 Y270. Radius 200mm, angle 270 N5 G15 G80 ; Polar coordinate command cancel
N1 G17 G90 G16 ; Polar coordinate command, X-Y plane selection The polar coordinate zero point is the zero point in the work- piece coordinate system.
N2 G85 X200. Y30. Z-20. F200. Radius 200mm, angle 30 N3 G91 Y90. Radius 200mm, angle +90 N4 Y150. Radius 200mm, angle +150 N5 G15 G80 ; Polar coordinate command cancel
200mm
X
Y
30
120
270
N4
N2
N3
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
105 IB-1501277-P
(1) If the high-accuracy commands are carried out during the polar coordinate command mode, or if the polar coor- dinate commands are carried out during the high-accuracy command mode, operations are performed depend- ing on your machine's specifications. Refer to "High-accuracy Control" and "High-speed High-accuracy Control" for details.
(2) When the mirror image (G code/parameter/PLC signal) is canceled anywhere except at the mirror image center during the polar coordinate command mode, the absolute position and machine position will deviate. The mirror center is set with an absolute position, so if the mirror center is commanded again in this state, the center may be set to an unpredictable position. Cancel the mirror image above the mirror center or, after cancellation, assign a positioning command using absolute command that the radius and angle of the polar coordinate command are designated.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
106IB-1501277-P
6.14 Spiral/Conical Interpolation; G02.1/G03.1 (Type 1), G02/G03 (Type 2)
This function carries out interpolation that smoothly joins the start and end points in a spiral. This interpolation is carried out for arc commands in which the start point and end point are not on the same circumference. Conical interpolation is carried out by designating the end point in the height direction.
There are two types of command formats, and they can be switched with the parameter.
Circular interpolation operations are carried out at the f1 speed by the commands above.
The path is toward the end point, following a spiral arc path centered at the position designated by distance i (X axis direction) and distance j (Y axis direction) in respect to the start point.
(1) The arc plane is designated by G17, G18 and G19. (Common for type 1 and 2)
(2) The arc rotation direction is designated by G02.1 (G02) or G03.1 (G03). (Common for type 1 and 2)
Function and purpose
Command format
Spiral/conical interpolation (Type 1: #1272 ext08/bit2=0)
G17 G02.1/G03.1 X__ Y__ I__ J__ P__ F__;
Spiral/conical interpolation (Type 2: #1272 ext08/bit2=1)
G17 G02/G03 X__ Y__ I__ J__ Q__/L__/K__ F__;
Description of each address
G17 Arc plane G02.1/G03.1 (Type 1) Arc rotation direction (Type 1) G02/G03 (Type 2) Arc rotation direction (Type 2) X Y End point coordinates (Conical Interpolation when the axis other than arc plane
axes is included.) I J Arc center P (Type 1) Number of pitches (number of spirals) (Type 1) Q (Type 2) Incremental/decremental amount of radius (Type 2) L (Type 2) Number of pitches (Number of spirals) (Type 2) K (Type 2) Increment/decrement amount of height (Type 2) F Feedrate (tool path direction speed)
G17 XY plane G18 ZX plane G19 YZ plane
G02.1/G02 Clockwise (CW) G03.1/G03 Counterclockwise (CCW)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
107 IB-1501277-P
(3) The end point coordinates are designated with XYZ. (Common for type 1 and 2) (Decimal point command is possible. Use mm (or inch) as the unit.) When designation of arc plane axes is omitted, the coordinates of the start point are inherited. If the axis other than arc plane axes is designated, conical interpolation is applied.
(4) The arc center is designated with IJK. (Common for type 1 and 2) (Decimal point command is possible. Use mm (or inch) as the unit.) I: Incremental designation in the X axis direction from the start point J: Incremental designation in the Y axis direction from the start point K: Incremental designation in the Z axis direction from the start point When either 1 axis of arc plane is omitted, the coordinates of the start point are inherited.
(5) P designates the number of pitches (number of spirals). (Type 1) The number of pitches and rotations are as shown below.
(6) Q designates the increment/decrement amount of radius per spiral rotation. (Type 2) The number of spiral rotations when the increment or decrement amount of radius is specified can be calculated with the following expression. Number of rotations= | (arc end point radius - arc start point radius) | / | increment or decrement amount of radius |
(7) L designates the number of pitches (number of spirals). (Type 2) (range: 0 to 99) When omitted, L1 is designated. The number of pitches and rotations are as shown below.
Q takes precedence over L if both Q and L have been designated at the same time.
(8) K designates the increment or decrement amount of height per spiral rotation in conical interpolation. (Type 2) The increment or decrement amount of height is designated with I/J/K for the axis other than arc plane. The relation between increment or decrement amount of height and the rotation plane is as shown below.
The number of rotations when the increment or decrement amount of height is specified can be calculated with the following expression.
Number of rotations = Height / | Increment/decrement amount of height |
If Q, K and L have been designated at the same time, the order of precedence is Q>K>L. Decimal point command is possible in the range of the increment or decrement amount of radius and height. Use mm (or inch) as the unit.
Number of pitches (0 to 99) Number of rotations
P0 Less than 1 rotation (Can be omitted.) P1 1 or more rotation and less than 2 rotations Pn n or more rotation and less than (n+1) rotations
Number of pitches (0 to 99) Number of rotations
L1 Less than 1 rotation L2 1 or more rotation and less than 2 rotations Ln (n-1) or more rotations and less than n rotations
Rotation plane Increment or decrement amount of height
G18 J command G19 I command
Other than G18/G19 K command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
108IB-1501277-P
(1) The arc rotation direction G02.1 is the same as G02, and G03.1 is the same as G03. (2) Normally the spiral interpolation is automatically enabled with the arc commands (G02, G03) when the difference
between the start point radius and the end point radius is less than the parameter setting value. (3) The axis combination that can be simultaneously commanded depends on the specifications. The combination
within that range is arbitrary. (4) The feedrate is the constant tangent speed. (5) The arc plane always follows G17, G18 and G19. The plane arc control is carried out by G17, G18 and G19,
even if designated by two addresses that do not match the plane. (6) Conical interpolation
When an axis designation other than the spiral interpolation plane is simultaneously designated, other axes are also interpolated in synchronization with the spiral interpolation.
(7) In the following cases, a program error will occur.
(a) Items common for type 1 and 2
(b) Items for type 2 only
Detailed description
Setting Items Command range (unit)
Error
End point coor- dinates
Range of coordinate command (mm/inch) (Decimal point com- mand is possible.)
If a value exceeding the command range is issued, a program error (P35) will occur. If an axis other than one which can be controlled with the command
system is commanded, a program error (P33) will occur.
Arc center Range of coordinate command (mm/inch) (Decimal point com- mand is possible.)
If a value exceeding the command range is issued, a program error (P35) will occur. If an axis other than one which can be controlled with the command
system is commanded, a program error (P33) will occur. If rotation plane axis is not designated completely, a program error
(P33) will occur. Number of pitches
0 to 99 If a value exceeding the command range is issued, a program error (P35) will occur.
Feedrate Range of speed com- mand (mm/min, inch/min) (Decimal point com- mand is possible.)
If a value exceeding the command range is issued, a program error (P35) will occur.
Setting Items Command range (unit)
Error
Increment or decrement amount of radi- us
Range of coordinate command (mm/inch) (Decimal point com- mand is possible.)
If the sign of designated increment or decrement amount is opposite from that of the difference between the start point radius and the end point radius, a program error (P33) will occur. If the end point position obtained from the speed and increment or
decrement amount is larger than "SpiralEndErr (#8075)", a program error (P70) will occur.
Increment or decrement amount of height
Range of coordinate command (mm/inch) (Decimal point com- mand is possible.)
If the sign of designated increment or decrement amount is opposite from that of the movement direction of height, a program error (P33) will occur. If the end point position obtained from the speed and increment or
decrement amount is larger than "SpiralEndErr (#8075)", a program error (P70) will occur.
G02.1/0G3.1 Program error (P34) will occur if G02.1/G03.1 are used during type 2.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
109 IB-1501277-P
(Example 1)
(Example 2)
(Example 3) In this example, the interpolation is truncated cone interpolation.
(1) Items common for type 1 and 2 Interpolation vector in the middle of a tool path is not assured. As the start point and end point are not on the same arc, a normal line control will not be applied correctly. If there is no center command when geometric is valid, a program error (P33) will occur. It cannot be issued as an arc command for geometric IB. If the spiral/conical interpolation is commanded to the second geometric block, the program error (P33) oc-
curs. A command cannot be issued to the geometric IB blocks even when the command format type 2 (G02/G03)
is being designated. (2) Items for type 2 only If the spiral interpolation command is issued during the mirror image, a program error (P34) will occur. If the spiral interpolation command is issued during the scaling, a program error (P34) will occur. If the spiral interpolation command is issued during the corner chamfering/corner rounding command, a pro-
gram error (P33) will occur.
Program example
G91 G17 G01 X60. F500 ; Y140. ; G2.1 X60. Y0 I100. P1 F300 ; G01 X-120. ; G90 G17 G01 X60. F500 ; Y140. ; G2.1 X120. Y140. I100. P1 F300 ; G01 X0 ;
(S) Start point (E) End point (C) Center
G91 G17 G01 X60. F500 ; Y140. ; G02.1X60.0 Z100.0 I100. P1 F300 ; -> Because this is the G17 plane, arc control is not carried out by X-Z. G01X-120 ; Arc control is carried out by X-Y.
G17 G91 G02.1 X100.Z150. I150.P3 F500; XY plane
XZ plane
Relationship with other functions
140. (S)
(E) (C)
Y
W X60.
X60.
120. 140.
110.
Y
ZZ
W
W
X
XX
Y
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
110IB-1501277-P
6.15 3-dimensional Circular Interpolation; G02.4, G03.4
To issue a circular command on a 3-dimensional space, an arbitrary point (intermediate point) must be designated on the arc in addition to the start point (current position) and end point. By using the 3-dimensional circular interpo- lation command, an arc shape which is uniquely determined by the three points (start point, intermediate point, end point) designated on the 3-dimensional space can be machined.
The validity of this function depends on the MTB specifications. If this specification is invalid and the 3-dimensional circular interpolation command is issued, the program error (P39) occurs.
The speed command during 3-dimensional circular interpolation is the tangent speed on the arc.
(1) The G02.4 and G03.4 operations are the same. (The rotation direction cannot be specified.) (2) The axes used as the reference in 3-dimensional circular interpolation are the three basic axes set with the pa-
rameters. (3) The X, Y, Z addresses in the block can be omitted. The intermediate point coordinates omitted in the 1st block
become the start point coordinates, and the end point coordinates omitted in the 2nd block become the interme- diate point coordinates.
Function and purpose
(S) Start point (Current position) (E) End point (C) Intermediate point
Command format
G02.4 (G03.4) Xx1 Yy1 Zz1 1 ; Intermediate point designation (1st block)
Xx2 Yy2 Zz2 2 ; End point designation (2nd block)
G02.4 (G03.4) 3-dimensional circular interpolation command (The rotation direction cannot be specified.)
x1, y1, z1 Intermediate point coordinates x2, y2, z2 End point coordinates Arbitrary axis other than axis used as the reference (X,Y,Z) in 3-dimensional circular
interpolation (Can be omitted.)
Z
X
Y
(S)
(C)
(E)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
111 IB-1501277-P
(4) When the 3-dimensional circular interpolation is commanded, an arbitrary axis can be commanded in addition to the orthogonal coordinate system (X, Y, Z) used as the reference. The arbitrary axis designated in the interme- diate point designating block (1st block) interpolates to the command point when the axis moves from the start point to intermediate point. The arbitrary axis designated in the end point command block (2nd block) interpo- lates to the command point when the axis moves from the intermediate point to the end point. The number of arbitrary axes that can be commanded differs according to the number of simultaneous contour control axes. The total of the basic three axes used as the reference of the 3-dimensional circular interpolation and the arbi- trary axes commanded simultaneously must be less than or equal to the number of simultaneous contour control axes.
(5) When the 3-dimensional circular interpolation is commanded while the incremental command is valid, designate the relative position of the intermediate point with respect to the start point in the intermediate point designation block. In the end point designation block, designate the relative position of the end point with respect to the in- termediate point.
When the 3-dimensional circular interpolation is commanded, an arc that exists over the 3-dimensional space can be uniquely determined by designating the intermediate point and the end point in addition to the current position which is the start point. (refer to following figure). Therefore, according to the command format, it is necessary to designate the intermediate point in the 1st block and the end point in the 2nd block. If only one block is commanded, the program error (P74) occurs.
Linear interpolation is applied when the end point match the start point in the 3-dimensional circular interpolation command (refer to "When linear interpolation is applied"). Thus, a true circle (360-degree rotation) cannot be des- ignated in the 3-dimensional circular interpolation.
In addition, designate the intermediate point in the middle of the start point and the end point. If the intermediate point is near the start point or the end point, arc accuracy may fall.
[Designation of arc in 3-dimensional space]
As shown in the above figure, when three points (start point, intermediate point, end point) are specified on 3-dimen- sional space, arc center coordinates can be obtained. An arc center cannot be obtained if only two points are spec- ified, and a linear interpolation is applied. If the intermediate point is near the start point or the end point, an error may occur when the center coordinate of the arc is calculated.
Detailed description
Designating intermediate point and end point
(P) Plane including start point, intermedi- ate point and end point (S) Start point (Current position) (E) End point (CP) Intermediate point (C) Center
(E)
(CP)
(S) (C)
(P)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
112IB-1501277-P
In the following cases, linear interpolation is applied without executing 3-dimensional circular interpolation.
(1) When the start point, intermediate point, and end point are on the same line (refer to the following figure) (If the end point exists between the start point and the intermediate point, axes move in the order of the start point, intermediate point, and end point.)
(2) When two of the start point, intermediate point and end point match (Linear interpolation is applied even if the end point matches the start point to command true circle. When the start point matches the end point, axes move in the order of the start point, intermediate point, and end point.)
[When linear interpolation is applied]
The 3-dimensional circular interpolation command G02.4 (G03.4) is a modal command belonging to the 01 group. Therefore, the command remains valid until another G command in the 01 group is issued. When the 3-dimensional circular interpolation commands are carried out continuously, the end point of the previous command is the start point of the next command.
When linear interpolation is applied
Start point (Current position)
Intermediate point (Block1)
End point (Block2)
When the three points are on the same line, linear interpolation is applied.
Start point (Current position)
End point (Block2)
Intermediate point (Block1)
Even if the end point exists between the start point and intermediate point, axes move in the order of the start point, intermediate point, and end point.
Modal command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
113 IB-1501277-P
G code command which leads to a program error during 3-dimensional circular interpolation modal
G code command which leads to a program error when 3-dimensional circular interpolation is commanded
Commands other than G code that causes a program error when commanded simultaneously with 3-dimensional circular interpolation
Relationship with other functions
Commands that cannot be used
G Code Function name Program error
G07.1 Cylindrical interpolation P485 G12/G13 Circular cutting CW/CCW P75 G12.1 Polar coordinate interpolation P485 G16 Polar coordinate command P75 G41/G42 Tool radius compensation P75 G41/G42 3-dimensional tool radius compensation P75 G41.1/G42.1 Normal line control P75 G43/G44 Tool length compensation P75 G43.1 Tool length compensation along the tool axis P75 G43.4/G43.5 Tool center point control P941 G43.7 Tool position compensation P75 G51 Scaling P75 G51.1 Mirror image P75 G66/G66.1 User macro P75 G67 User macro P276 G68 Coordinate rotation by program P75 G68 3-dimensional coordinate conversion P921 G73/G74/G76/G81/G82 G83/G84/G85/G86/G87 G88/G89
Fixed cycles P75
G code modal Function name Program error
G07.1 Cylindrical interpolation P481 G12.1 Polar coordinate interpolation P481 G16 Polar coordinate command P75 G41/G42 Tool radius compensation P75 G41/G42 3-dimensional tool radius compensation P75 G41.1/G42.1 Normal line control P75 G43.1 Tool length compensation along the tool axis P75 G43.4/G43.5 Tool center point control P942 G43.7 Tool position compensation P75 G51 Scaling P75 G51.1 Mirror image P75 G66/G66.1 User macro P75 G68 Coordinate rotation by program P75 G68 3-dimensional coordinate conversion P922
Command code Function name Program error
,C / ,R Corner chamfering/Corner R P75
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
114IB-1501277-P
If any of the following functions is used in 3-dimensional circular interpolation, an alarm occurs. Chopping Macro interruption Mirror image by parameter setting Mirror image by external input Corner chamfering/corner rounding
The path of 3-dimensional circular interpolation during the graphic check is drawn as linear in each range from the start point to the intermediate point and from the intermediate point to the end point.
Restart search cannot be performed on blocks in which 3-dimensional circular interpolation is performed. Doing so may cause the program error (P49).
To use 3-dimensional circular interpolation in combination with the tool length offset function, complete the tool com- pensation operation (movement of tool length and wear compensation amount) before starting 3-dimensional circu- lar interpolation. If 3-dimensional circular interpolation is commanded while the tool compensation operation is not completed, the arc path (refer to the following figure) is such that the start point coordinates of the arc are uncompensated and the intermediate point and end point coordinates are located at the compensated positions.
To cancel the tool length offset during the 3-dimensional circular interpolation modal, use the G49 (cancel) com- mand. If "G43 H0" is commanded, the program error (P75) occurs, and the tool length offset cannot be canceled.
Functions that cannot be used
Graphic check
Program restart
Tool length offset
(S) Start point (uncompensated) (E1) End point (before compensation) (E2) End point (after compensation) (CP1) Intermediate point (before compensa- tion) (CP2) Intermediate point (after compensa- tion)
Arc path
Arc path without compensation
Tool compensation amount
Z
X
Y (E2)
(S)
(CP2)
(CP1)
(E1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
115 IB-1501277-P
The high-speed machining mode II is temporarily canceled while 3-dimensional circular interpolation is being exe- cuted. Both of the high-speed high-accuracy control II and III function as the high-accuracy control mode. The SSS control is temporarily canceled while 3-dimensional circular interpolation is being executed.
Restrictions may be added for other functions as well. Refer to the explanation of each function.
(1) If this command is executed with a single block enabled, a block stop is carried out at the intermediate point.
High-speed machining mode II, High-accuracy control, High-speed high-accuracy control II/III
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
116IB-1501277-P
6.16 NURBS Interpolation; G06.2
This function realizes NURBS (Non-Uniform Rational B-Spline) curve machining by simply commanding NURBS curve parameters (stage, weight, knot, control point), which is used for the curved surface/line machining, without replacing the path with minute fine segments.
This function operates only in the high-speed high-accuracy control II/III mode, therefore, the high-speed high-ac- curacy control II/III function is also required as the specification.
(1) High-speed high-accuracy control III functions as high-speed high-accuracy control II while NURBS interpolation is ON.
However, if the curvature is large, the speed is clamped so that the machine's tolerable acceleration rate is not ex- ceeded.
Function and purpose
Command format
NURBS interpolation start
G06.2 Pp Kk1 X1 Yy1 Zz1 Rr1 Ff;
Kk2 Xx2 Yy2 Zz2 Rr2;
Kk3 Xx3 Yy3 Zz3 Rr3;
Kk4 Xx4 Yy4 Zz4 Rr4;
:
Kkn Xxn Yyn Zzn Rrn;
Kkn+1;
Kkn+2;
Kkn+3;
Kkn+4;
Pp Set the stage of the NURBS curve. Designate in the same block as G06.2 command. The NURBS curve of the stage p will be (p-1)th curve. When omitted, Pp means the same as P4. (Example) P2: Primary curve (linear)
Kkn Knot Set the knot for each NURBS interpolation block. Set the same value for the knot in the 1st block to the stage p block. NURBS interpo- lation is terminated if there is a block exclusively with knot.
Xxn Yyn Zzn Control point coordinate value. Designate the same coordinate value for the 1st block control point as that designated right before NURBS interpolation.
Rrn Control point weight. Set the weight of each NURBS interpolation control point. Ff Interpolation speed (Can be omitted)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
117 IB-1501277-P
(1) Designate the stage P for the 1st block of NURBS interpolation. (2) Designate the same coordinate value for the 1st block control point of NURBS interpolation as that designated
right before NURBS interpolation. (3) Designate all axes to be used in the subsequent NURBS interpolation blocks for 1st block of NURBS interpola-
tion. (4) Set the same value for knot K from the 1st block of NURBS interpolation to setting value block of the stage P. (5) Command knot K exclusive block of the same number as the setting value of the stage P for terminating NURBS
interpolation. At this time, set the same value for knot K setting.
(1) If an exclusive knot is commanded immediately after NURBS interpolation, NURBS interpolation mode is active again. An exclusive knot that is commanded immediately after NURBS interpolation is the same meaning as following command.
G06.2 Pp Km Xxn Yyn Zzn R1.0
Detailed description
Passes through control point
NURBS interpolation curve
(xn,yn,zn)
(x4,y4,z4) (x3,y3,z3)
(x2,y2,z2)
(x1,y1,z1)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
118IB-1501277-P
The example of program that has 4 stages (cubic curve) and 11 control points is shown below.
Program example
Control point
P0 P1 P2 P3 P4 P5 P6 P7 P8 P9 P10
Knot 0.0 0.0 0.0 0.0 1.0 2.0 3.0 4.0 5.0 6.0 7.0 8.0 8.0 8.0 8.0
: : G05 P10000; High-speed high-accuracy control II mode ON G90 G01 X0. Y0. Z0. F300 ; G06.2 P4 X0. Y0. R1. K0 ; P0 NURBS interpolation ON X1.0 Y2.0 R1. K0 ; P1 X2.5 Y3.5 R1. K0 ; P2 X4.4 Y4.0 R1. K0 ; P3 X6.0 Y0.5 R1. K1 ; P4 X8.0 Y0.0 R1. K2 ; P5 X9.5 Y0.5 R1. K3 ; P6 X11.0 Y2.0 R1. K4 ; P7 X10.5 Y4.5 R1. K5 ; P8 X8.0 Y6.5 R1. K6 ; P9 X9.5 Y8.0 R1. K7 ; P10 K8; K8; K8; K8; NURBS interpolation OFF G05 P0; High-speed high-accuracy control II mode OFF : :
Passes through control point
NURBS interpolation curve
P10(9.5,8.0)
P8(10.5,4.5)
P9(8.0,6.5)
P3(4.4,4.0)
P7(11.0,2.0)
P6(9.5,0.5)
P2(2.5,3.5)
P1(1.0,2.0)
P4(6.0,0.5) P0(0.0,0.0) P5(8.0,0.0)
10 1286420
0
1
2
3
4
5
6
7
8
9 Y
X
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
119 IB-1501277-P
All the G code, feedrate and MSTB code cannot be set during NURBS interpolation. However, when the fixed cycle G code is commanded in the same block where G06.2 is commanded, the fixed cycle G code is ignored. If a command other than the axis address designated in the 1st block of NURBS interpolation, R and K is command- ed, a program error will occur.
(1) Optional block skip "/" Cannot be set in the NURBS interpolation 2nd block or after.
(2) Control IN ")" and Control OUT "(" Cannot be set in the NURBS interpolation 2nd block or after.
(3) Local variables and common variables Can be referred but cannot be set in the NURBS interpolation. Setting the variables causes a program error (P29).
(4) System variable Cannot be referred nor set in the NURBS interpolation; a program error (P29) will occur.
The validity of program interruption/restart is shown below.
(*1) A single block stop is carried out at the last control points only. The single block stop is not applied during NURBS interpolation.
(*2) NURBS interpolation mode is canceled with Reset (Reset1/Reset2/Reset&Rewind).
(*3) The operation differs according to the manual absolute signal status. When the manual absolute signal OFF,
NURBS interpolation is carried out in the state where axis-coordinate system is shifted by the manual ab- solute movement amount. When the manual absolute signal ON
Upon automatic start after manual interruption, a program error (P554) will occur after moving by the re- maining distance. Note that the operation can run continually by returning the axis to the original position after manual inter- ruption.
(*4) "Macro interrupt" signal (UIT) is ignored.
(*5) "PLC interrupt" signal (PIT) is ignored.
Relationship with other functions
G code/Feed/Miscellaneous functions
Data format
Interruption/restart
Type During NURBS interpolation
Single block Valid (*1) Feed hold Enabled Resetting Valid (*2) Program stop Disabled Optional stop Disabled Manual interruption Invalid (*3) MDI interruption Disabled Restart search Disabled Macro interruption Invalid (*4) PLC interruption Invalid (*5)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
120IB-1501277-P
NURBS interpolation cannot be applied during graphic check (continuous/step check). Linear interpolation that connects the control points is applied during graphic check.
With the high-accuracy control in 2 part systems specification, NURBS interpolation can be commanded by 1st and 2nd part systems.
(1) Target axes for NURBS interpolation are 3 basic axes. (2) Command the control point for all the axes for which NURBS interpolation is carried out in the 1st block (G06.2
block). A program error (P32) will occur if an axis which was not commanded in the 1st block is commanded in the 2nd block or after.
(3) The first control point (G06.2 block coordinate value) should be commanded as the start point of the NURBS curve. Thus, the start point of the NURBS curve should be commanded to match the end point of the previous block. A program error will occur if the points do not match. (P552)
(4) The command range of the weight is 0.0001 to 99.9999. If "1" is commanded, the resulting command will be equal to "1.0". If more than 5 digits are commanded after the decimal point, a program error (P33) will occur.
(5) The knot command cannot be omitted, and must be commanded in each block. A program error (P33) will occur if omitted.
(6) As with knot, in the same manner as weight, up to 4 digits can be commanded after the decimal point. Even if the decimal point is omitted, the value will be handled as the one with a decimal point. If "1" is commanded, the result will be the same as "1.0". If more than 5 digits are commanded after the decimal point, a program error (P33) will occur.
(7) As with knot, command the same or greater value than the previous block. If a smaller value than previous block is set, a program error (P551) will occur.
(8) NURBS interpolation cannot be applied during graphic check (continuous/step check). Linear interpolation that connects the control points is applied during graphic check.
(9) NURBS interpolation mode is canceled with Reset (Reset1/Reset2/Reset&Rewind).
Graphic check
High-accuracy Control in 2 part Systems
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
121 IB-1501277-P
(10) NURBS interpolation can be commanded in only the following modes. If NURBS interpolation is commanded in other than the following modes, the program error (P29) will occur.
Type Mode in which NURBS interpolation can be commanded
G group 0 High-speed high-accuracy control II (G05 P10000) High-speed high-accuracy control III (G05 P20000)
G group 5 Asynchronous feed (G94) G group 7 Tool radius compensation cancel (G40) G group 8 Tool length offset +/-(G43/G44)
Tool length offset cancel (G49) G group 9 Fixed cycle cancel (G80)
G group 11 Scaling cancel (G50) G group 13 High-accuracy control ON (G61.1)
Cutting mode (G64) G group 14 User macro modal call cancel (G67) G group 15 Normal line control cancel (G40.1) G group 16 Programmable coordinate rotation mode OFF /3-dimensional coordinate conversion
mode OFF (G69) G group 17 Constant surface speed control OFF (G97) G group 18 Polar coordinate command OFF (G15) G group 19 G command mirror image cancel (G50.1) G group 21 Polar coordinate interpolation cancel (G13.1)
- Not during the coordinate rotation by parameter - Not during the mirror image by parameter setting - Not during the mirror image by external input
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
122IB-1501277-P
6.17 Hypothetical Axis Interpolation; G07
Take one of the axes of the helical interpolation or spiral interpolation, including a linear axis, as a hypothetical axis (axis with no actual movement) and perform pulse distribution. With this procedure, an interpolation equivalent to the helical interpolation or spiral interpolation looked from the side (hypothetical axis), or SIN or COS interpolation, will be possible.
Normal helical interpolation
Helical interpolation in the hypothetical axis interpolation mode
To perform the SIN interpolation on Z-X plane, execute the helical interpolation (Y-X plane: G17 G02) with Y axis, which is designated as the hypothetical axis. The hypothetical axis does not make any actual movement.
Function and purpose
Command format
G07 0 ; ... Hypothetical axis interpolation mode ON
G07 1 ; ... Hypothetical axis interpolation mode cancel
Axis name for which hypothetical axis interpolation is performed.
0.
5.
10.
-5.
-10.
20. 40. -10.0.
X X
YZ
0.
5.
10.
-5.
-10.
20. 40. -10.0.
X X
YZ
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
123 IB-1501277-P
(1) During G07 0 ; to G07 1 ;, axis will be the hypothetical axis.
(2) Any axis among the NC axes can be designated as the hypothetical axis.
(3) Multiple axes can be designated as the hypothetical axis.
(4) The number other than 0 (hypothetical axis interpolation mode ON) or 1 (cancel) is commanded, it will be han- dled as 1 (cancel). However, when only the axis name is designated without a number, it will be handled as 0 (mode ON).
(1) Interpolation functions that are used for hypothetical axis interpolation are helical interpolation and spiral inter- polation.
(2) Cancel the hypothetical axis interpolation before the high-speed high-accuracy control II (G05P10000) is com- manded.
(3) The hypothetical axis interpolation is valid only in the automatic operation. It is invalid in the manual operation mode. Handle interruption is valid even for the hypothetical axis, that is, axis will move by the interrupted amount.
(4) Movement command for the hypothetical axis will be ignored. The feedrate will be distributed in the same manner as actual axis.
(5) The protection functions such as interlock or stored stroke limit are valid for the hypothetical axis.
(6) Even when the hypothetical axis is applied for the hypothetical axis again, no error will occur and the hypothetical mode will be continued.
(7) When the hypothetical axis cancel is commanded to the actual axis, no error will occur and the axis remains as the actual axis.
(8) The hypothetical axis will be canceled by carrying out the reset 2 or reset & rewind.
Detailed description
Program example
N01 G07 Y0 ; Y axis is handled as hypothetical axis. N02 G17 G02 X0. Y0. Z40. I0. J-10. P2 F50; SIN interpolation is executed on X-Z plane. N03 G07 Y1 ; Y axis is returned to the actual axis.
Precautions
0.
5.
10.
-5.
-10.
20. 40.
X
Z
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
124IB-1501277-P
6.18 Involute Interpolation; G02.2/G03.2
Involute interpolation moves a tool along an involute curve. Also, a tool can helically travel while moving along an involute curve. This can be used for scroll machining of involute gears or compressors, and smooth accurate ma- chining can be performed without stepping of path from the command by fine segment or without acceleration/de- celeration by segment length. More accurate machining can be performed by using the automatic speed control function for the speed such as "involute interpolation override" and "acceleration rate clamping during involute interpolation".
Unless otherwise stated, the operation on the designated plane in the helical involute interpolation is the same as the normal involute interpolation.
Function and purpose
Involute Interpolation Helical Involute Interpolation
(S) Start point (E) End point
Program command path
XY plane projection path in command program
Involute curve is obtained with the following expression:
X() = R{cos (+0) + *sin (+0)} + X0
Y() = R{sin (+0) - *cos (+0)} + Y0
Circle in the right figure is the base circle.
R I
J
Y
(S)
(E)
X
X
(E)
(S)
Y
Z
(X,Y)
Y0 R
0
X
X0
Y
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
125 IB-1501277-P
The range of command value follows the input range of coordinate position data.
The range of command value follows the input range of coordinate position data.
Command format
Involute Interpolation
G02.2 (G03.2) X__ Y__ I__ J__ R__ F__; G17 plane
G02.2 (G03.2) Z__ X__ K__ I__ R__ F__; G18 plane
G02.2 (G03.2) Y__ Z__ J__ K__ R__ F__; G19 plane
G02.2/G03.2 Involute curve rotation direction (G02.2: clockwise; G03.2: counterclockwise) X End point of involute interpolation (X axis) Y End point of involute interpolation (Y axis) Z End point of involute interpolation (Z axis) I Incremental position from start point to center of base circle (X axis) J Incremental position from start point to center of base circle (Y axis) K Incremental position from start point to center of base circle (Z axis) R Base circle radius F Feedrate (in involute curve tangent direction)
Helical Involute Interpolation
G02.2 (G03.2) X__ Y__ __ I__ J__ R__ F__; G17 plane
G02.2 (G03.2) Z__ X__ __ K__ I__ R__ F__; G18 plane
G02.2 (G03.2) Y__ Z__ __ J__ K__ R__ F__; G19 plane
G02.2/G03.2 Involute curve rotation direction (G02.2: clockwise; G03.2: counterclockwise) X End point of involute interpolation (X axis) Y End point of involute interpolation (Y axis) Z End point of involute interpolation (Z axis) Linear axis end point
For , command the linear axis name. If it is used for a rotary axis, the program error (P33) occurs. Multiple linear axes can be commanded.
I Incremental position between start point and center of base circle (X axis) J Incremental position between start point and center of base circle (Y axis) K Incremental position between start point and center of base circle (Z axis) R Base circle radius F Feedrate (in involute curve tangent direction)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
126IB-1501277-P
The following information is required to perform the involute interpolation:
(1) Rotation direction (2) Start point of involute interpolation and end point coordinate (3) Base circle radius and center coordinate (4) Feedrate
The involute interpolation is performed on the selected plane. Plane selection is same as the circular command.
Operation example (G17 plane)
Detailed description
Details of operation (Involute interpolation)
G02.2 (When moving away from the base circle) G02.2 (When moving toward the base circle)
G03.2 (When moving toward the base circle) G03.2 (When moving away from the base circle)
(S) Start point (E) End point (B) Base circle
Y
(S)
(B)
(E) (Xx,Yy)
F
R
J
I (S)
(B)
(E) (Xx,Yy)
Y
F
J
R
I
(S)
(B)
(E) (Xx,Yy)
Y
F
J
I
R
(S)
(B)
(E) (Xx,Yy)
Y
F
J
I
R
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
127 IB-1501277-P
The program helically interpolates the involute curve while performing involute interpolation on the selected plane. Plane selection is same as the circular command.
Operation example (When the Z axis is commanded in the negative direction on the G17 plane)
Details of operation (Helical involute interpolation)
G02.2 (When moving away from the base circle) G02.2 (When moving toward the base circle)
G03.2 (When moving toward the base circle) G03.2 (When moving away from the base circle)
(S) Start point (E) End point (B) Base circle
Z
Y
(S)
(S)
(B) X
X (E) (X_,Z_)
(E) (X_,Y_)
J
I
R
Y
(S)
(S)
(B)
(E) (X_,Z_)
(E) (X_,Y_)
Z
J
I
R
X
X
(S)
(S)
(B)
(E) (X_,Z_)
(E) (Xx,Yy)
Z
X
X
J
I
Y
R
(S)
(S)
(B)
(E) (X_,Z_)
(E) (Xx,Yy)
Z
X
J
I
X
Y
R
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
128IB-1501277-P
Command the rotation direction with G02.2 (CW) or G03.2 (CCW). Plane selection (G17/G18/G19) and rotation di- rection (clockwise/counterclockwise) are the same as circular interpolation (G02/G03).
The start point of the involute interpolation is the current position. The end point coordinates are commanded by X and Y (or Z). The command value is either absolute or incremental based on G90/G91. There are two involute curves passing the start point, and one of them is selected as follows: When the end point is closer to the center of base circle than the start point, the involute curve moves toward
the base circle. When the end point is further from the center of base circle than the start point, the involute curve moves away
from the base circle. When the start point and the end point are at an even distance from the center of base circle, the program error
(P71) occurs because the direction of involute curve cannot be decided. When the end point is not commanded, the program error (P33) occurs. When either the start point or the end point is inside the base circle, the program error occurs (P71) because
the involute curve cannot be created. The following figure shows the positional relationship between the start point and the end point:
Command the base circle radius with R. The command value is always issued with a positive value. When the com- mand value is "0" or negative, the program error (P33) occurs. Command the center coordinate of base circle by I and J (or K). The command value is always issued with the incremental position from the start point regardless of G90/G91. Command I and J (or K) with a sign depending on the direction of base circle center as seen from the start point. When I and J (or K) is not commanded or the both are "0" (equal to the start point), the program error (P33) occurs.
Command the feedrate with "F". Command the feedrate with "F". The speed is in the involute curve tangent direc- tion.
Rotation direction
Start point and end point of involute interpolation
Base circle's radius and center coordinate
Feedrate
Y
X
When the end point is further than the start point
When the end point is closer than the start point
Start point
Base circle
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
129 IB-1501277-P
Tool radius compensation can be commanded even during the involute interpolation. Command the compensation with G40/G41/G42 in the same way as in circular interpolation. G40: Cancel tool radius compensation. G41: Compensate the left side facing forward. G42: Compensate the right side facing forward. For tool radius compensation of involute interpolation, the intersection points obtained using the approximated cir- cular command are regarded as the start and end points, and the interpolation is performed on the involute curve that connects the obtained intersection points. Command the feedrate with "F". Command the feedrate with "F". The speed is in the involute curve tangent direc- tion.
When the start point or the end point is inside the base circle as a result of compensation, the involute curve cannot be created. Therefore, even when the start point and the end point are outside the base circle before compensation, the program error (P71) occurs.
The speed at the cutting point varies depending on the curvature radius even when the feedrate of the tool center path is constant because the curvature of involute curve is not constant. This tendency is more obvious near the base circle, because the curvature radius is smaller there. The speed at the cutting point can be constant using the involute interpolation override function described later.
When the tool radius compensation is started or canceled in the involute interpolation modal or helical involute in- terpolation modal, the program error (P151) occurs.
During the involute interpolation or helical involute interpolation, interference avoidance cannot be performed. Even when the parameter "#8102 COLL. ALM OFF" is "1", the program error (P153) occurs if an interference occurs.
Tool radius compensation
Y
X
N3
N2 N1
Approximate circle of end point
Approximate circle of start point
Tool center path
Programmed path
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
130IB-1501277-P
The following two types of automatic speed control functions can be used during the involute interpolation, which can improve machining accuracy.
[Involute interpolation override]
For the tool radius compensation, the feedrate is commanded as the speed on the tool center path. However, the curvature of involute curve is inconstant, thus even when the feedrate on the tool center path is consistent, the speedat the cutting point varies depending on the curvature radius. This tendency is more obvious near the base circle, because the curvature radius is smaller there. "Involute interpolation override" function applies override to the speed on the tool center path according to the cur- vature radius so that the speed at the cutting point becomes the commanded speed.
Override value is calculated as follows:
(1) When the tool radius compensation is inside, the override may be considerably small near the base circle. The lower limit value of override can be set by "#1558 IvOMin" and the tool center speed is controlled so as not to be below the lower limit value of override. (This parameter setting depends on the MTB specifications.)
(2) When "0" is set in "#1558 IvOMin", the involute interpolation override function is invalid and the override during the tool radius compensation is always 100%.
(3) Note that when the tool radius compensation is outside, the actual travel speed becomes larger than the com- manded speed. Even in this case, the travel speed does not exceed the cutting feed clamp speed of each axis.
Automatic speed control
R: Curvature radius of tool center r: Tool radius compensation amount
Programmed path
Tool center path
Tool radius compensation Override
Inside R / (R + r) Outside R / (R - r)
Y
X
R
r
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
131 IB-1501277-P
[Involute interpolation acceleration rate clamp (High-accuracy control mode only)]
In the involute interpolation, even when the tool moves at a constant speed in the tangential direction, the acceler- ation rate increases because the curvature radius becomes smaller near the base circle. To prevent the excessive load on the machine, the speed in the tangent direction can be clamped to be at the acceleration rate set by the parameter or below according to the curvature radius in high-accuracy control mode. The allowable acceleration rate is determined by the following expression:
The clamp speed in the tangent direction is obtained by the following expression:
(Example) In the case of the following conditions:
Maximum speed "#1206 G1bF": 30000 (mm/min) Involute interpolation allowable acceleration rate "#1559 IvAMax": 600 (ms) Involute interpolation minimum feedrate "#1560 IvFMin": 1000 (mm/min)
Allowable acceleration rate is as follows:
30000 (mm/min)/600 (ms) 833.333 (mm/s2)
The clamp speed at the position of curvature radius 2 mm is as follows:
2 (mm) 833.333 (mm/s2) 2449.489 (mm/min)
(1) When "0" is set in "#1560 IvFMin", the involute interpolation acceleration rate clamp function is invalid and the speed in the tangent direction is constant regardless of the curvature radius.
(2) The clamp speed may be extremely small (or "0") near the base circle. The lower limit value of clamp speed can be set by "#1560 IvFMin" and the speed in the tangent direction is controlled so as not to be below the lower limit value of clamp speed.
(3) Note that the speed is nearly "0" when "0" is set in "#1560 IvFMin" and the curvature radius is extremely small.
Whether the normal speed designation or the involute plane component speed designation is valid depends on the MTB specifications.
Involute interpolation override is valid regardless of the setting of this parameter. Involute interpolation acceleration rate clamp is performed for the speed component on the involute plane.
(Allowable acceleration rate) = (Maximum speed)/(Involute interpolation allowable acceleration rate)
(Clamp speed) = (Curvature radius) x (Allowable acceleration rate)
: G00 X-5.708 Y0.; N1 G61.1; N2 G02.2 X0. Y10. I15.708 J10. R10. F3000; N3 G02.2 X5.708 Y0. I-10. J0. R10.; G64; :
Helical involute interpolation speed designation
#1235 set07/bit0 Meaning
0 Resultant speed designation of all the commanded axes 1 Involute plane component speed designation
Y
X
10.
N3N2
-5.708 5.7080
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
132IB-1501277-P
The program example of the absolute command on G17 plane is as below:
Program example
Involute Interpolation
G02.2 X223. Y34. I92. J-416. R100. F500; Start point of involute interpolation (50, 550) End point of involute interpolation (X, Y) 223, 34 Distance to the center of base circle (I, J) 92, -416 Base circle radius R 100 Feedrate (in curve tangent direction) 500
(S) Start point (E) End point (B) Base circle
Helical Involute Interpolation
G02.2 X223. Y34. Z-500. I92. J-416. R100. F500; Start point of involute interpolation (50., 550.) Linear axis (X axis) start point 0. End point of involute interpolation (X, Y) 223., 34. Linear axis end point (Z) -500. Incremental position between start point and cen- ter of base circle (I, J)
92., -416.
Base circle radius (R) 100. Feedrate (F) 500
(S) Start point (E) End point (B) Base circle
Y F
(S)
(B) (E)
I
J
R
X
Y
(B) (E)
(E)
(S)
(S)
F I
J
X
Z
X
R
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
133 IB-1501277-P
When the following commands are issued in involute interpolation or helical involute interpolation modal, the pro- gram error occurs.
When the following functions are used in involute interpolation modal or helical involute interpolation modal, the pro- gram error occurs. Corner rounding Corner chamfering (*1) G40 in the tool radius compensation mode causes the program error, but does not cause the error in the tool
radius compensation cancel mode.
(*2) G49 in the tool length offset mode causes the program error, but does not cause the error in the tool length offset cancel mode.
Relationship with other functions
Commands that cannot be issued in involute interpolation modal or helical involute interpolation modal
G code command G group Function
G05.1 Q2 0 Fine spline G31 0 Skip G31.1, G31.2, G31.3 0 Multi-step skip 1 to 3 G34, G35, G36, G37.1 0 Special fixed cycle G37 0 Automatic tool length measurement G38 0 Tool radius compensation vector designation G39 0 Tool radius compensation corner arc G45, G46, G47, G48 0 Tool position offset G53.1 0 Tool axis direction control G60 0 Unidirectional positioning G40 (*1) 7 Tool radius compensation cancel G41, G42 7 Tool radius compensation/3-dimensional tool radius compensa-
tion/nose radius compensation G41.2, G42.2 7 3-dimensional tool radius compensation (Tool's vertical-direction
compensation) G43, G44 8 Tool length offset G43.4, G43.5 8 Tool center point control G43.7 8 Tool position compensation G49 (*2) 8 Tool length offset cancel G51 11 Scaling ON G63 13 Tapping mode G63.1, G63.2 13 Synchronous tap mode G41.1, G42.1 G151, G152
15 Normal line control
G68 16 Coordinate rotation ON 3-dimensional coordinate conversion ON
G68.2, G68.3 16 Inclined surface machining command G69 16 Coordinate rotation cancel
3-dimensional coordinate conversion cancel G96 17 Constant surface speed control ON G16 18 Polar coordinate command ON G51.1 19 Mirror image by G code ON G7.1, G107 21 Cylindrical interpolation G12.1, G112 21 Polar coordinate command ON
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
134IB-1501277-P
When the involute interpolation (G02.2, G03.2) is commanded in the following modes, the program error occurs.
When the involute interpolation or helical involute interpolation (G02.2, G03.2) is commanded while the following are used, a program error occurs. Mirror image by parameter setting Mirror image by external input
Mode in which involute interpolation cannot be commanded
G code command G group Function
G05.1 Q2 0 Fine spline G10 0 Parameter input by program/Compensation data input G41, G42 7 Nose R compensation G41.2, G42.2 7 3-dimensional tool radius compensation (Tool's vertical-direction
compensation) G43.4 G43.5
8 Tool center point control
G43.7 8 Tool position compensation G51 11 Scaling G63 13 Tapping mode G63.1, G63.2 13 Synchronous tap mode G41.1, G42.1 G151, G152
15 Normal line control
G68 16 3-dimensional coordinate conversion G96 17 Constant surface speed control G16 18 Polar coordinate command G51.1 19 Mirror image by G code ON G7.1, G107 21 Cylindrical interpolation G12.1, G112 21 Polar coordinate interpolation
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
135 IB-1501277-P
(1) This function does not support SSS control. Even when "#8090 SSS ON" is "1" (ON), the involute block operates with SSS control OFF. It decelerates once before and after the involute block.
(2) Even when "#1572 cirorp" is "1" (ON), the overlap is not performed between a linear or arc block and involute block.
(3) Involute interpolation can be commanded in high-speed machining mode or high-speed high-accuracy mode, but does not support these modes. The fine segment processing capability is the same as the speed in the nor- mal mode.
(4) This function does not support graphic check. The start point and end point are traced linearly in the involute block.
(5) G68 is a G code that is common to the coordinate rotation by program and the 3-dimensional coordinate conver- sion. The involute interpolation can be commanded during the execution of the coordinate rotation by program; however, when it is commanded in 3-dimensional coordinate conversion, a program error occurs.
(6) When this function is carried out by selecting a plane other than the one designated with "#8621 Coord rot plane (H)" and "#8622 Coord rot plane (V)" during the execution of the coordinate rotation by program, a program error occurs.
(7) When you carried out the coordinate rotation by program or the 3-dimensional coordinate conversion, command the involute interpolation after performing positioning or linear interpolation with the absolute position for the two axes within the planes to which coordinate rotation was performed. If the involute interpolation is commanded without performing positioning or linear interpolation, a program error may occur.
(8) The involute interpolation does not support reverse run. If the reverse run is performed to this function, a program error occurs.
Note that if the end point is not on the involute curve that passes through the start point, the following operation re- sults: When the error L is greater than "#8077 Invlute error", the program error (P70) occurs at the start point of the
involute interpolation. When the error L is the same or smaller than "#8077 Invlute error", the curve is in the direction toward the
commanded end point.
When the end point error is large, the actual speed may be different from the commanded feedrate.
When the involute error is not set (setting value: 0.000), the allowable error is 0.1 (mm) as a default value.
Precautions and restrictions
End point error
L
Y
X
The involute curve through the end point
The involute curve through the start point
End pointStart point
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
6 Interpolation Functions
136IB-1501277-P
Set the number of revolutions within 100 from the start point of the curve at start/end point of involute interpolation. The times of rotations is obtained by the angle indicated with in the calculation formula of the involute curve in the "Function and purpose" section. ( 360 100)
X() = R{cos (+0) + *sin (+0)} + X0
Y() = R{sin (+0) - *cos (+0)} + Y0
When the number of revolutions exceeds 100 times, the program error (P35) occurs.
When involute interpolation override is combined with cutting override, it is performed before cutting override.
Number of revolutions
Cutting override
7
137 IB-1501277-P
Feed Functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
138IB-1501277-P
7Feed Functions 7.1 Rapid Traverse Rate 7.1.1 Rapid Traverse Rate
The rapid traverse rate can be set with parameters independently for each axis. The available speed ranges are from 1 mm/min to 10000000 mm/min. The upper limit is subject to the restrictions limited by the machine specifica- tions. Refer to the specifications manual of the machine for the rapid traverse rate settings. The feedrate is valid for the G00, G27, G28, G29, G30 and G60 commands. Two paths are available for positioning: the interpolation type where the area from the start point to the end point is linearly interpolated or the non-interpolation type where movement proceeds at the maximum speed of each axis. The type is selected with parameter "#1086 G0Intp". The positioning time is the same for each type.
If the high-accuracy control mode's rapid traverse rate is set, the axis will move at that feedrate during high-accuracy control, high-speed high-accuracy control I/II/III, high-accuracy spline control or SSS control. If the value set for the high-accuracy control mode rapid traverse rate is 0, the axis will move at the rapid tra-
verse rate. The high-accuracy control mode rapid traverse rate can be set independently for each axis. The high-accuracy control mode rapid traverse rate is effective for the following G commands: G00, G27, G28,
G29, G30 and G60. Override can be applied on the high-accuracy control mode rapid traverse rate using the PLC signal supplied.
(The operation of the PLC signal depends on the MTB specifications.)
(1) Rapid traverse override Override can be applied by a PLC input signal for both manual and automatic rapid traverse. There are 2 types which are determined by the PLC specifications. Type1 : Override in 4 steps (1%, 25%, 50% and 100%). Type2 : Override in 1% steps from 0% to 100%.
Function and purpose
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
139 IB-1501277-P
7.1.2 G00 Feedrate Command (,F Command)
Use this function to specify G00 (positioning command) and an axis feedrate in G00 mode. The speed of tool exchange, axis movement of gantry, etc. can be specified with the machining program so that the mechanical vibration can be suppressed. Operations other than the feedrate follows the G00 specification.
(1) ",F" command is in effect only in the block in which it is commanded. (2) If ",F" is commanded in G00, G27 to G30, G60, G00 mode, a block other than the one that specifies the move-
ment to the initial point of the hole position for the drilling cycle or a block that does not contain a movement command (axis address command), ",F" is ignored.
(3) ",F" command in the feed per revolution (G95) mode will also be considered a feed per minute feedrate. (4) The motion of the ",F" command varies depending on the status of parameter "#1086 G0Intp".
Feedrates when commanding G00 X200. Z300. ,F1000
fx: Actual X axis rate
fz: Actual Z axis rate
(5) When the ",F" command has not been issued, the rapid traverse rate set by the axis specification parameter will be valid. (*1)
Function and purpose
Command format
Rapid traverse at a feedrate specified with the ",F" command
G00 X_ Z_ (Y_) ,F1000;
,F Specifies the rapid traverse rates for G00, movement in G00 mode and the move- ment during the fixed cycle for drilling. The range is equal to the range of the feed per minute F command (mm/min, inch/ min) in the G01 mode. Switching inch/mm is invalid for rotary axes.
Detailed description
"#1086 G0Intp" Handling of ",F"command
OFF (see figure shown at below left) Handled as an interpolation speed. ON (see figure shown at below right) Handled as a commanded speed for each axis.
When "G0 non-interpolation" is OFF When "G0 non-interpolation" is ON
E
Z
X X
Z S S
E
300 fz = 832.05(mm/min) fz = 1000(mm/min)
1000(mm/min)
fz =
1 00
0( m
m /m
in )
fx =
5 54
.7 0(
m m
/m in
)
300
20 0
20 0
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
140IB-1501277-P
(6) The ",F" command is clamped by the rapid traverse rate set by the axis specification parameter. (*1) Feedrate clamping depends on the setting of parameter "#1086 G0Intp".
(*1) The rapid traverse rate parameter depends on the MTB specifications.
Typically, parameter "#2001 rapid" is selected.
(1) Feedrate command in G00 block and G00 mode (for G00 interpolation)
(2) Speed command for the movement to the initial point of the hole position for the drilling cycle (for the tapping cycle of machining center system)
"#1086 G0Intp" Speed clamp
OFF If it is found that, after converting ",F" command value (interpolation speed) into a speed for each axis, there is an axis for which the programmed feedrate exceeds the rapid traverse rate parameter, the interpolation speed is calculated so that it does not exceed the rapid traverse rate. (*1)
ON An axis whose ",F" command value (per axis speed) exceeds the rapid traverse rate parameter is clamped to a speed specified by the parameter. (*1) For an axis that does not exceed the rapid traverse rate parameter, the command- ed speed is applied.
Program example
: G00 X100. Z100. ,F1000 ; The tool moves at the combined feedrate, 1000 (mm/min), of XZ. X200. Z200. ; The X and Z axes interpolate at the fastest feedrate that does not exceed the
rapid traverse rate parameter for each of these axes. X300.Z300. ,F2500 ; The tool moves at the combined feedrate, 2500 (mm/min), of XZ.
:
: G88 X-20. Z30 R5. F1.D3 S500 ,R1 ,F2000 ;
The tool moves to the initial point (Z30.) of the hole position at 2000 (mm/min). Positioning (G00) during the drilling cycle moves at 2000 (mm/min).
X-20. Z35. R5. ; The tool moves to the initial point (Z35.) of the hole position at the X axis rapid traverse rate (parameter setting value).
X-20. Z40. R5.,F3000 ; The tool moves to the initial point (Z40.) of the hole position at 3000 (mm/min). Positioning (G00) during the drilling cycle moves at 2000 (mm/min).
G80 ; :
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
141 IB-1501277-P
When ",F" is specified, constant-gradient acceleration/deceleration control is applied to the feedrate specified by ",F". The feedrate (vertical axis in the figure below) varies depending on whether or not the ",F" command has been is- sued. When the ",F" command has not been issued, the parameter "#2001 rapid" (Rapid traverse rate) setting is applied to the feedrate. When the ",F" command has been issued, the ",F" command is applied to the feedrate.
The rapid traverse is performed at the feedrate specified with ",F" address.
The feedrate is accelerated or decelerated in accordance with the pattern of acceleration rate calculated from the following parameters: "#2001 rapid" (Rapid traverse rate) "#2151 rated_spd" (Rated speed) "#2153 G0t_rated" (G0 time constant up to rated speed) "#2152 acc_rate" (Acceleration rate in proportion to the maximum acceleration rate)
An override for ",F" command
The override cancel for the rapid traverse override is also invalid when ",F" is specified.
Relationship with Other Functions
Rapid traverse constant-gradient acceleration/deceleration
When the travel distance is short (a) Rapid traverse rate by #2001 or ",F" command speed
When the travel distance is long (Ts) Time constant
Rapid traverse constant-gradient multi-step acceleration/deceleration
Rated speed
Rapid Traverse Rate Feedrate specified by ",F"
Time
Rapid traverse override
Override cancel
(Ts)
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
142IB-1501277-P
Dry run is valid when the parameter "#1085 G00Drn" is ON and the rapid traverse is OFF. The axis will move at the manual feedrate that is set. If the manual override valid is turned ON, the cutting feed override also becomes valid.
It is also valid when ",F" is specified.
It is also valid when ",F" is specified.
",F" command is ineffective in tool center point control.
When an ",F" command is specified in the fixed cycle for drilling, the movement between hole positions is carried out at the speed commanded with ",F". ",F" commands in the same block as for the special fixed cycle are ignored.
When an ",F" command is specified in the same block as G60 (unidirectional positioning), the feedrate specified by ",F" is assumed.
When an ",F" command is specified in the same block as G27 (reference position check), G29 (start point return), and/or G30.n (tool change position return), the feedrate specified by ",F" is assumed.
When an ",F" command is specified in the same block as G28 (reference position return) and G30 (2nd to 4th ref- erence position return), the feedrate specified by ",F" is assumed. Axes not subject to high-speed reference position return are returned by the dog-type of in the same way as with the manual type. The feedrate depends on the MTB specifications (parameter "#2025 G28rap").
(1) If an ",F" command is specified when there is no specifications for the feedrate specified for G00, a program error (P39) will occur.
(2) ",F" and "F" commands may be specified in the same block. The "F" command is assumed to the feedrate for cutting feed.
(3) Depending on the MTB specifications (parameter "#1100 Tmove"), compensation may be performed on a block that does not contain a move command. If an ",F" is specified in a tool compensation command (T command) block in which no move command is spec- ified, compensation move is made at the feedrate specified by ",F" only in G00 mode.
(4) If an ",F" is specified in a tool radius compensation cancel command (G40) block in which no move command is specified, tool radius compensation is canceled at the specified feedrate only in G00 mode. This is the same as when using the tool nose radius compensation instead of tool radius compensation.
Dry run
External deceleration
Programmable in-position check
Tool center point control
Special fixed cycle
Unidirectional positioning
Reference position check, Start point return, Tool change position return
Reference position return, 2nd to 4th reference position return
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
143 IB-1501277-P
7.2 Cutting Feedrate
The cutting feedrate is assigned with address F and numerals. The cutting feedrate is valid for the G01, G02, G03, G02.1 and G03.1 commands.
If the cutting clamp feedrate for the high-accuracy control mode is set, the axis will move at that feedrate during high- accuracy control, high-speed high-accuracy control I/II/III, high-accuracy spline control or SSS control. If the value set for the high-accuracy control mode cutting clamp speed is "0", the axis will be clamped at the
cutting feed clamp speed. The cutting feedrate is clamped with high-accuracy control mode cutting clamp speed in the parameter.
Examples Feed per minute (asynchronous feed)
Speed range that can be commanded (when input setting unit is 1m)
(1) A program error (P62) will occur when there is no F command in the first cutting command (G01, G02, G03) after the power has been turned ON.
Function and purpose
Feedrate
G01 X100. Y100. F200 ; 200.0mm/min F200 or F200.000 gives the same rate. G01 X100. Y100. F123.4 ; 123.4mm/min G01 X100. Y100. F56.789 ; 56.789mm/min
Command Mode Feedrate command range
Remarks
mm/min 0.001 to 10000000 inch/min 0.0001 to 1000000
/min 0.001 to 10000000
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
144IB-1501277-P
7.3 F1-digit Feed
By setting the F1-digit feed parameter, the feedrate which has been set to correspond to the 1-digit number following the F address serves as the command value. When F0 is assigned, the rapid traverse rate is established and the speed is the same as for G00. (G modal does not change, but the acceleration/deceleration method follows the rapid traverse setting.) When F1 to F5 is assigned, the feedrate set to correspond to the command serves as the command value. If F1-digit feedrate changing valid signal is turned ON when F1-digit feed is commanded, the feedrate specified by the parameter can be increased or decreased by operation of manual handle. For the changing of F1-digit feedrate with the handle feed, refer to the instruction manual.
(1) To validate the F1-digit feed, the parameter "#8145 Validate F1 digit" or "#1079 f1digt" must be ON. (2) The feedrates that correspond to F1 to F5 depend on the MTB specifications (parameters "#1185 spd_F1" to
"#1189 spd_F5"). The increase/reduction range is from "0" to the set value of the parameter "#1506 F1_FM". An operation error (M01 0104) will occur when the feedrate is "0". When F0 is commanded, the acceleration or deceleration method follows the rapid traverse setting. Note that the G modal is not changed.
(3) Use of both the F1-digit command and normal cutting feedrate command is possible when the F1-digit is valid. (Example 1) F0 Rapid traverse rate F1 to F5 F1 digit F6 or more Normal cutting feedrate command
(4) The F1-digit command is valid in a G01, G02, G03, G02.1 or G03.1 modal. (5) The F1-digit command can also be used for fixed cycle. (6) The F1-digit feedrate command can also be used during high-speed high-accuracy control II.
However, a program error (P62) will occur when F0 command is issued. (7) The F1-digit command is modal. (8) The number of manual handle pulses is 1 pulse per scale unit regardless of the scaling factor. (9) During a F1-digit command, the F1-digit number and F1-digit command signal are output as the PLC signals.
(Based on the MTB specifications.)
Function and purpose
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
145 IB-1501277-P
(1) F1 to F5 are invalid in the G00 mode and the rapid traverse rate is established instead. (2) If F0 is used in the G02, G03, G02.1 or G03.1 mode, the program error (P121) will occur. The error will be elim-
inated if the F0 command is rewritten. (3) When F1. to F5. (with decimal point) are assigned, the 1mm/min to 5mm/min (direct numerical value command)
are established instead of the F1-digit feed command. (4) When the commands are used with inch units, one-tenth of the feedrate set correspond to F1 to F5 serves at the
assigned speed inch/min. (5) When the commands are used with the millimeter or degree units, the feedrate set to correspond to F1 to F5
serves as the assigned speed mm ()/min. (6) Even if the F1-digit feed is commanded during feed per revolution (G95), it is executed as a normal F command
(direct numerical value command). (7) When both the F1-digit feed command and inverse time feed command are present, the inverse time feed com-
mand will have priority. (The inverse time feed function is available only for a machining center system.)
(8) When both the F1-digit feedrate changing and the manual speed command are present, the manual speed com- mand will have the priority.
(9) In the synchronous tapping command, the speed cannot be changed with the handle.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
146IB-1501277-P
7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/
Synchronous Feed); G94,G95
By issuing the G94 command, the commands from that block are issued directly by the numerical value following F as the feedrate per minute (mm/min, inch/min).
By issuing the G95 command, the commands from that block are issued directly by the numerical value following F as the feedrate per spindle revolution (mm/rev, inch/rev). When this command is used, the rotary encoder must be attached to the spindle.
G94/G95 commands are modal commands.
(Example) After the G95 command is assigned, the G95 command is valid until the G94 command or G93 command (inverse time feed) is assigned next.
(1) The F code command range is as follows. Metric input
Function and purpose
Feed per minute (asynchronous feed)
Feed per revolution (synchronous feed)
Command format
Feed per minute (mm/min) (asynchronous feed)
G94;
Feed per revolution (mm/rev) (synchronous feed)
G95;
Detailed description
Input Setting unit B (0.001 mm) C (0.0001 mm)
Command Mode Feed per minute Feed per revolution Feed per minute Feed per revolution Command Address F (mm/min) F (mm/rev) F (mm/min) F (mm/rev) Minimum command unit
1 (=1.000) (1.=1.000)
1 (=0.001) (1.=1.000)
1 (=1.0000) (1.=1.0000)
1 (=0.0001) (1.=1.0000)
Command range 0.001 - 1000000.000
0.001 - 999.999
0.0001 - 1000000.0000
0.0001 - 999.9999
Input Setting unit D (0.00001mm) E (0.000001mm)
Command Mode Feed per minute Feed per revolution Feed per minute Feed per revolution Command Address F (mm/min) F (mm/rev) F (mm/min) F (mm/rev) Minimum command unit
1 (=1.00000) (1.=1.00000)
1 (=0.00001) (1.=1.00000)
1 (=1.000000) (1.=1.000000)
1 (=0.000001) (1.=1.000000)
Command range 0.00001 - 1000000.00000
0.00001 - 999.99999
0.000001 - 1000000.000000
0.000001 - 999.999999
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
147 IB-1501277-P
Inch input
(2) The effective rate (actual movement speed of machine) under per-revolution feed conditions is given in the fol- lowing formula (Formula 1). FC = F N OVR ...... (Formula 1) FC: Effective rate (mm/min, inch/min) F: Commanded feedrate (mm/rev, inch/rev) N: Spindle rotation speed (r/min) OVR: Cutting feed override When multiple axes have been commanded at the same time, the effective rate FC in formula 1 applies in the vector direction of the command.
(1) The effective rate (mm/min or inch/min), which is produced by converting the commanded speed, the spindle rotation speed and the cutting feed override into the per-minute speed, appears as the FC on the monitor 1. Screen of the setting and display unit.
(2) When the above effective rate exceeds the cutting feed clamp rate, it is clamped at that clamp rate. (3) If the spindle rotation speed is zero when feed per revolution is executed, an operation error (M01 0105) occurs. (4) Feedrate during the machine lock becomes the command speed. (5) Under dry run conditions, feed per minute applies and movement results at the manual feedrate (mm/min or inch/
min). (6) The fixed cycle G84 (tapping cycle) and G74 (reverse tapping cycle) are executed in accordance with the feed
mode that is already designated. (7) Whether feed per minute (G94) or feed per revolution (G95) is to be established when the power is turned ON
or when M02 or M30 depends on the MTB specifications (parameter "#1074 I_Sync").
Input Setting unit B (0.0001inch) C (0.00001inch)
Command Mode Feed per minute Feed per revolution Feed per minute Feed per revolution Command Address F (inch/min) F (inch/rev) F (inch/min) F (inch/rev) Minimum command unit
1 (=1.0000) (1.=1.0000)
1 (=0.0001) (1.=1.0000)
1 (=1.00000) (1.=1.00000)
1 (=0.00001) (1.=1.00000)
Command range 0.0001 - 100000.0000
0.0001 - 999.9999
0.00001 - 100000.00000
0.00001 - 999.99999
Input Setting unit D (0.000001inch) E (0.0000001inch)
Command Mode Feed per minute Feed per revolution Feed per minute Feed per revolution Command Address F (inch/min) F (inch/rev) F (inch/min) F (inch/rev) Minimum command unit
1 (=1.000000) (1.=1.000000)
1 (=0.000001) (1.=1.000000)
1 (=1.0000000) (1.=1.0000000)
1 (=0.0000001) (1.=1.0000000)
Command range 0.000001 - 100000.000000
0.000001 - 999.999999
0.0000001 - 100000.0000000
0.0000001 - 999.9999999
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
148IB-1501277-P
7.5 Inverse Time Feed; G93
During inside cutting when machining curved shapes with radius compensation applied, the machining speed on the cutting surface becomes faster than the tool center feedrate. Therefore, problems such as reduced accuracy may occur.
This reduced accuracy can be prevented with inverse time feed. This function can, in place of normal feed com- mands, issue one block of machining time (inverse) in F commands. The machining speed on the cutting surface is constantly controlled, even if radius compensation is applied to the machining program that expresses the free curve surface with fine segment lines.
Note that when the calculated machining time exceeds the cutting feed clamp speed, the F command value in the inverse time feed follows the cutting feed clamp speed.
Function and purpose
Regular F command
Actual machining speed: High Actual machining speed: Low The speed of tool center is commanded, thus the ac- tual speed at the cutting surface may become larger or smaller.
F command
Inverse time feed
The actual machining speed is constant. The actual speed at the cutting surface is command- ed, thus, the speed will be constant and machining speed can be maintained as commanded regard- less of the tool radius.
F command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
149 IB-1501277-P
Inverse time feed (G93) is a modal command. Once commanded, it will be valid until feed per minute or feed per revolution is commanded.
In movement blocks, since processing time is commanded to a line segment, command the feedrate "F" each time.
(1) Inverse time feed (G93) is a modal command. Once commanded, it is valid until feed per minute (G94) or feed per revolution (G95) is commanded, or until a reset (M02, M30, etc.) is executed.
(2) Command method of F command values in inverse time feed
(3) The initial modal after a restart is G94 (feed per minute) or G95 (feed per revolution). (4) The feedrate of the block inserted in tool radius compensation and corner R/C is the same speed as the feedrate
of the block immediately before it. (5) The feedrate of the block inserted in C axis normal line control (normal line control type II) is the same speed as
the feedrate of the movement block after turning.
Command format
Inverse time feed
G93;
G00 Xx1 Yy1; G93; -> Inverse time feed mode ON G01 Xx2 Yy2 Ff2; -> In inverse time feed mode G02 Xx3 Yy3 Ii3 Jj3 Ff3; : G94 (G95); -> Inverse time feed mode OFF
Detailed description
Metric command (G21) Inch command (G20)
In linear mode (G01)
Cutting point feedrate (mm/min)
Line segment length (mm)
Cutting point feedrate (inch/min)
Line segment length (inch) In arc mode (G02, G03)
(G02.1, G03.1)
Cutting point feedrate (mm/min)
Start point arc radius (mm)
Cutting point feedrate (inch/min)
Start point arc radius (inch) Command
range B 0.001 to 999999.999 (1/min) C 0.0001 to 999999.9999 (1/min) D 0.00001 to 999999.99999 (1/min) E 0.000001 to 999999.999999 (1/min)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
150IB-1501277-P
When using inverse time feed during tool radius compensation
Comparison between feed per minute and inverse time feed (Assuming that tool radius is 10. [mm]) (Unit: mm/min)
Program example
Feed per minute N01 G90 G00 X80. Y-80. ; N02 G01 G41 X80. Y-80. D11 F500 ; N03 X180. ; N04 G02 Y-280. R100. ; N05 G03 Y-480. R100. ; N06 G02 Y-680. R100. ; N07 G01 X80. F500 ; N08 Y-80. ; N09 G04 X80. Y-80. ; N10 M02 ;
Inverse time feed N01 G90 G00 X80. Y-80. ; N02 G01 G41 X80. Y-80. D11 F500 ; N03 X180. ; N04 G93 G02 Y-280. R100. F5 ; N05 G03 Y-480. R100. F5 ; N06 G02 Y-680. R100. F5 ; N07 G94 G01 X80. F500 ; N08 Y-80. ; N09 G04 X80. Y-80. ; N10 M02 ;
Sequence No. Feed per minute Inverse time feed
Feedrate of tool cen- ter
Feedrate of cutting point
Feedrate of tool cen- ter
Feedrate of cutting point
N04 F500 F450 F550 F500 N05 F500 F550 F450 F500 N06 F500 F450 F550 F500
The block seam pro- trudes due to the cut- ting speed change at the block seam.
The feedrate follows the command regard- less of the tool radius.
N4
N5
N6
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
151 IB-1501277-P
(1) Scaling (G51) When using a scaling function, issue a F command for the shape after scaling. For example, if a doublesize scal- ing is carried out, the machining distance will be twice.
Thus, if executing a cutting at the same speed as that of before scaling, command the value (F') calculated by dividing F value by the multiples of scaling.
(2) High-speed machining mode II (G05P2) With the inverse time feed (G93) modal, high-speed machining mode II (G05P2) is operated in the inverse time feed mode, instead of high-speed machining mode. High-speed machining mode will be valid when the inverse time feed mode is canceled.
(3) If the speed calculated in the G93 mode exceeds the speed range at the feed per minute, clamping is performed at the clamp speed set with parameters.
(4) The program error (P125) will occur when the commands below are issued in the inverse time feed (G93) mode.
(5) The program error (P125) will occur if inverse time feed (G93) is commanded in the following modes.
Relationship with other functions
F = Feedrate (mm/min) / Distance (mm)
Shape after scaling (Double size)
G code Function
G02.3, G03.3 Exponential interpolation G06.2 NURBS interpolation G12 Circular cutting CW G13 Circular cutting CCW G31 to G31.3 Skip G33 Thread cutting G34 to G36, G37.1 Special fixed cycle G37 Automatic tool length measurement G73 to G89 Fixed cycle G96 Constant surface speed control ON
G code Function
G02.3, G03.3 Exponential interpolation G33 Thread cutting G73 to G89 Fixed cycle G96 Constant surface speed control ON
F F' =
2
F
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
152IB-1501277-P
(1) The initial modal after a restart is G94 (feed per minute) or G95 (feed per revolution). (2) The F command in G93 modal is unmodal. Issue an F command for each block. The program error (P62) will
occur in blocks with no F command. (3) The program error (P62) will occur when F0 is commanded. (4) An F command is necessary when changing from G93 to G94 or G95. The program error (P62) will occur if there
is no F command. (5) The feed function is clamped at the maximum cutting speed. Consequently, the feed may be slower than the
commanded speed. (6) If an extremely slow speed such as F0.001 is designated, an error will occur in the machining time.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
153 IB-1501277-P
7.6 Feedrate Designation and Effects on Control Axes
It has already been mentioned that a machine has a number of control axes. These control axes can be divided into linear axes which control linear movement and rotary axes which control rotary movement. The feedrate is designed to assign the displacement speed of these axes, and the effect exerted on the tool movement speed which poses problems during cutting differs according to when control is exercised over the linear axes or when it is exercised over the rotary axes. The displacement amount for each axis is assigned separately for each axis by a value corresponding to the respec- tive axis. The feedrate is not assigned for each axis but assigned as a single value. Therefore, when two or more axes are to be controlled simultaneously, it is necessary to understand how this will work for each of the axes in- volved. The assignment of the feedrate is described with the following related items.
Function and purpose
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
154IB-1501277-P
Even when only one machine axis is to be controlled or there are two or more axes to be controlled simultaneously, the feedrate which is assigned by the F code functions as a linear speed in the tool advance direction.
(Example) When the feedrate is designated as "f" and linear axes (X and Y) are to be controlled:
When only linear axes are to be controlled, it is sufficient to designate the cutting feed in the program. The feedrate for each axis is such that the designated rate is broken down into the components corresponding to the movement amounts.
(Example) When the feedrate is designated as "f" and the linear axes (X and Y) are to be controlled using the circular interpolation function:
The rate in the tool advance direction, or in other words the tangential direction, will be the feedrate designated in the program.
In this case, the feedrate of the X and Y axes will change along with the tool movement. However, the combined speed will always be maintained at the constant value "f".
Detailed description
When controlling linear axes
... Feedrate for X axis
... Feedrate for Y axis
(S) Tool start point (E) Tool end point (F) Speed in this direction is "f".
(S) Tool start point (E) Tool end point (F) Speed in this direction is "f".
Y
Xx
y = f
x
= f y
x2 + y2
x2 + y2 (E)
(F)
(S)
fx
fy
y
x
Y
Xi
(E)
(F)
(S)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
155 IB-1501277-P
When rotary axes are to be controlled, the designated feedrate functions as the rotary speed of the rotary axes or, in other words, as an angular speed. Consequently, the cutting feed in the tool advance direction, or in other words the linear speed, varies according to the distance between the center of rotation and the tool. This distance must be borne in mind when designating the feedrate in the program.
(Example) When the feedrate is designated as "f" and rotary axis (C) is to be controlled ("f" units = /min)
In this case, the cutting feed (linear feed) in the tool advance direction "fc" is obtained as follows:
Therefore, the feedrate to be designated in the program must be as follows:
When controlling rotary axes
(S) Tool start point (E) Tool end point (CP) Center of rotation (F) Angular speed is "f".
(S) c
(E)
r (CP)
(F)
fc
fc = f r 180
f = fc 180 r
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
156IB-1501277-P
The controller proceeds in exactly the same way whether linear or rotary axes are to be controlled. When a rotary axis is to be controlled, the numerical value assigned by the coordinate word (A, B, C) is the angle and the numerical values assigned by the feedrate (F) are all handled as linear speeds. In other words, 1 of the rotary axis is treated as being equivalent to 1mm of the linear axis. Consequently, when both linear and rotary axes are to be controlled simultaneously, in the components for each axis of the numerical values assigned by F will be the same as previously described "When controlling linear axes". However, although in this case both the size and direction of the speed components based on linear axis control do not vary, the direction of the speed components based on rotary axis control will change along with the tool move- ment (their size will not change). This means, as a result, that the combined tool advance direction feedrate will vary along with the tool movement.
(Example) When the feedrate is designated as "f" and the linear axis (X) and the rotary axis (C) are to be controlled simultaneously:
In the figure below, the X axis incremental command value is "x" and the C axis incremental command values is "c":
X axis feedrate (linear speed) "fx" and C axis feedrate (angular speed) "" are expressed as:
Linear speed "fc" based on C axis control is expressed as:
If the speed in the tool advance direction at start point (S) is "ft" and the component speeds in the X axis and Y axis directions are "ftx" and "fty", respectively, then these can be expressed as:
Where "r" is the distance (in millimeters) between center of rotation and tool and "" is the angle (in degrees) between the (S) point and the X axis at the center of rotation.
When linear and rotary axes are to be controlled at the same time
(S) Tool start point (E) Tool end point (CP) Center of rotation
Size and direction are fixed for "fx". Size is fixed for "fc" but direction varies. Size and direction vary for "ft".
...... (1) ...... (2)
...... (3)
...... (4)
...... (5)
(S)
x
fc
c
fc ft
fx
fx
ft r
(E)
(CP)
fx = f x2 + c 2
x = f x2 + c 2
c
fc = 180
r
ftx = - rsin ( ) + fx 180
180
fty = - rcos ( )
180 180
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
157 IB-1501277-P
The combined speed "ft" according to (1), (2), (3), (4) and (5) is as follows:
Consequently, feedrate "f" designated by the program must be as follows:
"ft" in formula (6) is the speed at the (S) point and the value of changes as the C axis rotates, which means that the value of "ft" will also change. Consequently, in order to keep the cutting feed "ft" as constant as possible the angle of rotation which is designated in one block must be reduced to as low as possible and the extent of the change in the value must be minimized.
...... (6)
...... (7)
ftx 2 + fty 2 ft =
x2 - x c rsin ( ) + ( ) 2
x2 + c2 = f
90 r c
180
180
x2 - x c rsin( ) + ( ) 2
x2 + c2 f = ft
90 r c
180
180
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
158IB-1501277-P
7.7 Selection of Axis (Axes) for Feedrate Command; G130
This function designates the feedrate of a selected axis (using the F command) to perform machining. When the feedrate of a specific axis fluctuates wildly, it may not be possible to achieve the desired surface finish. Fluctuation can be suppressed using this function, which can result in improved surface quality.
(*1) Speed differs in each block.
(*2) Speed is kept constant.
Function and purpose
When the function is invalid When the function is valid (with X axis being selected)
Resul- tant speed of all axes
Speed Speed
Time Time
Feedrate of each axis
Speed Speed
Time Time
X Y Z
(*1) X Y Z
(*2)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
159 IB-1501277-P
(1) G130 is a non-modal command of group 0. (2) G130 must be commanded alone in a block. If it is commanded in the same block with other G codes, a program
error (P45) occurs. (3) Designate the axis name "n" using an axis address set in the parameter "#1013 axname". If the designated axis
does not exist, the program error (P32) occurs. (4) When an axis address enabled with the axis name extension function is specified for the axis name "n", the pro-
gram error (P32) occurs. (5) The selection of axis (axes) for feedrate command is canceled with Reset 1, Reset 2, Reset & rewind, or Emer-
gency stop.
When using this function, designate the resultant speed for the target axis of the speed command using the F com- mand. For an axis that is not targeted for the speed command, adjust the speed so that no deviation occurs on the inter- polation path.
[When not using the selection of axis (axes) for feedrate command]
[When using the selection of axis (axes) for feedrate command]
(1) When selecting only a single axis for the speed command:
Command format
Selection of axis (axes) for feedrate command
G130 Axis name 1 Axis name 2 ... Axis name n ;
Axis name n Axis address for which axis (axes) for feedrate command is performed
Selection of axis (axes) for feedrate command cancel
G130;
Operation example
: : G01 X100. Y150. Z200. F1000; The F command is issued as the resultant speed of all axes.
The travel speed is as follows: X axis: 371.391 (mm/min) Y axis: 557.086 (mm/min) Z axis: 742.781 (mm/min) All-axes resultant speed: 1000.000 (mm/min)
: :
: : G130 X; Select the X axis for the speed command. G01 X100. Y150. Z200. F1000; The F command is issued as the speed of the X axis.
The travel speed is as follows: X axis: 1000.000 (mm/min) Y axis: 1500.000 (mm/min) Z axis: 2000.000 (mm/min) All-axes resultant speed: 2692.582 (mm/min)
: :
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
160IB-1501277-P
(2) When selecting the linear axes for the speed command in the configuration of two linear axes and one rotary axis:
(3) When switching the rotary axis, which is currently selected for the speed command, to another axis:
The selection of axis (axes) for feedrate command is only available when G code group 1 is in the following modal.
If the selection of axis (axes) for feedrate command is applied during a modal other than the above, a program error (P581) occurs.
: : G130 XY; Select a linear axis for the speed command. G01 X100. Y150. C200. F1000; The F command is issued as the resultant speed of the linear axes.
The travel speed is as follows: X axis: 554.700 (mm/min) Y axis: 832.050 (mm/min) Linear-axis resultant speed: 1000.000 (mm/min) C axis: 1109.400 (mm/min) All-axes resultant speed: 1493.576 (mm/min)
: :
: : G130 C; Select the C axis for the speed command. G01 X100. Y150. C200. F1000; The rotation speed is as follows:
C axis: 1000.000 (mm/min) G130 XY; Select a linear axis for the speed command.
(The previously selected C axis is canceled.) G01 X200. Y300. C400. F800; The travel speed is as follows:
Linear-axis resultant speed: 800.000 (mm/min) G130; Cancel of axis (axes) for feedrate command G01 X300. Y450. C600. F500; The travel speed is as follows:
All-axes resultant speed: 500.000 (mm/min) : :
Relationship with other functions
Relationship with G code group 1
G code Function name Operation in selection of axis (axes) for feedrate com- mand
G00 Positioning Operates at rapid traverse rate. G01 Linear interpolation The F command is issued as the resultant speed of the axis
for the speed command. G02/G03 Circular interpolation
Helical interpolation The F command is issued as the resultant speed of all axes.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
161 IB-1501277-P
The selection of axis (axes) for feedrate command cannot be combined with the functions shown in the table below.
Column A: Operation when the combination function is commanded while the selection of axis (axes) for feedrate command is enabled
Column B: Operation when the selection of axis (axes) for feedrate command is commanded while the combi- nation function is enabled
(1) When this function is used, the travel speed does not exceed the clamp speed of each axis. (2) If all the movement axes are targeted for the speed command, the system performs the same operation as when
this function is not used. (3) When the movement axis is not targeted for the speed command, the F command is handled as the all-axes
resultant speed. (4) The selection of axis (axes) for feedrate command does not support the F 1-digit feed function. If the F 1-digit
feed function is used, the speed commanded by F 1-digit command is handled as the resultant speed. (5) The selection of axis (axes) for feedrate command does not support the dry run function. If the dry run function
is used, the manual feedrate is handled as the resultant speed. (6) The selection of axis (axes) for feedrate command does not support the variable-acceleration pre-interpolation
acceleration/deceleration function. When the variable-acceleration pre-interpolation acceleration/deceleration is used, the F command is handled as the all-axes resultant speed.
Functions that cannot be combined with the selection of axis (axes) for feedrate command
G code Function name A B
G07 Hypothetical axis interpolation - P582 G12 Circular cutting G31 Skip G31.1-G31.3 Multi-step skip G34-G36,G37.1 Special fixed cycle G07.1 Cylindrical interpolation P581 G12.1/G112 Polar coordinate interpolation P581 G41.2/G41.3 3-dimensional tool radius compensation P162 G43.4/G43.5 Tool center point control P942 G54.4 Workpiece installation error compensation P545 G68 3-dimensional coordinate conversion
Coordinate rotation by program P581
G68.2 Inclined surface machining command P951 G70-G89 Fixed cycle P45 G93 Inverse time feed P581 M98 Figure rotation P581 - Coordinate rotation by parameter P581
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
162IB-1501277-P
7.8 Rapid Traverse Constant-gradient Acceleration/Deceleration
This function performs acceleration and deceleration at a constant gradient during linear acceleration/deceleration in the rapid traverse mode. The constant-gradient acceleration/deceleration method can be more beneficial in re- ducing cycle time in comparison to the acceleration/deceleration with fixed time constant method.
(1) Rapid traverse constant-gradient acceleration/deceleration are valid only for a rapid traverse (G00) command. Also, this function is effective only when the rapid traverse command acceleration/deceleration mode is linear acceleration/deceleration or soft acceleration/deceleration.
(2) The acceleration/deceleration patterns in the case where rapid traverse constant-gradient acceleration/deceler- ation are performed are as follows. [When the interpolation distance is long enough for the rapid traverse rate to be achieved]
Function and purpose
Detailed description
rapid : Rapid traverse rate Ts : Acceleration/deceleration time constant Td : Command deceleration check time : Acceleration/deceleration gradient T : Interpolation time L : Interpolation distance
rapid
G00 Xx1 ;L
Ts Ts Td
T
T = L
rapid +Ts
Td = Ts + (0 - 14ms)
= tan-1 rapid
Ts ( )
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
163 IB-1501277-P
[When the interpolation distance is so short that the rapid traverse rate is not achieved]
(a) Acceleration/deceleration with fixed time constant: Even if the interpolation distance is short, interpolation takes twice as long as the time constant.
(b) Constant-gradient acceleration/deceleration: The interpolation time is shorter than the acceleration/deceleration with fixed time constant.
rapid : Rapid traverse rate (Parameter "#2001 rapid") Ts1 : Acceleration/deceleration time (Parameter "#2004 G0tL") Ts2 : Acceleration/deceleration time to reach the maximum speed Td : Command deceleration check time : Acceleration/deceleration gradient
T1 : Interpolation time (Acceleration/deceleration with fixed time constant) T2 : Interpolation time (Constant-gradient acceleration/deceleration)
L : Interpolation distance
Td
L
Ts1 Ts1
T1
Ts2
rapid
Time
Speed
Next block
2Ts1
0 - 14 ms)(2 T2Td +=
rapid LTs12T2 =
=
) Ts1
rapid(tan 1
=
T1
Td
L
Ts1
rapid
T2 Ts2
Next block
Time
Speed
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
164IB-1501277-P
(3) The time required for the command deceleration check during rapid traverse constant-gradient acceleration/de- celeration is the longest one among the deceleration check times of the axes which are commanded simultane- ously. The deceleration check times of each axis is determined by the following items; rapid traverse rate (set by the parameter "#2001 rapid"); rapid traverse acceleration/deceleration time constant (set by the parameter "#2004 G0tL"); and interpolation distance (L). When multi-axis simultaneous interpolation (linear interpolations) is performed during rapid traverse constant- gradient acceleration/deceleration, the longest one among the acceleration/deceleration times of all axes is ap- plied to the other axes which were commanded simultaneously. The acceleration/deceleration time is determined for each axis by the following items; rapid traverse rate; rapid traverse acceleration/deceleration time constant; and the interpolation distance. Consequently, linear interpola- tion is performed even when the acceleration/deceleration time constant for each axis is different. However, the axis of which the acceleration/deceleration time constant is greater than the rapid traverse accel- eration/deceleration time constant ("#2004") is accelerated/decelerated with the rapid traverse acceleration/de- celeration time constant.
[2-axis simultaneous interpolation (When linear interpolation is used, Tsx < Tsz, Lx Lz)]
When the result is "Tsx < Tsz", the acceleration/deceleration time (Ts) of this block is set to Tsz (acceleration/ deceleration time of the Z axis). Since "Tdx < Tdz" is obtained as the result, the command deceleration check time (Td) of this block is set to Tdz (command deceleration check time of the Z axis).
Tsx : X axis acceleration/deceleration time Tsz : Z axis acceleration/deceleration time Tdx : X axis commanded deceleration check time Tdz : Z axis commanded deceleration check time
Lx : X axis interpolation distance Lz : Z axis interpolation distance
Tsx
Tsz Tsz Tdz
Tsx Tdx
Lx
Lz
rapid X
rapid Z
Speed
Next block
Time
Next block
Time
X axis
Z axis
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
165 IB-1501277-P
(4) If a minimum time constant for constant-gradient acceleration/deceleration has been set by the parameter, ac- celeration/deceleration speed is adjusted to prevent the acceleration/deceleration time calculated by interpola- tion distance from going below the minimum time constant.
[When the interpolation distance is so short that the acceleration/deceleration time is shorter than the
minimum time constant for constant-gradient acceleration/deceleration]
(5) Use the "Rapid traverse time constant: Switchover request" signal to switch the rapid traverse time constant. The operations via PLC signals and the settings of related parameters depend on the MTB specifications. The time constant is switched in the block next to where the "Rapid traverse time constant: Switchover request" signal is turned ON/OFF.
rapid traverse time constant or the rapid traverse time constant (primary delay)/2nd step time constant of soft acceleration/deceleration.
(6) The program format of G00 (rapid traverse command) when rapid traverse constant-gradient acceleration/decel- eration are executed is the same as when this function is invalid (acceleration/deceleration with fixed time con- stant).
rapid : Rapid traverse rate (Parameter "#2001 rapid") Ts1 : Acceleration/deceleration time (Parameter "#2004 G0tL") Ts2 : Acceleration/deceleration time to reach the maximum speed Ts3 : Minimum time for constant-gradient acceleration/deceleration (Parameter "#2198 G0tMin") Td : Command deceleration check time T : Interpolation time L : Interpolation distance
Basic rapid traverse time constant (signal OFF)
Rapid traverse time constant for switching (signal ON)
Rapid traverse time constant #2004 G0tL #2598 G0tL_2 Rapid traverse time constant (primary delay) / 2nd step time constant of soft acceleration/ deceleration
#2005 G0t1 #2599 G0t1_2
L
Ts2
Ts3
Ts1 Td
T
T = 2 Ts2
rapid
Speed
Next block
Time
Td = + (0 to 14 ms)T 2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
166IB-1501277-P
(1) The constant-gradient acceleration/deceleration during dry run is disabled. When the constant-gradient acceleration/deceleration is valid and the speed is changed by dry run during axis traveling, dry run is disabled in the currently executed block, and the constant-gradient acceleration/deceleration is performed at the same speed as before. Dry run is enabled from the next block, and the manual feedrate is applied. However, the acceleration/deceleration time remains unchanged. When dry run is enabled and it canceled during axis traveling, dry run is immediately disabled, and the cutting feedrate is applied. After the speed was changed, the constant-gradient acceleration/deceleration is enabled. When the high-speed machining mode is valid (under G5P2, under G5P10000, etc.), dry run is disabled. How- ever, when the high-speed machining mode is canceled by the positioning command (G00 command) or single block stop command, dry run is enabled. To enable dry run during the constant-gradient acceleration/deceleration, use the high-accuracy control function (G61.1). Do not use this function.
[When constant-gradient acceleration/deceleration is enabled and the "Dry run" signal is turned ON
during axis traveling]
[When dry run is enabled and the "Dry run" signal is turned OFF during axis traveling]
Relationship with other functions
clamp : Maximum cutting feedrate (Parameter "#2002 clamp") F : Cutting feedrate
mF : Manual feedrate Ts1 : Acceleration/deceleration time (Parameter "#2007 G1tL") Ts2 : Acceleration/deceleration time to reach the cutting feedrate : Acceleration/deceleration gradient
ON : "Dry run" signal ON OFF : "Dry run" signal OFF
clamp
ON
F
Ts2
mF
Ts2 Ts2
Ts1 Ts1
Ts2 Ts2Ts2
clamp
OFF
F
mF
Ts1 Ts1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
167 IB-1501277-P
(2) The constant-gradient acceleration/deceleration is valid for the rapid traverse command in the fixed cycle. To switch the rapid traverse time constant in the fixed cycle, issue the "Rapid traverse time constant: Switchover request" during G80 mode. If the "Rapid traverse time constant: Switchover request" is issued in the fixed cycle, the time constant may not be switched.
(1) Rapid traverse constant-gradient acceleration/deceleration is performed only when the motion path of the rapid traverse command is the interpolation type (parameter "#1086 G0Intp" is set to "0").
(2) When "#2003 smgst" (acceleration/deceleration mode) is set to the soft acceleration/deceleration, and "#1219 aux03 bit7" (time constant setting changeover for soft acceleration/deceleration) is set to "1", the acceleration/ deceleration speed is adjusted to prevent the sum of the 1st step and 2nd step acceleration/deceleration times from going below the minimum time constant for constant-gradient acceleration/deceleration. In this case, the acceleration time will be "G0tL+G0t1" or "G1tL+G1t1".
(3) When "#2003 smgst" (acceleration/deceleration mode) is set to the soft acceleration/deceleration, if the acceler- ation/deceleration is shorter than G0tL (or G1tL), the 2nd step time constant will be reduced by the same rate as the 1st step time constant.
(4) If a commanded travel distance in a block is small, acceleration/deceleration time becomes quite short when the constant-gradient acceleration/deceleration method is enabled. Although this does contribute to reduce the cycle time, this can also be a cause of machine vibrations. In these cases, if the minimum time constant for constant- gradient acceleration/deceleration is set in parameter "#2198 G0tMin", it is possible to perform acceleration/de- celeration to prevent the acceleration/deceleration time from being below this setting value. This parameter de- pends on the MTB specifications.
(5) When the parameter "#1253 set25/bit2" (Acceleration/deceleration mode change in hole drilling cycle) is set to "1" (constant-gradient, acceleration/deceleration after interpolation), the rapid traverse in the fixed cycle modal is set to the constant-gradient acceleration/deceleration regardless of the setting of the parameter "#1200 G0_acc" (Validate acceleration and deceleration with inclination constant G0).
(6) If any one of the following commands is issued in the next block in which the "Rapid traverse time constant: Swi- tchover request" signal is turned ON, the time constant switching may be delayed. G27 (Reference position check) G28 to G30 (Reference position return) G30.1 to G30.6 (Tool exchange position return) G60 (Unidirectional positioning)
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
168IB-1501277-P
7.9 Rapid Traverse Constant-gradient Multi-step Acceleration/Deceleration
This function carries out the acceleration/deceleration according to the torque characteristic of the motor in the rapid traverse mode during automatic operation. (This function is not available in manual operation.) The rapid traverse constant-gradient multi-step acceleration/deceleration method makes for improved cycle time because the position- ing time is shortened by using the motor ability to its maximum.
In general, the servomotor has the characteristic that the torque falls in the high-speed rotation range.
In the rapid traverse constant-gradient acceleration/deceleration method, the acceleration rate is treated as constant because this torque characteristic is not considered. So, It is necessary to use a minimum acceleration rate within the used speed range. Therefore, the margin of acceleration rate must be had in a low-speed range. Or if the accel- eration rate is used to its maximum, the upper limit of the rotation speed must be slowed.
Then, to use the servomotor ability to its maximum, acceleration/deceleration to which the torque characteristic is considered is carried out by the rapid traverse constant-gradient multi-step acceleration/deceleration method.
The acceleration/deceleration patterns in the case where rapid traverse constant-gradient multi-step acceleration/ deceleration are performed are as follows.
Function and purpose
[Rapid traverse constant-gradient multi- step acceleration/deceleration]
[Rapid traverse constant-gradient acceleration/ deceleration]
Number of steps is automatically adjusted by parameter setting.
It was necessary to slow down the acceleration rate for high speed rotation.
(f) Speed (t) Time (a) Acceleration rate
t bt a
(f)
(t)
(f)
(t)
(t)
(t)
(a) (a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
169 IB-1501277-P
(1) The validity of this function depends on the MTB specifications. (Parameter "#1205 G0bdcc") However, note the following conditions. (a) "2" cannot be set to parameter "#1205 G0bdcc" except the 1st part system. When "2" is set to other than 1st
part system, an MCP alarm (Y51 0017) will occur. (b) When there is no specification for the rapid traverse constant-gradient acceleration/deceleration, "2" cannot
be set to parameter "#1205 G0bdcc". Even if the parameter is set to "2", this function is invalid. A normal time constant acceleration/deceleration (acceleration/deceleration after interpolation) is applied.
(c) Even if "2" is set to "#1205 G0bdcc" when G00 non-interpolation type ("#1086 G00Intp" = "1"), this function is invalid. In this case, a normal acceleration/deceleration with fixed time constant (acceleration/deceleration after interpolation) is applied.
(2) To use this function, the following parameters must be set for each axis.
Acceleration rate in proportion to the maximum acceleration rate = Acceleration rate at rapid traverse rate / max- imum acceleration rate
(3) When either of the following conditions applies, this function is invalid and operates as "rapid traverse constant- gradient acceleration/deceleration". For the axis for which the rapid traverse constant-gradient multi-step accel- eration/deceleration is not necessary, set "0" to "#2151 rated_spd", "#2152 acc_rate" and "#2153 G0t_rated". However, these parameters depend on the MTB specifications. (a) When "#2151 rated_spd" (rated speed) is "0" or larger than "#2001 rapid" (rapid traverse) (b) When "#2152 acc_rate" (Acceleration rate in proportion to the maximum acceleration rate) is "0" or "100" (c) Even if "2" is set to "#1205 G0bdcc" when G00 non-interpolation type ("#1086 G00Intp" = "1"), this function
is invalid. In this case, a normal acceleration/deceleration with fixed time constant (acceleration/deceleration after interpolation) is applied.
Detailed description
Use conditions
#2001 rapid Rapid traverse [mm/min] #2151 rated_spd Rated speed [mm/min] #2153 G0t_rated Acceleration time to rated speed [ms] #2152 acc_rate Acceleration rate at rapid traverse in ratio to the maximum
acceleration rate [%]
Speed
rapid
rated_spd
Time
Acceleration rate
Maximum acceleration rate
Acceleration rate at rapid traverse rate
Time
(G0t_rated)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
170IB-1501277-P
(4) The comparison of the acceleration/deceleration patterns by the parameter setting is in the table below. Mode Rapid traverse constant-
gradient multi-step accel- eration/deceleration
#1086 G00Intp
#1205 G0bdcc
Operation
G00 command ON 0 0 Time constant acceleration/decelera- tion (interpolation type)
1 Constant-gradient acceleration/decel- eration (acceleration/deceleration be- fore interpolation)
2 Constant-gradient multi-step accelera- tion/deceleration
1 Arbitrary Acceleration/deceleration with fixed time constant (non-interpolation type)
OFF 0 0 Acceleration/deceleration with fixed time constant (interpolation type)
1 Constant-gradient acceleration/decel- eration (acceleration/deceleration be- fore interpolation)
2 Acceleration/deceleration with fixed time constant (interpolation type)
1 Arbitrary Acceleration/deceleration with fixed time constant (non-interpolation type)
Manual rapid traverse
Arbitrary Arbitrary Arbitrary Acceleration/deceleration with fixed time constant (non-interpolation type)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
171 IB-1501277-P
For rapid traverse constant-gradient multi-step acceleration/deceleration, the number of steps is automatically ad- justed by set parameter.
The acceleration rate per step is assumed to be a decrease by 10% of the maximum acceleration rate per step. Therefore, the number of steps is decided as follows.
The acceleration/deceleration pattern when the parameter setting value is shown below.
Decision method of steps
"Step" = (100 - "#2152 acc_rate") / 10 + 1 (Discard fractions less than 1)
No. Item Setting value
2001 rapid Rapid traverse rate 36000 [mm/min] 2151 rated_spd Rated speed 16800 [mm/min] 2152 acc_rate Acceleration rate in proportion to the maxi-
mum acceleration rate 58 [%]
Acceleration rate
f: Speed
rapid =36000
rated_spd =16800
amax
0.58amax
0.9amax
0.8amax
0.7amax
10
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
172IB-1501277-P
When there are two or more rapid traverse axes with a different pattern of the acceleration rate, there are the fol- lowing two operation methods.
Interpolation type (#1086 G0Intp = 0) : Moves from the start point to the end point by straight line Non-interpolation type (#1086 G0Intp = 1) : Each axis moves separately at the speed of the parameter Rapid traverse constant-gradient multi-step acceleration/deceleration are valid only for an interpolation type. For the interpolation type, the pattern of the acceleration rate operates to the maximum acceleration rate within the range where tolerable acceleration rate of each axis is not exceeded.
Pattern of acceleration rate at two or more axis interpolation
[Pattern of acceleration rate of Y axis] [Pattern of acceleration rate of X axis]
[Pattern of acceleration rate in the composite direction]
(a) Acceleration rate (f) Speed (S) Start point (E) End point (ac1) Pattern of acceleration rate when the axis moved to composite direction at Y axis rapid traverse rate (ac2) Pattern of acceleration rate when the axis moved to composite direction at X axis rapid traverse rate (ac3) Pattern of acceleration rate in the composite direction
Y
a y
v y (f)
(a)
4
3 5
(S)
(E)
X
a x
v x (f)
(a)
a x / 0.8
a y / 0.6
vy / 0.6 vx / 0.8
(ac2)
(a)
(f)
(ac3)
(ac1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
173 IB-1501277-P
With S-pattern filter control, this enables the rapid traverse constant-gradient multi-step acceleration/deceleration fluctuation to further smoothen.
This can be set in the range of 0 to 200 (ms) with the base specification parameter "#1569 SfiltG0" (G00 soft accel- eration/deceleration filter). With "#1570 Sfilt2" (Soft acceleration/deceleration filter 2), this also enables the acceler- ation/deceleration fluctuation to further smoothen.
S-pattern filter control
(f) Speed (t) Time
No S-pattern filter control S-pattern filter control
SfiltG0 + Sfilt2
(f)
(t)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
174IB-1501277-P
During high-accuracy control, high-speed high-accuracy control I/II/III or high-accuracy spline control, the high-ac- curacy control mode's rapid traverse rate ("#2109 Rapid (H-precision)") can be set besides rapid traverse rate ("#2001 rapid").
Operation when the value is set at the high-accuracy control mode's rapid traverse rate is as follows.
(1) When "The high-accuracy control mode rapid traverse rate" > "rapid traverse rate" This function is invalid and operates as "rapid traverse constant-gradient acceleration/deceleration".
(2) When "The high-accuracy control mode rapid traverse rate" < "rapid traverse rate" The rapid traverse is performed at the feedrate set in the parameter "#2109 Rapid (H-precision)". The feedrate is accelerated or decelerated in accordance with the pattern of acceleration rate calculated from the following parameters: "#2001 rapid" (Rapid traverse rate) "#2151 rated_spd" (Rated speed) "#2153 G0t_rated" (G0 time constant up to rated speed) "#2152 acc_rate" (Acceleration rate in proportion to the maximum acceleration rate)
The high-accuracy control mode rapid traverse rate
(f) Speed (t) Time (r) Rapid traverse rate (ac) Acceleration rate
Larger than the rated speed Smaller than the rated speed
(f) Speed (f1) Rated speed (f2) The high-accuracy control mode rapid traverse rate (t) Time (t1) Acceleration time to rated speed (ac) Acceleration rate (ac1) Maximum acceleration rate (ac2) Acceleration rate at rapid traverse rate (r) Rapid traverse rate
#2004 G0tL
(f)
(ac)
(r)
(t)
(t)
(f) (r)
(t)
(f2) (f1)
(t)
(ac) (ac1)
(ac2)
(t1)
(f)
(ac)
(f2) (f1)
(r)
(t)
(t)
(ac1)
(ac2)
(t1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
175 IB-1501277-P
(1) Rapid traverse constant-gradient multi-step acceleration/deceleration are valid only for a rapid traverse com- mand. Note that when the manual rapid traverse, rapid traverse constant-gradient multi-step acceleration/decel- eration cannot be used. In this case, an acceleration/deceleration with fixed time constant (acceleration/deceleration after interpolation) is applied. Therefore, acceleration/deceleration is decided by the following parameters. #2001 rapid : Rapid traverse rate #2003 smgst : Acceleration/deceleration mode #2004 G0tL: G00 time constant (linear) #2005 G0t1: G00 time constant (primary delay) The acceleration time (time constant) is different between the rapid traverse constant-gradient multi-step accel- eration/deceleration and the manual rapid traverse as shown in figure.
(2) Rapid traverse constant-gradient multi-step acceleration/deceleration cannot be used in part system excluding 1st part system. However, even if two or more part systems are used, it is possible to use this function in case of the 1st part system.
(3) When there is no specification for the rapid traverse constant-gradient acceleration/deceleration, this function is invalid even if "2" is set to the parameter "#1205 G0bdcc". In this case, a normal acceleration/deceleration with fixed time constant (acceleration/deceleration after interpolation) is applied.
(4) When G00 non-interpolation type ("#1086 G0Intp" = "1"), rapid traverse constant-gradient multi-step accelera- tion/deceleration cannot be used. It is valid in interpolation mode only.
(5) When the rapid traverse constant-gradient multi-step acceleration/deceleration is applied, rapid traverse accel- eration/deceleration types ("#2003 smgst" bit0 to bit3) are ignored.
(6) When the rapid traverse constant-gradient multi-step acceleration/deceleration is valid, G0 constant-gradient ("#1200 G0_acc") cannot be used. Even if G0 constant-gradient is valid ("#1200 G0_acc" = "1"), the setting is ignored.
(7) When the rapid traverse constant-gradient multi-step acceleration/deceleration is valid, programmable in-posi- tion check cannot be used. The in-position width will be ignored even if commanded.
(8) This function cannot be used during the tool center point control.
Precautions
Rapid traverse constant-gradient multi-step acceleration/deceleration
(f) Speed (t) Time (ac) Acceleration rate
Rapid traverse constant-gradient multi-step acceleration/deceleration Manual rapid traverse (linear) S-pattern filter control Soft acceleration/deceleration
(t)(f)
(f) (ac)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
176IB-1501277-P
7.10 Cutting Feed Constant-gradient Acceleration/Deceleration
This function performs linear acceleration/deceleration at a constant inclination in the cutting feed mode. The con- stant-gradient acceleration/deceleration method can be more beneficial in reducing cycle time in comparison to the acceleration/deceleration with fixed time constant method.
(1) Cutting feed constant-gradient acceleration/deceleration function is effective only when the commanded cutting feed acceleration/deceleration mode is linear method or soft method in linear interpolation (G01) command.
(2) The program format of linear interpolation when cutting feed constant-gradient acceleration/deceleration is exe- cuted is the same as when this function is invalid (acceleration/deceleration with fixed time constant).
Function and purpose
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
177 IB-1501277-P
(3) The acceleration/deceleration patterns in the case where cutting feed constant-gradient acceleration/decelera- tion is performed are as follows. [When the interpolation distance is long enough for the cutting feedrate to be achieved]
(a) Acceleration/deceleration with fixed time constant:
(b) Constant-gradient acceleration/deceleration:
In the case of acceleration/deceleration with fixed time constant, the acceleration/deceleration gradient is deter- mined by the cutting feedrate. In the case of constant-gradient acceleration/deceleration, it is determined by the maximum cutting feedrate; therefore, the cycle time will be shorter than in the former case.
clamp : Maximum cutting feedrate (Parameter "#2002 clamp") F : Cutting feedrate
Ts1 : Acceleration/deceleration time (Parameter "#2007 G1tL") 1 : Acceleration/deceleration gradient (Acceleration/deceleration with fixed time constant) 2 : Acceleration/deceleration gradient (Constant-gradient acceleration/deceleration) T1 : Interpolation time (Acceleration/deceleration with fixed time constant) T2 : Interpolation time (Constant-gradient acceleration/deceleration)
L : Interpolation distance
Ts1
L
Ts1
clamp
T1
F
1
21Ts F L
T1 +=
) Ts1 F
(tan-1=1
Ts1
L
Ts1
2
clamp
T2
F clamp FTs1
F L
T2
+=
) Ts1
clamp (tan2 -1=
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
178IB-1501277-P
[When the interpolation distance is so short that the cutting feedrate is not achieved]
The acceleration/deceleration gradient is determined by the maximum cutting feedrate.
[When the interpolation distance is so short that the maximum cutting feedrate is not achieved and the
override for cutting feed constant-gradient acceleration/deceleration is activated]
clamp : Maximum cutting feedrate (Parameter "#2002 clamp") F : Cutting feedrate
Ts1 : Acceleration/deceleration time (Parameter "#2007 G1tL") Ts2 : Acceleration/deceleration time to reach the cutting feedrate : Acceleration/deceleration gradient T : Interpolation time L : Interpolation distance
clamp : Maximum cutting feedrate (Parameter "#2002 clamp") F : Cutting feedrate
OVR : Maximum override value for cutting feed constant-gradient acceleration/deceleration (Parameter "#1367 G1AccOVRMax")
Ts1 : Acceleration/deceleration time (Parameter "#2007 G1tL") Ts2 : Acceleration/deceleration time to reach the cutting feedrate : Acceleration/deceleration gradient
) Ts1
clamp (tan -1=
L
Ts1
clamp
T
F
Ts2
clamp LTs22T =
L
Ts1
clamp
T
F OVR
Ts2
) Ts1
clamp (tan -1=
2T = clamp
OVRLTs2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
179 IB-1501277-P
[2-axis simultaneous interpolation (When Tsx < Tsz, Lx Lz)]
When multi-axis simultaneous interpolation is performed during linear interpolation constant-gradient accelera- tion/deceleration, the longest one among the acceleration/deceleration times of all axes is applied to the other axes which were commanded simultaneously. The acceleration/deceleration time is determined for each axis by the following items; maximum cutting fee- drates (parameter "#2002 clamp"); cutting feed acceleration/deceleration time constant (parameter "#2007 G1tL"); cutting feed rates (F); and the interpolation distance (L). However, the axis of which the acceleration/deceleration time constant is greater than the cutting feed acceler- ation/deceleration time constant (parameter "#2007 G1tL") is accelerated/decelerated with the cutting feed ac- celeration/deceleration time constant.
When Tsx < Tsz, the acceleration/deceleration time (Ts) of this block is set to Tsz (acceleration/deceleration time of the Z axis).
Tsx : X axis acceleration/deceleration time Tsz : Z axis acceleration/deceleration time Lx : X axis interpolation distance Lz : Z axis interpolation distance Fx : X axis feedrate Fz : Z axis feedrate
clampX
clampZ
Tsx
Tsz Tsz
Tsx
Lx
Fx
Fz
X
Lz
Z
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
180IB-1501277-P
[When the feedrate is so low that the acceleration/deceleration time is shorter than the minimum time
constant for constant-gradient acceleration/deceleration]
Acceleration/deceleration speed is adjusted to prevent the acceleration/deceleration time calculated by the cut- ting feedrate from going below the minimum time constant.
[When the interpolation distance is so short that the acceleration/deceleration time is shorter than the
minimum time constant for constant-gradient acceleration/deceleration]
Acceleration/deceleration speed is adjusted to prevent the acceleration/deceleration time calculated by interpo- lation distance from going below the minimum time constant.
clamp : Maximum cutting feedrate (Parameter "#2002 clamp") F : Cutting feedrate
Ts1 : Acceleration/deceleration time (Parameter "#2007 G1tL") Ts2 : Acceleration/deceleration time to reach the cutting feedrate Ts3 : Minimum time for constant-gradient acceleration/deceleration (Parameter "#2199 G1tMin")
T : Interpolation time L : Interpolation distance
clamp : Maximum cutting feedrate (Parameter "#2002 clamp")
F : Cutting feedrate Ts1 : Acceleration/deceleration time (Parameter "#2007
G1tL") Ts2 : Acceleration/deceleration time to reach the cutting
feedrate Ts3 : Minimum time for constant-gradient acceleration/
deceleration (Parameter "#2199 G1tMin") T : Interpolation time L : Interpolation distance
L
Ts1
clamp
T
Ts3
F
Ts2
Ts32 F
L T +=
L
Ts1
clamp
T
Ts3
F
Ts2
Ts32T =
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
181 IB-1501277-P
(1) The constant-gradient acceleration/deceleration during dry run is disabled. When the constant-gradient acceleration/deceleration is valid and the speed is changed by dry run during axis traveling, dry run is disabled in the currently executed block, and the constant-gradient acceleration/deceleration is performed at the same speed as before. Dry run is enabled from the next block, and the manual feedrate is applied. However, the acceleration/deceleration time remains unchanged. When dry run is enabled and it canceled during axis traveling, dry run is immediately disabled, and the cutting feedrate is applied. After the speed was changed, the constant-gradient acceleration/deceleration is enabled. When the high-speed machining mode is valid (under G5P2, under G5P10000, etc.), dry run is disabled. How- ever, when the high-speed machining mode is canceled by the positioning command (G00 command) or single block stop command, dry run is enabled. To enable dry run during the constant-gradient acceleration/deceleration, use the high-accuracy control function (G61.1). Do not use this function.
[When constant-gradient acceleration/deceleration is enabled and the "Dry run" signal is turned ON
during axis traveling]
[When dry run is enabled and the "Dry run" signal is turned OFF during axis traveling]
Relationship with other functions
clamp : Maximum cutting feedrate (Parameter "#2002 clamp") F : Cutting feedrate
mF : Manual feedrate Ts1 : Acceleration/deceleration time (Parameter "#2007 G1tL") Ts2 : Acceleration/deceleration time to reach the cutting feedrate : Acceleration/deceleration gradient
ON : "Dry run" signal ON OFF : "Dry run" signal OFF
clamp
ON
F
Ts2
mF
Ts2 Ts2
Ts1 Ts1
Ts2 Ts2Ts2
clamp
OFF
F
mF
Ts1 Ts1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
182IB-1501277-P
(2) The constant-gradient acceleration/deceleration is valid for the linear interpolation command in the fixed cycle. However, the constant-gradient acceleration/deceleration for linear interpolation is invalid for the linear interpo- lation command in the synchronous tapping cycle. (The synchronous tapping acceleration/deceleration is enabled.)
(1) If a value greater than 100 (%) is designated for cutting feed override under cutting feed constant-gradient ac- celeration/deceleration control, the acceleration/deceleration gradient becomes steeper as the feedrate increas- es. To use the cutting feed override function at a rate higher than 100%, set the parameter "#1367 G1AccOVRMax" accordingly. (This parameter depends on the MTB specifications.) When the setting of this parameter is between 0 and 99 for "#1367 G1AccOVRMax", the override value is handled as 100% even if the specified cutting feed override is greater than 100%.
(2) If there are one or more NC control axes that are set to soft acceleration/deceleration for G1, the parameter "#1367 G1AccOVRMax" setting will be ignored and the cutting feed override value is handled as 100%.
(3) When "#2003 smgst"(acceleration/deceleration mode) is set to the soft acceleration/deceleration, and "#1219 aux03 bit7: Time constant setting changeover for soft acceleration/deceleration" is set to "1": Acceleration time is obtained by G0tL+G0t1 (G1tL+G1t1)", acceleration/deceleration speed is adjusted to prevent the sum of the 1st step and 2nd step acceleration/deceleration times from going below the minimum time constant for constant- gradient acceleration/deceleration.
(4) When "#2003 smgst" (acceleration/deceleration mode) is set to the soft acceleration/deceleration, if the acceler- ation/deceleration is shorter than G0tL (or G1tL), the 2nd step time constant will be reduced by the same rate as the 1st step time constant.
(5) If the commanded travel distance in the block is small or the commanded linear interpolation (G01) feedrate is low, acceleration/deceleration time becomes quite short when the constant-gradient acceleration/deceleration method is enabled. Although this does contribute to reduce the cycle time, this can also be a cause of machine vibrations. In these cases, if the minimum time constant for constant-gradient acceleration/deceleration is set in parameter "#2199 G1tMin", it is possible to perform acceleration/deceleration to prevent the acceleration/decel- eration time from being below this setting value. This parameter depends on the MTB specifications.
(6) If the linear interpolation command is continuously executed in two blocks for the same axis during constant- gradient acceleration/deceleration for linear interpolation, the gradient at deceleration becomes greater than the reference value. Therefore, the load of the servo system may increase. Consider so that the speed command (F command value) does not change suddenly.
Precautions
: Reference value of gradient
) Ts
clamp(tan1=
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
183 IB-1501277-P
(1) When the linear interpolation command is continuously executed in two or more blocks for the same axis during constant-gradient acceleration/deceleration for linear interpolation, processing of the 3rd block is started after the deceleration processing of the 1st block was completed.
Restrictions
: :
N10 G01 X100. ; N20 G01 X20. ; N30 G01 X70. ;
: :
(1) Processing start of 2nd block (2) Processing of the 3rd block is not started because deceleration processing of the 1st block is not com-
pleted. (3) Processing start of 3rd block
N10
(1) (2)(3)
N20
N30
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
184IB-1501277-P
7.11 Exact Stop Check; G09
In order to prevent roundness during corner cutting and machine shock when the tool feedrate changes suddenly, there are times when it is desirable to start the commands in the following block once the in-position state after the machine has decelerated and stopped or the elapsing of the deceleration check time has been checked. The exact stop check function is designed to accomplish this purpose. A deceleration check is performed when the G09 (exact stop check) command has been designated in the same block. The G09 command is unmodal. Either the deceleration check time or in-position state is based on the parameter settings specified by the MTB. (Re- fer to section "7.13 Deceleration Check".) The in-position width is set in servo parameter "#2224 sv024", "#2077 G0inps" or "#2078 G1inps". This parameter also depends on the MTB specifications.
The exact stop check command G09 has an effect only with the cutting command (G01 - G03) in its particular block.
Function and purpose
Command format
Exact stop check
G09 G01 (G02, G03);
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
185 IB-1501277-P
[With continuous cutting feed]
[With cutting feed in-position check]
The in-position width, as shown in the figure above, is the remaining distance (shaded area in the above figure) of the previous block when the next block is started is set in the servo parameter "#2224 sv024". (This depends on the MTB specifications.) The in-position width is designed to reduce the roundness at the workpiece corners to below the constant value.
To eliminate corner roundness, set the value as small as possible to servo parameter "#2224 sv024" and perform an in-position check or assign the dwell command (G04) between blocks. (The parameter setting depends on the MTB specifications.)
Detailed description
Ts : Cutting feed acceleration/deceleration time constant In-position width
Ts
G00 Xx2;G00 Xx1;
G00 Xx1; G00 Xx2;
Ts Ts
Lc
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
186IB-1501277-P
(1) With linear acceleration/deceleration
(2) With exponential acceleration/deceleration
(3) With exponential acceleration/linear deceleration
The time required for the deceleration check during cutting feed is the longest among the cutting feed decelera- tion check times of each axis determined by the cutting feed acceleration/deceleration time constants and by the cutting feed acceleration/ deceleration mode of the axes commanded simultaneously.
To execute exact stop check in a fixed cycle cutting block, insert command G09 into the fixed cycle subpro- gram.
With deceleration check
Ts: Acceleration/deceleration time constant
Td: Deceleration check time Td = Ts + (0 to 10ms)
Ts: Acceleration/deceleration time constant
Td: Deceleration check time Td = 2 x Ts + (0 to 10ms)
Ts: Acceleration/deceleration time constant
Td: Deceleration check time Td = 2 x Ts + (0 to 10ms)
Ts
Td
G00 Xx1; G00 Xx2;
Ts
Td
G00 Xx1; G00 Xx2;
Td Ts
G00 Xx1; G00 Xx2;
2Ts
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
187 IB-1501277-P
[Exact stop check result]
Program example
N001 G09 G01 X100.000 F150 ; The commands in the following block are started once the deceleration check time or in-position state has been checked after the machine has decelerated and stopped.
N002 Y100.000 ;
f: Commanded speed Tool
t: Time
Solid line indicates speed pattern with G09 command Broken line indicates speed pattern without G09 command
N001X
Y
N001
N002
N002
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
188IB-1501277-P
7.12 Exact Stop Check Mode; G61
Whereas the G09 exact stop check command checks the in-position status only for the block in which the command has been assigned, the G61 command functions as a modal. This means that deceleration will apply at the end points of each block to all the cutting commands (G01 to G03) subsequent to G61 and that the in-position status will be checked. The modal command is released by the following commands.
G61.1........ High-accuracy control mode
G62 .......... Automatic corner override
G63 .......... Tapping mode
G64 .......... Cutting mode
In-position check is executed when the G61 command has been selected, and thereafter, the in-position check is executed at the end of the cutting command block until the check mode is canceled.
Function and purpose
Command format
G61 ; ... Exact stop check mode
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
189 IB-1501277-P
7.13 Deceleration Check 7.13.1 Deceleration Check
The deceleration check reduces the machine shock that occurs when the control axis feedrate is suddenly changed and prevents corners from becoming rounded. This is accomplished by decelerating the motor to a stop at axis movement block joints before the next block is executed.
The conditions for executing a deceleration check are described below.
(1) Deceleration check in the rapid traverse mode In the rapid traverse mode, the deceleration check is always performed when block movement is completed be- fore executing the next block.
(2) Deceleration check in the cutting feed mode In the cutting feed mode, the deceleration check is performed and the program starts moving the next block when one of the following conditions is satisfied. (a) When G61 (Exact stop check mode) is selected (b) When the G09 (Exact stop check) command has been designated in the same block (c) When the error detect switch (PLC signal) is ON
There are three methods for deceleration check: command deceleration check method, smoothing check method, and in-position check method. The method that is selected for rapid traverse or cutting feed depends on the MTB specifications (combination of parameters "#1306 InpsTyp", "#1389 G1SmthChk", "#1223 aux07/bit1", and "#1193 inpos"). Depending on the MTB specifications, different deceleration check methods may be used for each feed command during rapid traverse command and cutting feed command (parameter "#1306 InpsTyp").
Function and purpose
Without deceleration check With deceleration check
N010 G01 X100 ; N011 G01 Y-50 ;
Corner rounding occurs because the N011 block is started before the N010 command is completely finished.
N010 G09 G01 X100 ; N011 G01 Y-50 ;
A sharp edge is formed because the N011 block is started after the N010 command is decelerated and stopped.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
190IB-1501277-P
(*1) Deceleration check time is automatically calculated from the acceleration/deceleration mode and time constant.
Detailed description
Behavior for each combination of movement commands
Next block Current block
G00 G01 G00/G01 without move- ment
G00 () (1)(2) G01 () (1)(3) Others () (1)
Deceleration check is performed () (1) A deceleration check is performed when the error detection signal is ON or when G09 or G61 is en-
abled. (2) A command deceleration check is performed when G01 => G00 block is specified, "#1502 G0Ipfg"
is ON, or the movement reverses to the opposite direction. (3) A command deceleration check is performed when G01 => G01 block is specified, "#1503 G1Ipfg"
is ON, or the movement reverses to the opposite direction. For the deceleration check when movement in the opposite direction is reversed, refer to "7.13.2 Decel- eration Check When Movement in the Opposite Direction Is Reversed". A deceleration check is not performed if the above conditions are not satisfied.
Deceleration check is not performed.
Types of deceleration check
(1) Command deceleration check method Deceleration is completed after the deceleration check time (*1) has passed after the interpola- tion.
(2) Smoothing check method Deceleration is completed after the deceleration check time (*1) has passed after the interpola- tion and all axis smoothing has become zero.
(3) In-position check method The deceleration is completed after the deceleration check time (*1) had passed after the interpolation, all axis smoothing has become zero, and all axes have become in-position.
NC command speed Deceleration check time
Block is completedInterpolation is completed
Speed
Block is completed
NC command speed Deceleration check time
Interpolation is completed
Speed
NC command speed
Actual motor rotation speed
Deceleration check time
Interpolation is completed
Speed
Block is completed
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
191 IB-1501277-P
(1) When a rapid traverse command (G00/G53) block is to be executed
(2) When a cutting command (G01/G02/G03) block is to be executed When parameter "#1306 InpsTyp" is "0", the following occurs (MTB specifications).
When parameter "#1306 InpsTyp" is "1", the same method as for rapid traverse in (1) is used regardless of the value of parameter "#1389 G1SmthChk".
Selecting deceleration checks (MTB specifications)
Parameters Deceleration check method Conditions of deceleration check
#1193 inpos
0 Command deceleration check meth- od
Deceleration check time has elapsed.
1 In-position check method Deceleration check time has elapsed, all axis smoothing has become zero, and all axes have become in-position.
2 Smoothing check method Deceleration check time has elapsed, and smoothing zero for all axes.
Parameters Deceleration check method Conditions of deceleration check
#1389 G1SmthChk
#1223 aux07/bit1
0 0 Command deceleration check meth- od
Deceleration check time has elapsed.
1 In-position check method Deceleration check time has elapsed, all axis smoothing has become zero, and all axes have become in-position.
1 - Smoothing check method Deceleration check time has elapsed, and smoothing zero for all axes.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
192IB-1501277-P
Execution of the next block starts after confirming that the deceleration of the command system is completed upon completion of interpolation for one block. The following explains an example of transition from the current block (rapid traverse) to the next block. The time required for the deceleration check is the longest among the deceleration check times of each axis deter- mined by the acceleration/deceleration mode and time constants of the axes commanded simultaneously.
(a) For linear acceleration/deceleration
(b) For exponential acceleration/deceleration
(c) For soft acceleration/deceleration
Command deceleration check method
(Ts) Linear acceleration/deceleration time constant (Td) Deceleration check time: Td = Ts + (0 to 10 ms)
(Ts) Exponential acceleration/deceleration time constant (Td) Deceleration check time: Td = 2 x Ts + (0 to 10 ms)
(Ts) Soft acceleration/deceleration time constant (Td) Deceleration check time: Td = 2 x Ts + (0 to 10 ms)
Td
Ts
Execution block Next block
Td
Ts
Execution block Next block
command
Td
Ts
Execution block Next block
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
193 IB-1501277-P
Execution of the next block starts after the command deceleration check is performed and after confirming that the smoothing for all axes in the part system has reached zero.
For exponential acceleration/deceleration
Execution of the next block starts after the command deceleration check is performed and after confirming that the remaining distances for all axes in the part system are below certain values. The confirmation of the remaining distance should be done with the imposition width. The bigger one of the servo parameter "#2224 SV024" or G0 in-position width "#2077 G0inps" (For G01, in-position width "#2078 G1inps"), will be adapted as the in-position width. (For a rotary axis, the setting value of spindle parameter "#13024 SP024" is assumed to be the in-position width.)
With linear acceleration/deceleration
As shown in the figure above, the in-position width is the remaining distance from the previous block at the start of the next block. (Shaded area of the figure above).
Smoothing check method
(Ts) Exponential acceleration/deceleration time constant (Td) Deceleration check time (Tp) Waiting time for a block to complete
In-position check method
(Ts) Linear acceleration/deceleration time constant (Td) Deceleration check time (Tp) Waiting time for a block to complete
Td
Tp
Ts Smoothing zero for all axes
Execution block Next block
Command
Td
Tp
Ts
Execution block Next block
In-position width
Servo
Command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
194IB-1501277-P
The purpose of the deceleration check is to minimize the positioning time. The bigger the setting value for the in- position width, the shorter the time is, but the remaining distance of the previous block at the start of the next block also becomes larger, and this could become an obstacle in the actual processing work. The check for the remaining distance is done at set intervals. Accordingly, it may not be possible to get the effect of time reduction for positioning as in-position width setting value.
(1) In-position check by the G0inps: When SV024 < G0inps (Stop is judged at A in the figure.)
(2) In-position check by the SV024: When G0inps < SV024 (Stop is judged at A in the figure.)
Command to motor
Outline of motor movement
: G0inps
: SV024
Command to motor
Outline of motor movement
: G0inps
: SV024
G0inps
SV024
A
SV024
G0inps
A
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
195 IB-1501277-P
This command commands the in-position width for the positioning command from the machining program.
Execution of the next block starts after confirming that the position error amount in the block in which the decelera- tion check is to be performed is less than the in-position width. The in-position width specified by parameter (SV024, G0inps (G1inps for G01)) or the one specified in the program, whichever is greater, will be adapted as the in-position width. When there are several movement axes, the system confirms that the position error amount of each movement axis in each part system is less than the in-position width issued in this command before executing the next block. For ",I" command, also refer to "6.1 Positioning (Rapid Traverse); G00".
The differences between the in-position check with parameter and with programmable command are as follows:
(1) In-position check with parameter After completing deceleration of the command system ("A" in the figure), the servo system's position error amount and the parameter setting value (in-position width) are compared.
(2) In-position check with programmable command (",I" address command) After starting deceleration of the command system ("A" in the figure), the position error amount and commanded in-position width are compared.
Programmable in-position width command
G00 X_ Z_(Y_) ,I_ ;
X,Z(,Y_) Positioning coordinate value of each axis ,I In-position width (setting range: 1 to 999999)
The differences of In-position check
(Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = Ts + (0 to 10 ms)
Servo machine position Command In-position width (Servo system position error amount)
(Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = Ts + (0 to 10 ms)
Servo machine position Command In-position width (Servo system position error amount)
G00 Xx1;
Ts
Td
A
G00 Xx1;
Ts
Td
A
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
196IB-1501277-P
The deceleration check acts on the compensated block when tool compensation is performed.
The automatic error detection is disabled in a block in which deceleration check is enabled.
When the axis movement reverses to the opposite direction in a G01 G01 successive block during the high-speed machining mode other than high-speed machining mode I (G05 P1) the commanded deceleration will not take place even if parameter "#1503 G1Ipfg" is set to 1. Note that the G0Ipfg setting will be followed if the axis direction reverses to the opposite direction in a G01 G00 successive block.
A deceleration check is performed even when high-speed simple program check is running. During high-speed sim- ple program checking, the deceleration check time is reduced according to the time reduce coefficient.
(1) When the in-position check is valid, the parameter for the in-position width "#2224 SV024" must be set. (Based on the MTB specifications.)
(2) This function is disabled for an axis to which automatic machine lock is applied. (3) If MSTB is commanded in the block that follows a cutting command, the MSTB code is output before deceleration
is completed in the cutting command. If an MSTB command must be executed after the completion of axis move- ment, check the PLC signals (DEN) before executing it. (The behavior depends on the MTB specifications.)
(4) If there is an axis in control axis synchronization/superimposition in the part system for which the in-position check method is specified, deceleration is considered to be completed when all axis smoothing has become ze- ro. (Equivalent to smoothing check method)
(5) If thread cutting commands are specified in succession, a deceleration check is not carried out at block joints. (6) If the parameter "#1205 G0bdcc" is set to "1", the value set with the parameter "#2224 SV024" (in-position de-
tection width) will be used as the in-position width. The setting of the parameter "#2077 G0inps" (G0 in-position width) and the programmable in-position check with ",I" address are disabled. These parameters depend on the MTB specifications.
Relationship with Other Functions
Tool compensation
Automatic error detection
High-speed machining mode
High-speed simple program check
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
197 IB-1501277-P
7.13.2 Deceleration Check When Movement in the Opposite Direction Is Reversed
A deceleration check cannot be designated for G01 -> G00 or G01 -> G01, but it can be designated in the following manner only when the movement reverses to the opposite direction in successive blocks. A deceleration check can also be executed if even one axis is moving in the opposite direction while several axes are interpolating. For the relation with other functions and precautions, refer to "Deceleration Check".
If the axis movement reverses to the opposite direction in a G01 to G00 successive block, the deceleration check for the movement in the opposite direction can be changed with the MTB specifications (parameter "#1502 G0Ipfg").
Function and purpose
Detailed description
Designating deceleration check for G01 -> G00 opposite direction movement reversal
Same direction Opposite direction
#1502 = 0
The acceleration rate is excessive due to the G01 and G00 composite speed.
Enlarged figure
(a) Commanded speed (b) Resultant speed
G01 G00
G01 G00
G01
G00
(a) (b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
198IB-1501277-P
Example of program: When there is a deceleration check in the movement of several axes
(1)
(2)
(3)
(4)
(5)
#1502 = 1
Command deceleration Enlarged figure
(a) Commanded speed (b) Resultant speed (c) Command deceleration is completed.
G91 G01 X100. Y100. F4000 ; G00 X-100. Y120. ;
A deceleration check is carried out, because the X axis moves in the reverse direction in the program.
G91 G01 X100. Y-100. F4000 ; G00 X80. Y100. ;
A deceleration check is carried out, because the Y axis moves in the reverse direction in the program.
G90 G01 X100. Y100. F4000 ; G00 X80. Y120. ;
A deceleration check is carried out, because the X axis moves in the reverse direction in the program. (When the program start position is X0 Y0)
G91 G01 X100. Y100. F4000 ; G00 X100. Y100. ;
A deceleration check is not carried out, because both the X axis and the Y axis move in the same direction in the program.
G91 G01 X100. Y80. F4000 ; G00 X80. ;
A deceleration check is not carried out, because the X axis moves in the same direction, and there is no Y axis movement command in the program.
Same direction Opposite direction
G01 G00
G01 G00
G01
G00
(c)
(a) (b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
199 IB-1501277-P
If the axis movement reverses to the opposite direction in a G01 to G01 successive block, the deceleration check for the movement in the opposite direction can be changed with the MTB specifications (parameter "#1503 G1Ipfg").
Example of program: When there is a deceleration check in the movement of several axes
(1)
(2)
(3)
(4)
(5)
Designating deceleration check for G01 -> G01 opposite direction movement reversal
Same direction Opposite direction
#1503 = 0
The acceleration rate is excessive due to the G01 and G01 composite speed.
#1503 = 1
Command deceleration
G91 G01 X100. Y100. F4000 ; G01 X-100. Y120. ;
A deceleration check is carried out, because the X axis moves in the reverse direction in the program.
G91 G01 X100. Y-100. F4000 ; G01 X80. Y100. ;
A deceleration check is carried out, because the Y axis moves in the reverse direction in the program.
G90 G01 X100. Y100. F4000 ; G01 X80. Y120. ;
A deceleration check is carried out, because the X axis moves in the reverse direction in the program. (When the program start position is X0 Y0)
G91 G01 X100. Y100. F4000 ; G01 X100. Y100. ;
A deceleration check is not carried out, because both the X axis and the Y axis move in the same direction in the program.
G91 G01 X100. Y80. F4000 ; G01 X80. ;
A deceleration check is not carried out, because the X axis moves in the same direction, and there is no Y axis movement command in the program.
G01 G01
G01 G01
G01 G01
G01 G01
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
200IB-1501277-P
7.14 Rapid Traverse Block Overlap; G0.5 P1
This function enables the next block to start (overlap) without waiting for positioning (G00) or reference position re- turn (G28/G30). Consequently, cycle time of machining including operation of positioning (G00) or reference position return (G28/ G30) can be reduced. Adjust the overlap amount according to the command issued by the machining program or with the parameter, and specify it as in-position width for rapid traverse block overlap. Also, the operation does not decelerate between blocks if the movement command continues in same direction. The overlap is also valid when G00 is followed by a G01 block, rather than G00 or G28/G30. It is not invalid when G28 is followed by G00 or G28/G30. The validity of this function depends on the MTB specifications.
Example of behavior and velocity waveform 1 (example of application of rapid traverse block overlap in tool
change motion)
Example of behavior and velocity waveform 2 (example of application of rapid traverse block overlap in con-
tinuous drilling motion)
Function and purpose
Intermediate point
Speed
In-position width
Time
Speed Cycle time is reduced.
Time Program path Command path from NC
In-position width Speed
Time Speed Cycle time is reduced.
Time
Program path Command path from NC
N2(G28)
N2(G28)
N1(G00)
N1
N1 N2 N3
N2
N3(G00) N4(G00)
N5(G01)
N2(G00)
N1(G01)
N1
N1 N2 N3 N4 N5
N2 N3 N4 N5
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
201 IB-1501277-P
For a deceleration check method that uses the in-position width for rapid traverse (G00) or reference position return (G28/G30), a function with a higher priority that is enabled will be applied. If none of the functions is enabled, the command deceleration is carried out.
For G00 overlap, refer to "7.14.1 Rapid Traverse Block Overlap for G00; G0.5". For G28/G30 overlap, refer to "7.14.2 Rapid Traverse Block Overlap for G28".
Deceleration check method using in-position width
Function
Enabling conditions
Deceleration Check
Priority (Deceleration check
method) Enabled behav-
ior
Programmable in-posi- tion
Valid when the in-position width is designated with address ",I" in the same block as G00. (It is valid only for a block in which address ",I" is specified.) (For details, refer to "6.1 Positioning (Rapid Tra- verse); G00" and "7.13 Deceleration Check".)
G00 1
Rapid traverse block overlap (this function)
(1) For G00 Parameter "#1442 G0ol" must be "1" and G00 rapid traverse block overlap must be valid modal code (G0.5P1).
G00/G28/G30 2
(2) For G28/G30 Parameter "#1443 G28ol" must be "1".
In-position check by pa- rameter settings
Parameter "#1193 inpos" must be "1". (For details, refer to "7.13 Deceleration Check".)
G00 3
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
202IB-1501277-P
7.14.1 Rapid Traverse Block Overlap for G00; G0.5
This function enables the next block to start (overlap) without waiting for positioning (G00) or reference position re- turn (G28/G30). For the rapid traverse block overlap function, also refer to "7.14 Rapid Traverse Block Overlap; G0.5 P1". G28/G30 can be overlapped when the rapid traverse block overlap for G28 is enabled. For details, refer to "7.14.2 Rapid Traverse Block Overlap for G28".
(1) A program error (P35) will occur when this command is not issued alone in a block. (2) This block can be specified simultaneously with an N code (sequence number). (3) The in-position width at joints between two blocks containing G28/G30 cannot be changed with G0.5P1 com-
mand. (4) G0.5P1 and G0.5P0 are modal. (5) Address J in G20 must be programmed in inches. (6) If an address is omitted, the width determined by the MTB specifications becomes valid. (Parameters "#2224
SV024" and "#13024 SP024") If a value less than the width determined by the MTB is specified, that width becomes valid.
(7) If address J or K is set to "0", the conventional deceleration check is performed.
Function and purpose
Command format
Starting rapid traverse block overlap for G00
G0.5 P1 J_ K_;
P Starting or canceling the rapid traverse block overlap function (0: Cancel, 1: Start) J Liner axis in-position width (0.000 to 1000.000 (mm)) K Rotary axis in-position width (0.000 to 1000.000 ())
Canceling rapid traverse block overlap for G00
G0.5 P0;
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
203 IB-1501277-P
The rapid traverse block overlap function for G00 becomes effective when all of the following conditions are satisfied.
(1) The rapid traverse block overlap for G00 must be enabled. Refer to the MTB specifications (parameter "#1442 G0ol").
(2) G0.5P1 modal must be active. To make G0.5P1 modal active: Specify a G code (G0.5P1) in which rapid traverse block overlap is enabled in the machining program. Set parameter "#12056 I_G0oL G00" to "1" (valid).
(1) When the rapid traverse block overlap for G00 is enabled, a G code (positioning (G00) or linear interpolation (G01)) following positioning (G00) may not be subject to rapid traverse block overlap depending on the current control mode or parameter settings that are specified by the MTB. (Parameters "#1086 G0intp" and "#1205 G0bdcc") For details, refer to the table below.
: Motion subject to rapid traverse block overlap for G00
: Motion not subject to rapid traverse block overlap for G00
Detailed description
Enabling conditions
N1 G0.5 P1; Rapid traverse block overlap function: Enabled N2 G91 G00 X10.; N3 G00 X20.; N4 G0.5 P0; Rapid traverse block overlap function: Disabled :
Motion subject to rapid traverse block overlap
Control mode Parameters G code following positioning (G00)
High-accuracy mode
#1086 #1205 G00 G01
OFF 0 0 1 2
1 0/1/2 ON 0 0
1 2
1 0/1/2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
204IB-1501277-P
(2) When executing a rapid traverse block overlap in G00 multi-step acceleration/deceleration, the next block (N2 in the following program) will be started after the deceleration at the last step in the execution bock (N1) has started. The hatched area in the figure below is an area in which the in-position width can be specified.
(3) When the rapid traverse block overlap for G00 is enabled, this function is valid if positioning (G00) is followed by a fixed cycle, subprogram or macro call command block. In addition, this function is valid if a fixed cycle, subprogram or macro program contains consecutive move com- mands to which this function is applied. (If the in-position width is specified in a fixed cycle command, that value is given priority.)
The start position of overlap when a rapid traverse block overlap for G00 is executed can be adjusted with the in- position width. The next block is started when the remaining distances of all movement axes in the current move- ment block are smaller than the in-position width. (Refer to following figure.) When setting the in-position width with J and K commands, set a value for each linear and rotary axis. Setting the in-position width for axes with parameter settings depend on the MTB specifications (parameter "#2631 G0olinps").
The start position of the next block based on the remaining distance and in-position width for each movement axis is shown below. This shows an example of when the X axis in-position width is set to 0.5 mm and the Y axis in-position width to 1 mm.
N1 G91 G00 X10.; N2 X10.;
Speed Command to motor Start of deceleration at the last step
Time
Motor movement Deceleration stop
Adjustment of start position of overlap
(a) For X axis (b) For Y axis
Program example Program example
N1 G91 G00 X50.; N2 Y50.;
N1 G91 G00 Y50.; N2 X-50.;
Operation Operation
Start position of N2 block Y axis in-position width = 1mm
X axis in-position width = 0.5mm Start position of N2 block
N1 N2
N1
N2
N1
N2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
205 IB-1501277-P
The in-position width is determined by the G code address or parameter value.
(1) When specifying the in-position width with a G code, the one specified with address J/K becomes effective. Note that if address J or K is set to "0", the rapid traverse block overlap is disabled.
(2) If a command with address J/K is omitted, the in-position width determined for each of positioning and cutting feed by the MTB specifications becomes effective. (Parameters "#2631 G0olinps" and "#2632 G1olinps") (a) Positioning (G00) - Positioning (G00): Parameter "#2631 G0olinps" (b) Positioning (G00) - Cutting feed (G01)(high-accuracy mode is OFF): Parameter "#2632 G1olinps"
(1) Upper limit for in-position width When rapid traverse block overlap is enabled, the in-position check is performed after starting deceleration spec- ified in the speed command ("A" in the figure). Thus, the distance from the servo machine position after starting the command deceleration to the commanded position (hatched area in the figure below) is the upper limit for the actual in-position width.
(2) Lower limit for in-position width The lower limit for the in-position width depends on the MTB specifications (parameters "#2224 SV024" or "#13024 SP024"). The value of this parameter is applied even if a value less than or equal to this parameter is specified as an in- position width.
(c) For X and Y axes
Program example
N1 G91 G00 X50. Y50.; N2 X-50. Y50.;
Operation
If the position error amount is smaller than the in-position width for both of the X and Y axes, the next block is started.
Y axis in-position width = 1mm
If the Y axis position error amount is smaller than the in-position width, but the X axis position error amount is larg- er than that width, the next block is not started.
Start position of N2 block
X axis in-position width = 0.5mm
Upper and lower limits for in-position width
Speed
Time
Motor movement Command to motor Upper limit for in-position width
N1
N2
A
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
206IB-1501277-P
The conventional deceleration check (in-position check method) applies the same in-position width regardless of the path (corner angle). Therefore, an extra speed change occurs and cycle time is increased even though path direction stays almost the same. The rapid traverse block overlap automatically compensates for the in-position width based on the path (corner angle). However, the in-position width is not compensated for based on the path if a block without a movement command is inserted between the movement commands to be overlapped. (1) If the angle is greater than 90, the rapid traverse block overlap function is temporarily canceled. (2) If the angle is less than 90, the in-position width is compensated for so that it matches the amount of droop at
a corner when the corner angle is 90.
The following are examples of using G00 rapid traverse block overlap in combination with G00 (rapid traverse) and G01 (cutting feed). (When the high-accuracy control mode is OFF)
Compensation for in-position width based on the path
Program example
When the in-position width is specified with address J (G0.5P1 J_)
Parameter setting X axis Z axis
#2631(G0olinps) 2mm 1.5mm #2632(G1olinps) 1 mm 0.5 mm
N1 G0.5P1 J1.0; N2 G91 G01 Z25.; N3 G00 Z25.; N4 G00 Z50.; N5 G00 X125.; N6 G00 Z-75.; N7 G01 Z-25. F1000.;
Z axis in-position width is set to 1 mm with the J address command.
X axis in-position width is set to 1 mm with the J address command.
Program path Command path from NC
Speed
Time Speed
Time
Cycle time is re- duced.
N5 N6
N7 N2
N4
Z
X
N3
N2 N3 N4 N5 N6 N7
N3 N4 N5 N6 N7N2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
207 IB-1501277-P
When specifying G00 (positioning) -> G81 (drilling)
Example behavior in fixed cycle
(Main program) (G81 program)
N10 G0.5 P1 J0.5; N31 G00 X50. Y0.; N20 G91 G98 G64 G00 X50.; N32 G00 Z-25.; N30 G81 X50. Y0. Z-25. R-25. F1000. L1. ,I2.0 ,J1.0; N33 G01 Z-25. F1000.; N40 G00 X50. ; N34 G00 Z50.;
Rapid traverse block overlap function: Enabled (Start G81 command before positioning is com- pleted.) Rapid traverse block overlap function: Invalid (Valid when address ",I" is omitted)
Rapid traverse block overlap function: Invalid (Valid when address ",J" is omitted)
R point position Rapid traverse block overlap function: Enabled
Hole bottom position Rapid traverse block overlap function: Enabled
Program path Command path from NC
N33
N32
N31
N40
N20
N34
(R)
Z
X
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
208IB-1501277-P
If an ",I" address command is used to specify the in-position width from the program when the rapid traverse block overlap is enabled, the in-position width of programmable in-position is given priority. Because the programmable in-position is an unmodal command, the in-position width specified with the rapid tra- verse block overlap enabled is assumed for commands following ",I" address. This shows an example of when the X and Y axis in-position widths for G00 are set to 1 mm by parameters.
(*1) The in-position width is the parameter setting value because the programmable in-position is an unmodal com- mand.
(1) The programmable in-position (",I" command) for G00 pre-interpolation acceleration/deceleration can only be used when the rapid traverse block overlap is enabled.
(2) When G00 is followed by a block without a movement command, a command of address ",I", if specified for G00, is handled as a command specifying a rapid traverse block overlap. Therefore, the overlap takes place only when overlapped movements are executed.
Relationship with Other Functions
Programmable in-position
N1 G0.5 P1; G0.5 command (for G00) N2 G91 G00 X50.; Rapid traverse block overlap for G00: Valid N3 Y50. ,I1.5; ",I" address command is valid N4 X50.; Rapid traverse block overlap for G00: Valid N5 Y50.; :
In-position width: 1.5 mm (",I" address command is given priority.)
In-position width: 1 mm (Parameter setting value) (*1)
Program path
Command path from NC
In-position width: 1 mm (Parameter setting value) (*1)
N2
Y
X
N3
N4
N5
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
209 IB-1501277-P
When the rapid traverse block overlap is enabled, the conventional deceleration check is disabled for the behavior subject to this function. When the rapid traverse block overlap is disabled, the conventional deceleration check is enabled. This shows an example of when the X and Y axis in-position widths for G00 are set to 1 mm by parameters.
(1) When a block without a movement command is inserted between blocks that are subject to the rapid traverse block overlap, blocks are overlapped if the high-accuracy mode is OFF (they are not overlapped if the mode is ON). If the high-accuracy mode is OFF, a block without movement that is inserted between a G00 command and G28/ 30 block is not overlapped when the rapid traverse block overlap for G00 is disabled ("#1442 G0ol" is "0") and rapid traverse block overlap for G28 is enabled ("#1443 G28ol" is "1").
(2) When a block without a movement command is inserted between blocks that are subject to the rapid traverse block overlap, the in-position width is not compensated for based on the path.
(3) When the high-accuracy control mode is selected or the parameter #1205 is set to "1" or "2", the next block will not be performed until the speed is reduced below the rapid speed (#2001) if the speed at the completion of in- position check is higher than the rapid speed (parameter #2001) of the next block.
(4) Even when the overlap process blocks continue, if one or more axes are moved in reversed direction, the overlap function is temporarily canceled.
(5) (Only for C80 series) The rapid traverse block overlap function is temporarily canceled in the following cases: when the high-accuracy control mode is selected; when the parameter #1205 is set to "1" or "2" and the param- eters #1569 and #1570 are set to "0".
Deceleration Check
N1 G0.5 P1; G0.5 command (for G00) N2 G91 G00 X50.; Rapid traverse block overlap for G00 is valid N3 Y50.; Deceleration check is valid. N4 G0.5 P0; N5 X50.; Deceleration check is valid. N6 Y50.; Deceleration check is valid. :
Deceleration check is valid. (Command deceleration method/in-position check method)
Program path
Command path from NC
In-position width: 1 mm (Parameter setting value)
Precautions
N2
Y
X
N3
N6 N5
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
210IB-1501277-P
7.14.2 Rapid Traverse Block Overlap for G28
This function enables the next block to start (overlap) without waiting for positioning (G00) or reference position re- turn (G28/G30). For the rapid traverse block overlap function, also refer to "7.14 Rapid Traverse Block Overlap; G0.5 P1". G00 can be overlapped when the rapid traverse block overlap for G00 is enabled. For details, refer to "7.14.1 Rapid Traverse Block Overlap for G00; G0.5".
The rapid traverse block overlap function for G28 becomes effective when all of the following conditions are satisfied.
(1) The rapid traverse block overlap for G28 is enabled. (Refer to the MTB specifications. "#1443 G28ol")
(2) High-speed reference position return is active. (Dog-type is not subject to this.) (3) When the rapid traverse block overlap for G00 is enabled, a G00 command is followed by G28 or G30 positioning
command.
For G28/G30, whether or not the appropriate block, if its movement is made via an intermediate point, is over- lapped depends on the MTB specifications (parameters "#1205 G0bdcc" and "#1086 G0intp").
If G28/G30 command is followed by another G28/G30, blocks are not overlapped in rapid traverse. (Blocks are not overlapped.
The start position of overlap when a rapid traverse block overlap for G28 is executed can be adjusted with the in- position width. The next block is started when the remaining distances of all movement axes in the current move- ment block are smaller than the in-position width. The in-position width depends on the MTB specifications (parameter "#2633 G28olinps").
Function and purpose
Detailed description
Enabling conditions
Intermediate point
Rapid traverse block overlap
Adjustment of start position of overlap
Note
N1:G00
N2:G02
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
211 IB-1501277-P
The following are examples of using rapid traverse block overlap for G28 in combination with G28/G30 (reference position return) and G00 (rapid traverse).
Initial position of axes: X axis = -50 mm; Z axis = -100 mm
Refer to "7.14 Rapid Traverse Block Overlap; G0.5 P1".
Refer to "7.14 Rapid Traverse Block Overlap; G0.5 P1".
Program example
Parameter setting X axis Z axis
#2633 G28olinps 0.5 mm 1 mm
Intermediate point
In-position width: 1 mm
N1 G91 G00 Z50.; N2 G91 G28 X0.Z50.;
Program path Command path from NC
Relationship with Other Functions
Precautions
N2(G28)
N2(G28)
N1(G00)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
212IB-1501277-P
7.15 Automatic Corner Override
With tool radius compensation, this function reduces the load during inside cutting of automatic corner R, or during inside corner cutting, by automatically applying override to the feedrate. There are two types of automatic corner override: Automatic corner override (G62) and inner arc override. Automatic corner override (G62) is valid until the tool radius compensation cancel (G40), exact stop check mode (G61), high-accuracy control mode (G61.1), tapping mode (G63), or cutting mode (G64) command is issued. The inner arc override is valid whenever the machine is in the tool radius compensation mode (G41/G42), regardless of the automatic corner override (G62) mode.
When cutting an inside corner, as shown in the figure below, the machining allowance amount increases and a greater load is applied to the tool. To remedy this, override is applied automatically within the corner set range, the feedrate is reduced, the increase in the load is reduced and cutting is performed effectively. However, this function is valid only when finished shapes are programmed.
[Operation]
(1) If there is no G62 command: When the tool moves in the order of P1 -> P2 -> P3 in the above figure, the machining allowance at P3 increase by an amount equivalent to the area of shaded section S compared to P2 and so that tool load increases.
(2) If there is G62 command: When the inside corner angle in the above figure is less than the angle set in the parameter, the override set into the parameter is automatically applied in the deceleration range Ci.
Function and purpose
Detailed description
Machining inside corners
Workpiece
Program path (Finished shape) Machining allowance
Workpiece surface shape
Tool center path
Deceleration range Ci (IN)
Tool
: Max. angle at inside corner
Ci
P1
P3 P2
S
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
213 IB-1501277-P
[Parameter setting]
The following parameters are set into the machining parameters. Refer to the Instruction Manual for details on the setting method.
(1) The override set in the parameter is automatically applied at the deceleration range Ci and corner R section for inside offset with automatic corner R. (There is no angle check.)
# Parameters Setting range
#8007 Override 0 to 100 (%) #8008 MAX ANGLE 0 to 180 [] #8009 DSC.ZONE 0 to 99999.999 [mm] or
0 to 3937.000 [inches]
Automatic corner R
Program path Tool center path
Corner R center Corner R section
Deceleration range (Ci)
Workpiece surface shape
Machining allowance
Workpiece
Ci
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
214IB-1501277-P
The lines in the figure denote:
(1) Linear - linear corner
The override set in the parameter (#8007) is applied in the deceleration range Ci.
(2) Linear - arc (outside offset) corner
The override set in the parameter (#8007) is applied in the deceleration range Ci.
(3) Arc (outside offset) - linear corner
(4) Linear - arc (inside offset) corner
During cutting of arc (inside offset), an inner arc override is applied.
Application example
Programmed path Tool center Arc (inside offset)
(a) If there is a G62 command: (b) If there is no G62 command:
For straight lines, the override set in the parameter (#8007) is applied in the deceleration range Ci.
Ci
Ci
Ci
Ci
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
215 IB-1501277-P
(5) Arc (inside offset) - linear corner
(*1) The deceleration range Ci where the override is applied is the length of the arc with an arc command. During cutting of arc (inside offset), an inner arc override is applied. Automatic corner override will not be applied to straight lines.
(6) Arc (inside offset) - arc (outside offset) corner
(*1) The deceleration range Ci where the override is applied is the length of the arc with an arc command. During cutting of arc (inside offset), an inner arc override is applied. Automatic corner override will not be applied to straight lines.
(a) If there is a G62 command: (b) If there is no G62 command:
In addition to the inner arc override, the override set in the parameter (#8007) is applied in the deceleration range Ci. (*1) F (speed command value) x (inner arc override) x (set- ting for #8007)
(a) If there is a G62 command: (b) If there is no G62 command:
In addition to the inner arc override, the override set in the parameter (#8007) is applied in the deceleration range Ci. (*1) F (speed command value) x (inner arc override) x (set- ting for #8007)
Ci
Ci
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
216IB-1501277-P
Relationship with other functions
Function Operation of automatic corner over- ride (G62)
Operation of inner arc override
F1-digit Feed Automatic corner override is applied to the F1-digit speed.
Inner arc override is applied to the F1- digit speed.
Cutting feed override Cutting feed override is applied to auto- matic corner override.
Cutting feed override is applied to the feedrate to which inner arc override has been applied.
Override cancel Automatic corner override will not be can- celed by override cancel.
Inner arc override is not canceled by override cancel.
External deceleration External deceleration speed will be ap- plied after automatic corner override is applied to the cutting feedrate.
External deceleration is applied to the feedrate to which the inner arc override has been applied.
Speed clamp Clamp speed will be applied after auto- matic corner override is applied to the cutting feedrate.
Clamp speed is applied to the feedrate to which the inner arc override has been ap- plied.
Dry run Automatic corner override will not be ap- plied.
Inner arc override is not applied.
Synchronous feed Automatic corner override is applied to the synchronous feedrate.
Inner arc override is applied to the syn- chronous feedrate.
Thread cutting Automatic corner override will not be ap- plied.
Inner arc override is not applied.
G31 Skip Program error occurs with G31 command during tool radius compensation.
Same as on the left.
Machine lock Automatic corner override is applied even in the machine lock state.
Inner arc override is applied even in the machine lock state.
Positioning (G00)
Automatic corner override is not applied to the positioning command.
Inner arc override is not applied to the po- sitioning command.
Linear interpolation (G01)
Automatic corner override is applied to linear interpolation.
Inner arc override is not applied to linear interpolation.
Circular Interpolation (G02, G03)
Automatic corner override is applied to circular interpolation.
Inner arc override is applied to circular in- terpolation.
Spiral/conical interpolation (G02.1,G03.1)
Automatic corner override is applied to spiral/conical interpolation.
Inner arc override is applied to spiral/con- ical interpolation.
Involute Interpolation (G02.2, G03.2)
Automatic corner override is applied to in- volute interpolation.
Inner arc override is not applied to invo- lute interpolation (*1).
Tool radius compensation cancel (G40)
Automatic corner override will not be ap- plied while the tool radius compensation is being canceled.
Inner arc override is not applied while the tool radius compensation is canceled.
3-dimensional tool radius compensation (Compensation vector des- ignation type) (G41, G42)
Automatic corner override is not applied during 3-dimensional tool radius com- pensation (compensation vector desig- nation type).
Inner arc override is applied during 3-di- mensional tool radius compensation (compensation vector designation type).
3-dimensional tool radius compensation (Tool's vertical-direction compensation type) (G41.2, G42.2)
If G62 is commanded during 3-dimen- sional tool radius compensation (tool's vertical-direction compensation type), a program error will occur.
The 3-dimensional tool radius compen- sation (tool's vertical-direction compen- sation type) cannot be combined with circular interpolation or circular cutting; therefore, a program error will occur.
Nose radius compensation (G41, G42, G46)
Automatic corner override is applied during the nose radius compensation.
Inner arc override is not applied during the nose radius compensation.
Circular cut (G12, G13)
Automatic corner override will not be ap- plied during circular cutting.
The operation is switched by the param- eter "#19421 Arc inside min ovr type". For details, refer to "7.15.2 Inner Arc Over- ride".
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
217 IB-1501277-P
(* 1) Involute interpolation provides involute interpolation override (equivalent to inner arc override) to adjust the speed so that the tool center speed does not exceed the lower limit (#1558 IvOMin) of override when tool radius compensation inside is set. To designate the minimum override value for inner arc cutting in involute interpolation, set the parameter above. (This parameter setting depends on the MTB specifications.)
Circular cutting cycle (G75)
Automatic corner override will not be ap- plied during the circular cutting cycle.
Inner arc override is not applied during the circular cutting cycle.
High-speed machining mode I/II (G05P1, G05P2)
Automatic corner override is applied during high-speed machining mode.
Inner arc override is applied during high- speed machining mode.
High-speed high-accuracy control I, II (G05.1Q1, G05P10000)
Automatic corner override is applied during high-speed high-accuracy control I/II.
Inner arc override is applied during high- speed high-accuracy control I or II.
High-accuracy control (G08P1)
A program error will occur if the G62 com- mand is issued during high-accuracy control (G08P1).
Inner arc override is not applied during high-accuracy control mode (G08P1).
High-accuracy control (G61.1)
Both high-accuracy control (G61.1) and automatic corner override are functions of G code group 13; therefore, they can- not be combined.
Inner arc override is applied during high- accuracy control mode (G61.1).
High-accuracy spline inter- polation 1,2 (G61.2, G61.3)
Both high-accuracy spline interpolation 1/ 2 and automatic corner override are func- tions of G code group 13; therefore, they cannot be combined.
High-accuracy spline interpolation 1/2 is enabled when G code group 01 is set to linear interpolation (G01); therefore, it cannot be combined with inner arc over- ride.
SSS Control Automatic corner override is applied to SSS control.
Inner arc override is applied to SSS con- trol.
Corner rounding Automatic corner override is applied to corner rounding.
Inner arc override is not applied to the corner R.
Feedrate override OFF (#3004 bit1 = ON)
Automatic corner override will not be ap- plied while the feedrate override is inval- id.
Inner arc override is applied while the feedrate override is invalid.
Function Operation of automatic corner over- ride (G62)
Operation of inner arc override
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
218IB-1501277-P
(1) Automatic corner override (G62) is valid only in the G01, G02, and G03 modes; it is not effective in the G00 mode. When switching from the G00 mode to the G01 (or G02 or G03) mode at a corner (or vice versa), automatic corner override will not be applied at that corner in the G00 block.
(2) Even if the automatic corner override mode is entered, the automatic corner override will not be applied until the tool radius compensation mode is entered.
(3) Automatic corner override will not be applied on a corner where the tool radius compensation is started or can- celed.
(4) Automatic corner override will not be applied on a corner where the tool radius compensation I, K vector com- mand is issued.
(5) Automatic corner override will not be applied when intersection calculation cannot be executed. Intersection calculation cannot be executed in the following case. When the movement command block does not continue for four or more times.
(6) The deceleration range with an arc command is the length of the arc. (7) The inside corner angle, as set by parameter, is the angle on the programmed path. (8) When the parameters are set as shown below, the automatic corner override (G62) or inner arc override is dis-
abled. (a) Conditions that disable the automatic corner override (G62) #8007 (override) is set to 0 or 100 #8008 (max. angle) is set to 0 or 180 #8009 (DSC.ZONE) is set to 0
(b) Condition that disables the inner arc override #19418 (minimum OVR for inner arc) is set to 0 or 100
(9) The inclined surface machining command is not available during automatic corner override modal. To perform inclined surface machining, command G64 (cutting mode) in advance, then cancel the modal mode.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
219 IB-1501277-P
7.15.1 Automatic Corner Override ; G62
Automatic corner override (G62) is valid until the nose R compensation cancel (G40), exact stop check mode (G61), high-accuracy control mode (G61.1), tapping mode (G63), or cutting mode (G64) command is issued. For detailed description, execution example, the relationship with other functions and precautions, refer to "7.15 Au- tomatic Corner Override".
Command format
G62 ; ... Automatic Corner Override
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
220IB-1501277-P
7.15.2 Inner Arc Override
When cutting an arc (inside offset), applying the override given by the following expression to the commanded fee- drate (F) causes that feedrate to become the F value for which the feedrate of the programmed path is commanded.
The inner arc override is valid whenever the machine is in the tool radius compensation mode (G41/G42), regardless of the automatic corner override (G62) mode.
Inner arc override will not be applied when the machine is in automatic corner R. Inner arc override can be enabled by the parameter "#19420 Arc inside ovr ON" while the tool radius compensation mode (G41/G42) and automatic corner override mode (G62) are ON.
(C) Arc center R1: Radius of tool center path R2: Radius of program path
If the radius (R1) of tool center path is very small compared to the radius (R2) of program path, R1/R2 is nearly equal to 0, causing the tool feed to stop.
To prevent the tool feed from being stopped, set the parameter "#19418 Arc inside min ovr". When the value of inner arc override is the same or smaller than the parameter setting (*1), the tool feed speed is as follows:
F x Parameter setting value / 100
(*1) R1/R2 #19418
The operation of inner arc override during the circular cutting (G12/G13) can be switched by the parameter "#19421 Arc inside ovr typ". When #19421 is type 1, the inner arc override during the circular cutting is invalid. When #19421 is type 2, the inner arc override during the circular cutting is valid. Compensation by D address (compensation number) of the circular cutting is not added to the value of inner arc override. The value of inner arc override is calculated using the path after the compensation by D address as the program path and the path with tool radius compensation added to the path as the tool center path.
For detailed description, execution example, the relationship with other functions and precautions, refer to "7.15 Au- tomatic Corner Override".
Detailed description
R1: Radius of tool center path R2: Radius of program path
Programmed path
Tool center path
F R1 R2
R1
R2
(C)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
221 IB-1501277-P
7.16 Tapping Mode; G63
The G63 command allows the control mode best suited for tapping to be entered, as indicated below:
(1) Cutting override is fixed at 100%.
(2) Deceleration commands at joints between blocks are invalid.
(3) Feed hold is invalid.
(4) Single block is invalid.
(5) In-tapping mode signal is output.
G63 is released by the exact stop check mode (G61), high-accuracy control mode (G61.1), automatic corner over- ride (G62), or cutting mode (G64) command.
The machine is in the cutting mode status when its power is turned ON.
Function and purpose
Command format
G63; ... Tapping mode
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
7 Feed Functions
222IB-1501277-P
7.17 Cutting Mode; G64
The G64 command allows the cutting mode in which smooth cutting surfaces are obtained to be established. Unlike the exact stop check mode (G61), the next block is executed continuously with the machine not decelerating and stopping between cutting feed blocks in this mode.
G64 is released by the exact stop check mode (G61), high-accuracy control mode (G61.1), automatic corner over- ride (G62), or tapping mode (G63).
The machine is in the cutting mode status when its power is turned ON.
Function and purpose
Command format
G64; ... Cutting mode
8
223 IB-1501277-P
Dwell
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
8 Dwell
224IB-1501277-P
8Dwell 8.1 Dwell (Time-based Designation); G04
The machine movement is temporarily stopped by the program command to make the waiting time state. Therefore, the start of the next block can be delayed. The waiting time state can be canceled by inputting the skip signal.
When the asynchronous feed mode (G94) is being executed, there is no need to specify G94.
The setting unit of the dwell time depends on the parameter settings. For addresses X and U, the dwell time setting unit is 1 (ms) when the parameter "#1078 Decimal pnt type 2" is set to "0" and 1 (s) when it is set to "1". If the address "P" is designated, the setting unit of the dwell time is determined by the setting value of the parameters "#8112 DEC- IMAL PNT-P" and "#19014 G04 P factor". For details, refer to "Detailed description".
(1) The decimal point command is enabled for the dwell time designation with X. (2) When designating the dwell time with P, the availability of the decimal point command can be selected with the
parameter "#8112 DECIMAL PNT-P". When the decimal point command is set to be invalid, the command value below the decimal point with P is ignored.
(3) When the decimal point command is valid or invalid, the range of dwell time is as follows.
(4) The dwell time setting unit applied when there is no decimal point can be made 1 (s) by setting "1" in the param- eter "#1078 Decimal point type 2". This is effective only for X and P for which the decimal command is valid.
Function and purpose
Command format
Dwell (Time-based designation)
G94 G04 X__ ;
G94 G04 P__;
X/P Dwell time
Detailed description
Command range when the decimal point com- mand is valid
Command range when the decimal point command is invalid
0 to 99999.999 (s) 0 to 99999999 (ms)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
8 Dwell
225 IB-1501277-P
(5) The setting unit of the P command can be changed with the parameter "#19014 G04 P factor" under the following conditions. "#8112 DECIMAL PNT-P" is set to "0". "#8112 DECIMAL PNT-P" is set to "1", "#1078 Decimal pnt type 2" is set to "0" and the value of address "P"
has no decimal point. The actual duration of dwell (time) can be obtained from the following formula.
P10n
P: command value of address "P" n: setting value of #19014 ("-3" to "3")
(6) When a cutting command is in the previous block, the dwell command starts calculating the dwell time after the machine has decelerated and stopped. When it is commanded in the same block as an M, S, T or B command, the calculation starts simultaneously.
(7) If a feed hold signal is input during dwelling, dwelling is interrupted, and after the machine has been restarted, dwelling is performed using the remaining wait time required to execute the next block.
(8) The dwell is valid during the interlock. (9) The dwell is valid even for the machine lock. (10) Depending on the MTB specifications, the dwell can be canceled by the skip signal (parameter "#1173 dwlskp").
If the set skip signal is input during the dwell time, the remaining time is discarded, and the following block will be executed.
Setting value of #19014 Command increment (ms) Maximum duration of dwell (ms)
-3 0.001 99999.999 (ms) -2 0.01 999999.99 (ms) -1 0.1 9999999.9 (ms) 0 1 99999999 (ms) 1 10 999999.99 (s) 2 100 9999999.9 (s) 3 1000 99999999 (s)
Previous block cutting command
Dwell command
Dwell section
Next block
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
8 Dwell
226IB-1501277-P
Here is a program example which satisfies the following conditions.
#100 = 1000 ; The parameter "#19014 G04 P factor" is set to "0".
(*1) When the parameter "#19014 G04 P factor" is set to a value other than "0", refer to the description for the pa- rameter #19104 in "Detailed description".
The G04 operation in the fixed cycle subprogram follows the asynchronous feed (G94) or synchronous feed (G95) mode that is set when the fixed cycle is commanded. However, if the parameter "#8130 Dwell in rev." is invalid, the dwell (time-based designation) is carried out.
The G04 operation in the synchronous tapping cycle subprogram is set to the dwell (time-based designation) re- gardless of whether the asynchronous (G94) or synchronous (G95) mode is set.
(1) To use this function, G04 must be commanded before "X". When "X" is commanded before G04, the dwell time may differ from the estimated one.
Program example
Command Dwell time [s]
#1078 = 0 #1078 = 1
#8112 = 0 #8112 = 1 #8112 = 0 #8112 = 1
G04 X500 ; 0.5 500 G04 X5000 ; 5 5000 G04 X5 ; 5 5 G04 X#100 ; 1000 1000 G04 P5000 ; 5 (*1) 5 (*1) 5000 G04 P12.345 ; 0.012 (*1) 12.345 0.012 (*1) 12.345 G04 P#100 ; 1 (*1) 1000 1 (*1) 1000
Relationship with Other Functions
Fixed cycle command
Synchronous tapping cycle command
Precautions and restrictions
9
227 IB-1501277-P
Miscellaneous Functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
228IB-1501277-P
9Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits)
The miscellaneous functions are also known as M functions, and they command auxiliary functions, such as spindle forward and reverse rotation, operation stop and coolant ON/OFF.
These functions are designated by an 8-digit number (0 to 99999999) following the address M, and multiple com- mands can be issued in a single block. The number of M commands that can be issued within the same block de- pends on the MTB specifications (parameter "#12005 Mfig").
(Example) G00 Xx Mm1 Mm2 Mm3 Mm4;
When the number of M commands in a single block is greater than the setting value of the parameter "#12005 Mfig", the commands issued later are valid.
Whether to BCD output or binary output the 2nd miscellaneous function can be selected by a parameter.
The eight commands of M00, M01, M02, M30, M96, M97, M98 and M99 are used as auxiliary commands for specific objectives and so they cannot be used as general auxiliary commands.
Reference should be made to the instructions issued by the MTB for the actual correspondence between the func- tions and numerical values. When the M00, M01, M02, and M30 functions are used, the next block is not read into the pre-read buffer due to pre-read inhibiting. If the M function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which sequence applies.
(1) The M function is executed after the movement command. (2) The M function is executed at the same time as the movement command. Processing and completion sequences are required in each case for all M commands except M96, M97, M98 and M99.
When the NC has read this function, it stops reading the next block. As far as the NC system's functions are con- cerned, it only stops reading the next block. Whether machine functions such as the spindle rotation and coolant supply are stopped or not differs according to the machine in question. Re-start is enabled by pressing the automatic start button on the machine operation board. Whether resetting can be initiated by M00 depends on the machine specifications.
Function and purpose
Detailed description
Program stop (M00)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
229 IB-1501277-P
If the M01 command is read when the optional stop switch on the machine operation board is ON, it will stop reading the next block and perform the same operation as the M00. If the optional stop switch is OFF, the M01 command is ignored.
(Example)
This command is normally used in the final block for completing the machining, and so it is primarily used for cueing up the machining program. Whether the program is actually cued up or not depends on the machine specifications. Depending on the machine specifications, the system is reset by the M02 or M30 command upon completion of cue- ing up the program and any other commands issued in the same block. (Although the contents of the command position display counter are not cleared by this reset action, the modal com- mands and compensation amounts are canceled.) The next operation stops when the cueing up operation is completed (the in-automatic operation lamp goes off).
To restart the unit, the automatic start button must be pressed or similar steps must be taken. When the program is restarted after M02 and M30 are completed, if the first movement command is designated only with a coordinate word, the interpolation mode will function when the program ends. It is recommended that a G function always be designated for the movement command designated first.
(1) Individual signals are also output respectively for the M00, M01, M02 and M30 commands and these outputs are each reset by pressing the reset key.
(2) M02 or M30 can be assigned by manual data input (MDI). At this time, commands can be issued simultaneously with other commands.
M96 and M97 are M codes for user macro interrupt control. To use M96 and M97 as miscellaneous functions, change to another M code with the parameter ("#1109 subs_M", "#1110 M96_M" and "#1111 M97_M"). Sequence processing is unnecessary for the M commands (No M code signal nor strove signal is output).
These commands are used as the return instructions from branch destination subprograms and branches to sub- programs. Sequence processing is unnecessary for the M commands (No M code signal nor strove signal is output).
Internal processing suspends pre-reading when the M00, M01, M02 or M30 command has been read. Other tape rewinding operations and the initialization of modals by resetting differ according the machine specifications.
Optional stop (M01)
: N10 G00 X1000 ; The state and operation of optional stop switch N11 M01 ; Stops at N11 when the switch is ON N12 G01 X2000 Z3000 F600 ; Next command (N12) is executed without stopping at N11 when the
switch is OFF :
Program end (M02 or M30)
Macro interruption (M96, M97)
Subprogram call/completion (M98, M99)
Internal processing with M00/M01/M02/M30 commands
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
230IB-1501277-P
9.2 Second Miscellaneous Functions (A8-digits, B8-digits or C8-digits)
These serve to assign the indexing table positioning, etc. In this controller, they are assigned by an 8-digit number from 0 to 99999999 following address A, B or C. The MTB determines which codes correspond to which positions.
The address that is used for the second miscellaneous function (A, B, or C) depends on the MTB specifications (pa- rameter "#1170 M2name"). (Except the address that is used for the axis name and the increment command axis name.)
The second miscellaneous function can be issued for up to 4 sets in a block. The number of commands that can be issued within the same block depends on the MTB specifications (parameter "#12011 Bfig"). Whether to BCD output or binary output the second miscellaneous function can be selected by a parameter. If the A, B or C function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which sequence applies.
(1) The A, B or C function is executed after the movement command. (2) The A, B or C function is executed simultaneously with the movement command.
Processing and completion sequences are required for all secondary miscellaneous functions. The table below gives address combinations. It is not possible to use an address that is the same for the axis name of an additional axis and secondary miscellaneous function.
(1) When A has been assigned as the secondary miscellaneous function address, the following commands cannot be used. Linear angle commands (",A" can be used.) Geometric command
Function and purpose
Detailed description
Additional axis name
A B C
2nd miscellaneous function A - B - C -
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
231 IB-1501277-P
9.3 Index Table Indexing
Index table indexing can be carried out by setting the index axis. The indexing command only requires specifying the indexing angle to the axis set for indexing. It is not necessary to command special M codes for table clamping and unclamping, thus simplifying the program. There are the following two types for this function. Which type is valid and which axis is set as the indexing axis depend on the MTB specifications (parameters "#1282 ext18/bit3" and "#2076 index_x"). Type A: When the unclamp command signal is turned OFF, the clamp operation is performed. Type B: When the clamp command signal is turned ON, the clamp operation is performed. The PLC operation and each signal input/output depend on the MTB specifications.
(1) The movement command (either absolute or incremental) for the selected axis is executed with the program command.
(2) The unclamp command signal is now output prior to the axis movement. (3) When the axes are unclamped, the unclamp completion signal is turned ON by the PLC.
(Turn the signal ON after performing required process such as servo ON or the unclamp process.) (4) After checking the unclamp completion signal, the designated axis starts moving. (5) Upon completion of the movement, the unclamp command signal is turned OFF. (6) Clamp the axes and turn the unclamp completion signal OFF with the PLC.
(Turn the signal OFF after performing required process such as in-position check, servo OFF or the clamp pro- cess.)
(7) After checking that the unclamp completion signal is OFF, processing of the next block is initiated. [Operation time chart]
Function and purpose
Command format
G00 B90 ;
B Index table indexing axis (designated with parameter "#2076 index_x")
Detailed description
Type A operations
Programmed command
Unclamp command (CNC -> PLC)
Unclamp completion (PLC -> CNC)
B axis movement
T10 FIN WAIT 0800 T10 FIN WAIT 0800
G00 B90.;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
232IB-1501277-P
(1) The movement command (either absolute or incremental) for the selected axis is executed with the program command.
(2) The unclamp command signal is now output prior to the axis movement. (3) When the axes are unclamped, the unclamp completion signal is turned ON by the PLC.
(Turn the signal ON after performing required process such as servo ON or the unclamp process.) (4) After checking the unclamp completion signal, turn the unclamp command signal OFF and the designated axis
starts moving. (5) Turn the unclamp completion signal OFF with the PLC. (6) Upon completion of the movement, the clamp command signal is turned ON. (7) Clamp the axes and turn the clamp completion signal ON with the PLC.
(Turn the signal OFF after performing required process such as in-position check, servo OFF or the clamp pro- cess.)
(8) After checking that the clamp completion signal is ON, turn the clamp command signal OFF and processing of the next block is initiated.
(9) Turn the clamp completion signal OFF with the PLC.
When the cutting feed of index table indexing axes is prohibited, the cutting feed can be prohibited by issuing a pro- gram error (P20) if all of the following conditions are satisfied during automatic operation.
The indexing axis movement command is issued. (*1) The modal of G code group 1 is other than "G00" or "G60".
(*1) If a cutting feed command without axis movement (such as "G01 B0;" during incremental command) is issued, the program error does not occur. Also, the unclamp command is not output.
The cutting feed prohibit function is valid for both type A and type B, and the parameter settings depend on the MTB specifications (Parameter "#2580 index_Gcmd").
Type B operations
Programmed command
Unclamp command (CNC -> PLC)
Unclamp command (PLC -> CNC )
Clamp command (CNC -> PLC)
Clamp completion (PLC -> CNC)
Axis movement
T10 FIN WAIT 0800 T10 FIN WAIT 0800
Cutting feed prohibit of index table indexing axes
G00 B90.;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
233 IB-1501277-P
(*1) The unidirectional positioning function can be used in the machining center system only. If parameter "#8209 G60 SHIFT" is not in the indexing unit, a program error (P20) will occur. When an axis command that cannot be divided in the command unit is issued, a program error (P20) will
occur. In a single block operation, the block stop is carried out for the indexing axis at the position specified by
parameter #8209, and the clamp or unclamp operation is carried out.
The clamp and unclamp operations are not executed when the movement commands of the index table indexing axis are successively issued. Note that the clamp and unclamp operations are executed even when the movement commands are continued during single block operation. A combination of G codes that executes clamp or unclamp operation with continuous blocks is listed below. (The unclamp operation is executed before the axis movement of previous block is started, and the clamp operation is executed after the axis movement of the next block.)
(1) Clamp and unclamp operations between continuous blocks
(*1) The clamp and unclamp operations are executed between blocks.
(*2) The clamp and unclamp operations are NOT executed between blocks.
(*3) The clamp and unclamp operations are executed during workpiece installation error compensation (G54.4) or during inclined surface machining command (G68.2).
Relationship with other functions
Index table indexing and other functions
Function Details
Machine coordinate system selection (G53) Possible. Unidirectional positioning (*1) Servo ON/OFF signal control Perform the required process on the PLC.
Single block
Command Continuous block Condition and result
Reference position check (G27) G00 -> G27 (*1) G27 -> G00 (*2)
Start position return (G29) G00 -> G29 (*1) G29 -> G00 (*1)
Tool change position return 1 to 6 Lathe system: G30.1 to G30.5 Machining center system: G30.1 to G30.6
G00 -> G30.1 (*1)
Normal line control cancel (G40.1) (Machining center system only)
G40.1 -> G00 (*1)
Basic machine coordinate system selection (G53) G00 -> G53 (*3) G53 -> G00
Unidirectional positioning (G60) (Machining center system only)
G00 -> G60 (*1) G60 -> G00 (*2) G60 -> G60
Program stop (M00) M00 (*1) Optional stop (M01) M01 (*1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
234IB-1501277-P
(2) Clamp and unclamp operations between continuous blocks (Reference position return) The operation during reference position return depends on the ignoring of intermediate points during return, and it depends on the MTB specifications (Parameter "#1091 Mpoint").
(*1) Performs the clamp operation at the end of G00 movement, and performs the unclamp operation before ref- erence position return.
(*2) The clamp/unclamp operation will not be performed until the reference position return is completed. (*3) Performs the clamp operation after the reference position return, and performs the unclamp operation before
G00 movement. (*4) The clamp/unclamp operation will not be performed when movement to the intermediate point is completed.
The clamp operation will be performed after the reference position return, and the unclamp operation will be performed before G00 movement.
Clamp/unclamp operations during macro interrupt are as follows.
(1) When the macro interrupt program, executed during indexing axis movement, contains a movement command. The commands in the interrupted block are lost, and the interrupt program is executed. After completion of inter- rupt program, when executing from the block next to the interrupt block, the clamp/unclamp operation is execut- ed even if the interrupt program and main program specify the continuous movement.
(Example)
(a) Performs unclamp operation at the beginning of main program N130 block. (b) Executes macro interrupt during main program N130 execution. (c) Performs clamp operation after end of interrupt program O621 N100 block B1. (d) Performs unclamp operation at the beginning of main program N132 block, and performs clamp operation
after axis movement.
Command Continuous block Condition and result
#1091 = 1 #1091 = 0
1st reference position return (G28) G00 -> G28 (*1) (*2) G28 -> G00 (*3) (*4)
2nd to 4th reference position return (G30) G00 -> G30 (*1) (*2) G30 -> G00 (*3) (*4)
Macro interruption
Parameter Settings
#1112 S_TRG 0 Edge trigger mode #1113 INT_2 0 Immediately start the interrupt program without waiting for
the completion of currently executing block. #8101 MACRO SINGLE 1
[Main program] [Interrupt program]
O620(MINT MAIN)
N100 G90G94;
N110 G28B0.X0.;
N120 M96P621;
N130 G01X10.B10.F150.;
N132 G01B15.;
N140 G04X3.;
N150 M97;
M02;
O621(MINT SUB)
N100 G01B1.F500.;
M99;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
235 IB-1501277-P
(2) When the macro interrupt program, executed during indexing axis movement, does not contain a movement command When executing the remaining blocks after completion of interrupt program, perform the unclamp operation at the restart of main program. Also, perform the clamp/unclamp operation even when the next block continues. (Example)
(a) Performs unclamp operation at the beginning of main program N130 block. (b) Executes macro interrupt during main program N130 execution. (c) Interrupt program O623 execution is completed. (d) Performs unclamp operation at the restart of main program N130 block, and performs clamp operation after
completion of axis movement. (e) Performs unclamp operation at the beginning of main program N132 block, and performs clamp operation
after completion of axis movement.
(1) Several axes can be set as index table indexing axes. (2) The movement speed of index table indexing axes follows the feedrate of the modal (G00/G01) at that time. (3) The unclamp command for the indexing axes is also issued when the index table indexing axes are commanded
in the same block as other axes. Thus, the movement of other axes commanded in the same block is not carried out until the unclamp operation completes. Note that the movement of other axes commanded in the same block is carried out during a non-interpolation commands.
(4) Index table indexing axes are used as normal rotation axes, but this function performs an unclamp operation even for linear axes.
(5) If some error that makes unclamp command OFF occurs during indexing axis movement in automatic operation, the unclamp state will remain, and the indexing axis will execute a deceleration stop. Other axes commanded in the same block will also execute a deceleration stop, except during non-interpolation commands.
(6) If the axis movement is interrupted by an interlock, etc., during indexing axis movement, the unclamp state will remain.
(7) The clamp and unclamp operations are not executed when the movement commands of the index table indexing axis are successively issued. Note that the clamp and unclamp operations are executed even when the movement commands are continued during single block operation. Refer to "Single block" of the "Relationship with other functions".
(8) Make sure that the command position is at a position where clamping is possible. (9) Set the unidirectional positioning (G60) parameter "#8209 G60 SHIFT" in indexing increment. A program error
(P20) will occur if it is not set in indexing increment. In a single block operation, the block stop is carried out at the "#8209 G60 SHIFT" position, and the clamp or unclamp operation is carried out.
[Main program] [Interrupt program]
Precautions
O622(MINT MAIN)
N100 G90G94;
N110 G28B0.X0.;
N120 M96P623;
N130 G01X10.B10.F150.;
N132 G01B15.;
N140 G04X3.;
N150 M97;
M02;
O623(MINT SUB)
N100 #100=#100+1;
M99;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
9 Miscellaneous Functions
236IB-1501277-P
10
237 IB-1501277-P
Spindle Functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
238IB-1501277-P
10Spindle Functions 10.1 Spindle Functions
(1) Spindle function (S 8-digit) This function allows you to designate an S command with an 8-digit number (0 to 99999999) following address S and include one pair of S commands in a single block. The output signal is a 32-bit binary data with sign and start signal. Processing and completion sequences are required for all S commands.
(2) Spindle function (S 6-digit analog) When the S 6-digit function is added, S commands can be designated in the range from S0 to S999999. This function outputs the appropriate gear signal or the voltage and start signals matching the spindle rotation speed (r/min) to be commanded using the 6-digit numerical command following the S code. Processing and completion sequences are required for all S commands. If the gear level is switched manually while an S command is not running, this function obtains the appropriate voltage from the rotation speed designated for the gear level and the previously commanded rotation speed, and outputs the result.
Function and purpose
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
239 IB-1501277-P
10.2 Constant Surface Speed Control; G96, G97
This function adjusts the spindle rotation speed (constant surface speed control) in accordance with the movement of the tool nose point so that the cutting point always remains at the constant speed (constant surface speed). Using this function for processes such as a cutting-off process is effective in terms of machining time, tool life, etc. Note that when the tool nose point is moving to the workpiece zero point, the rotation may be at the maximum rota- tion speed defined in the machine specifications; this is dangerous. Be sure to specify the maximum clamp rotation speed with the spindle clamp speed setting command (G92/G50).
Constant surface speed control at constant surface speed command G96 S314 m/min
To keep the surface speed constant, this function obtains and automatically adjusts the spindle rotation speed in accordance with the movement of the tool nose point. In the example above, to keep the surface speed (314 (m/min)) constant, the rotation speed is changed from 999 (r/min) to 1999 (r/min) with changes of the workpiece radius (50mm 25mm).
(1) When the surface speed constant control is commanded under Inch system, the error of the spindle rotation speed specification depends on the MTB specifications (parameter "#1255 set27/bit0").
Function and purpose
Workpiece diameter: 50 mm (Radius value)
Workpiece diameter: 25mm (Radius value)
Spindle rotation speed (r/min) = Surface speed (m/min) / Workpiece surface (m/r) G96 command value Automatically calculated from the workpiece zero
point and tool nose position
314(m/min)
999(r/min) 1999(r/min)
50. 25.314(m/min)
XX
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
240IB-1501277-P
(1) The S command is handled as the absolute value (the sign is ignored). (2) If the value of the S command exceeds the allowable range, a program error will occur (P35). (3) If the value of the P command exceeds the allowable range, a program error will occur (P133).
(1) The S command is handled as the absolute value (the sign is ignored).
Command format
Constant surface speed ON
G96 S__ P__ ;
S Surface speed (-99999999 to 99999999 (m/min), -99999999 to 99999999 (feet/min)) P Constant surface speed control axis 0 to n (n: Number of axes that can be controlled in
the part system with G96 commanded)
Constant surface speed cancel
G97 S__ ;
S Spindle rotation speed (-99999999 to 99999999 (r/min))
Note
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
241 IB-1501277-P
(1) When the P0 or P command is not specified, the operation depends on the MTB specifications (parameter "#1181 G96_ax"). However, if this parameter is set to "0", the first axis is used as the surface speed axis regardless of whether address P is specified or not. 0: Fixed at 1st axis (P command invalid) 1: 1st axis 2: 2nd axis :
(2) To change the constant surface speed control axis in the constant surface speed control mode, specify the com- mand in the G96 P_ format. (However, when the parameter above is set to "0", no change can be made.) If the S command is issued simultaneously, the surface speed can also be changed.
(3) The spindle to be controlled is determined in the MTB specifications (parameter "#1300 ext36/bit0"). For multiple-spindle control II (*1), the spindle is determined by the spindle selection signal from the PLC. (*1) Multiple-spindle control with the PLC signal used. Whether the specification is provided and the details de-
pend on models and MTB specifications.
(4) Specify the spindle surface speed with the S command when constant surface speed control ON is commanded. In constant surface speed control mode, the surface speed can only be changed with the S command.
(5) The spindle clamp speed setting (G92 S__ Q__) is to be commanded when the spindle speed needs to be limited depending on the workpiece to be machined, the chuck to be mounted on the spindle and the tool specifications, etc. Whether the spindle clamp speed setting is made valid only in the constant surface speed control mode or also made valid for normal spindle rotation commands depends on the MTB specifications (parameter "#1227 aux11/ bit5"). Once the maximum clamp rotation speed and the minimum clamp rotation speed are set using the spindle clamp speed setting (G92 S__ Q __), the maximum speed clamp will not be canceled even if the command "G92 S0" is issued. Whether the commanded spindle clamp speed setting is kept when NC is reset during constant surface speed control depends on the MTB specifications (parameter "#1210 RstGmd/bit19").
Detailed description
Machining program
Control axis sequence in constant surface speed command part sys-
tem Details of Operation
1st axis 2nd axis 3rd axis
: G96 S200 P1; : :
X1
Z1
C1
The X1 axis is used as the constant surface speed control axis. (Controls the spindle rotation so that the surface speed is set to 200 (m/min) for the X1 axis.)
G96 P2; :
The Z1 axis is used as the constant surface speed control axis.
Machining program
Control axis sequence in constant surface speed command part sys-
tem Details of Operation
1st axis 2nd axis 3rd axis
: G96 S200 P1; : : :
Z1
C1
- - - - -
The Z1 axis is used as the constant surface speed control axis. (Controls the spindle rotation so that the surface speed is set to 200 (m/min) for the Z1 axis.)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
242IB-1501277-P
(6) Whether the surface speed is always calculated or at the end of a block when the rapid traverse command is issued depends on the MTB specifications (parameter "#1087 G96_G0").
(7) The constant surface speed cancel command (G97) cancels constant surface speed control in the part system that has executed the constant surface speed ON command (G96). The constant surface speed control cannot be canceled from another part system. The spindle rotation speed is maintained at the speed specified when the constant surface speed cancel com- mand (G97) has been executed.
(8) If NC is reset during constant surface speed control, the spindle rotation speed is changed to "0" (r/min) after reset.
When the constant surface speed control is commanded, check whether the spindle speed clamp is valid. If the constant surface speed control axis is near the zero point, it causes the spindle to rotate at the maximum ro- tation speed. Check the spindle speed clamp command to prevent the spindle from rotating at high speed.
(1) In multiple-spindle control II, if the speed clamp command is not valid for the selected spindle, it causes an op- eration error (M01 1043). When such an error occurs, reset to finish the program, and issue the spindle speed clamp command after selecting a spindle. When the operation error above occurs, execute the commands in the same block.
(2) When spindle speed clamp command check is valid, the spindle speed clamp command value is set to "0" if the G92/G50 S0 command is issued.
(3) In multiple-spindle control II, spindle speed clamp check is conducted for the spindle selected in the G96S com- mand. Specify the spindle speed clamp command for all the currently selected spindles.
(4) Whether to conduct spindle speed clamp command check depends on the MTB specifications (parameters "#1146 Sclamp" and "#1284 ext20/bit0".) If parameter "#1146 Sclamp" is set to "0", the spindle speed clamp command cannot be executed when constant surface speed control is turned off; therefore, the spindle speed clamp command cannot be issued before con- stant surface speed control. Parameter "#1284 ext20/bit0" has the following setting:
0: Checks the spindle speed clamp. 1: Does not check the spindle speed clamp.
(5) The spindle speed clamp may be performed only in the constant surface speed mode depending on the MTB specifications (parameter "#1227 aux11/bit5"). If the program is then reset, the clamp may be rendered ineffec- tive. For information on whether the setting is configured to keep the clamp status, refer to the MTB specifications. (Parameter "#1210 RstGmd/bit10, bit19")
BIT10: Group 17, constant surface speed control command modal BIT19: Spindle rotation clamp speed
(6) When operating the system in the initial constant surface speed mode or with the constant surface speed modal by holding the constant surface speed control command modal, the constant surface speed control mode is set by the S command (surface speed). When spindle speed clamp command check is valid, issue the spindle speed clamp command before the S command.
Relationship with Other Functions
Checking the maximum clamp rotation speed
(a) G96 S100 M03 com- mand:
When the spindle forward rotation signal is input from the user PLC by the M03 command, the spindle runs forward. (The spindle speed is set to the previously commanded rotation speed.)
(b) G96 S100 X30. com- mand:
If an error occurs, axis movement is performed until the program is reset.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
243 IB-1501277-P
(1) If constant surface speed control axes are rearranged by the arbitrary axis exchange command, the spindle ro- tation speed is maintained at the value specified before rearrangement.
(2) If a new surface speed is specified by the S command while the spindle rotation speed is maintained, it becomes valid when the rearranged constant surface speed axes are returned to the original status.
(3) If the constant surface speed command is re-executed when constant surface speed axes are rearranged and the spindle rotation speed is maintained at the constant rotation speed, the kept spindle rotation speed is can- celed, and the reissued constant surface speed control command is executed.
(4) If constant surface speed axes are returned to the original status by rearrangement while constant surface speed control is temporarily canceled, the spindle rotation speed will be maintained. After this, the surface speed be- comes constant when it is specified with the S command.
(5) If the surface speed is specified by the S command with the rearrangement of the constant surface speed axes while the constant surface speed control is in the temporary cancel state, the spindle rotation speed kept at tem- porary cancellation is applied, and the surface speed becomes constant when the constant surface speed axes are returned to the original arrangement.
Arbitrary axis exchange control
Other functions
Function name Operation
Spindle Clamp Speed Setting (G92/G50) The spindle clamp speed setting is valid in the constant surface speed control mode. Whether the commanded spindle clamp speed setting is kept when NC is reset during constant surface speed control depends on the MTB specifications. (parameter "#1210 RstGmd BIT19")
Cylindrical Interpolation (G07.1) The constant surface speed control cannot be commanded during the cylindrical interpolation mode. Program error (P481) will occur. The cylindrical interpolation cannot be commanded during the con- stant surface speed control mode. Program error (P485) will occur.
Thread Cutting (Designation of lead or number of ridges) (G32)
When the constant surface speed command is issued in the same part system during execution of the thread cutting or thread cutting cycle command or when the thread cutting or thread cutting cycle command is issued in the same part system in the constant surface speed control mode, the spindle rotation speed for constant surface speed control remains unchanged. (The constant surface speed control is not performed.) This function keeps the spindle rotation speed specified at execution of the thread cutting or thread cutting cycle command. When the thread cutting or thread cutting cycle command is terminat- ed, the spindle rotation speed is changed to the value obtained from the position of the constant surface speed control axis and the sur- face speed. The constant surface speed command cannot be issued from other part systems to the spindle for which the thread cutting command is currently executed. Also, the thread cutting command cannot be is- sued from other part systems to the spindle in the constant surface speed control mode. An operation error (M01 1113) will occur.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
244IB-1501277-P
Tapping cycle (G84/G88) Synchronous tapping cycle (G84/G88)
If the constant surface speed command is issued in the same part system during execution of the tapping cycle or synchronous tapping cycle command or the tapping cycle command is issued in the same part system in the constant surface speed control mode, the spindle rotation speed for constant surface speed control remains un- changed. (The constant surface speed control is not performed.) This function keeps the spindle rotation speed specified at execution of the tapping cycle command. When the tapping cycle or synchronous tapping cycle command is terminated, the spindle rotation speed is changed to the value ob- tained from the position of the constant surface speed control axis and the surface speed. The constant surface speed command cannot be issued from other part systems to the spindle for which the tapping cycle or synchro- nous tapping cycle command is currently executed. Also, the tapping cycle or synchronous tapping cycle command cannot be issued from other part systems to the spindle in the constant surface speed con- trol mode. An operation error (M01 1113) will occur. The synchronous tapping cycle command cannot be executed in the constant surface speed control mode. Program error (P182) will oc- cur. Also, the constant surface speed command cannot be executed during execution of the synchronous taping cycle command. Program error (P186) will occur.
Spindle-Mode Servo Motor Control The system also runs when a spindle-mode servo is specified for con- stant surface speed control
External Spindle Deceleration If the external spindle deceleration signal is set to OFF for the spindle under constant surface speed control, the spindle is clamped at the external spindle deceleration speed. The S analog maximum/mini- mum over signal (SOVE) is set on.
High-Speed Simple Program Check The surface speed is calculated, but the actual rotation speed of the spindle remains set to the value specified before the part system syn- chronization machine lock high-speed operation is selected.
NC reset (Reset 1/2, reset & rewind) When NC is reset during constant surface speed control, the spindle rotation speed is set to "0" (r/min).
Function name Operation
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
245 IB-1501277-P
(1) Under the constant surface speed control (during G96 modal), if the axis targeted for the constant surface speed control (normally X axis for a lathe) moves toward the spindle center, the spindle rotation speed will increase and may exceed the allowable speed of the workpiece or chuck, etc. In this case, the workpiece, etc. may jump out during machining, which may break tools or the machine or injure the operators. Therefore, make sure to use this control while the "spindle speed clamp" is enabled. When the constant surface speed control is commanded, keep enough distance from the program zero point.
Program example
(Example 1) When the parameter "#1146 Sclamp" is set to "0"
(Example 2) When the parameter "#1146 Sclamp" is set to "1"
(2) When the G96 command is issued, do not omit the "S_" surface speed command. If omitted, the system will fol- low the previous "S_" command. The S command ("S_" command) for the spindle in the constant surface speed control mode specifies the sur- face speed.
(3) If the spindle speed clamp is not commanded when the constant surface speed control axis is near the zero point, it causes the spindle to rotate at the maximum rotation speed. We recommend that you command the spindle speed clamp before the constant surface speed command. In this case, the parameter "#1146 Sclamp" must be made valid, but this function depends on the MTB specifi- cations.
(4) If an axis number not registered in the command part system is commanded when the constant surface speed command is specified, it causes a program error (P133).
Precautions
G96 S200 ; The spindle rotation speed is controlled so that the surface speed is 200 m/min. G92 S4000 Q200 ; The spindle rotation speed is clamped up to 4000 r/min and down to 200 r/min. M3 ; The rotation command to the spindle
G92 S4000 Q200 ; The spindle rotation speed is clamped up to 4000 r/min and down to 200 r/min. G96 S200 ; The spindle rotation speed is controlled so that the surface speed is 200 m/min. M3 ; The rotation command to the spindle
WARNING
Under the constant surface speed control (during G96 modal), if the axis targeted for the constant surface speed
control (normally X axis for a lathe) moves toward the spindle center, the spindle rotation speed will increase
and may exceed the allowable speed of the workpiece or chuck, etc. In this case, the workpiece, etc. may jump
out during machining, which may break tools or the machine or injure the operators.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
246IB-1501277-P
10.3 Spindle Clamp Speed Setting; G92
The maximum clamp rotation speed of the spindle can be assigned by address S following G92 and the minimum clamp rotation speed by address Q. Use this command when the spindle speed needs to be limited depending on the workpiece to be machined, the chuck to be mounted on the spindle and the tool specifications, etc.
(1) Besides this command, parameters can be used to set the rotation speed range up to 4 stages in 1 r/min units to accommodate gear selection between the spindle and spindle motor. The lowest upper limit and highest lower limit are valid among the rotation speed ranges based on the parameters and based on "G92 S_ Q_;".
(2) Whether to carry out rotation speed clamp only in the constant surface speed mode or even when the constant surface speed is canceled depends on the MTB specifications (parameters "#1146 Sclamp" and "#1227 aux11/ bit5").
The address Q following the G92 command is handled as the spindle speed clamp command regardless of the constant surface mode.
(3) The command value of the spindle clamp rotation speed will be cleared by modal reset (reset 2 or reset & rewind). Note that the modal is retained if the parameter "#1210 RstGmd / bit19" is ON. It is set to "0" during power ON.
Function and purpose
Command format
Spindle clamp speed setting
G92 S__ Q__ ;
S Maximum clamp rotation speed Q Minimum clamp rotation speed
Detailed description
Sclamp=0 Sclamp=1
aux11/bit5=0 aux11/bit5=1 aux11/bit5=0 aux11/bit5=1
Command In G96 Rotation speed clamp command Rotation speed clamp command In G97 Spindle rotation speed command Rotation speed clamp command
Operation In G96 Rotation speed clamp execution Rotation speed clamp execution In G97 No rotation speed clamp Rotation speed clamp
command No rotation speed
clamp
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
247 IB-1501277-P
(1) Once the maximum clamp speed and the minimum clamp speed are set using the spindle clamp speed setting (G92 S__ Q __), the maximum speed clamp will not be cancelled even if the command "G92 S0" is issued. During this time, the Q__ value is still valid and S0 < Q__ is established. The Q__ value is treated as the maxi- mum speed clamp, and S0 is treated as the minimum speed clamp.
(2) Note that if the spindle clamp speed setting (G92 S__ Q__) is not commanded, the speed may increase to the machine's maximum specified speed that is set by the parameter. Especially when the constant surface speed control (G96 S__) is commanded, command the spindle clamp speed setting as well as the spindle maximum rotation speed. As the tool moves closer to the spindle center, the spindle rotation speed will increase and may exceed the allowable speed of the workpiece or chuck, etc.
Precautions
WARNING
The spindle clamp speed setting command is a modal command, but make sure to confirm that the G and F
modal and coordinate values are appropriate if the operation is started from a block in the middle of the pro-
gram. If there are coordinate system shift commands or M, S, T and B commands before the block set as the
start position, carry out the required commands using the MDI, etc. If the program is run from the set block with-
out carrying out these operations, the machine interference may occur or the machine may operate at an unex-
pected speed.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
248IB-1501277-P
10.4 Spindle Position Control (Spindle/C Axis Control)
This function controls a spindle as the rotary axis. After switching the spindle to the rotary axis, the positioning and the interpolation between the spindle and other NC axes can be operated in the same way as the NC axis by exe- cuting the position command (the movement command). Using this function, the NC axis for controlling the spindle stock as the rotary axis or the machinery for switching the spindle and NC axis (such as a gear switching machinery) had been necessary for controlling a spindle stock readily as the rotary axis, but they are not necessary with this function. For information on how to validate or invalidate this function, each setting to use this function, and the mechanism of your machine, refer to the specifications or the instruction manual issued by the MTB. There are two methods to switch the spindle and rotary axis: PLC signal method and program command method. The available method depends on the MTB specifications (parameter "#3129 cax_spec/bit0"). For details, refer to the specifications issued by the MTB. This section describes the program command method. In this manual, the state of controlling an axis as a spindle is referred to as "spindle mode", and the state of con- trolling an axis as a rotary axis is referred to as "C axis mode".
The PLC signal processing and operation depends on the MTB specifications. Refer to the instruction manual issued by the MTB for details.
For the encoder-based spindle position control (PLG and external encoder), set the Z phase position of the encoder as the first reference point of the C axis. This first reference point is used as the coordinate zero point; however, the spindle zero point position can be adjusted with the spindle/C axis reference position return shift amount parameter, which is determined in the MTB specifications. This parameter is determined in the MTB specifications (parameter "#3113 cax_sft").
(1) In the machining program, the program switches to the C axis mode with G00 command, and to the spindle mode with S command. The C axis servo OFF signal (*SVFn) must be always kept ON while the program command method is selected. This depends on the MTB specifications. When the servo OFF signal is set to OFF, operations are performed as follows. The mode cannot be switched from the spindle mode to the C axis mode. However, it can be switched from the C axis mode to the spindle mode. In the spindle mode, the axis does not run as a spindle even if the forward run command (SRN) or reverse run command (SRI) is executed. In the C axis mode, an operation error (M01 0005) occurs if the movement command is executed. In the servo OFF mode, operations follow the setting of the parameter "#1064 svof" (error correction) MTB speci- fications).
(2) It depends on the MTB specifications (the parameter "#3129 cax_spec/bit2") either the spindle mode or the C axis mode is set when the power is turned ON. If the power is turned ON in the C axis mode setting, the mode shifts to the C axis mode after the Z phase de- tection and reference position return operations have been performed. For Z phase detection, the spindle rotates in the C axis zero point return direction (*2) at the C axis zero point return speed (*1). (*1) Depends on the MTB specifications (parameter "#3112 cax_spd").
(*2) Depends on the MTB specifications (parameter "#3106 zrn_typ/bit9, bitA").
(3) It depends on the MTB specifications (the parameter "#3129 cax_spec/bit3") either the spindle mode or the C axis mode is set when NC is reset.
Function and purpose
Coordinate zero point and zero point adjustment in C axis mode
Program command method
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
249 IB-1501277-P
Command "G00 C_ " in the NC program during the spindle mode. The axis is positioned directly to the specified position. The non-interpolation positioning for each axis is performed by specifying "G00 X__ Z__ C__" regardless of the G00-interpolation OFF parameter ("#1086 G0Intp" in the MTB specifications) setting, and C axis is switched to the C axis mode. Only the G00 command is valid to switch the mode. If the mode is commanded with another G code, it causes
a program error (P430). Designate the axis for spindle position control with the absolute address or absolute command (G90). If the axis
is designated with the incremental address or incremental command (G91), it causes a program error (P32). The reference position return type (*1) is set at switching, and the direction to return from the rotation mode to
the zero point follows the rotation direction (*2). The direction for returning from the stop mode to the reference position and the interpolation mode depend on the MTB specifications (parameters "#3106 zrn_typ/bit9,bitA", "#3106 zrn_typ/bitD,bitE" and "#1256 set28/bit1"). (*1) Type to necessarily return to the reference position when switching from the spindle mode to the C axis mode.
This depends on the MTB specifications (parameter "#3106 zrn_typ/bit8").
(*2) Depends on the MTB specifications (parameter "#3106 zrn_typ/bitB").
If the Z phase is not detected and if switching is commanded, the spindle is rotated in the zero point return di- rection (*4) at the zero point return speed (*3). Then, the zero point return operation is executed after the Z phase detection. (*3) Depends on the MTB specifications (parameter "#3112 cax_spd").
(*4) Depends on the MTB specifications (parameter "#3106 zrn_typ/bitA-9").
[C axis mode switching conditions] When switching is commanded, all the following conditions must be satisfied. The C axis servo OFF signal (*SVFn) is ON.
The switching is performed with the spindle forward run signal (SRN) ON or the spindle reverse run signal (SRI) ON and the S command. The switching is performed with the startup of the spindle forward run signal (SRN) or the spindle reverse run
signal (SRI). [Spindle mode switching condition]
When switching is commanded, all the following conditions must be satisfied.
The C axis servo OFF signal (*SVFn) is ON. The C axis selection signal (CMD) is OFF. The C axis is stopped.
Command format
Switching from spindle mode to C axis mode (C axis)
G00 C__ ;
C Target C axis in C axis mode
Switching C axis mode to spindle mode
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
250IB-1501277-P
(1) Example in which the mode is switched to the spindle mode with the forward run command and the rotation com- mand (S command) M03 command -> Forward run command (SRN) ON and reverse run command (SRI) OFF M04 command -> Reverse run command (SRI) ON and forward run command (SRN) OFF
(2) Example in which the mode is switched to the spindle mode by a change from the forward run command to the reverse run command M03 command -> Forward run command (SRN) ON and reverse run command (SRI) OFF M04 command -> Reverse run command (SRI) ON and forward run command (SRN) OFF
Detailed description
Mode switching
Program example Mode Description
M03 S1000; Spindle mode The spindle rotates at forward run speed 1000 (r/min). : : G00 C90.; C axis mode The axis is positioned at 90 degrees directly based on the rotation
mode. After positioning, the mode is switched from the spindle mode to the C axis mode.
G01 X10. C20. F100; In the C axis mode, the spindle can be commanded as the rotary axis. : In the C axis mode, interpolation with another NC axis is possible. M03 S1500; Spindle mode The mode is switched from the C axis mode to the spindle mode with
the forward run command and rotation command (S command). : : After being switched to the spindle mode, the spindle rotates at for-
ward run speed 1500 (r/min). G00 X20.C270.; C axis mode The axis is positioned at 270 degrees directly based on the rotation
mode, and stops at the position. Simultaneously, the X axis is posi- tioned at 20mm with interpolation. After positioning, the mode is switched from the spindle mode to the C axis mode.
Program example Mode Description
M03 S1000; Spindle mode The spindle rotates at forward run speed 1000 (r/min). : : G00 C90.; C axis mode The axis is positioned at 90 degrees directly based on the rotation
mode. After positioning, the mode is switched from the spindle mode to the C axis mode.
G01 X10. C20. F100 ; In the C axis mode, the spindle can be commanded as the rotary axis. : In the C axis mode, interpolation with another NC axis is possible. M4; Spindle mode The mode is switched from the C axis mode to the spindle mode with
the reverse run command. : After being switched to the spindle mode, the spindle rotates at re-
verse run speed 1000 (r/min). : G00 X20.C270.; C axis mode The axis is positioned at 270 degrees directly based on the rotation
mode, and stops at the position. Simultaneously, the X axis is posi- tioned at 20 mm with interpolation. After positioning, the mode is switched from the spindle mode to the C axis mode.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
251 IB-1501277-P
(3) Example in which the mode is not switched from the C axis mode to the spindle mode M03 command -> Forward run command (SRN) ON and reverse run command (SRI) OFF
When the program command method is selected, switching operation is performed with the reference position return type.
Program example Mode Description
M03 S1000; Spindle mode The spindle rotates at forward run speed 1000 (r/min). : : G00 C90.; C axis mode The axis is positioned at 90 degrees directly based on the rotation
mode. After positioning, the mode is switched from the spindle mode to the C axis mode.
G01 X10. C20. F100; In the C axis mode, the spindle can be commanded as the rotary axis. : In the C axis mode, interpolation with another NC axis is possible. M3; C axis mode The rotation command (S command) is omitted between the forward
run commands, and the rising edge (change) of the forward run com- mand is not detected; therefore, the mode is not switched to the spin- dle mode. The forward run command must be changed from OFF to ON with the rotation command (S command) or M3 command.
: :
Switching operation
Machining program
Spindle rotation speed (C axis speed)
Spindle
X axis speed
PLCNC
Servo OFF signal *SVFn
Forward run command SRN
NCPLC
Servo ready RDYn
C axis mode SVMD
M03 S1000 G00 X10.C45. M03 S1000G01 C180. F90
45.0(deg)
180.0(deg)
X axis positioning (non-interpolation)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
252IB-1501277-P
To rotate the spindle/C axis as the C axis in the manual operation mode, change the "C axis selection" signal (CMOD) from OFF to ON to switch to the C axis mode while the "Servo OFF" signal (*SVFn) is ON. When switching to the spindle mode, change the C axis selection signal from ON to OFF. The switching operation is performed with the reference position return type. In the C axis mode, the axis can be moved by selecting the manual mode (jog mode, handle mode, incremental feed mode, manual arbitrary-feed mode, or reference position return mode).
If the C axis selection signal (CMOD) is changed while either the C axis mode or spindle mode is selected in the program command method, the mode is set as follows. The mode is not switched to the C axis mode or spindle mode in the program command method during automatic running when the C axis selection signal is turned ON. Switching follows the state of the C axis selection signal (CMOD).
Manual operation with the program command method selected
PLCNC
Servo OFF signal *SVFn
Manual mode ON
C axis selection signal CMODn
C axis feed axis selection (+J/-J)
Forward run command SRN
NCPLC
Servo ready RDYn
C axis mode SVMD
C axis selec- tion signal (CMOD)
During automatic operation During reset
C axis mode by "G00 C_ com- mand"
Spindle mode by "S command"
C axis mode Spindle mode
OFF to ON C axis mode C axis mode C axis mode C axis mode ON to OFF C axis mode Spindle mode Spindle mode Spindle mode Remarks Whether the mode is
switched to the C axis mode during reset depends on the MTB specifications. (#3129 cax_spec/bit2) (#3129 cax_spec/bit3)
Reference position return
C axis Spindle
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
253 IB-1501277-P
The mode is switched to the C axis mode regardless of the state of the spindle forward-run start (SRN) or spindle reverse-run start (SRI) signal. In the C axis mode, spindle forward-run start and spindle reverse-run start are invalid. When [PLC signal method] is selected, the spindle rotates by carrying out the spindle forward-run start or spindle reverse-run start again (OFF to ON operation) after the C axis mode has been canceled. When [Program command method] is selected, the spindle rotates by carrying out the spindle forward-run start or spindle reverse-run start again (OFF to ON operation) in the C axis mode or by issuing the S command with the spindle forward-run start or spindle reverse-run start set ON.
[M8 Series]
The mode is switched to the C axis mode regardless of the state of the "Spindle orientation command" signal (ORC). However, in the C axis mode, the "Spindle orientation command" signal (ORC) is invalid. [C80]
The "Spindle orientation command" signal (ORC) is invalid in the C axis mode. The spindle position control com- mand (Spindle/C axis control) is also invalid under spindle orientation.
Gear switching cannot be performed in the C axis mode. After the mode has been changed from the C axis mode to the spindle mode, gear switching is performed. Also, the mode cannot be switched to the C axis mode during gear switching. After gear switching has been completed, the mode is switched to the C axis mode.
Coil switching is invalid in the C axis mode. Conduct coil switching before switching to the C axis mode. If switching to the C axis mode is commanded during coil switching, switching to the C axis mode is executed after coil switching has been completed.
(1) Spindle synchronization I If the reference spindle or the synchronized spindle under the synchronization control is switched to the C axis mode, it causes an operation error (M01 1026). Also, if the reference spindle command or synchronized spindle command is issued to the spindle in the C axis mode, it causes an operation error (M01 1026). The alarm can be deactivated by canceling the synchronization command or the C axis mode.
enables the spindle position control by the reference spindle under spindle synchronization control.
The spindle override is invalid for the reference position return operation at switching to the C axis mode. In the C axis mode, the spindle override is invalid. The cutting feed override or rapid traverse override of the NC axes is valid in the C axis mode.
Relationship with other functions
Spindle forward-run start (SRN) and spindle reverse-run start (SRI)
Spindle orientation signal (ORC)
Spindle gear switching
Coil switching
Spindle synchronization I
Spindle override
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
254IB-1501277-P
The spindle position control is valid, excluding the following differences.
(1) Speed pattern of the reference position return operation The reference position return from the stop mode is performed by the same operation as for the normal spindle. However, when the spindle returns from the rotation mode to the zero point, the rotation speed decelerates up to the C axis zero point return speed with the multi-step acceleration/deceleration pattern. After the C axis zero point return speed has been reached, the spindle inclines to the zero point, and stops while decelerating at the constant speed The multi-step acceleration/deceleration pattern and C axis reference position return speed de- pend on the MTB specifications (parameters "#3054 sptc1" to "#3061 spdiv1" and "#3112 cax_spd").
The spindle position control is invalid.
The absolute position detection is invalid in the C axis mode.
When Program command method is selected, the mode is switched from the C axis mode to the spindle mode if the surface speed command S (m/min) and the spindle forward-run start (SRN) or spindle reverse-run start (SRI) signal is set to ON.
When the program command method is selected, "block switched from spindle mode to C axis mode (example: G00 C_) and "block switched from C axis mode to spindle mode (example: M03 S1000)" is handled as a reverse run prohibited block. The reverse run cannot be carried out back through blocks with the mode switched.
The offset values of the coordinate system setting and local coordinate system setting configured in the C axis mode are retained even in the spindle mode.
After this, whether these offset values designated in the previous C axis mode are to be retained when the spindle mode is switched to the C axis mode depends on the MTB specifications (parameter "#3129 cax_spec/bit5").
Spindle-mode servo motor control
Stop mode Rotation mode
Multi-step acceleration/deceleration
Spindle zero point
Spindle zero point
Analog spindle, spindle control with pulse train output
Absolute position detection
Constant surface speed control
Manual arbitrary reverse run
Coordinate system setting (G92), Local coordinate system setting (G52)
#3115 sp2_t1
#3112 cax_spd
#3001 slimt1
#3115 sp2_t1
#3112 cax_spd
#3001 slimt1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
255 IB-1501277-P
(1) If the movement is commanded while the servo OFF signal (*SVFn) is set to OFF, it causes an operation error (M01 0005). Reset NC to cancel the error, and set the servo OFF signal on to restart machining. If the spindle command is issued, the spindle does not rotate.
(2) If the servo OFF signal (*SVFn) is set to OFF during C axis movement, it causes an operation error (M01 0005). Reset NC to cancel the error.
(3) To switch from the spindle mode to the C axis mode, issue the G00 command. If a command other than the G00 command is issued, it causes a program error (P430).
(4) The spindle position control axis must be commanded with the absolute address or absolute command (G90). If the incremental address or incremental command (G91) is used, it causes a program error (P32).
(5) When the spindle mode is switched to the C axis mode, in-position check is applied regardless of the deceleration check designation type (*1). (*1) This designation depends on the MTB specifications (parameter "#1193 inpos").
Precautions and restrictions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
256IB-1501277-P
10.5 Spindle Speed Fluctuation Detection; G162/G163
When this function is valid and the spindle actual speed fluctuates relative to the programmed speed due to external factors such as load fluctuation, the NC outputs the signal (Spindle speed out of setting range) to PLC and causes the operation error (M01 1105) at the same time. PLC can take the necessary measure for the fluctuation of the spindle speed using the output signal (spindle speed out of setting range) from the NC. The operation error (M01 1105) output from the NC does not stop the cycle operation or the spindle. Whether or not to output the operation error during spindle speed fluctuation detection (G162) depends on the MTB specifications (parameter "#1242 set14/bit2").
The following descriptions are the meanings of the terms used in this manual.
Function and purpose
Term
Term Meaning
Spindle command speed
Spindle command speed is the command speed to which the spindle override and the spindle clamp speed have been added. This is the spindle last command speed sent to the spindle drive unit.
Spindle actual speed This is the speed fed back from the spindle, at which the spindle actually runs. Allowable fluctua- tion range
This indicates the allowable deviation range from the command speed in spindle speed fluctuation detection. The calculation result for the command speed of "spindle speed fluc- tuation allowance rate" (R address or parameter) or "allowable spindle speed fluctuation range" (I address or parameter), whichever is greater, is used as the allowable fluctuation range. When the calculation result for the command speed of "detection range to achieve spindle speed", which is used to determine whether or not the spindle rotation speed achieves the command speed, is greater than the calculation result for the command speed of "allow- able fluctuation rate of spindle speed" or "allowable fluctuation range of spindle speed", the range of "detection range to achieve spindle speed" is used as allowable fluctuation range.
(r/min)
(S)
Spindle rotation speed
Spindle speed fluctuation detection in monitor
Allowable fluctuation speed range (Set by "R" or "I" address.)
In spindle speed fluctuation detection
Spindle speed fluctuation detection: Spindle speed out of setting range
Commanded speed
Actual speed
Time
G162 command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
257 IB-1501277-P
Command format
Starting the spindle speed fluctuation detection
G162 S__ P__ Q__ R__ I__ ;
S Spindle name of detection target P Spindle speed fluctuation detection start delay time Q Spindle up-to-speed detection width R Allowable fluctuation rate of spindle speed I Allowable fluctuation range of spindle speed
Spindle speed fluctuation detection cancel
G163 S__ ;
S Spindle name of detection target
Detailed description
Description of each address
Address Command range (unit) Remarks
S 1 to 9 This sets the name of the spindle which performs the spindle speed fluctu- ation detection. The spindle number is used for this command, but the val- ue set by the parameter (#3077) is used when the spindle name method is valid. When this address is omitted from the G162 command, the spindle selected
in the commanded part system is treated as the commanded spindle. When this address is omitted from the G163 command, the fluctuation de- tection for all spindles is canceled. When the set spindle is not mounted, the program error (P35) occurs.
P 0 to 99.999(s) This sets the delay time from the time when the spindle speed fluctuation detection (G162) is commanded to the time to start the fluctuation detec- tion. Also when the spindle command speed changes, the delay time is set. The change of the spindle command speed means the change of the spin- dle last command sent to the spindle drive unit. When this address is omitted, the value set in the parameter "#43071
sp_spd_flc_dtc_p" is used. When the command value exceeds the command range, the program error
(P35) occurs. Q 1 to 100 (%) This sets the range for the spindle speed command, with which the control
determines whether the spindle reaches the command speed in order to start fluctuation detection. When this address is omitted, the value set in the parameter "#3105 sut" is
used. When the command value exceeds the command range, the program error
(P35) occurs.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
258IB-1501277-P
(1) This function is valid when the spindle speed fluctuation detection (G162) is commanded during the cycle oper- ation.
(2) When G162 is commanded during the cycle operation, it is valid until G163 command (cancel command), cycle operation end, reset or emergency stop.
(3) If any function that is unusable with this function is enabled while this function is valid, this function is temporarily canceled. After that, when the said unusable function is disabled, this function is enabled.
(4) When G162 is commanded while any unusable function is valid, this function is temporarily canceled. After that, when the said unusable function is disabled, this function is enabled.
R 1 to 100 (%) This sets the allowable fluctuation speed range calculated for the spindle command speed. When the actual spindle speed exceeds the range, the signal is output to PLC and the operation error (M01 1105) occurs. This sets the ratio of the speed deviation to the command speed. When this address is omitted, the value set in the parameter "#43072
sp_spd_flc_dtc_r" is used. When the command value exceeds the command range, the program error
(P35) occurs. When the speed deviation for the command speed is smaller than 45 r/min,
the allowable range of the speed deviation is 45 r/min. I 0 to 999999 (r/min) This sets the allowable fluctuation speed range calculated for the spindle
command speed. When the actual spindle speed exceeds the range, the signal is output to PLC and the operation error (M01 1105) occurs. This sets the speed deviation from the command speed. When this address is omitted, the value set in the parameter "#43073
sp_spd_flc_dtc_i" is used. When the command value exceeds the command range, the program error
(P35) occurs.
Enabling conditions of the function
Address Command range (unit) Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
259 IB-1501277-P
When one of the following conditions is satisfied after G162 command, the spindle speed fluctuation detection starts: Case in which the start delay time of the spindle speed fluctuation detection (set by "P") elapses (Refer to (1)
figure.) Case in which the spindle actual speed is within the detection range to achieve spindle speed (set by "Q") (Refer
to (2) figure.) (1) Case in which the start delay time of the spindle speed fluctuation detection (set by "P") elapses
Operation example
Start timing of spindle speed fluctuation detection
N1 G97 G98; N2 S__; N3 M3; N4 G162 S__ P__ Q__; :
0
N2 N3 N4
Commanded speed
Actual speed
Commanded speed
Spindle forward run start (SRN)
Spindle speed fluctuation detection state
Spindle rotation speed
Waiting for start In fluctuation detection
S command
Delay time elapses Achieved the range to achieve speed
Range to achieve speed (Q)Allowable fluctuation range
Delay time to start spindle speed fluctuation detection (P)
Time
Invalid
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
260IB-1501277-P
(2) Case in which the spindle actual speed is within the detection range to achieve spindle speed (set by "Q")
N1 G97 G98; N2 S__; N3 M3; N4 G162 S__ P__ Q__; :
0
Commanded speed
Actual speed
Commanded speed
Spindle forward run start
Spindle speed fluctuation detection state
Spindle rotation speed
Waiting for start In fluctuation detection
S command
Delay time elapses
Achieved the range to achieve speed
Range to achieve speed (Q)Allowable fluctuation range
Delay time to start spindle speed fluctuation detection (P)
Time
Invalid
N2 N3 N4
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
261 IB-1501277-P
When the spindle command speed is changed by S command or spindle override, the state is the same as the one immediately after G162 command and the fluctuation detection is not performed until the condition of "Start timing of spindle speed fluctuation detection" is satisfied. When this condition is satisfied, the fluctuation detection is start- ed. Also, if the speed of synchronized spindle, which is driven based on the reference spindle speed under synchro- nization etc., changes, the control interprets that the spindle command speed is changed. (Spindle synchronization control/Polygon machining/Hobbing/Spindle superimposition control)
The spindle speed fluctuation detection function cannot be combined with the following functions. This is because these functions cause the spindle speed to be changed frequently without ensuring the spindle rotation at a constant speed. Synchronous tapping (Synchronous tapping cycle/Pecking tapping cycle/Deep-hole tapping cycle/High-speed
synchronous tapping) Spindle orientation C axis mode of spindle position control (spindle/C axis control) When any of the functions above is enabled while the spindle speed fluctuation detection is enabled, this function is temporarily canceled. After that, when the said unusable function becomes invalid, this function is enabled. When this function is commanded while an unusable function is running, this function is temporarily canceled. After that, when the said unusable function becomes invalid, this function is enabled. When this function is enabled, the state is the same as the one immediately after G162 command. Fluctuation detection is started if the condition of "Start timing of spindle speed fluctuation detection" is satisfied.
Fluctuation detection start timing when the spindle command speed is changed
Temporary cancellation operation of spindle speed fluctuation detection
N1 G97 G98; N2 S__; N3 M3; N4 G162 S__ P__ Q__; : N5 S__; :
N5
Commanded speed
Actual speed
Commanded speed
Spindle forward run start (SRN)
Spindle speed fluctuation detection state
Spindle rotation speed
Waiting for startIn fluctuation detection In fluctuation detection
S command (N5)S command (N2)
Delay time elapses
Achieved the range to achieve speed
Delay time to start spindle speed fluctuation detection (P)
Range to achieve speed (Q)Allowable fluctuation range
Change of the spindle command speed
Time
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
10 Spindle Functions
262IB-1501277-P
When the command with the exact same settings is given to the axis where this function is enabled, the command is ignored. On the other hand, when at least one of the settings other than S address (P, Q, I, or R) is different, the setting is changed to the new one. After that, the state is the same as the one immediately after G162 command. Fluctuation detection is started if the condition of "Start timing of spindle speed fluctuation detection" is satisfied. Changing the S address means that the spindle speed fluctuation detection is commanded to a different spindle.
This function is temporarily canceled during synchronous tapping (synchronous tapping cycle/pecking tapping cycle/ deep-hole tapping cycle/high-speed synchronous tapping).
When G162 command is commanded omitting S address, the operation is performed to the spindle which is selected by multiple-spindle control.
This function is temporarily canceled during spindle orientation.
This function is temporarily canceled in the C axis mode. The fluctuation detection can be performed in the spindle mode.
Constant surface speed control can be combined with this function. However, the fluctuation detection is not per- formed unless the fluctuation detection start condition is satisfied each time the spindle speed fluctuates; therefore, the fluctuation detection may not be performed much.
Manual arbitrary reverse run cannot be performed to the command of this function.
(1) While the spindle is stopped, the spindle speed fluctuation detection is not performed. (2) The spindle speed fluctuation detection is not performed to the speed which is the minimum rotation speed (pa-
rameter #3032) or less. (3) The spindle speed fluctuation detection is not performed during synchronous tapping, spindle orientation, C axis
control mode of spindle or C axis. (4) When any other command is issued at the same time, the program error (P45) occurs.
When the spindle speed fluctuation detection command (G162) is performed during the spindle speed fluc- tuation detection
Relationship with other functions
Synchronous tapping
Multiple-spindle control I/II
Spindle orientation
Spindle position control (Spindle/C axis)
Constant surface speed control
Manual arbitrary reverse run
Precautions
11
263 IB-1501277-P
Tool Functions (T command)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
11 Tool Functions (T command)
264IB-1501277-P
11Tool Functions (T command) 11.1 Tool Functions (T8-digit BCD)
The tool functions are also known as T functions and they assign the tool numbers. This control unit specifies a tool number with an 8-digit (0 to 99999999) number following the address T, and up to four sets can be commanded into one block. However, the number of sets that can be commanded within the same block depends on the MTB spec- ifications (parameter "#12009 Tfig"). One of the following output signals is issued depending on the parameter setting (depends on the machine specifi- cations). - 8-digit BCD code and start signal - Signed 32-bit binary data and start signal - Unsigned 32-bit binary data and start signal If the T function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which sequence applies.
(1) The T function is executed after completion of the movement. (2) The T function is executed simultaneously with the movement command. Processing and completion sequences are required for all T commands.
Function and purpose
12
265 IB-1501277-P
Tool Compensation Functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
266IB-1501277-P
12Tool Compensation Functions 12.1 Tool Compensation 12.1.1 Tool Compensation
The basic tool compensation function includes the tool length compensation and tool radius compensation. Each compensation amount is designated with the tool compensation No. Each compensation amount is input from the setting and display unit or the program.
Function and purpose
Tool length compensation
Basic point
Tool length
(Side view)
Tool radius compensation
(Plane view)
Right compensation
Left compensation
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
267 IB-1501277-P
There are two types of tool compensation memories, types I and II, used to set and select the tool compensation amount. (The type used is determined by the MTB specifications.) Each of types I and II can be changed to type III depending on the MTB settings (parameter "#1046 T-ofs disp type"). If the tool compensation memory is changed to type III, you can register the tool compensation amount of the base axes I, J, and K and the tool tip point, enabling tool compensation for a turning tool. The details of type III are also displayed on the screen. If the tool compensation memory is reset to the original type, the turning tool compensation items are not displayed. However, when it is changed to type III, the previously registered data is displayed.
The compensation amount settings are preset with the setting and display unit.
Type I is selected when parameter "#1037 cmdtyp" is set to "1", and type II is selected when set to "2".
(*1) Distinguished between tool length compensation and tool nose radius compensation.
Tool compensation memory
Type of tool compensation memo- ry
Classification of length compen- sation, radius compensation
Classification of shape compen- sation, wear compensation
Type I No No Type II Yes Yes Type III (*1) Yes
Basic point
Basic tool
Tool length com- pensation
Shape
Wear amount
Tool radius compensation Shape Wear amount
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
268IB-1501277-P
Type I
One compensation amount corresponds to one compensation No. as shown below. Thus, these can be used commonly regardless of the tool length compensation amount, tool radius compensation amount, shape com- pensation amount and wear compensation amount. (D1) = a1 , (H1) = a1 (D2) = a2 , (H2) = a2 : : (Dn) = an , (Hn) = an
If the tool compensation type is changed from type I to type III, the tool compensation amount of type I is handled as tool length Z of type III.
Type II
The shape compensation amount related to the tool length, wear compensation amount, shape compensation related to the tool radius and the wear compensation amount can be set independently for one compensation No. as shown below. The tool length compensation amount is set with H, and the tool radius compensation amount with D. (H1) = b1 + c1 , (D1) = d1 + e1 (H2) = b2 + c2 , (D2) = d2 + e2 : : (Hn) = bn + cn , (Dn) = dn + en
If the tool compensation type is changed from type II to type III, data registered for type II is handled as the fol- lowing data.
Compensation No. Compensation amount
1 a1 2 a2 3 a3 : : : : n an
Compensation No. Tool length (H) Tool radius (D)/(Position compensation)
Shape compensa- tion amount
Wear compensa- tion amount
Shape compensa- tion amount
Wear compensation amount
1 b1 c1 d1 e1 2 b2 c2 d2 e2 3 b3 c3 d3 e3 : : : : : : : : : : n bn cn dn en
Type II Type III
Length dimension Tool length Z Length wear Z wear Radius dimension Tool nose R Radius wear R wear
CAUTION
If the tool compensation amount is changed during automatic operation (including during single block stop), it
will be validated from the next block or multiple blocks onwards.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
269 IB-1501277-P
This address designates the tool compensation No.
(1) H is used for the tool length compensation, and D is used for the tool position compensation and tool radius com- pensation.
(2) The tool compensation No. that is designated once does not change until a new H or D is designated. (3) The compensation No. can be commanded once in each block. (If two or more Nos. are commanded, the latter
one will be valid.) (4) For 40 sets:
Designate with the H01 to H40 (D01 to D40) numbers. (5) If a value larger than this is set, the program error (P170) will occur. (6) The setting value ranges are as follows for each No.
The compensation amount for each compensation No. is preset with the setting and display unit.
Tool compensation No. (H/D)
Setting Shape compensation amount Wear compensation amount
Metric system Inch system Metric system Inch system
#1003=B 999.999 (mm) 99.9999 (inch) 999.999 (mm) 99.9999 (inch) #1003=C 999.9999 (mm) 99.99999 (inch) 999.9999 (mm) 99.99999 (inch) #1003=D 999.99999 (mm) 99.999999 (inch) 999.99999 (mm) 99.999999 (inch) #1003=E 999.999999 (mm) 99.9999999 (inch) 999.999999 (mm) 99.9999999 (inch)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
270IB-1501277-P
12.1.2 Number of Tool Offset Sets Allocation to Part Systems
The number of tool offset sets can be set per part system. This function is divided into the following methods and which one is used depends on the MTB specifications (pa- rameters "#1438 Ofs-SysAssign", "#12054 Tol-Ofsnum").
Arbitrary allocation: Arbitrarily allocates to each part system. Fixed allocation: Automatically and evenly allocates to each part system.
The arbitrary allocation enables the efficient allocation because when a certain part system needs only a small num- ber of offset sets, the rest can be allocated to another part system. If an auxiliary-axis part system does not need the tool offset set at all, the number of tool offset sets can be set to "0" for the auxiliary-axis part system. While this function is available if the specification allows allocation by tool compensation memory part system, this parameter depends on the MTB specification parameter "#1051 MemTol"). Subsequent description is an example in the case where the number of tool offset sets in the system is 999. Number of tool offset sets in system is the total number of tool offset sets of all part systems.
(1) Arbitrary allocation (with #1438=1) The number of tool offset sets allocated to each part system depends on the MTB specifications (parameter "#12054 Tol-ofsnum"). (a) When the number of tool offset sets is increased for the 1st part system of 4-part system
(b) When the number of offset sets is set to "0 sets" for the 3rd part system to use the 3rd part system as auxiliary- axis part system
(2) Fixed allocation (with #1438=0)
(*1) The maximum number of tool offset sets per part system is 999.
(*2) If there is any remainder, the remainder sets are allocated to the 1st part system.
Function and purpose
(Lathe system only) (Lathe system only)
250
250
250
250
200
200
200
400 $1
$2
$3
$4
$1
$2
$3
$4
334
333
333 500
0
500 $1
$2
$3
$1
$2
$3
500
333
333 500
334
999
250
250
250
250
$1
$2
$3
$1
$2
$1
$1
$2
$3
$4
(*2)
(*1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
271 IB-1501277-P
(1) The maximum number of tool offset sets for 1-part system is 999. (2) For 1-part system, up to the number of tool offset sets in the system is available regardless of the parameter
setting. (3) When the value of the parameter "#12054 Tol-Ofsnum" (the number of tool offset sets by arbitrary allocation) is
equal to or below the number of tool offset sets in the system, the remainder is not allocated to any part system even if the specification allows arbitrary allocation.
(4) When the tool compensation memory is provided commonly for the part systems ("#1051 MemTol"=1), the num- ber of tool offset sets in the system are commonly used by all part systems regardless of the parameter setting. The setting of parameter #1051 depends on the MTB specifications, so check it in your machine specifications.
(5) Even if the specification allows arbitrary allocation, fixed allocation is applied if the parameter is "#12054 Tol- Ofsnum"= 0.
(6) When entering offset data, if the number of offset data exceeds that of current tool offset sets, the excess offset data cannot be entered.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
272IB-1501277-P
12.2 Tool Length Compensation/Cancel; G43, G44 / G49
The end position of the movement command for each axis can be compensated for by the preset amount when this command is issued. A continuity can be applied to the program by setting the actual deviation from the tool length value decided during programming as the compensation amount using this function.
Function and purpose
Command format
Tool length compensation start
G43 Zz Hh ; (+ direction)
G44 Zz Hh ; (- direction)
Tool length compensation cancel
G49 Zz ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
273 IB-1501277-P
The movement amount is calculated with the following expressions when the G43 or G44 tool length compensation command or G49 tool length compensation cancel command is issued.
lh1; Compensation amount for compensation No. h1
Regardless of the absolute command or incremental command, the actual end point will be the point compensated for by the compensation amount designated for the programmed movement command end point coordinate value.
The G49 (tool length compensation cancel) mode is entered when the power is turned ON or when M02 has been executed.
Detailed description
Tool length compensation movement amount
Z axis movement amount Operation
G43 Zz Hh1; z + (lh1) Compensation in + direction by tool compensation amount G44 Zz Hh1; z - (lh1) Compensation in - direction by tool compensation amount G49 Zz; z - (+) (lh1) Compensation amount cancel
(Example 1) For absolute command H01 = -100000 N1 G28 Z0 T01 M06 ; N2 G90 G92 Z0 ; N3 G43 Z5000 H01 ; N4 G01 Z-50000 F500 ;
(Example 2) For incremental command H01 = -100000 N1 G28 Z0 T01 M06 ; N2 G91 G92 Z0 ; N3 G43 Z5000 H01 ; N4 G01 Z-55000 F500 ;
Tool length compensation H01=-100.
R
5.000
0 W
50.000
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
274IB-1501277-P
(1) The compensation amount differs according to the compensation type. The following example shows a case in which "G43 Hh1;" is commanded.
(2) The valid range of the compensation No. will differ according to the specifications (No. of compensation sets). (3) If the commanded compensation No. exceeds the specification range, the program error (P170) will occur. (4) Tool length cancel will be applied when H0 is designated. (5) The compensation No. commanded in the same block as G43 or G44 will be valid for the following modals.
(Example 3)
(6) If G43 is commanded in the G43 modal, a compensation of the difference between the compensation No. data will be executed. (Example 4)
The same applies for the G44 command in the G44 modal.
Compensation No.
Type I The compensation amount lh1 commanded with compensation No. h1 will be applied commonly regardless of the tool length compen- sation amount, tool radius compensation amount, shape compen- sation amount or wear compensation amount.
Type II The compensation amount lh1 commanded with compensation No. h1 is as follows.
lh1: Shape compensation (b) + wear compensation amount (a)
Type III The compensation amount lh1 commanded with compensation No. h1 is as follows. (Refer to the figure of type II.) lh1: Tool length compensation amount in Z axis direction (b) + Wear compensation amount in Z axis report (a)
G43 Zz1 Hh1 ; Tool length compensation is executed with h1. : G45 Xx1 Yy1 Hh6 ; : G49 Zz2 ; Tool length compensation is canceled. : G43 Zz2 ; Tool length compensation is re-executed with h1. :
G43 Zz1 Hh1 ; The axis moves by "z1 + (lh1)". : G43 Zz2 Hh2 ; The axis moves by "z2 + (lh2 - lh1)". :
l h1
R
l h1
R
(a)
(b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
275 IB-1501277-P
(1) When parameter "#1080 Dril_Z" is set to "1", the tool length compensation is always applied to the Z axis. (2) When parameter "#1080 Dril_Z" is set to "0", the axis will depend on the axis address commanded in the same
block as G43. The order of priority is shown below. Zp > Yp > Xp (Example 5)
The handling of the additional axis will follow the parameters "#1029 aux_I" to "1031 aux_K" settings. If the tool length compensation is commanded for the rotary axis, set the rotary axis name for one of the parallel axes.
(3) If H (compensation No.) is not designated in the same block as G43, the Z axis will be valid. (Example 6)
(1) If reference position return is executed with G28 and manual operation, the tool length compensation will be can- celed when the reference position return is completed. (Example 7)
(2) The movement is commanded to the G53 machine coordinate system, the axis will move to the machine position without tool compensation amount. When the G54 to G59 workpiece coordinate system is returned to, the position returned to will be the coordinates shifted by the tool compensation amount.
Axis valid for tool length compensation
G43 Xx1 Hh1; + compensation to X axis : G49 Xx2 ; : G44 Yy1Hh2; - compensation to Y axis : G49 Yy2 ; : G43 1 Hh3; + compensation to additional axis : G49 1 ; : G43 Xx3Yy3Zz3 ; Compensation is applied on Z axis. : G49 ;
G43 Hh1 ; Compensation and cancel to Z axis : G49 ; :
Movement during other commands in tool length compensation modal
G43 Zz1 Hh1 ; : G28 Zz2 ; Canceled when reference position is reached. (Same as G49) : G43 Zz2Hh2 ; : G49 G28Zz2 ; The tool length compensation will be included when positioning the intermediate point.
Canceled when reference position is reached.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
276IB-1501277-P
When there is no movement command in the same block where the tool length offset start (G43 or G44) or the tool length offset cancel (G49) is commanded, the movement by the compensation amount may not be carried out de- pending on the MTB specifications (parameter "#1247 set19/bit0" (movement by tool length compensation com- mand)).
(1) For the G49 command, command it at a safe position where the tool does not interfere with the machine in con- sideration of the compensation canceling operation. When the parameter "#1247 set19/bit0" is set to "0", the axis moves to the position where the compensation was canceled even though there is no axis command in the G49 command block.
Movement by tool length compensation command
G43/G44/G49 Not move by the offset amounts (#1247/bit0 = 1)
Moves by the offset amounts (#1247/bit0 = 0)
Without move- ment com- mands
: G54 A0. C0. ; G68.2 ; G53.1 ; G00XxYyZz ; G43H1 ; : G49 ;
: G54 A0. C0. ; G68.2 ; G53.1 ; G00XxYyZz ; G43H1 ; : G49 ;
If tool position compensation is commanded alone in a block, the axis does not move, but the tool compen- sation amount is applied to the program position counter.
If tool position compensation is commanded alone in a block, the axis moves by the tool length compensation amount.
With move- ment com- mands
: G54 A0. C0. ; G68.2 ; G53.1 ; G00XxYyZz ; G43H1Z0 ; : G49Z10. ;
: G54 A0. C0. ; G68.2 ; G53.1 ; G00XxYyZz ; G43H1Z0 ; : G49Z10. ;
If tool length compensation is commanded with movement commands, the axis moves by the tool length compensation amount.
If tool length compensation is commanded with move- ment commands, the axis moves by the tool length compensation amount.
Mx
MyMz
G43 G49
Positioning
Cutting
Machine coordinate system
Mx
My Mz
G43 G49
Positioning
Cutting
Machine coordinate system
Mx
My Mz
G43 G49
Positioning
Cutting
Machine coordinate system
Mx
My Mz
G43 G49
Positioning
Cutting
Machine coordinate system
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
277 IB-1501277-P
Tool length compensation method for multiple axis synchronization control depends on the MTB specifications (pa- rameter "#1255 set27/bit5"). When "#1255 set27/bit5" is set to "1
Tool length compensation for multiple axis synchronization control is enabled and different amount of tool length compensation for each axis can be applied to the target axis for multiple axis synchronization control. Even when the tool with different length for each head is mounted with multi head configuration machine, the different amount of tool length compensation can be applied to each head and the tool length error between heads can be compensated.
When "#1255 set27/bit5" is set to "0 Tool length compensation for multiple axis synchronization control is disabled and the same tool length com- pensation amount as the master axis is applied to the slave axis.
[Operation of tool length compensation]
With tool length compensation for multiple axis synchronization control, the tool compensation amount of difference tool compensation No. can be applied to each axis. Tool compensation amount of the tool compensation No. which the value of the "2675 tcmp_top" added to commanded No.is applied.
Tool length compensation for multiple axis synchronization control is applicable only to axes which are actually in the synchronized state. Therefore, the axis where the bit of PLC signal Synchronization control operation method signal (R2589) is turned OFF is not the target for tool length compensation.
Tool length compensation for multiple axis synchronization control is started with G43, G44 command in the same way as the normal tool length compensation. To cancel the tool length compensation, command G49 in the same way as the normal tool length compensation.
With tool length compensation for multiple axis synchronization control, the movement is performed for the amount of tool length compensation in G43, G44, G49 commanded blocks. With tool length compensation for multiple axis synchronization control, the parameter setting "#1247 set19/bit0" is disabled. However, if the target axis for tool length compensation is not the target axis for multiple axis synchronization control, the parameter setting "#1247 set19/bit0" is reflected.
If H0 is commanded in G43, G44 commanded blocks, "0" is applied to the compensation amount value of the axis where "#2675 tcmp_top" is set to "0", and the tool compensation amount value of the tool compensation No. corre- sponding to the parameter setting value is applied to the axis where"#2675 tcmp_top" is set to other than "0".
The following shows the example conditions for the system with XYZUVW axis configuration. Set the parameter so that Z axis is the master, U and Z axes are the slave axes. The machine position when the multiple axis synchronization control is started is the same on master and slave
axes. Mount the tools with different length. Other settings are as below. Setting values of the parameter "#2675 tcmp_top
Z axis: 0 U axis: 20 V axis: 33
Setting values of tool compensation amount Compensation No. 5: 20.0 mm Compensation No. 25: 27.0 mm Compensation No. 38: 35.0 mm
Tool length compensation command G44 H5
Tool length compensation of multiple axis synchronization control function
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
278IB-1501277-P
(1) When "#1255 set27/bit5" is set to "0" As the same tool length compensation amount as the master axis is applied to the slave axis, 20.0 mm compen- sation of the compensation No. 5 is applied to Z, U and V axes. Tool compensation amount setting screen
Z axis U axis V axis Z axis U axis V axis
Before tool length compensation After tool length compensation
20.0mm
20.0mm
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
279 IB-1501277-P
(2) When "#1255 set27/bit5" is set to "1" Independent tool length compensation amount is applied to master and slave axes. For the master and slave axes, the tool compensation amount of the tool compensation No. where "5" is added to the No. specified with the parameter "#2675 tcmp_top" is applied; therefore, the tool compensation amount No. 5 is applied to Z axis, No. 25 is applied to U axis and No. 38 is applied to V axis. Tool compensation amount setting screen
Z axis U axis V axis Z axis U axis V axis
Before tool length compensation After tool length compensation
35.0mm27.0mm20.0mm
35.0mm 27.0mm20.0mm
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
280IB-1501277-P
12.3 Tool Radius Compensation; G38,G39/G40/G41,G42
This function compensates the radius of the tool. The compensation can be done in the random vector direction by the radius amount of the tool selected with the G command (G38 to G42) and the D command. When using tool nose radius compensation, refer to "12.4 Tool Nose Radius Compensation (for Machining Center System)".
The number of sets for the compensation differ according to machine specification. (The No. of sets is the total of the tool length offset, tool position offset and tool radius compensation sets.) The H command is ignored during the tool radius compensation, and only the D command is valid. The compensation will be executed within the plane designated with the plane selection G code or axis address 2 axis, and axes other than those included in the designated plane and the axes parallel to the designated plane will not be affected. Refer to the section on plane selection for details on selecting the plane with the G code.
Function and purpose
Command format
G40 X__Y__; Tool radius compensation cancel
G41 X__Y__ D__; Tool radius compensation (Left)
G42 X__Y__ D__; Tool radius compensation (Right)
G38 I__J__; Change or hold of compensation vector (Can be commanded only during the radius compensation mode.)
G39 X__Y__; Corner changeover (Can be commanded only during the radius compensa- tion mode.)
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
281 IB-1501277-P
12.3.1 Tool Radius Compensation Operation
The tool radius compensation cancel mode is established by any of the following conditions.
(1) After the power has been switched on (2) After the reset button on the setting and display unit has been pressed (3) After the M02 or M30 command with reset function has been executed (4) After the compensation cancel command (G40) is issued
The compensation vectors are zero in the compensation cancel mode, and the tool nose point path coincides with the programmed path. Programs including tool radius compensation must be terminated in the compensation cancel mode.
Tool radius compensation starts when all the following conditions are met in the compensation cancel mode.
(1) The movement command is issued after G41 or G42. (2) The tool radius compensation offset No. is 0 < D <= max. offset No. (3) The movement command of positioning (G00) or linear interpolation (G01) is issued.
Whether in continuous or single block operation, compensation always starts after reading three blocks, or if the three blocks do not contain any movement command, up to five continuous blocks will be pre-read. In compensation mode, too, up to 5 blocks are pre-read and the compensation is arithmetically processed.
There are two ways of starting the compensation operation: type A and type B. The type depends on the setting of the parameter "#8157 Radius comp type B". This type is used in common with the compensation cancel type.
Detailed description
Tool radius compensation cancel mode
Tool radius compensation start (startup)
[Control state diagram]
Execution block Pre-read Buffer
After pre-reading G41, start pre-reading Max. 5 blocks
N16 G02_; N15 G01_; N14 G41_; N13 G00_; N12 S_; N11 T_;
N16 G02_; N15 G01_; N14 G41_; N13 G00_; N12 S_; N11 T_;
N16 G02_; N15 G01_;
N16 G02_; N15 G01_; N14 G41_; N13 G00_; N12 S_; N11 T_;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
282IB-1501277-P
(1) Machining an inside corner
(2) Machining an outside corner (obtuse angle) [90 <= < 180]
Start operation for tool radius compensation
Linear -> Linear Linear -> Circular
(S) Start point (CP) Center of circular r : Compensation amount s: Stop point with single block
Program path Tool center path
Linear -> Linear (Type A) Linear -> Circular (Type A)
Linear -> Linear (Type B) Linear -> Circular (Type B)
(S) Start point (CP) Center of circular r : Compensation amount s: Stop point with single block
Program path Tool center path
G42
s
(S)
r
s
G42
r
(S) (CP)
G41 r
s
(S)
G41
r
s
(S) (CP)
G41
r r
s
(S)
G41
r r
s
(S) (CP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
283 IB-1501277-P
(3) Machining an outside corner (acute angle) [ < 90]
If there is no axis movement command in the same block as G41 or G42, compensation is performed perpen- dicularly to the next block's direction.
Calculate the tool center path from the linear line/circular arc to perform compensation to the program path (G00, G01, G02, G03). Even if the same compensation command (G41, G42) is issued in the compensation mode, the command will be ignored. When 4 or more blocks without movement command are continuously specified in the compensation mode, over- cutting or undercutting will occur. When the M00 command has been issued during tool radius compensation, pre-reading is prohibited.
Linear -> Linear (Type A) Linear -> Circular (Type A)
Linear -> Linear (Type B) Linear -> Circular (Type B)
(S) Start point (CP) Center of circular r : Compensation amount s: Stop point with single block
Program path Tool center path
Operation in compensation mode
G41
r
s
(S) G41
r
s
(S)
(CP)
G41
r
r
s
(S)
G41
r
r
s
(S)
(CP)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
284IB-1501277-P
(1) Machining an outside corner Linear -> Linear (90<= < 180) Linear -> Linear (0 < < 90)
Linear -> Circular (90 <= < 180) Linear -> Circular (0 < < 90)
Circular -> Linear (90 <= < 180) Circular -> Linear (0 < < 90)
Circular -> Circular (90 <= < 180) Circular -> Circular (0 < < 90)
(CP) Center of circular r : Compensation amount s : Single block stop point
Program path Tool center path
s
r
r
s
s
r r
(CP)
r
r
s
(CP)
r r
s
(CP)
r
r
s
(CP)
r r
s
(CP)
(CP)
r r
s (CP) (CP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
285 IB-1501277-P
(2) Machining an inside corner Linear -> Linear (Obtuse angle) Linear -> Linear (Acute angle)
Linear -> Circular (Obtuse angle) Linear -> Circular (Acute angle)
Circular -> Linear (Obtuse angle) Circular -> Linear (Acute angle)
Circular -> Circular (Obtuse angle) Circular -> Circular (Acute angle)
(CP) Center of circular r : Compensation amount s : Single block stop point
Program path Tool center path
r
s
r
r s
r
s
(CP)
r
r
s
(CP)
r s
(CP)
r
s
(CP)
r
s
(CP)(CP)
r
s
(CP)
(CP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
286IB-1501277-P
(3) When the circular end point is not on the circular Spiral circular command ... The area from the arc start point to the end point is interpolated as a spiral arc. Normal circular command If the error after compensation is within the parameter value ("#1084 RadErr"), it is interpolated as a spiral arc.
(4) When the inner intersection point does not exist In cases like the figure below, the intersection point of circulars A and B may not exist depending on the com- pensation amount. In such cases, program error (P152) appears and the tool stops at the end point of the previous block. In the pattern 1 and 2 in this figure, machining is possible because compensation amount r is small. In pattern 3, compensation r is so large that an intersection does not exist and program error (P152) will occur.
(E) End point of circular (CP) Center of circular r : Compensation amount
(CP) Center of circular A r : Compensation amount
Program path Tool center path
r
r s
R
(E)
(CP)
r
r
A B
P152 (CP)
3
2 1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
287 IB-1501277-P
Tool radius compensation cancel If either of the following conditions is met in the tool radius compensation mode, the compensation will be canceled. However, there must be any movement command except a circular command. If the compensation is canceled by a circular command, program error (P151) will occur.
(1) The G40 command has been executed. (2) Executed the compensation No.D00.
The cancel mode is established once the compensation cancel command has been read, 5-block pre-reading is sus- pended and 1-block pre-reading will be operated.
(1) Machining an inside corner
Tool radius compensation cancel
Tool radius compensation cancel operation
Linear -> Linear Circular -> Linear
(E) End point (CP) Center of circular r : Compensation amount s : Single block stop point
Program path Tool center path
r
s
G40
(E)
G40
r
s
(CP) (E)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
288IB-1501277-P
(2) Machining an outside corner (obtuse angle) [90 <= < 180] Linear -> Linear (Type A) Circular -> Linear (Type A)
Linear -> Linear (Type B) Circular -> Linear (Type B)
(E) End point (CP) Center of circular r : Compensation amount s : Single block stop point
Program path Tool center path
r
s
G40
(E)
G40
r
s
(CP) (E)
r
s
G40
r
(E)
G40
r
s
r
(CP) (E)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
289 IB-1501277-P
(3) Machining an outside corner (acute angle) [ < 90] Linear -> Linear (Type A) Circular -> Linear (Type A)
Linear -> Linear (Type B) Circular -> Linear (Type B)
(E) End point (CP) Center of circular r : Compensation amount s : Single block stop point
Program path Tool center path
r
s
G40
(E)
s
G40
r
(CP)
(E)
r
s
G40
r
(E)
r
s
G40
r
(E)
(CP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
290IB-1501277-P
12.3.2 Other Commands and Operations during Tool Radius Compensation
An arc that uses the compensation amount as the radius is inserted without calculating the point of intersection at the workpiece corner when G39 (corner arc) is commanded.
Detailed description
Insertion of corner arc
(With G39 com- mand)
(No G39 com- mand)
(With G39 com- mand)
(No G39 com- mand)
[For outer side compensation] [For inner side compensation]
(a) Inserted circular (b) Point of intersection r : Compensation amount
s: Stop point with single block
N1 G28 X0 Y0 ; N2 G91 G01 G42 X20. Y20. D1 F100 ; N3 G39 X40. ; N4 G39 Y40. ; N5 G39 X-40. ; N6 Y-40. ; N7 G40 X-20. Y-20. ; N8 M02 ;
Programmed path
Tool center path
s(a) (b)
r s
(a)
(b)
r
N2
N1
D1=5.000
N3
N4
N5
N6
N7
Y
X
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
291 IB-1501277-P
The compensation vector can be changed or held during tool radius compensation by using the G38 command.
(1) Holding of vector
When G38 is commanded in a block having a movement command, the point of intersection will not be calculated at the program end point, and instead the vector of the previous block will be held.
G38 Xx Yy;
This can be used for pick feed, etc.
Changing and holding of compensation vector
[Holding the inside compensation vector]
N11 G01 Xx11 ; N12 G38 Xx12 Yy12 ; N13 G40 Xx13 ;
r1: Vector at N11-N12 block intersection calculation
[Holding the outside compensation acute angle]
N11 G01 Xx11 Yy11 ; N12 G38 Xx12 Yy12 ; N13 G40 Xx13 ;
r1: Vector at N11-N12 block intersection calculation
[Holding the outside compensation obtuse angle]
N11 G01 Xx11 Yy11 ; N12 G38 Xx12 Yy12 ; N13 G40 Xx13 ;
r1: Vector at N11-N12 block intersection calculation
Programmed path
Tool center path
N11
N12
N13
r1
r1
N11 N12
N13
r1
r1
N11 N12
N13
r1
r1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
292IB-1501277-P
(2) Changing of vector A new compensation vector direction can be commanded with I, J and K, and a new compensation amount with D.
(These can be commanded in the same block as the movement command.)
G38 Ii Jj Dd ; (I, J and K will differ according to the selected plane.)
The compensation amount d vector is created in the commanded i and j vector direction.
If G38 is commanded in the same block as the circular block (G02/G03) I and J commands, I and J will be han- dled as the G38 vector, and an error will occur.
N11 G01 Xx11 ; N12 Yy12 ; N13 G38 Xx13 Ii Jj Dd ; N14 G40 Xx14 Yy14 ;
Programmed path
Tool center path
N13
N12
N11
i
j
N14
d d
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
293 IB-1501277-P
The compensation direction is determined by the tool radius compensation commands (G41, G42) and compensa- tion amount sign.
The compensation direction can be changed by changing the compensation command during the compensation mode without canceling the mode. However, it is impossible to change the direction in the compensation start block and the next block.
(1) Linear -> Linear (a) When there is an intersection (A) at the change of compensation direction (b) When there is no intersection at the change of compensation direction
(2) Linear <-> Circular (a) When there is a point of intersection (A) when the compensation direction is changed. (b) When there is no point of intersection when the compensation direction is changed.
Changing the compensation direction during tool radius compensation
G Code Compensation amount sign + Compensation amount sign -
G41 Left-side compensation Right-side compensation G42 Right-side compensation Left-side compensation
Program path Tool center path
r
G41
r
G41 G42
r
r
(a)
(b)
A
r
G41
r
G41 G42G41G42
r
r
r
r
A
(b)
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
294IB-1501277-P
(3) Circular -> Circular (a) When there is an intersection at the change of compensation direction (b) When there is no intersection at the change of compensation direction
(4) Linear return
(5) When the compensation direction is switched using G41/G42, it is possible that the arc may exceed 360. If the arc exceeds 360, compensation will be performed as shown in the figure and uncut section will be left.
(CP) Center of circular
: G42 G01 X_ Y_; G41 G02 X_ Y_ I_ J_; G42 G01 X_ Y_; :
Program path Tool center path
Section left uncut
G42G41G41
G41
G41
G42
(CP)
(CP)
(a)
(b) r
r
r
G41
G42 r
G41
G42
G42
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
295 IB-1501277-P
When the following command is issued in the compensation mode, the compensation vectors are temporarily elim- inated and then, compensation mode will automatically return. In this case, the compensation is not canceled, and the tool goes directly from the intersection point vector to the point without vectors, in other words, to the programmed command point. When returning to the compensation mode, it goes directly to the intersection point.
(1) Reference position return command Temporarily no compensation vectors at intermediate point. (Reference position when there is no intermediate point).
(2) The compensation vector will be eliminated temporarily with the G53 command (Basic machine coordinate sys- tem selection).
(3) G33 thread cutting command Tool radius compensation does not apply to the G33 block.
Command for eliminating compensation vectors temporarily
(G41) : (CP) Intermediate point N5 G91 G01 X60. Y30. ; N6 G28 X50. Y-40. ; Temporarily no compensation vectors at intermediate
point. (Reference position when there is no intermediate point)
N7 X30. Y-60. ; N8 X70. Y40. ;
:
(CP)
N6N5
S
S
S
N8 N7
r
G33
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
296IB-1501277-P
The following blocks are known as blocks without movement.
M00, M01, M02 and M30 are handled as pre-read inhibit M codes.
(1) When command is assigned at start of the compensation Compensation vector cannot be created when there are four or more successive blocks without movement, or when pre-reading prohibiting M command is issued.
Blocks without movement
M03 ; M command S12 ; S command T45 ; T command G04X500 ; Dwell G22 X200. Y150. Z100 ; Machining prohibited region setting G10 L10; P01 R50; Compensation amount setting G92 X600. Y400. Z500. Coordinate system setting (G17) Z40. Movement outside the compensation plane G90 ; G code only G91 X0; Movement amount 0
N1 X30.Y60 ; N2 G41 D10 ;
Block without movement N3 G04 X1000 ; N4 F100 ; N5 S500 ; N6 M3 ; N7 X20.Y-50. ; N8 X50.Y-20. ;
N1
N2, 3, 4, 5, 6
N7
N8
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
297 IB-1501277-P
(2) When command is assigned in the compensation mode Compensation vector will be created as normal when there are not four or more successive blocks without move- ment, or when pre-read prohibiting M command is not issued.
Block N7 is executed at N7 in the figure.
Compensation vector will be created perpendicularly to the end point of the previous block when there are four or more successive blocks without movement, or when pre-read prohibiting M command is issued. In this case, a cut may occur.
(3) When commanded together with compensation cancel Only the compensation vectors are canceled when a block without movement is commanded together with the G40 command.
N6 G91 X100. Y200. ; N7 G04 X1000; ... Block without movement N8 X200. ;
N6 X100. Y200. ; N7 G04 X1000 ;
Block without movement N8 F100 ; N9 S500 ; N10 M4 ; N11 X100. ;
N6 X100. Y200. ; N7 G40 M5 ; N8 X100. Y50. ;
N8N7
N6
N7 N10
N6
N11
N6
N7
N8
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
298IB-1501277-P
(1) If the final movement command block in the four blocks before the G40 block is the G41 or G42 mode, it will be assumed that the movement is commanded in the vector I, J or K direction from the end point of the final move- ment command. After interpolating between the hypothetical tool center path and point of intersection, it will be canceled. The compensation direction will not change.
In this case, the point of intersection will always be obtained, regardless of the compensation direction, even when the commanded vector is incorrect as shown below.
[When the I and J symbols in the above program example are incorrect]
If the compensation vector obtained via a point of intersection calculation is extremely large, a perpendicular vec- tor will be created in the block before G40.
When I, J, K are commanded in G40
N1 (G41) G01 X_ ; N2 G40 Xa Yb Ii Jj ;
Program path
Tool center path
Hypothetical tool center path
r N1
(i,j) N2 A
(a,b)
rG41
rN1
(i,j)
N2
A
(a,b)
r
G41
r
G40
(i,j)
A
(a,b)
r
G41
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
299 IB-1501277-P
(2) If the arc is 360 or more due to the details of I, J and K at G40 after the arc command, an uncut section will occur.
When a multiple number of compensation vectors are created at the joints between movement command blocks, the tool will move in a straight line between these vectors. This action is called corner movement. When the vectors do not coincide, the tool moves in order to machine the corner although this movement is part and parcel of the joint block. Consequently, operation in the single block mode will execute the previous block + corner movement as a single block and the remaining joining movement + following block will be executed as a single block in the following op- eration.
N1 (G42,G91) G01 X200. ; N2 G03 J150.; N3 G40 G01 X150. Y-150. I-100. J100. ;
Programmed path
Tool center path
Section left uncut
Corner movement
(CP) Center of circular r: Compensation amount s: Single block stop point
Programmed path Tool center path
r
N1
(i,j)
N2
r
G42
r
G40 N3
r
N1
N2
r
s
(CP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
300IB-1501277-P
12.3.3 G41/G42 Commands and I, J, K Designation
The compensation direction can be intentionally changed by issuing the G41/G42 command and I, J, K in the same block.
Assign a linear command (G00, G01) in a movement mode.
This section describes the new I,J type vectors (G17 plane) created by this command. (Similar descriptions apply to vector K, I for the G18 plane and to J, K for the G19 plane.) As shown in the following figures, I, J type vectors create compensation vectors which are perpendicular to the di- rection designated by I, J and equivalent to the compensation amount, without the intersection point calculation of the programmed path. The I, J vectors can be commanded even in the mode (G41/G42 mode in the block before) and even at the compensation start (G40 mode in the block before).
(1) When I, J is commanded at compensation start
Function and purpose
Command format
G17 (X-Y plane) G41/G42 X__ Y__ I__ J__ ;
G18 (Z-X plane) G41/G42 X__ Z__ I__ K__ ;
G19 (Y-Z plane) G41/G42 Y__ Z__ J__ K__ ;
Detailed description
I, J type vectors (G17 X-Y plane selection)
Program path
Tool center path
(G40)
N100 G91 G41 X100. Y100. I150. D1 ;
N110 G04 X1000 ;
N120 G01 F1000 ;
N130 S500 ;
N140 M03 ;
N150 X150. ;
N150
N100
Y
X
N110 N120 N130 N140
D1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
301 IB-1501277-P
(2) When there are no movement commands at the compensation start.
(3) When I, J has been commanded in the G41/42 mode (G17 plane)
Program path
Tool center path
(a) I, J type vector (b) Intersection point calculation type vector
Program path
Tool center path
Path after intersection point calculation
(G40)
N1 G41 I150. D1 ;
N2 G91 X100. Y100. ;
N3 X150. ;
N3
N2
Y
X
D1 N1
(G17 G41 G91)
N100 G41 G00 X150. J50. ;
N110 G02 I150. ;
N120 G00 X- 150. ;(N120)
N100
Y
X
N120
( I ,J)N110
D1
(a) (b)
(b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
302IB-1501277-P
(Reference)
(a) G18 plane
(b) G19 plane
(4) When I, J has been commanded in a block without movement
(G18 G41 G91)
N100 G41 G00 Z150. I50. ;
N110 G02 K50. ;
N120 G00 Z - 150. ; (N120)
N100
Z
X
N120
(K,I) N110
(G19 G41 G91)
N100 G41 G00 Y150. K50. ;
N110 G02 J50. ;
N120 G00 Y - 150. ; (N120)
N100
Z
Y
N120
(J,K) N110
N1 G41 D1 G01 F1000 ;
N2 G91 X100. Y100. ;
N3 G41 I50. ;
N4 X150. ;
N5 G40 ;
N3
N2
D1
N1
N4
(I,J) N5
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
303 IB-1501277-P
(1) In G41 mode
Direction produced by rotating the direction commanded by I,J by 90 to the left when looking at the zero point from the forward direction of the Z axis (3rd axis).
(2) In G42 mode
Direction produced by rotating the direction commanded by I, J by 90 to the right when looking at the zero point from the forward direction of the Z axis (3rd axis).
G41 and G42 modals can be switched over at any time.
Compensation vector direction
(Example 1) With I100. (Example 2) With I-100.
(100, 0) IJ direction (-100, 0) IJ direction
Compensation vector direction Compensation vector direction
(Example 1) With I100. (Example 2) With I-100.
(100, 0) IJ direction (-100, 0) IJ direction
Compensation vector direction Compensation vector direction
Selection of compensation modal
N1 G28 X0 Y0 ;
N2 G41 D1 F1000 ;
N3 G01 G91 X100. Y100. ;
N4 G42 X100. I100. J - 100.
D2 ;
N5 X100. Y- 100. ;
N6 G40 ;
N7 M02 ;
%
N3
x
D1 N2
N6
(I,J)
N5
y
N4 D2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
304IB-1501277-P
The compensation amount is determined by the offset No. (modal) in a block with the IJ designation.
(1) Issue the I, J type vector in a linear mode (G00, G01). If it is in an arc mode at the start of compensation, program error (P151) will occur. When it is in the compensation mode as well as in the arc mode, I, J will be designated at the center of the cir- cular.
(2) When the I,J type vector is designated, it will not be deleted (Interference avoidance) even if there is interference. Consequently, overcutting may occur. In the figure below, cutting will occur in the shaded section.
Compensation amount for compensation vectors
Precautions
(G41 D1 G91)
N100 G41 X150. I50. ;
N110 X100. Y- 100. ; X
N110
(I,J)
A
Y N100
D1 D1
(G41 D1 G91)
N200 G41 X150. I50. D2 ;
N210 X100. Y- 100. ;
X N210
(I,J)
B
Y N200
D2
D1
N1 G28 X0 Y0 ;
N2 G42 D1 F1000 ;
N3 G91 X100. ;
N4 G42 X100. Y100. I10. ;
N5 X100. Y - 100. ;
N6 G40 ;
N7 M02 ;
Y
X
N5
(I,J)
N4
N3
N2 N6
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
305 IB-1501277-P
(3) The vectors differ for the G38 I _J_ (K_) command and the G41/G42 I_J_(K_) command.
(4) Refer to the following table for the compensation methods depend on the presence or absence of G41/G42 com- mand and I, K, (J) command.
During the I, J type vector compensation, the A insertion block will not exist.
G38 G41/G42
Example : (G41)
: G38 G91 X100. I50. J50. ;
:
: (G41)
: G41 G91 X100. I50. J50. ;
:
Vector in IJ direction having a compensation amount (a) size
Vector perpendicular in IJ direction and having a compensation amount (b) size
G41/42 I, J (K) Compensation methods
No No Intersection point calculation type vector No Yes Intersection point calculation type vector Yes No Intersection point calculation type vector Yes Yes I, J, type vector
No insertion block
(I J)
(a) (I J)
(b)
Y
X N5
(I,J)
N4
N3
N2
N1
N1 G91 G01 G41 X200. D1 F1000 ; N2 X-150. Y150. ; N3 G41 X300. I50. ; N4 X-150. Y-150. ; N5 G40 X-200. ;
(A)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
306IB-1501277-P
12.3.4 Interrupts during Tool Radius Compensation
Tool radius compensation is valid in any automatic operation mode - whether tape, memory or MDI mode. The figure below shows what happens by MDI interruption after stopping the block during tape or memory mode. S in the figure indicates the stop position with single block.
(1) Interrupt without movement (tool path does not change)
(2) Interrupt with movement The compensation vectors are automatically re-calculated in the movement block after interrupt.
With linear interrupt
With circular interruption
Detailed description
MDI interruption
Automatic operation MDI interruption N1 G41 D1; N2 X20. Y50. ;
<--- S1000 M3; N3 G03 X40. Y-40. R70. ;
Automatic operation MDI interruption N1 G41 D1; N2 X20. Y50. ;
<--- X50. Y-30. ; X30. Y50. ;
N3 G03 X40.Y-40. R70. ;
Automatic operation MDI interruption N1 G41 D1; N2 X20. Y50. ;
<--- G02 X40. Y-40. R70. ; G01 X40. ;
N3 G03 X40. Y-40. R70. ;
N2
S
N3
S
S
N2
N3
S
S
N2 N3
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
307 IB-1501277-P
(1) Interrupt with manual absolute OFF. The tool path will deviate from the compensated path by the interrupt amount.
(2) Interrupt with manual absolute ON In the incremental mode, the same operation will be performed as the manual absolute OFF. In the absolute mode, however, the tool returns to its original path at the end point of the block following the in- terrupted block, as shown in the figure.
Manual interruption
Program path
Tool path after compensation
Interrupt (A)
Tool path after interrupt
[Line-Line-Line] [Line-arc-Line]
Program path
Tool path after compensation
Interrupt (A)
Tool path after interrupt
A
A A
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
308IB-1501277-P
12.3.5 General Precautions for Tool Radius Compensation
(1)The offset amounts can be designated with the D code by designating an offset amount No. Once designated, the D code is valid until another D code is commanded. If an H code is designated, the program error (P170) No COMP No will occur. Besides being used to designate the compensation amounts for tool radius compensation, the D codes are also used to designate the compensation amounts for tool position compensation.
(2) Compensation amounts are normally changed when a different tool has been selected in the compensation can- cel mode. However, when an amount is changed during the compensation mode, the vectors at the end point of the block are calculated using the compensation amount designated in that block.
If the compensation amount is negative (-), the figure will be the same as if G41 and G42 are interchanged. Thus, the axis that was rotating around the outer side of the workpiece will rotate around the inner side, and vice versa. An example is shown below. Normally, the compensation amount is programmed as positive (+). However, if the tool path center is programmed as shown in (a) and the compensation amount is set to be negative (-), the move- ment will be as shown in (b). On the other hand, if the program is created as shown in (b) and the offset amount is set to be negative (-), the movement will be as shown in (a). Thus, only one program is required to execute machin- ing of both male and female shapes. The tolerance for each shape can be randomly determined by adequately se- lecting the offset amount. (Note that a circle will be divided with type A when compensation is started or canceled.)
Precautions
Assigning the compensation amounts
Compensation amount symbols and tool center path
G41 offset amount (+) or G42 offset amount (-) (a)
G41 offset amount (-) or G42 offset amount (+) (b)
Tool center path
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
309 IB-1501277-P
12.3.6 Changing of Compensation No. during Compensation Mode
As a principle, the compensation No. must not be changed during the compensation mode. If changed, the move- ment will be as shown below.
When compensation No. (compensation amount) is changed: G41 G01 ........ Dr1 ; ( = 0,1,2,3) N101 G0 Xx1 Yy1 ; N102 G0 Xx2 Yy2 Dr2 ; ................................... Compensation No. changed N103 Xx3 Yy3 ;
Function and purpose
During linear -> linear
The compensation amount designated with N101 will be applied.
The compensation amount designated with N102 will be applied.
Program path
Tool center path
N101 r2
r2r1
r1 N102
N103
r1
r1
r1 r1
r2
r2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
310IB-1501277-P
Linear ->circular
(CP) Arc center
Program path
Tool center path
N101
N102 r1
r2
G02r1
N102
N101
G03
r1
r1
r1 r1
r2
(CP)
(CP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
311 IB-1501277-P
Circular -> circular
(CP) Arc center
Program path
Tool center path
r1 N101
r1 r2
N102
r1 r1
r1 r1
r2
(CP)
(CP)
(CP)
(CP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
312IB-1501277-P
12.3.7 Start of Tool Radius Compensation and Z Axis Cut in Operation
Often when starting cutting, a method of applying a radius compensation (normally the XY plane) beforehand at a position separated for the workpiece, and then cutting in with the Z axis is often used. When using this method, cre- ate the program so that the Z axis movement is divided into the two steps of rapid traverse and cutting feed after nearing the workpiece.
When the following type of program is created:
With this program, at the start of the N1 compensation the program will be read to the N6 block. The relation of N1 and N6 can be judged, and correct compensation can be executed as shown above.
If the above program's N4 block is divided into two
In this case, the four blocks N2 to N5 do not have a command in the XY plane, so when the N1 compensation is started, the program cannot be read to the N6 block. As a result, the compensation is done based only on the information in the N1 block, and the compensation vector is not created at the start of compensation. Thus, an excessive cut in occurs as shown above.
Function and purpose
Program example
N1 G91 G00 G41 X500. Y500. D1 ; N2 S1000 ; N3 M3 ; N4 G01 Z-300. F1 ; N6 Y100. F2 ; : :
N4 Z axis lowers (1 block)
Tool center path
N1 G91 G00 G41 X500. Y500. D1 ; N2 S1000 ; N3 M3 ; N4 Z-250. ; N5 G01 Z-50. F1 ; N6 Y100. F2 ;
(c) Cut in
N1 Y
X
N1 Y
Z
N4 N6 N6
N4
N1
N1
N4
N5N6
XX
Y Z
N6
(c)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
313 IB-1501277-P
In this case, consider the calculation of the inner side, and before the Z axis cutting, issue a command in the same direction as the direction that the Z axis advances in after lowering, to prevent excessive cutting.
The movement is correctly compensated as the same direction as the N6 advance direction is commanded in N2.
N1 G91 G00 G41 X500. Y400. D1 ; N2 Y100. S1000 ; N3 M3 ; N4 Z-250. ; N5 G01 Z-50. F1 ; N6 Y100. F2 ;
N1 Y
Z
N5
N6
N2
N1
N2
Y
X
N6 N6
N4
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
314IB-1501277-P
12.3.8 Interference Check
When tool radius is larger than the program path, a tool, compensated for by the tool radius compensation function, may sometimes cut into the workpiece. This is known as interference, and interference check is the function which prevents this from occurring. The table below shows the three functions of interference check and each can be selected for use by parameter.
When there is a movement command in three of the five pre-read blocks, and if the compensation calculation vectors which are created at the contacts of movement commands intersect each other, it will be viewed as interference.
Function and purpose
Function Parameters Operation
#8102 #8103
COLL. ALM OFF COLL. CHK OFF
(1) Interference check alarm function
0 0 Operation stops with a program error (P153) before executing a block which will cause cutting.
(2) Interference check avoidance function
1 0 The tool path is changed to prevent cutting from occurring. If the path cannot be changed, a program error (P153) occurs and the program will be stopped.
(3) Interference check in- valid function
0/1 1 Cutting continues as is, even if the work- piece is cut into. Use in the fine segment program.
Detailed description
Conditions viewed as interference
r : Compensation amount (a) Vectors intersect
Program path
Tool center pathN1 N3
N2
r
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
315 IB-1501277-P
(Example 1) When operating a program including a short segment with a tool with a large radius, cutting will occur in the shaded section.
(1) With alarm function. An alarm is output before N1 is executed. The buffer correction function can thus be used to change N1 to the following, enabling machining to continue: N1 G01 X20. Y-40.;
(2) With avoidance function The intersection of N1 and N3 is calculated to create interference avoidance vectors. Tool center path is (a) -> (e).
(3) With interference check invalid function. The tool passes while cutting the N1 and N3 line. Tool center path is (a)->(b)->(c)->(d)->(e) .
(G41) N1 G91 G01 X50. Y-100. ; N2 X70. Y-100. ; N3 X120. Y0 ;
N1 N3
N2
(a)
(b)
(c)
(d)
(e)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
316IB-1501277-P
(Example 2) When operating a program including a small circular with a tool with a large radius, cutting occurs near the start point/end point of the circular in the following figure.
Interference check processing
(1) With alarm function The alarm occurs before N1 is executed.
(2) With avoidance function With the above process, the vectors (1), (2), (3)' and (4)' will remain as the valid vectors. The tool center path will follow the path that connects vectors (1), (2), (3)' and (4)', as the interference avoidance path.
(3) With interference check invalid function The tool center path will follow the path that connects (1), (2), (3), (4), (1)', (2)', (3)', (4)', as the interference avoid- ance path while cutting.
Vectors (1) (4)' check -> No interference Vectors (2) (3)' check -> No interference Vectors (3) (2)' check -> Interference -> Erase vectors (3) (2)'
Erase vectors (4) (1)'
(Thick broken line path)
(Thin broken line path)
(4)(2)
(1)
N1
N3
N2
(2)
(4) (1)
(3)
(3)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
317 IB-1501277-P
(1) When three of the movement command blocks cannot be pre-read (when there are three or more blocks in the five pre-read blocks that are not moving)
(2) When there is an interference following the fourth movement block
When interference check cannot be executed
(a) Interference check is not possible
Program path
Tool center path
N1
N3
N2
N4
N5
N6
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
318IB-1501277-P
The movement will be as shown below when the interference avoidance check is valid.
Operation when interference avoidance function is valid
(a) Program path (b) Tool center path
Program path
Tool center path without interference check
Tool center path when interference is avoided (*: Linear movement)
Valid vector
Invalid vector
N1 N3
N2
(b) (a)
N1
N3N2
N1
N3N2
r
r (CP)
*
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
319 IB-1501277-P
If all of the line vectors for the interference avoidance are deleted, create a new avoidance vector as shown in below to avoid the interference.
In the case of the figure below, the groove will be left uncut.
Tool center path (*1)
Program path
Tool center path 2 (*1) Tool center path 1 (*1)
Program path (a) Avoidance vector
(*1) Tool center path when interference is avoided
Program path
Tool center path without interference check
Tool center path when interference is avoided
N1
N3
N2
N1
N3
N2
r1
N4
r2
r1 r2
(a)2
(a)1
(a)
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
320IB-1501277-P
The interference check alarm occurs under the following conditions.
(1) When the interference check alarm function has been selected When all vectors at the end of its own block have been deleted
As shown in the figure below, when vectors 1 through 4 at the end point of the N1 block have all been deleted, program error (P153) will occur prior to N1 execution.
(2) When the interference check avoidance function has been selected (Example 1) When there are valid vectors at the end point of the following blocks even when all the vectors at the
end point of its own block have been deleted
When, in the figure below, the N2 interference check is conducted, the N2 end point vectors are all de- leted but the N3 end point vectors are regarded as valid. Program error (P153) now occurs at the N1 end point and the operation stops.
In the case shown in the figure below, the tool will move in the reverse direction at N2. Program error (P153) now occurs before executing N1 and the operation stops.
Interference check alarm operation
N1
P153
2 3
N2 1
N3 4
N1
2 N21
N3 43
N4
P153
N1
P153
N2 N3
N4
1 2 3 4
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
321 IB-1501277-P
(Example 2) When avoidance vectors cannot be created
Even when, as in the figure below, the conditions for creating the avoidance vectors are satisfied, it may still be impossible to create avoidance vectors, or the interference vectors may interfere with N3. Program error (P153) will occur at the N1 end point when the vector intersecting angle is more than 90 and the operation will stop.
(Example 3) When the program advance direction and the advance direction after compensation are reversed
When grooves that are narrower than the tool diameter with parallel or widening bottom are pro- grammed, it will still be regarded as interference even if there is actually no interference.
N1
N2
N3
N4
P153
N1
N2
N3
N4
P153
P153
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
322IB-1501277-P
(Example 4) When vectors at the end point of the block immediately before the command to eliminate compensation vectors temporarily cause an interference
Interference check will be executed also at the end point of the block immediately before the command to eliminate compensation vectors temporarily, similarly with the case compensation vectors are not eliminated. It may be regarded as an interference even if there is actually no interference. If regarded as an interference, program error (P153) will occur.
In the figure below, only vector 1 is left as an end point vector in N2 because of the N3 G53 command to temporarily eliminate compensation vectors. However, the interference check will still be conducted to vector 1 to 4 and an interference will be detected. Program error (P153) now occurs at the end point of the previous block and the operation stops.
Program path
Tool center path
Tool center path when the interference check is invalid
Tool center path when the interference check is invalid in N3 due to a command (G01 etc.) not to eliminate compensation vectors.
Valid vector
Invalid vector (Invalid, however, subject to interference check)
N1(G01)
N2(G03)
N3(G53)
1
2
3 4
P153
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
323 IB-1501277-P
When starting compensation operation, the tool center path is determined with the movement command of the same block as G41/G42 and the next movement command. The interference check is not executed at that time. To check interference, set the parameter "#1241 set13/bit1" (MTB specifications). Note that an alarm is output and the oper- ation is stopped even when the collision avoidance setting "#8102 COLL. ALM OFF" is set to "1" and that the inter- ference avoidance is not applied.
Interference check for start-up block
(a) Interference check for start-up block invalid (b) Interference check for start-up block valid "#1241 set13/bit1" = "0" or "#8103 COLL. CHK OFF" = "1"
"#1241 set13/bit1" = "1" and "#8103 COLL. CHK OFF" = "0"
Tool center path Alarm stop
The interference with the compensation calculation vec- tor of the contact between the N2 block and N3 block is not checked. Doing so will cause a cut in the N3 block.
The interference with the compensation calculation vec- tor of the contact between the N2 block and N3 block is checked, and this is judged to be an alarm.
N1(G41 G01)
N2(G01)
N3(G01)
N1(G41 G01)
N2(G01)
N3(G01)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
324IB-1501277-P
12.3.9 Diameter Designation of Compensation Amount
With this function, the tool radius compensation amount can be designated by tool diameter. When the control pa- rameter "#8117 OFS Diam DESIGN" is ON, the compensation amount specified to the commanded tool No. will be recognized as the diameter compensation amount, and the amount will be converted to the radius compensation amount when executing the compensation.
When the tool radius compensation amount D=10.0 is commanded, tool radius compensation amount "d" is 5.0 if the parameter "#8117" is ON (set to "1"). (Tool radius compensation amount "r" is 10.0 if the parameter "#8117" is OFF (set to "0").)
(1) Linear -> linear corner (acute angle)
Function and purpose
Operation example
Operations when designating the compensation amount with diameter
Outside of the corner Inside of the corner
Program path
Tool center path (When #8117 is ON)
Tool center path (When #8117 is OFF)
rd
20 20
d s
r
d
r
d r
d
r
s
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
325 IB-1501277-P
(2) Linear -> arc (obtuse angle)
(3) Arc -> linear (obtuse angle)
(1) If tool radius compensation amount has already been set, the compensation amount is not be changed even if the parameter "8117" is changed.
(2) Make sure not to change the parameter #8117 during the compensation. When the parameter is changed using parameter input by program function, the program error (P421) will occur.
(3) If the parameter #8117 is set to ON with the parameter "#1037 cmdtyp" set to 2, the tool radius wear data is also regarded as the diameter compensation amount, thus, it will be converted to the radius value and compen- sation will be performed.
(4) Diameter designation of tool radius compensation amount can be used for the tool life management data.
(5) There is no effect by #8117 on the tool radius measurement function.
Outside of the corner Inside of the corner
Outside of the corner Inside of the corner
Program path
Tool center path (When #8117 is ON)
Tool center path (When #8117 is OFF)
(CP) Arc center
Restrictions
s
d
r
(CP)
r
s
d
(CP)
d
sr
(CP)
d s
r
d
r
(CP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
326IB-1501277-P
12.3.10 Workpiece Coordinate Changing during Radius Compensation
When the tool radius compensation is executed, the tool center path is calculated based on the position on the co- ordinate system. The based coordinate system is different depending on setting of the parameter "#1246/bit2 Switch coordinate systems for radius compensation". (This depends on the MTB specifications.)
When the parameter is "0", the tool radius compensation is calculated based on the position on the workpiece co- ordinate system. When the parameter is "1", the tool radius compensation is calculated based on the position on the program coor- dinate system. The program coordinate systems are defined as shown in the figure below.
Function and purpose
Detailed description
(R1) 1st reference position (a) 1st reference position offset (b) Interrupt amount offset (c) Extended workpiece coordinate system offset (d) G92 offset (e) Workpiece coordinate system offset (f) Local coordinate system offset (g) G53 Basic machine coordinate system (h) Program coordinate system (i) G54 to G59/G54.1Pn Workpiece coordinate system/Extended workpiece coordinate system (j) G52Local coordinate system
(b)
(c)
(e)
(f)
(a)
(h)
(R1)
(i)
(j)
(g)
(d)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
327 IB-1501277-P
The coordinate system changed by parameter is as follows.
D3 =5.000 G54 offset X15.000 Y15.000
G90 G54 G00 X15. Y20.; N1 G41 D3 X5. Y10. ; N2 G01; Y-20 F1000; N3 G40 X20. ; M30 ;
(1) Parameter = 0
(2) Parameter = 1
Program path (a) Compensation vector
Tool center path (b) Program coordinate system
G54
10.0
5.0
- 20.0
20.0
G53
N2
N3
N1
(a)
(b)
G54
N2
N3
N1
25.0
- 5.0
20.0 35.0
G53
(a)
(b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
328IB-1501277-P
12.4 Tool Nose Radius Compensation (for Machining Center System)
Because a tool nose is generally rounded, a hypothetical tool nose point is used for programming. Due to this round- ness of the tool nose, there will be a gap between the programmed shape and the actual cutting shape during taper cutting or circular cutting. Tool nose radius compensation (nose R compensation) compensation is a function for automatically calculating and offsetting this error by setting the tool nose radius (cutter radius) value. The validity of this function depends on the MTB specifications. (The tool nose must be set to "1" to "8" in the pa- rameter "#1037 cmdtyp".) If the tool nose is set to "0" or "9", tool radius compensation is carried out. When G46 is commanded, the tool position offset reduction function is enabled. (The automatic direction identifica- tion mode is not available.) Refer to "Programming Manual Lathe System" for details of the tool nose radius compensation.
Function and purpose
(a) Tool nose center (b) Hypothetical tool nose point (r) Tool nose radius
Tool nose center path with no nose R compensation (Shaded part indicates the cutting shape gap)
Tool nose center path with nose R compensation
Command format
G40; Tool nose radius compensation cancel
G41 (X__ Z__ D__); Tool nose radius compensation left
G42 (X__ Z__ D__); Tool nose radius compensation right
X X axis end point coordinate (Absolute position of workpiece coordinate system) Z Z axis end point coordinate (Absolute position of workpiece coordinate system) D Compensation No. (The compensation No. setting range will differ according to the specifications
(No. of compensation sets). )
(a)
(b)
r
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
329 IB-1501277-P
(1) G41 works on condition that the tool is located on the left of the workpiece to the direction of motion. G42 works on condition that the tool is located on the right of the workpiece to the direction of motion. G40 cancels the tool nose radius compensation mode.
(2) Nose R compensation pre-reads the data in the following two movement command blocks (up to 5 blocks when there is no movement command) and controls the tool nose radius center path by the intersection point calcula- tion method so that it is offset from the programmed path by an amount equivalent to the nose R. In the figure below, "r" is the tool nose radius compensation amount (nose R). The nose R compensation amount corresponds to the tool length No. and should be preset along with the tool nose point.
(3) If there are 4 or more blocks without movement amounts among 5 continuous blocks, overcutting or undercutting will occur. Blocks in which optional block skip is valid are ignored.
(4) Tool nose radius compensation is also valid for fixed cycle. (5) Compensation mode will be temporarily canceled in 1 block before the thread cutting command block. (6) The compensation plane, movement axes and next advance direction vector follow the plane selection command
designated by G17, G18 or G19.
Detailed description
G17 XY plane X,Y,I,J G18 ZX plane Z,X,K,I G19 YZ plane Y,Z,J,K
G42
X
Z
G41
N1
N2
N3
r
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
330IB-1501277-P
(1) For nose radius compensation for machining center system, the compensation amount should always be spec- ified with radius value.
(2) Compensation amounts are normally changed when a different tool has been selected in the compensation can- cel mode. However, when an amount is changed during the compensation mode, the vectors at the end point of the block are calculated using the compensation amount designated in that block.
(1) The criterion to execute the outer rounding at the small corner in tool radius compensation depends on the MTB specifications (parameter "#1289 ext25/bit0").
(1) There two methods to set the tool nose point for machining center system. (This depends on the MTB specifica- tions.) Set a value in the system variable #23000+n ("n" corresponds to the compensation number) using the ma-
chining program. Set the parameter "#1046 T-ofs disp type" to change the compensation type to III, then, set a value in the
tool compensation amount screen.
(1) An error will occur when any of the following commands is programmed during tool nose radius compensation. G17, G18, G19 (when a plane different from the one used during the compensation is commanded (P112)) G31 (P608) G74,G75,G76 (P155) G81 to G89(P155)
(2) A program error will occur when a circular command is issued in the first or last block of the tool nose radius compensation. (P151)
(3) A program error will occur during tool nose radius compensation when the intersection point of single block skip in the interference block processing cannot be calculated. (P152)
(4) A program error will occur when there is an error in one of the pre-read blocks during tool nose radius compen- sation.
(5) A program error will occur when an interference occurs under no interference avoidance conditions during tool nose radius compensation. (P153)
(6) A program error will occur when a tool nose radius compensation command is issued even though the tool nose radius compensation specification is not provided. (P150)
(7) If a tool nose radius compensation command is issued in mirror image, a program error will occur. (P803)
Precautions
Assigning the compensation amounts
Corner judgment method
Designating the tool nose point
Errors during tool nose radius compensation
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
331 IB-1501277-P
12.5 3-dimensional Tool Radius Compensation; G40/G41, G42
The 3-dimentional tool radius compensation compensates for the tool in a 3-dimensional space following the com- manded three-dimensional vectors.
As shown above, the tool is moved in the tool center coordinate position (x', y', z') (d) which is compensated for by the tool radius "r" (c) in respect to the program coordinate position (x, y, z) (b) following the plane normal line vector (I, J, K) (a).
Though two-dimensional tool radius compensation creates the vectors at a right angle to the (I, J, K) direction, three- dimensional tool radius compensation creates the vector in the (I, J, K) direction. (The vector is created at the end point of the block.)
The three-dimensional compensation vector (compensation) (e) axis elements are as below.
Thus, the tool center coordinate position (x', y', z') (d) is each expressed as below. Note that (x, y, z) are the program coordinate position.
(1) Three-dimensional compensation vector (Hx, Hy, Hz) refers to the plane normal line vector whose direction is same as the plane normal line vector (I, J, K ) and the size equals to the tool radius "r".
(2) When the machining parameter "#8071 3-D CMP" is set to a value other than "0", the value of "#8071 3-D CMP" will be used as the value. (Refer to the s Setup Manual for details.)
Function and purpose
x' = x + Hx y' = y + Hy z' = z + Hz
(x', y', z')
Y (J) X (I)
Z (K)
(x, y, z)
(I, J, K)
(b)
(c)
(a) (d)
(e)
I Hx = r
( I 2 + J
2 + K
2 )
J H Y = r
( I 2 + J
2 + K
2 )
K HZ = r
( I 2 + J
2 + K
2 )
Note
( I2 + J 2 + K 2 )
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
332IB-1501277-P
Command, for all three axes, the compensation No. D and plane normal line vector (I, J, K) in the same block as the three-dimensional tool radius compensation command G41 (G42).
If only one or two axes are commanded, the normal tool radius compensation mode will be applied. (When the com- mand value for I, J, K is set to "0", this command is valid.)
Command format
3-dimensional tool radius compensation start
G41(G42) X__ Y__ Z__ I__ J__ K__ D__ ;
New plane normal line vector is commanded in the compensation mode.
X__ Y__ Z__ I__ J__ K__;
3-dimentional tool radius compensation cancel
G40; (or D00;)
G40 X__ Y__ Z__; (or X__ Y__ Z__ D00;)
G41 Three-dimensional tool radius compensation command (+ direction) G42 Three-dimensional tool radius compensation command (- direction) G40 Three-dimensional tool radius compensation cancel command X, Y, Z Movement axis command compensation space I, J, K Plane normal line vector D Compensation No.
(Note that when "D00" is issued, three dimensional tool radius compensation will be canceled even if G40 is not commanded.)
G Code Compensation amount: D00
+ -
G40 Cancel Cancel Cancel G41 I, J, K direction Reverse direction of I, J, K Cancel G42 Reverse direction of I, J, K I, J, K direction Cancel
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
333 IB-1501277-P
Detailed description
The compensation space is determined by the axis address commands (X, Y, Z, U, V, W) of the block where the three-dimensional tool radius compensa- tion starts.
(Example) G17 ; G41 Xx Yy Zz Ii Jj Kk ;
X Y Z space
G17 ; G41 Yy Ii Jj Kk ;
X Y Z space
Here, U, V and W are each the additional axes for the X, Y and Z axis. If the X axis and U axis (Y and V, Z and W) are com- manded simultaneously in the three-dimensional tool radius compensation start block, the currently com- manded plane selection axis will have the priority. If the axis address is not commanded, it will be inter- preted that the X, Y and Z axes are commanded for the coordinate axes.
G17 V ; G41 Xx Vv Zz Ii Jj Kk ;
X V Z space
G17 W ; G41 Ww Ii Jj Kk ;
X Y W space
G17 ; G41 Xx Yy Zz Ww Ii Jj Kk ;
X Y Z space
G17 W ; G41 Xx Yy Zz Ww Ii Jj Kk ;
X Y W space
G17 ; G41 Ii Jj Kk ;
X Y Z space
G17 U ; G41 Ii Jj Kk ;
U Y Z space
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
334IB-1501277-P
Operation example
Compensation start: When there is a movement command
(S) Start point
Tool center path
Programmed path
Three-dimensional compensation vec- tor
Compensation start: When there is no movement command
(S) Start point
Tool center path
Three-dimensional compensation vec- tor
Movement during the compensation: When there is a movement command and a plane normal line vector command
(S) Start point (a) Old vector (b) New vector
Tool center path
Programmed path
Movement during the compensation: When there is no plane normal line vector command
(S) Start point (a) Old vector (b) New vector
Tool center path
Programmed path
G41 Xx Yy Zz Ii Jj Kk Dd ;
(S)
G41 Ii Jj Kk Dd ;
(S)
Xx Yy Zz Ii Jj Kk ;
(a)
(b)
(S)
Xx Yy Zz Ii Jj Kk ;
(a)
(S)
(b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
335 IB-1501277-P
The I, J, K commands for a circular or helical cutting are regarded as the circular center commands, thus, the new vector is equivalent to the old vector.
Even for the R-designation method, commanded I, J, K addresses will be ignored, then the new vector will be equiv- alent to the old vector.
G02 Xx Yy (Zz) Ii Jj ; I, J(K) means the circular center Or G02 Xx Yy (Zz) Rr ; R-designated arc
(1) The center coordinate will not shift during the circular or helical cutting. Thus, when I, J, K are commanded with the vector as below, the program error (P70) will occur.
G02 Xx Yy (Zz) Ii Jj ; I, J(K) means the circular center Or G02 Xx Yy (Zz) Rr ; R-designated arc
(1) If I, J, K are not commanded in a block where the compensation amount is to be changed, the vector will be equivalent to the old vector. In this case, the modal will change, however, the compensation amount will change when I, J, K are commanded.
Movement during the compensation: For arc or helical cutting
(S) Start point (a) Old vector (b) New vector
Tool center path
Programmed path
(S) Start point (a) Old vector (b) New vector
(CP) Arc center
Tool center path
Programmed path
Movement during the tool radius compensation: When compensation amount is to be changed
(S) Start point (a) Old vector (b) New vector
Tool center path
Programmed path
(a) (b)
(S)
Note
(b)(a)
r
(CP)
r
(S)
G41 Xx Yy Zz Ii Jj Kk Dd1 ;
G41 Xx Yy Zz Ii Jj Kk Dd2 ;
(b)
(S)
(a)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
336IB-1501277-P
(1) If I, J and K are not commanded in a block where the compensation direction is to be changed, the vector will be equivalent to the old vector and the compensation direction will not be changed. In this case, the modal will change, however, the compensation direction will change when I, J and K are commanded.
(2) If the compensation direction is changed in an arc (G02/G03) block, I, J will be the center of the arc, thus, the compensation direction will not change. Even for the R-designation method, commanded I, J and K will be ignored, and the compensation direction can- not be changed.
G40 Xx Yy Zz ; (or Xx Yy Zz D00 ;)
G40; (or D00;)
Movement during the tool radius compensation: When compensation direction is to be changed
(S) Start point (a) Old vector (b) New vector
Tool center path
Programmed path
Movement during the tool radius compensation: When there is a movement command
(S) Start point (E) End point (a) Old vector
Tool center path
Programmed path
Tool radius compensation cancel: When there is no movement command
(a) Old vector
Tool center path
Programmed path
G41 Xx Yy Zz Ii Jj Kk Dd1 ;
G42 Xx Yy Zz Ii Jj Kk ; (b)
(a)
(S)
Note
(S)
(a)
(E)
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
337 IB-1501277-P
If the plane normal line vector (I, J, K) is not commanded for all three axes in the three-dimensional tool radius com- pensation start block, the normal tool radius compensation mode will take place. If G41 (G42) is commanded without commanding the plane normal line vector during three-dimensional tool radius compensation, the modal will change, however, the old vector will be used. If G41 (G42) with the plane normal line vector is commanded during tool radius compensation, this command will be ignored and the normal tool radius compensation will take place.
Tool length compensation is applied to the coordinate after three-dimensional tool radius compensation.
Tool position offset is applied to the coordinate after three-dimensional tool radius compensation.
The program error (P155) will occur.
Scaling is applied to the coordinate before three-dimensional tool radius compensation. Scaling is not applied to the plane normal line vector (I, J, K).
(a) Plane normal line vector
Programmed path
Program path after compensation
Program path after scaling
Program path after scaling and compensation
Relationship with other functions
Normal tool radius compensation
Tool length compensation
Tool position offset
Fixed cycle
Scaling
D1=10. G90 ; G51 X0 Y0 P0.5 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-30. Y-30. Z-20. ; N3 X-50. Y-20. Z-10. ; N4 Y0. ; N1( -5.000, -10.000, -10.000 ) N1( -10.773, -15.773, -15.773 ) N2( -15.000, -15.000, -20.000 ) N2( -20.773, -20.773, -25.773 ) N3( -25.000, -10.000, -10.000 ) N3( -30.773, -15.773, -15.773 ) N4( -25.000, 0.000, -10.000 ) N4( -30.773, -5.773, -15.773 )
* Upper: Program position after scaling Lower: Position after scaling and compensation
X
X - 50.
(a)
(a)
- 30. - 20.
- 20.
- 30.
- 10.
- 30.
Y
Z
- 10.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
338IB-1501277-P
Coordinate rotation by program is applied to the coordinate before three-dimensional tool radius compensation. The plane normal line vector (I, J, K) will not rotate.
(a) Plane normal line vector
Programmed path
Program path after compensation
Program path after coordinate rotation
Program path after coordinate rotation and compensation
Parameter coordinate rotation is applied to the coordinates after three-dimensional tool radius compensation. The plane normal line vector (I, J, K) rotates.
Mirror image is applied to the coordinates after three-dimensional tool radius compensation. Mirror image is applied to the plane normal line vector (I, J, K).
The program error (P608) will occur.
The compensation amount will not be canceled. Thus, if this is commanded during three-dimensional tool radius compensation, the path will be deviated by the compensation amount, thus the program error (P434) will occur.
Coordinate rotation by program
D1=10. G90 ; G68 X0 Y0 R45. ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-30. Y-30. Z-20. ; N3 X-50. Y-20. Z-10. ; N4 Y0. ; N1( 7.071, -21.213, -10.000 ) N1( 7.071, -29.378, -15.773 ) N2( 0.000, -42.426, -20.000 ) N2( 0.000, -50.591, -25.773 ) N3( -21.213, -49.497, -10.000 ) N3( -21.213, -57.662, -15.773 ) N4( -35.355, -35.355, -10.000 ) N4( -35.355, -43.520, -15.773 )
* Upper: Program position after coordinate ro- tation Lower: Position after coordinate rotation and compensation
Coordinate rotation by parameter
Mirror image
Skip
Reference position check
- 20.
- 30.
- 10.
- 20.
X
Y
Z
X
- 50.
(a)
(a)
- 30. - 20. - 10.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
339 IB-1501277-P
Automatic corner override is invalid during three-dimensional tool radius compensation.
(1) For the absolute command, all axes will be temporarily canceled at the commanded coordinate position.
Programmed path
Program path after compensation
(2) For the incremental command, the axis will move by the amount obtained by subtracting each axis vector from the incremental movement amount. (The compensation amount is temporarily canceled.)
Programmed path
Program path after compensation
Automatic corner override
Machine coordinate system selection
D1=10. G90 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-30. Y-30. Z-20. ; N3 X-50. Y-20. Z-10. ; N4 G53 Y0 ; N1( -10.000, -20.000, -10.000 ) N1( -15.773, -25.773, -15.773 ) N2( -30.000, -30.000, -20.000 ) N2( -35.773, -35.773, -25.773 ) N3( -50.000, -20.000, -10.000 ) N3( -55.773, -25.773, -15.773 ) N4( -50.000, 0.000, -10.000 ) N4( -50.000, 0.000, -10.000 )
* Upper: Program position Lower: Program position after compensation
D1=10. G91 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-20. Y-10. Z-10. ; N3 X-20. Y10. Z10. ; N4 G90 G53 Y0.; N1( -10.000, -20.000, -10.000 ) N1( -15.773, -25.773, -15.773 ) N2( -30.000, -30.000, -20.000 ) N2( -35.773, -35.773, -25.773 ) N3( -50.000, -20.000, -10.000 ) N3( -55.773, -25.773, -15.773 ) N4( -50.000, 0.000, -10.000 ) N4( -50.000, 0.000, -10.000 )
* Upper: Program position Lower: Program position after compensation
X - 50. - 30. - 20. - 10.
X
- 20.
- 30.
Y
- 10.
- 20.
Z
X
X
Y
Z
- 50. - 30. - 20. - 10.
- 30.
- 20.
- 10.
- 20.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
340IB-1501277-P
When commanded in the same block as the coordinate system setting, the coordinate system will be set, and op- eration will start up independently with the plane normal line vector (I, J, K).
Programmed path
Program path after compensation
Coordinate system setting
D1=10. G91 ; N1 G92 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-20. Y-10. Z-10. ; N3 X-30. Y-10. Z10. ; N4 Y20. ; N1( -10.000, -20.000, -10.000 ) N1( -10.000, -20.000, -10.000 ) N2( -30.000, -30.000, -20.000 ) N2( -35.773, -35.773, -25.773 ) N3( -50.000, -20.000, -10.000 ) N3( -55.773, -25.773, -15.773 ) N4( -50.000, 0.000, -10.000 ) N4( -55.773, -5.773, -15.773 )
* Upper: Program position Lower: Program position after compensation
- 20. G92
- 30.
Y
- 10.
- 20.
Z
X
X
- 50. - 30. - 20. - 10. W(0,0)
W(0,0)
G92
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
341 IB-1501277-P
All the axes will be temporarily canceled at the intermediate point.
Programmed path
Program path after compensation
Three-dimensional tool radius compensation will be canceled if NC reset is executed during three-dimensional tool radius compensation.
Three-dimensional tool radius compensation will be canceled by the emergency stop or emergency stop cancel during three-dimensional tool radius compensation.
Reference position return completed
D1=10. G91 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-20. Y-10. Z-10. ; N3 X-20. Y10. Z10. ; N4 G28 X0 Y0 Z0 ; N1( -10.000, -20.000, -10.000 ) N1( -15.773, -25.773, -15.773 ) N2( -30.000, -30.000, -20.000 ) N2( -35.773, -35.773, -25.773 ) N3( -50.000, -20.000, -10.000 ) N3( -55.773, -25.773, -15.773 ) N4( 0.000, 0.000, 0.000 ) N4( 0.000, 0.000, 0.000 ) N4( 20.000, 10.000, 10.000 ) N4( 20.000, 10.000, 10.000 )
* Upper: Workpiece coordinate position Lower: Program position after compensa- tion
NC reset
Emergency stop
X
X
Z
- 30. - 20. - 10.
- 40.
- 20.
- 10.
- 30.
W(0,0)
M(0,0)
- 10.
Y
- 30.
- 20.
M(0,0)
W(0,0)
- 20.
- 10.
- 50.
- 30. - 20.- 70. - 50.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
342IB-1501277-P
(1) The compensation No. is selected with the D address, however, the D address is valid only when G41 or G42 is commanded. If D is not commanded, the number of the previous D address will be valid.
(2) Switch the mode to the compensation mode in the G00 or G01 mode. When changed during the arc mode, the program error (P150) will occur. The compensation direction and compensation amount after the mode change will become valid from the block where I, J and K are commanded in the G00 or G01 mode. If three-dimensional tool radius compensation is com- manded in a block not containing the plane normal line vector (I, J, K) during the arc mode, only the modal infor- mation will be changed. The plane normal line vector will be validated from the block where I, J and K are commanded next.
(3) During the 3-dimensional tool radius compensation mode in a certain space, it is not possible to switch the space to another one and to execute three-dimensional tool radius compensation. To switch the compensation space, always cancel the compensation mode with G40 or D00 first. (Example)
(4) If the compensation No. D is other than the range of 1 to 40 with the standard specifications or 1 to 800 (max.) with the additional specifications, the program error (P170) will occur.
(5) Only the G40 and D00 commands can be used to cancel 3-dimensional tool radius compensation.
(6) If the size (I2+J2+K2) of the vector commanded with I, J and K overflows, the program error (P35) will occur.
Restrictions
G41 Xx Yy Zz Ii Jj Kk ; Compensation starts in X, Y, Z space. : : : :
G41 Uu Yy Zz Ii Jj Kk ; Compensation is carried out in X, Y, Z space, and U axis moves by commanded value.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
343 IB-1501277-P
12.6 Tool Position Offset; G45 to G48
Using the G45 to G46 commands, the movement distance of the axes specified in the same block can be extended or reduced by a preset compensation length.
Furthermore, the compensation amount can be similarly doubled (x 2 expansion) or halved (x 2 reduction) with com- mands G47 and G48.
The number of sets for the compensation differ according to machine specification. Refer to Specifications Manual.
D01 to Dn
(The numbers given are the total number of sets for tool length compensation, tool position compensation and tool radius compensation.)
Function and purpose
Start point End point G45 command
Expansion by compensa- tion amount only
Internal arithmetic processing
Movement amount
G46 command
Reduction by compensa- tion amount only
Internal arithmetic processing
Movement amount
G47 command
2 expansion by compen- sation amount
Internal arithmetic processing
Movement amount
G48 command
2 reduction by compensa- tion amount
Internal arithmetic processing
Movement amount
(Program command value) (compensation amount) (Movement amount after compensation)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
344IB-1501277-P
Details for incremental positions are given below.
Command format
G45 X__ Y__ Z__ D__ ; Expansion of movement amount by compensation amount set in compen- sation memory
G46 X__ Y__ Z__ D__ ; Reduction of movement amount by compensation amount set in compensa- tion memory
G47 X__ Y__ Z__ D__ ; Expansion of movement amount by double the compensation amount set in compensation memory
G48 X__ Y__ Z__ D__ ; Reduction of movement amount by double the compensation amount set in compensation memory
X, Y, Z Movement amount of each axis D Tool compensation No.
Detailed description
Command Movement amount of equivalent com- mand
Example
(assigned compensation amount = l) (when X = 1000)
G45 Xx Dd X(x+l) l= 10 X= 1010 l= -10 X= 990
G45 X-x Dd X-(x+l) l= 10 X= -1010 l= -10 X= -990
G46 Xx Dd X(x-l) l= 10 X= 990 l= -10 X= 1010
G46 X-x Dd X-(x-l) l= 10 X= -990 l= -10 X= -1010
G47 Xx Dd X(x+2*l) l= 10 X= 1020 l= -10 X= 980
G47 X-x Dd X-(x+2*l) l= 10 X= -1020 l= -10 X= -980
G48 Xx Dd X(x-2*l) l= 10 X= 980 l= -10 X= 1020
G48 X-x Dd X-(x-2*l) l= 10 X= -980 l= -10 X= -1020
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
345 IB-1501277-P
Tool position compensation with 1/4 arc command
It is assumed that compensation has already been provided in the + X direction by D01 = 200.
Even if the compensation numbers are not assigned in the same block as the G45 to G48 commands, compensation is provided with the tool position compensation number previously stored in the memory.
If the commanded compensation No. exceeds the specification range, the program error (P170) will occur.
These G codes are unmodal and are effective only in the command block.
Even with an absolute command, the amount of the movement is extended or reduced for each axis with respect to the direction of movement from the end point of the preceding block to the position assigned by the G45 to G48 block.
In other words, even for an absolute command, compensation can be applied to movement amounts (incremental position) in the same block.
When a command for "n" number of simultaneous axes is given, the same compensation will be applied to all axes. It is valid even for the additional axes. (but it must be within the range of the number of axes that can be controlled simultaneously.)
Program example
(Example 1)
(S) Start point (E) End point (CP) Programmed arc center
Tool
Programmed path Tool center path
G91 G45 G03 X -1000 Y1000 I -1000 F1000 D01 ;
G01 G45 X220. Y60. D20 ; (D20) = +50. 000
End point after compensation
Programmed end point
(S) Start point
Y
X
(E)
(S)
1000
1000
200
(CP)
X (S)
Y
60. 50.
50.
110.
220. 270.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
346IB-1501277-P
(1) If compensation is applied to two axes, over-cutting or under-cutting will result, as shown in the figures below. In cases like this, use the cutter compensation commands (G40 to G42).
G01 G45 Xx 1 Dd1 ; Xx2 Yy 2 ; G45 Yy3 ;
G01 Xx1 ; G45 Xx2 Yy2 Dd 2 ; Yy3 ;
Programmed path Tool center path
Workpiece
Undercutting (figure above) or overcutting (figure below) l = Compensation amount setting
Note
l
Y
X
l Y
X
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
347 IB-1501277-P
(Example 2)
N1 G46 G00 Xx1 Yy1 Dd1 ; N2 G45 G01 Yy2 Ff2 ; N3 G45 G03 Xx3 Yy3 Ii3 ; N4 G01 Xx4 ;
Program path Tool center path
N4
N3
Y
X N1
N2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
348IB-1501277-P
When the G45 to G48 command is assigned, the compensation amount for each pass is the amount assigned by the compensation number, and the tool does not move for the difference from the previous compensation as it would do with the tool length compensation command (G43).
Compensation amount D01 = 10.000mm (Compensation amount of tool radius)
(Example 3)
(S) Start point (a) Programmed path (b) Tool center path
N100 G91 G46 G00 X40.0 Y40.0 D01 ; N101 G45 G01 X100.0 F200 ; N102 G45 G03 X10.0 Y10.0 J10.0 ; N103 G45 G01 Y40.0 ; N104 G46 X0 ; N105 G46 G02 X-20.0 Y20.0 J20.0 ; N106 G45 G01 Y0 ; N107 G47 X-30.0 ; N108 Y-30.0 ; N109 G48 X-30.0 ; N110 Y30.0 ; N111 G45 X-30.0 ; N112 G45 G03 X-10.0 Y-10.0 J-10.0 ; N113 G45 G01 Y-20.0 ; N114 X10.0 ; N115 Y-40.0 ; N116 G46 X-40.0 Y-40.0 ; N117 M02 ; %
4030
N101
10
N102
30
30
30
40
40
10
N100
N105N108N110
N103
N115
N114
N116
N113 N109
N112
N104
N106
N107
20R
10R
10R
N111
(b)(a)
(S)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
349 IB-1501277-P
(1) These commands should be used when operation is not in a fixed cycle mode. (They are ignored even if they are assigned during a fixed cycle.)
(2) As a result of the internal arithmetic processing based on the expansion or reduction, the tool will proceed to move in the opposite direction when the command direction is reversed.
(3) When a zero movement amount has been specified in the incremental command (G91) mode, the result is as follows.
When a zero movement amount has been specified with an absolute command, the operation is completed im- mediately and the tool does not move for the compensation amount.
Precautions
Program command G48 X20.000 D01 ;
Compensation Compensation amount = +15.000
Tool movement Actual movement = X - 10.000
(S) Start point (E) End point
Compensation No. : D01 Compensation amount corresponding to D01 : 1234
NC command G45 X0 D01 ; G45 X-0 D01 ; G46 X0 D01 ; G46 X-0 D01; Equivalent command X1234; X -1234 ; X -1234 ; X1234;
(S)
(E)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
12 Tool Compensation Functions
350IB-1501277-P
(4) In the case of circular interpolation, tool radius compensation is possible by the G45 to G48 commands only for one quadrant, two quadrants (semi sphere) or three quadrants when the start and end points are on the axis. The commands are assigned as follows depending on whether the compensation is applied for outside or inside the arc programmed path.
However, in this case, compensation must already be provided in the desired direction at the arc start point. (If a compensation command is assigned for the arc independently, the arc start point and end point radius will shift by an amount equivalent to the compensation amount.) The program path is indicated by the heavy line in the figure.
[1/4 circular arc]
[1/2 circular arc]
[3/4 circular arc]
G45 for compensation outside the circle G46 for compensation inside the circle
Program path Compensated path
G47 for compensation outside the circle G48 for compensation inside the circle
Program path Compensated path
G45 for compensation outside the circle G46 for compensation inside the circle
Program path Compensated path
G46
G45
G48
G47
G46
G45
13
351 IB-1501277-P
Fixed Cycle
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
352IB-1501277-P
13Fixed Cycle 13.1 Fixed Cycles
These fixed cycles are used to perform prepared sequences of machining programs, such as positioning, hole drill- ing, boring and tapping in one block. The available machining sequences are listed in the table below. By editing the standard fixed cycle subprograms, the fixed cycle sequences can be changed by the user. The user can also register and edit an original fixed cycle program. For the standard fixed cycle subprograms, refer to the list of the fixed cycle subprograms in the appendix of the operation manual. The list of fixed cycle functions for this con- trol unit is shown below.
A fixed cycle mode can be canceled by G80 command and other hole machining modes or G command in the 01 group. At the same time, various other data will also be cleared to zero.
Function and purpose
G code Hole drilling start (-Z direction)
Operation at hole bottom
Return operation (+Z direction)
Retract at high speed
Application
Dwell Spindle
G80 - - - - - Cancel G81 Cutting feed - - Rapid traverse Possible Drill, spot drilling cycle G82 Cutting feed Yes - Rapid traverse - Drill, counter boring cycle G83 Intermittent feed - - Rapid traverse Possible Deep hole drilling cycle G84 Cutting feed Yes Reverse
rotation Cutting feed - Tapping cycle
G85 Cutting feed - - Cutting feed - Boring cycle G86 Cutting feed Yes Stop Rapid traverse - Boring cycle G87 Rapid traverse - Forward
rotation Cutting feed - Back boring cycle
G88 Cutting feed Yes Stop Rapid traverse - Boring cycle G89 Cutting feed Yes - Cutting feed - Boring cycle G73 Intermittent feed Yes - Rapid traverse Possible Stepping cycle G74 Cutting feed Yes Forward
rotation Cutting feed - Reverse tapping cycle
G75 Cutting feed - - Rapid traverse - Circular cutting cycle G76 Cutting feed - Oriented
spindle stop
Rapid traverse - Fine boring cycle
G187 Cutting feed - - Rapid traverse - Thread milling cycle
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
353 IB-1501277-P
There are 7 actual operations which are each described below.
(1) This indicates the X and Y axes positioning, and executes positioning with G00. (2) This is an operation done after positioning is completed (at the initial point), and when G87 is commanded, the
M19 command is output from the control unit to the machine. When this M command is executed and the finish signal (FIN) is received by the control unit, the next operation will start. If the single block stop switch is ON, the block will stop after positioning.
(3) The tool is positioned to the R point by rapid traverse. (4) Hole machining is conducted by cutting feed. (5) This operation takes place at the hole bottom position, and depending on the fixed cycle mode, the operation
can be the spindle stop (M05), the rotary tool reverse rotation (M04), rotary tool forward rotation (M03), dwell or tool shift.
(6) The tool is retracted to the R point at the cutting feed or the rapid traverse rate, depending on the fixed cycle mode.
(7) The tool is returned to the initial point at rapid traverse rate.
(1) Whether the fixed cycle is to be completed at operation 6 or 7 can be selected by G98/G99 commands. (Refer to "Initial point and R point level return; G98, G99")
Detailed description
Basic operations of fixed cycle for drilling
(I) Initial point (R) R point return
Difference between absolute command and incremental command
For absolute command For incremental command
(R) R point
(2)
(4)
(3)
(5)
(6)
(7) (R)
(I)(1)
Note
+r
- z
(R)
-r
- z
(R)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
354IB-1501277-P
The fixed cycle has basic control elements for the positioning plane and hole drilling axis. The positioning plane is determined by the G17, G18 and G19 plane selection commands, and the hole drilling axis is the axis perpendicular (X, Y, Z or their parallel axis) to the above plane.
Xp, Yp and Zp indicate the basic axes X, Y and Z or an axis parallel to the basic axis.
An arbitrary axis other than the hole drilling axis can be commanded for positioning.
The hole drilling axis is determined by the axis address of the hole drilling axis commanded in the same block as G81 to G89, G73, G74 or G76. The basic axis will be the hole drilling axis if there is no designation.
(Example 1) When G17 (X-Y plane) is selected, and the axis parallel to the Z axis is set as the W axis.
(1) The hole drilling axis can be fixed to the Z axis with parameter #1080 Dril_Z. (2) Changeover of the hole drilling axis must be done with the fixed cycle canceled.
In the following explanations on the movement in each fixed cycle mode, the XY plane is used for the positioning plane and the Z axis for the hole drilling axis. Note that all command values will be incremental positions, the posi- tioning plane will be the XY plane and the hole drilling axis will be the Z axis.
This commands the in-position width for commanding the fixed cycle from the machining program. The commanded in-position width is valid only in the eight fixed cycles; G81 (drill, spot drill), G82 (drill, counter boring), G83 (deep drill cycle), G84 (tap cycle), G85 (boring), G89 (boring), G73 (step cycle) and G74 (reverse tap cycle). The ", I" ad- dress is commanded in respect to the positioning axis, and the ",J" address is commanded in respect to the drilling axis.
Positioning plane and hole drilling axis
Plane selection Positioning plane Hole drilling axis
G17 (X-Y) Xp-Yp Zp G18 (Z-X) Zp-Xp Yp G19 (Y-Z) Yp-Zp Xp
G81 .... Z_ ; The Z axis is used as the hole drilling axis. G81 .... W_; The W axis is used as the hole drilling axis. G81 .... ; (No Z or W) The Z axis is used as the hole drilling axis.
Programmable in-position width command in fixed cycle
Address Meaning of address Command range (unit) Remarks
,I Positioning axis in-position width(position error amount)
0.001 to 999.999 (mm) If a value exceeding the command range is commanded, a program er- ror (P35) will occur.
,J Drilling axis in-position width(position error amount)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
355 IB-1501277-P
When L (number of repetitions) is designated twice or more times in the fixed cycle, the commanded in-position width will be valid in the repetition block (5) to (8) below.
:
G91 G81 X-50. Z-50. R-50. L2 F2000 ,I0.2 ,J0.3;
:
In the following machining program, the commanded in-position width is valid for the Fig. 2 block. In the (B) block, the in-position width (, I) commanded regarding to positioning in the previous block (A) is invalid (5). However, when returning from the hole bottom, the in-position width (, J) commanded in the previous block (A) is valid (8). To validate the in-position width for positioning, command again as shown in block (C) (9).
In-position check in fixed cycle
Operation pattern ,I ,J (1) Valid - (2) - Invalid (3) - Invalid (4) - Valid (5) Valid - (6) - Invalid (7) - Invalid
Fig. 1 Operation when number of repetitions L is designated (8) - Valid
: G91 G81 X-50. Z-50. R-50. F2000 ,I0.2 ,J0.3 ; (A) X-10. ; . (B) X-10.,I0.2 ; (C)
Operation pattern ,I ,J (1) Valid - (2) - Invalid (3) - Invalid (4) - Valid (5) Invalid - (6) - Invalid (7) - Invalid (8) - Valid (9) Valid -
(10) - Invalid (11) - Invalid
Fig. 2 Operation in fixed cycle modal (12) - Valid
(6)
(5)(1)
(8) (7)
(4)
(3)
(2)
- 10.
- 10. - 50.
(6)
(5)(1)
(8)
(7)
(4)
(3)
(2)
(9)
(11)
(10)
(12)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
356IB-1501277-P
13.1.1 Drilling, Spot Drilling; G81
The operation stops at after the (1), (2) and (4) commands during single block operation.
Command format
G81 Xx1 Yy1 Zz1 Rr1 Ff1 Ll1,Ii1,Jj1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Ll1 Designation of number of repetitions. (0 to 9999)
When 0 is set, no execution. ,Ii1 Positioning axis in-position width ,Jj1 Drilling axis in-position width
Detailed description
Operation pattern i1 j1 Program
(1) Valid - G00 Xx1 Yy1; (2) - Invalid G00 Zr1; (3) - Invalid G01 Zz1 Ff1; (4) - Valid G00 Z- z1+r1; G98 mode
G00 Z-z1; G99 mode
G98 G99
(1)
(2)
(3) (4)
x1 , y1
z1 (4)
r 1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
357 IB-1501277-P
13.1.2 Drilling, Counter Boring; G82
The operation stops at after the (1), (2) and (5) commands during single block operation.
Command format
G82 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1 Ll1 ,Ii1 ,Jj1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Pp1 Designation of dwell time at hole bottom position (the values after the decimal points will
be ignored) (modal) Ll1 Designation of number of repetitions (0 to 9999)
When 0 is set, processing is not executed. ,Ii1 Positioning axis in-position width ,Jj1 Drilling axis in-position width
Detailed description
Operation pattern i1 j1 Program
(1) Valid - G00 Xx1 Yy1; (2) - Invalid G00 Zr1; (3) - Invalid G01 Zz1 Ff1; (4) - - G04 Pp1 ; Dwell (5) - Valid G00 Z-(z1+r1); G98 mode
G00 Z-z1; G99 mode
G98 G99
(1)
(2)
(3)
(4)
x1 , y1
z1 (5)
r 1
(5)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
358IB-1501277-P
13.1.3 Deep Hole Drilling Cycle; G83 13.1.3.1 Deep Hole Drilling Cycle
Command format
G83 Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Ll1 ,Ii1 ,Jj1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Qq1 Cut amount for each cutting pass (incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Ll1 Designation of number of repetitions. (0 to 9999)
When 0 is set, no execution. ,Ii1 Positioning axis in-position width ,Jj1 Drilling axis in-position width
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
359 IB-1501277-P
When executing a second and following cuttings in the G83 as shown above, the movement will change from rapid traverse to cutting feed "m" mm before the position machined last. After reaching the hole bottom, the axis will return according to the G98 or G99 mode. "m" will differ according to the parameter "#8013 G83 return". Program so that q1 > m. The operation stops at after the (1), (2) and (n) commands during single block operation.
Detailed description
Operation pattern i1 j1 Program
(1) Valid - G00 Xx1 Yy1; (2) - Invalid G00 Zr1; (3) - Invalid G01 Zq1 Ff1; (4) - Invalid G00 Z-q1; (5) - Invalid G00 Z(q1-m); (6) - Invalid G01 Z(q1+m) Ff1; (7) - Invalid G00 Z-2*q1; (8) - Invalid G00 Z(2*q1-m); (9) - Invalid G01 Z(q1+m) Ff1;
(10) - Invalid G00 Z-3*q1; :
(n)-1 - Invalid (n) - Valid G00 Z-(z1+r1); G98 mode
G00 Z-z1; G99 mode
(1)
(2)
(3) (4) (5)
(6)
(7) (8)
(9)
(10)
(n) (n)
G98 G99
(n) -1
x1,y1
q1
q1
q1
r 1
z1
m
m
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
360IB-1501277-P
13.1.3.2 Small Diameter Deep Hole Drilling Cycle Command format
G83 Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Ii1 Pp1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Qq1 Cut amount for each cutting pass (incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Ii1 The feedrate from R point to the cutting start position, the speed (mm/min) for returning
from the hole bottom are stored only in the same block as G83, and it is valid until the small diameter deep hole drilling cycle is canceled. (It follows the setting of "#8085 G83S Forward F", "#8086 G83S Back F" when omitted.)
Pp1 Dwell time at hole bottom position
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
361 IB-1501277-P
"i1" follows the parameter "#8085 G83S Forward F" when there is no I command. "i2" follows the parameter "#8086 G83S Back F" when there is no I command.
Detailed description
c: Parameter "#8084 G83S Clearance" qs: Cut amount when small diameter deep hole
drilling cycle signal (YCCA) is input skip: Small diameter deep hole drilling cycle signal
(YCCA) input
Operation pattern Program
(1) G00 Xx1 Yy1,Ii1; (2) G00 Zr1; (3) G01 Zq1 Ff1; (4) G01 Z-q1 Fi2; (5) G01 Z(q1-c) Fi1; (6) G01 Z(q1+c) Ff1; (7) G01 Z-2q1 Fi2; (8) G01 Z(2q1-c) Fi1; (9) G01 Z(q1+c) Ff1;
(10) G01 Z-(2q1+qs) Fi2; (11) G01 Z(2q1+qs-c) Fi1; (12) G01 Z(z1-q1*n-qs) Ff1; (13) G01 Z-(z1+r1) Fi2; G98 mode
G01 Z-z1 Fi2; G99 mode
q1
c
x1,y1
r 1
z1
G98
(1)
(2)
(3) (4) (5)
(6) (7)
(8)
(9)
skip
(10)
(11)
q1 qS
G99
q1 c
c
(12)
(13) (13)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
362IB-1501277-P
In deep hole drilling, cutting and retract are repeated and the workpiece is machined multiple times. In addition, when PLC signals are input during cutting, the cutting for the time concerned is skipped. In this way, this cycle reduces the load applied to the tool.
The small-diameter deep-hole drilling cycle mode is established by designating the M code command that was set in the parameter "#8083 G83S mode M". If the G83 command is designated in this mode, the small-diameter deep-hole drilling cycle is executed. The mode is canceled by the following conditions. Designation of a fixed cycle cancel command (G80, G commands in Group 1) Resetting
It is not immediately switched to the small diameter deep hole drilling cycle mode even the small diameter deep hole drilling cycle switch M command is issued during G83 deep hole drilling cycle modal. Then, when G83 is command- ed, the small diameter deep hole drilling cycle mode is applied.
When the small diameter deep hole drilling cycle signal (YCCA) is input during the cutting operation (9), the remain- ing cutting command is skipped and the axis returns to the R point at the cutting speed "i2".
"In small diameter deep hole cycle signal (XCC1)" is output between the positioning to the R point of drilling axis (2) and the R point/initial point return after finishing the drilling (13).
"c" depends on the parameter "#8084 G83S Clearance".
Program the small diameter deep hole drilling cycle to make it "q1 > c".
The operation stops at after the (1), (2) and (13) commands during single block operation.
If there is no "I" command, or either the parameter "#8085 G83S Forward F" or "#8086 G83S Back F" is set to "0", a program error (P62) will occur.
Confirm the following related parameters before using the small hole diameter drilling cycle. #8083 G83S modeM #8084 G83S Clearance #8085 G83S Forward F #8086 G83S Back F
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
363 IB-1501277-P
13.1.4 Tapping Cycle; G84
(1) ",S" command is held as a modal information. When the value of the ",S" command is lower than the spindle rotation speed (S command), operations depend on the MTB specifications. (Whether it operates on the spindle rotation speed at the return or on the spindle rotation speed of S command is determined according to the parameter "#1241 set13/bit7" setting.) When the spindle speed at the return is not "0", the value of tap return override "#1172 tapovr" is invalid. When ",S" command is omitted or when ",S0" is commanded, the value of "spindle rotation speed at return" is obtained by the following formula.
((S command value) (setting value of the parameter "#1172 tapovr")) / 100
Command format
G84 Xx1 Yy1 Zz1 Rr1 Qq1 Ff1(Ee1) Pp1, Rr2 Ss1 ,Ss2 ,Ii1 ,Jj1 Ll1 (Kk1);
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Qq1 Cut amount for each cutting pass (incremental position) (modal) Ff1 During synchronous tapping: Designation of drilling axis feed amount (tapping pitch) per
spindle revolution (modal) During asynchronous tapping: Designation of the feedrate for cutting feed (modal)
Ee Cutting feedrate at synchronous tapping (Number of screw threads per inch) If this command is issued simultaneously with the F command, the F command is valid.
Pp1 Designation of dwell time at hole bottom position (the values after the decimal points will be ignored) (modal)
,Rr2 Synchronization method selection (r2=1: synchronous, r2=0: asynchronous) (When omitted, the mode will follow the setting of parameter "#8159 Synchronous tap")
Ss1 Spindle rotation speed command
(n:spindle number, *****: rotation speed) If an S command is issued during synchronous tapping modal, a program error
(P186) will occur. ,Ss2 Spindle rotation speed during return ,Ii1 Positioning axis in-position width ,Jj1 Drilling axis in-position width Ll1 Designation of number of repetitions (0 to 9999)
Not executed when "0" is set. Kk1 Number of repetitions (It can be commanded when the parameter "#1271 ext07/bit1" is
"1" )
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
364IB-1501277-P
When r2 = 1, the synchronous tapping mode will be applied, and when r2 = 0, the asynchronous tapping mode will be applied. If there is no r2 command, mode will follow the parameter setting.
When G84 is executed, the override will be canceled and automatically be set to 100%.
Dry run is valid for the positioning command when the control parameter "G00 DRY RUN" is ON. If the feed hold button is pressed during G84 execution, and the sequence is at (3) to (6), the movement will not stop immediately, and instead will stop after (6). During the rapid traverse in sequence (1), (2) and (9), the movement will stop imme- diately.
The operation stops at after the (1), (2) and (9) commands during single block operation.
During the G84 mode, the NC signal "Tapping" will be output.
During the G84 synchronous tapping modal, the M3, M4, M5 and S code will not be output.
When it is interrupted by such as the emergency stop during the tapping cycle, enable the "Tap retract" signal (TRV); a tool can be taken out from the workpiece by tap retract operation.
Detailed description
Normal tapping cycle (When Q is not designated)
Operation pattern i1 j1 Program
(1) Valid - G00 Xx1 Yy1; (2) - Invalid G00 Zr1; (3) - Invalid G01 Zz1 Ff1; (4) - - G04 Pp1; (5) - - M4; Spindle forward rotation (6) - Invalid G01 Z-z1 Ff1; (7) - - G04 Pp1; (8) - - M3; Spindle forward rotation (9) - Valid G00 Z-r1; G98 mode
No movement G99 mode
(4)(5)
r 1
z1
G98 G99
(1)
(2)
(3) (6) (6)
(9)
x1 , y1
(8) (7)(8) (7)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
365 IB-1501277-P
m : parameter (#8018 G84/G74 n)
This program is for the G84 command.
The spindle forward rotation (M3) and reverse rotation (M4) are reversed with the G74 command.
Pecking Tapping Cycle (When the Q command is designated #1272 ext08/bit4=0)
Operation pattern Program
(1) G00 Xx1 Yy1 ,Ii1; (2) G00 Zr1; (3) G01 Zq1 Ff1; (4) M4; Spindle reverse rotation (5) G01 Z-m Ff1; (6) M3 ; Spindle forward rotation (7) G01 Z(q1+m) Ff1; (8) M4; Spindle reverse rotation (9) G01 Z-m Ff1;
(10) M3 ; Spindle forward rotation (11) G01 Z(q1+m) Ff1;
: : (n1) G01 Z(z1-q1*n) Ff1; (n2) G04 Pp1; (n3) M4; Spindle reverse rotation (n4) G01 Z-z1 Ff1 Ss2; (n5) G04 Pp1; (n6) M3; Spindle forward rotation (n7) G00 Z-r1 ,Jj1; G98 mode
No movement G99 mode
(1)
(2)
(3)
(4) (5)
(6)
(7)
(8)
(9)
(10)
(11)
(n1)
(n2)(n3)
(n4) (n4)
(n5)(n6) (n5)(n6)
(n7) r 1
z1
G98 G99
q1
q1
q1
x1,y 1
m
m
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
366IB-1501277-P
The load applied to the tool can be reduced by designating the depth of cut per pass (Q) and cutting the workpiece to the hole bottom for a multiple number of passes. The amount retracted from the hole bottom is set to the param- eter "#8018 G84/G74 n". Whether the pecking tapping cycle or the deep-hole tapping cycle is valid depends on the MTB specifications (parameter "#1272 ext08/bit4"). When "depth of cut per pass Q" is designated in the block con- taining the G84 or G74 command with the pecking tapping cycle selected, the pecking tapping cycle will be execut- ed. In the following cases, the normal tapping cycle will be carried out. When Q is not designated. When the command value of Q is zero.
(R) R point
(1) This program is for the G84 command.
The spindle forward rotation (M3) and reverse rotation (M4) are reversed with the G74 command.
Deep-hole Tapping Cycle (When the Q command is designated #1272 ext08/bit4=1)
Operation pattern Program
(1) G00 Xx1 Yy1; (2) G00 Zr1; (3) G09 G01 Zq1 Ff1; (4) M4 ; Spindle reverse rotation (5) G09 G01 Z-q1 Ff1; (6) G04 Pp1; (7) M3; Spindle forward rotation (8) G09 G01 Z(2*q1) Ff1; (9) M4 ; Spindle reverse rotation
(10) G09 G01 Z-(2*q1) Ff1; (11) G04 Pp1; (12) M3; Spindle forward rotation (13) G09 G01 Z(3*q1) Ff1;
: : (n1) G09 G01 Zz1 Ff1; (n2) G04 Pp1;
(1)
r 1
z1
G98 G99
q1
x1,y 1
(R)
q1
q1
(2)
(3)
(4)
(5)
(6)(7)
(8)
(10)
(13)
(11)(12)
(9)
(n7)
(n5)(n6)
(n1) (n4) (n4)
(n2)(n3)
(n5)(n6)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
367 IB-1501277-P
(a) In the deep-hole tapping, the load applied to the tool can be reduced by designating the depth of cut per pass and cutting the workpiece to the hole bottom for a multiple number of passes. Under the deep-hole tapping cycle, the tool is retracted to the R-point every time.
(b) Whether the pecking tapping cycle or the deep-hole tapping cycle is valid depends on the MTB specifications (parameter "#1272 ext08/bit4"). When "depth of cut per pass Q" is designated in the block containing the G84 or G74 command in the state where the deep-hole tapping cycle is selected by parameter, the deep-hole tapping cycle is executed. In the following cases, the normal tapping cycle will be carried out. When Q is not designated. When the command value of Q is zero.
(c) When G84 is executed, the override will be canceled and the override will automatically be set to 100% in the cutting operation. And the override set in the parameter "#1172 tapovr" will also be disabled. (When "#1272 ext08/bit5" = 1, the setting of "#1172 tapovr" will be enabled only during a pulling operation)
(d) Dry run is valid for a positioning command when the parameter "#1085 G00 DRY RUN" is "1" and is valid for the positioning command. If the feed hold button is pressed during G84 execution, the tool does not stop immediately during cutting or returning, and it stops after completing an R point return.
(e) During single block operation, the tool does not stop during cutting or returning, but stops after completing an R point/initial point return.
(f) During the G84 mode, the NC signal "Tapping" will be output. (g) During the G84 synchronous tapping modal, the M3, M4, M5 and S code will not be output. (h) If the command value of F becomes extremely small such as around "F < 0.01 mm/rev" during synchronous tap-
ping, the spindle does not rotate smoothly. So make sure to command a value larger than "0.01 mm/rev". The unit of F can be selected between mm/rev and mm/min.
(i) If the external deceleration signal is turned ON during synchronous or asynchronous tapping, the feed rate does not change even when deceleration conditions are satisfied.
(j) If the operation is interrupted by a cause such as an emergency stop or reset during the deep-hole tapping cycle, a tap retract is executed when the tap retract signal is input.
(k) When the reference position return signal is input during the deep-hole tapping cycle, a tap retract is carried out, and a reference position return will be executed from the end point of the tap retract.
(n3) M4; Spindle reverse rotation (n4) G09 G01 Z-z1 Ff1; (n5) G04 Pp1; (n6) M3; Spindle forward rotation (n7) G00 Z-r1; G98 mode
No movement G99 mode
Operation pattern Program
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
368IB-1501277-P
This function enables to make spindle acceleration/deceleration pattern closer to that of the speed loop by dividing the spindle and drilling axis acceleration/deceleration pattern into up to three stages during synchronous tapping. The acceleration/deceleration pattern can be set up to three stages for each gear. (This depends on the MTB spec- ifications.) When returning from the hole bottom, rapid return is possible at the spindle rotation speed during return. The spindle rotation speed during return is held as modal information.
(1) When tapping rotation speed < spindle rotation speed during return synchronous tapping changeover spindle rotation speed 2
Spindle acceleration/deceleration pattern during synchronous tapping
S Command spindle rotation speed S' Spindle rotation speed during return S1 Tapping rotation speed (spindle specification parameters #3013 to #3016) S2 Synchronous tapping changeover spindle rotation speed 2 (spindle specification parameters #3037 to
#3040) S3 Maximum spindle rotation speed for synchronous tapping (spindle specification parameters #43046 to
#43049) However, when those parameters are set to "0", processing is performed based on "#3005" to "#3008". #3005 to #3008 can be designated using up to six digits (999999); however, they are limited to five digits (99999) for this function.
T1 Tapping time constant (spindle specification parameters #3017 to #3020) T2 Synchronous tapping changeover time constant 2 (spindle specification parameters #3041 to #3044)
S2 S3
S(S1)
S1 S' S2 S3
T1
T1T1
T1
T2
T2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
369 IB-1501277-P
(2) When synchronous tapping changeover spindle rotation speed 2 < spindle rotation speed during return
S Command spindle rotation speed S' Spindle rotation speed during return S1 Tapping rotation speed (spindle specification parameters #3013 to #3016) S2 Synchronous tapping changeover spindle rotation speed 2 (spindle specification parameters #3037 to
#3040) S3 Maximum spindle rotation speed for synchronous tapping (spindle specification parameters #43046 to
#43049) However, when those parameters are set to "0", processing is performed based on "#3005" to "#3008". #3005 to #3008 can be designated using up to six digits (999999); however, they are limited to five digits (99999) for this function.
T1 Tapping time constant (spindle specification parameters #3017 to #3020) T2 Synchronous tapping changeover time constant 2 (spindle specification parameters #3041 to #3044) T3 Synchronous tapping changeover time constant 3 (spindle specification parameters #3045 to #3048)
S3 S2
S(S1)
S1 S2
S'(S3)
T1
T2 T1T1
T1
T2
T3
T3
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
370IB-1501277-P
The feedrates for the tapping cycle and tapping return are as shown below.
(1) Selection of synchronous tapping cycle/asynchronous tapping cycle
"-" is irrelevant to the setting
(2) Selection of asynchronous tapping cycle feedrate
"-" is irrelevant to the setting
(3) Spindle rotation speed during return of synchronous tapping cycle
The M code set with the parameter "#3028 sprcmm" is output as the M code for spindle forward/reverse rotation that is output at "hole bottom" or at "R point" during asynchronous tapping cycle. Note that the M code for forward rotation is output as "M3" and that for reverse rotation is as "M4" if the parameter "#3028 sprcmm" is set to "0".
Feedrate for tapping cycle and tapping return
Program G84, Rxx
Control parameter Synchronous tapping
Synchronous/asynchronous
,R00 - Asynchronous ,Rxx
No designation OFF ON Synchronous
,R01 -
G94/G95 Control parameter F1-digit valid
F command value Feed designation
G94 OFF F designation Feed per minute ON Other than F0 to F8
F0 to F8 (no decimal point)
F1-digit Feed
G95 - F designation Feed per revolution
Address Meaning of ad- dress
Command range (unit)
Remarks
,S Spindle rotation speed during return
0 to 99999 (r/min) The data is held as modal information. If the value is smaller than the spindle ro- tation speed, the spindle rotation speed value will be valid even during return. If the spindle rotation speed is not 0 during return, the taping retract override value will be invalid.
M code for forward/reverse rotation command in asynchronous tapping cycle
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
371 IB-1501277-P
Enable the feed per minute command of the synchronous tapping by the setting of parameter "#1268 ext04/bit2". When this parameter is valid, G94 and G95 modal will be applied.
(*1) The F command is set to feed per minute (mm/min, inch/min).
Pitch = F command value / S command value
(*2) The F command is set to feed per revolution (mm/rev, inch/rev).
(1) The G94 command, which is a modal command, is valid until the G95 (feed per revolution) command is issued next.
(2) If the E address (number of screw threads per inch) is issued while feed per minute is valid, the program error (P32) will occur.
(3) The F address of the synchronous tapping command does not affect the F modal for cutting feed.
You can restrict the maximum value (minimum value of the E address for the number of screw threads) of the pitch F address for synchronous tapping (parameter "#19004 tap feedrate limit"). The program error (P184) will occur if the machining program is executed when the value of "F" address (pitch) exceeds the maximum value or when the value of "E" address (number of the screw threads per inch) is below the minimum value. When the parameter "#19004" is set to "0", the pitch command by the F address is set as follows.
(*1) When feed per minute is commanded, the pitch calculation result for the spindle rotation speed is range-restrict- ed in this parameter setting.
Feed per minute command of the synchronous tapping
During G94 modal (feed per minute) During G95 modal (feed per revolution)
#1268/bit2 = 1 Feed per minute (*1) Feed per revolution (*2) #1268/bit2 = 0 Feed per revolution (*2) Feed per revolution (*2)
Range restriction of maximum cutting feedrate command for synchronous tapping
Command unit Pitch F E setting (number of screw threads) (*1)
B (0.001mm) 0.001 to 999.999 mm/rev 0.0255 to 999.99 screw threads/inch C (0.0001mm) 0.0001 to 999.9999mm/rev 0.026 to 999.999 screw threads/inch D (0.00001mm) 0.00001 to 999.99999 mm/rev 0.0255 to 999.9999 screw threads/inch E (0.000001mm) 0.000001 to 999.999999 mm/rev 0.02541 to 999.99999 screw threads/inch B (0.0001inch) 0.000001 to 39.370078inch/rev 0.03 to 9999.9999 screw threads/inch C (0.00001inch) 0.0000001 to 39.3700787inch/rev 0.026 to 9999.99999 screw threads/inch D (0.000001inch) 0.00000001 to 39.37007874inch/rev 0.0255 to 9999.999999 screw threads/
inch E (0.0000001inch) 0.000000001 to 39.370078740inch/rev 0.02541 to 9999.9999999 screw threads/
inch
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
372IB-1501277-P
(*1) Carry out in-position check by tapping in-position width.
(1) The I point refers to the initial point.
Synchronous tapping in-position check (Parameter setting values and tapping axis movement)
#1223 aux07 "P" designation of G84/ G74 command
In-position check during synchronous tap- pingbit3 bit4 bit5 bit2
Synchronous tap in-posi-
tion check im- provement
Hole bottom
R point I point -> R point
Hole bottom R point I point -> R point
0 - - - - yes yes yes 1 - - - No "P" designation
Example: G84 F1. Z-5. S1000 R-5.
no no no
1 1 1 1 "P" designation Example: G84 F1. Z-5.
S1000 P0 R-5.
(*1) yes yes
1 1 0 1 "P" designation Example: G84 F1. Z-5.
S1000 P0 R-5.
(*1) no yes
1 0 1 1 "P" designation Example: G84 F1. Z-5.
S1000 P0 R-5.
yes yes yes
1 0 0 1 "P" designation Example: G84 F1. Z-5.
S1000 P0 R-5.
no no yes
1 1 1 0 "P" designation Example: G84 F1. Z-5.
S1000 P0 R-5.
(*1) yes no
1 1 0 0 "P" designation Example: G84 F1. Z-5.
S1000 P0 R-5.
(*1) no no
1 0 1 0 "P" designation Example: G84 F1. Z-5.
S1000 P0 R-5.
no yes no
1 0 0 0 "P" designation Example: G84 F1. Z-5.
S1000 P0 R-5.
no no no
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
373 IB-1501277-P
In-position width and tapping axis movement for a synchronous tapping in-position check
(a) In-position completion of the G00 feed from the R point (b) G01 deceleration start at tapping cut-in (c) G01 deceleration start at tapping return (d) Start of G00 feed to the R point
(1) Section in which the in-position check is carried out by G0inps. (2) Section in which the in-position check is carried out by TapInp. (3) Section in which the in-position check is carried out by G1inps. (4) Section in which the in-position check is carried out by sv024.
R point: In-position check by the G1inps
I point: In-position check by the G0inps
Hole bottom: In-position check by the TapInp
(Z) Hole bottom (R) R point
FIN
(1) (2) (3) (4)
(Z) (R) (d) (c)(b)(a)(F)
(T)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
374IB-1501277-P
Relation between the parameter setting values and tapping axis movement for a synchronous tapping in-position check
(1) The I point refers to the initial point. (2) Note that vibration or deterioration in accuracy may occur when invalidating the in-position check at R point. Con-
firm the accuracy when invalidating it. Processing may take some time if no in-position check is performed at each point.
#1223 aux07 Hole bottom wait time Operation at hole bottom
Operation at R point
Operation at I point -> R pointbit3 bit4 bit5 bit2
Synchronous tap in-posi-
tion check im- provement
Hole bot- tom
R point
I point -> R point
0 - - - Time designated by "P" Several 10 ms as process- ing time when no "P".
Operation deter- mined by setting of inpos (#1193) and aux07 (#1223/bit1) pa- rameters.
Operation deter- mined by setting of inpos (#1193) and aux07 (#1223/bit1) pa- rameters.
Operation deter- mined by setting of inpos (#1193) and aux07 (#1223/bit1) pa- rameters.
1 0 0 1 The larger value of "P" and TapDwl (#1313) is valid. No dwell is executed if both values are "0".
Wait until time in the left column elapses.
Wait until comple- tion of in-position check by G0inps.
1 0 1 1 The larger value of "P" and TapDwl (#1313) is valid. No dwell is executed if both values are "0".
Wait until time in the left column elapses.
Wait until comple- tion of in-position check by G1inps.
Wait until comple- tion of in-position check by G0inps.
1 1 0 1 The larger value of "P" and TapDwl (#1313) is valid. No dwell is executed if both values are "0".
Wait until dwell time in the left col- umn elapses after completion of in- position check.
Wait until comple- tion of in-position check by G0inps.
1 1 1 1 The larger value of "P" and TapDwl (#1313) is valid. Several 10 ms as process- ing time when both of them are "0".
Wait until dwell time in the left col- umn elapses after completion of in- position check.
Wait until comple- tion of in-position check by G1inps.
Wait until comple- tion of in-position check by G0inps.
1 0 0 0 The larger value of "P" and TapDwl (#1313) is valid. No dwell is executed if both values are "0".
Wait until time in the left column elapses.
1 0 1 0 The larger value of "P" and TapDwl (#1313) is valid. No dwell is executed if both values are "0".
Wait until time in the left column elapses.
Wait until comple- tion of in-position check by G1inps.
1 1 0 0 The larger value of "P" and TapDwl (#1313) is valid. No dwell is executed if both values are "0".
Wait until dwell time in the left col- umn elapses after completion of in- position check.
1 1 1 0 The larger value of "P" and TapDwl (#1313) is valid.
Wait until dwell time in the left col- umn elapses after completion of in- position check.
Wait until comple- tion of in-position check by G1inps.
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
375 IB-1501277-P
This function allows you to carry out tapping by selecting and moving the drilling axis with manual handle operation after performing block stop or feed hold stop processing during synchronous tapping cycle. Whether to synchronize the drilling axis for manual synchronous tapping with the spindle when moving it depends on the MTB specifications. (Parameter "#11030 Man tap sync cancl") Designate this command in the same format as for synchronous tapping.
[Operation procedure]
The following example shows the procedure when the parameter "#11030 Man tap sync cancl" is set to "0".
(1) Execute the synchronous tapping cycle program in the MDI mode. G91 G84 X0 Y0 Z0 R0 F2. S1000;
(2) Set to the handle mode. (3) Determine the drilling position using the X/Y axis handle. (4) Perform drilling using the drilling axis handle. (5) Perform pulling out from the home bottom using the drilling axis handle. (6) When continuing machining, return to step (4). (7) Reset the G84 modal.
[Precautions and restrictions]
(1) The manual synchronous tapping is only required in the handle mode. (2) If necessary, you can perform the manual synchronous tapping using the handle after switching to another op-
eration mode until it is reset or canceled with the G80 command. (3) The spindle is synchronized in the pitch commanded with "F" of machining program G84 (G74).
(Example) N1 G28 X0 Y0 Z0 ; N2 G91 G01 F1000 ; N3 G84 X-50. Y-50. Z-100. R-50. F2. S1000. ,R1 ; N4 G80 M02 ; When the handle is turned while the handle magnification is set to "100", the Z axis moves synchronously with the spindle. "2mm/rev" is set to the F2 command, so the spindle rotates by one revolution when the handle is turned by 20 pulses.
(4) For manual synchronous tapping, the acceleration/deceleration time constant is the same as for the normal han- dle operation. Also, the tap return override is invalid.
(5) The spindle rotation speed for manual synchronous tapping is not clamped with parameters "#3013 stap1" to "#3016 stap4" (maximum tapping rotation speed) in the S command of the program.
(6) Manual synchronous tapping becomes valid from the timing when block stop or feed hold stop mode is set during automatic operation. However, the feed hold stop mode during cutting is changed to the block stop mode after "cutting -> movement to R point".
(7) The dwell time (P command) at the hole bottom is invalid during manual synchronous tapping. (8) When the automatic operation is started in the miscellaneous function lock ("MST lock" ON), the spindle is not
synchronized even after block stop or feed hold stop processing has been ended. (9) The manual synchronous tapping operation in 3-dimensional coordinate conversion is different from the above.
(Not supported.)
Manual synchronous tapping
Depends on the parameter (#11030) setting. OFF: Synchronizes with the spindle (tapping). ON: Does not synchronize with the spindle (positioning).
Z
X
Spindle
Step (3)
Step (4)Step (5)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
376IB-1501277-P
This function performs tapping using the analog-connected spindle. By using this function, various tapping cycle functions can be used using the analog-connected spindle by inverter, etc.
When this function is used, the analog spindle with the function to control the spindle position needs to be connected. Also, the parameter "#1295 ext31/bit6" (Analog spindle synchronous tapping ON) needs to be set to "1".
The voltage value to be output to the analog spindle is between -10V and 10V and it is determined by the ratio of the setting value of the parameters "#3001 slimit1" to "#3004 slimit4" which correspond to the command to the an- alog spindle.
[Relationship with other functions]
(1) The following function cannot be combined with the analog spindle synchronous tapping. If the analog spindle synchronous tapping is commanded while the following function is used, the program error (P182) occurs. Coordinate rotation by program 3-dimensional coordinate conversion Parameter coordinate conversion Inclined surface machining Workpiece installation error compensation R-Navi Mixed control Arbitrary axis exchange control
(2) When the reset or emergency stop is performed during the execution of the synchronous tapping with analog I/ F spindle, the tap retract can be used as well as the normal synchronous tapping. However, when the emergency stop is canceled before commanding the tapping retract, the analog I/F spindle needs to be ready to rotate by a voltage command from the NC.
[Precautions]
(1) The pecking tapping cycle or deep-hole tapping cycle cannot be commanded while the analog spindle synchro- nous tapping is used. If commanded, a program error (P182) occurs.
(2) The synchronous tap with multi-step acceleration deceleration cannot be used while the analog spindle synchro- nous tapping is used. Command by setting the parameter "#1223 aux07/bit7" (Synchronous tap method) to "1".
(3) The high-speed synchronous tapping cannot be used while the analog spindle synchronous tapping is used. Re- gardless of the value of the parameter "#1281 ext17/bit5" (High-speed synchronous tapping valid), the normal synchronous tapping operation is performed.
(4) If the synchronous tapping is commanded to the analog spindle in multiple spindle control mode when the pa- rameter "#1295 ext31/bit6" (Analog spindle synchronous tapping ON) is set to "0", the following error occurs. In multiple-spindle control I mode: Program error (P182) In multiple-spindle control II mode: Operation error (M01 0054)
(5) The analog spindle synchronous tapping can be used only in one part system. In multiple spindle control mode, if the analog spindle synchronous tapping is performed in the part system other than the one where the param- eter "#11717 astap_sysno" (Analog spindle synch tap: Part system selection) is set, the following errors occur. In multiple-spindle control I mode: Program error (P182) In multiple-spindle control II mode: Operation error (M01 0054)
(6) When multiple spindles are selected using the multiple spindle control, do not command the synchronous tapping with the analog-connected spindle and the serial-connected spindle being mixed.
(7) With the analog spindle synchronous tapping, the synchronous tapping error display function is disabled and the synchronous tapping error display always shows "0".
(8) When the reset or emergency stop is performed during analog spindle synchronous tapping, the voltage output value to the spindle becomes "0" and the spindle operation stops.
Synchronous tapping with analog I/F spindle (analog spindle synchronous tapping)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
377 IB-1501277-P
This function performs tapping using the spindle controlled with pulse train output. By using this function, various tapping cycle functions can be used using the spindle connected to the inverter, etc.
When this function is used, the inverter, etc. which supports the function to control the spindle operation with the pulse train input needs to be connected. Also, the parameter "#1295 ext31/bit6" (Analog spindle synchronous tap- ping ON) needs to be set to "1".
[Relationship with other functions]
(1) The following functions cannot be combined with the synchronous tapping using the pulse-train output spindle. If the synchronous tapping using the pulse-train output spindle is commanded while the following function is used, the program error (P182) occurs. Coordinate rotation by program
(2) When the reset or emergency stop is performed during the execution of the synchronous tapping with pulse train output, the tap retract can be used as well as the normal synchronous tapping. However, when the emergency stop is canceled before commanding the tapping retract, the connected inverter spindle needs to be ready to rotate by the pulse train output from the NC.
(3) Spindle selection can be performed for the pulse-train output spindle by multiple-spindle control. However, to use encoder input, set the pulse-train output spindle to the 1st spindle.
[Precautions]
(1) The pecking tapping cycle or deep-hole tapping cycle cannot be commanded for the synchronous tapping using the pulse-train output spindle. If commanded, the program error (P182) occurs.
(2) The synchronous tap with multi-step acceleration deceleration cannot be used for the synchronous tapping using the pulse-train output spindle. Regardless of the value of the parameter "#1223 aux07/bit7" (Synchronous tap method), the acceleration/deceleration operation for synchronous tapping is performed in the conventional meth- od.
(3) The high-speed synchronous tapping cannot be used for the synchronous tapping using the pulse-train output spindle. Regardless of the value of the parameter "#1281 ext17/bit5" (High-speed synchronous tapping valid), the normal synchronous tapping operation is performed.
(4) If the synchronous tapping is commanded to the pulse-train output spindle in multiple-spindle control mode when the parameter "#1295 ext31/bit6" (synchronous tapping with analog I/F spindle ON) is set to "0", the following error occurs. In multiple-spindle control I mode: Program error (P182) In multiple-spindle control II mode: Operation error (M01 0054)
(5) The synchronous tapping error display function is disabled for the synchronous tapping using the pulse-train out- put spindle, and the synchronous tapping error display always shows "0".
(6) If the reset or emergency stop is performed during the synchronous tapping using the pulse-train output spindle, the controller stops outputting pulse signals to the spindle.
(7) For the spindle control with pulse train output, a different acceleration/deceleration control method is used at spindle rotation command and synchronous tapping, compared to the normal spindle control. Therefore, to op- erate a program that transitions from the spindle rotation command to the synchronous tapping command, wait until the spindle has sufficiently slowed down, and issue the synchronous tapping command.
(8) If reset is performed during forward rotation or reverse rotation of pulse-train output spindle, the pulse train will not stop being output, and the spindle remains rotated. However, if an emergency stop is performed during for- ward rotation or reverse rotation, the controller stops outputting pulse signals to the spindle.
Synchronous tapping by spindle control with pulse train output
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
378IB-1501277-P
13.1.5 Boring; G85
The operation stops at after the (1), (2), (4) or (5) commands during single block operation.
Command format
G85 Xx1 Yy1 Zz1 Rr1 Ff1 Ll1 ,Ii1 ,Jj1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Ll1 Designation of number of repetitions (0 to 9999)
When 0 is set, processing is not executed. ,Ii1 Positioning axis in-position width ,Jj1 Drilling axis in-position width
Detailed description
Operation pattern i1 j1 Program
(1) Valid - G00 Xx1 Yy1; (2) - Invalid G00 Zr1; (3) - Invalid G01 Zz1 Ff1; (4) - Invalid G01 Z-z1 Ff1; (5) - Invalid G00 Z-r1; G98 mode
No movement G99 mode
r1
z1
G98 G99
(1)
(2)
(3) (4) (4)
(5)
x1 , y1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
379 IB-1501277-P
13.1.6 Boring; G86
The operation stops at after the (1), (2) and (7) commands during single block operation.
Command format
G86 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1 Ll1 ;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Pp1 Designation of dwell time at hole bottom position (the values after the decimal points will
be ignored) (modal) Ll1 Designation of number of repetitions (0 to 9999)
When 0 is set, processing is not executed.
Detailed description
Operation pattern Program
(1) G00 Xx1 Yy1; (2) G00 Zr1; (3) G01 Zz1 Ff1; (4) G04 Pp1; (5) M5; Spindle stop (6) G00 Z-(z1+r1); G98 mode
G00 Z-z1; G99 mode (7) M3; Spindle forward rotation
(4)(5) G98 G99
(1)
(2)
(3) (6)
(7)
x1 , y 1
z1 (6)
r 1
(7)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
380IB-1501277-P
13.1.7 Back Boring; G87
(1) Be careful of the designation of "z1" and "r1" (the sign of "z1" is opposite to that of "r1"). Also, the R point return is not performed.
Command format
G87 Xx1 Yy1 Zz1 Rr1 Iq1 Jq2 Kq3 Ff1 Ll1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Iq1 Jq2 Kq3
Designation of shift amount (incremental position) (modal) The command address for each plane selection is as follows. When G17 plane is selected: IJ When G18 plane is selected: KI When G19 plane is selected: JK Depending on the parameter setting, the shift amount can be designated by Q address. Refer to "Designation of shift amount (I,J,K)".
Ff1 Designation of feedrate for cutting feed (modal) Ll1 Designation of number of repetitions (0 to 9999)
Not executed when "0" is set.
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
381 IB-1501277-P
The operation stops at after the (1), (4), (6) and (11) commands during single block operation.
Detailed description
Operation pattern Program
(1) G00 Xx1 Yy1; (2) M19 ; Spindle orientation (3) G00 Xq1 (Yq2) ; Shift (4) G00 Zr1; (5) G00 X-q1(Y-q2)/G01 X-q1(Y-q2)Ff1 ; Shift (6) M3; Spindle forward rotation (7) G01 Zz1 Ff1; (8) M19 ; Spindle orientation (9) G00 Xq1 (Yq2); Shift
(10) G00 Z-(r1+z1); G98 mode G00 Z-(r1+z1); G99 mode
(11) G00 X-q1(Y-q2); Shift (12) M3; Spindle forward rotation
(1)
r 1
Xq1(Yq2)(3)
(2) (12)(11)
(8) (9) (10)
(4)
(7)
(6) (5)
z1
x1 , y1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
382IB-1501277-P
When this command is issued, high precision drilling machining that does not scratch the machining surface can be done. Positioning to the hole bottom and escaping (return) after cutting are carried out in the state shifted to the di- rection opposite of the cutter. (The bold arrow shown in the figure indicates the tool shift amount.)
Whether the tool moves by the designated shift amount (*1) with rapid traverse (G00) or linear interpolation (G01) depends on the MTB specifications (parameter "#1255 set27/bit4").
(*1) Refers to the movement using operation pattern (5) shown in the figure in "Detailed description". When the rapid traverse is selected, the route at positioning is set to the interpolation type regardless of the setting of the parameter "#1086 G0Intp". When the linear interpolation is selected, the feedrate follows the F command.
(1) To move the tool by the designated shift amount with rapid traverse, it is necessary to upgrade the M8 series software to version C4 or later and to replace the fixed cycle program. For details, consult the MTB.
(2) Command I, J, and K with incremental positions in the same block as the hole position data. I, J and K will be handled as modal during the fixed cycle.
(3) If the parameter "#1080 Dril_Z" which fixes the hole drilling axis to the Z axis is set, the shift amount can be des- ignated with address Q instead of I, J. In this case, whether to shift or not and the shift direction are set with parameter "#8207 G76/87 No shift" and "#8208 G76/87 Shift (-)". The sign for the Q value is ignored and the value is handled as a positive value. The Q value is a modal during the fixed cycle. Then, be sure to note that the Q value is commonly used for the cutting amount with G73/G83 or the shift amount with G83/G87.
Designation of shift amount (I,J,K)
A: Tool position during cutting B: Tool position when positioning to the hole bottom and, also, when escaping after cutting
A B
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
383 IB-1501277-P
Whether the tool node shift is performed in the commanded coordinate system or machine coordinate system de- pends on the MTB specifications (parameter "#1751 cfgPR01/bit1"). When the plane perpendicular to the tool axis is assigned to the rotation coordinate system by the G68 command (coordinate rotation by program), etc., the shift direction is set as shown below depending on the setting value.
The figure below shows the shift direction when the X-Y plane perpendicular to the Z axis (tool axis) is rotated.
(1) In order to switch the coordinate system to shift the tool nose, the system must be upgraded to the M8 series S/ W version E1 or later, and then the fixed cycles need to be replaced. Contact the MTB to use this function.
(2) When the plane including the tool axis is rotated, shift the tool nose in the commanded coordinate system re- gardless of the setting of the parameter "#1751 cfgPR01/bit1".
(3) The tool nose shift in the mirror image ON state is performed in the mirror image OFF state; therefore, the tool nose shifts to the tool nose direction regardless of the setting of the parameter "#1751 cfgPR01/bit1". However, the shift direction is designated based on the parameter setting when: The coordinate rotation is commanded in the mirror image ON state. Mirror image is turned ON during the coordinate rotation command.
(4) When the machine coordinate system is set (#1751 cfgPR01/bit1 = 1), do not use the figure rotation simultane- ously.
Coordinate system at tool node shift
Shifted in the commanded coordinate system. (#1751 cfgPR01/bit1 = 0)
Shifted in the machine coordinate system (in the same direction as the tool nose). (#1751 cfgPR01/bit1 = 1)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
384IB-1501277-P
13.1.8 Boring; G88
The operation stops at after the (1), (2), (6) and (9) commands during single block operation.
Command format
G88 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1 Ll1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Pp1 Designation of dwell time at hole bottom position (the values after the decimal points will
be ignored) (modal) Ll1 Designation of number of repetitions (0 to 9999)
When 0 is set, processing is not executed.
Detailed description
Operation pattern Program
(1) G00 Xx1 Yy1; (2) G00 Zr1; (3) G01 Zz1 Ff1; (4) G04 Pp1; (5) M5; Spindle stop (6) Stop when single block stop switch is ON (7) Automatic start switch ON (8) G00 Z-(z1+r1); G98 mode
G00 Z-z1; G99 mode (9) M3 ; Spindle forward rotation
(4)(5)(6)(7) G98 G99
(1)
(2)
(3) (8)
(9)
x1 , y1
z1 (8)
r 1
(9)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
385 IB-1501277-P
13.1.9 Boring; G89
The operation stops at after the (1), (2), (5) or (6) commands during single block operation.
Command format
G89 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1 Ll1 ,Ii1,Jj1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Pp1 Designation of dwell time at hole bottom position (the values after the decimal points will
be ignored) (modal) Ll1 Designation of number of repetitions (0 to 9999)
When 0 is set, processing is not executed. ,Ii1 Positioning axis in-position width ,Jj1 Drilling axis in-position width
Detailed description
Operation pattern i1 j1 Program
(1) Valid - G00 Xx1 Yy1; (2) - Invalid G00 Zr1; (3) - Invalid G01 Zz1 Ff1; (4) - - G04 Pp1; (5) - Invalid G01 Z-z1 Ff1; (6) - Valid G00 Z-r1; G98 mode
No movement G99 mode
(4)
r 1
z1
G98 G99
(1)
(2)
(3) (5) (5)
(6)
x1 , y1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
386IB-1501277-P
13.1.10 Stepping Cycle; G73
Command format
G73 Xx1 Yy1 Zz1 Qq1 Rr1 Ff1 Pp1 Ll1 ,Ii1 ,Jj1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Qq1 Cut amount for each cutting pass (incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Ff1 Designation of feedrate for cutting feed (modal) Pp1 Designation of dwell time at hole bottom position (the values after the decimal points will
be ignored) (modal) Ll1 Designation of number of repetitions (0 to 9999)
When 0 is set, processing is not executed. ,Ii1 Positioning axis in-position width ,Jj1 Drilling axis in-position width
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
387 IB-1501277-P
When executing a second and following cutting in the G73 as shown above, the movement will return several "m" mm with rapid traverse and then will change to cutting feed. The return amount "m" will differ according to the pa- rameter "#8012 G73 return". The operation stops at after the (1), (2) and (n) commands during single block operation.
Detailed description
Operation pattern i1 j1 Program
(1) Valid - G00 Xx1 Yy1; (2) - Invalid G00 Zr1; (3) - Invalid G01 Zq1 Ff1; (4) - - G04 Pp1; (5) - Invalid G00 Z-m; (6) - Invalid G01 Z(q1+m) Ff1; :
(n)-1 - Invalid (n) - Valid G00 Z-(z1+r1); G98 mode
G00 Z-z1; G99 mode
(1)
(2)
(3)
(4)
x1 , y1
z1
r 1
(5) (6)
q1
q1
q1
(n)
m
(n) - 1
(n)
G98 G99
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
388IB-1501277-P
13.1.11 Reverse Tapping Cycle; G74
(1) When asynchronous tapping mode is applied, F address becomes the cutting feed speed.
Command format
G74 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1 ,Rr2 Ss1 ,Ss2 Ll1 ,Ii1,Jj1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Ff1 Z-axis feed amount (tapping pitch) per spindle rotation (modal) Pp1 Designation of dwell time at hole bottom position (the values after the decimal points will
be ignored) (modal) ,Rr2 Synchronization method selection (r2=1 synchronous, r2=0 asynchronous) (modal)
(When omitted, the mode will follow the setting of parameter "#8159 Synchronous tap") Ss1 Spindle rotation speed command
(n:spindle number, *****: rotation speed) If an S command is issued during synchronous tapping modal, a program error
(P186) will occur. ,Ss2 Spindle rotation speed during return Ll1 Designation of number of repetitions (0 to 9999)
When 0 is set, processing is not executed. ,Ii1 Positioning axis in-position width ,Jj1 Drilling axis in-position width
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
389 IB-1501277-P
When r2 = 1, the synchronous tapping mode will be applied, and when r2 = 0, the asynchronous tapping mode will be applied. If there is no r2 command, mode will follow the parameter setting. When G74 is executed, the override will be canceled and the override will automatically be set to 100%. Dry run is valid for the positioning command when the parameter "#1085 G00 Drn" is set to "1". If the feed hold button is pressed during G74 execution, and the sequence is at (3) to (6), the movement will not stop immediately, and instead will stop after (6). During the rapid traverse in sequence (1), (2) and (9), the movement will stop immediately. The operation stops at after the (1), (2) and (9) commands during single block operation. During the G74 and G84 modal, the "Tapping" NC output signal will be output. During the G74 synchronous tapping modal, the M3, M4, M5 and S code will not be output.
Refer to "13.1.4 Tapping Cycle; G84".
Refer to "13.1.4 Tapping Cycle; G84".
Refer to "13.1.4 Tapping Cycle; G84".
Refer to "13.1.4 Tapping Cycle; G84".
Detailed description
Operation pattern i1 j1 Program
(1) Valid - G00 Xx1 Yy1; (2) - Invalid G00 Zr1; (3) - Invalid G01 Zz1 Ff1; (4) - - G04 Pp1; (5) - - M3; Spindle forward rotation (6) - Invalid G01 Z-z1 Ff1; (7) - - G04 Pp1; (8) - - M4; Spindle reverse rotation (9) - Valid G00 Z-r1; G98 mode
No movement G99 mode
Spindle acceleration/deceleration pattern during synchronous tapping
Feedrate for tapping cycle and tapping return
M code for forward/reverse rotation command in asynchronous tapping cycle
Parameter setting values and tapping axis
(4)(5)
r 1
z1
G98 G99
(1)
(2)
(3) (6) (6)
(9)
x1 ,y1
(8) (7)(8)
(7)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
390IB-1501277-P
13.1.12 Circular Cutting; G75
Circular cutting starts with the X and Y axes positioned at the center of the circle, and the Z axis cuts into the com- manded position. Then, the tool cuts the inner circumference of the circle drawing a true circle and returns to the center position.
Function and purpose
Command format
G75 Xx1 Yy1 Zz1 Rr1 Qq1 Pp1 Ff1 Ll1 ;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Qq1 Radius of outer circumference (modal) Pp1 Tool radius compensation No. (modal) Ff1 Designation of feedrate for cutting feed (modal) Ll1 Designation of number of repetitions (0 to 9999)
When 0 is set, processing is not executed.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
391 IB-1501277-P
The operation stops at after the (1), (2) and (6) commands during single block operation.
Detailed description
Operation pattern Program
(1) G00 Xx1 Yy1; (2) G00 Zr1; (3) G01 Zz1 Ff1; (4) Gn X-(q1-r) I-(q1/2); Inner circumference half
circle n:q1 0 G02
q1 <0 G03 r: Tool radius compensation amount of the No. commanded with p1.
(5) Iq1; Outer circumference (6) X(q1-r) I(q1/2); Inner circumference half
circle (7) G00 Z-(z1+r1); G98 mode
G00 Z-z1; G99 mode
(4)
G98 G99
(1)
(2)
(3)
(6)
(7)
x1 , y1
z1
r 1
(5)
(7)
r
q1
Y
X
Z
X
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
392IB-1501277-P
13.1.13 Fine Boring; G76
Command format
G76 Xx1 Yy1 Zz1 Rr1 Iq1 Jq2 Kq3 Ff1 Ll1;
Xx1 Designation of hole drilling position (absolute/incremental position) Yy1 Designation of hole drilling position (absolute/incremental position) Zz1 Designation of hole bottom position (absolute/incremental position) (modal) Rr1 Designation of R point position (absolute/incremental position) (modal) Iq1 Jq2 Kq3
Designation of shift amount (incremental position) (modal) The command address for each plane selection is as follows: G17 plane: IJ G18 plane: KI G19 plane: JK Depending on the parameter setting, the shift amount can be designated by Q address. Refer to "Designation of shift amount (I,J,K)".
Ff1 Designation of feedrate for cutting feed (modal) Ll1 Designation of number of repetitions (0 to 9999) When 0 is set, processing is not ex-
ecuted.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
393 IB-1501277-P
The operation stops at after the (1), (2) and (7) commands during single block operation.
Refer to "Designation of shift amount (I,J,K)" in "13.1.7 Back Boring; G87".
Refer to "Coordinate system at tool nose shift" in "13.1.7 Back Boring; G87".
Detailed description
Operation pattern Program
(1) G00 Xx1 Yy1; (2) G00 Zr1; (3) G01 Zz1 Ff1; (4) M19; Spindle orientation (5) G00 Xq1(Yq2)/G01 Xq1(Yq2)Ff1 ; shift (6) G00 Z-(z1+r1); G98 mode
G00 Z-z1; G99 mode (7) G00 X-q1 (Y-q2); shift (8) M3; Spindle forward rotation
Designation of shift amount (I,J,K)
Coordinate system at tool nose shift
(4)(5) G98 G99
(1)
(2)
(3) (6)
(7)
x1 , y1
z1(6)
r 1
(7)
(8)
(8)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
394IB-1501277-P
13.1.14 Thread Milling Cycle; G187
This function is a fixed cycle that performs thread machining by helicoidally operating the tool referred to as a thread milling tool. This function allows a thick female thread cutting or female thread cutting in any pitch that is impossible using a tapping tool. This function is a fixed cycle using circular interpolation (helical interpolation); therefore, plane selection is required in advance.
Function and purpose
Command format
G187 Z__ I/J__ P__ F__ D__ Q__ ;
Z Designation of pole bottom position I/J Arc radius, approach direction P Pitch F Feedrate D Rotation direction Q Dwell time
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
395 IB-1501277-P
Detailed description
Detailed address setting
Address Command range (unit)
Remarks
Z -99999.999 to 99999.999 (mm)
Designate the hole bottom position. If an axis other than the drilling axis is commanded or the address is omit-
ted, a program error (P33) will occur. I/J -99999.999 to
99999.999 (mm) Designate the arc radius and approach direction. The approach direction can be designated with the address I/J and the sign of the commanded value.
(Example) If "J-5" is designated, the radius and direction are obtained as shown below. Arc radius: 5 (mm) Approach direction: -Y direction
Designate the radius for helical operation, not the hole radius. For the arc radius, designate a radius value. A program error (P33) will oc-
cur in the following cases. The drilling axis direction (K) has been designated. The command has been omitted, or two axes have been commanded si-
multaneously. The command value is set to "0".
P 0.001 to 99999.999 (mm)
Designate the pitch (drilling axis feed amount per revolution). For the pitch, designate a radius value. If the command is omitted, a program error (P33) occurs. If the command value is set to "0", a program error (P35) occurs.
F 0.001 to 10000000 (mm/min)
Designate the feedrate. Designate the helical operation speed, not the cutting speed. The normal F modal value will not change. If the command is omitted or the command value is set to "0", a program
error (P62) occurs. In the same way as for the normal helical interpolation, the speed desig-
nation is selected by the parameter "#1235 set07/bit0". (Based on the MTB specifications.)
D 0, 1 Designate the rotation direction. 0: CW 1: CCW If the command is omitted, the rotation direction is set to CW.
Q 0 to 99999.999(s) Designate the dwell period from the time when the axis moves from the hole center to the radius direction to the time when the helical interpolation starts. When the command is omitted, dwelling is not performed. The relationship between the time and designated value is the same as
for the values designated in "G04P".
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
396IB-1501277-P
The thread milling cycle runs as shown below.
(1) The axis moves (approaches) with G01 from the center of the hole to the radius direction. (2) If the dwell time is designated, dwelling is performed. (3) Helical interpolation is performed in the commanded pitches. (4) After the hole bottom position has been reached, the axis moves to the center of the hole bottom with G01. (5) Pull out the tool vertically from the center of the hole bottom with G00.
(1) Modal/Unmodal The thread milling cycle (G187) is unmodal, which must be commanded for each cycle. All the data commanded with the address is also unmodal.
(2) Hole drilling axis The drilling axis is determined by plane selection (G17, G18, or G19). For details, refer to "Relationship between plane selection and drilling axis".
(3) Command format The hole position and the number of repetitions cannot be designated.
(4) Operation Positioning to the initial point or R point is not performed. Drilling is started using the position, at which the thread milling cycle (G187) is commanded, as the center.
Operation example
Differences from another fixed cycle for drilling
X
Z
Y
(4)
(5)
(1) (2)
(3)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
397 IB-1501277-P
The drilling axis is determined by plane selection (G17, G18, or G19). The axis (X, Y, Z, or its parallel axis) vertical to the plane designated in G17, G18, or G19 is used as the drilling axis. The setting of the parameter "#1080 Dril_Z" is invalid for the thread milling cycle.
Xp, Yp and Zp indicate the base axes X, Y and Z or an axis parallel to the base axis.
The command format, etc. of this function are explained, assuming that G17 (drilling axis = Z axis) is designated for plane selection.
In the following usage example, finishing is carried out up to the thread top by repeating the command that increases the arc radius by degrees. Always designate the same value for the pitch (P).
(S) Start point
Refer to "13.1.16 Precautions for Using a Fixed Cycle" in addition to the following description. (1) When a manual interruption is performed in automatic operation "pause", the end point of the interrupted block
and the end point of the bock in thread milling cycle move parallel by the manual movement amount. (The operation with the manual absolute (ABS) signal set OFF is performed during the thread milling cycle.)
Relationship between plane selection and drilling axis
Plane selection Hole drilling axis
G17 (X-Y) Zp G18 (Z-X) Yp G19 (Y-Z) Xp
: N01 G90 G00 X30.; N02 Z45.; N03 G17; N04 G187 Z25. I2. P5. F100 D0; N05 G187 Z25. I3. P5. F100 D0; N06 G187 Z25. I4. P5. F100 D0; N07 G187 Z25. I5. P5. F100 D0; : M30;
Precautions
(S)
(S)
Z
Y
X
X
N04 N05 N06 N07
N02
N01
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
398IB-1501277-P
13.1.15 Punchtap Cycle
This function performs cutting and tapping by synchronously controlling the spindle and servo axis using the dedi- cated tool for Punchtap. In general, the machining time can be shortened compared to the tapping cycle. The fixed cycle subprogram dedicated to the Punchtap cycle must be registered.
There are three patterns of operations in the Punchtap cycle, which are selected by the G code.
Function and purpose
Pattern Features
PT1.0 Fastest process out of three patterns PT1.5 Process that optimizes the machining load, including the "deburring process" PT2.0 Process that minimizes the machining load, including the "deburring process" and "screw
cleaning process"
Dotted line: Path of the tool nose in conventional tapping Solid line: Path of the tool nose in Punchtap
(1) Helical grooving (2) Tapping (3) Retract
(1)
(2)
(3)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
399 IB-1501277-P
When the drilling axis advances in the negative direction, the spindle rotates forward in the positive Punchtap cycle. The spindle rotation reverses in the reverse Punchtap cycle.
Command format
Positive Punchtap cycle
G84.5 X__ Y__ Z__ R__ F__ I__ S__ ,S__ P__ ,I__ ,J__ ,D__ L__ ; Performance PT1.0
G84.6 X__ Y__ Z__ R__ F__ I__ S__ ,S__ P__ ,I__ ,J__ ,D__ L__ ; Medium PT1.5
G84.8 X__ Y__ Z__ R__ F__ I__ S__ ,S__ P__ ,I__ ,J__ ,D__ L__ ; Soft PT2.0
Reverse Punchtap cycle
G74.5 X__ Y__ Z__ R__ F__ I__ S__ ,S__ P__ ,I__ ,J__ ,D__ L__ ; Performance PT1.0
G74.6 X__ Y__ Z__ R__ F__ I__ S__ ,S__ P__ ,I__ ,J__ ,D__ L__ ; Medium PT1.5
G74.8 X__ Y__ Z__ R__ F__ I__ S__ ,S__ P__ ,I__ ,J__ ,D__ L__ ; Soft PT2.0
X Hole position data Y Hole position data Z Hole bottom position (Z) R R point position F Tapping speed (PD) I Helical grooving speed (Ph) S Spindle rotation speed command ,S Spindle rotation speed command at retract of Punchtap cycle P Dwell time required to pull up the tool from the hole bottom or R point ,I Positioning axis in-position width ,J Drilling axis in-position width ,D Untwisting retract amount (BF) L Number of repetitions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
400IB-1501277-P
The positioning plane is determined by the G17, G18 and G19 plane selection commands, and the hole drilling axis is the axis perpendicular to the plane.
High-speed tapping is performed by the Punchtap cycle that performs the helical grooving up to the hole bottom with the cutting edge for the helical groove on the tip of the tool and the tapping with the cutting edge, and then pulls up the tool along the helical groove. The cutting edges for tapping are arranged helically on the tool, and by cutting the helical groove according to this pitch, the tool makes cuttings up to the hole bottom.
Operations (2), (3) and (5) make cuttings at the helical grooving speed (Ph) (mm/rev), and operation (4) makes cut- tings at the tapping speed (PD) (mm/rev). Refer to the figure below for the stop position during single block operation. The tool does not stop at the in-position check position (does not stop during cutting).
Explanation of address
Address Command range (unit) Remarks
X -99999.999 to 99999.999 (mm) Designate the hole drilling position on the X axis. The command can be omitted.
Y -99999.999 to 99999.999 (mm) Designate the hole drilling position on the Y axis. The command can be omitted.
Z -99999.999 to 99999.999 (mm) Designate the hole bottom position. R -99999.999 to 99999.999 (mm) Designate the R point position.
The command can be omitted. F 0.001 to 1000000.000 (mm/min) or
0.001 to 999.999 (mm/rev) Designate the tapping feedrate for cutting feed.
The unit "mm/min" is used for G94 modal and "mm/rev" is used for G95 modal.
I 0.001 to 999999999.999 (mm/min) or 0.001 to 999.999 (mm/rev)
Designate the helical grooving feedrate for cutting feed. The unit "mm/min" is used for G94 modal and "mm/rev" is used for G95 modal.
S -99999999 to 99999999 (r/min) S commands of the "Sn = *****" type are ignored in the Punchtap cycle. (n: spindle number, *****: rotation speed) If an S command is issued during the Punchtap cycle modal,
the program error (P186) occurs. If no S command is included in the same block, the program er-
ror (P181) occurs. ,S 0 to 99999 (r/min) When the value is smaller than the spindle rotation speed (S
command), the value of the spindle speed is valid even at the retract. When the spindle rotation speed at retract is not "0", the param-
eter "#1172 tapovr" (tap retract override) is invalid. The command can be omitted.
P 0 to 99999 (s) The command can be omitted. When the command is omitted, dwelling is not performed. Compared to the setting value of the parameter "#1313 Tap-
Dwl" (synchronous tapping hole bottom waiting time), the larg- er value is set as the dwell time.
,I 0.001 to 999.999 (mm) The command can be omitted. ,J 0.001 to 999.999 (mm) The command can be omitted. ,D -99999.999 to 99999.999 (mm) The sign is ignored.
The command can be omitted. L 0 to 9999 The command can be omitted.
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
401 IB-1501277-P
For tapping, the spindle rotation amount (g) and drilling axis movement amount (Tg) is obtained as shown below. For 180 in the calculation formula, the setting value of the parameter "#11773 ptapag" (rotation angle of tapping) is actually used.
Spindle rotation amount (angle)
Drilling axis movement amount (mm)
Rapid traverse
Cutting feed
In-position check
Stop position at single block operation
(A) Spindle rotation direction and angle (bottom view) (I) Initial point height (R) R point height (Z) Hole bottom height (Tg) Movement amount at tapping (BF) Retract amount
Operation Details of operation Spindle rotation amount
Spindle rota- tion direction
(1) Moves the tool to the R point with rapid traverse. - Stop (2) Performs helical grooving at the helical grooving speed
(Ph). If a dwell command is issued, dwelling is performed. CW
(3) Retracts the tool by the untwisting retract amount (BF) at the helical grooving speed (Ph).
CCW
(4) Performs tapping at the tapping speed (PD). g CCW (5) Pulls up the tool to the R point at the helical grooving
speed (Ph). If a dwell command is issued, dwelling is per- formed.
CCW
(6) Pulls up the tool to the initial point. - Stop
g = 180 (1 + )PD Ph - PD
g 360Tg = PD
(1)
(2)
(A)
(I)
(R)
(Z)
(Tg)
(BF)
CW CCW CCW CCW (3) (4) (5)
(6)
Z Ph360
BF Ph360
Z - BF - Tg Ph360 ( )
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
402IB-1501277-P
This section describes how each Punchtap cycle operates by each G code.
The "D" of G84.6 (PT1.5) and G84.8 (PT2.0) is "#11772 ptapd" (deburring adjustment amount), which is set when the finish is substandard.
Details of operation
G84.5 (PT1.0)
G84.5 Xx1 Yy1 Zz1 Rr1 Ff1 Ii1 Ss1 ,Ss2 Pp1 ,Ii1 ,Jj1 ,Dd1 Ll1;
BF: Retract amount (,D) tg: Tapping movement amount
Operation pattern Program
(1) G00 Xx1 Yy1 ; (2) G00 Zr1 ; (3) G01 Zz1 Ii1 ; Helical grooving (Forward rotation, Helical grooving
speed) (4) G04 Pp1 ; (5) G01 Z-BF Ii1 ; Untwisting retract (Reverse rotation, Helical grooving
speed) (6) G01 Z-tg Ff1 ; Tapping (Reverse rotation, Tapping speed) (7) G01 Z-(z1-BF-tg) Ii1 ; Retract (Reverse rotation, Helical grooving speed) (8) G04 Pp1 ; (9) G98 mode G00 Z-r1 ;
G99 mode No movement
(1)
(2)
(3)
(4) (5)
(6)
(7)
(8)
(9)
x1 , y1
r1
z1
tg
BF
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
403 IB-1501277-P
G84.6 (PT1.5)
G84.6 Xx1 Yy1 Zz1 Rr1 Ff1 Ii1 Ss1 ,Ss2 Pp1 ,Ii1 ,Jj1 ,Dd1 Ll1;
BF: Retract amount (,D) tg: Tapping movement amount D: "#11772 ptapd"
(Deburring adjustment amount)
Operation pattern Program
(1) G00 Xx1 Yy1 ; (2) G00 Zr1 ; (3) G01 Zz1 Ii1 ; Helical grooving (Forward rotation, Helical grooving
speed) (4) G04 Pp1 ; (5) G01 Z-BF Ii1 ; Untwisting retract (Reverse rotation, Helical grooving
speed) (6) G01 Z-tg Ff1 ; Tapping (Reverse rotation, Tapping speed) (7) G01 Z(BF+tg-D) Ii1 ; Deburring (Reverse rotation, Helical grooving speed) (8) G01 Z-(z1-D) Ii1 ; Retract (Reverse rotation, Helical grooving speed) (9) G04 Pp1 ;
(10) G98 mode G00 Z-r1 ; G99 mode No movement
(1)
(2)
(3)
(4) (5)
(6)
(7)
(8)
(9)
(10)
x1 , y1
r1
z1
tg
BF D
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
404IB-1501277-P
G84.8 (PT2.0)
G84.8 Xx1 Yy1 Zz1 Rr1 Ff1 Ii1 Ss1 ,Ss2 Pp1 ,Ii1 ,Jj1 ,Dd1 Ll1;
BF: Retract amount (,D) tg: Tapping movement amount D: "#11772 ptapd"
(Deburring adjustment amount)
Operation pattern Program
(1) G00 Xx1 Yy1 ; (2) G00 Zr1 ; (3) G01 Zz1 Ii1 ; Helical grooving (Forward rotation, Helical grooving
speed) (4) G04 Pp1 ; (5) G01 Z-BF Ii1 ; Untwisting retract (Reverse rotation, Helical grooving
speed) (6) G01 Z-tg Ff1 ; Tapping (Reverse rotation, Tapping speed) (7) G01 Z(BF+tg-D) Ii1 ; Deburring (Reverse rotation, Helical grooving speed) (8) G01 Z-(BF+tg-D) Ii1 ; Deburring retract (Reverse rotation, Helical grooving
speed) (9) G01 Z-tg Ff1 ; Screw cleaning (Forward rotation, Tapping speed)
(10) G01 Z-(z1-BF) Ii1 ; Retract (Reverse rotation, Helical grooving speed) (11) G04 Pp1 ; (12) G98 mode G00 Z-r1 ;
G99 mode No movement
(1)
(2)
(3)
(4) (5)
(6)
(7) (8)
(9)
(10)
(11)
(12)
x1 , y1
r1
z1
tg
BF D
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
405 IB-1501277-P
The in-position check in each process other than the R point retract of the Punchtap cycle can be finely adjusted by the parameter setting. The parameter setting depends on the MTB specifications.
In the Punchtap cycle, it is possible to set whether or not to perform the in-position check at each of points (1) to (6) in the figure below. Each of points (1) to (6) corresponds to each bit of the parameter "# 1702 cfg02", which can be set to "valid" or "in- valid" individually. Dwelling is also performed at the P point. No switching parameter is provided to pull up the tool to the R point, and the in-position check is always performed. When the "Error detection" signal is ON, the in-position check is performed with the parameter "#11771 PTapInp" regardless of the setting value of the parameter "#1702 cfg02".
[Setting example of parameter to perform in-position check at points (1), (3), (4), and (6) above]
Set bit0, bit2, bit3, and bit5 of the parameter #1702 to "1".
In-position check
Parameter Setting value Deceleration check operation
#1702 cfg02/bit0 to bit5 0 Command deceleration 1 In-position check with "#11771 PTapInp"
For G84.5 (PT1.0) For G84.6 (PT1.5)
For G84.8 (PT2.0)
(I) Initial point (R) R point (r) (A) Hole bottom
#1702 bit5 bit4 bit3 bit2 bit1 bit0
G84.5 (PT1.0) - - - (3) (2) (1) G84.6 (PT1.5) - - (4) (3) (2) (1) G84.8 (PT2.0) (6) (5) (4) (3) (2) (1)
(1)
(2)
(3)
P
P (1)
(2)
(3)
P
P
(4)
(1)
(2)
(3)
P
(I)
(R)
(A)P (4)
(5)
(6)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
406IB-1501277-P
The following parameters are used to judge the in-position check at each point.
(*1) The setting value of the parameters "#2077 G0inps" and "#2078 G1inps", is compared with parameter "#2224 SV024 INP", and the larger value is used to perform in-position check.
(*2) When the parameter "#11771 PTapInp" is set to "0", in-position check is performed with the value of the param- eter "#2224 SV024 INP".
For G84.8 (PT2.0)
(I) Initial point (R) R point (r) (A) Hole bottom
Parameters used for in-position check
(1) "#2077 G0inps" or "#2224 SV024 INP" (*1) (2) "#2077 G0inps" or "#2224 SV024 INP" (*1) (3)
"#11771 PTapInp" for each (*2)
(4) (5) (6) (7) (8) (9) "#2078 G1inps" or "#2224 SV024 INP" (*1)
(1)
(2)
(3) (4)
(5)
(6)
(7)
(8)
(9)
(I)
(R)
(A)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
407 IB-1501277-P
The spindle zero point return operation in Punchtap is the same as the synchronous tapping. In addition, the parameter in the zero point return operation can be changed with the G10L70 command.
The tapping speed and helical grooving speed specified with the Punchtap cycle command can be switched to the feed per minute using the parameter.
The combination of the parameter "#1268 ext04/bit2" (Enable synchronous tapping per minute) and G code deter- mines the meaning of the F command (tapping speed) and I command (helical grooving speed).
To update the F modal, set the parameter "#1292 ext28/bit1" (Address F given in sync tap cycle) to "1", not the pa- rameter "#1268 ext04/bit2" (Enable synchronous tapping per minute).
Feed per minute
Feed per revolution
The I command is retained in each of G94 and G95, and it is retained even after the fixed cycle is canceled with G80. If the I command is omitted, Punchtap is performed using the previous I command as the helical grooving speed. If the I command is omitted without issuing the I command even once, a program error (P184) will occur.
Spindle zero point return operation in Punchtap
Feedrate
#1268/bit2 During G94 modal (feed per minute) During G95 modal (feed per revolution)
1 Feed per minute Feed per revolution 0 Feed per revolution Feed per revolution
Ff1, Ii1 : Feedrate (mm/min, inch/min) (Pitch calculation formula) Pitch = F command value / S command value
Ff1, Ii1 : Feedrate (mm/rev, inch/rev)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
408IB-1501277-P
Program example
G90 G98 ; G00 X30. Y0. Z30. ; G95 ; G84.5 X30. Z5. R20. F1. S500 I31.5. ; G80 ; G94 ;
(I) Initial point (R) R point (Sp) Spindle
Rapid traverse
Cutting feed
30(I)
(Sp)
(R)
Z
20
5
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
409 IB-1501277-P
(1) High-speed synchronous tapping Even in the Punchtap cycle, the high-speed synchronous tapping that corrects the tracking delay in the commu- nication between drive units is valid. The reduction rate in Punchtap depends on the MTB specifications (parameter "#3136 ptaptr"). Other parameters are also used as the synchronous tapping. The restrictions and enabling conditions related to the high-speed synchronous tapping are the same as for the synchronous tapping.
(2) Tapping retract The "Tap retract" signal (YC5C) is invalid in the Punchtap cycle. The "Tap retract possible" signal is not output even if the Punchtap cycle is interrupted. Tapping retract is not available when the Punchtap cycle is used. When the Punchtap cycle machining is interrupted due to power OFF, etc., pull out the tool by one of the follow- ing methods. Rotate the spindle in the same direction as when the Punchtap cycle is commanded, crush the screw thread,
and pull out the tool. While rotating the spindle in the opposite direction to when the Punchtap cycle is commanded, manually
operate the Z axis to pull out the tool. (3) Reference position retract
The "Reference position retract" (YC2D) signal is invalid in cutting feed of the Punchtap cycle, and the reference position return is also not performed without a reset stop. This signal is valid in rapid traverse, and the reference position return is performed after a reset stop.
(4) Coordinate system operation, inclined surface machining command Do not command the Punchtap cycle while the hole drilling axis (Z axis) is rotated by coordinate rotation by pro- gram or 3-dimensional coordinate conversion. Also, do not command the Punchtap cycle during the inclined surface machining command. If any of these commands are issued, tapping may not be available.
(5) Chopping The Punchtap cycle can even be executed during chopping, however, if the chopping axis is included in the po- sitioning axis or drilling axis, the operation error (M01 0151) occurs, and the machine stops in the interlock state.
(6) Stroke limit The stroke limit is valid for both the positioning axis and drilling axis. When the drilling axis is stopped at the stroke limit, the spindle also stops synchronously.
(7) Coil switch In the Punchtap cycle, the spindle motor operates with L coil regardless of the spindle rotation speed. However, when the parameter "#1239 set11/bit0" (Coil switching method) is set to "1" and the parameter "#1223 aux07/bit7" (Synchronous tap method) is set to "0", the type of coil is switched to H coil according to the change of the spindle rotation speed. Since the torque may get insufficient in such a case, command the spindle rotation speed of the L coil so that the coil is not switched. (The settings of these parameters depend on the MTB spec- ifications.) When the coil switch is performed during the Punchtap cycle, the coil is switched after the cycle ends.
(8) Graphic check The helical grooving speed is not reflected on the cutting speed.
(9) Synchronous tapping with analog I/F spindle The Punchtap cycle is not available for the analog spindle. The program error (P182) occurs if commanded.
(10) Manual arbitrary reverse run The manual arbitrary reverse run is only valid in the actual cutting mode. If the Punchtap cycle is commanded while the dry run operation mode is enabled, the program error (P182) occurs. Also, the Punchtap cycle is han- dled as a reverse run prohibited block.
(11) Finish shape view programming The Punchtap cycle is not reflected. The G code of the Punchtap cycle is ignored, and the subsequent codes are reflected on the finishing shape.
Relationship with other functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
410IB-1501277-P
(12) Synchronous control When the reference axis of synchronous control is a tapping axis, in-position check in the Punchtap cycle is dis- abled.
(1) The multi-step acceleration/deceleration is invalid in the Punchtap cycle. (2) Dry run is valid only for rapid traverse sections. (3) If the "External deceleration" signal is turned ON during Punchtap, the feedrate does not change even when de-
celeration conditions are satisfied. (4) The cutting feed override is disabled during the Punchtap cycle, and the feedrate is 100%. Rapid traverse over-
ride is valid. (5) The spindle override is invalid during the Punchtap cycle. (6) The automatic machine lock is valid. If the Punchtap cycle is executed while the drilling axis is machine-locked,
the spindle does not rotate either. (7) The parameters ("#3106", "#3110", and "#3111") of the tap starting angle are also used with the synchronous
tapping. (8) The G94 command is a modal command and valid until the G95 command is issued next. (9) For the "F" command and "I" command, the feed per minute and the feed per revolution are switched in the same
conditions. (10) When the automatic operation is started in the miscellaneous function lock ("MST lock" is ON), the spindle is
not synchronized even after block stop or feed hold stop processing has been ended. (11) The "NC output" signal under tapping is output during the Punchtap cycle. (12) The Punchtap cycle is always set in the synchronous mode. The ",R0" command is ignored. The setting of the
parameter "#1229 set01/bit4" (synchronous tapping) is also irrelevant. (13) The "Spindle OFF mode" signal is valid. If an attempt is made to execute the Punchtap cycle in the Spindle OFF
mode, the Punchtap cycle is executed without rotating the spindle. This is used for program check. Dry run is enabled in the Spindle OFF mode.
(14) When the feed hold button is pressed during cutting feed of the punch tapping cycle, the machining does not stop immediately but stops when the block to pull-up tool on the helical groove is completed. When the feed hold button is pressed during rapid traverse, the machining stops immediately.
(15) The "Synchronous tapping command polarity reversal" signal is valid. (16) The tapping error displayed by selecting [Drv mon] - [Spindle unit] is not displayed correctly during the Punchtap
cycle. To check the tapping error, sample the commanded position and FB position of the tapping axis, and the com- mand position and FB position of the spindle, and then calculate the error using the following formula. Switch the pitch depending on the FB position of the tapping axis and the spindle.
Precautions
Tapping error [deg] = |Spindle command position Spindle FB position|
Tapping axis command position Tapping axis FB position
Pitch of each process 360
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
411 IB-1501277-P
13.1.16 Precautions for Using a Fixed Cycle
(1) Before the fixed cycle is commanded, the spindle must be rotating in a specific direction with a miscellaneous function command (M3; or M4;). Note that for the G87 (back boring) command, the spindle rotation command is included in the fixed cycle so only the rotation speed command needs to be commanded beforehand.
(2) If there is data for the basic axis, additional axis or R in the block during the fixed cycle mode, the hole drilling operation will be executed. If there is no data, the hole drilling operation will not be executed. Note that even when the X axis data exists, the hole will not be drilled if the data is a dwell (G04) time command.
(3) Command the hole machining data (Q, P, I, J, K) in a block where hole drilling is executed (Block containing a basic axis, additional axis or R data).
(4) The fixed cycle can be canceled by the G00 to G03 or G33 command besides the G80 command. If these are designated in the same block as the fixed cycle, the following will occur.
Note that for the G02 and G03 commands, R will be handled as the arc radius.
(5) If M00 or M01 is commanded in a same block with a fixed cycle or during a fixed cycle mode, the fixed cycle will be ignored. Instead, M00 and M01 will be output after positioning. The fixed cycle is executed if X, Y, Z or R is commanded.
(6) If an M function is commanded in the same block as the fixed cycle command, the M code and MF will be output during the initial positioning. The axis will move to the next operation with FIN (finish signal). If there is a designation of No. of times, the above control will be executed only for the first drilling.
(7) If another control axis (ex. rotary axis, additional axis) is commanded in the same block as the fixed cycle control axis, the fixed cycle will be executed after the other control axes start to move.
(8) If the No. of repetitions L is not designated, L1 will be set. If L0 is designated in the same block as the fixed cycle G code command, the hole machining data will be memorized, but the hole machining will not be executed. (Example) G73 X_Y_Z_R_Q_P_F_L0_;
Memorize only the codes with an execution address
(9) When the fixed cycle is executed, only the modal command issued in the fixed cycle program will be valid in the fixed cycle subprogram. The modal of the program which called the fixed cycle will not be affected.
(10) Other subprograms cannot be called from the fixed cycle subprogram. (11) Decimal points in the movement command of the fixed cycle subprogram will be ignored. (12) If the No. of repetitions L is 2 or more during the incremental mode, the positioning will also be incremented
each time. (Example) G91 G81 X10. Z-50. R-20. F100. L3;
Precautions
m = 00 to 03, 33 n = Fixed cycles
Gm Gn X_Y_Z_R_Q_P_L_F_;
Gm : Execution Gn : Ignore X_Y_Z : Execution R_Q_P_L : Ignore F : Record
X Y 10. 10. 10.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
412IB-1501277-P
(13) If the spindle rotation speed value during return is smaller than the spindle speed value, the spindle rotation speed value is valid even during return.
(14) If gradients of the 2nd and 3rd acceleration/deceleration stages according to the spindle rotation speed and time constants set in the parameters are each steeper than the previous stage's gradients, the previous stage's gradient will be valid.
(15) If the values set in the spindle specification parameter "tap rotation speed" and "the synchronous tap change- over spindle rotation speed 2" exceed the maximum rotation speed, the spindle rotation speed will be clamped at the maximum rotation speed.
(16) If the spindle rotation speed is not 0 during return, the taping retract override value will be invalid. (17) As shown below, in a block where the movement direction of either axis reverses, the servo system load will
greatly increase, so do not command the in-position width in the machining program. G01 X100. ,I10.0;
X-200.;
(18) If the in-position width commanded by the programmable in-position width command is increased, the position- ing time and linear interpolation time can be reduced. However, the position error amount of the previous block will also increase before the next block starts, and the actual machining could be obstructed.
(19) The in-position width and the position error amount are constantly compared, so the position error amount at the point to be judged as in-position will be smaller than the commanded in-position width.
(20) If the in-position width commanded with the programmable in-position command is small, the commanded de- celeration check or in-position check by the parameters may be carried out first.
(21) Synchronous or asynchronous tapping can be selected with the M function. Base specification parameters
Synchronous tapping cannot be selected with the M function when this parameter is OFF.
Base specification parameters
The synchronous tapping mode is selected with the miscellaneous function code set with this parameter. The M function can be commanded just before or in the same block as the tapping command. To use this parameter, validate "#1272 ext08/bit1" (M function synchronous tapping cycle).
The selection of synchronous or asynchronous tappinf will follow the combination shown below.
(22) Even when the parameter "#1151 rstinit" is OFF, the fixed cycle will be canceled if NC reset 1 is carried out while executing the fixed cycle.
(23) If a tapping axis is under machine lock, normal synchronous tapping is applied even though high-speed syn- chronous tapping function is enabled.
# Item Details Setting range
1272 (PR)
ext08 bit1 M-function synchronous tapping cycle valid.
0: Invalid 1: Valid
# Item Details Setting range
1513 stapM M code for synchronous tapping selection 0 to 99999999
Combination
Program command (,R0/1) 0 0 0 0 1 1 1 1 No command #8159 Synchronous tap 0 0 1 1 0 0 1 1 0 0 1 1 M function code (M**) Synchronous/asynchronous selection
A A A A B B B B A B B B
Not commanded A Asynchronous tapping Commanded B Synchronous tapping
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
413 IB-1501277-P
13.1.17 Initial Point and R Point Level Return; G98, G99
Whether to use R point or initial level as the return level in the final sequence of the fixed cycle can be selected.
The relation of the G98/G99 mode and the number of repetition designation is as shown below.
Function and purpose
Command format
G98; ... Initial level return
G99; ... R point level return
Detailed description
No. of hole drilling times
Program example G98 G99
(At power ON, at cancel with M02, M30, and reset button)
Only one exe- cution
G81 X100. Y100. Z-50. R25. F1000 ;
Initial level return is executed. R point level return is executed. Two or more executions
G81 X100. Y100. Z-50. R25. L5 F1000 ;
Initial level return is executed for all times.
(a) First time (b) Second time (c) Last time
(I)
(R)
(I)
(R)
(a) (b) (c) (a) (b) (c)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
414IB-1501277-P
13.1.18 Setting of Workpiece Coordinates in Fixed Cycle Mode
The designated axis moves in the workpiece coordinate system set for the axis. The Z axis becomes valid from the R point positioning after positioning is completed or from Z axis movement.
(1) When the workpiece coordinates change, re-program the addresses Z and R, even if the values are the same.
Function and purpose
G54 Xx1 Yy1 Zz1; G81 Xx1 Yy2 Zz2 Rr2; G55 Xx3 Yy3 Zz2 Rr2 Re-command even if Z and R are the same as the previous value. Xx4 Yy4 ; Xx5 Yy5 ;
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
415 IB-1501277-P
13.1.19 Drilling Cycle High-Speed Retract
This function retracts the drill from the hole bottom at high speed in drilling machining. This helps extending the drill life by reducing the time of drilling in vain at hole bottom.
The drill moves up at high-speed ((1) in the figure) and returns to the initial point or R point in rapid traverse ((2) in the figure).
The command format is the same as fixed cycle.
Function and purpose
Command format
(1) (2)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
416IB-1501277-P
(1) This function is available only when "#8123 H-spd retract ON" is enabled in the following fixed cycles. G81 (Drill spot drilling cycle) G83 (Deep whole drilling cycle) G73 (Step cycle)
(2) When "#8123 H-spd retract ON" is ON, the tool is retracted from the hole bottom at high speed using the lost motion compensation function. (a) Set the lost motion compensation type 2 or 3 to the servo parameter. Then set the following parameters to
adjust the retract amount. These parameters depend on the MTB specifications. #2170 Lmc1QR (Lost motion compensation gain 1 for high-speed retract)
(corresponds to "#2216 SV016 (LMC1)" (Lost motion compensation 1)) #2171 Lmc2QR (Lost motion compensation gain 2 for high-speed retract)
(corresponds to "#2241 SV041 (LMC2)" (Lost motion compensation 2)) (b) When the lost motion compensation timing, lost motion compensation 3 spring constant, or lost motion com-
pensation 3 viscous coefficient is set in addition to the ordinary lost motion compensations, its setting value depends on the MTB specifications (parameter shown below). #2172 LmcdQR (Lost motion compensation timing for high-speed retract)
(correspond to "#2239 SV039 (LMCD)" (Lost motion compensation timing)) #2173 LmckQR (Lost motion compensation 3 spring constant for high-speed retract)
(correspond to "#2285 SV085 (LMCk)" (Lost motion compensation 3 spring constant)) #2174 LmccQR (Lost motion compensation 3 viscous coefficient for high-speed retract)
(correspond to "#2286 SV086 (LMCc)" (Lost motion compensation 3 viscous coefficient)) (c) If the hole drilling axis is synchronously controlled, set the same value in both parameters for master axis and
slave axis. (3) While G80 (Fixed cycle cancel) command is issued, this function will be canceled by issuing any other fixed cycle
of the same group (Group 9) or any Group 1 command. (4) This function is invalid during the following command modal:
In this case, the drill moves in the ordinary rapid traverse even if "#8123" is enabled. G43.1 (Tool length compensation in the tool axis direction) G43.4, G43.5 (Tool center point control) G68 (3-dimensional coordinate conversion)
(5) While the multiple-axis synchronization control is being executed, if the drilling cycle high-speed retract in which the master axis is set as the drilling axis is commanded, the slave axis moves at the same speed as the master axis.
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
417 IB-1501277-P
During single block operation, the axis stops after (1), (2) and (5) only.
During single block operation, the axis stops after (1), (2) and (10) only.
Details of operation
Operation at G81 command
(1) Moves from start point to initial point (2) Moves from initial point to R point (3) Cutting feed (4) Retracted at high-speed (5) Returns to R point or initial point
(I) Initial point (S) Start point (R) R point
Operation at G83 command
(1) Moves from start point to initial point (2) Moves from initial point to R point (3) Cutting feed (4) Retracted at high-speed (5) Returns to R point (6) Moves to the position where the "G83 Return amount"
is added to the previous cutting feed position. (7) Cutting feed (8) Repeats (4) to (7) (9) Retracted at high-speed (10) Returns to R point or initial point
(I) Initial point (S) Start point (R) R point (m) G83 Return amount
(1) (2)
(3) (4)
(5)
G98
G99
(S)
(R)
(I)
(10)
(1) (2)
(3)
(4)
(7)
(5) (6)
(9)
(8)
(I)
(R)
(S)
(m)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
418IB-1501277-P
During single block operation, the axis stops after (1), (2) and (8) only. If a dwell command is issued, the high-speed retract will be executed after the command.
Operation at G73 command
(1) Moves from start point to initial point (2) Moves from initial point to R point (3) Cutting feed (4) Retracted at high-speed (5) Moves to the position set with "G73 return amount" (6) Repeats (3) to (5) (7) Retracted at high-speed (8) Returns to R point or initial point
(I) Initial point (S) Start point (R) R point (n) G73 Return amount
(8)
(7)
(6)
(5) (4)
(3)
(1)
(2)
G98
G99
(I)
(R)
(S)
(n)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
419 IB-1501277-P
13.1.20 Acceleration/Deceleration Mode Change in The Fixed Cycle for Drilling
This function switches the acceleration/deceleration mode for fixed cycle for drilling between the constant-gradient method and the acceleration/deceleration after interpolation.
The command formats are the same as those of the fixed cycles G83, G87, and G83.2.
With parameter "#1253 set25/bit2" (Acceleration/deceleration mode change in the fixed cycle for drilling) enabled, operation will be as follows.
(1) Acceleration/deceleration mode will be either linear or soft method. (Unless soft acceleration/deceleration is ap- plied, the linear method will always be applied.)
(2) Operation is performed based on the parameter setting that enables the constant-gradient acceleration/deceler- ation after interpolation. Acceleration/deceleration gradient for G00 (rapid traverse) is determined with "#2001 rapid" (rapid traverse rate) and "#2004 G0tL" (G0 time constant (linear)), and acceleration/deceleration gradient for G01 (cutting feed) is determined with "#2002 clamp" (cutting feedrate for clamp) and "#2007 G1tL" (G1 time constant (linear)). Refer to "7.9 Rapid Traverse Constant-gradient Multi-step Acceleration/Deceleration" or "7.10 Cutting Feed Constant-gradient Acceleration/Deceleration" for details on the constant-gradient acceleration/deceleration.
Function and purpose
Command format
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
420IB-1501277-P
The below illustrates the processes of hole-bottom deceleration check of a drilling axis following the parameter "#19417 Hole dec check 2" settings.
Operation example
Operation example of "acceleration/deceleration mode change in hole drilling cycle" being enabled
(a) Cut point (b) Hole bottom
#19417 G81 G82 G83 G73 0 (a) Cut point Deceleration Check Perform no deceleration check.
(b) Hole bottom Perform no deceleration check. 1 (a) Cut point Perform no command deceleration
check. Command deceleration check
(b) Hole bottom Command deceleration check 2 (a) Cut point Command deceleration check Perform in-position
check (sv024). (b) Hole bottom Perform in-position check (sv024).
(1)
(2)
(3)
(a)
(a)
(4) (7)
(9)(6) (5)
(8)
(b)
(11)
(10)
(12)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
421 IB-1501277-P
13.2 Special Fixed Cycle
The special fixed cycle is used with the standard fixed cycle. Before using the special fixed cycle, record the hole machining data except for the positioning data (except for X, Y plane) by the standard fixed cycle. The tool is positioned to the hole drilling position when the special fixed cycle is executed. The drilling operation is executed with the fixed cycle for drilling. Even after the special fixed cycle is executed, the recorded standard fixed cycle will be kept until canceled. If the special fixed cycle is designated when not in the fixed cycle mode, only positioning will be executed, and the hole drilling operation will not be carried out. If the special fixed cycle is commanded without commanding the fixed cycle for drilling, positioning will be executed following the current 01 group modal G code.
Function and purpose
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
422IB-1501277-P
13.2.1 Bolt Hole Cycle; G34
This function is used to drill "n" holes, dividing the circumference by "n", on the circumference with radius R centering the coordinates designated with X and Y. The drilling starts at the point which makes the angle with X axis. The hole drilling operation at each hole will follow the standard fixed cycle. The movement between hole positions will all be done in the G00 mode. G34 will not hold the data after the com- mand is completed.
As shown in the example, the tool position after the G34 command is completed is above the final hole. When mov- ing to the next position, the coordinate value must be calculated to issue the command with an incremental position. Thus, use of the absolute mode is handy.
(1) If an address other than the selected plane's vertical axis, horizontal axis, G, N, I, J, K, H, O, P, F, M, S or 2nd miscellaneous function is issued in the same block as the G34 command, a program error (P32) will occur.
Function and purpose
Command format
G34 Xx1 Yy1 Ir J Kn ;
Xx1,Yy1 Positioning of bolt hole cycle center. This will be affected by G90/G91. Ir Radius r of the circle. The unit follows the input setting unit, and is given with a positive
No. J Angle of the point to be drilled first. The CCW direction is positive.
(The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001.)
Kn No. of holes to be drilled: n 1 to 9999 can be designated, but 0 cannot be designated. When the value is positive, positioning will take place in the CCW direction, and when negative, will take place in the CW direction. If "0" is designated, a program error (P221) occurs.
Program example
N001 G91; N002 G81 Z-10.000 R5.000 L0 F200 ; N003 G90 G34 X200.000 Y100.000 I100.000 J20.000 K6; N004 G80 ; --------------- (G81 cancel) N005 G90 G00 X500.000 Y100.000. ;
(a) Position before G34 execution
(500mm, 100mm)
20
x1=200mm n=6
I=100mmy1=100mm
(a) N005 G00
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
423 IB-1501277-P
13.2.2 Line at Angle; G35
Using the position designated by X and Y as the start point, the n holes will be drilled with interval d in the direction which makes an angle with X axis. The hole drilling operation at each hole will follow the standard fixed cycle. The movement between hole positions will all be done in the G00 mode. G35 will not hold the data after the com- mand is completed.
(1) If the K command is K0 or if there is no K command, the program error (P221) will occur. (2) If the K value is more than four digits, the last four digits will be valid. (3) If an address other than the selected plane's vertical axis, horizontal axis, G, N, I, J, K, H, O, P, F, M, S or 2nd
miscellaneous function is issued in the same block as the G35 command, a program error (P32) will occur. (4) If G command of group 0 is issued in the same block as the G35 command, the command issued later has the
priority.
(5) If there is G72 to G89 commands in the same block as the G35 command, the fixed cycle will be ignored, and the G35 command will be executed.
Function and purpose
Command format
G35 Xx1 Yy1 Id J Kn ;
Xx1,Yy1 Designation of start point coordinates. This will be affected by G90/G91. Id Interval d. The unit follows the input setting unit. If d is negative, the drilling will take
place in the direction symmetrical to the center of the start point. J Angle . The CCW direction is positive.
(The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001.)
Kn Number of holes: n 1 to 9999 can be designated, and the start point is included.
Program example
G91 ; G81 Z-10.000 R5.000 L0 F100 ; G35 X200.000 Y100.000
I100.000 J30.000 K5 ;
(a) Position before G35 execution
(Example) G35 G28 Xx1 Yy1 Ii1 Jj1 Kk1 ; G35 is ignored G 28 is executed as Xx1 Yy1
y1=100mm
=30
n=5
d=100mm
x1=200mm (a)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
424IB-1501277-P
13.2.3 Arc; G36
The "n" holes aligned with the angle interval will be drilled starting at the point which makes the angle with the X axis on the circumference with a radius R centering the coordinates designated with X and Y. The hole drilling operation at each hole will follow the standard fixed cycle. The movement between hole positions will all be done in the G00 mode. G36 will not hold the data after the com- mand is completed.
(1) If an address other than the selected plane's vertical axis, horizontal axis, G, N, I, J, K, H, O, P, F, M, S or 2nd miscellaneous function is issued in the same block as the G36 command, a program error (P32) will occur.
Function and purpose
Command format
G36 Xx1 Yy1 Ir J P Kn ;
Xx1,Yy1 Center coordinates of arc. This will be affected by G90/G91. Ir Radius r of arc. The unit follows the input setting unit, and is given with a positive No. J Angle of the point to be drilled first. The CCW direction is positive. (The decimal point position
will be the degree class. If there is no decimal point, the unit will be 0.001.) P Angle interval . When the value is positive, the drilling will take place in the CCW direction, and in
the CW direction when negative. (The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001.)
Kn No. of holes n to be drilled. The setting range is 1 to 9999.
Program example
N001 G91 ; N002 G81 Z-10.000 R5.000 F100 ; N003 G36 X300.000 Y100.000 I300.000 J10.000
P15000 K6 ;
(a) Position before G36 execution
n=6
x1=300mm
=10
= 15
y1=100mm
(a)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
425 IB-1501277-P
13.2.4 Grid; G37.1
The nx points on a grid are drilled with an interval x parallel to the X axis, starting at the position designated with X, Y. The hole drilling operation at each hole will follow the standard fixed cycle. The movement between hole positions will all be done in the G00 mode. G37.1 will not hold the data after the com- mand is completed.
Function and purpose
Command format
G37.1 Xx1 Yy1 Ix Pnx Jy Kny ;
Xx1,Yy1 Designate the coordinates at the start point. This will be affected by G90/G91. I x Interval x of the X axis. The unit will follow the input setting unit. If x is positive, the
interval will be in the forward direction looking from the start point, and when negative, will be in the reverse direction looking from the start point.
Pnx No. of holes nx in the X axis direction. The setting range is 1 to 9999. J y Interval y of the Y axis. The unit will follow the input setting unit. If y is positive, the
interval will be in the forward direction looking from the start point, and when negative, will be in the reverse direction looking from the start point.
Kny No. of holes ny in the Y axis direction. The setting range is 1 to 9999.
Program example
G91 ; G81 Z-10.000 R5.000 F20 ; G37.1 X300.000 Y-100.000 I50.000 P10
J100.000 K8 ;
(a) Position before G37.1 is executed
ny=8
nx=10x1=300mm
y= 100mmy1=100mm
x=50mm
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
426IB-1501277-P
(1) If the P and K commands are P0 or K0, or if there is no P or K command, the program error (P221) will occur. If the P or K value is more than four digits, the last four digits will be valid.
(2) If an address other than the selected plane's vertical axis, horizontal axis, G, N, I, J, K, H, O, P, F, M, S or 2nd miscellaneous function is issued in the same block as the G37.1 command, a program error (P32) will occur.
(3) If G command of group 0 is issued in the same block as the G37.1 command, the command issued later has the priority.
(4) If there is G72 to G89 command in the same block as the G37.1 command, the fixed cycle will be ignored, and the G37.1 command will be executed.
(5) If the G22/G23 command is programmed in the same block as the G37.1 command, the G22/G23 command will be ignored, and the G37.1 command will be executed.
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
427 IB-1501277-P
13.3 Fixed Cycle for Turning Machining
When performing rough cutting and other cuttings by turning machining, fixed cycles are effective in simplifying ma- chining programs. The whole commands can be performed in a single block, which normally requires several blocks. The types of fixed cycles for turning machining are listed below.
(1) Fixed cycle commands are modal G codes. They are valid until another command in the same modal group or a cancel command is issued.
(2) The fixed cycle call becomes the movement command block call. By the movement command block call, the fixed cycle macro subprogram is called only when there is an axis movement command during the fixed cycle mode. It is executed until the fixed cycle is canceled.
(3) A manual interruption can be applied while a fixed cycle for turning machining is being executed. Upon comple- tion of the interrupt, however, the tool must be returned to the position where the manual interruption was applied and then the fixed cycle for turning machining should be resumed. If it is resumed without returning the tool, all subsequent operations will deviate from the original path by the man- ual interruption amount.
Function and purpose
G code Function
G174 Longitudinal cutting cycle
G175 Thread cutting cycle
G176 Face cutting cycle
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
428IB-1501277-P
13.3.1 Longitudinal Cutting Cycle; G174
The longitudinal cutting cycle performs continuous straight and taper cutting in the longitudinal direction.
(*1) If the commanded axis and selected plane are different when the fixed cycle for turning machining is command- ed, or if the movement amount is not specified in either or both of the selected plane axis commands, a program error (P114) will occur. Whether this is judged to be a program error depends on the MTB specifications (pa- rameter "#1241 set13/bit4" ("fixed cycle for turning machining" selected-plane axis check disabled)).
Function and purpose
Command format
Straight cutting
G174 X__ Z__ F__ ;
X X axis end point coordinate (*1) Z Z axis end point coordinate (*1) F Feedrate
Taper cutting
G174 X__ Z__ R__ F__ ;
X X axis end point coordinate (*1) Z Z axis end point coordinate (*1) R Taper depth (radius designation, incremental position, sign required) F Feedrate
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
429 IB-1501277-P
Detailed description
Straight cutting
(R) Rapid traverse (F) Cutting feed (E) End point coordinates
Taper cutting
(R) Rapid traverse (F) Cutting feed (E) End point coordinates
Z
X
1(R)
4(R)
2(F)
3(F)(E) (x,z)
Z
X
1(R)
2(F) 4(R)
3(F)(E) (x,z)
r
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
430IB-1501277-P
With a single block, the tool stops at the end points of operations 1, 2, 3 and 4 shown above.
Depending on the signs of x, z and r, the following shapes are created.
Program error (P191) will occur in (b) and (c) unless the following condition is satisfied.
|x| |r|
Detailed description
(a) z < 0, x < 0, r < 0 (b) z < 0, x < 0, r > 0
(c) z > 0, x < 0, r < 0 (d) z > 0, x <0 , r > 0
Z
X
z
r x
1(R)
3(F)
4(R)2(F)
Z
X
r
x
z
1(R)
3(F)
2(F) 4(R)
Z
X
r x
z
1(R)
3(F)
4(R)2(F)
x
r
4(R)
Z
X
z
1(R)
3(F)
2(F)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
431 IB-1501277-P
13.3.2 Thread Cutting Cycle; G175
Thread cutting cycle is a fixed cycle which performs straight and taper thread cutting.
(*1) If the commanded axis and selected plane are different when the fixed cycle for turning machining is command- ed, or if the movement amount is not specified in either or both of the selected plane axis commands, a program error (P114) will occur. Whether this is judged to be a program error depends on the MTB specifications (pa- rameter "#1241 set13/bit4" ("fixed cycle for turning machining" selected-plane axis check disabled)).
Function and purpose
Command format
Straight thread cutting
G175 X__ Z__ F/E__ Q__;
X X axis end point coordinate (*1) Z Z axis end point coordinate (*1) F/E Lead of long axis (axis which moves most) direction Q Thread cutting start shift angle
Taper thread cutting
G175 X__ Z__ R__ F/E__ Q__;
X X axis end point coordinate (*1) Z Z axis end point coordinate (*1) R Taper depth (radius designation, incremental position, sign required) F/E Lead of long axis (axis which moves most) direction Q Thread cutting start shift angle
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
432IB-1501277-P
With a single block, the tool stops at the end points of operations 1, 3 and 4.
With a single block, the tool stops at the end points of operations 1, 3 and 4.
Detailed description
Straight thread cutting
(R) Rapid traverse (F) Thread cutting cycle (E) End point coordinates
Taper thread cutting
(R) Rapid traverse (F) Thread cutting cycle (E) End point coordinates
Z
X
1(R)
2(F) 4(R)
3(R) (E) (x,z)
Z
X
1(R)
2(F) 4(R)
3(R) (E) (x,z)
r
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
433 IB-1501277-P
(1) Details for chamfering
If thread chamfering amount is bigger than a thread lead length, a program error(P192) will occur before starting thread cutting.
The operation in the thread cutting cycle when the result of the thread cutting tool retract with chamfering exceeds the cycle start point depends on the MTB specifications.
<#1270 ext06/bit4 = 0> A program error (P192) will occur before thread cutting is started.
<#1270 ext06/bit4 = 1> A program error (P192) will not occur. After the thread cutting tool retraction is stopped and the thread cutting block ends at the cycle start point ("A" in the figure), the axis moves to the end coordinate ("B" in the figure) at rapid traverse feed.
Thread cutting tool retraction when "#1270 ext06/bit4" is set to "1"
(2) When the feed hold is applied during the thread cutting cycle, automatic operation will stop if it is applied when thread cutting is not being executed or when a cutting command is issued but the axis is yet to move. When the feed hold is applied during thread cutting, the thread cutting cycle retract is performed.
Detailed description
: Thread chamfering amount This value is set in the parameter "#8014 CDZ- VALE". The available range is 0 to 12.7 leads. It can be set in 0.1L units. : Thread chamfering angle This value is set in the parameter "#8015 CDZ- ANGLE". The setting range is 0 to 89. It can be set in 1 units.
3(R)
2(F)
4(R)
1(R)
A
B
Cycle start point
(F): Thread cutting (R): Rapid traverse
Chamfering end point
Chamfering start point
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
434IB-1501277-P
(3) Depending on the signs of x, z and r, the following shapes are created.
Program error (P191) will occur in (b) and (c) unless the following condition is satisfied.
|x| |r|
as "Q0". If a value exceeding "360.000" is commanded in G175 Q address, this will be handled as "Q360.000". G175 cuts one row with one cycle. To cut two rows, change the Q value, and issue the same command. Also, follow the precautions for the thread cutting command (G33).
(a) z < 0, x < 0, r < 0 (b) z < 0, x < 0, r > 0
(c) z > 0, x < 0, r < 0 (d) z > 0, x < 0, r > 0
Z
X
z
r x
1(R)
3(R)
4(R)2(F)
Z
X
r
x
z
1(R)
3(R)
2(F) 4(R)
Z
X
r x
z
1(R)
3(R)
2(F) 4(R)
Z
X
x
r
4(R) z
1(R)
3(R)
2(F)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
435 IB-1501277-P
13.3.3 Face Cutting Cycle; G176
The face cutting cycle performs continuous straight and taper cutting in the face direction.
(*1) If the commanded axis and selected plane are different when the fixed cycle for turning machining is command- ed, or if the movement amount is not specified in either or both of the selected plane axis commands, a program error (P114) will occur. Whether this is judged to be a program error depends on the MTB specifications (pa- rameter "#1241 set13/bit4" ("fixed cycle for turning machining" selected-plane axis check disabled)).
Function and purpose
Command format
Straight cutting
G176 X__ Z__ F__ ;
X X axis end point coordinate (*1) Z Z axis end point coordinate (*1) F Feedrate
Taper cutting
G176 X__ Z__ R__ F__ ;
X X axis end point coordinate (*1) Z Z axis end point coordinate (*1) R Taper depth (radius designation, incremental position, sign required) F Feedrate
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
436IB-1501277-P
Detailed description
Straight cutting
(R) Rapid traverse (F) Cutting feed (E) End point coordinates
Taper cutting
(R) Rapid traverse (F) Cutting feed (E) End point coordinates
Z
X
1(R) 2(F)
4(R)
3(F)
(E) (x,z)
Z
X
r
1(R)
2(F)
4(R)
3(F)
(E) (x,z)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
437 IB-1501277-P
With a single block, the tool stops at the end points of operations 1, 2, 3 and 4 shown above.
Depending on the signs of x, z and r, the following shapes are created.
Program error (P191) will occur in (b) and (c) unless the following condition is satisfied.
|z| |r|
Detailed description
(a) z < 0, x < 0, r < 0 (b) z < 0, x < 0, r > 0
(c) z > 0, x < 0, r < 0 (d) z > 0, x < 0, r > 0
Z
X
z
r
x
13
4
2 Z
X
z r
x
1
3
4
2
Z
X
z
r
1 3
4
2
x
Z
X r
1z 3
4
2
x
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
13 Fixed Cycle
438IB-1501277-P
14
439 IB-1501277-P
Macro Functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
440IB-1501277-P
14Macro Functions 14.1 Subprogram Control; M98, M99, M198
14.1.1 Subprogram Call; M98, M99
Fixed sequences or repeatedly used parameters can be stored in the memory as subprograms that can then be called from the main program when required. M98 serves to call subprograms and M99 serves to return operation from the subprogram to the main program. Furthermore, it is possible to call other subprograms from particular sub- programs. The nesting depth depends on the model.
The table below shows the functions that can be executed by adding and combining the tape memory/editing func- tions, subprogram control functions and fixed cycle functions.
(*1) Symbol "" denotes available functions and symbol "" denotes unavailable functions.
(*2) Variables cannot be transferred with the M98 command, but variable commands in subprograms are available if the variable command specifications are provided.
(*3) The depth of nesting call depends on the model.
Function and purpose
Case 1 Case 2 Case 3 Case 4
1. Tape memory and editing Yes Yes Yes Yes 2. Subprogram control No Yes Yes No 3. Fixed cycles No No Yes Yes
Function 1. Memory mode 2. Tape editing (main memory) 3. Subprogram call 4. Subprogram variable designation (*2) 5. Subprogram nesting call (*3) 6. Fixed cycles 7. Editing subprogram for fixed cycle
M98 P1 ;
P1000 P1 P2 Pn
M99 ;
M99 ; M99 ;
M02/M30 ;
M98 P2 ;
M98 P3 ;
Main program: Level 0 (P1000)
Subprogram: Level 1 (P1)
Subprogram: Level 2 (P2)
Subprogram: Level n (Pn)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
441 IB-1501277-P
(*1) To use memory2 (extended area), additional specification of part program storage capacity of 2560 [m] or 5120 [m] is required. If the specification is invalid, program error occurs when ",D1" is designated.
(*2) Program in extended area can be called as a subprogram from the program in basic area and program within the other extended area. Note that program in extended area can call a program in basic area as well.
Command format
Subprogram call
M98 P__ H__ L__ ,D__ ;
M98
P Program number in subprogram to be called (own program if omitted) Note that P can be omitted only for memory mode, MDI operation, high-speed program server operation, SD card operation, hard disk operation, or USB operation. (Numeric value of up to 8 digits) Use a parameter to specify a 4- or 8-digit subprogram No. starting with O. However, if the commanded value is bigger than the digit number set with parameter, a subprogram call is carried out as commanded.
H Program sequence number in subprogram to be called (head block if omitted) L Number of subprogram repetitions
(If omitted, it is assumed to be "L1", and processing is not carried out when "L0" is set.)
(1 to 9999 times depending on the 4-digit value)
For instance, M98 P1 L3; is equivalent to the following: M98 P1 ; M98 P1 ; M98 P1 ;
,D [M8]
Subprogram device No. (0 to 4) The subprogram is searched according to the setting of parameter "#8890 Subpro srch odr D0" to "#8894 Subpro srch odr D4" when ",D" is omitted. The device No. is set to the parameter, such as "#8880 Subpro stor D0: dev".
,D [C80]
Subprogram device No. (0 to 1) When ",D" command is omitted, the subprogram is searched in the area where main pro- gram is being executed. ,D0: Basic area (memory) ,D1: Extended area (memory2) (*1)
Return to main program from subprogram
M99 P__ ;
P Sequence No. of return destination (returned to block that follows the calling block)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
442IB-1501277-P
Subprograms have the same format as machining programs for normal memory mode, except that the subprogram completion instruction "M99 (P_);" must be commanded alone in the last block.
(1) The above program is registered by editing operations at the setting and display unit. For further details, refer to the section on "program editing" in the Instruction Manual.
(2) Only those subprogram Nos. ranging from 1 to 99999999 designated by the optional specifications can be used. When there are no program Nos. on the tape, they are registered as the setting No. for "program input."
(3) If a program is called from a subprogram over the nesting depth determined in the specifications, the program error (P230) will occur.
(4) Main programs and subprograms are registered in the order they were read without distinction. Therefore, main programs and subprograms should not be given the same Nos. (If they are, error "E11" will be displayed at reg- istration.)
(5) Main programs can be executed during memory, tape, MDI, or BTR mode, but subprograms must be in the mem- ory mode.
(6) Besides the M98 command, subprogram nesting is subject to the following commands: G65: Macro call G66: Modal call G66.1: Modal call G Code call Miscellaneous function call MDI interruption Automatic tool length measurement Macro interruption Multiple-step skip function
(7) The following commands can be called even if the nesting depth exceeds the determined depth in the specifica- tions because they are not subject to subprogram nesting. Fixed cycles Pattern cycles
(8) To repeatedly use the subprogram, it can be repeated l1 times by programming M98 Pp1 Ll1;. (9) When using the multi-part system, if the subprogram attributed to the part system with the call command is emp-
ty, the subprogram call operation will change according to the parameters. (These parameters depend on the MTB specifications.)
Detailed description
Creating and registering subprograms
O******** ; Program No. as subprogram No. ....... ; : ....... ;
Main body of subprogram
M99 ; Subprogram return command %(EOR) Registration completion code
#1285 ext21/ bit1
Description
OFF The subprogram registered in the memory for the selected part system is called out. ON The subprogram registered in the memory for the selected part system is called out. If the sub-
program in the selected part system is empty, the subprogram with the same No. in the 1st part system is called out.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
443 IB-1501277-P
When there are 3 subprogram calls (known as 3 nesting levels)
Sequence of execution: (a)-(b)-(c)-(c')-(b')-(a')
(1) For nesting, the M98 and M99 commands should always be paired off on a 1:1 basis; (a)' for (a), (b)' for (b), etc. (2) Modal information is rewritten in the order of execution sequence without distinction between main programs and
subprograms. Therefore, after calling a subprogram, attention must be paid to the modal data status when pro- gramming.
The M98 H_ ; M99 P_ ; commands designate the sequence Nos. in a program with a call instruction.
Program example
Program example 1
Program example 2
M98P10; M98P20;
M99; M99; M99;
O1;
M98P1;
M02;
O10; O20;
(a')
(a) (b) (c)
(b') (c')
Main program Subprogram 1 Subprogram 2 Subprogram 3
M98H3;
N3___;
M99;
M98H__ ;
N100___; M98P123; N200_; N300___; N400___;
O123;
M99P200;
M99P__ ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
444IB-1501277-P
(1) The program error (P232) will occur when the designated P (program No.) cannot be found. (2) The M98 P_ ; M99 ; block does not perform a single block stop. If any address except O, N, P, L or H is used,
single block stop can be executed. (With "X100. M98 P100 ;", the operation branches to O100 after X100. is executed.)
(3) When M99 is commanded by the main program, operation returns to the head. (This is the same as for MDI.) (4) Branching from tape and BTR mode to the subprogram with M98 P_; is possible, but the return destination se-
quence No. cannot be designated with M99 P_ ; . (P_ is ignored.) (5) Note that it takes time to search when the sequence No. is designated by M99 P_ ;. (6) When using a file name for the subprogram, specify the file name with 32 characters or less, including the ex-
tension. If a file name exceeding 32 characters is specified, a program error (P232) will occur. (7) All the programs are registered as files. For example, when calling a file "0100" as a subprogram, "0100" cannot
be searched with M98P100 or M98P0100. When numerical values are specified after P, 0 is ignored. In this case, it is regarded that the program No. (file) "100" is specified. To call a program like "0100" , specify the file name using the M98<0100> format.
(8) A subprogram added O No. is searched with the parameter setting (#8129="1" or "2") which calls a subprogram with O No. as priority. If a subprogram with O No. is not found, a subprogram with a name specified with the P command is searched.
ple, 123, O0123 and O00000123 can be considered identical.) Refer to the next page for operation examples of subprogram search with the setting which calls subprograms with O No. as priority.
(a) With designation of device No. Only the designated devices are subject to search. (The following is an example of M8 series.)
[Parameter setting]
#8129 Subpro No. select = 1 (Four-digit program No. beginning with O No.) #8880 Subpro stor D0 dev = R (Memory card) #8882 Subpro stor D1 dev = D (Data server) #8884 Subpro stor D2 dev = G (Hard disk)
Precautions
444
O0333
222
O0111
M02;
M98 P222,D1;
HD (D2)
Memory card (D0)
Memory card not inserted
Data server (D1)
Calling program
Main program
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
445 IB-1501277-P
(b) Without designation of device No. [M8] A subprogram with O No. is searched according to the settings of #8890 (D0 in order of subprogram search) to #8894 (D4 in order of subprogram search). (Refer to the solid line arrows "a" and "b" in the figure.) If a subprogram with O No. is not found, subprograms with a name designated with the P command are searched in order of the parameter setting. (Refer to the broken lines "c" and "d" in the figure.) If none of the designated subprogram storage locations are subject to search, memories are searched.
If any device or directory designated as the subprogram storage location is not found due to a reason such as absence, poor contact and contact failure of a memory card, the said device or directory will be excluded from the search target.
[Parameter setting]
#8129 Subpro No. select = 1 (Four-digit program No. beginning with O No.) #8880 Subpro stor D0 dev = R (Memory card) #8882 Subpro stor D1 dev = D (Data server) #8884 Subpro stor D2 dev = G (Hard disk) #8890 Subpro srch odr D0 = 1 #8891 Subpro srch odr D1 = 2 #8892 Subpro srch odr D2 = 3
[C80] Subprogram is searched inside of the currently selected device.
(9) When a program in an external device such as a USB memory device is executed, a period of processing time is required in the subprogram call or in the instruction to change the flow of the program such as GOTO or DO- END; therefore, interpolation may be decelerated or stopped.
Note
d
b
c
a
(3)
(2)
(1)
444
O0333
222
O0111
M02;
M98 P444;
Main program
Calling program
Subprogram search order
HD (D2)
Data server (D1)
Memory card not inserted
Memory card (D0)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
446IB-1501277-P
14.1.2 Subprogram Call; M198
Programs registered in the SD card can be called as a subprograms. To call a program in the SD card as a subpro- gram, command the following with the main program.
(1) Sequence No. call (M198 H***) cannot be commanded.
(1) The device that can be used for M198 subprogram call differs depending on the NC models. The SD card in the front side is available for M800S/M80, and the SD card in the control unit is available for M800W. (The M198 command is not available for the C80 series.)
(2) The subprogram can be called with the M198 command once in the subprogram nest. The subprogram can be called only from the memory or MDI program.
(3) The section from the head of the program to the first LF (line feed code, 0x0A hexadecimal) is invalid, and is not run or displayed. Note that if the head starts with a O No., the program will be valid from the head.
(4) A program registered in an SD card can be executed from only one part system. A program error will occur if an attempt is made to execute the programs in the SD card simultaneously by two or more part systems. If all the part system is reset when the error occurred, programs will be displayed as only "%" except for the first part sys- tem.
(5) Refer to "14.1.1 Subprogram Call; M98, M99" for
Function and purpose
Command format
Subprogram call
M198 P__ L__ ;
M198
P Program No. in SD card to be called as a subprogram. (Max. 8 digits) Use a parameter to specify a 4- or 8-digit subprogram No. starting with O. However, if the commanded value is bigger than the digit number set with parameter, a subprogram call is carried out as commanded.
L Number of subprogram repetitions. (Max. 4 digits) This can be omitted. (In this case, the subprogram will be called once.) When "L0" is designated, the subprogram call will not be executed.
Return to main program from subprogram
M99 ;
Detailed description
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
447 IB-1501277-P
14.1.3 Figure Rotation; M98 I_J_K_
If the same pattern is used repeatedly on a concentric circle, one of the rotating machining patterns can be registered as a subprogram. When the subprogram is called from the main program, if the rotation center is designated, a path similar to the rotary phase can be easily created on the concentric circle. This simplifies creation of the program.
Function and purpose
Command format
Subprogram call command
M98 I__ J__ K__ P__ H__ L__ ,D__ ;
M98 I__ J__ K__
I, J, K Rotation center coordinates P Program number in subprogram to be called (own program if omitted)
Note that P can be omitted only for memory mode, MDI operation, high-speed program server operation, SD card operation, hard disk operation, or USB operation. (Numeric value containing up to eight digits) Use a parameter to specify a 4- or 8-digit subprogram No. starting with O.
H Program sequence number in subprogram to be called (head block if omitted) L Number of subprogram repetitions
(If omitted, it is assumed to be "L1", and processing is not carried out when "L0" is set.) (1 to 9999 times depending on the 4-digit value)
,D Subprogram device No. (0 to 4). The subprogram in the memory can be used when ,D is omitted. The device No. is set with the machining parameters.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
448IB-1501277-P
(1) The first subprogram called out with subprogram call is executed at 0 rotation angle. The path is created as commanded.
(2) If the number of repetitions is set to twice or more, the rotation angle is obtained from the called subprogram's start point, end point and rotation center coordinate. The path of the first subprogram is used as the basic figure and is rotated and arranged for the designated number of call repetitions, using the rotation center coordinates as a reference.
(3) All blocks in the subprogram are rotated. (4) If the subprogram start point and end point are not on the same circle having the commanded figure rotation
center coordinates as the center, the axis will interpolate using the subprogram's end point as the start point, and the end point in the first movement command block in the rotated subprogram as the end point.
(5) Both absolute command and incremental command can be used in the figure rotation subprogram. Even if com- manded with an absolute command, the rotation will be the same as when commanded with an incremental com- mand.
(6) I, J and K are commanded with the incremental amount from the start point. (7) A subprogram of which figure is rotating cannot be branched to the other subprogram. (8) The figure is rotated on the workpiece coordinate system, and can be shifted with the G92, G52, G54 to G59
(workpiece coordinate system shift) command. (9) Functions (reference position return, uni-direction positioning, etc.) on the machine coordinate system for the ro-
tary plane axis cannot be used while the figure is rotated. However, the machine coordinate system functions can be used for axes other than the rotation plane.
(10) Refer to "14.1.1 Subprogram Call; M98, M99" for
Detailed description
(a) Basic figure (b) Center of rotation
J
I
(a)
(b)
L
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
449 IB-1501277-P
(1) A program error will occur if figure rotation is commanded during figure rotation. (2) Figure rotation and program coordinate rotation cannot be commanded simultaneously. The program error will
occur.
Program example
Main program (O1000) N01 G90 G54 G00 X0 Y0 ; N02 G01 G41 X200. Y150. D01 F500 ; N03 G01 Z-50. F300 ; N04 M98 P2200 L5 J-100. ; N05 G90 G01 Z50. F500 ; N06 G40 ; N07 G00 X0 Y0 ;
Subprogram (O2200) N01 G91 G01 X29.389 Y-59.549 ; N02 X65.717 Y-9.549 ; N03 M99 ;
(a) Basic figure
Precautions
200.
100. 300.
Y
X
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
450IB-1501277-P
14.2 Variable Commands
Programming can be endowed with flexibility and general-purpose capabilities by designating variables, instead of giving direct numerical values to particular addresses in a program, and by assigning the variable values depending on the conditions that exist when executing the program. All common variables are retained even when the power is turned OFF. When the power is turned OFF or reset, the common variables can be set to
(1) The 4 standard operators are +, -, * and /. (2) Functions cannot be used unless the user macro specifications are available. (3) Error (P241) will occur when a variable No. is negative. (4) Examples of incorrect variable expressions are given below.
Function and purpose
Command format
#= ;
#*** = [formula] ;
Detailed description
Variable expressions
Example
#m m = value consisting of 0 to 9 #100 # [f] f = one of the followings in the formula #[-#120]
Numerical value m 123 Variable #543 Formula Operator Formula #110+#119 - (minus) formula -#120 [Formula] [#119] Function [formula] SIN[#110]
Incorrect Correct
#6/2 # [6/2] (#6/2 is regarded as [#6] /2.) #--5 #[-[-5]] #-[#1] #[-#1]
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
451 IB-1501277-P
The following table gives the types of variables. The common variables are divided into the following two types. Common variables 1: Used in common through all part systems Common variables 2: Used in common in the programs of the part system
(*1) Common variable address #400s can only be used when there are 700 or more sets of common variables and the MTB specifications are valid (parameter "#1336 #400_Valtyp"). When common variable address #400s can be used, these can be displayed and set on the common variable screen. It also becomes possible to input/output data of common variable address #400s.
(*2) When the parameter "#1052 MemVal" is set to "1" in multi-part system (MTB specifications), some or all of com- mon variables "#100 to #199" and "#500 to #999" can be shared and used between part systems. The number of variables sharable in part systems depends on the MTB specifications (parameters "#1303 V1comN" and "#1304 V0comN").
(Example) When "#1304 V0comN" is set to "5":
Depending on the MTB specifications, the common variables #100 to #199 are used for each part system, and variables #500 to #999 are common for the part systems (parameter "#1052 MemVal"). Address #400s, that can be used as common variable with 700 or more sets of variable, is common for the part systems regardless of the setting of parameter "#1052 MemVal".
(*3) When "#1052 MemVal" is set to "1", #900000 to #907399 available for 8,000 sets of variable are not available.
Types of Variables
Type No. Function
Common variable Common variables 1 Common variables 2
Can be used in common throughout main, sub and macro programs. When using common variables in the
multi-part system, the number of com- mon variables shared between the part systems can be specified depending on the MTB specifications (parameter "#1052 MemVal").
(*2) (Only for C80 series) Can be read from/
written to each common variable by us- ing ZR80000 or later. Refer to "PLC Interface Manual" for the correspondence between the ZR de- vice No. and the common variable No.
1 part sys- tem
200 sets 500 - 599 100 - 199 600 sets 500 - 999
100100 - 800199 (*4) 100 - 199
700 sets 400 - 999 (*1) 100100 - 800199 (*4)
100 - 199
8000 sets 400 - 999 (*1) 100100 - 800199 (*4) 900000 - 907399 (*3)
100 - 199
Multi-part systems (n = number of part sys- tems)
600 + 100 * n sets
400 - 999 (*1) 100100 - 800199 (*4)
100 - 199 *n
7900 + 100 * n sets
400 - 999 (*1) 100100 - 800199 (*4) 900000 - 907399 (*3)
100 - 199 *n
Local variables 1 - 33 Can be used as local variables in macro programs.
ZR device access variables (only for C80 series)
50000 - 50749 51000 - 51749 52000 - 52749
Can be read and written by the PLC or GOT.
System variable 1000 - Application is fixed by system. Fixed cycle variables 1 - 32 Local variables in fixed cycle programs.
#500 to #504: Common for the part systems #505 to #999: Each part system
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
452IB-1501277-P
(*4) When the parameter "#1316 CrossCom" is set to "1", the common variables #100100 to #800199 can be shared between the part systems. (This depends on the MTB specifications.) The part system common variable which can be used is shown in the table below.
(Example)
<1-part system>
Common variables for each part system #100 to #199" in other part system can be used.
The PLC data reading function cannot be used, which uses system variables #100100 to #100110, and variables #100100 to #100110 are used as common variables.
The setting of number of common variables shared between the part systems (The parameter #1052 MemVal" is set to "1") becomes invalid, thus the movement is the same as "0" is set.
When the parameters "#1128 RstVCl", "#1129 PwrVCl" are set to "1", the operation is as follows. "#1128 RstVCl" The common variables shared between the part systems equivalent to #100 to #199 of the reset part sys- tem are cleared. (Example) If the 1st part system is reset, #100100 to #100199 are cleared.
If the 2nd part system is reset, #200100 to #200199 are cleared. "#1129 PwrVCl" The common variables shared between the part systems equivalent to #100 to #199 in the valid part sys- tem are cleared. (Example) In 1st part system, #100100 to #100199 are cleared.
In 2nd part system, #100100 to #100199 and #200100 to #200199 are cleared. Common variables shared between the part systems #100100 to #800199 can be displayed and set on
the common variable screen. If common variables #100100 to #800199 are used when the number of sets of common variables is
less than 600 sets or the parameter "#1316 CrossCom" is "0", a program error (P241) will occur.
Variable sets Common variables 1 (When "#1316 CrossCom" = "1")
Variable sets specification
600 sets (500 + 100 sets) #100100 to #100199 (Equivalent to # 100 to #199 in 1st part system) #200100 to #200199 (Equivalent to # 100 to #199 in 2nd part system) #300100 to #300199 (Equivalent to # 100 to #199 in 3rd part system) #400100 to #400199 (Equivalent to # 100 to #199 in 4th part system) #500100 to #500199 (Equivalent to # 100 to #199 in 5th part system) #600100 to #600199 (Equivalent to # 100 to #199 in 6th part system) #700100 to #700199 (Equivalent to # 100 to #199 in 7th part system) #800100 to #800199 (Equivalent to # 100 to #199 in 8th part system)
700 sets (600 + 100 sets)
8000 sets (7900 + 100 sets)
#100100=200 ; Equivalent to #100 = 200 ; #200105=#100 ; "200" is set to #200105. #300110=#100100 ; "200" is set to #300110. #800199=#500120 ; The variable value of "#500120" is set to #800199.
$1 #200100=-100 ; "-100" is set to #100 of 2nd part system. #101=#200102 ; "#101" is set to #102 of 2nd part system. #300105=#200103 ; "#103" of 2nd part system is set to #105 of 3rd part system. #110=#500107 ; The variable value of "#500107" is set to #110.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
453 IB-1501277-P
(1) When inputting the common variable data, if the following illegal variable No. data exist in the input file, the illegal variable No. data is ignored and only the correct common variable data will be input. Variable data that is not common variables such as local variables (#1 to #33) or system variables (#1000
and after) Variable data of which the number of common variable sets does not match the pre-specified value (Example)
If variables of # numbers undefined in the specifications exist in the input file when there are 700 sets of common variables (#100 to #199, #500 to #999, and #100100 to #800199), they are ignored, and only the variables de- fined in the specifications are input.
Variables can be used for all addresses except O, N and / (slash).
(1) When the variable value is used directly:
(2) When the complement of the variable value is used:
(3) When defining variables:
(4) When defining the variable arithmetic formula:
(1) A variable cannot be defined in the same block as an address. It must be defined in a separate block.
(2) Up to five sets of square parentheses [ ] may be used. #543 = -[[[[[#120]/2+15.]*3-#100]/#520+#125+#128]*#130+#132]
(3) There are no restrictions on the number of characters and number of variables for variable definition. (4) The variable values should be within the range of 0 to 99999999.
If this range is exceeded, the arithmetic operations may not be conducted properly. (5) The variable definitions become valid when definitions are made.
#1 = 100 ; ............................. #1 = 100 #1 = 200 #2 = #1 + 200 ; ..... #1 = 200, #2 = 400 #3 = #1 + 300 ; ..................... #3 = 500
(6) Variable quotations are always regarded as having a decimal point at the end. When #100 is set to 10 X#100; is set to X10..
(7) The significant digits of the variable are up to 15 decimal digits. Note that the calculation may cause an error. For example, in the following formula, correct judgment cannot be made due to the error. IF [#10 EQ #20] Calculate with attention to the error when comparing variables. If the difference between the variables to be com- pared falls within the specified error range as in the following formula, consider them as equal. If the error is less than 0.01, describe the formula as follows. IF [ABS [#10 - #20] LT 0.01]
Variable quotations
X#1 Value of #1 is used as the X value.
X-#2 Value with the #2 sign changed is used as the X value.
#3 = #5 Variable #3 uses the equivalent value of variable #5. #1 = 1000 Variable #1 uses the equivalent value 1000. ("1000" is assumed to be "1000.".)
#1 = #3 + #2 - 100 Value of the operation result of "#3 + #2 - 100." is used as the #1 value. X[#1 + #3 + 1000] Value of the operation result of "#1 + #3 + 1000" is used as the X value.
Incorrect Correct X#1 = #3 + 100 ; #1 = #3 + 100 ;
X#1 ;
Note
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
454IB-1501277-P
(1) If the common variable protection function is valid, the common variables in the range specified in the parameters (#12111 to #12114) cannot be changed from machining program or screen operation, or user operation such as file input. This function depends on the MTB specifications (parameter "#1391 User level protect").
(2) If an attempt is made to change the value or name of the protected variable on the machining program, the pro- gram error (P243) will occur, causing the operation to be stop. Such a variable value or name can be changed using the machine tool builder macro program, but cannot be done by the user. Multiple variable names can be changed in one block with the SETVNn command. However, if at least one of them is protected, the program error (P243) will occur.
(3) If "#1128 RstVCl" is set to "1", the variables (#100 to #199) are cleared after reset even if common variables (#100 to #199) are protected.
(4) If "#1129 PwrVCl" is set to "1", the variables (#100 to #199) are cleared at the power-ON even if common vari- ables (#100 to #199) are protected.
(5) For common variables used common to the part systems, the variable values and variable names can be changed by the displayed part system.
Protection of common variable
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
455 IB-1501277-P
14.3 User Macro
A group of control and arithmetic instructions can be registered and used as a macro program to make it one inte- grated function. Macro programs use variables, control and arithmetic instructions to create subprograms which function to provide special-purpose controls. By combining the user macros with variable commands, it is possible to use the macro program call, arithmetic op- erations, data input/output with PLC, control, decision, branch and many other instructions for measurement and other such applications.
These special-purpose control functions (macro programs) are called by the macro call instructions from the main program when needed.
(1) When the G66 or G66.1 command is entered, the specified user macro program will be called every time a block is executed or after a movement command in blocks with a movement command is executed, until the G67 (can- cel) command is entered.
(2) The G66 (G66.1) and G67 commands must be paired in a same program.
Function and purpose
G code Function
G65 User macro Simple call G66 User macro Modal call A (Movement command call)
G66.1 User macro Modal call B (Per-block call) G67 User macro Modal call (G66, G66.1) cancel
Detailed description
;;
G65/G66/G66.1
M30; M99;
Main program Subprogram
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
456IB-1501277-P
14.4 Macro Call Instructions
Macro call commands include the simple calls which call only the instructed block and the modal calls (types A and B) which call a block in the call modal.
When the macro argument L/P valid function is enabled, the addresses L (number of subprogram repetitions) and P (calling program No.) used as commands in user macro can be used as arguments.
The validity of this parameter depends on the MTB specifications (Parameter "#1241 set13"/bit5 (Macro argument L/P valid)). For C80, the macro argument L/P function is unavailable. When a program in an external device such as a USB memory device is executed, a machining program stored in USB memory cannot be called with a macro call such as G65, G66, or G66.1. Using such a macro calls a macro program in memory.
14.4.1 Simple Macro Calls; G65
(*1) Can also be used as an argument at the same time as the macro argument L/P valid function is enabled. (M8 Series)
Function and purpose
Function and purpose
M99 is used to terminate the user macro subprogram.
Command format
Simple macro calls
G65 P__ L__ argument ;
Simple macro calls
G65
P Program No. (*1) Use a parameter to specify a 4- or 8-digit subprogram No. starting with O.
L Number of repetitions (*1)
If omitted, this value is set to "1". (0 to 9999) Argument Specify variable data
Subprogram(O__)
G65 P__ L__ ;
O__
M99 ;
Main program
to Subprogram
to Main program
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
457 IB-1501277-P
(1) When the argument must be transferred as a local variable to a user macro subprogram, the actual value should be designated after the address. In this case, regardless of the address, a sign and decimal point can be used in the argument. There are 2 ways in which arguments are designated.
Format : A_ B_ C_ ......X_ Y_ Z_
(a) Arguments can be designated using any address except G, L, N, O and P. (b) I, J and K must be designated in alphabetical order.
I_ J_ K_...Correct J_ I_ K_...Incorrect
(c) Except for I, J and K, there is no need for designation in alphabetical order. (d) Addresses which do not need to be designated can be omitted. (e) The following table shows the correspondence between the addresses which can be designated by argument
designation I and the variable numbers in the user macro main body.
(*1) Can be used while G66.1 command is modal
(*2) Can be used while the macro argument L/P valid function is enabled.
Detailed description
Argument designation I
Address and variable No. correspondence Addresses available for call instructions
Argument designation I ad- dress
Variable in macro G65, G66 G66.1
A #1 B #2 C #3 D #7 E #8 F #9 G #10 (*1) H #11 I #4 J #5 K #6 L #12 (*1)(*2) M #13 N #14 (*1) O #15 P #16 (*1)(*2) Q #17 R #18 S #19 T #20 U #21 V #22 W #23 X #24 Y #25 Z #26
: Available : Unavailable
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
458IB-1501277-P
Format: A__B__C__I__J__K__I__J__K__...
(a) In addition to address A, B and C, up to 10 groups of arguments with I, J, K serving as 1 group can be designated. (b) When the same address is duplicated, designate the addresses in the specified order. (c) Addresses which do not need to be designated can be omitted. (d) The following table shows the correspondence between the addresses which can be designated by argument
designation II and the variable numbers in the user macro main body.
(1) The numbers 1 to 10 accompanying I, J and K indicate the sequence of the commanded sets, and are not required in the actual command.
Argument designation II
Argument designation II address
Variable in macro Argument designation II address
Variable in macro
A #1 J5 #17 B #2 K5 #18 C #3 I6 #19 I1 #4 J6 #20 J1 #5 K6 #21 K1 #6 I7 #22 I2 #7 J7 #23 J2 #8 K7 #24 K2 #9 I8 #25 I3 #10 J8 #26 J3 #11 K8 #27 K3 #12 I9 #28 I4 #13 J9 #29 J4 #14 K9 #30 K4 #15 I10 #31 I5 #16 J10 #32
K10 #33
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
459 IB-1501277-P
(1) If addresses corresponding to the same variable are commanded when both types I and II are used to designate arguments, the latter address will become valid. (Example 1)
In the above example, I7.7 argument is valid when both arguments D3.3 and I7.7 are commanded for the #7 variable.
(2) If calling a subprogram numbered with O is enabled, a sub program number starting with O and specified by P command value is called with a priority. However, when P command value is less than the digit number set with parameter "#8129 Subpro No. select", increase the digit number of command value by adding leading zeros. (Example) When parameter "#8129 Subpro No. select"="1", call the subprogram "O0012" with "G65 P12" com- mand.
(3) In the following cases, a subprogram of P command value without O No. is called even with a setting to call a subprogram with O No. The digit number of P command value is over the digit number of the program number set with parameter
"#8129 Subpro No. select". A subprogram starting with commanded O No. does not exist.
Using arguments designations I and II together
Call command
Variable
G65 A1.1 B-2.2 D3.3 I4.4 I7.7;
#1: 1.1
#2:-2.2
#3:
#4: 4.4
#5:
#6: #7: 3.3 7.7
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
460IB-1501277-P
14.4.2 Modal Call A (Movement Command Call) ; G66
When the block with a movement command is commanded between G66 and G67, the movement command is first executed and then the designated user macro subprogram is executed. A number of user macro subprograms are designated with "L". The argument is the same as for a simple call.
(*1) Can also be used as an argument at the same time as the macro argument L/P valid function is enabled. (M8 Series)
Function and purpose
Command format
Modal call A
G66 P__ L__ argument ;
G66
P Program No. (*1) Use a parameter to specify a 4- or 8-digit subprogram No. starting with O.
L Number of repetitions (*1) Argument Specify variable data
Modal call end
G67;
G66 P__ L__ ;
G67 ;
O__
M99 ;
Main program Subprogram
to Subprogram
to Subprogram
to Main program
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
461 IB-1501277-P
(1) When the G66 command is entered, the specified user macro program will be called after the movement com- mand in a block with the movement commands has been executed, until the G67 (cancel) command is entered.
(2) The G66 and G67 commands must be paired in a same program. A program error will occur when G67 is issued without G66. (Example) Drill cycle
(3) If calling a subprogram numbered with O is enabled, a sub program number starting with O and specified by P command value is called with a priority. However, when P command value is less than the digit number set with parameter "#8129 Subpro No. select", increase the digit number of command value by adding leading zeros. (Example) When parameter "#8129 Subpro No. select"="1", call the subprogram "O0012" with "G66 P12" command.
(4) In the following cases, a subprogram of P command value without O No. is called even with a setting to call a subprogram with O No. The digit number of P command value is over the digit number of the program number set with parameter
"#8129 Subpro No. select". A subprogram starting with commanded O No. does not exist.
Detailed description
N1 G90 G54 G0 X0 Y0 Z0;
N2 G91 G00 X-50.Y-50.Z-200.;
N3 G66 P9010 R-10.Z-30.F100;
N4 X-50.Y-50.;
N5 X-50.;
N6 G67;
O 9010
N10 G00 Z #18 M0;
N20 G09 G01 Z #26 F#9;
N30 G00 Z- #18+#26 ;
M99
W N1
N10
N20 N30
N2
N3
N4 N5
X
-50.
-50.
-100.
-100.-150.
Y Argument F
Argument R
Argument Z
Main program
To subprogram after axis command execution
To subprogram after axis command execution
Subprogram
To main program
to subprogramto subprogram
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
462IB-1501277-P
14.4.3 Modal Call B (for Each Block); G66.1
The specified user macro subprogram is called unconditionally for each command block that is assigned between G66.1 and G67 and the subprogram will be repeated for the number of times specified in L. The argument is the same as for a simple call.
(*1) Can also be used as an argument at the same time as the macro argument L/P valid function is enabled. (M8 Series)
Function and purpose
Command format
Modal call B
G66.1 P__ L__ argument ;
G66.1
P Program No. (*1) Use a parameter to specify a 4- or 8-digit subprogram No. starting with O.
L Number of repetitions (*1) Argument Specify variable data
Modal call end
G67;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
463 IB-1501277-P
(1) In the G66.1 mode, everything except the O, N and G codes in the various command blocks which are read are handled as the argument without being executed. Any G code designated last or any N code commanded after anything except O and N will function as the argument.
(2) All significant blocks in the G66.1 mode are handled as when G65 P_ is assigned at the head of a block. (Example 1) In "G66.1 P1000;" mode, "N100 G01 G90 X100. Y200. F400 R1000 ;" is the same as "N100 G65 P1000 G01 G90 X100. Y200. F400 R1000 ;".
tween the argument address and the variable number is the same as for G65 (simple call). (3) The range of the G and N command values that can be used anew as variables in the G66.1 mode is subject to
the restrictions as normal NC command values. (4) Program number O, sequence numbers N and modal G codes are updated as modal information. (5) If calling a subprogram numbered with O is enabled, a sub program number starting with O and specified by P
command value is called with a priority. However, when P command value is less than the digit number set with parameter "#8129 Subpro No. select", increase the digit number of command value by adding leading zeros. (Example) When parameter "#8129 Subpro No. select"="1", call the subprogram "O0012" with "G66.1 P12" command.
(6) In the following cases, a subprogram of P command value without O No. is called even with a setting to call a subprogram with O No. The digit number of P command value is over the digit number of the program number set with parameter
"#8129 Subpro No. select". A subprogram starting with commanded O No. does not exist.
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
464IB-1501277-P
14.4.4 G Code Macro Call
User macro subprogram with prescribed program numbers can be called merely by issuing the G code.
(*1) Functions as an argument when the macro argument L/P valid function is enabled. (M8 Series) It cannot be used when the macro argument L/P valid function is disabled.
(1) The instruction functions in the same way as the instructions below, however, the correspondence between G codes and instructions can be set by parameters. (The parameter settings of the instructions depend on the MTB specifications.) a: M98 P****; b: G65 P****
When the parameters corresponding to "c" and "d" above are set, issue the cancel command (G67) either in the user macro or after the call code has been commanded so as to cancel the modal call.
(2) The correspondence between the "G**" (or "G*.*") which conducts the macro call and the macro program number "P****" to be called is set by parameters.
(3) The number of available G codes is up to 538, which is total of the following ones. Among G01 through G9999, 10 G codes can be set individually, and 255 G codes by batch setting. Among G0.1 through G999.9, 10 G codes can be set individually, and 255 G codes by batch setting. Other 8 G codes: G200, G300, G400, G500, G600, G700, G800, G900
(4) G codes used in the system becomes available as G code macro when the parameter "#1081 Gmac_P" is set to "1".
(5) These commands cannot be issued in a program which has been called by a G code macro. If issued in such a program, they will be handled as ordinary G commands.
(6) When ",D" or "<(Character string)>"is commanded in a block that is calling a G code macro, a miscellaneous command macro, or an ASCII macro while the macro argument L/P valid function is enabled, a program error (P33) will occur. This parameter setting depends on the MTB specifications. (Parameter "#1241 set13/bit5")
Function and purpose
Command format
Macro call via G code
G** P__ L__ argument ;
Macro call via G code with decimal point
G*.* P__ L__ ;
G** (G*.*) G code for macro call P (*1) L (*1)
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
465 IB-1501277-P
(7) The batch setting of macro call via G code is available. The batch setting of up to 255 consecutive macro pro- grams is possible by specifying the first G code, the first program number, the number of consecutive programs, and the type of macro call with the parameters. The same type applies to all macro programs. (Example) When the first G code is "152", the first program number is "7625", the number of consecutive programs is "10", and the type is "0".
(8) The batch setting of macro call via G code with decimal point is available. The batch setting of up to 255 consec- utive macro programs is possible by specifying the first G code, the first program number, the number of con- secutive programs, and the type of macro call with the parameters. The same type applies to all macro programs. (Example) When the first G code is "23.4", the first program number is "9012", the number of consecutive programs is "9", and type is "2".
(9) The batch setting of macro call via G code needs to satisfy the following conditions. When the number exceeds the limit, the batch settings of macro call via G code are all invalid. (First G code + Number of consecutive programs - 1) 9999 (First program number + Number of consecutive programs - 1) 99999999
(10) The batch setting of macro call via G code with decimal point needs to satisfy the following conditions. When the number exceeds the limit, the batch settings of macro call via G code with decimal point are all invalid. (First G code + Number of consecutive programs / 10 - 0.1) 999.9 (First program number + Number of consecutive programs - 1) 99999999
(11) When batch setting of macro call via G code duplicates, the command is executed in the following priority from top to bottom. Individual settings of macro call via G code (#7201 to #7293) Batch settings of macro call via G code (#7421 to #7424) Other 8 G code settings: G200, G300, ... , G900 (#7322 to #7393)
(12) When macro call via G code with decimal point duplicates, the command is executed in the following priority from top to bottom. Individual settings of macro call via G code with with decimal point (#56501 to #56593) Batch settings of macro call via G code with with decimal point (#7431 to #7434)
G code Equivalent command
G152 M98 P7625 G153 M98 P7626 G154 M98 P7627
: : G160 M98 P7633 G161 M98 P7634
G code Equivalent command
G23.4 arguments G66 P9012 arguments G23.5 arguments G66 P9013 arguments G23.6 arguments G66 P9014 arguments
: : G24.1 arguments G66 P9019 arguments G24.2 arguments G66 P9020 arguments
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
466IB-1501277-P
14.4.5 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call)
The user macro subprogram of the specified program number can be called merely by issuing an M (or S, T, B) code. (Registered M code and all S, T and B codes.)
[M8 Series]
[C80]
(*1) Functions as an argument when the macro argument L/P valid function is enabled. (M8 Series) It cannot be used when the macro argument L/P valid function is disabled.
(1) The above instruction functions in the same way as the instructions below, however, the correspondence be- tween M codes and instructions can be set by parameters. (Same for S, T and B codes)
When the parameters corresponding to "c" and "d" above are set, issue the cancel command (G67) either in the user macro or after the call code has been commanded so as to cancel the modal call.
(2) The correspondence between the "M**" which conducts the macro call and the macro program number P**** to be called is set by parameters. Up to 10 M codes from M00 to M9999 can be registered. Note that the codes to be registered should exclude those basically required for the machine and the following M codes. M0, M1, M2, M30, M96, M97, M98, M99, M198, and M codes for G83 specified in the parameter "#8083"
(3) As with M98, it is displayed on the screen display of the setting and display unit but the M codes and MF are not output.
(4) Even if the registered miscellaneous commands above are issued in a user macro subprogram which are called by an M code, it will not be regarded as a macro call and will be handled as a normal miscellaneous command. (Same for S, T and B codes)
(5) All S, T and B codes call the subprograms in the prescribed program numbers of the corresponding S, T and B functions.
Function and purpose
Command format
Miscellaneous command macro call
M** P__ L__ ; (or S** ; , T** ; , B** ;)
M**; (or S**;, T**;, B**;)
M** M code for macro call (or S, T, B code) P (*1) L (*1)
Detailed description
a: M98 P**** ; M98, M** are not output. b: G65 P**** M** ; c: G66 P**** M** ; d: G66.1 P**** M** ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
467 IB-1501277-P
(6) Up to 10 M codes can be set.
case, the alphabet before the M,S,T,B code macro is not handled as an argument. For example, commanding the M code and T code in the same block changes the operation depending on the order of the address. (Example) To register M06 in M code macro
(7) The address L and address P can be used as an argument when the macro argument L/P valid function is en- abled. This parameter setting depends on the MTB specifications (parameter "#1241 set13"/bit5). The argument address L is designated with variable #12 in the macro, and the argument address P with variable #16 in the macro.
(8) When the macro argument L/P function is enabled and the value is designated with macro type "M98", if address L and address P are commanded, a program error (P33) will occur.
(9) Even when the macro argument L/P valid function is enabled, argument codes G, L, N, O, and P are not dis- played on the local variable screen.
(10) When ",D" or "<(Character string)>" is commanded in a block that is calling a G code macro, a miscellaneous command macro, or an ASCII code macro while the macro argument L/P valid function is enabled, a program error (P33) will occur. This parameter setting depends on the MTB specifications. (Parameter "#1241 set13"/bit5)
(11) Even when the miscellaneous function lock signal (AFL) is enabled, the macro call instruction is executed.
M06 T02 The value of T is treated as variable #20 in macro. The value is entered in the T code at the same time.
T02 M06 The value is not entered in the variable #20 in macro. The value is entered in the T code.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
468IB-1501277-P
14.4.6 Detailed Description for Macro Call Instruction
(1) The argument can be designated for G65 but not for M98.
(2) The sequence number can be designated for M98, but not for G65, G66 and G66.1.
(3) M98 executes subprograms after all the commands except M, P, H and L in the M98 block are executed, but G65 branches directly to the subprogram without any further operation.
(4) When any address except O, N, P, H or L is included in the M98 block, the single block stop will be conducted, but not for the G65.
(5) The level of the M98 local variables is fixed but it varies in accordance with the nesting depth for G65. ("#1" before and after M98, for instance, has the same significance, but they have different significance in G65.)
(6) The M98 nesting depth extends up to 10 levels in combination with G65, G66 and G66.1. The G65 nesting depth extends up to only 4 levels in combination with G66 and G66.1.
Up to 4 nesting levels are available for macro subprogram calls by simple call or modal call. The argument for a macro call instruction is valid only within the called macro level. Since the nesting depth for mac- ro calls extends up to 4 levels, the argument can be used as a local variable for the programs of each macro call of each level.
(1) When a G65, G66, G66.1 G code macro call or miscellaneous command macro call is conducted, this is regarded as a nesting level and the level of the local variables is also incremented by one.
(2) With modal call A, the designated user macro subprogram is called every time a movement command is execut- ed. However, when the G66 command is duplicated, the next user macro subprogram is called to movement commands in the macro every time an axis is moved. User macro subprograms are called from the one commanded last.
(Example 1)
Detailed description
Differences between M98 and G65 commands
Macro call command nesting depth
Main program User macro operation
Note
G66Pp 1 ; p1
x1
p1 p1 p1
x2 M99w1
x1 x2 M99w1
x1 x2 M99w1
p2
p1
G66Pp 2 ;
Zz1 ;
Zz2 ;
Zz3 ;
Zz4 ; Zz5 ;
G67 ;
G67 ;
p1 call
After Z1 execution
p2 call
p2 cancel
After Z3 execution
p1 cancel
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
469 IB-1501277-P
(3) When M98 command is executed in G66 (G66.1) modal, the program designated by G66 (G66.1) will be exe- cuted after completing the movement command in the subprogram called by M98 (in case of G66.1, after com- pleting each block).
(Example 2)
When the program numbers of p1 and p2 are same, the program numbers of subprograms 1 and 2 will be same.
G66 Pp1;
G01 Xx1;
M98 Pp2;
G67;
G00 Xx2;
M99;
G00 Xx3;
M99;
G00 Xx2;
M99;
Main program
Subprogram 1
Subprogram 2 Subprogram 1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
470IB-1501277-P
14.4.7 ASCII Code Macro
A macro program can be called out by setting the correspondence of a subprogram (macro program) preregistered with the parameters to codes, and then commanding the ASCII code in the machining program. This function can be used in addition to the G, M, S, T and B miscellaneous command macro call function. These parameters depend on the MTB specifications.
(Execution example 1) M98 type
After outputting "2000" to common variable #146, the program No. 200 subprogram is called with the M98 subpro- gram call type.
Parameters
(Execution example 2) G65 type
After outputting "500" to local variable #1, the program No. 3000 subprogram is called out with the G65 macro call type.
Parameters
Function and purpose
#7401 (ASCII call Valid/Invalid) 1 (Valid) #7402 (ASCII code) D #7403 (Call type) 0 (M98 type) #7404 (Program No.) 200 #7405 (Common variable) 146
#7411 (ASCII call Valid/Invalid) 1 (Valid) #7412 (ASCII code) A #7413 (Call type) 1 (G65 type) #7414 (Program No.) 3000 #7415 (Common variable) 100 (Not used)
O0002; : D2000; : M30;
O200 : : : M99;
Main program Subprogram
O0003; : A500; : M30;
O3000 : : : M99;
Main program Subprogram
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
471 IB-1501277-P
(*1) Functions as an argument when the macro argument L/P valid function is enabled. (M8 Series) It cannot be used when the macro argument L/P valid function is disabled.
(1) The above command performs the same operations as the commands listed below. The correspondence of com- mands is set for each ASCII code with the parameters.
0 : M98 P****; 1 : G65 P****
When parameters corresponding to items 2 and 3 above are set, the modal call will be canceled. Thus, com- mand the cancel command (G67) after commanding the call code or during the user macro.
(2) The ASCII code for calling the macro and the program No. P**** to be called are set with the parameters. Up to two ASCII codes can be registered.
(3) The code section is output to the variables, but the output destination differs according to the call type and ad- dress. (a) For M98 type
The code section is output to a common variable and the variable No. is set with a parameter. When corresponding to the first address (parameter #7401), the section is output to the common variable which is indicated by the first variable No. (parameter #7404). (These parameters depend on the MTB spec- ifications.)
(b) For G65/G66/G66.1 type The code section is output to a local variable. The variable No. differs according to the address, and corre- sponds to the following table.
A, B, D, F, H, I, J, K, M, Q, R, S, T
Command format
**** P__ L__ ; ... Designates the address and code
ASCII code for calling out a macro (one character) **** Value or expression output to variable
(Setting range: 999999.9999) P (*1) L (*1)
Detailed description
Address # Address # Address #
A 1 K 6 U 21 B 2 L 12 V 22 C 3 M 13 W 23 D 7 N 14 X 24 E 8 O 15 Y 25 F 9 P 16 Z 26 G 10 Q 17 H 11 R 18 I 4 S 19 J 5 T 20
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
472IB-1501277-P
(4) When ",D" or "<(Character string)>"is commanded in a block that is calling a G code macro, a miscellaneous command macro, or an ASCII macro while the macro argument L/P valid function is enabled, a program error (P33) will occur. This parameter setting depends on the MTB specifications. (Parameter "#1241 set13/bit5")
A macro cannot be called with an ASCII code from a macro-called program with an ASCII code. The other patterns are shown below. If it is judged that a macro cannot be called, the command will be handled as a normal command.
Up to 4 nesting levels are available for macro subprogram calls using simple call (G65) and modal call (G66/G66.1). The macro call command's argument is valid only in the called macro level. Since the macro call nest level is four, the argument can be used in the program as a local variable for each macro call.
Counting the main program as 0, up to ten levels of subprograms can be called (M98) from a subprogram. The following commands are used for subprogram nesting.
(1) M98 (2) G65 G66 G66.1 (3) G code call Miscellaneous function call (M/S/T/B) (4) MDI interruption (5) Automatic tool length measurement (6) Multiple-step skip function
The following commands can be issued regardless of nesting.
(7) Fixed cycles (8) Macro interruption
Precautions
Calling a macro with an ASCII code from a macro-called program
Called side
ASCII GMSTB macro G65/66/66.1 M98
Calling side ASCII GMSTB macro G65/66/66.1 M98
Nest level of macro call commands
Nest level of subprogram call command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
473 IB-1501277-P
If "M" is designated for the ASCII code address, it may overlap with the codes basically necessary for that machine. In this case, commands will be identified with the following priority using code values.
(1) M98, M99, M198 (subprogram call command) M00 (program stop command) M01 (optional stop command) M02, M30 (end command) M96, M97 (macro interruption command)
(2) When corresponding to miscellaneous code (M) call macro command (3) When corresponding to ASCII code macro command (4) Used as normal miscellaneous command
If "S", "T" and "B" are designated for the ASCII code address, commands will be identified with the following priority.
(1) When corresponding to miscellaneous code (S, T, B) call macro command (2) When corresponding to ASCII code macro command (3) Used as normal command
If the other addresses do not correspond to the ASCII code macro command, they will be identified as normal com- mands. If the command to be used, overlaps with an ASCII code macro command, it must be commanded in the macro-called program with the ASCII code. Note that there are cases where the command will be unconditionally handled as a normal command, as explained in below.
(1) When there is a data setting command (G10) in the same block. (2) When ASCII code macro call is executed after the G code macro call command in the same block (also applies
for M, S, T, B and ASCII) (Example) When address "D" (G65 type) is set in the ASCII code macro, and M50 is set in the macro call (G65 type).
(3) When inputting parameters (4) When there is a comma (,) before the address. (For example, ",D", ",R", etc.) (5) When commanded in fixed cycle (6) When commanded in macro subprogram called with G code macro call
(Also applies when macro is called with M, S, T, B or ASCII)
Order of command priority
Conditions where the address set is handled as a normal command
M50 D200 ; Execute M code macro with argument (200 set in #7)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
474IB-1501277-P
14.5 Variables Used in User Macros
Both the variable specifications and user macro specifications are required for the variables that are used with the user macros. The compensation amounts of the local, common and system variables among the variables for this NC system ex- cept #33 are retained even when the unit's power is switched off. (Common variables can also be cleared by param- eter "#1129 PwrVCl".)
When the user macro specifications are applied, variable Nos. can be turned into variables (multiple uses of vari- ables) or replaced by
(Example 1) Multiple uses of variables
(Example 2) Example of multiple designations of variables
(Example 3) Replacing variable Nos. with
Function and purpose
Detailed description
Use of multiple variable
#1=10 #10=20 #20=30 ; #5=# [#[#1]] ;
# [# [#1]] = # [#10] from #1 = 10. # [#10] = #20 from #10 = 20. Therefore, #5 = #20 or #5 = 30.
#1=10 #10 =20 #20=30 #5=1000; #[#[#1]]=#5;
# [# [#1]] = # [#10] from #1 = 10. # [#10] = #20 from #10 = 20. Therefore, #20 = #5 or #20 = 1000.
#10=5;
#10=5 ; #[#10 + 1] = 1000 ; In which case, #6 = 1000. #[#10 - 1] = -1000 ; In which case, #4 = -1000. #[#10 * 3] = 100 ; In which case, #15 = 100. #[#10/2] = -100 ; In which case, #2 = -100.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
475 IB-1501277-P
When applying the user macro specifications, variables which have not been used even once after the power was switched on or local variables which were not specified by the G65, G66 or G66.1 commands, can be used as
(1) Arithmetic expressions
Note that
(2) Variable quotations When only the undefined variables are quoted, they are ignored including the address itself. When #1 =
(3) Conditional expressions
(1) EQ and NE should be compared only for integers. For comparison of numeric values with decimals, GE, GT, LE, and LT should be used.
Undefined variables
#1 = #0; #1 =
G00 X#1 Z1000 ; Equivalent to G00 Z1000 ; G00 X#1+10 Z1000 ; Equivalent to G00 X10 Z1000 ;
When #101 =
#101EQ#0
#101EQ#0 0 =
#101NE0
#101NE0 0 0 Not established
#101GE#0
#101GE#0 0 >=
#101GT0
#101GT0 0 > 0 Not established
#101LE#0
#101LE#0 0 <=
#101LT0
#101LT0 0 < 0 Not established
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
476IB-1501277-P
14.5.1 Common Variables
Common variables can be used commonly from any position. Number of the common variables sets depends on the specifications. Refer to the explanation about Variable Commands for details.
Any name (variable name) can be given to common variables #500 to #599. It must be composed of not more than 7 alphanumerics and it must begin with a letter. Do not use "#" in variable names. It causes an alarm when the pro- gram is executed.
Variable names are separated by a comma (,).
(1) Once variable names have been set, they will not be cleared even when the power is turned off. (2) Variables in programs can be quoted by their variable names. In this case, the variables should be enclosed in
square parentheses [ ]. (Example 1) G01X [#POINT1] ;
(3) The variable Nos., data and variable names are displayed on the screen of the setting and display unit. (Example 2) Program... SETVN500 [A234567, DIST, TOOL25] ;
(1) Do not use characters (SIN, COS, etc.) predetermined by the NC and used for operation commands at the head of a variable name.
Detailed description
Variable name setting and quotation
SETVNn [ NAME1,NAME2, .....] ;
n Head No. of variable to be named (500 to 599) NAME1 #n name (variable name) NAME2 #n + 1 name (variable name)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
477 IB-1501277-P
14.5.2 Local Variables (#1 to #33)
Local variables can be defined as an
The
The following table shows correspondences points between the addresses designated by
[Argument designation I]
"" in the above table denotes argument addresses which cannot be used. However, provided that the G66.1 mode has been established, an argument address denoted by the asterisk can be added for use. The hyphen (-) mark indicates that there is no corresponding address. A "" mark denotes an argument address which may be used depending on the MTB specifications. (Parameter "#1241 set13"/bit5)
Detailed description
G65 P__ L__
P Program No. L Number of repetitions
Call command Argument ad- dress
Local vari- able No.
Call command Argument ad- dress
Local vari- able No.G65 G66 G66.1 G65 G66 G66.1
A #1 Q #17 B #2 R #18 C #3 S #19 D #7 T #20 E #8 U #21 F #9 V #22 * G #10 W #23 H #11 X #24 I #4 Y #25 J #5 Z #26 K #6 - #27 * L #12 - #28 M #13 - #29 * N #14 - #30 O #15 - #31 * P #16 - #32
- #33
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
478IB-1501277-P
[Argument designation II]
The numbers 1 to 10 accompanying I, J and K indicate the sequence of the commanded sets, and are not re- quired in the actual command.
(1) Local variables in subprograms can be defined by means of the
Argument designa- tion II address
Variable in macro Argument designa- tion II address
Variable in macro
A #1 J5 #17 B #2 K5 #18 C #3 I6 #19 I1 #4 J6 #20 J1 #5 K6 #21 K1 #6 I7 #22 I2 #7 J7 #23 J2 #8 K7 #24 K2 #9 I8 #25 I3 #10 J8 #26 J3 #11 K8 #27 K3 #12 I9 #28 I4 #13 J9 #29 J4 #14 K9 #30 K4 #15 I10 #31 I5 #16 J10 #32
K10 #33
Note
G65 P9900 A60. S100. F800;
M02; M99;
A(#1)= 60.000
F(#9)= 800
S(#19)= 100.000
G91 G01 X #19*COS #1 Y #19*SIN #1 F#9;
Main program
Subprogram
Local variables set by argument
Local variable data table
Refer to the local variables and control the movement, etc.
Subprogram O9900
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
479 IB-1501277-P
(2) The local variables can be used freely in that subprogram.
In the front surface milling example, argument J is programmed as the milling pitch 10. mm. However, this is changed to 8.333 mm to create an equal interval pitch. The results of the No. of reciprocation data calculation is set in local variable #30.
G65 P1 A100. B50. J10. F500; #30=FUP #2/#5/2 ;
#5=#2/#30/2 ;
M98 H100 L#30 ;
X#1 ;
M99 ;
N100 G1 X#1 F#9 ;
Y#5 ;
X-#1 ;
Y#5 ;
M99 ;
A(#1) 100.000
B(#2) 50.000
F(#9) 500
J(#5) 10.000 8.333
(#30) 3
B
A
J
Local variables set by argument
The local variables can be changed in the subprogram.
Main program
Example of front surface milling
Local variable data table
Subprogram
To subprogram
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
480IB-1501277-P
(3) Local variables can be used independently on each of the macro call levels (4 levels). Local variables are also provided independently for the main program (macro level 0). Arguments cannot be used for the level 0 local variables.
The status of the local variables is displayed on the setting and display unit. Refer to the Instruction Manual for details.
14.5.3 System Variables
Data such as the workpiece offset amount can be read using system variables other than common variables or local variables. Refer to "23 System Variables" for details.
#1 0.100 #2 0.200 #3 0.300
#1=0.1 #2=0.2 #3=0.3;
G65 P1A1. B2. C3.;
M02;
#32
A (#1) 10.000 B (#2) 20.000 C (#3) 30.000 D (#7)
Z (#26)
G65 P100A100. B200.;
M99;
#32
A (#1) 1.000 B (#2) 2.000 C (#3) 3.000 D (#7)
Z (#26)
G65 P10A10. B20. C30.;
M99;
#32
A (#1) 100.000 B (#2) 200.000 C (#3)
Z (#26)
M99;
#32
Main program (Local level 0)
O1 (Local level 1)
O10 (Local level 2)
O100 (Local level 3)
Local variable (0) Local variable (3)Local variable (2)Local variable (1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
481 IB-1501277-P
14.6 User Macro Commands
14.6.1 Operation Commands
A variety of operations can be performed between variables.
Function and purpose
Command format
#i =
(1) Definition and sub- stitution of vari- ables
#i = #j Definition, substitution
(2) Addition operation #i = #j + #k Addition #i = #j - #k Subtraction #i = #j OR #k Logical sum (at every bit of 32 bits) #i = #j XOR #k Exclusive OR (at every bit of 32 bits)
(3) Multiplication oper- ation
#i = #j * #k Multiplication #i = #j / #k Division #i = #j MOD #k Remainder #i = #j AND #k Logical product (at every bit of 32 bits)
(4) Functions #i = SIN [#k] Sine #i = COS [#k] Cosine #i = TAN [#k] Tangent tan uses sin/cos. #i = ASIN [#k] Arcsine #i = ATAN [#k] Arctangent (ATAN or ATN may be used) #i = ACOS [#k] Arccosine #i = SQRT [#k] Square root (SQRT or SQR may be used) #i = ABS [#k] Absolute value #i = BIN [#k] Conversion from BCD to BIN #i = BCD [#k] Conversion from BIN to BCD #i = ROUND[#k] Rounding off (ROUND or RND may be used) #i = FIX [#k] Discarding fractions after decimal point #i = FUP [#k] Add for fractions less than 1 #i = LN [#k] Natural logarithm #i = EXP [#k] Exponent with e (=2.718 .....) as bottom #i = POW [#j, #k] Power [M8]
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
482IB-1501277-P
(1) A value without a decimal point is basically treated as a value with a decimal point at the end (1 = 1.000). (2) Compensation amounts from #10001 and workpiece coordinate system compensation values from #5201 are
handled as data with a decimal point. Consequently, data with a decimal point will be produced even when data without a decimal point have been defined in the variable numbers. (Example)
(3) The
(1) The sequence of the operations (a) to (c) is performed in the following order; the function, the multiplication op- eration and the addition operation.
(2) The part to be given priority in the operation sequence should be enclosed in square parentheses [ ]. Up to 5 pairs of such parentheses, including those for the functions, may be used.
Operation Commands Common variables after execution
#101 = 1000 ; #10001 = #101 ; #102 = #10001 ;
#101 1000.000 #102 1000.000
Detailed description
Sequence of operations
(a) Function (b) Multiplication operation (c) Addition operation
Note
#101=#111+#112*SIN #113
#101=SQRT #111-#112 *SIN #113 +#114 *#115 ; First pair of brackets
Second pair of brackets Third pair of brackets
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
483 IB-1501277-P
Examples of operation commands
(1) Main program and argument designation
G65 P100 A10 B20.; #101 = 100.000 #102 = 200.000;
#1 10.000 #2 20.000 #101 100.000 #102 200.000
(2) Definition and substitution =
#1 = 1000 #2 = 1000.
#1 1000.000 #2 1000.000
#3 = #101 #4 = #102
#3 100.000 #4 200.000
From common vari- ables
#5 = #10001 (#10001 = -10.) #5 -10.000 From tool compensa- tion
(3) Addition and subtraction + -
#11 = #1 + 1000 #12 = #2 - 50. #13 = #101 + #1 #14 = #10001 - 3. (#10001 = -10.) #15 = #10001 + #102
#11 2000.000 #12 950.000 #13 1100.000 #14 -13.000 #15 190.000
(4) Multiplication and division * /
#21 = 100 * 100 #22 = 100. * 100 #23 = 100 * 100. #24 = 100. * 100. #25 = 100 / 100 #26 = 100. / 100 #27 = 100 / 100. #28 = 100. / 100. #29 = #10001 * #101 (#10001 = -10.) #30 = #10001 / #102
#21 10000.000 #22 10000.000 #23 10000.000 #24 10000.000 #25 1.000 #26 1.000 #27 1.000 #28 1.000 #29 -1000.000 #30 -0.050
(5) Remainder MOD
#19 = 48 #20 = 9 #31 = #19 MOD #20
#19/#20 = 48/9 = 5 Remainder 3 #31 = 3
(6) Logical sum OR
#3 = 100 #4 = #3 OR 14
#3 = 01100100 (binary) 14 = 00001110 (binary) #4 = 01101110 = 110
(7) Exclusive OR XOR
#3 = 100 #4 = #3 XOR 14
#3 = 01100100 (binary) 14 = 00001110 (binary) #4 = 01101010 = 106
(8) Logical product AND
#9 = 100 #10 = #9 AND 15
#9 = 01100100 (binary) 15 = 00001111 (binary) #10 = 00000100 = 4
(9) Sine SIN
#501 = SIN [60] #502 = SIN [60.] #503 = 1000 * SIN [60] #504 = 1000 * SIN [60.] #505 = 1000. * SIN [60] #506 = 1000. * SIN [60.]
#501 #502 #503 #504 #505 #506
0.866 0.866 866.025 866.025 866.025 866.025
(10) Cosine COS
#541 = COS [45] #542 = COS [45.] #543 = 1000 * COS [45] #544 = 1000 * COS [45.] #545 = 1000. * COS [45] #546 = 1000. * COS [45.]
#541 #542 #543 #544 #545 #546
0.707 0.707 707.107 707.107 707.107 707.107
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
484IB-1501277-P
(11) Tangent TAN
#551 = TAN [60] #552 = TAN [60.] #553 = 1000 * TAN [60] #554 = 1000 * TAN [60.] #555 = 1000. * TAN [60] #556 = 1000. * TAN [60.]
#551 #552 #553 #554 #555 #556
1.732 1.732 1732.051 1732.051 1732.051 1732.051
(12) Arcsine ASIN
#531 = ASIN[100.500 / 201.] #532 = ASIN[100.500 / 201] #533 = ASIN[0.500] #534 = ASIN[-0.500]
#531 #532 #533 #534
30.000 30.000 30.000 -30.000
#534 will be 330. (13) Arctangent
ATN or ATAN
#561 = ATAN [173205 / 100000] #562 = ATAN [173205 / 100000.] #563 = ATAN [173.205 / 100] #564 = ATAN [173.205 / 100.] #565 = ATAN [1.73205]
#561 #562 #563 #564 #565
60.000 60.000 60.000 60.000 60.000
(14) Arccosine ACOS
#521 = ACOS [100 / 141.421] #522 = ACOS [100. / 141.421]
#521 #522
45.000 45.000
(15) Square root SQR or SQRT
#571 = SQRT [1000] #572 = SQRT [1000.] #573 = SQRT [10. * 10. + 20. * 20]
#571 #572 #573
31.623 31.623 22.360
with the operation inside parentheses as much as possible.
(16) Absolute value ABS
#576 = -1000 #577 = ABS [#576] #3 = 70. #4 = -50. #580 = ABS [#4 - #3]
#576 #577 #580
-1000.000 1000.000 120.000
(17) BIN, BCD #1 = 100 #11 = BIN [#1] #12 = BCD [#1]
#11 #12
64 256
(18) Rounding off RND or ROUND
#21 = ROUND [14 / 3] #22 = ROUND [14. / 3] #23 = ROUND [14 / 3.] #24 = ROUND [14. / 3.] #25 = ROUND [-14 / 3] #26 = ROUND [-14. / 3] #27 = ROUND [-14 / 3.] #28 = ROUND [-14. / 3.]
#21 #22 #23 #24 #25 #26 #27 #28
5 5 5 5 -5 -5 -5 -5
(19) Discarding frac- tions below dec- imal point FIX
#21 = FIX [14 / 3] #22 = FIX [14. / 3] #23 = FIX [14 / 3.] #24 = FIX [14. / 3.] #25 = FIX [-14 / 3] #26 = FIX [-14. / 3] #27 = FIX [-14 / 3.] #28 = FIX [-14. / 3.]
#21 #22 #23 #24 #25 #26 #27 #28
4.000 4.000 4.000 4.000 -4.000 -4.000 -4.000 -4.000
(20) Adding frac- tions less than 1 FUP
#21 = FUP [14 / 3] #22 = FUP [14. / 3] #23 = FUP [14 / 3.] #24 = FUP [14. / 3.] #25 = FUP [-14 / 3] #26 = FUP [-14. / 3] #27 = FUP [-14 / 3.] #28 = FUP [-14. / 3.]
#21 #22 #23 #24 #25 #26 #27 #28
5.000 5.000 5.000 5.000 -5.000 -5.000 -5.000 -5.000
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
485 IB-1501277-P
(1) Notes on logical relation EQ, NE, GT, LT, GE and LE conduct the same calculation as addition and subtraction. Pay careful attention to errors. For example, to determine whether or not #10 and #20 are equal in the following example, it is not always possible to judge correctly because of the error.
IF [#10 EQ #20] Therefore when the difference between #10 and #20 falls within the designated error range, both values should be considered equal.
IF [ABS [#10 - #20] LT 0.01] (2) If an operation command using a function is executed, a program error (P282) will occur when: A number that sets cos to "0" has been designated in the argument of the tangent command (TAN). A negative number has been designated in the argument of the square root command (SQR). A negative number has been designated in the argument of the logarithm natural command (LN). "0" has been set to argument 1 and "0" or less to argument 2 in the power command (POW). [M8] A negative number has been set to argument 1 and a non-integer to argument 2 in the power command
(POW). [M8] (3) A method of processing macro operation (*1) can be changed. (This depends on the MTB specifications (param-
eter "1259 set31/bit7").) When this is set to "0" (high speed), a high-speed macro operation is available because display update data will not be created. (*1) This specifies whether to update the display data every time the certain number of macro blocks are exe-
cuted for processing consecutive macro blocks.
(21) Natural loga- rithms LN
#10 = LN [5] #102 = LN [0.5] #103 = LN [-5]
#101 #102 Error
1.609 -0.693 "P282"
(22) Exponents EXP
#104 = EXP [2] #105 = EXP [1] #106 = EXP [-2]
#104 #105 #106
7.389 2.718 0.135
(23) Power POW [M8]
#107 = POW [2, 3] #108 = POW [2, -3] #109 = POW [2.5, 3.5] #110 = POW [0, -1] #111 = POW [-2, 2.5]
#107 #108 #109 Error Error
8.000 0.125 24.705 "P282" "P282"
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
486IB-1501277-P
14.6.2 Control Commands
The flow of programs can be controlled by "IF-GOTO-", "IF-THEN-ELSE-ENDIF", and "WHILE-DO-". When a program in an external device such as a USB memory device is executed, a period of processing time is required in the subprogram call or in the instruction to change the flow of the program such as GOTO or DO-END; therefore, interpolation may be decelerated or stopped.
When the condition is satisfied, control branches to "n" and when it is not satisfied, the next block is executed. IF [conditional expression] can be omitted and, when it is, control branches to "n" unconditionally. The following types of [conditional expressions] are available.
"n" of "GOTO n" must always be in the same program. If not, program error (P231) will occur. A formula or variable can be used instead of i, #j and n. In the block with sequence number "n" which will be executed after a "GOTO n" command, the sequence number "Nn" must always be at the head of the block. Otherwise, program error (P231) will occur. If "/" is at the head of the block and "Nn" follows, control can be branched to the sequence number.
(1) When searching the sequence number of the branch destination, the search is conducted up to the end of the program (% code) from the block following IF............; and if it is not found, it is then conducted from the top of the program to the block before IF............;. Therefore, branch searches in the opposite direction to the program flow will take longer time compared with branch searches in the forward direction.
(2) EQ and NE should be compared only for integers. For comparison of numeric values with decimals, GE, GT, LE, and LT should be used.
Function and purpose
Detailed description
Branch (IF-GOTO-)
IF [conditional expression] GOTO n; (n = sequence number in the program)
#i EQ #j = When #i and #j are equal #i NE #j When #i and #j are not equal #i GT #j > When #i is greater than #j #i LT #j < When #i is less than #j #i GE #j >= When #i is #j or more #i LE #j <= When #i is #j or less
N100 X#22 ; #1=#1+1 ;
N100
N10 #22=#20 ; IF #2 EQ1 GOTO100 ; #22=#20 -#3 ;
Branching to N100 when content of #2 is 1 Branch
search Branch search
With N10 To head
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
487 IB-1501277-P
(1) When the condition is satisfied, THEN-side processing is executed. Otherwise, ELSE-side processing is exe- cuted.
(2) Designate the conditional expression in the same way as for the "IF-GOTO-" command. (3) If neither the THEN nor ELSE command is designated in the same block as for the IF command (the IF statement
is commanded alone), a program error (P33) will occur. (4) When the run command has an executable statement or multiple commands are designated, enclose them in
the IF, THEN, ELSE, and ENDIF rows as shown in format (a). (5) If the run command is an operation instruction, it can be described following THEN or ELSE as shown in formats
(b) and (c). (6) If the ENDIF command is omitted in format (a), a program error (P289) will occur.
In format (b) or (c), the ENDIF command can be described like format (a). When the IF statement is used as a nesting in format (b) or (c), designate the ENDIF command.
[Operation] The following operation is performed depending on whether the ENDIF command is designated in "C". ENDIF command designated: ELSE processing is executed when the IF condition of A is false. ENDIF command undesignated: ELSE processing is executed when the IF condition of B is false.
(7) The THEN-side processing or ELSE-side processing can be omitted in any of formats (a) to (c).
(8) Formats (a) and (b) can be combined to issue commands.
(9) If any of THEN, ELSE, and ENDIF is commanded with no IF command issued, a program error (P289) will occur.
Branch (IF-THEN-ELSE-ENDIF)
(a) IF [conditional expression] THEN ; Macro statement or executable statement : ELSE ; Macro statement or executable statement : ENDIF ;
(b) IF [conditional expression] THEN operation command ; ELSE operation command ;
(c) IF [conditional expression] THEN operation command ELSE operation command ;
IF[ #100 EQ 0 ] THEN ; A IF[ #110 EQ 1 ] THEN #120 = 10 ; B ENDIF ; C ELSE ; #120 = 20; ENDIF ;
When ELSE-side processing is omitted: IF[ #100 EQ 0 ] THEN ; #100 = 2 ; G00 X#101 ; ENDIF ;
When THEN-side processing is omitted: IF[ #100 EQ 0] ELSE #110 =10 ;
IF[ #100 EQ 0 ] THEN ; #100 = 2 ; G00 X#101 ; ELSE #110 =10 ; ENDIF ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
488IB-1501277-P
(10) The IF statement can be commanded up to 10 nesting levels. When the nesting level exceeds 10, a program error (P288) will occur. The following shows an example in which the nesting level is set to 3.
(11) You can set a branch from the inside of the IF to ENDIF range to the outside.
(12) Do not set a branch to the inside of the IF to ENDIF range, including the ENDIF block. Branching disables the skipped IF command and executes all the commands designated up to the ENDIF command that is paired with the IF command.
(13) If IF to ENDIF is intersected with WHILE-DO to END, a program error (P288, P289, or P294) will occur.
If "A" to "C" are repeated 11 times or more while the IF condition in "B" is true, a program error (P288) will occur in "B". When the IF condition in "B" is false, "C" is not executed, so "A" to "C" are not processed repeatedly.
3 2 1
IF[ #100 EQ 0 ] THEN ; IF[ #110 GT #111 ] THEN ; : ELSE ; IF[ #120 EQ #121 ] THEN ; : ELSE ; : ENDIF ; ENDIF ; ELSE ; : ENDIF ;
IF[ #100 EQ 0 ] THEN ; IF[ #110 GT #111 ] GOTO100 ; : ENDIF ; : N100 ; :
IF[ #110 GT #111 ] GOTO100 ; : IF[ #100 EQ 0 ] THEN ; : N100 ; : ENDIF ;
WHILE[ #110 GT #111 ] DO1;
:
IF[ #100 EQ 0 ] THEN;
:
END1;
:
ENDIF;
A
B
C Not
possible
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
489 IB-1501277-P
(14) You can call a subprogram (M98, G65, G66, etc.) from the inside of the IF to ENDIF range. Also, you can execute the IF, THEN, ELSE, and ENDIF commands in a subprogram. The IF statement can be commanded up to 10 nesting levels even in a subprogram. (The IF statement can be commanded up to 10 nesting levels for each program.)
(15) The IF statement processing (IF to ENDIF) must be ended in the same program. If processing is not ended in the same program, a program error (P289) will occur.
(16) The block skip ("/") for the IF/THEN/ELSE/ENDIF command block is valid only when it is assigned to the head of the block. The block skip ("/") assigned to the middle of the IF/THEN/ELSE/ENDIF command block is handled as shown below regardless of the setting of the optional block skip type (parameter "#1226 aux10/bit1"). When the block skip ("/") is assigned just after the THEN or ELSE command, it is ignored. Otherwise, the block skip ("/") is handled as a division command.
formed as shown below.
While the conditional expression is established, the blocks from the following block to ENDm are repeatedly execut- ed; when it is not established, execution moves to the block following ENDm. DOm may come before WHILE. "WHILE [conditional expression] DOm" and "ENDm" must be used as a pair. If "WHILE [conditional expression]" is omitted, these blocks will be repeatedly ad infinitum. The repeating identification Nos. range from 1 to 127. (DO1, DO2, DO3, .....DO127) Up to 27 nesting levels can be used.
/ IF[ #100 EQ 0 ] THEN #100 =10 ; When "Optional block skip" signal is ON, IF statement will not be executed.
Repetitions
WHILE [conditional expression] DOm ; (m =1, 2, 3 ..... 127) :
:
END m ;
(1) Same identification No. can be used any number of times.
(2) Any number may be used as the WHILE-DOm identification No.
END1;
WHILE DO1;
END1;
WHILE DO1;
END1;
WHILE DO1;
END3;
WHILE DO3;
END2;
WHILE DO2;
END1;
WHILE DO1;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
490IB-1501277-P
(3) Up to 27 nesting levels can be used for WHILE-DOm. "m" is any number from 1 to 127 for the nesting depth.
For nesting, "m" which has been used once cannot be used.
(4) The number of WHILE-DOm nesting levels can- not exceed 27.
(5) WHILE - DOm must be designated first and ENDm last.
(6) WHILE - DOm and ENDm must correspond on a 1:1 (pairing) basis in a same program.
(7) Two WHILE - DOm's must not overlap. (8) Branching externally out of the WHILE - DOm range, is possible.
(9) No branching into WHILE - DOm, is possible. (10) Subprograms can be called by M98, G65 or G66 between WHILE - DOm's.
END1;
WHILE DO1;
END2;
WHILE DO2;
END27;
WHILE DO27;
DO1
DO2
DO27
END28;
END3;
END2;
END1;
WHILE DO1;
WHILE DO2;
WHILE DO3;
WHILE DO28;
Not possible
WHILE DO1;
END 1;
Not possible
WHILE DO1;
END1;
WHILE DO1;
Not possible
END2;
END1;
WHILE DO2;
WHILE DO1;
Not possible
WHILE DO1;
END1;
IF GOTOn;
Nn;
IF GOTOn;
WHILE DO1;
END1;
WHILE DO1;
Nn; Nn;
END1;END1;
IF GOTOn;
WHILE DO1; Not possible
Not possible
G65 P100;
END1;
WHILE DO1; WHILE DO02;
END2;
M99;M02;
(MP) (SP)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
491 IB-1501277-P
Even if a fixed cycle containing WHILE is called, the nesting level will be counted up.
(11) Calls can be initiated by G65 or G66 between WHILE - DOm's and commands can be issued again from 1. Up to 27 nesting levels are possible for the main program and subprograms.
(12) A program error will occur in M99 if WHILE and END are not paired in the subprogram (including macro subprogram).
(MP) Main program (SP) Subprogram
G65 P100;
END1;
WHILE DO1; WHILE DO1;
END1;
M99;M02;
(MP) (SP)(100)
DO1; WHILE
(SP)(MP)
M99;
M98 P100;
M02; DOn ENDn illegal usage.
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
492IB-1501277-P
14.6.3 External Output Commands; POPEN, PCLOS, DPRNT
Besides the standard user macro commands, the following macro instructions are also available as external output commands. They are designed to output the variable values or characters to external devices. The data output port can be chosen from RS-232C or memory card.
Command sequence
Function and purpose
Command format
Open command
POPEN
Closed command
PCLOS
Data output command
DPRNT
POPEN For preparing the data outputs
PCLOS For terminating the data outputs
DPRNT For character output and digit-by-digit variable numerical output
...Open command
... Data output command
... Closed command
POPEN
PCLOS
DPRNT
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
493 IB-1501277-P
(1) The command is issued before the series of data output commands. (2) The DC2 control code and % code are output from the NC system to the external output device. (3) Once POPEN; is issued, it will remain valid until PCLOS; is issued.
(1) This command is issued when all the data outputs are completed. (2) The DC4 control code and % code are output from the NC system to the external output device. (3) This command is used together with the open command and it should not be issued unless the open mode has
been established. (4) Issue the close command at the end of the program even when the operation is suspended by resetting or some
other operation during data output.
(1) The character output and decimal output of the variable values are done with ISO codes. (2) The commanded character string is output as it is by the ISO code.
Alphanumerics (A to Z, 0 to 9) and special characters (+, -, *, /) can be used. Note that asterisk (*) is output as a space code.
(3) The required significant digits above and below the decimal point of the variable values are each commanded within square parentheses. As a result, the commanded number of digits of variable values are output in ISO code in decimal notation from the high-order digits including the decimal point. In this case, trailing zeroes are not omitted.
(4) Leading zeroes are omitted. The omitted leading zero can be replaced by a space by the setting of a parameter. This can justify the last digit of the data output to the printer.
(5) Linefeed (LF) code will be output to the end of the output data. And by setting the parameter "#9112 to #9512 DEV0 - 4 CR OUTPUT" to "1", (CR) code will be written in just before EOB (LF) code.
A data output command can be issued even in two-part system mode. In this case, however, note that the out- put channel is shared by both part systems. So, be careful not to execute data output by both part systems simultaneously.
(1) The output port can be selected by the parameter "#9007 MACRO PRINT PORT". (2) When the port is a memory card, the file name of the port can be designated by the parameter "#9054 MACRO
PRINT FILE". (3) When the port is a memory card, the port directory is fixed to root directory.
Detailed description
Open command : POPEN
Close command : PCLOS
Data output command : DPRNT
DPRNT [l1#v1 [d1 c1] l2#v2 [d2 c2] ...... ] ;
l1 Character string v1 Variable No. d1 Significant digits above decimal point c + d <= 8 c1 Significant digits after decimal point
Data output port
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
494IB-1501277-P
(*1) Designate a blank line when opening an output file on an edit screen. If not, it will be regarded that no information is provided in the head line of the file on the NC edit screen.
Use example:
#1127 DPRINT (DPRINT alignment) = 1 (Align the minimum digit and output) #9007 MACRO PRINT PORT = 9 (Output to a memory card by an external output command) #9008 MACRO PRINT DEV. = 0 (Device 0 is selected for an external output command) #9054 MACRO PRINT FILE = DPRNT_OUT (File name to store output data of an external output
command) #9112 DEV0 CR OUTPUT = 1 (Insert the CR code just before the LF code)
#1=12.34; #2=#0 #100=-123456789.; #500=-0.123456789; POPEN; DPRNT[]; (*1) DPRNT[VAL-CHECK]; DPRNT[1234567890]; DPRNT[#1[44]]; DPRNT[#2[44]]; DPRNT[#100[80]]; DPRNT[#500[80]]; DPRNT[#100[08]]; DPRNT[#500[08]]; PCLOS; M30; %
Blank Linefeed code
Values above the number of significant figures are rounded down
Values below the number of significant figures are round- ed off
(CR) (LF)
V A L - C H E C K (CR) (LF)
1 2 3 4 5 6 7 8 9 0 (CR) (LF)
1 2 . 3 4 0 0 (CR) (LF)
0 . 0 0 0 0 (CR) (LF)
- 2 3 4 5 6 7 8 9 (CR) (LF)
- 0 (CR) (LF)
- . 0 0 0 0 0 0 0 0 (CR) (LF)
- . 1 2 3 4 5 6 7 9 (CR) (LF)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
495 IB-1501277-P
(1) An external output command during restart-searching is ignored. After using the restart-search type 2 to restart-search between a POPEN command and a PCLOS command, execute a POPEN command by such as an MDI interruption before restarting the program.
(2) An external output command during graphic check is ignored. (3) A program error (P460) will occur if an external output command is issued when the output device is unable to
output due to a lack of connection, a low free space etc. (4) The NC automatically conducts a closing processing when it is reset between a POPEN command and a PCLOS
command. So, execute a POPEN command by such as an MDI interruption before executing the rest of the ma- chining program.
(5) If a program error occurs between a POPEN command and a PCLOS command, NC will not automatically con- duct a closing processing. So, there is no need to execute a POPEN command by such as an MDI interruption before executing the rest of the machining program.
(6) If a program error occurs to the output port due to the setting of the memory card, execute an NC reset and close the output file before demounting the card.
(7) When the output port is a memory card, the output file may be destroyed if the card is dismounted or the power is turned off without issuing a PCLOS command or NC reset after a POPEN command is issued.
(8) As for M800 series, output data of an external output command can be output to a memory card only when the drive name of the card is "E:" or "F:". Drive name "E" is given the priority. A program error (P460) will occur if the output port executes the external output command of the memory card when the drive name is neither "E:" nor "F:".
(9) When the data is output to a memory card, the maximum number of files that can be created is determined by the FAT16 format.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
496IB-1501277-P
14.6.4 Precautions
When the user macro commands are employed, it is possible to combine conventional control commands such as movement commands and the M, S, T commands with macro commands such as the arithmetic, decision, branching for creating the machining programs. When the former commands are made into executable statements and the latter commands into macro statements, since macro statement processing is not directly related to machine control, it is an effective means for reducing machining time. By setting the parameter "#8101 MACRO SINGLE", the macro statements can be processed concurrently with the execution of the executable statement. (During normal machining, set the parameter OFF to process macro statements in a batch, and during a program check, set the parameter ON to execute the macro statements block by block. Setting can be chosen depending on the purpose.)
By setting the parameter "#1701 cfg01/bit4" to "1", macro statements are processed in a batch to perform a contin- uous operation regardless of the setting of the parameter "#8101 MACRO SINGLE". (Only for C80 series)
The operation of the macro statement is as shown in the table below.
There is a signal to notify this macro single setting status to the sequence program. This signal is turned ON when the control parameter "#8101 MACRO SINGLE" is set to "1" (Stop every block during signal block operation). (Only for C80 series) The operation of the PLC signal depends on the MTB specifications.
Program example
Macro statements here refer to the following commands.
(a) Arithmetic commands (block including "=") (b) Control commands (block including GOTO, DO-END, etc.) (c) Macro call commands (Includes macro calls and cancel commands based on G codes (G65, G66, G66.1, G67).)
Execution statements refer to statements other than macro statements.
Precautions
#8101 Operation method #1701 cfg01/bit4 Operation
0 Continuous operation 0 Processes macro statements in batch 0 Continuous operation 1 Processes macro statements in batch 0 Single operation 0 Processes macro statements in batch 0 Single operation 1 Processes macro statements in batch 1 Continuous operation 0 Processes macro statements block by
block 1 Continuous operation 1 Processes macro statements in batch 1 Single operation 0 Processes macro statements block by
block 1 Single operation 1 Processes macro statements block by
block
N1 G91 G28 X0 Y0 ; ......(1) N2 G92 X0 Y0 ; ......(2) N3 G00 X-100. Y-100. ; ......(3) N4 #101 = 100. * COS[210.] ; ......(4) (4), (5) Macro statements N5 #103 = 100. * SIN[210.] ; ......(5) N6 G01 X#101 Y#103 F800 ; ......(6)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
497 IB-1501277-P
Flow of processing by the program example in the previous page
N4, N5 and N6 are processed in parallel with the control of the executable statement of N3. If the analysis of N4, N5, and N6 is in time during N3 control, the machine movement is continuously controlled.
N4 is processed in parallel with the control of the executable statement of N3. After N3 is finished, N5 and N6 are analyzed, and then N6 is executed. Therefore, the machine control is held on standby during the N5 and N6 analysis time.
Program analysis
Executing block
Program analysis
Executing block
(1) (2) (4)(5)(6)(3)
(1) (2) (4)(5)(6)(3)
(1) (2) (3)
(1) (2) (3)
(4) (5) (6)
(4) (5) (6)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
498IB-1501277-P
14.6.5 Actual Examples of Using User Macros
The following three examples will be described.
(Example 1) SIN curve
(Example 2) Bolt hole circle
(Example 3) Grid
(Example 1) SIN curve
Program example
G65 Pp1 Aa1 Bb1 Cc1 Ff1; a1; Initial value 0 b1; Final value 360 c1; R of R*SIN f1; Feedrate
(SIN ) Y
X
100.
- 100.
0 90. 270. 360.180.
G65 P9910 A0 B360.C100.F100;
#1=0 #2=360.000 #3=100.000 #9=100.000
WHILE #1LE#2 DO1; #101=#3*SIN #1 ; G90 G01 X#1 Y#10 F#9; #1=#1+10.; END1; M99;
Main Program
Local variables set by argument
O9910(Subprogram)
To subprogram
(Note 1)Commanding with one block is possbiel when 90G01X#1Y[#3*SIN[#1]] F#9; is issued.
(Note 1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
499 IB-1501277-P
(Example 2) Bolt hole circle
After defining the hole data with fixed cycle (G72 to G89), the macro command is issued as the hole position com- mand.
G81 Z-100.R50.F300L0 G65 P9920 Aa1 Bb1 Rr1 Xx1 Yy1;
#101=0; #102=#4003; #103=#5001; #104=#5002; #111=#1;
WHILE #101LT#2 DO1;
#120=#24+#18*COS #111 ; #121=#25+#18*SIN #111 ;
#122=#120 #123=#121; IF #102EQ90 GOTO100;
#122=#120-#103; #123=#121-#104;
#103=#120; #104=#121;
N100 X#122 Y#123; #101=#101+1; #111=#1+360.*#101/#2;
END1; M99;
-X x1
W
y1
-Y
a1
Radius*COS[#111] +Center coordinates X #120 Radius*SIN [#111] +Center coordinates Y #121 #120 #122 #121 #123
O9920
#102=90
N100 X#122 Y#123
Y
Y
N
N
END
#120-#103 #122 #121-#104 #123 #120 #103 #121 #104
Main program
O9920(Subprogram)
(Note 1)
(Note 1)
(Note 1)
(Note 1)
(Note 1)
a1;Start angle b1;No. of holes r1;Radius x1;X axis center position y1;Y axis center position
#101=No. of hole count
#102=G90 or G91
#103=X axis current position #104=Y axis current position #111=Start angle
#120=Hole position X coordinates #121=Hole position Y coordinates #122=X axis absolute position #123=Y axis absolute position
Judgment of G90, G91 mode #122=X axis incremental position #123=Y axis incremental position X axis current position update Y axis current position update
#101 No. of holes
Drilling command
No.of holes counter up
#111=Hole position angle
#101+1 #101 360 *#101/No. of holes +#1 #111
(Note 1) The processing time can be shortened by programming in one block.
To subprogram
0 #101 G90,G91 mode Read in #102 Read previous coordinates X #103 Y #104 Start angle #111
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
500IB-1501277-P
(Example 3) Grid
After defining the hole data with the fixed cycle (G72 to G89), macro call is commanded as a hole position command.
G28 X0 Y0 Z0;
T1 M06;
G90 G43 Z100.H01;
G54 G00 X0 Y0;
G81 Z-100.R3.F100 L0 M03;
G65 P9920 X-500.Y-500.A0 B8 R100.;
G65 P9920 X-500.Y-500.A0 B8 R200.;
G65 P9920 X-500.Y-500.A0 B8 R300.;
-X
200R 300R
100R
-500.
-500. W
-Y
To subprogram
To subprogram
To subprogram
G81 Zz1 Rr1 Ff1; G65 Pp1 Xx1 Yy1 Ii1 Jj1 Aa1 Bb1;
-X
i1
x1
W
j1 y1
-Y
x1; X axis hole position y1; Y axis hole position i1; X axis interval j1; Y axis interval a1; No. of holes in X direction b1; No. of holes in Y direction
Subprogram is on next page
G28 X0 Y0 Z0; T1 M06; G90 G43 Z100.H01; G54 G00 X0 Y0; G81 Z-100.R3.F100 L0 M03; G65 P9930 X0 Y0 I-100. J-75. A5B3;
G84 Z-90. R3. F250 M03; G65 P9930 X0 I-100. J-75. A5B3;
-X
-X
100.100.
-75.
-75.
100.
-100.
W
-Y
-Z
To subprogram
To subprogram
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
501 IB-1501277-P
END
#106>0
#105>0
X#101 Y#102
#101+#103 #101
#105-1 #105
#101-#103 #101 #102+#104 #102
-#103 #103
#106-1 #106
N
Y
#101=#24; #102=#25;
#103=#4; #104=#5;
#106=#2;
WHILE #106GT0 DO1;
#105=#1;
WHILE #105GT0 DO2;
G90 X#101 Y#102;
#101=#101+#103; #105=#105-1;
END2;
#101=#101-#103; #102=#102+#104;
#103=-#103; #106=#106-1;
END1;
M99;
O9930
#101 #102 #103 #104 #106
:x 1 :y 1 :i 1 :j 1 :b 1
#105No. of holes in X direction: a 1
O9930(Subprogram)
(Note 1)
(Note 1)
(Note 1)
#101=X axis start point #102=Y axis start point #103=X direction interval #104=Y direction interval #106=No. of holes in Y direction
Y direction drilling completion check
No. of holes in X direction set
No. of holes in Y direction check
Positioning, drilling
X coordinates update
No. of holes in X direction 1
X axis drilling direction reversal
No. of holes in Y direction 1
X coordinates revision Y coordinates update
(Note 1) The processing time can be shortened by programming in one block.
Start point X coordinates
Start point Y coordinates
X axis interval
Y axis interval
No. of holes in Y direction
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
502IB-1501277-P
14.7 Macro Interruption; M96, M97
A user macro interrupt signal (UIT) is input from the machine to interrupt the program currently being executed, and instead calls and executes another program. This is called the user macro interrupt function. Use of this function allows the program to operate flexibly enough to meet varying conditions.
Function and purpose
Command format
User macro interruption enable
M96 P__ H__ ;
M96
P Interrupt program No. Use a parameter to read out a 4- or 8-digit interrupt program No. starting with O.
H Interrupt sequence No.
User macro interruption disable
M97 ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
503 IB-1501277-P
(1) The user macro interrupt function is enabled and disabled by the M96 and M97 commands programmed to make the user macro interrupt signal (UIT) valid or invalid. That is, if an interrupt signal (UIT) is input from the machine side in a user macro interruption enable period from when M96 is issued to when M97 is issued or the NC is reset, a user macro interruption is caused to execute the program specified by P__ instead of the one being ex- ecuted currently.
(2) Another interrupt signal (UIT) is ignored until M96 is commanded while one user macro interrupt is in service. It is also ignored in a user macro interrupt disable state such as after an M97 command is issued or the system is reset.
(3) M96 and M97 are processed internally as user macro interrupt control M codes. (4) If calling a subprogram numbered with O is enabled, a program number starting with O and specified by P com-
mand value is called with a priority. However, when P command value is less than the digit number set with parameter "#8129 subprogram number selection", increase the digit number of command value by adding leading zeros. (Example) When parameter "#8129 subprogram number selection"="1", call the subprogram "O0012" with "M96 P12" command.
(5) In the following cases, a subprogram of P command value without O No. is called even with a setting to call a subprogram with O No. The digit number of P command value is over the digit number of the program number set with parameter
"#8129 subprogram number selection". An interrupt program starting with commanded O No. does not exist.
A user macro interruption is enabled only during execution of a program. The enabling conditions are as follows:
(1) An automatic operation mode or MDI has been selected. (2) The system is running in automatic mode. (3) No user macro interruption is being processed.
(1) A macro interruption is disabled in manual operation mode (JOG, STEP, HANDLE, etc.)
Detailed description
Enabling conditions
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
504IB-1501277-P
(1) When a user macro interrupt signal (UIT) is input after an M96Pp1 ; command is issued by the current program, interrupt program Op1 is executed. When an M99; command is issued by the interrupt program, control returns to the main program.
(2) If M99 Pp2; is specified, the blocks from the one next to the interrupted block to the last one are searched. If none is found, blocks between the first block of the program and the one before the interrupted block are searched. Control then returns to the block with sequence number Np2 that is found first in the above search.
Outline of operation
M99(Pp2) ;
M96 Pp1;
Np2 ;
Np2 ;
M97 ;
M30 ;
Op1 ;
User macro interrupt signal (UIT)
"User macro interruption" signal is acceptable.
"User macro interruption" signal is not acceptable.
Interrupt signal (UIT) not acceptable within a user macro program
(If Pp2 is specified)
Interrupt program
Current program
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
505 IB-1501277-P
Interrupt types 1 and 2 can be selected by the parameter "#1113 INT_2".
[Type 1]
(1) When an interrupt signal (UIT) is input, the system immediately stops moving the tool and interrupts dwell, then permits the interrupt program to run.
(2) If the interrupt program contains a move or miscellaneous function (MSTB) command, the commands in the in- terrupted block are lost. After the interrupt program completes, the main program resumes operation from the block next to the interrupted one.
(3) If the interrupted program contains no move and miscellaneous (MSTB) commands, it resumes operation, after completion of the interrupt program, from the point in the block where the interrupt was caused.
If an interrupt signal (UIT) is input during execution of a miscellaneous function (MSTB) command, the NC system waits for a completion signal (FIN). The system thus executes a move or miscellaneous function command (MSTB) in the interrupt program only after input of FIN.
[Type 2]
(1) When an interrupt signal (UIT) is input, the interrupt program is executed after the commands in the block exe- cuted at that time have been completed. Even if the interrupt program contains a move or miscellaneous function (MSTB) command, the same processing is performed.
(2) If the interrupt program contains no move and miscellaneous function (MSTB) commands, the interrupt program is executed without interrupting execution of the current block.
However, if the interrupt program has not ended even after the execution of the original block is completed, the sys- tem may stop machining temporarily.
Interrupt type
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
506IB-1501277-P
block 1
block 1
block 1
block 3
block 3
block 3
block 2
block 1 block 3block 2
block 1 block 3block 2
block 1 block 3block 2
block 2
block 2 block 2
User macro interruption signal
If the interrupt program contains a move or miscellaneous function command, the reset of block (2) is lost.
User macro interruption signal
User macro interruption signal
User macro interruption signal
Interrupt program
Interrupt program
Interrupt program
Main program [Type 1]
[Type 2] Main program
Executing
Interrupt program
If the interrupted program contains no move and miscellaneous commands, it resumes operation from where it left in block (2), that is, all the reset commands.
If the interrupted program contains no move and miscellaneous commands, the interrupted program is kept executed in parallel to execution of the current program.
The move or miscellaneous command in the interrupt program is executed after completion of the current block.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
507 IB-1501277-P
User macro interruption is classified into the following two types depending on the way an interrupt program is called. These two types of interrupt are selected by parameter "#8155 Sub-pro interrupt". This setting also involves the MTB settings (parameter "#1229 set01/bit0"). Both types of interrupt are added to the calculation of the nest level. The subprograms and user macros called in the interrupt program are also added to the calculation of the nest level.
A user macro interruption signal (UIT) is accepted in the following two methods. These two methods are selected by a parameter "#1112 S_TRG".
M99 (P__) ;
An M99 command is issued in the interrupt program to return to the main program. Address P is used to specify the sequence number of the return destination in the main program. The blocks from the one next to the interrupted block to the last one in the main program are first searched for the block with designated sequence No. If it is not found, all the blocks before the interrupted one are then searched. Control thus returns to the block with sequence No. that is found first in the above search. (This is equivalent to M99P__ used after M98 calling.)
Calling method
Subprogram type in- terrupt
The user macro interruption program is called as a subprogram. As with calling by M98, the local variable level remains unchanged before and after an interrupt.
Macro type interrup- tion
The user macro interpretation program is called as a user macro. As with calling by G65, the local variable level changes before and after an interrupt. No arguments in the main program can be passed to the interrupt program.
Acceptance of user macro interruption signal (UIT)
Status trigger method The user macro interruption signal (UIT) is accepted as valid when it is ON. If the interrupt signal (UIT) is ON when the user macro interrupt function is enabled by M96, the interrupt program is activated. By keeping the interrupt signal (UIT) ON, the interrupt program can be executed re- peatedly.
Edge trigger method The user macro interrupt signal (UIT) is accepted as valid at its rising edge, that is, at the instance it turns ON. This mode is useful to execute an interrupt program once.
Returning from user macro interruption
ON
OFF
User macro interruption signal (UIT)
User macro interruption signal (UIT)
User macro interruption
(Status trigger method)
(Edge trigger method)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
508IB-1501277-P
If modal information is changed by the interrupt program, it is handled as follows after control returns from the inter- rupt program to the main program.
Modal information affected by user macro interruption
Returning with M99; The change of modal information by the interrupt program is invalidated and the original modal information is restored. With interrupt type 1, however, if the interrupt program contains a move com- mand, miscellaneous function (MSTB) command, or specific command (*1), the original modal information is not restored.
Returning with M99P__ ; The original modal information is updated by the change in the interrupt pro- gram even after returning to the main program. This is the same as in returning with M99P__; from a program called by M98, etc.
Op1 ;
Np2 ;
M99(p2) ;
M96Pp1 ;
User macro interruption signal (UIT)
Modal before interrupt is restored.
Main program being executed
Modal modified by interrupt program remains effective.
Interrupt program
(Modal change)
(With Pp2 specified)
Modal information affected by user macro interruption
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
509 IB-1501277-P
(*1) When interrupt type 1 is applied, modal information is not restored for the commands shown below after control has been returned from the interrupt program.
The lathe-system commands are shown based on the G code system 3. Hyphen "-" indicates that no specification is provided.
Command Function
Machining center system
Lathe system
G04 G04 Dwell G11 G11 Data input by program cancel
Tool life management data registration cancel G27 G27 Reference position check G92 G92 Spindle clamp speed setting G92.1 G92.1 Workpiece coordinate system preset - G110 Mixed control (cross axis control) I - G111 Axis name switch - G113 Spindle synchronization I cancel
Tool spindle synchronization IA (spindle - spindle synchro- nization) cancel Tool spindle synchronization II (hobbing) cancel
- G114.1 Spindle synchronization I - G114.2 Tool spindle synchronization IA (Spindle - spindle synchro-
nization) - G114.3 Tool spindle synchronization II (Hobbing) G115 G115 Start point designation timing synchronization Type 1 G116 G116 Start point designation timing synchronization Type 2 G120.1 G120.1 Machining condition selection I G121 G121 Machining condition selection I cancel - G125 Control axis synchronization between part systems - G126 Control axis superimposition G127 G127 All part system reverse run prohibit command ! ! Timing synchronization (! code)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
510IB-1501277-P
Modal information when control passes to the user macro interruption program can be known by reading system variables #4401 to #4520. The unit specified with a command applies.
The above system variables are available only in the user macro interrupt program. If they are used in other programs, program error (P241) will occur.
(*1) Programs are registered as files. When the program No. (file name) is read with #4515, the character string will be converted to a value. (Example 1) The file name "123" is the character string 031, 032, 033, so the value will be (031-030)*100 + (032-030)*10 + (033-030) = 123.0. Note that if the file name contains characters other than numbers, it will be "blank". (Example 2) If the file name is "123ABC", it contains characters other than numbers, so the result will be "blank".
The user macro interruption is controlled by M96 and M97. However, these commands may have been used for other operations. To be prepared for such cases, these command functions can be assigned to other M codes. (This invalidates program compatibility.)
User macro interrupt control with substitute M codes is possible by setting the substitute M code in parameters "#1110 M96_M" and "#1111 M97_M" and by validating the setting by selecting parameter "#1109 subs_M".
If the parameter "#1109 subs_M" used to enable the substitute M codes is not selected, the M96 and M97 codes remain effective for user macro interrupt control. In either case, the M codes for user macro interrupt control are processed internally and not output to the outside.
Modal information variables (#4401 to #4520)
System vari- able
Modal information
#4401 :
#4421
G code (group 01) : G code (group21)
Some groups are not used.
#4507 D code #4509 F code #4511 H code #4513 M code #4514 Sequence No. #4515 Program No. (*1) #4519 S code #4520 T code
M code for control of user macro interruption
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
511 IB-1501277-P
(1) Subprogram call validity "#8155 Sub-pro interrupt" ("#1229 set01/bit0" (*1)) 1: Subprogram type user macro interruption 0: Macro type user macro interruption
(2) Status trigger mode validity "#1112 S_TRG" (*1) 1: Status trigger mode 0: Edge trigger mode
(3) Interrupt type 2 validity "#1113 INT_2" (*1) 1: The executable statements in the interrupt program are executed after completion of execution of the current block. (Type 2) 0: The executable statements in the interrupt program are executed before completion of execution of the current block. (Type 1)
(4) Validity of substitute M code for user macro interruption control "#1109 subs_M" (*1) 1: Valid 0: Invalid
(5) Substitute M codes for user macro interruption control (*1) Interrupt enable M code (equivalent to M96) "#1110 M96_M" Interrupt disable M code (equivalent to M97) "#1111 M97_M" Specify "03" to "97", excluding "30".
(6) Subprogram number selection "#8129 Subpro No. select" Select a subprogram number to be called preferentially under subprogram control. 0: Commanded program number 1: 4-digits program number beginning with O No. 2: 8-digits program number beginning with O No.
(*1) These parameter settings depend on the MTB specifications.
The program called by the user macro, figure rotation, macro interruption, or compound type fixed cycle also conforms to this setting.
(1) If the user macro interruption program uses system variables #5001 and after (position information) to read co- ordinates, the coordinates pre-read in the buffer are used.
(2) If an interrupt is caused during execution of the tool nose R compensation or tool radius compensation, a se- quence No. (M99P__;) must be specified with a command to return from the user macro interrupt program. If no sequence No. is specified, control cannot return to the main program normally.
(3) With interrupt type 1, when the interrupt program contains a move or MSTB command, do not command the macro interruption to the waiting part system among multiple part systems. Doing so stops machining while the part system that does not perform an interruption remains set in the waiting standby state. If an interruption is carried out, machining can be started by the "ignore the timing synchronization between part systems" signal; however, the operation of this signal depends on the MTB specifications.
Parameters
Precautions
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)
14 Macro Functions
512IB-1501277-P
15
513 IB-1501278-P
Program Support Functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
514IB-1501278-P
15Program Support Functions 15.1 Corner Chamfering I/Corner Rounding I
Chamfering at any angle or corner rounding is performed automatically by adding ",C_" or ",R_" to the end of the block to be commanded first among those command blocks which shape the corner with lines only.
15.1.1 Corner Chamfering I ; G01 X_ Y_ ,C
This chamfers a corner by connecting the both side of the hypothetical corner which would appear as if chamfering is not performed, by the amount commanded by ",C_".
Corner chamfering is performed at the point where N100 and N200 intersect.
(1) The start point of the block following the corner chamfering is the hypothetical corner intersection point.
(2) If there are multiple or duplicate corner chamfering commands in a same block, the last command will be valid.
(3) When both the corner chamfer and corner rounding commands exist in the same block, the latter command is valid.
(4) Tool compensation is calculated for the shape which has already been subjected to corner chamfering.
(5) When the block following a command with corner chamfering does not contain a linear command, a corner cham- fering/corner rounding II command will be executed.
(6) Program error (P383) will occur when the movement amount in the corner chamfering block is less than the chamfering amount.
(7) Program error (P384) will occur when the movement amount in the block following the corner chamfering block is less than the chamfering amount.
(8) Program error (P382) will occur when a movement command is not issued in the block following the corner cham- fering I command.
Function and purpose
Function and purpose
Command format
N100 G01 X__ Y__ ,C__ ;
N200 G01 X__ Y__ ;
,C Length up to chamfering starting point or end point from hypothetical corner
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
515 IB-1501278-P
Program example
(1) G91 G01 X100. ,C10.; (2) X100. Y100.;
(a) Chamfering start point (b) Hypothetical corner intersection point (c) Chamfering end point
X100.0 X100.0
10.0
10.0
X
Y
Y100.0
(1)
(2)
(a) (b)
(c)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
516IB-1501278-P
15.1.2 Corner Rounding I ; G01 X_ Y_ ,R_
The hypothetical corner, which would exist if the corner were not to be rounded, is rounded with an arc that has a radius commanded by ",R_" only when configured of linear lines.
Corner rounding is performed at the point where N100 and N200 intersect.
(1) The start point of the block following the corner rounding is the hypothetical corner intersection point.
(2) When both corner chamfering and corner rounding are commanded in the same block, the latter command will be valid.
(3) Tool compensation is calculated for the shape which has already been subjected to corner rounding.
(4) When the block following a command with corner rounding does not contain a linear command, a corner cham- fering/corner rounding II command will be executed.
(5) Program error (P383) will occur when the movement amount in the corner rounding block is less than the R value.
(6) Program error (P384) will occur when the movement amount in the block following the corner rounding block is less than the R value.
(7) Program error (P382) will occur if a movement command is not issued in the block following the corner rounding.
Function and purpose
Command format
N100 G01 X__ Y__ ,R__ ;
N200 G01 X__ Y__ ;
,R Arc radius of corner rounding
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
517 IB-1501278-P
Program example
(1) G91 G01 X100. ,R10.; (2) X100. Y100.;
(a) Corner rounding start point (b) Corner rounding end point (c) Hypothetical corner intersection point
X100.0 X100.0
X
Y
Y100.0
(1)
(2)
R10.0(a)
(b)
(c)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
518IB-1501278-P
15.1.3 Corner Chamfering Expansion/Corner Rounding Expansion
Using an E command, the feedrate can be designated for the corner chamfering and corner rounding section. In this way, the corner section can be cut into a correct shape.
Example
Function and purpose
F200.
E100.
F200.
F200.
Y F200.
(G94) G01Y70.,C30. F200.E100.; X-110.;
(G94) G01Y70.,R30. F200.E100.; X-110.;
X
E100.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
519 IB-1501278-P
(1) The E command is modal. It is also valid for the feed in the next corner chamfering/corner rounding section.
Example
(2) E command modal has separate asynchronous feedrate modal and synchronous feedrate modal functions. Which one is validated depends on the asynchronous/synchronous mode (G94/G95).
(3) When the E command is 0, or when there has not been an E command up to now, the corner chamfering/corner rounding section feedrate will be the same as the F command feedrate.
Example
(4) E command modal is not cleared even if the reset button is pressed. It is cleared when the power is turned OFF. (In the same manner as F commands.)
(5) All E commands except those shown below are at the corner chamfering/corner rounding section feedrate. - E commands during thread cutting modal - E commands during thread cutting cycle modal
Detailed description
(G94) G01Y30.,C10. F100.E50.; X-50.,C10.; Y50.,C10.; X-50.;
F100.
F100.
F100.
E50.
E50.
E50.
F100.
Y
X
F100. F100.
F100.
F100.
F100.
F100.
F100.
F100. F100. F100.
F100.
E50.
E50. E50.
Y
X
(G94) G01Y30.,C10. F100.E50.; X-50.,C10.; Y50.,C10. E0; X-50.;
(G94) G01Y30.,C10. F100.; X-50.,C10.; Y50.,C10. E50; X-50.;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
520IB-1501278-P
15.1.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding
(1) Shown below are the operations of manual interruption during corner chamfering or corner rounding.
(2) With a single block during corner chamfering or corner rounding, the tool stops after these operations are exe- cuted.
Detailed description
With an absolute command and manual absolute switch ON.
N1 G28 XY; N2 G00 X120.Y20. ; N3 G03 X70. Y70.I-50. ,R20. F100 ; N4 G01 X20. Y20. ;
With an incremental command and manual absolute switch OFF
N1 G28 XY; N2 G00 X120. Y20. ; N3 G03 X-50. Y50. I-50. ,R20. F100 ; N4 G01 X-50. Y-50.;
Interrupt amount
Path in interrupt case
Path in non-interrupt case
X
140.
40.
20. 70.
N4 N3
120.
Y
(mm)
X
140.
40.
20. 70.
N4 N3
120.
Y
(mm)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
521 IB-1501278-P
15.2 Corner Chamfering II/Corner Rounding II
Corner chamfering and corner rounding can be performed by adding ",C" or ",R" to the end of the block which is commanded first among the block that forms a corner with continuous arbitrary angle lines or arcs.
15.2.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_
The corner is chamfered by commanding ",C" in the 1st block of the two continuous blocks containing an arc. For an arc, this will be the chord length.
Corner chamfering is performed at the point where N100 and N200 intersect.
(1) If this function is commanded while the corner chamfer or corner rounding command is not defined in the spec- ifications, it causes a program error (P381).
(2) The start point of the block following the corner chamfering is the hypothetical corner intersection point. (3) If there are multiple or duplicate corner chamfering commands in a same block, the last command will be valid. (4) When both corner chamfering and corner rounding are commanded in the same block, the latter command will
be valid. (5) Tool compensation is calculated for the shape which has already been subjected to corner chamfering. (6) Program error (P385) will occur when positioning or thread cutting is commanded in the corner chamfering com-
mand block or in the next block. (7) Program error (P382) will occur when the block following corner chamfering contains a G command other than
group 01 or another command. (8) Program error (P383) will occur when the movement amount commanded in the corner chamfering block is less
than the chamfering amount. (9) Program error (P384) will occur when the movement amount is less than the chamfering amount in the block
following the block commanding corner chamfering. (10) Even if a diameter is commanded, it will be handled as a radial command value during corner chamfering. (11) Program error (P382) will occur when a movement command is not issued in the block following the corner
chamfering II command.
Function and purpose
Function and purpose
Command format
N100 G03 X__ Y__ I__ J__ ,C__ ;
N200 G01 X__ Y__ ;
,C Length up to chamfering starting point or end point from hypothetical corner
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
522IB-1501278-P
(1) Linear - arc
(2) Arc - arc
Program example
Absolute command N1 G28 XY; N2 G90 G00 X100. Y100.; N3 G01 X50.Y150.,C20. F100; N4 G02 X0 Y100. I-50. J0; :
Incremental command N1 G28 XY; N2 G91 G00 X100. Y100.; N3 G01 X-50.Y50.,C20. F100; N4 G02 X-50. Y-50. I-50. J0; :
(a) Hypothetical corner intersection point
Absolute command N1 G28 XY; N2 G91 G00 X140. Y10.; N3 G02 X60.Y50.I0 J100. ,C20. F100; N4 X0 Y30.I-60.J80.; :
Incremental command N1 G28 XY; N2 G91 G00 X140. Y10.; N3 G02 X-80.Y40. R100. ,C20. F100; N4 X-60. Y-20. I-60. J80.; :
(a) Hypothetical corner intersection point
Y
150.
100.
X 100.50.
N4
C20. C20.
N3
(a)
(mm)
Y
130.
110.
50.
30.
10. X
140.60.
N4 C20.
C20.
N3
(a)
(mm)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
523 IB-1501278-P
15.2.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_
The corner is rounded by commanding ",R_" in the 1st block of the two continuous blocks containing an arc.
Corner rounding is performed at the point where N100 and N200 intersect.
(1) If this function is commanded while the corner chamfer or corner rounding command is not defined in the spec- ifications, it causes a program error (P381).
(2) The start point of the block following the corner rounding is the hypothetical corner intersection point. (3) When both corner chamfering and corner rounding are commanded in a same block, the latter command will be
valid. (4) Tool compensation is calculated for the shape which has already been subjected to corner rounding. (5) Program error (P385) will occur when positioning or thread cutting is commanded in the corner rounding com-
mand block or in the next block. (6) Program error (P382) will occur when the block following corner rounding contains a G command other than
group 01 or another command. (7) Program error (P383) will occur when the movement amount in the corner rounding block is less than the R value. (8) Program error (P384) will occur when the movement amount is less than the R value in the block following the
corner rounding. (9) Even if a diameter is commanded, it will be handled as a radial command value during corner rounding. (10) A program error (P382) will occur if a movement command is not issued in the block following corner rounding.
Function and purpose
Command format
N100 G03 X__ Y__ I__ J__ ,R__ ;
N200 G01 X__ Y__ ;
,R Arc radius of corner rounding
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
524IB-1501278-P
(1) Linear - arc
(2) Arc - arc
15.2.3 Corner Chamfering Expansion/Corner Rounding Expansion
For details, refer to "Corner Chamfering I / Corner Rounding" and "Corner Chamfering Expansion / Corner Rounding Expansion".
15.2.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding
For details, refer to "Corner Chamfering I / Corner Rounding" and "Interrupt during Corner Chamfering Interrupt during / Corner Rounding".
Program example
Absolute command N1 G28 XY; N2 G90 G00 X100. Y30.; N3 G01 X50.Y80.,R10. F100; N4 G02 X0 Y30. I-50.J0; : Incremental command N1 G28 XY; N2 G91 G00 X100. Y30.; N3 G01 X-50.Y50.,R10. F100; N4 G02 X-50. Y-50. I-50.J0; :
(a) Hypothetical corner intersection point
Absolute command N1 G28 XY; N2 G90 G00 X100. Y30.; N3 G02 X50.Y80. R50.,R10.F100; N4 X0 Y30. R50.; : Incremental command N1 G28 XY; N2 G91 G00 X100. Y30.; N3 G02 X-50.Y50. I0 J50.,R10.F100; N4 X-50. Y-50. I-50. J0; :
(a) Hypothetical corner intersection point
Y
80.
30.
X 100.50.
N4 N3
(a)
(mm)
R10.
Y
80.
30.
X 100.50.
N4 N3
(a)
(mm)
R10.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
525 IB-1501278-P
15.3 Linear Angle Command; G01 X_/Y_ A_/,A_
The end point coordinates are automatically calculated by commanding the linear angle and one of the end point coordinate axes.
This designates the angle and the X or Y axis coordinates. Select the command plane with G17 to G19.
(1) The angle is set based on the positive (+) direction of the horizontal axis for the selected plane. The counter- clockwise (CCW) direction is indicated by a positive sign (+), and the clockwise (CW) direction by a negative sign (-).
(2) Either of the axes on the selected plane is commanded for the end point. (3) The angle is ignored when the angle and the coordinates of both axes are commanded. (4) When only the angle has been commanded, this is treated as a geometric command. (5) The angle of either the start point (a1) or end point (a2) may be used. (6) This function is valid only for the G01 command; it is not valid for other interpolation or positioning commands. (7) The range of slope "a" is between -360.000 and 360.000.
When a value outside this range is commanded, it will be divided by 360 (degrees) and the remainder will be commanded. (Example) If 400 is commanded, 40 (remainder of 400/360) will become the command angle.
(8) If an address A is used for the axis name or the 2nd miscellaneous function, use ",A" as the angle. (9) If "A" and ",A" are commanded in a same block, ",A" will be interpreted as the angle.
A program error (P33) will occur if this function is commanded during the high-speed machining mode or high- speed high-accuracy mode.
Function and purpose
Command format
N1 G01 Xx1(Yy1) Aa1;
N2 G01 Xx2(Yy2) A-a2; (A-a2 can also be set as Aa 3. )
N1 G01 Xx1(Yy1) ,Aa1;
N2 G01 Xx2(Yy2) ,A-a2;
Detailed description
Y
y2
y1 ( x1,y1)
N1
X
N2
a1
a2
a3
( x2,y2)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
526IB-1501278-P
15.4 Geometric I; G01 A_
When it is difficult to calculate the intersection point of two straight lines of consecutive linear interpolation com- mands, the end point of the first straight line will be automatically calculated inside the NC and the movement com- mand will be controlled, provided that the gradient of the first straight line as well as the end point coordinates and gradient of the second straight line are commanded.
(1) If the parameter "#1082 Geomet" is set to "0", geometric I will not function.
(1) The gradient indicates the angle to the positive (+) direction of the horizontal axis for the selected plane. The counterclockwise (CCW) direction is indicated by a positive sign (+), and the clockwise (CW) direction by a neg- ative sign (-).
(2) The range of gradient "a" is between -360.000 and 360.000. When a value outside this range is commanded, it will be divided by 360 (degrees) and the remainder will be commanded. (Example) If 400 is commanded, 40 (remainder of 400/360) will become the command angle.
(3) The gradient of the line can be commanded on either the start or end point side. Whether designated gradient is the starting point or the end point will be automatically identified in NC.
(4) When the angle where the two straight lines intersect is less than 1, program error (P392) occurs. (5) The end point coordinates of the second block should be commanded with absolute position. If incremental com-
mand is used, program error (P393) occurs. (6) The feedrate can be commanded for each block. (7) Instead of G01, thread cutting (G33) or variable lead thread cutting (G34) can be specified as a linear path com-
mand. Only G02/G03 commands can be specified as arc path commands. If another G code is programmed in the second block, the program error (P394) is issued.
(8) Axes cannot be specified in the first block. If an axis is specified, the command is not treated as a geometric command, but a normal linear/arc path command.
(9) If address "A" is used for an axis name or a second miscellaneous function, geometric I cannot be used. The commands are treated as normal linear path commands, not geometric commands.
Function and purpose
Command format
N1 G01 Aa1 (A-a2) Ff1;
N2 Xx2 Yy2 Aa4 (A-a3) Ff2;
Aa1, A-a2, A-a3, Aa4 Angle Ff1, Ff2 Speed Xx2, Yy2 End point coordinates of the next block
(C) Current position (E) End point coordinates (I) Intersection point (calculated automatically)
Detailed description
Note
a1
Y
X N1 N2a2
a3
a4
(x2,y2)
(I)
(E) (C)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
527 IB-1501278-P
A description is provided using the following examples.
(C) Current position (E) End point coordinates (I) Intersection point (calculated automatically) (1) Corner chamfering and corner rounding can be commanded after the angle command in the 1st block.
(2) The geometric command I can be issued after the corner chamfering or corner rounding command.
(3) The geometric command I can be issued after the linear angle command.
Relationship with other functions
(Example 1) N1 Aa1 ,Cc1 ; N2 Xx2 Yy2 Aa2 ;
(Example 2) N1 Aa1 ,Rr1 ; N2 Xx2 Yy2 Aa2 ;
(Example 3) N1 Xx2 Yy2 ,Cc1 ; N2 Aa1 ; N3 Xx3 Yy3 Aa2 ;
(Example 4) N1 Xx2 Aa1 ; N2 Aa2 ; N3 Xx3 Yy3 Aa3 ;
N2
N1
(x2,y2)
a2
a1
c1
c1
(x1,y1)(C)
(I)
(E)
N2
N1
(x2,y2)
a1
a2
r1
(x1,y1)(C)
(I)
(E)
N2
N1(x2,y2)
(x3,y3) a2
a1
c1
c1
(x1,y1)
N3
(C)
(I) (E)
N2
N1(x2,y2)
(x3,y3) a3
a2
(x1,y1)
N3
a1
(C)
(I) (E)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
528IB-1501278-P
15.5 Geometric IB
Geometric IB is used to obtain the contact point or the intersection point for two travel commands in consecutive blocks when at least one of the commands is a circular path command. The center point of the circular arc or the slope angle of the straight line is required instead of the end point of the first block.
(1) If the parameter "#1082 Geomet" is not set to "2", geometric IB will not function. (2) Instead of G01, thread cutting (G33) or variable lead thread cutting (G34) can be specified as a linear path com-
mand. Only G02/G03 commands can be specified as circular path commands. If another G code is programmed in the second block, the program error (P394) occurs.
(3) Axes cannot be specified in the first block. If an axis is specified, the command is not treated as a geometric command, but a normal linear/circular path command.
(4) If address "A" is used for an axis name or a second miscellaneous function, a linear path command cannot be used. In such cases, the commands are treated as normal linear/circular path commands, and the intersection point of straight line and circular arc or the contact point between straight line and circular arc are not automati- cally calculated.
Function and purpose
Contact point of two contacting arcs (Refer to 15.5.1.)
The following diagrams are described using the follow- ing examples. (C) Current position (E) End point (I) Intersection point (calculated automatically) (T) Contact point (calculated automatically)
Intersection point between linear and arc (or, arc and linear) (Refer to 15.5.2.)
Contact point between linear and arc (or, arc and linear) (Refer to 15.5.3.)
Note
N2
N1
r2
r1
Y
X (C)
(T) (E)
N2
N2 N1
N1
Y
X
r1
r1
(C)
(C)
(I)
(I)
(E)
(E)
N2
N2
N1 N1
r1 r1
Y
X
(C)
(C)
(E)
(E)
(T)
(T)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
529 IB-1501278-P
15.5.1 Geometric IB (Automatic Calculation of Contact Point of Two Circular Arcs); G02/G03 P_Q_ /R_
When the contact point of two consecutive contacting circular arcs is not indicated in the drawing, it can be automat- ically calculated using any one of the following commands. Command the center coordinate position of the 1st arc as well as the end point (absolute position) and center co-
ordinate position of the 2nd arc. Command the center coordinate position of the 1st arc and the radius of the 2nd arc. Command the radius of the 1st arc as well as the end point (absolute position) and center coordinate position of
the 2nd arc.
(*1) This command can be issued using P and Q (X and Z axes circle center coordinates (absolute position)) instead of I and K.
The circle center point for Y axis of G17 or G19 plane is specified with J (incremental position) or A (absolute position).
P, A, and Q are treated as addresses that are irrelevant to geometric command, not as a circle center point.
Function and purpose
Command format
N1 G02(G03) Ii1 Kk1 Ff1;
N2 G03(G02) Xx2 Yy2 Ii2 Kk2 Ff2;
N1 G02(G03) Ii1 Kk1 Ff1;
N2 G03(G02) Xx2 Yy2 Rr2 Ff2;
N1 G02(G03) Rr1 Ff1;
N2 G03(G02) Xx2 Yy2 Ii2 Kk2 Ff2;
I, K (*1) Circle center coordinates (incremental position) (diameter/radius value command) in X and Z axes 1st block arc : Radius command incremental amount from the start point to the center 2nd block arc : Radius command incremental amount from the end point to the center
R Arc radius (when a (-) sign is attached, the arc is judged to be 180 or more)
r2
r1
(x2,y2)
Y
X
(i2,k2)
(i1,k1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
530IB-1501278-P
(1) The end point coordinates of the 2nd block should be commanded with the absolute position. A program error (P393) occurs before the 1st block if commanded with the incremental position.
(2) A program error (P390) occurs before the 1st block if there is no geometric IB specification. (3) In case of the 2nd block arc, a program error (P395) occurs before the 1st block if the R command (*1) or I/K (P/
Q) command is not issued. (*1) In this case, the 1st block must be set with the I or K (P or Q) command.
(4) A program error (P397) occurs before the 1st block if two arcs that do not contact are commanded. (5) The accuracy to calculate the contact point is 1 m (fractions rounded up). (6) The error range at calculating the contact point is set in parameter "#1084 RadErr".
(7) When I or K is omitted, the values are regarded as "I0" and "K0". P and Q cannot be omitted. (8) If the start point and the end point of an arc block is identical, the R-designated arc command finishes immedi-
ately. To command a true circle, use the IK (PQ)-designated arc command. (9) When the 2nd block arc inscribes the 1st block arc and the 2nd block is an R-designated arc, the path by the arc
command depends on the R sign. When the R sign is positive, the path is set the inward turning arc command (refer to the path of "R+" in the figure). When the R sign is negative, the path is set to the outward turning arc command (refer to the path of "R-" in the figure).
(10) When the arc center of the 2nd block for geometric IB is commanded with IJK and the pitch is designated with address "P" or ",P", the helical interpolation is carried out for the arc of the 2nd block after geometric IB has been completed. Refer to "6.7 Helical Interpolation; G02, G03" for details.
(11) Single block operation stops at the 1st block. (12) G codes of the G modal group 1 in the 1st/2nd block can be omitted.
Detailed description
Tool path
"Arc error"
R-
R+
N2
N1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
531 IB-1501278-P
15.5.2 Geometric IB (Automatic Calculation of Intersection Point between Line And Circular Arc) ; G01 A_ , G02/G03 P_Q_H_
When the intersection point between a line and a circular arc is not indicated in the drawing though they intersect, it can be automatically calculated by commanding the following program.
(*1) This command can be issued using P and Q (X and Z axes circular arc center coordinates (absolute position)) instead of I and K.
The circular arc center point for Y axis of G17 or G19 plane is specified with J (incremental position) or A (ab- solute position).
P, A, and Q are treated as addresses that are irrelevant to geometric command, not as a circle center point.
Function and purpose
Command format (For G18 plane)
N1 G01 Aa1(A-a2) Ff1 ;
N2 G02(G03) Xx2 Yy2 Ii2 Kk2 Hh2 (,Hh2) Ff2 ;
N1 G02(G03) Ii1 Kk1 Hh1 (,Hh1) Ff1 ;
N2 G01 Xx2 Yy2 Aa3 (A-a4) Ff2 ;
A Linear angle (-360.000 to 360.000) I, K (*1) Circular arc center coordinates (incremental position) (diameter/radius value command)
in X and Z axes 1st block arc : Radius command incremental amount from the start point to the center 2nd block arc : Radius command incremental amount from the end point to the center
H (,H) Selection of intersection point between line and circular arc 0: Intersection of the shorter line 1: Intersection of the longer line
Path at H = 0
Path at H = 1
(I) Intersection point (calculated automatically) at H = 0 or 1
H=1 H=1
H=0
N2 N1
H=0
N1 a1
N2 a3
- a4 - a2 (x2,y2)
(x2,y2) Y
X
(I) (I)
(I) (I)
(i2,k2) (i1,k1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
532IB-1501278-P
(1) A program error (P390) occurs before the 1st block if there is no geometric IB specification. (2) The gradient of the line is the angle to the positive (+) direction of its horizontal axis of the selected plane. The
counterclockwise (CCW) direction is considered as positive (+) and the clockwise direction (CW) as negative (-). (3) The gradient of the line can be commanded on either the start or end point side. Whether designated gradient is
the starting point or the end point will be automatically identified. (4) In case of the 2nd block arc, a program error (P395) occurs before the 1st block if there is no I/K (P/Q) command.
A program error (P395) also occurs if there is no designation of "A" for the line. (5) The end point coordinates of the 2nd block should be commanded with the absolute position. A program error
(P393) occurs before the 1st block if commanded with the incremental position. (6) A program error (P397) occurs before the 1st block if a straight line and arc that do not contact or intersect are
commanded. (7) The accuracy to calculate the intersection point is 1 m (fractions rounded up). (8) If the start point of an arc block is identical with the end point, the result is a true circle. (9) The error range at calculating the intersection point is set in parameter "#1084 RadErr".
(10) When I or K is omitted, the values are regarded as "I0" and "K0". P and Q cannot be omitted. (11) When H is omitted, the value is regarded as "H0". (12) If R is commanded instead of P, Q (I, K) designation, the contact point between line and circular arc is calculated
automatically. (13) When the distance to the intersection from the line is the same as the distance from the arc (as in the figure
below), the control by address H (short/long distance selection) is invalidated. In this case, the judgment is car- ried out based on the angle of the line.
(14) Addresses being used as axis names cannot be used as command addresses for angles, circular arc center coordinates or intersection selections.
(15) If address "H" is used as an axis name, the intersection point must be specified with ",H". (16) If "H" and ",H" are programmed in the same block, ",H" is treated as specifying the intersection point. (17) When the circular arc center of the 2nd block for geometric IB is commanded with IJK and the pitch is desig-
nated with address "P" or ",P", the helical interpolation is carried out for the arc of the 2nd block after geometric IB has been completed. Refer to "6.7 Helical Interpolation; G02, G03" for details.
(18) Single block operation stops at the 1st block. (19) G codes of the G modal group in the 1st block can be omitted. (20) When geometric IB is commanded, two blocks are pre-read.
Detailed description
Tool path
Arc error
N2 G2 Xx2 Yy2 Ii2 Kk2 Ff2 ; N1 G1 A a1 Ff1;
N1 G1 A a2 Ff1; N2 G2 Xx2 Yy2 Ii2 Kk2 Ff2 ;
(i2,k2)
-a2
a1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
533 IB-1501278-P
Relationship with other functions
Command Tool path
Geometric IB + corner chamfering
N1 G02 P_ Q_ H_ ; N2 G01 X_ Y_ A_ ,C_ ; G01 X_ Y_ ;
N2
N1 X
Y
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
534IB-1501278-P
15.5.3 Geometric IB (Automatic Calculation of Contact Point between Line And Circular Arc) ; G01 A_ , G02/G03 R_H_
When the contact point between a line and a circular arc is not indicated in the drawing though they are in contact, it can be automatically calculated by commanding the following program.
Function and purpose
Command format (For G18 plane)
N1 G01 Aa1(A-a2) Ff1;
N2 G03(G02) Xx2 Yy2 Rr2 Ff2;
N1 G03(G02) Rr1 Ff1;
N2 G01 Xx2 Yy2 Aa3(A-a4) Ff2;
A Linear angle (-360.000 to 360.000) R Circular arc radius
(C) Current position (E) End point coordinates (T) Contact point (calculated automatically)
Y
X
N1
(E) (x2,y2)
N1N2
N2
(E) (x2,y2)
a3
- a4
- a2 r2 r1
a1
(T) (T)
(C)
(C)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
535 IB-1501278-P
(1) A program error (P390) occurs before the 1st block if there is no geometric IB specification. (2) The gradient of the line is the angle to the positive (+) direction of its horizontal axis of the selected plane. The
counterclockwise (CCW) direction is considered as positive (+) and the clockwise direction (CW) as negative (-). (3) The gradient of the line can be commanded on either the start or end point side. Whether the commanded slope
is on the start or end point side is identified automatically inside the NC unit. (4) In case of the 2nd block arc, a program error (P395) will occur before the 1st block if there is no R designation.
A program error (P395) also occurs if there is no designation of "A" for the line. (5) The end point coordinates of the 2nd block should be commanded with the absolute position. A program error
(P393) occurs before the 1st block if commanded with the incremental position. (6) A program error (P397) occurs before the 1st block if a straight line and arc that do not contact are commanded. (7) If the start point and the end point of an arc block is identical, the circular path command finishes immediately.
A true circle cannot be specified. (8) The accuracy to calculate the contact point is 1 m (fractions rounded up). (9) The error range at calculating the contact point is set in parameter "#1084 RadErr".
(10) If I or K (P or Q) is commanded instead of the R designation, the contact point between line and circular arc is calculated automatically.
(11) When the arc center of the 2nd block for geometric IB is commanded with IJK and the pitch is designated with address "P" or ",P", the helical interpolation is carried out for the arc of the 2nd block after geometric IB has been completed. Refer to "6.7 Helical Interpolation; G02, G03" for details.
(12) Single block operation stops at the 1st block. (13) G codes of the G modal group 1 in the 1st block can be omitted. (14) When geometric IB is commanded, two blocks are pre-read.
Detailed description
Relationship with other functions
Command Tool path
Geometric IB + corner chamfering
N1 G03 R_ ; N2 G01 X_ Y_ A_ ,C_ ; G01 X_ Y_ ;
Geometric IB + corner rounding
N1 G03 R_ ; N2 G01 X_ Y_ A_ ,R_ ; G01 X_ Y_ ;
Tool path
Arc error
X
Y
N1
N2
X
Y
N1
N2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
536IB-1501278-P
15.6 Mirror Image by G code ; G50.1,G51.1
When cutting a shape that is symmetrical on the left and right, programming time can be shortened by machining one side and then using the same program to machine the other side. The mirror image function is effective for this. For example, when using a program as shown below to machine the shape on the left side (A), a symmetrical shape (B) can be machined on the right side by applying mirror image and executing the program.
Function and purpose
Mirror axis
Command format
Mirror image ON
G51.1 Xx1 Yy1 Zz1;
x1, y1, z1 Mirror image center coordinates (Mirror image will be applied regarding this position as a center)
Mirror image OFF
G50.1 Xx2 Yy2 Zz2;
x2, y2, z2 Mirror image cancel axis (The values of x2, y2, z2 will be ignored.)
Y
X
(A) (B)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
537 IB-1501278-P
(1) At G51.1, command the mirror image axis and the coordinate to be a center of mirror image with the absolute command or incremental command.
(2) At G50.1, command the axis for which mirror image is to be turned OFF. The values of x2, y2, and z2 will be ignored.
(3) If mirror image is applied on only one axis of the designated plane, the rotation direction and compensation di- rection will be reversed for the arc or tool radius compensation and coordinate rotation, etc.
(4) This function is processed on the local coordinate system, so the center of the mirror image will change when the counter is preset or when the workpiece coordinates are changed.
(5) Reference position return during mirror image If the reference position return command (G28, G30) is executed during the mirror image, the mirror image will be valid during the movement to the intermediate point, but will not be applied to the movement to the reference position after the intermediate point.
(6) Return from zero point during mirror image If the return command (G29) from the zero point is commanded during the mirror image, the mirror will be applied to the intermediate point.
(7) The mirror image will not be applied to the G53 command.
Detailed description
Path on which mirror is applied Mirror center Programmed path
Intermediate point when mirror is applied
Intermediate point
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
538IB-1501278-P
(1) Combination with radius compensation The mirror image (G51.1) will be processed after the radius compensation (G41, G42) is applied, so the following type of cutting will take place.
Relationship with other functions
Programmed path Path with mirror image applied
Programmed path
Path with only radius compensation applied
Path with only mirror image applied
Path with mirror image and radius compensa- tion applied
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
539 IB-1501278-P
If mirror image is not canceled at the mirror center, the absolute position and machine position will deviate as shown below. (This state will last until an absolute command (positioning with G90 mode) is issued, or a reference position return with G28 or G30 is executed.) The mirror center is set with an absolute position, so if the mirror center is com- manded again in this state, the center may be set to an unpredictable position. Cancel the mirror at the mirror center or position with the absolute command after canceling.
Precautions
CAUTION
Turn the mirror image ON and OFF at the mirror image center.
Absolute position (position commanded in program)
Machine position
When moved with the incremental command after mirror cancel
Mirror cancel command
Mirror axis command
Mirror center
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
540IB-1501278-P
15.7 Normal Line Control; G40.1/G41.1/G42.1 (G150/G151/G152)
The C axis (rotary axis) turning will be controlled so that the tool constantly faces the normal line direction in respect to the movement of the axes in the selected plane during program operation. At the block seams, the C axis turning is controlled so that the tool faces the normal line direction at the next block's start point.
During arc interpolation, the rotary axis turning is controlled in synchronization with the operation of the arc interpo- lation.
The normal line control I and II can be used according to the C axis turning direction during normal line control. Which method is to be used depends on the MTB specifications (parameter "#1524 C_type").
Function and purpose
C axis center (rotary axis)
Tool end position
C axis turning
Rotation axis center (C axis)
Tool end position
Normal line con- trol type
Turning direction Turning speed Turning speed in arc in- terpolation
Type I Direction that is 180 or less (shortcut direction)
Parameter speed (#1523 C_feed)
Speed when the program path follows the F com- mand
(#1524 C_type = 0)
Type II As a principle, the com- manded direction
Feedrate Speed when the tool nose follows the F command (#1524 C_type = 1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
541 IB-1501278-P
The normal line control axis depends on the MTB specifications (parameter #1522 C_axis). Normal line control is carried out in respect to the movement direction of the axis which is selecting the plane. G17 plane I-J axes G18 plane K-I axes G19 plane J-K axes Whether the normal line control is canceled at resetting depends on the MTB specifications (parameter #1210 Rst- Gmd/ bitE).
Command format
Normal line control cancel
G40.1 (G150)X__ Y__ F__ ;
Normal line control left ON
G41.1 (G151)X__ Y__ F__ ;
Normal line control right ON
G42.1 (G152)X__ Y__ F__ ;
X X axis end point coordinate Y Y axis end point coordinate F Feedrate
G41.1 Normal line control left side G42.1 Normal line control right side
(a) Center of rotation (b) Tool end(b) Tool end
Programmed path
Tool end path
(a)
(b)
(a)
(b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
542IB-1501278-P
The normal line control angle is 0 (degree) when the tool is facing the horizontal axis (+ direction) direction. The counterclockwise direction turning is + (plus), and the clockwise direction turning is - (minus).
Detailed description
Definition of the normal line control angle
G17 plane (I - J axes) ... The axis angle is 0(degree) when the tool is facing the +I direction.
G18 plane (K - I axes) ...The axis angle is 0(degree) when the tool is facing the +K direction.
G19 plane (J - K axes) ... The axis angle is 0(degree) when the tool is facing the +J direction.
0 I+
J+
90
180
270
0 K+
I+
90
180
270
0 J+
K+
90
180
270
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
543 IB-1501278-P
(1) Start-up After the normal line control axis turns to the right angle of the advance direction at the start point of the normal line control command block, the axis which is selecting the plane is moves. Note that the normal line control axis at the start up turns in the direction that is 180 or less (shortcut direction) in both the normal line control type I and II.
(2) During normal line control mode (a) Operation in block
During interpolation of the linear command, the angle of the normal line control axis is fixed, and the normal line control axis does not turn. During the arc command, the normal line control axis turns in synchronization with the operation of the arc interpolation.
Normal line control turning operation in respect to movement command
: N1 G01 Xx1 Yy1 Ff1 ; N2 G41.1 ; Without movement
commands in the G41.1 block
N3 Xx2 Yy2 ; :
: N1 G01 Xx1 Yy1 Ff1 ; N2 G41.1 Xx2 Yy2 ; With movement com-
mands in the G41.1 block
:
: G41.1 ; N1 G02 Xx1 Yy1 Ii1 Jj1 ; :
Programmed path
Tool end path
(x2,y2)
(x1,y1) N3
N3
N1
G41.1
(x2,y2)
(x1,y1) N2
N2
N1
G41.1
(i1,j1)
(x1,y1)
N1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
544IB-1501278-P
(b) Block seam
(3) Cancel The normal line control axis will not turn, and the plane selecting axis will be moved by the program command.
No tool radi- us compen- sation
After the normal line control axis is turned to be at the right angle of the plane selecting movement in the next block, the operation moves to the next block.
Liner - Liner Liner - Arc Arc - Arc
Programmed path Tool end path
With tool ra- dius com- pensation
If tool radius compensation is applied, normal line control is carried out along the path to which the tool radius compensation is applied.
Liner - Liner Liner - Arc Arc - Arc
Programmed path
Tool radius compensation path
Tool end path
: N1 G01 Xx1 Yy1 Ff1 ; N2 G40.1 ; Without movement com-
mands in the G40.1 block
N3 Xx2 Yy2 ; :
: N1 G01 Xx1 Yy1 Ff1 ; N2 G40.1 Xx2 Yy2 ; With movement com-
mands in the G40.1 block
:
(x2,y2)
(x1,y1) N3
N1
G40.1
(x2,y2)
(x1,y1) N2
N1
G40.1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
545 IB-1501278-P
During normal line control, the turning operation for the normal line control axis is not carried out at the seam be- tween a block and the next block, in which the movement amount is smaller than that set with the parameter (#1535 C_leng).
(1) For liner block; When the movement amount of the N2 block is smaller than the parameter(#1535 C_leng), the normal line con- trol axis is not turned at the seam between the N1 block and N2 block. It stays the same direction as the N1 block.
(2) For arc block; When the diameter value of the N2 block is smaller than the parameter(#1535 C_leng), the normal line control axis is not turned at the seam between the N1 block and N2 block. It stays the same direction as the N1 block. During arc interpolation of the N2 block, the normal line control axis does not turn in synchronization with the operation of arc interpolation.
Since operation fractions are created by calculating the intersection point of two segments, the turning operation may or may not be carried out when the parameter (#1535 C_leng) and the segment length are equal.
Normal line control temporary cancel
N2 block movement amount < Parameter(#1535 C_leng)
N2 block diameter value < Parameter (#1535 C_leng)
(a) Diameter value
N3N1 N2
N3N1
N2
(a)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
546IB-1501278-P
The normal line control axis turning direction at block seam differs according to the normal line control type I or II (parameter #1524 C_type). The turning angle is limited by the angle set with the parameter (#1521 C_min). These parameter settings depend on the MTB specifications.
Normal line control axis turning direction at block seam
Item Normal line control type I Normal line control type II
Normal line control axis turning direction at block seam
Direction that is 180 or less. (shortcut direction)
G41.1: - direction (CW) G42.1: + direction (CCW)
Normal line control axis turning angle at block seam
When | | < , turning is not performed. : Turning angle : Parameter (#1521 C_min) When the turning angle is 180 degrees,
the turning direction is undefined re- gardless of the command mode.
[G41.1/G42.1 When the normal line control axis is at 0]
(a) The normal line control axis turns coun- terclockwise. (b) The normal line control axis turns clock- wise. (c) The axis does not turn.
When | | < , turning is not per- formed. : Turning angle : Parameter (#1521 C_min)
The operation error (0118) will occur in the following cases: [For G41.1] <= < 180 - [For G42.1] 180 + < <= 360 - [G41.1 When the normal line control axis is at 0]
[G42.1 When the normal line control axis is at 0]
(c) The axis does not turn. (d) The normal line control axis turns. (e) Operation error (0118)
-
0180
270
90 (a)
(b) (c)
-
0180
270
90
180 -
(c) (d)
(e)
-
0180
270
90
180 +
(c)
(d)
(e)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
547 IB-1501278-P
(1) Normal line control type I Normal line control axis turning
angle at block seam: G41.1 G42.1
1. - < <
No turning No turning
2. <= < 180
3. 180 <= <= 360-
Shortcut direction Shortcut direction
-
0180
270 (-90 )
90
0180
270 (-90 )
90
360 -
0180
270 (-90 )
90
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
548IB-1501278-P
(2) Normal line control type II
(*1) If the axis turns into the command direction, it turns inside the workpiece, causing an operation error.
Normal line control axis turn- ing angle at block seam:
G41.1 G42.1
1. - < <
No turning No turning
2. <= < 180-
Operation error (0118) (*1)
3. 180- <= <= 180+
4. 180+ < <= 360-
Operation error (0118) (*1)
-
0180
270 (-90 )
90
0180
270 (-90 )
90
180 -
180 -
0180
270 (-90 )
90
180 +
360 -
0180
270 (-90 )
90
180 +
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
549 IB-1501278-P
The turning angle falls to or below the minimum turning angle (parameter "#1521 C_min") before the circular inter- polation starts; therefore, turning operation may not be inserted. In this case, it depends on the parameter "#12105 C_minTyp" whether to interpolate the turning angle which was not inserted before the tool reaches the end point of circular interpolation. These parameters depends on the MTB specifications. If the turning angle set before the linear interpolation starts falls to or below the minimum turning angle, turning is not carried out.
[The turning angle is interpolated up to the end point of the arc (#12105 C_minTyp = 0).] The turning angle in the section in which the normal line control axis is not turned is interpolated up to the end point of the circular interpolation.
[The turning angle is not interpolated (#12105 C_minTyp = 1).] The turning angle in the section in which the normal line control axis is not turned is not interpolated during circular interpolation.
Operation to be performed when the turning angle set before the circular interpolation starts falls below the minimum turning angle
N1 N2
The turning angle falls below the value of parameter #1521.
Programmed path
Tool end path
Circular center
(The control does not insert the turning movement)
N1 N2
The turning angle falls below the value of parameter #1521.
Circular center
Programmed path
Tool end path (The control does not insert the turning movement)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
550IB-1501278-P
Normal line control axis turning speed Turning speed at block seam (select from type I or type II)
(1) Normal line control axis turning speed at block seam (a) Rapid traverse
Therefore, an operation error will occur.
Normal line control type I Normal line control type II
Dry run OFF The rapid traverse rate (#2001 rapid) is applied. Normal line control axis turning speed f = Rapid traverse rate * (Rapid traverse override) ( / min)
Dry run OFF Normal line control axis turning speed f = F * 180 / ( * R) * (Rapid traverse override) (/min) When R = 0, follow the formula below. Normal line control axis turning speed f = F * (Rapid traverse override) ( /min) F: Rapid traverse rate (#2001 rapid) (mm/min) R: Parameter (#8041 C-rot.R) (mm) (Length from normal line control axis center to tool nose)
(1) If the normal line control axis turning speed ex- ceeds the rapid traverse rate (#2001 rapid), the rapid traverse rate will be applied.
Dry run ON The manual feedrate is applied. Normal line control axis turning speed f = Manual feedrate * (Cutting feed override) ( /min)
(1) When the manual override valid is ON, the cutting feed override is valid.
(2) If the normal line control axis turning speed ex- ceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be ap- plied.
(3) When the rapid traverse is ON, the dry run is in- valid.
Dry run ON Normal line control axis turning speed f = F * 180 / ( * R) * (Rapid traverse override) (/min) When R = 0, follow the formula below. Normal line control axis turning speed f = F * (Rapid traverse override) ( /min) F: Rapid traverse rate (#2001 rapid) (mm/min) R: Parameter (#8041 C-rot.R) (mm) (Length from normal line control axis center to tool nose)
(1) If the normal line control axis turning speed ex- ceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be ap- plied.
(2) If the normal line control axis turning speed ex- ceeds the rapid traverse rate (#2001 rapid), the rapid traverse rate will be applied.
(3) When the rapid traverse is ON, the dry run is in- valid.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
551 IB-1501278-P
(b) Cutting feed Normal line control type I Normal line control type II
Dry run OFF
The normal line control axis turning speed set with the parameter (#1523 C_feed) is applied. Normal line control axis turning speed f = Parameter (#1523 C_feed) * (Cutting feed override) ( /min)
The feedrate at the tool nose is the F command. The normal line control axis turning speed is the normal line control axis speed that follows this F command. Normal line control axis turning speed f = F * 180 / ( * R) * (Cutting feed override) (/min) When R = 0, follow the formula below. Normal line control axis turning speed f = F ( /min) F: Feedrate command (mm/min) R: Parameter (#8041 C-rot.R) (mm) (Length from normal line control axis center to tool nose)
Dry run ON (Rapid traverse ON)
The cutting feed clamp speed (#2002 clamp) is ap- plied. Normal line control axis turning speed f = Cutting feed clamp speed (/min) Dry run ON (Rapid traverse OFF) The manual feedrate is applied. Normal line control axis turning speed f = Manual feedrate * (Cutting feed override) ( /min)
(1) When the manual override valid is ON, the cutting feed override is valid.
(2) If the normal line control axis turning speed ex- ceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be ap- plied.
F: Feedrate command f: Normal line control axis turning speed
(1) If the normal line control axis turning speed ex- ceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be ap- plied.
(2) When the dry run is ON, the normal line control axis turning speed is obtained by the same ex- pression as the rapid traverse.
F: Feedrate command f: Normal line control axis turning speed R: Parameter (#8041 C-rot.R)
(F)
(f) =F*180/( *R)
(F)
(f)
(R)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
552IB-1501278-P
(2) Normal line control axis turning speed during circular interpolation
(1) If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the speed will be as follows; - Normal line control axis turning speed = Cutting feed clamp speed. Normal line control axis turning speed = Cutting feed clamp speed Moving speed during arc interpolation = The speed according to the normal line control axis turning speed
Normal line control type I Normal line control type II
The normal line control axis turning speed is the rota- tion speed obtained by feedrate F. Normal line control axis turning speed f = F * 180 / ( * r) ( /min) F : Feed command speed (mm/min) r : Arc radius (mm)
The feedrate at the tool nose is the F command. The normal line control axis turning speed is the rotation speed that follows this F command. Normal line control axis turning speed f = F * 180 / ( * (R + r)) ( /min) F : Feed command speed (mm/min) R : Parameter (#8041 C-rot. R) (mm) (Length from normal line control axis center to tool nose) r : Arc radius (mm)
=F*180/( *r)
(F)
(r)
(f)
=F*180/( *(R+r))
(F)
(R) (r)
(f)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
553 IB-1501278-P
During normal line control, an arc is automatically inserted at the corner in the axis movement of the plane selection. This function is for the normal line control type I. The radius of the arc to be inserted is set with the parameter (#8042 C-ins.R). This parameter can be read and written using the macro variable #1901. Normal line control is performed also during the interpolation for the arc to be inserted.
The corner arc is not inserted in the following cases: linear and arc, arc and arc, linear and moveless or move- less and linear blocks or when a line is shorter than the radius of the arc to insert.
During the radius compensation, the radius compensation is applied to the path that the corner arc is inserted.
Automatic corner arc insertion function
Parameter (#8042 C-rot. R)
Corner R is not inserted.
Radius compensation path Parameter (#8042 C-rot. R)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
554IB-1501278-P
The stop point of the single block and block start interlock is as follows.
The stop point of the cutting start interlock is as follows.
Stop point
Stop point
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
555 IB-1501278-P
Program example
Normal line control type I
Main program
O500
Sub-program
O501 G91X0Y0;G28C0; G90G92G53X0Y0; G00G54X25.Y-10.; G03G41.1X35.Y0.R10.F10.; #10=10; WHILE[#10NE0]DO1;
M98P501;
#10=#10-1; END1; G03X25.Y10.R10.; G40.1; G28X0Y0; M02;
G03X8.Y9.R15.; G02X-8.R10.; G03Y-9.R-15.; G02X8.R10.; G03X35.Y0.R15.;
M99;
(0,0)
R10
R10R15
20.20.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
556IB-1501278-P
(Example 1)
(a) C-axis (b) Tool
Normal line control type II
Main program
O500
Sub-program
O1001 G91X0Y0; G28Z0; G28C0; G90G92G53X0Y0Z0; G00G54G43X35.Y0.Z100.H1; G00Z3.; G01Z0.1F6000; G42.1;
M98P1001L510;
M98P1002L2;
G91G01Y10.Z0.05; G40.1; G90G00Z100.; G28X0Y0Z0; M02;
G17G91G01Y20.,R10.Z-0.01; X-70.,R10.; Y-40.,R10.; X70.,R10.; Y20.;
M99;
(Corner chamfering/Corner R specifica- tions are required)
O1002 G17G91G01Y20.,R10.; X-70.,R10.; Y-40.,R10.; X70.,R10.; Y20.;
M99;
(Corner chamfering/Corner R specifica- tions are required)
5.
(b)
0.1
10.
(a)
20.
(0,0)
R10
20.
35. 35.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
557 IB-1501278-P
(Example 2) Main program
O2000
Sub-program
O2001 G91G28Z0; G28X0Y0; G28C0; G90G92G53X0Y0Z0; G00G54X30.Y0.; G00Z3.; G41.1G01Z0.1F5000;
M98P2001L510;
M98P2002L2;
G91G01X-30.Z0.05; G40.1; G90G00Z100.; G28X0Y0Z0; M02;
G17G91G01X-60.Z-0.01; X60.;
M99;
O2002 G17G91G01X-60.; X60.;
M99;
(a) C-axis (b) Tool
5.
(b)
0.1
(a)
(0,0)
30. 30.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
558IB-1501278-P
Relationship with other functions
Function name Notes
Unidirectional positioning Normal line control is not applied. Helical cutting Normal line control is applied normally. Spiral interpolation As the start point and end point are not on the same arc, a normal line control will
not be applied correctly. Exact stop check The operation will not decelerate and stop for the turning movement of the normal
line control axis. Error detect Error detect is not applied to the turning movement of the normal line control axis. Override Override is applied to the turning movement by normal line control axis. Coordinate rotation by pro- gram
Normal line control is applied to the shape after coordinate rotation.
Scaling Normal line control is applied to the shape after scaling. Mirror image Normal line control is applied to the shape after mirror image. Thread cutting Normal line control is not applied. Geometric command Normal line control is applied to the shape after geometric command. Automatic reference position return
Normal line control is not applied.
Start position return Normal line control is not applied to the movement to the intermediate point posi- tion. If the base specification parameter "#1086 G0Intp" is OFF, normal line control is applied to the movement from the intermediate point to a position designated in the program.
High-speed machining mode III
This cannot be commanded during normal line control. A program error (P29) will occur. The normal line control command during high-speed machining mode III cannot be issued, either. A program error (P29) will occur.
High-accuracy control This cannot be commanded during normal line control. A program error (P29) will occur. The normal line control command during high-accuracy control cannot be issued, either. A program error (P29) will occur.
Spline This cannot be commanded during normal line control. A program error (P29) will occur. The normal line control command during spline cannot be issued, either. A program error (P29) will occur.
High-speed High-accuracy control I/II
This cannot be commanded during normal line control. A program error (P29) will occur. The normal line control command during high-speed High-accuracy control I/II cannot be issued either. A program error (P29) will occur.
Cylindrical interpolation This cannot be commanded during normal line control. A program error (P486) will occur. The normal line control command during cylindrical interpolation cannot be is- sued, either. Program error (P481) will occur.
Workpiece coordinate sys- tem offset
The workpiece coordinate system cannot be changed during normal line control. A program error (P29) will occur. The program parameter input (G10L2) cannot be commanded either. A program error (P29) will occur.
Local coordinate system off- set
The local coordinate system cannot be changed during normal line control. A pro- gram error (P29) will occur.
Program restart The program including the normal line control command cannot be restarted. "E98 CAN'T RESEARCH" will occur.
Dry run The feedrate is changed by the dry run signal even in respect to the turning move- ment of the normal line control axis.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
559 IB-1501278-P
(1) During normal line control, the program coordinates are updated following the normal line control axis movement. Thus, program the normal line control on the program coordinate system.
(2) The normal line control axis will stop at the turning start position for the single block, cutting block start interlock and block start interlock.
(3) If the movement command is issued to the normal line control axis (C axis) during normal line control, it is ig- nored.
(4) The coordinate system preset command (G92 C_;) cannot be issued to the normal line control axis during C axis normal line control (during G41.1 or G42.1 modal). The program error (P901) will occur if commanded.
(5) When a mirror image is applied to the axis in plane selection mode, normal line control is carried out for the shape processed with the mirror image.
(6) The rotary axis must be designated as the normal line control axis (parameter "#1522 C_axis"). Designate so that the axis is not duplicated with the axis on the plane where normal line control is to be carried out. If an illegal axis is designated, the program error (P902) will occur when the program (G40.1, G41.1, G42.1) is commanded. The program error (P902) will also occur if the parameter "#1522 C_axis" is "0" when commanding a program. This parameter setting depends on the MTB specifications.
(7) The movement of the normal line control axis is counted as one axis of number of simultaneous contouring con- trol axes. If the number of simultaneous contouring control axes exceeds the specification range by movement of the nor- mal line control axis, the program error (P10) will occur.
Graphic check The section turned by normal line control is not drawn. The axes subject to graphic check are drawn.
G00 non-interpolation Normal line control is not applied. Polar coordinate interpola- tion
This cannot be commanded during normal line control. A program error (P486) will occur. The normal line control command during polar coordinate interpolation cannot be issued either. Program error (P481) will occur.
Exponential interpolation If the normal line control axis is the same as the rotary axis of exponential interpo- lation, a program error (P612) will occur. If they are different, an error will not occur, but normal line control is not applied.
Plane selection This cannot be commanded during normal line control. A program error (P903) will occur.
Mixed control This cannot be commanded during normal line control. An operation error (M01 1035) will occur.
System variable The block end coordinate (#5001 - ) for the normal line control axis during normal line control cannot obtain a correct axis position.
Precautions
Function name Notes
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
560IB-1501278-P
15.8 Manual Arbitrary Reverse Run Prohibition ; G127
The manual arbitrary reverse run function controls the feedrate, which is under automatic operation in memory or MDI mode, in proportion to the manual feedrate by the jog or the rotation speed by the manual handle, and manually carries out the reverse run. After the automatic operation has been stopped in a block, the reverse run can be carried out back through the blocks (up to 20 blocks) that were executed before the block. If necessary, it is possible to correct the program buffer and execute the fixed program after carrying out the reverse run up to the return position.
This function (G127) is available to prevent the program from backing to blocks before the commanded block when carrying out the manual arbitrary reverse run. The detailed setting and operation vary depending on the machine specifications. Refer to the Instruction Manual issued by the MTB. "Forward run" means to execute blocks in the same order as for the automatic operation. "Reverse run" means to process the executed blocks backward. Whether the reverse run is prohibited for each part system depends on the MTB specifications (system variable #3003). Refer to "List of System Variables" for details.
This command disables the program from running reverse to blocks before G127. In part systems that do not have this command executed, the program cannot run reverse before the timing with G127 commanded in any part sys- tem even if a block is in process. No commands in the machining program can be backed in the reverse run mode. For some G codes, the operation differs from the above. Refer to "Relationship with Other Functions".
Function and purpose
Command format
All part system reverse run prohibit command
G127 ;
The reverse run is disabled before the G127 block in the 2nd part system. The reverse run is canceled in the middle of a block in part systems other than the 2nd part system.
G127
$1
$2
$3
$4
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
561 IB-1501278-P
The following shows the relationship between the manual arbitrary reverse run command and G code.
Fixed cycles or MSTB commands may be prohibited to reverse run or the reverse run operation on tapping cy- cle may differ depending on the MTB specifications (parameter "#1260 set32" or related PLC signals). Refer to the specifications of your machine tool.
Even if the G61.1 or G05, for which reverse run is prohibited, is not commanded in the machining program, when the initial high-accuracy control (#1148) is valid, reverse run is to be prohibited because of the modal of G61.1 (the value of #1148 is "1") or G05 (the value of #1148 is "2", "3" or "4").
Relationship with other functions
Symbol in "Reverse run"
column
Operation
*1 Block with reverse run enabled *2 Block with restricted-reverse run enabled Refer to the Remarks for restrictions. Block with reverse run ignored. This block is ignored in both the forward and reverse run modes. *3 Block with reverse run prohibited. This is intended only for the command blocks. *4 Block with reverse run prohibited. The reverse run is also prohibited for all blocks after the mode
has been switched by this block. *5 Prohibits the reverse run in all part systems.
G code Function name Reverse run
Remarks
G00 Positioning *1 - G01 Linear interpolation *1 - G02 Circular interpolation CW
Spiral/conical interpolation CW (type2) *1 -
G03 Circular interpolation CCW Spiral/conical interpolation CCW (type2)
*1 -
G02.1 Spiral/conical interpolation CW (type1) *3 - G03.1 Spiral/conical interpolation CCW (type1) *3 - G02.2 Involute interpolation CW *3 - G03.2 Involute interpolation CCW *3 - G02.3 Exponential interpolation CW *3 - G03.3 Exponential interpolation CCW *3 - G02.4 3-dimensional circular interpolation *3 - G03.4 3-dimensional circular interpolation *3 - G04 Dwell *1 Dwell skip is invalid. G05 High-speed high-accuracy control II/III /
High-speed machining mode *4 This includes the initial high-accuracy control
(#1148). G05.1 High-speed high-accuracy control I / Spline *4 - G06.2 NURBS interpolation *4 - G07 Hypothetical axis interpolation *3 - G07.1 G107
Cylindrical interpolation *4 -
G08 High-accuracy control *4 - G09 Exact stop check *1 - G10 Program data input (Parameter / Compen-
sation amount / Coordinate rotation by pa- rameter data) / Life management data registration
The reverse run is enabled, but data is not recovered.
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
562IB-1501278-P
G10.6 Tool retract command *3 - G11 Program parameter input / cancel The reverse run is enabled, but data is not
recovered. G12 Circular cutting CW *3 - G13 Circular cutting CCW *3 - G12.1 G112
Polar coordinate interpolation ON *4 -
G13.1 G113
Polar coordinate interpolation cancel *4 -
G15 Polar coordinate command OFF *4 - G16 Polar coordinate command ON *4 - G17 X-Y plane selection *2 Data is recovered using the modal informa-
tion storage block. G18 Z-X plane selection *2 Data is recovered using the modal informa-
tion storage block. G19 Y-Z plane selection *2 Data is recovered using the modal informa-
tion storage block. G20 Inch command *1 Switched with the movement command just
after commanded. G21 Metric command *1 Switched with the movement command just
after commanded. G22 Stroke check before travel ON *3 - G23 Stroke check before travel OFF *3 - G27 Reference position check *3 - G28 Automatic reference position return *3 - G29 Start position return *3 - G30 2nd, 3rd and 4th reference position return *3 - G30.1 Tool change position return 1 *3 - G30.2 Tool change position return 2 *3 - G30.3 Tool change position return 3 *3 - G30.4 Tool change position return 4 *3 - G30.5 Tool change position return 5 *3 - G30.6 Tool change position return 6 *3 - G31 Skip/Multi-step skip function 2 *3 - G31.1 Multi-step skip function 1-1 *3 - G31.2 Multi-step skip function 1-2 *3 - G31.3 Multi-step skip function 1-3 *3 - G33 Thread cutting *2 The reverse run is enabled, but the synchro-
nous feed is invalid. Actual cutting mode available.
G34 Special fixed cycle (bolt hole circle) *4 - G35 Special fixed cycle (write at angle) *4 - G36 Special fixed cycle (arc) *4 - G37 Automatic tool length measurement *3 - G37.1 Special fixed cycle (grid) *4 - G38 Tool radius compensation vector designa-
tion *3 -
G39 Tool radius compensation corner arc *3 - G40 Tool radius compensation cancel / 3-dimen-
sional tool radius compensation cancel *2 Data is recovered using the modal informa-
tion storage block. G41 Tool radius compensation left / 3-dimen-
sional tool radius compensation left *2 Data is recovered using the modal informa-
tion storage block.
G code Function name Reverse run
Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
563 IB-1501278-P
G42 Tool radius compensation right / 3-dimen- sional tool radius compensation right
*2 Data is recovered using the modal informa- tion storage block.
G40.1 G150
Normal line control cancel *4 -
G41.1 G151
Normal line control left ON *4 -
G42.1 G152
Normal line control right ON *4 -
G43 Tool length compensation (+) *2 Data is recovered using the modal informa- tion storage block.
G44 Tool length compensation (-) *2 Data is recovered using the modal informa- tion storage block.
G43.1 Tool length compensation along the tool axis
*3 -
G43.4 Tool center point control type1 ON *4 - G43.5 Tool center point control type2 ON *4 - G45 Tool position offset (expansion) *2 Data is recovered using the modal informa-
tion storage block. G46 Tool position offset (reduction) *2 Data is recovered using the modal informa-
tion storage block. G47 Tool position offset (double) *2 Data is recovered using the modal informa-
tion storage block. G48 Tool position offset (decreased by half) *2 Data is recovered using the modal informa-
tion storage block. G49 Tool length compensation cancel / Tool cen-
ter point control cancel *1/ *3
If tool length compensation cancel is desig- nated, reverse running is enabled.
G50.2 Scaling cancel *4 - G51.2 Scaling ON *4 - G50.1 Mirror image by G code cancel *3 - G51.1 G command mirror image ON *3 - G52 Local coordinate system setting *2 Data is recovered using the modal informa-
tion storage block. G53 Machine coordinate system selection *2 Data is recovered using the modal informa-
tion storage block. G54 Workpiece coordinate system 1 selection *2 Data is recovered using the modal informa-
tion storage block. G55 Workpiece coordinate system 2 selection *2 Data is recovered using the modal informa-
tion storage block. G56 Workpiece coordinate system 3 selection *2 Data is recovered using the modal informa-
tion storage block. G57 Workpiece coordinate system 4 selection *2 Data is recovered using the modal informa-
tion storage block. G58 Workpiece coordinate system 5 selection *2 Data is recovered using the modal informa-
tion storage block. G59 Workpiece coordinate system 6 selection *2 Data is recovered using the modal informa-
tion storage block. G54.1 Workpiece coordinate system selection 48
/ 96 sets extended *2 Data is recovered using the modal informa-
tion storage block. G60 Unidirectional positioning *3 - G61 Exact stop check mode *1 - G61.1 High-accuracy control ON *4 This includes the initial high-accuracy control
(#1148). G61.2 High-accuracy spline *4 - G62 Automatic corner override *1 -
G code Function name Reverse run
Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
564IB-1501278-P
G63 Tapping mode *1 - G63.1 Synchronous tapping mode (Forward tap-
ping) *4 -
G63.2 Synchronous tapping mode (Reverse tap- ping)
*4 -
G64 Cutting mode *1 - G65 Macro call Simple call *1 - G66 User macro Modal call A *1 - G66.1 User macro Modal call B *1 - G67 User macro Modal call cancel *1 - G68 Coordinate rotation by program mode ON /
3-dimensional coordinate conversion mode ON
*4 -
G68.2 Inclined surface machining command *3 - G68.3 Inclined surface machining command
(Based on tool axis direction) *3 -
G69 Coordinate rotation by program mode can- cel / 3-dimensional coordinate conversion mode cancel / Inclined surface machining command cancel
*4 -
G70 User fixed cycle *3 - G71 User fixed cycle *3 - G72 User fixed cycle *3 - G73 Fixed cycle (step) *1 Data is created for each movement block in
the fixed cycle. G74 Fixed cycle (reverse tap) *2 The reverse run is enabled, but the synchro-
nous feed is invalid. Actual cutting mode available.
G74.5 G74.6 G74.8
Fixed cycle (reverse Punchtap cycle) *4 The command is valid only in the actual cut- ting mode. The program error (P182) occurs in the dry run mode.
G75 Fixed cycle (circular cutting cycle) *1 Data is created for each movement block in the fixed cycle.
G76 Fixed cycle (Fine boring) *1 Data is created for each movement block in the fixed cycle.
G77 User fixed cycle *3 - G78 User fixed cycle *3 - G79 User fixed cycle *3 - G80 Fixed cycle for drilling cancel *1 - G81 Fixed cycle (drill/spot drill) *1 Data is created for each movement block in
the fixed cycle. G82 Fixed cycle (drill/counter boring) *1 Data is created for each movement block in
the fixed cycle. G83 Fixed cycle (deep drilling) *1 Data is created for each movement block in
the fixed cycle. G84 Fixed cycle (tapping) *2 The reverse run is enabled, but the synchro-
nous feed is invalid. Actual cutting mode available.
G84.5 G84.6 G84.8
Fixed cycle (Punchtap cycle) *4 The command is valid only in the actual cut- ting mode. The program error (P182) occurs in the dry run mode.
G85 Fixed cycle (boring) *1 Data is created for each movement block in the fixed cycle.
G code Function name Reverse run
Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
565 IB-1501278-P
G86 Fixed cycle (boring) *1 Data is created for each movement block in the fixed cycle.
G87 Fixed cycle (back boring) *1 Data is created for each movement block in the fixed cycle.
G88 Fixed cycle (boring) *1 Data is created for each movement block in the fixed cycle.
G89 Fixed cycle (boring) *1 Data is created for each movement block in the fixed cycle.
G90 Absolute command *2 Switched with the movement command just after commanded.
G91 Incremental command *2 Switched with the movement command just after commanded.
G92 Coordinate system setting *1 - G92.1 Workpiece coordinate system preset *1 - G93 Inverse time feed *1 - G94 Asynchronous feed (feed per minute) *1 - G95 Synchronous feed (feed per revolution) *1 - G96 Constant surface speed control ON *2 Switched with the movement command just
after commanded. G97 Constant surface speed control OFF *2 Switched with the movement command just
after commanded. G98 Fixed cycle
(Initial level return) *1 -
G99 Fixed cycle R point level return *1 - G115 Start point designation timing synchroniza-
tion Type 1 *1 -
G116 Start point designation timing synchroniza- tion Type 2
*1 -
G118.2 Parameter switching (Spindle) *3 - G119.2 Inertia Estimation (Spindle) *3 - G100 - G225
User macro (G code call) Max. 10 *1 -
M98 Subprogram call *1 -
G code Function name Reverse run
Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
566IB-1501278-P
15.9 Data Input by Program 15.9.1 Parameter Input by Program; G10 L70, G11
The parameters set from the setting and display unit can be changed in the machining programs.
For commanding data with decimal point, and character string data. The data's command range conforms to the setting range of each parameter.
(1) The sequence of addresses in a block must be as shown above. When an address is commanded two or more times, the last command will be valid.
(2) The part system No. is set in the following manner. "1" for the 1st part system, "2" for 2nd part system, and so forth. If the address S is omitted, the part system of the executing program will be applied. As for the parameters common to part systems, the command of part system No. will be ignored.
(3) The axis No. is set in the following manner. "1" for 1st axis, "2" for 2nd axis, and so forth. If the address A is omitted, the 1st axis will be applied. As for the parameters common to axes, the command of axis No. will be ignored.
(4) Address H is commanded with the combination of setting data (0 or 1) and the bit designation (0 to 7). Hd0: Sets the dth bit OFF. (d: 0 to 7) Hd1: Sets the dth bit ON. (d: 0 to 7)
(5) Only the decimal number can be commanded with the address D. The value that is smaller than the input setting increment (#1003 iunit) will be round off to the nearest increment.
(6) The character string must be put in angled brackets "<" and ">". If these brackets are not provided, the program error (P33) will occur. Up to 63 characters can be set.
Function and purpose
Command format
Data setting start command
G10 L70 ;
P__ S__ A__ H__ ; Bit parameter
P__ S__ A__ D__ ; Numerical value parameter
P__ S__ A__
P Parameter No. S Part system No. A Axis No. H Bit type data D Numeric type data character string Character string data
Data setting end command
G11 ;
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
567 IB-1501278-P
(7) G11 must be commanded alone in a block. A program error (P33 or P421) will occur if it is not commanded alone in a block.
(8) The parameter "#1078 Decimal pnt type 2" is disabled. (9) The following data cannot be changed with the G10 L70 command: Tool compensation data workpiece coordinate data PLC switch PLC axis parameter Device open parameters SRAM open parameters DeviceNet parameters
(10) The settings of the parameters with (PR) in the parameter list will be enabled after the power is turned OFF and ON. Refer to the parameter list in your manual.
The timing for updating the spindle parameter and the NC axis parameter settings depends on the MTB specifica- tions (parameter "#1254 set26/bit3").
(*1) The parameters of the target spindle are not updated while the functions below are active. The parameters are updated after the functions have been completed. Synchronous tapping cycle The spindle for spindle position control is in C axis mode and the C axis is in motion.
(*2) The program updates the exchange axis under the arbitrary axis exchange control, waiting for "all axes smooth- ing zero" in the exchange destination part system.
Precautions
Parameter update timing
#1254 set26/bit3 Spindle parameter NC axis parameter
Invalid The program updates the parameter settings, waiting for "all axes smoothing zero" in all part systems.
Valid The program updates the parameter set- tings without waiting for "smoothing zero". (*1)
The program updates the parameter set- tings, waiting for "all axes smoothing zero" in control part systems. (*2)
Program example
G10 L70 ; P6401 H71 ; Sets "1" to "#6401 bit7". P8204 S1 A2 D1.234 ; Sets "1.234" to "#8204 of the 1st part system 2nd axis". P8621
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
568IB-1501278-P
15.9.2 Compensation Data Input by Program (Tool Compensation Amount) ; G10 L10/L11/L12/L13, G11
The tool compensation can be set or changed by the program using the G10 command.
During the absolute command (G90) mode, the commanded offset amount serves as the new offset amount, where- as during the incremental command (G91) mode, the sum of present offset and the commanded offset serves as the new offset amount.
Tool compensation memory type I
Tool compensation memory type II
(1) Type I is selected when parameter "#1037 cmdtyp" is set to "1", and type II is selected when set to "2".
(1) G10 is a non-modal command and is valid only in the commanded block. (2) The G10 command does not perform any movement, but must not be used with G commands other than G90 or
G91. (3) Do not command G10 in the same block as the fixed cycle and subprogram call command. This will cause mal-
functioning and program errors. (4) The workpiece offset input command (L2 or L20) should not be issued in the same block as the tool compensa-
tion input command (L10). (5) If an illegal L No. or compensation No. is commanded, the program errors (P172 and P170) occur respectively.
If the offset amount exceeds the maximum command value, the program error (P35) occurs. (6) Decimal point inputs can be used for the offset amount. (7) If the G command that cannot be combined with G10 is issued in the same block, a program error (P45) occurs. (8) A program error (P35) occurs for any value that does not match the compensation amount setting unit after com-
mand unit conversion. With an incremental command, the setting range for the compensation amount is the sum of the present setting value and commanded value.
Function and purpose
Command format
Tool compensation input (L10/L11/L12/L13)
G10 L10 P_ R_ ;
P Compensation No. R Compensation amount
G10 L10 P_ R_ ; Tool length compensation (Shape compensation)
G10 L11 P_ R_ ; Tool length compensation (Wear compensation)
G10 L12 P_ R_ ; Tool radius compensation (Shape compensation)
G10 L13 P_ R_ ; Tool radius compensation (Wear compensation)
Compensation input cancel
G11 ;
Detailed description
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
569 IB-1501278-P
(1) Input the compensation amount.
H10=-12.345, H05=9.8765, H30=2.468
(2) Updating of compensation amount (Example 1) Assume that "H10 = -1000" is already set.
(Example 2) Assume that "H10 = -1000" is already set.
Main program
Subprogram O1111
Program example
N1 G01 G90 G43 Z-100000 H10 F100 ; (Z=-101000) N2 G28 Z0 ; N3 G91 G10 L10 P10 R-500 ; (The mode is the G91 mode, so -500 is added.) N4 G01 G90 G43 Z-100000 H10 ; (Z=-101500)
N1 G00 X100000 ; a N2 #1=-1.; N3 M98 P1111 L4 ; b1, b2, b3, b4
N1 G01 G91 G43 Z0 H10 F100 ; c1, c2, c3, c4 G01 X1000 ; d1, d2, d3, d4 #1=#1-1.; G90 G10 L10 P10 R#1 ; M99 ;
; G10 L10 P10 R-12.345 ; G10 L10 P05 R9.8765 ; G10 L10 P30 R2.468 ;
(a) (b1) (b2) (b3) (b4)
1000 1000 1000 1000
10 00
10 00
10 00
10 00c1
d1
c3 d3
c2 d2
c4 d4
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
570IB-1501278-P
(Example 3) The program for Example 2 can also be written as follows.
Main program
Subprogram O1111
(1) Even if this command is displayed on the screen, the offset No. and variable details will not be updated until ac- tually executed.
N1 G00 X100000 ; N2 M98 P1111 L4 ;
N1 G01 G91 G43 Z0 H10 F100 ; N2 G01 X1000 ; N3 G10 L10 P10 R-1000 ; N4 M99 ;
Precautions
N1 G90 G10 L10 P10 R-100 ; N2 G43 Z-10000 H10 ; N3 G00 X-10000 Y-10000 ; N4 G90 G10 L10 P10 R-200 ; The H10 offset amount is updated when the N4 block is executed.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
571 IB-1501278-P
15.9.3 Compensation Data Input by Program (Workpiece Offset Amount) ; G10 L2/L20, G11
The workpiece offset can be set or changed by the program using the G10 command.
During the absolute command (G90) mode, the commanded offset amount serves as the new offset amount, where- as during the incremental command (G91) mode, the sum of present offset and the commanded offset serves as the new offset amount.
(1) The compensation amount in the G91 will be an incremental amount and will be accumulated each time the pro- gram is executed. Command G90 or G91 before G10 as much as possible.
(2) When address P is omitted, set the offset amount in the currently selected workpiece coordinate system (G54 to G59). When the G54.1 modal is active, a program error (P35) occurs.
(1) The specifications of the extended workpiece coordinate system selection are required. (2) When address P is omitted, set the offset amount in the currently selected "G54.1 Pn". When the G54 to G59
modals are active, a program error (P33) occurs.
Function and purpose
Command format
Workpiece coordinate system offset input (L2)
G90 (G91) G10 L2 P_ X_ Y_ Z_ ;
P 0 : External workpiece 1 : G54 2 : G55 3 : G56 4 : G57 5 : G58 6 : G59 Other than 0 to 6: Program error
X, Y, Z Offset amount of each axis
Extended workpiece coordinate system offset input (L20)
G90 (G91) G10 L20 P_ X_ Y_ Z_ ;
P "n" No. of G54.1 Pn (1 to 300) X, Y, Z Offset amount of each axis
Note
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
572IB-1501278-P
(1) When both of addresses P and L are omitted, set the offset amount in the currently selected workpiece coordi- nate system (one of G54 to G59, or G54.1 Pn).
(1) G10 is non-modal command and is valid only in the commanded block. (2) The G10 command does not perform any movement, but must not be used with G commands other than G54 to
G59, G90 or G91. (3) Do not command G10 in the same block as the fixed cycle and subprogram call command. This will cause mal-
functioning and program errors. (4) The workpiece offset input command (L2 or L20) should not be issued in the same block as the tool compensa-
tion input command (L10). (5) If an illegal L No. is commanded, the program error (P172) occurs.
If the offset amount exceeds the maximum command value, the program error (P35) occurs. (6) Decimal point inputs can be used for the offset amount. (7) The offset amounts for the external workpiece coordinate system and the workpiece coordinate system are com-
manded as distances from the basic machine coordinate system zero point. (8) The workpiece coordinate system updated by inputting the workpiece coordinate system will follow the previous
modal (G54 to G59) or the modal (G54 to G59) in the same block. (9) L2/L20 can be omitted when the workpiece offset is input. (10) When the P command is omitted for workpiece offset input, it will be handled as the currently selected work-
piece compensation input. (11) If the G command that cannot be combined with G10 is issued in the same block, a program error (P45) occurs. (12) A program error (P35) occurs for any value that does not match the compensation amount setting unit after
command unit conversion. With an incremental command, the setting range for the compensation amount is the sum of the present setting value and commanded value.
Offset input to the currently selected workpiece coordinate system (When the L command is omitted)
G90 (G91) G10 P_ X_ Y_ Z_ ;
P (1) During G54 to G59 modal 0 : External workpiece offset (EXT) 1 to 6 : Workpiece offset input (G54 to G59) Other than 0 to 6 : Program error (P35) (2) During G54.1 Pn modal 1 to 300 : Extended workpiece coordinate offset amount set-
ting (G54.1 Pn) Other than 1 to 300 : Program error (P35)
X, Y, Z Offset amount of each axis
Compensation input cancel
G11 ;
Detailed description
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
573 IB-1501278-P
(1) When updating the workpiece coordinate system offset amount Assume that the previous workpiece coordinate system offset amount is as follows.
X=-10.000, Y=-10.000
The G54 workpiece position display data will change before and after the workpiece coordinate system is changed with G10 in N101.
When workpiece coordinate system offset amounts are set in G54 to G59
Program example
N100 G00 G90 G54 X0 Y0 ; N101 G90 G10 L2 P1 X-15.000 Y-15.000 ; N102 X0 Y0 ; M02 ;
Basic machine coordinate system zero point
G54 coordinate before change
G54 coordinate after change
X = 0
Y = 0
-> X = +5.000
Y = +5.000
G90 G10 L2 P1 X-10.000 Y-10.000 ; G90 G10 L2 P2 X-20.000 Y-20.000 ; G90 G10 L2 P3 X-30.000 Y-30.000 ; G90 G10 L2 P4 X-40.000 Y-40.000 ; G90 G10 L2 P5 X-50.000 Y-50.000 ; G90 G10 L2 P6 X-60.000 Y-60.000 ;
- X - 20. - 10.
- 10.
- 20.
- Y
- Y
- Y
- X
- X
N100
N101
N102
M
(W1)
W1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
574IB-1501278-P
(2) When using one workpiece coordinate system as multiple workpiece coordinate systems
(1) Even if this command is displayed on the screen, the offset No. and variable details will not be updated until ac- tually executed.
(2) It is recommended to command G10 in a block different from the one in which any of G54 to G59 and G54.1 is commanded. When G10 and any of G54 to G59 and G54.1 are commanded in the same block, it operates as follows. When "#1274 ext10/bit5" is set to "0"
When "#1274 ext10/bit5" is set to "1" ("G54 Pn" is handled as "G54.1 Pn")
Main program : #1=-50. #2=10. ; M98 P200 L5 ; M02 ; %
Subprogram O200
N1 G90 G54 G10 L2 P1 X#1 Y#1 ; N2 G00 X0 Y0 ; N3 X-5. F100 ; N4 X0 Y-5. ; N5 Y0 ; N6 #1=#1+#2 ; N7 M99 ; %
Basic machine coordinate system zero point
Precautions
G10 G54 Pn Xx ; Changes the modal to G54 and executes "G10 Pn". G10 G54 Xx ; (without "P") Changes the modal to G54 and executes G10 for G54. G10 G54.1 Pn Xx ; Changes the modal to G54.1 Pn and executes G10 for "G54.1
Pn". G10 G54.1 Xx ; (without "P") Program error (P33)
G10 G54 Pn Xx ; Program error (P33) G10 G55 Pn Xx ; Changes the modal to G55 and executes "G10 Pn". G10 G54 Xx ; (without "P") Changes the modal to G54 and executes G10 for G54. G10 G54.1 Pn Xx ; Program error (P33) G10 G54.1 Xx ; (without "P") Program error (P33)
- X - 10.
- 10.
M
- 20.
- Y - 50.
- 30.
- 60.
- 40.
G54'' ''
W
W
W
W
W
G54'' '
G54''
G54'
G54
- 50. - 40. - 30. - 20.
1
2
3
5
4
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
575 IB-1501278-P
15.9.4 Compensation Data Input by Program (Turning Tool) ; G10 L12/L13, G11
If the tool compensation type is changed to type III by the compensation type selection function, it is possible to write the offset amount for three base axes, nose R compensation amount, and tool nose point (parameter "#1046 T-ofs disp type"). During the absolute (G90) mode, the commanded tool compensation amount serves as a new one. During the incremental (G91) mode, the currently set compensation amount plus the commanded compensation amount serves as the new compensation amount.
The commanded range and unit of the compensation amount are as follows. Program error (P35) occurs for any value not listed in the table after command unit conversion. With an incremental command, the commanded range for the compensation amount is the sum of the present setting value and com- mand value.
Function and purpose
Command format
Turning tool compensation input (L12/L13)
G10 L12 P__ X__ Y__ Z__ R__ Q__ ; (Shape compensation)
P Tool shape compensation No. (1 to number of tool compensation sets) X, Y, Z Compensation amount for each axis R Nose R compensation amount Q Hypothetical tool nose point
G10 L13 P__ X__ Y__ Z__ R__ Q__ ; (Wear compensation)
P Wear compensation No. (1 to number of tool compensation sets) X, Y, Z Compensation amount for each axis R Nose R compensation amount Q Hypothetical tool nose point
Compensation input cancel
G11 ;
Detailed description
Setting Compensation amount
Metric system Inch system
#1003=B 9999.999 (mm) 999.9999 (inch) #1003=C 9999.9999 (mm) 999.99999 (inch) #1003=D 9999.99999 (mm) 999.999999 (inch) #1003=E 9999.999999 (mm) 999.9999999 (inch)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
576IB-1501278-P
(1) The X, Y, and Z addresses are set to the axis names specified in the parameters for three base axes (parameters "#1026 base_I", "#1027 base_J", and "#1028 base_K"). The compensation data input by program of the tool offset is not available for an axis address that is not specified in the parameters for three base axes. Therefore, be sure to carry out compensation data input by program after specifying the parameters for three base axes.
(2) The compensation data input by program is available using a command (G10 L10, L11, L12, or L13) in a normal machining center system, but only the compensation amount of the Z axis and nose R can be input as data.
Precautions
G10 L10 P__ R__; Z axis shape compensation G10 L11 P__ R__; Z axis wear compensation G10 L12 P__ R__; Nose R shape compensation G10 L13 P__ R__; Nose R wear compensation
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
577 IB-1501278-P
15.9.5 Tool Shape Input by Program; G10 L100, G11
This function sets tool shape data of the tool management screen by the machining program. Using this function saves the step to input tool shapes on the screen when the 3D checks is executed.
Function and purpose
Command format
Tool shape settings from the program
G10 L100; Data setting start command
P_ T_ K_ D_ H_ I_ J_ C_ ; Data setting command
P Data No. Specify the data No. on the tool management screen. (Cannot be omitted.) The maximum value of data No. varies depending on the number of tool management data sets.
T Tool No. Specify the tool No. (Cannot be omitted.) 0 to 99999999 When "0" is specified, all the tool shape data of data No. specified by address P will be "0". In this case, only the tool shape data is changed.
K Type Designate the tool type using a numerical value. [Mill tool] 1: Ball end mill 2: Flat end mill 3: Drill 4: Radius end mill 5: Chamfer 6: Tap 7: Face mill
D Shape data 1 Designate shape data of the tool. (Decimal point input enabled) The setting details of shape data differ depending on the tool type.H Shape data 2
I Shape data 3 Refer to the following "Correspondence between tool types and shape data" for the settings for each tool type.J Shape data 4
C Tool color Specify the tool color. 1: Gray 2: Red 3: Yellow 4: Blue 5: Green 6: Light blue 7: Purple 8: Pink
G11; Data setting end command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
578IB-1501278-P
[Correspondence between tool types and shape data]
[Mill tool]
(*1) When "#8968 Tool shape radius validity" is set to "0", input the diameter value. When it is set to "1", input the radius value.
(1) Omitted addresses cannot be set. (2) If address "P" or "T" is omitted, a program error (P422) will occur. (3) For M80 Series, the tool shape data on the Tool management screen is rewritten during the graphic check. (4) For M800W Series, M800S Series, and M80W Series, this change is only reflected on the graphic check drawing.
The tool shape data on the Tool management screen is not rewritten.
This function sets the tool shape of the Tool management screen from the machining program. The 3D check switches the drawing of tools at the timing of a tool change command. Therefore, the machining pro- gram should be prepared to run a tool shape setting command prior to the tool change command being issued.
(a) The tool is drawn with the shape that has been changed by the machining program.
(b) The tool is drawn with a shape that has been registered on the tool management screen.
(c) The tool is drawn with a new shape that has been registered by the machining program.
Shape data Item by tool type
Ball end mill Flat end mill Drill Radius end mill
Chamfer Tap Face mill
1 Tool radius (*1) 2 Tool length 3 - - Tool nose
angle Corner rounding
End angle Pitch Cutter length
4 - - - - End diame- ter (*1)
Thread di- ameter
Shank diam- eter
Detailed description
Tool shape settings from the program
Note
G10 L100; P1 T201 ...; P3 T203 ...;
G11;
O200
(a)
(b)
(c)
T201; (Replaced with tool A.)
T202; (Replaced with tool B.)
T203; (Replaced with tool C.)
Machining program Tool shape data
Tool A
Tool B Tool C
3D check screen
Tool management screen
(Change the shape of tool A.)
(Newly register the shape of tool C.)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
579 IB-1501278-P
(1) Tool shape settings from the program
(1) If the G10 or G11 command is not issued alone in a block, a program error (P422) will occur. (2) If a block contains an address whose data is out of range, a program error (P35) will occur. (3) If a block contains an illegal address, a program error (P32) will occur. (4) The parameter "#1078 Decpt2" is valid for position commands (K address, W address).
Other command addresses comply with the minimum input unit ("#1015 cunit"). (MTB specifications) (5) The parameter "#8044 UNIT*10" is invalid. (6) The command unit of parameters to be input in mm/inch can be switched by G20/G21. (7) The maximum value of "G10 L100" data No. (address P) is "80".
Program example
G10 L100; P1 T1 K3 D5. H20. I0 J0 C2 ; Sets the data of data No. 1. P2 T10 D10. ; Sets the tool diameter of data No. 2 to "10.". P8 T0; Sets the tool shape data of data No. 8 to "0". G11;
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
580IB-1501278-P
15.9.6 R-Navi Data Input by Program; G10 L110/L111, G11, G68.2, G69
The R-Navi setup parameters can be configured from a machining program. Command setting values with absolute positions. The input unit conforms to the input setting unit of the 1st part system and the initial inch. In either case, the input unit depends on the MTB specifications (parameters "#1003 iunit" and "#1041 I_inch"). The parameter "#8044 UNIT*10" is invalid.
G10 must be commanded alone in a block, which also applies to G11. A program error (P423) will occur if it is not commanded alone in a block.
Address Q cannot be omitted. If omitted, a program error (P423) will occur. For the omitted addresses, data remains unchanged. Cancel the selected machining surface before data setting.
If data is set to a machining workpiece including the selected machining surface, a program error (P423) will occur.
Symbols "\", "/", ",", "*", "?", """, "<", ">", "|", " " (space), "@", and "~" cannot be used as one-byte symbols. If an available symbol is set, a program error (P35) or (P32) will occur.
For details on each of input data, refer to the instruction manual.
Function and purpose
Command format
Workpiece registration and setting
G69; Canceling the selected machining surface
G10 L110; Start setting workpiece data
Q_ <_> F_ C_ R_ X_ Y_ Z_ I_ J_ K_; Data setting
G11; End data setting
Q Workpiece registration No. (1 to 10) < > Workpiece name
Designate the name using up to 20 one-byte alphanumeric characters, including symbols. (If "0" is entered, the setting value is cleared.)
F Workpiece shape 0: Rectangular parallelepiped 1: Circular cylinder
C Basic coordinate system of machining workpiece 0 to 5: G54 to G59 6 to 305: G54.1P1 to G54.1P300
R Marked point No. When the workpiece shape is set to rectangular parallelepiped, designate the marked point to set the basic coordinate system zero point. (0 to 8)
X, Y, Z, Workpiece size When the shape is set to circular cylinder, designate the diameter with X and the height with Y. (0.000 to 99999.999)
I, J, K Workpiece shift Set the shift amount from the marked point to the basic coordinate system zero point. (-99999.999 to 99999.999)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
581 IB-1501278-P
G10 must be commanded alone in a block, which also applies to G11. A program error (P423) will occur if it is not commanded alone in a block.
Addresses P, Q, and D cannot be omitted. If omitted, a program error (P423) will occur. For the omitted addresses, data remains unchanged. For the machining surface designated with P0, set the coordinate axis direction with P1 and P2. Be sure to first
command P0. If P1 or P2 is commanded before P0, a program error (P423) will occur.
The machining surface cannot be registered for an undefined workpiece. If the registration command is issued, a program error (P423) will occur.
Cancel the selected machining surface before data setting. If data is set to the selected machining surface, a program error (P423) will occur.
(1) Command address to register the machining surface
Symbols "\", "/", ",", "*", "?", """, "<", ">", "|", " " (space), "@", and "~" cannot be used as one-byte symbols. If an available symbol is set, a program error (P35) or (P32) will occur.
For details on each of input data, refer to the instruction manual.
Machining surface registration and setting
G69; Canceling the selected machining surface
G10 L111; Start setting machining surface data
P0 Q_ D_ <_> X_ Y_ Z_ A_; Machining surface setting (Refer to (1).)
P1 M_ B_ C_ E_ F_ H_ I_; Designate the coordinate axis direction (1st axis). (Refer to (2).)
P2 M_ B_ C_ E_ F_ H_ I_; Designate the coordinate axis direction (2nd axis). (Refer to (2).)
G11; End data setting
G68.2 P10 Q_ D_; Selecting the registered machining surface
P Machining surface registration (0)
Q Workpiece registration No. (1 to 10) D Machining surface registration No.
(2 to 17) < > Designate the name of the machining surface using up to 15 one-byte alphanu-
meric characters, including symbols. (If "0" is entered, the setting value is cleared.)
X, Y, Z Designate the coordinate system zero point (feature coordinate system zero point) of the machining surface with the offset from the basic coordinate zero point. In this case, designate the coordinate axis direction of the basic coordinate sys- tem. (-99999.999 to 99999.999)
A From three orthogonal axes (X, Y, and Z axes), select two coordinate axes to des- ignate the coordinate axis direction along the machining surface. 0: Z/X axis 1: Y/Z axis 2: X/Y axis
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
582IB-1501278-P
(2) Command address to designate the coordinate axis direction
(*1) The setting details vary depending on the coordinate axis direction designation method (M address).
[M address: 0 (On-axis point (+))] B, C, E: Coordinate value on X, Y, or Z axis F to I: Vacuous
[M address: 1 (Latitude/Longitude)] B: Latitude (1) C: Longitude (2) E to I: Vacuous
[M address: 2 (Latitude/Projection angle)] B: Latitude (1) C: Projection angle (2) E to I: Vacuous
[M address: 3 (Start point/End point)] B: Start point coordinate value (X) C: Start point coordinate value (Y) E: Start point coordinate value (Z) F: End point coordinate value (X) H: End point coordinate value (Y) I: End point coordinate value (Z)
[M address: 4 (Indexing angle)] B: 1st rotation angle (1) C: 2nd rotation angle (2) E to I: Vacuous
Method 5 (indexing angle) in the coordinate axis direction designation method is only available in the Z axis direction. If a command is issued to an axis other than the Z axis designated by the coordinate axis selection command (P0Ax), a program error (P423) will occur.
For details on each of input data, refer to the instruction manual.
P Coordinate axis direction designation axis 1: 1st axis 2: 2nd axis
M Coordinate axis direction designation method Designate the method to set the coordinate axis direction along the machining sur- face. 0: [Method 1] On-axis point (+) 1: [Method 2] Latitude/Longitude 2: [Method 3] Latitude/Projection angle 3: [Method 4] Start point/End point 4: [Method 5] Indexing angle (Z axis direction only)
B, C, E, F, H, I Coordinate axis direction setting (*1) (-99999.999 to 99999.999)
P0 A0 (Z/X axis) P2 M4 setting causes an error. (Method 5 is not able to be selected on the 2nd axis.)P0 A1 (Y/Z axis)
P0 A2 (X/Y axis) P1M4 or P2M4 setting causes an error. (Method 5 is not able to be select- ed.)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
583 IB-1501278-P
This function enables the R-Navi setup parameters to be configured from a machining program. After the parameters have been configured from the program, you can check the values or select the machining surface from the setup screen.
(1) If the machining surface is selected or canceled while the block start interlock signal (*BSL) is turned OFF, an operation error (M01 0109) will occur. After this, if the block start interlock signal (*BSL) is turned ON, the ma- chining surface is selected or canceled. The operation of the PLC signal depends on the MTB specifications.
Operation example
Restrictions
WORK1
WORK2
BASE-SURFACE
SURFACE1-2
O200
Canceling the selected machining surface G69; (Setting of workpiece) G10 L110; Q1
(Setting the machining surface) G10 L111; (Workpiece : 1, surface : 2) P0 Q1 D2
Machining program
Setup parameters
Setup screen
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
584IB-1501278-P
15.10 Tool Life Management 15.10.1 Inputting the Tool Life Management Data by G10 L3 Command; G10 L3, G11
Using the G10 command (non-modal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted.
In tool life management II/III, it is possible to register, change, or add tool life management data and delete a regis- tered group using the "G10L3" or "G10L30" command. Such a command is not available in tool life management I. If commanded, a program error (P39) occurs.
Only group No. 1 can be used to register, change and add for the tool life management III.
Function and purpose
Command format
Start of tool life management data registration
G10 L3 ;
P_ L_ Q_ ; (First group) T_ H_ D_ ;
T_ H_ D_ ;
P_ L_ Q_ ; (Next group) T_ H_ D_;
P Group No. L Tool life Q Management method T Tool No. The spare tools are selected in the order of the tool Nos. registered here. H Tool length compensation No. D Tool radius compensation No.
Start of tool life management data change or addition
G10 L3 P1;
P_ L_ Q_ ; (First group) T_ H_ D_ ;
T_ H_ D_ ;
P_ L_ Q_ ; (Next group) T_ H_ D_;
P Group No. L Tool life Q Management method T Tool No. H Tool length compensation No. D Tool radius compensation No.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
585 IB-1501278-P
(*) The setting range of the tool compensation No. varies depending on the specification of the "number of tool offset sets". If a value exceeding each command range is issued, a program error (P35) occurs.
Start of tool life management data deletion
G10 L3 P2;
P_ ; (First group) P_ ; (Next group)
P Group No.
End of tool life management data registration, change, addition or deletion
G11 ;
Detailed description
Command range
Item Command range
Group No. ( Pn ) 1 to 99999999 (Only group No. 1 can be used for the tool life management III)
Tool life ( Ln ) 0 to 65000 times (Managed by the number of times the tool was attached) 0 to 4000 minutes (Managed by the cutting hours)
Management method ( Qn ) 1 to 3 1: Managed by the number of times the tool was attached 2: Managed by the cutting hours 3: Managed by the number of cuttings
Tool No. ( Tn ) 1 to 99999999 Tool length compensation No.
( Hn ) 0 to 999 (*)
Tool radius compensation No.
( Dn ) 0 to 999 (*)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
586IB-1501278-P
Operation example
Program example Operation
Data registration G10 L3 ; After deleting all group data, registration starts. P10 L10 Q1 ; Group No. "10" is registered. T10 H10 D10 ; Tool No. "10" is registered in group No. "10". G11 ; Registration ends. M02 ; The program ends.
Group change, addi- tion
G10 L3 P1 ; Changing and addition of the group and tool starts. P10 L10 Q1 ; T10 H10 D10 ;
The change and addition operation takes place in the following manner.
(1) When group No. "10" has not been registered. Group No. "10" is additionally registered. Tool No. "10" is registered in group No. "10".
(2) When group No. "10" has been registered, but tool No. "10" has not been registered. Tool No. "10" is additionally registered in group No.
"10". (3) When group No. "10" and tool No. "10" have been both reg-
istered. The tool No. "10" data is changed.
G11; The group and tool change and addition ends. M02 ; The program ends.
Group deletion G10 L3 P2 ; The group deletion starts. P10 ; The group No. "10" data is deleted. G11 ; The group deletion ends. M02 ; The program ends.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
587 IB-1501278-P
15.10.2 Inputting the Tool Life Management Data by G10 L30 Command; G10 L30, G11
Using the G10 command (non-modal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted. Only group No. 1 can be used to register, change and add for the tool life management III. To specify additional compensation amount or direct compensation amount by management method, the tool length compensation and tool radius compensation can be registered/changed with the tool compensation amount format.
L_, Q_, T_, H_, and R_ cannot be omitted. If omitted, a program error (P33) occurs.
L_, Q_, T_, H_, and R_ cannot be omitted. If omitted, a program error (P33) occurs.
Function and purpose
Command format
Start of life management data registration
G10 L30 ;
P_ L_ Q_ ; (First group) T_ H_ R_ ;
T_ H_ R_ ;
P_ L_ Q_ ; (Next group) T_ H_ R_;
P Group No. L Tool life Q Management method T Tool No. The spare tools are selected in the order of the tool Nos. registered here. H Tool length compensation No. or tool length compensation amount R Tool radius compensation No. or tool radius compensation amount
Start of life management data change or addition
G10 L30 P1;
P_ L_ Q_ ; (First group) T_ H_ R_ ;
T_ H_ R_ ;
P_ L_ Q_ ; (Next group) T_ H_ R_;
P Group No. L Tool life Q Tool length compensation data format, tool radius compensation data format, manage-
ment method T Tool No. H Tool length compensation No. or tool length compensation amount D Tool radius compensation No. or tool radius compensation amount
Start of life management data deletion
G10 L30 P2;
P_ ; (First group) P_ ; (Second group)
P Group No.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
588IB-1501278-P
(*1) The setting range of the tool compensation No. varies depending on the specification of the "number of tool offset sets". If a value exceeding each command range is issued, a program error (P35) occurs.
End of life management data registration, change, addition or deletion
G11 ;
Detailed description
Command range
Item Command range
Group No. ( Pn ) 1 to 99999999 (Only group No. 1 can be used for the tool life manage- ment III)
Tool No. ( Tn ) 1 to 99999999 Management method ( Qabc ) abc: Three integer digits
a. Tool length compensation data format 0: Compensation No. 1: Incremental compensation amount 2: Absolute compensation amount b. Tool radius compensation data format 0: Compensation No. 1: Incremental compensation amount 2: Absolute compensation amount c. Tool management method 0: Cutting hours 1: Number of mounts 2: Number of cuttings
Tool life ( Ln ) Refer to the table below. Tool length compensation No./amount
( Hn )
Tool radius compensation No./amount
( Rn )
Management method (Qabc)
Tool length compensation (Hn)
Tool radius compensation (Rn)
Tool life (Ln)
a b c
0 - - 0 to 4000 (Cutting hours) 1 - - 0 to 65000 (Number of times
the tool was mounted) 2 - - 0 to 65000 (Number of cut-
tings) 0 - 0 to 999 (Compensation No.)
(*1) -
1 - 99999.999 (Incremental compensation amount)
-
2 - 99999.999 (Absolute com- pensation amount)
-
0 0 to 999 (Compensation No.) (*1)
- -
1 99999.999 (Incremental compensation amount)
- -
2 99999.999 (Absolute com- pensation amount)
- -
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
589 IB-1501278-P
Operation example
Program example Operation
Data registration G10 L30 ; P10 L10 Q001 ; T10 H10 R10 ;
G11 ;
M02 ;
1. After deleting all group data, the registration starts.
2. Group No. "10" is registered. Tool management method is number of mounts Compensation No. method is applied to tool length compensation and tool radius compensation.
3. Tool No. "10" is registered in group No. "10".
4. The registration ends.
5. The program ends. Group change, addi- tion
G10 L30 P1 ; P10 L10 Q122 ; T10 H0.5 R0.25 ;
G11;
M02 ;
1. Changing and addition of the group and tool starts.
2. The change and addition operation takes place in the following manner.
(1) When group No. "10" has not been registered. (a) Group No. "10" is additionally registered.
About the change and addition tool; Tool management method: count the number of cut-
tings Tool length compensation: the incremental compensa-
tion amount method Tool radius compensation: the absolute compensation
amount method. (b) Tool No. "10" is registered in group No. "10". (c) "0.5" is registered to the length data that the compensa-
tion No. of the tool length shows, and "0.25" is registered to the radius data that the compensation No. of the tool radius shows.
(2) When group No. "10" has been registered, but tool No. "10" has not been registered. Tool No. "10" is additionally registered in group No.
"10". (3) When group No. "10" and tool No. "10" have both been reg-
istered. The tool No. "10" data is changed.
3. The group and tool change and addition ends.
4. The program ends. Group deletion G10 L30 P2 ;
P10 ;
G11 ;
M02 ;
1. The group deletion starts.
2. The group No. "10" data is deleted.
3. The group deletion ends.
4. The program ends.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
590IB-1501278-P
15.10.3 Precautions for Inputting the Tool Life Management Data
(1) The tool life data is registered, changed, added to or deleted by executing the program in the memory or MDI mode.
(2) The group No. and tool No. cannot be commanded in duplicate. The program error (P179) will occur. (3) When two or more addresses are commanded in one block, the latter address will be valid. (4) If the life data (L_) is omitted in the G10L3 command, the life data for that group will be "0". (5) If the control method (Q_) is omitted in the G10L3 command, the control method for that group will follow the
base specification parameter "#1106 Tcount". Note that when carrying out the No. of cutting times control method, command the method from the program.
(6) If the control method (Q_) is not designated with 3-digit by G10 L30 command, the omitted high-order are equiv- alent to "0". Therefore, "Q1" is equivalent to "Q001", and "Q12" is equivalent to "Q012".
(7) If the length compensation No. (H_) is omitted in the G10L3 command, the length compensation No. for that group will be "0".
(8) If the radius compensation No. (D_) is omitted in the G10L3 command, the radius compensation No. for that group will be "0".
(9) Programming with a sequence No. is not possible between G10 L3 or G10 L30 and G11. The program error (P33) will occur.
(10) If the usage data count valid signal (YC8A) is ON, G10 L3 or G10 L30 cannot be commanded. The program error (P177) will occur.
(11) The registered data is held even if the power is turned OFF. (12) When G10 L3 or G10 L30 is commanded, the commanded group and tool will be registered after all of the reg-
istered data is erased. (13) The change and addition conditions in the G10 L3 P1 or G10 L30 P1 command are as follows:
(a) Change conditions Both the commanded group No. and tool No. are registered.
Change the commanded tool No. data. (b) Additional conditions Neither the commanded group No. nor tool No. is registered.
Additionally register the commanded group No. and tool No. data. The commanded group No. is registered, but the commanded tool No. is not registered.
Additionally register the commanded tool No. data to the commanded group No. (14) When the tool No. is newly registered with G10L30 command, the same length compensation No. and radius
compensation No. as the tool No. are automatically allocated. When the tool which is outside the compensation No. range is newly registered, the length compensation No. and radius compensation No. of that tool are "0". By selecting the compensation No. with the management method, the length compensation No. and radius com- pensation No. can be changed to arbitrary Nos.
(15) G10L3 command/G10L30 command cannot be used for the tool life management I. If commanded, the program error (P39) occurs.
(16) The setting range of the tool compensation No. depends on the MTB specifications. (17) Only group No. 1 can be used to register, change and add for the tool life management III.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
591 IB-1501278-P
15.10.4 Allocation of the Number of Tool Life Management Sets to Part Systems
The number of tool life management sets can be set per part system. This function is divided into following methods and which one is used depends on the MTB specifications (parame- ters "#1439 Tlife-SysAssign", "#12055 Tol-lifenum").
Arbitrary allocation: Arbitrarily allocates the number of tool life management sets to each part system. Fixed allocation: Automatically and evenly allocates the number of tool life management sets to each part system.
The arbitrary allocation enables the efficient allocation because when a certain part system needs only a small num- ber of tool life management sets, the rest can be allocated to another part system. If an auxiliary-axis part system does not need the tool life management sets at all, the number of tool life management sets can be set to "0" for the auxiliary-axis part system. Subsequent description is an example in the case where the number of tool life management sets in the system is 999 sets.
(1) Arbitrary allocation (with #1439=1) The number of sets allocated to each part system depends on the MTB specifications (parameter "#12055 Tol- lifenum"). The following example shows the number of tool offset sets allocated when the lathe system is a 4-part system. (a) When the number of tool life management sets is increased for the 1st part system ($1) of 4-part system
(b) When the number of tool life management sets is set to "0 sets" for the 3rd part system ($3) of 3-part system to use that part system as an auxiliary-axis part system
Function and purpose
250
250
250
250
200
200
200
400 $1
$2
$3
$4
$1
$2
$3
$4
334
333
333 500
0
500 $1
$2
$3
$1
$2
$3
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
592IB-1501278-P
(2) Automatic and even allocation (with #1439=0)
(*1) The maximum number of tool life management sets per part system is 999.
(*2) If there is any remainder, the remainder is allocated to the 1st part system.
(1) The maximum number of tool life management sets for 1-part system is 999. (2) For 1-part system, up to the number of tool life management sets in the system is available regardless of the
parameter setting. (3) When the value of the parameter "#12055 Tol-lifenum" is equal to or lower than the number of tool life manage-
ment sets in the system, the remainder is not allocated to any part system even if the specification allows arbi- trary allocation.
(4) When the value of the parameter "#12055 Tol-lifenum" is equal to or lower than the number of tool life manage- ment sets in the system, system alarm (Y05) is generated even if the specification allows arbitrary allocation.
(5) Even if the specification allows arbitrary allocation, fixed allocation is applied if the parameter is "#12055 Tol- lifenum"= "0" for all part systems.
(6) When entering data into the tool life management file, if the number of tool life management data exceeds that of current tool life management sets, the excess tool life management data cannot be entered.
1-part system 2-part system 3-part system (Lathe system only)
4-part system (Lathe system only)
Precautions
500
333
333 500
334
999
250
250
250
250
$1
$2
$3
$1
$2
$1
$1
$2
$3
$4
(*2)
(*1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
593 IB-1501278-P
15.11 Interactive Cycle Insertion; G180 15.11.1 Interactive Cycle Insertion
The machining and setup support cycles can be interactively inserted to a program which is opened on the edit screen. Using this function leads the programming time to be shortened. The cycle can be easily inserted by editing the data on the interactive window. The block of the cycle once inserted to the program can be directly edited in the edit screen. As long as the cycle format is not changed, the program can be reedited in the cycle edit window.
Blocks between cycle header block (G180 P1) and cycle footer block (G180 P0) are handled as blocks of interactive cycle insertion. G180 is a G code in group 0, and an unmodal command.
Function and purpose
Command format
G180 P__ A__ ;
P Cycle information identification No. 1: Cycle header 0: Cycle footer 11: Arbitrary shape header 10: Arbitrary shape footer 31: Hole position header 30: Hole position footer
A Cycle ID (Only when the cycle information identification No. is set to "1")
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
594IB-1501278-P
Program format of cycle inserted with this function is indicated as follows:
Detailed description
No. Process part Description Program image
(1) Cycle header Block that indicates the cycle starting. Header includes cycle ID (8-digit number) and cycle name.
Used to identify the cycle type at the time of cycle reed- iting.
G180 P1 A_ (cycle name); A: Cycle ID
(2) Arbitrary shape header
The header that indicates the start of the arbitrary shape is output before an arbitrary shape block.
G180 P11;
(3) Arbitrary shape footer
The footer that indicates the end of the arbitrary shape is output at the end of an arbitrary shape block.
G180 P10;
T_;
G00 X_ Z_;
G180 P1 A10201 (CONT-FACE);
S_ M_;
G00 X_ Y_ Z_;
G17;
G12.1;
M8;
G65 P
WHILE[ ] DO_;
G00 X_ Y_ Z_;
G01 Z_ F_;
WHILE[ ] DO_;
F_;
G180 P11;
G01 X_ Y_;
G01 X_ Y_;
G02 X_ Y_ R_;
:
G01 X_ Y_;
G180 P10;
END_;
END_;
G00 Z_;
G13.1;
M9;
G00 Z_;
G180 P0;
G00 Z_;
Processing
(4) Cycle footer
Processing after machining
Move to machining end position
(1) Cycle header
Move to machining start position
(2) Arbitrary shape header
Arbitrary shape block
(3) Arbitrary shape footer
Processing before machining
Cycle
Program being edited on the edit screen
Cycle edit window
Edit the cycle data interactively and output to the program.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
595 IB-1501278-P
(1) The program block output between header and footer differs for each cycle. (2) G180 block does not perform since it is the block to identify the cycle information. The operation is same as the
block which only has EOB (;). The operation will also be the same when specified other than cycle information identification No. designated by format (G180 P99 etc.). When the specifications of interactive cycle insertion are invalid, it will result the program error (P39) at the G180 block.
(3) Since G code of G180 is inserted automatically, manual input is not required.
(4) Cycle footer The footer that indicates the end of the cycle is output at the end of the cycle.
G180 P0;
- Hole position head- er
The header that indicates the start of the hole position is out- put before the block to specify the hole position.
G180 P31;
- Hole position footer The footer that indicates the end of the hole position is out- put after the block to specify the hole position.
G180 P30;
No. Process part Description Program image
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
596IB-1501278-P
15.11.2 Interactive Macro
Interactive macro means a macro program used for interactive cycle insertion. It is stored in the dedicated area. The command format is the same as when an interactive cycle is inserted. Refer to "15.11.1 Interactive Cycle Insertion".
A macro call command during a cycle inserted by this function calls the interactive macro stored in the interactive macro area. You cannot edit the interactive macros which are stored in this area. However, if you set "1" to "#8133 Intrctv macro call", a machining program in the machining program area can be called as a macro program. You can newly create and edit the program because it is in the machining program area. When you want programs to be operated differently from the standard interactive macro, you can edit and call them there.
(*1) When a program with the same name as standard interactive macro exists in the machining program area, the program in the machining program area is called first.
(*2) When a program with the same name as a standard interactive macro does not exist in the machining program area, the program in the interactive macro area is called.
(1) Do not change the name of macro program for macro call command. If you change the name to other than stan- dard interactive macro program name, the program error (P232) occurs. When you change it to the standard interactive macro program name, you can call the interactive macro program which has the name you have changed; however, the cycle cannot be reedited.
(2) Do not add macro call (G65) or subprogram call (M98) during the cycles (G180P1 to G180P0). If you add the macro call other than the standard interactive macro programs, the program error (P232) occurs. When adding with the standard interactive macro program name, you can call the interactive macro you have added; however, the cycle cannot be reedited if you insert a block.
(3) Do not add the "macro interruption command (M96/M97)" during the cycles (G180P1 to G180P0). If you add, the program error (P232) occurs to call the macro in the interactive macro area. Once "1" is set to the parameter "#8133 Intrctv macro call", a macro program or subprogram in the machining program area can be called even during a cycle; however, the cycle cannot be reedited if a block is inserted.
(4) Subprogram and macro program call nesting levels include interactive macros. The maximum nesting level in which a macro program or subprogram can be called depends on your CNC specifications.
(5) For the programs inserted cycles using this function, if modifications that do not conform to the cycle format have been made manually, data may not be read properly at the time of reedit. In that case, even if the menu "Reedit" is pressed in the cycle list window, an error occurs, and the cycle cannot be reedited.
(6) G180 block does not perform anything. Therefore, even if G180 block is added to the program manually, the error does not occur, and it handled as the same operation as the block only EOB (;).
(7) In this function, saving cycles to the program is possible even if cycle data is unset state. The setting values of unset items are output as "0" or "?". If the program output "?" is operated, the program error (P33) occurs at the block which unset data is output.
(8) Only the machining program, which contains the cycle of the type designated in the parameter "#8992 Cycle switch", is operable. If the machining program containing a different type of cycle is operated, a program error (P232) occurs in the block.
Function and purpose
Detailed description
Parame- ters
Program area Program display ONB display Buffer correction
#8133 0 Interactive macro area Hide Hide Disabled 1 Machining program area (*1) Show Show Enabled
Interactive macro area (*2) Hide Hide Disabled
Precautions and restrictions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
597 IB-1501278-P
15.12 Axis Name Extension
The axis name (command axis name) used for giving the absolute/incremental command to NC control axis can be expanded to two characters. When this function is invalid, the command axis name (#1013 axname) is set with one character from A, B, C, U, V, W, X, Y or Z, therefore the number of axes is limited if the increment command axis name is used (*1). When this function is valid, the incremental axis name can be used for all axes by this function. The name-extended axis cannot be designated in the parameter which sets the command axis name such as plane configuration axis I, J or K (*2). Thus, apply this function to a miscellaneous axis which is not used for machining (cutting).
(*1) When two alphabetical characters are used per axis.
(*2) This indicates the axis names of I, J or K set by the parameters "#1026 base_I" to "#1028 base_K".
[Use example]
The settings of these parameters depend on the MTB specifications.
(*3) "H" can be set to "incax".
The following descriptions are the meanings of the terms used in this manual.
In order to use this function, validate this function by the parameter and set the second character of the name-ex- tended axis. These parameters depend on the MTB specifications (parameters "#1266 ext02/bit0" and "#1601 axnameEx").
Function and purpose
# Item 1st axis 2nd axis 3rd axis 4th axis 5th axis 6th axis 7th axis
1013 axname Axis name X Z C X Z X Z 1014 incax Incremental command
axis name U W H (*3) U W U W
1601 axnameEx Axis name extension character
None None None A A B B
Absolute command axis name X Z C XA ZA XB ZB Incremental command axis name U W H UA WA UB WB
Term
Term Meaning
Name-extended axis Axis of which the command axis name is specified with two characters by this function Name-unextended axis
Axis of which the command axis name is specified with a single character (the axis where this function is not used)
Axis name extension character
2nd character of the name-extended axis
Enabling conditions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
598IB-1501278-P
(1) Relationship between parameter setting and command axis name Relationship between parameter related to axis name and command axis name is as follows: When the first character is not set, the program command cannot be issued to that axis. [Parameter configuration example]
(*1) This sets the first character of the axis name.
(*2) This sets the second character of the axis name.
(*3) This depends on the MTB specifications (available when the parameter "#1076 AbsInc" is set to "1").
(2) Program commands to name-extended axis When the axis name of the name-extended axis is "XA", the program command format to the name-extended axis is as follows. When "X" and "XA" exist in the command axis name in the part system, "XA10000" in the com- mand code example below is not interpreted as "X0 A10000" because "XA" is judged preferentially.
Name-extended axis cannot be designated because only one letter can be set to the user parameter which sets axis name shown below. Thus, apply axis name extension to miscellaneous axis which is not used for machining (cut- ting).
(*1) Name-extended axis cannot be designated for parameters "#1026 base_I" to "#1028 base_K" (base axes I, J, and K); however, the NC operates as follows depending on the current setting of base axis I, J, or K:
(a) When the setting value of the base axis I, J, or K corresponds to any name-unextended axis in the part sys- tem, the corresponded axis is identified as base axis I, J, or K.
(b) When the NC is operated with the setting value of the base axis I, J, or K as follows, the program error (P11) occurs. It does not correspond with any of the name-unextended axes in the part system. It corresponds with the first character of any of the name-extended axis.
Detailed description
Program commands for axis name extension
# Item 1st axis 2nd axis 3rd axis 4th axis
1013 axname Axis name (*1) X Z Z Y 1014 incax Incremental command axis name
(*1) U W None V
1601 axnameEx Axis name extension character (*2) A A B None Absolute command axis name XA ZA ZB Y Incremental command axis name (*3) UA WA None V
Type of command Command code example
Numerical command XA10000; Decimal point command XA12.345; Variable command XA[#100];
Relationship with axis name setting parameters
# Item Description
1026 base_I Name of base axis configuring plane (*1) 1027 base_J 1028 base_K 1029 aux_I Name of axis parallel to "base_I" 1030 aux_J Name of axis parallel to "base_J" 1031 aux_K Name of axis parallel to "base_K" 8317 - Name of delivery axis when the right chuck and tailstock barrier is movable. 8621 - Axis name of the plane (horizontal axis) for coordinate rotation control 8622 - Axis name of the plane (vertical axis) for coordinate rotation control
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
599 IB-1501278-P
(c) When the base axis I, J, or K is not set or in the following state, they are set as shown in the table below: It does not correspond with any of the name-unextended axes in the part system. It does not correspond with the first character of any of the name-extended axis.
Because in the environment where the arbitrary axis exchange control is available, only the name of name-unex- tended axis can be designated in the parameters "#12071 adr_abs[1]" to "#12078 adr_abs[8]", other axes cannot be assigned to the command axis name of name-extended axis. However, regardless of the setting of these param- eters, you can designate the axis name of name-extended axis or use the name-extended axis as target axis for axis exchange. (For the name-unextended axis, the axis name cannot be designated without setting these param- eters.) (1) to (3) show the examples of command code in the case of the following axis configuration.
[Example of axis configuration]
(1) Other axes cannot be assigned to the command axis name of name-extended axis.
(2) Name-extended axis can be used as the target axis for axis exchange.
To return the command address to "ZA", carry out the axis exchange return with G141 or G142.
(3) You can command a name of name-extended axis regardless of G140 command.
Parameter of base axis I, J, or K
Which axis "# 1013 axname" is used for the base axes I, J, and K?
L system M system
#1026 base_I 1st axis 1st axis #1027 base_J 3rd axis 2nd axis #1028 base_K 2nd axis 3rd axis
Relationship with arbitrary axis exchange control
$1 1st axis 2nd axis 3rd axis 4th axis
#1013 axname X Z X Z #1022 axname2 X1 Z1 X9 Z9 #1601 axnameEx - - A A Command axis name X Z XA ZA
G140 XA=X1; Program error (P33)
G140 X=X1 Z=Z9; Assign "Z9 axis" to the command address Z.
G140 X=X1 Z=Z1; G00 X10. XA15.; Both X1 and X9 axes move to the commanded coordinate.
Y
Y
Y
N
N
N
(a) (b) (c)
With either #1026, #1027 or #1028 setting
Corresponds with the name- unextended axis in the part system
Corresponds with the first letter of the name-extended axis in the part system
Sets the name-unextended axis as the basic axis I/J/K
The setting can be done, but an error occurs in the actual operation
Sets "axname" of the first to third axis as the basic axis I/J/K
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
600IB-1501278-P
The following list shows the G codes whose functions are available for the name-extended axis among the G codes using an axis name as argument. Also, the operations when the name-extended axis is commanded in the same block or in the G-code mode are shown.
(1) List of G codes that can be used for the name-extended axis (M system)
(1) G10 command in the machining program Data input can be performed to the commands which designate the data input target axis by the axis number; however, it cannot be performed to the commands which designate by the axis name. When the name-extended axis is designated, the program error (P33) occurs. (a) Commands to which the data input of name-extended axis is disabled (when designating by axis number) (b) Commands to which the data input of name-extended axis is disabled (when designating by axis name) (c) Command where input data is not per axis (when the axis is not designated)
(*1) Lathe system
(*2) Machining center system
G codes which can use name-extended axis
G code Group G code function Operation when the name-extended axis is com- manded in the same block or in the G-code mode
G00 1 Positioning Move to the commanded coordinates G01 1 Linear interpolation Move to the commanded coordinates G09 0 Exact stop check Move to the commanded coordinates G28 0 Automatic reference position return Reference position return G30 0 2nd, 3rd and 4th reference position return Return to 2nd, 3rd and 4th reference positions G53 0 Basic machine coordinate system selection Move to the commanded machine coordinates G54 12 Workpiece coordinate system selection 1 Move to the commanded coordinates on G54 G55 12 Workpiece coordinate system selection 2 Move to the commanded coordinates on G55 G56 12 Workpiece coordinate system selection 3 Move to the commanded coordinates on G56 G57 12 Workpiece coordinate system selection 4 Move to the commanded coordinates on G57 G58 12 Workpiece coordinate system selection 5 Move to the commanded coordinates on G58 G59 12 Workpiece coordinate system selection 6 Move to the commanded coordinates on G59 G54.1 12 Extended workpiece coordinate system se-
lection Move to the commanded coordinates on G54.1Pn
G61 13 Exact stop check mode Move to the commanded coordinates G160 0 Torque limitation skip Move to the commanded coordinates
Relationship with other functions
Relationship with data input by program
(a) (b) (c)
G10 L70 Parameters G10 L2 Workpiece offset G10 L100 Tool shape for 3D check G10 L20 Extended workpiece
offset G10 L10 Tool length shape com-
pensation (*2) G10 L10 Tool length shape
compensation (*1) G10 L11 Tool length wear com-
pensation (*2) G10 L11 Tool length wear
compensation (*1) G10 L12 Tool radius shape com-
pensation G10 L14 Current limit G10 L13 Tool radius wear com-
pensation G10 L3 Tool life management G10 L30 Tool life management G10 I_J_K_ Coordinate Rotation Pa-
rameter
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
601 IB-1501278-P
(2) G10 command in input/output file The input/output can be performed for the workpiece offset (G10 L2/L20) and L system tool offset (G10 L10/L11) by G10 command written in the file (WORK.OFS, TOOL.OFS), and the data input/output for the name-extended axis can be performed by G10 command in this case. The example shows the relationship between the NC internal data and the file contents in the case of the follow- ing axis configuration: [Example of axis configuration]
[Workpiece offset file (WORK.OFS)]
[Tool offset file (TOOL.OFS)]
R address: Tool nose radius compensation amount
Q address: Tool nose point P number
(1) When the second axis name parameter "#1022 axname2" is not set, the command axis name is set automatically at the time of power ON.
(2) When judging a character string described in the machining program, and if the result after analyzing the char- acter string from the top is a reserved word (*1) of the user macro, it is identified as reserved word. When the character string is not the reserved word, it is identified as an axis name, but the name of the name-extended axis is identified preferentially. When the axis name and the reserved word are written in a row, enclose the mac- ro command in "[ ]" and do not omit the axis command value "0" so that it does not become an unintentional command. (*1) Reserved word here indicates as follows: Available functions during program mode (such as ABS and SIN) Control statement (such as IF and WHILE) Comparison operator (such as EQ and LT)
$1 1st axis 2nd axis 3rd axis 4th axis
#1013 axname X Z X Z #1022 axname2 X1 Z1 X9 Z9 #1601 axnameEx - - A A Command axis name X Z XA ZA
Precautions
Name-extended axis The axis names after the extension (1st character: "#1013 axname", 2nd char- acter: "#1601 axnameEx") is set.
Name-unextended axis The axis name set in "#1013 axname" is set.
INPUT
OUTPUT $1 G10 L2 P1 X10. Z20. XA30. A40. ;
G54
X1 10. Z1 20. X9 30. Z9 40. WORK.OFS
INPUT
OUTPUT
TOOL.OFS
X1 Z1 X9 Z9 1 1. 2. 3. 4. 2 11. 12. 13. 14.
15 5. 5. 5. 5.
$1 G10 L10 P1 X1.Z2. XA3. ZA4.R0. Q0 ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
602IB-1501278-P
[Case in which the following axis names exist]
(*) When the name of name-extended axis is written following comma ",", the command address with comma is identified preferentially.
(3) In the following cases, the program error (P11) occurs because the axis names are duplicated: When the name "#1013 axname" of name-unextended axis in the part system is duplicated
When "#1076 AbsInc" = "1", the duplication check is performed including the increment command axis name "#1014 incax".
When the name of name-extended axis in the part system (1st letter: "#1013 axname", 2nd letter: "#1601 axnameEx") is duplicated When "#1076 AbsInc" = "1", the duplication check is performed including the increment command axis name (1st character: "#1014 incax", 2nd character: "#1601 axnameEx").
(4) When the name-unextended axis is configured following the name-extended axis in the part system, the sys- tem error (Z23) occurs at the time of power ON.
(*) This is incorrect axis configuration because XA axis is set before Z axis.
(5) You cannot input "#1601 axnameEx" by the parameter input by program (G10 L70). When designated, the program error (P421) occurs.
(6) If the parameter "#1266 ext02/bit0" (Axis name extension valid) is set to "0" (invalid) and the program using the "Name-extended axis" is executed as it is, the machine may operate differently from the original command. For example, the command "XA10.000" for the "Name-extended axis" may be interpreted as "X0 A10.000". To prevent such misinterpretation in commands, it is recommended to use the parameter "#1227 aux11/bit4" as "1" (valid).
Axis names Run command Operation
AB #100 = ABS[#101]; Set to the ABS command of a macro. (This is not regarded as "#100 = AB0 S[#101];".)
AB, XA XA[ABS[#100]]; The ABS command result of a macro is used as the command value of the XA axis.
XAABS[#100]; Same as above (This is not regarded as "XA0 AB0 S[#100];".)
X, XA XABS[#100]; This is regarded as "XA0 B0 S[#100];". (If the B axis does not exist, a pro- gram error (P32) will occur.) When you want to use the ABS command result of a macro as the com- mand value of the X axis, describe "X[ABS[#100]];".
AX ,AX100.; This is regarded as ",A0 X100.;". (*)
$1 Normal axis configuration Abnormal axis configuration (System error (Z23) occurs.)
1st axis 2nd axis 3rd axis 4th axis 1st axis 2nd axis 3rd axis 4th axis
#1013 axname X Z X Z X X Z Z #1601 axnameEx - R A A - A - A Command axis name X Z XA ZA X XA (*) Z ZA
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
603 IB-1501278-P
15.13 Machining Interruption [C80]; G26
Machining interruption is a function which enables interrupt operations in the table below while a program is normally executed. Interruption programs (called "retraction programs") need to be prepared in advance to validate various interruption operations. This function is available only during memory mode operation, but not during MDI operation.
Function and purpose
Interrupt operation Details of operation Purpose
Program-based re- traction
When the retract button is pressed, the program immedi- ately branches to the predetermined retraction program. A safe tool-path that avoids interference can be pro- grammed in the retraction program. On returning from the retraction program, the tool returns to the programmed position called "machining start point", from which the operation can be restarted.
e.g. when machining is tempo- rarily suspended due to events such as when tools break, and then restarted after the issue is solved.
Returns to the machining start point from the status of machining in progress.
MS: Machining start point ME: Machining end point
Emergency stop When an emergency stop occurs during program execu- tion, machining stops in a feed hold status. When the NC is restarted after the cancellation of an emergency stop, a tool returns from the stop position (caused by the emer- gency stop) to the interpolation restart position, and then operation restarts along the original program path.
e.g. when machining is tempo- rary suspended due to such as the emergency stop.
EMG: Emergency stop STOP: Stop position RE: Interpolation restart position
Returns to the interpolation interrupted position from the emergency stop position as shown above, then the inter- polation restarts.
MS ME
EMG
RE
STOP
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
604IB-1501278-P
To perform an interruption operation such as a program-based retraction, add the dedicated commands to the pro- gram in advance.
Program a mark that indicates both the machining start point and machining end point.
Command for the machining start point or the machining end point must be issued alone in a block. If a command other than "N" (sequence No.) is included in the block that has the machining start point or the
machining end point specified, a program error (P33) occurs. After commanding the machining start point, always specify the machining end point. If the machining start point
is commanded while the machining end point remains unspecified, a program error (P727) occurs.
Term
Term Meaning
Machining start point Starting point of a single machining module. The program returns to this block after the retraction program is executed.
Machining end point Ending point of a single machining module, which is paired with the machining start point. Program-based retraction is possible in a section from the machining start point to the machining end point.
Process start point Starting point of machining process by a single tool. Indicates the tool change com- mand block.
Selected point Indicates one of the machining start point, machining end point, and process start point.
Retraction program Program to retract the tool safely during each process. Executed when retraction is started.
Machining interruption program
Program (retraction program) that is started by the interruption operation.
Slide amount Distance from the current machine position to the output position obtained by in- terpolation calculation.
Slide-movement Movement (equivalent to the slide amount) from the current machine position to the output position obtained by the interpolation calculation. This movement is conducted automatically when the program is restarted after an emergency stop.
Slide speed Speed to perform slide-movement operation. This setting depends on the MTB specifications (parameter "#12125 slide-F").
Command format
Machining start point and machining end point
,Qqqqqq; Machining start point
,Q0; Machining end point
,Q For "qqqqq", command the sequence No. of a retraction program. When ",Q0" is specified, it is judged to be the machining end point.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
605 IB-1501278-P
The tool change command is handled as the process start point.
"M06" refers to the miscellaneous function code for the tool change command. The M code of the miscellaneous command for tool change, which is assumed to be the process start point,
depends on the MTB specifications (parameter "#12126 Mcngit_Tch_M").
When the stop code (T03 0320) (stop at the selected point) is issued at the process start point, it indicates that the tool change command has not yet been executed. The tool change command is executed when the auto- matic operation is activated.
Create a retraction program in the same program following the machining program. A single retraction program begins with the sequence No. that matches "qqqqq" (setting value of ",Q" address) of the machining start point.
The retraction program is configured in the standard subprogram format. The G26 (selected point return/tapping retract) command is available in the retraction program. To end the retraction program, command M99. Command M99 alone in a block. If a command other than "N" (sequence No.) is issued in the same block, a
program error (P33) occurs. The retraction programs are required as many programs as the number of the sequence Nos. specified in ",Q".
Process start point
T** M06;
Retraction program
Nqqqqq; Mark that indicates the head of a retraction program. ("qqqqq" indicates the sequence No.)
G26 Z0.; Selected point return command/tapping retract command
:
M99; Retraction program end command
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
606IB-1501278-P
The G26 command returns the axis commanded in the same block to the selected point that was executed previ- ously. (*1) The G26 command is available only in the machining interruption (retraction) program. If the command is issued in a program other than the machining interruption program, a program error (P721) occurs.
The specified axis is returned to the selected point that was executed previously. The specified coordinate position is ignored. In normal circumstances, specify "0". The rotating type rotary axis moves with a shortcut even if the parameter "#8213 Rotation axis type" is set to
"Short-cut invalid" (0). On returning to the selected point, linear interpolation is applied with the feedrate of the F modal value. (*1) If retraction start is performed while the tapping cycle is running, only the first G26 command in the retraction
program is operated as the tapping retract command, not the selected point return command. (The second and subsequent G26 commands are operated as the selected point return command.)
(*1) Do not command a position under point R (*2) (in the hole bottom direction). If commanded, a program error (P730) occurs.
(*2) When point R is not specified in the tapping cycle, the initial point is assumed to be specified.
Pull up the hole drilling axis to the commanded position. The hole drilling axis moves only when retraction start is performed during cutting or dwelling in the tapping cy-
cle. If retraction start is performed in other states, the hole drilling axis does not move. Only the hole drilling axis can be commanded in the same block as the tapping retract command. In addition,
the S code cannot be commanded. When an axis other than the hole drilling axis or the S code is commanded, a program error (P33) occurs.
Do not perform axis movement in the process from the head of the retraction program to the tapping retract command. In addition, when the currently executed tapping cycle is in synchronous tapping mode, do not issue the S command. (If commanded, a program error (P729) occurs.)
G26 (Selected point return/tapping retract)
G26 X0. Y0. Z0.; Selected point return
G26 Zz1.; Tapping retract
Zz1 Commands the pull-up position (*1) with the absolute position or the incremental position from point R (*2). When the hole drilling axis is a diameter axis, command the diameter value even in the incremental command.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
607 IB-1501278-P
In a general machining program, a single machining process consists of one or more machining processes (for ex- ample, multiple hole drilling) by one tool. A machining program consists of such machining processes that are de- scribed in sequence. A machining process begins with the tool change command. This position on the program is referred to as "process start point".
MS: Machining start point ME: Machining end point PS: Process start point
"Operation with single block at selected point" refers to an operation in which the machining stops at the machining start point, machining end point, or process start point. When the "operation mode with single block at selected point" signal is set to ON, the operation with single block at selected point is performed. "Stop at selected point" refers to an operation that the machining stops at the machining start point, machining end point, or process start point. In this case, the stop code is T320. The following types of selected point stop states exist. Various interruption operations are possible in the selected point stop state.
(1) Macro single ON is set during the operation mode with single block at selected point. (The machining stops at the macro block during single-block operation.)
Detailed description
Machining start point and machining end point, Process end point
Machining process 1
Machining process 2
End of machining
Operation with single block at selected point
Block where "Stop at selected point" is applied Available interruption operation
,Qqqqqq; - ,Q0; Program-based retraction M06; (M system) T****; (L system)
-
T01
T02
M30;
PS1
MS1 ME1
ME3 MS3
PS2
MS1 ME1
ME3 MS3
Drilling 1
Drilling 2
Drilling 3
:
:
Tapping 1
Tapping 2
Tapping 3
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
608IB-1501278-P
While "Stop at selected point" is active, the machining will stop before executing the block to be stopped at. At this time, a signal indicating each stop state is output. ("Stopping at machining start point", "Stopping at machining end point", or "Stopping at process start point" signal) When cycle start is restarted from this stop state, machining is restarted from a command in the stopped block.
Program-based retraction is available only when the "retraction executable" signal is set to ON (*1). When the "re- traction start" signal is set to ON while the "retraction executable" signal is ON, the program branches immediately to the sequence No. indicated by the address Q (the head of the retraction program) that is commanded at the ma- chining start point.
(*1) The operation (the condition to be "ON", etc.) of the "retraction executable" signal or "retraction start" signal de- pends on the MTB specifications.
For the retraction program, describe a program to retract the tool safely during each process. In the retraction program, the G26 command can be used to return the commanded axis to the machining start point. In addition, if retraction start is performed while the tapping cycle is running, the G26 command operates as a tap- ping retract command to pull up the hole drilling axis to the specified position. The retraction program ends with "M99;" in the same way as for a normal subprogram. In this case, the axis that is not returned to the machining start point automatically returns to the machining start point.
The return to the machining start point depends on the command type: - For the selected point return command (G26), linear interpolation is applied. - For the retraction program end command (M99), the travel varies depending on the modal of the currently execut- ed G code (group 1). (When G00 is commanded, the axis travels in rapid traverse mode; otherwise, it travels in linear interpolation mode.) In addition, when G26 is operated as the tapping retract command, the hole drilling axis travels in linear interpolation mode. However, when tapping retract is performed while synchronous tapping cycle is running, the spindle rotates synchronously with the movement of the hole drilling axis.
When the retraction program ends, the modal is restored to the state that is set at the machining start point. Each axis stops at the machining start point block after returned to the machining start point. If cycle start is performed in this block stop state, the commanded rotation speed and commanded signal (forward rotation start/reverse rotation start, etc.) of the spindle are restored to the state that was set at the machining start point.
(1) When reset is performed while the retraction program is running, the currently executed program ends. In addi- tion, if the "reset 2" signal is input, the program is executed from the machining start point at the next cycle start operation.
(2) If an MDI interruption is conducted, the retraction executable state is released. An MDI interruption can not be conducted while the retraction program is running.
(3) When retraction start is performed while the miscellaneous function is running (in the state in which the corre- sponding strobe signal is set to ON and waiting the FIN signal), the strobe signal is set to OFF, and also the FIN signal wait state is canceled.
(4) Tool radius compensation is canceled when the retraction program is started. Command the tool radius compensation after the machining start point, and cancel it before the machining end point.
(5) When the retraction program is executed, the program nesting level is incremented by one in the same way as subprogram calling. Therefore, the retraction program cannot be started if the nesting level has reached the max- imum.
(6) The operation at the start of the retraction program conforms to that at the start of macro interruption. However, the interruption method is fixed to Type 1 (operation to immediately stop the currently executed block and start the retraction program).
Stop at selected point
Program-based retraction
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
609 IB-1501278-P
(7) To return each modal to the state that was set at the machining start point when the retraction program is ended (M99 is executed), the machining operates as shown below. [G96 mode at machining start point]
The spindle stops with "S0" just before the retraction program ends.
[G97 mode at machining start point]
When the following multiple conditions are specified together, the rotation speed may increase. The constant surface speed control axis is near the center of the spindle. The G96 modal and surface speed were recovered when the retraction program was ended. Therefore, retract the constant surface speed control axis to the position at which the following conditions are satisfied before the retraction program is ended. Position sufficiently far away from the center of the spindle Position at which the axis does not pass near the center of the spindle when it moves to the machining
start point (8) In the retraction executable state, control is moved to the retraction program by retraction start even when the
block of timing synchronization between part systems is executed. When the machining of another part system executes a block late, the block is not completed. Do not perform timing synchronization operation between part systems in the retraction executable section (from the machining start point to the machining end point).
(9) Do not perform the following operations related to the coordinate system in the retraction executable section (from the machining start point to the machining end point) and in the retraction program. Local coordinate system setting Change of external workpiece coordinate system offset Coordinate system setting Workpiece coordinate system preset
When the parameter "#11020 Mcngit_Spec/bit0" is set to "1" (Enable), operation will not be ended even if emergen- cy stop occurs during automatic operation, which causes the machining to be placed in the automatic operation pause state (stop code (T02 0200)). After an emergency stop is released, operation can be restarted by the auto- matic operation start. (This parameter setting depends on the MTB specifications.) When operation is restarted, slide-movement (moved with rapid traverse to the interruption point obtained by the interpolation calculation) and spindle state recovery is performed, and then the interrupted block operation (interpo- lation) is restarted. The travel speed to the interruption point depends on the MTB specifications (parameter "#12125 slide-F"). For details on the spindle recovery, refer to the "PLC Interface Manual".
(1) The interruption point obtained by the interpolation calculation precedes the actual machine position; therefore, the restart position will be placed before the emergency stop position.
(2) After an emergency stop occurred during MDI operation, the operation can be restarted; however, slide-move- ment and spindle state recovery are not performed at restart.
(3) Operation can also be restarted while the machining interruption program is running. To restart the operation, use the start signal to suit the currently executed machining interruption program. In addition, while the retraction program is running, slide-movement is not performed even when there is a slide amount (difference between the interruption position obtained by the interpolation calculation and the actual ma- chine position). However, the slide amount is compensated for the axis moved by G26 (selected point return/ tapping retract command) or M99 (retraction program end command), or the axis with the absolute position spec- ified. (The slide amount is added to the travel amount required to the end point.)
(4) Slide-movement is performed not only after an emergency stop is released but also when the manual interruption amount is provided when the automatic operation is restarted. The manual interruption amount can be viewed on the operation screen or drive monitor screen.
(5) If the automatic operation pause occurs by Door open I, slide-movement and spindle state recovery are not per- formed even when Door open I is released.
(6) When you want to use the C axis mode of the spindle position control (spindle/C axis) function, the parameter "#11020/bit0" must be set to "0" (Disable). (This parameter setting depends on the MTB specifications.)
Emergency stop
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
610IB-1501278-P
This example shows program-based retraction (drilling) at two locations using the drill tool.
(1), (6): Positioning command to the drilling position.
(2), (7): Indicates the machining start point just before drilling.
(5), (10): Indicates the machining end point after drilling.
The "retraction executable" signal is set to ON and program-based retraction can be executed in the sections be- tween (3) and (5) and between (8) and (10).
[During linear interpolation] EMG: Emergency stop RUN: Coasting after an emergency stop STOP: Stop position SLIDE: Slide position RE: Interpolation restart position E: Program end point
[During circular interpolation]
Program example
Drilling
(1) G00 G91 X100. Y50.; (2) ,Q1000; (3) G01 Z-165.2 F600; Retraction executable
section(4) Z165.2 F2000; (5) ,Q0; (6) G00 X100. Y50.; (7) ,Q1000; (8) G01 Z-165.2 F600; Retraction executable
section(9) Z165.2 F2000; (10) ,Q0; M30; N1000 G26 Z0.; Retraction program
M99; Retraction executable section
EMG
RE
E
STOP SLIDE
RUN
RUN
SLIDE
STOP EMG
RE
E
(1) (2) (5)
(3) (4)
(6) (7) (10
(8) (9)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
611 IB-1501278-P
Column A: Case to start retraction while the related function is running
Column B: Case to execute the related function during retraction
Column C: Case that emergency stop occurs while the related function is running, and that operation is restarted after an emergency stop is released.
: Can be combined with the related function.
: Cannot be combined with the related function. Do not use the functions, which cannot be combined (indicated as "x") with the retraction start operation, in the section from the machining start point to the machining end point.
-: Not related.
: It is not impossible to create this combination; however, machining cannot be continued even if specified.
Functions not described in this table cannot be combined (same as "x") as a rule.
Relationship with other functions
All functions
Related function A B C
Positioning/Interpolation Positioning Unidirectional positioning Linear interpolation Circular interpolation Helical interpolation Spiral/conical interpolation Cylindrical interpolation Polar coordinate interpolation Milling interpolation
Curve interpolation Involute Interpolation Exponential interpolation Spline interpolation NURBS interpolation 3-dimensional circular interpolation
Speed Feed per minute - Feed per revolution - Inverse time feed - F1-digit feed - Manual speed command - Rapid traverse override - Cutting feed override - 2nd cutting feed override - Override cancel -
Acceleration/Deceleration Automatic acceleration/deceleration after Interpolation - Rapid traverse constant-gradient acceleration/deceler- ation
-
Rapid traverse constant-gradient multi-step accelera- tion/deceleration
-
Thread cutting Thread cutting
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
612IB-1501278-P
Variable lead thread cutting Synchronous tapping cycle Chamfering - High-speed synchronous tapping
Spindle, tool, miscellaneous function Spindle control Constant surface speed Multiple-spindle control I Multiple-spindle control II Spindle orientation Spindle position control (Spindle/C axis control) Spindle synchronization T function (*1) - Miscellaneous functions (*1) - 2nd miscellaneous functions (*1) -
Tool compensation Tool length offset - Tool radius compensation - 3-dimensional tool radius compensation - Tool nose radius compensation (G40/41/42) -
Operation support functions Program restart - - -
Program support functions Subprogram control - Scaling Macro call - Macro interruption - Fixed cycle for drilling Special fixed cycle Fixed cycle for turning machining Compound type fixed cycle for turning machining Mirror image Coordinate rotation by program 3-dimensional coordinate conversion Corner chamfering/Corner R Linear angle command Geometric command Polar coordinate command Chopping - Normal line control Circular cut Timing synchronization between part systems Start point designation synchronization Mixed control (Cross axis control) - Control axis synchronization between part systems Balance cut Common memory for part systems - 2-part system simultaneous thread cutting Multi-part system program management - Machining modal -
Related function A B C
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
613 IB-1501278-P
(*1) If retraction start is executed while a miscellaneous function is running (when the corresponding strobe signal is set to ON and waiting the FIN signal), the strobe signal is set to OFF, and the FIN signal wait state is canceled.
Automatic corner override - - Deceleration check - - High-speed machining mode High-speed high-accuracy control I (G5.1Q1) High-speed high-accuracy control II (G5P10000) High-accuracy control (G61.1/G08) High-accuracy spline interpolation 1 (G61.2) High-accuracy spline interpolation 2 (G61.3) SSS Control
Automation support functions Skip Automatic tool length measurement
Safety and maintenance Emergency stop - - Stored stroke limit - - Stroke check before travel - - Chuck barrier/tailstock barrier check - - External deceleration -
Machine support functions Synchronous control Inclined axis control
Related function A B C
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
614IB-1501278-P
To perform retraction start while tapping cycle, pecking tapping cycle, or deep-hole tapping cycle is running, execute the tapping retract command (G26) to pull up the tool. In the synchronous tapping cycle, if tapping retract is performed, the spindle rotates in the direction opposite to the cutting work synchronously with the movement of the hole drilling axis. In the asynchronous tapping cycle, the spin- dle does not rotate even if the tapping retract is executed. Therefore, issue the spindle rotation command before the tapping retract command as necessary. The below table shows the fixed cycles in which tapping retract is possible.
(1) When retraction is performed while the tapping cycle is running, only the G26 first commanded in the retraction program operates as the tapping retract command. The subsequently issued G26 commands operate as the se- lected point return command.
(2) The hole drilling axis is pulled up by the tapping retract command only when retraction start is performed during cutting or dwelling in the tapping cycle. If retraction start is performed during non-cutting in the tapping cycle, the hole drilling axis does not move with the tapping retract command.
(3) In the retraction program, the axis movement cannot be performed before the tapping retract command. In addition, when retraction start is performed during the synchronous tapping cycle, the S command cannot be executed. (If commanded, a program error (P729) occurs.)
(4) In the retraction program for tapping cycle, always execute the tapping retract commands (G26 and hole drilling axis commands). If the retraction program is ended (the M99 block is executed) while the tapping retract com- mand remains unexecuted, a program error (P729) occurs.
(5) The spindle rotation speed for tapping retract is the same as for cutting. The ",S" command and the parameter "#1172 tapovr" (MTB specifications) are invalid.
[Example to apply program-based retraction to the asynchronous tapping cycle]
(*1) In the synchronous tapping cycle, specify the spindle rotation speed with the synchronous tapping command block.
(*2) In the synchronous tapping cycle, the spindle reverse or spindle stop block is not required.
(*3) When tapping retract is performed during non-cutting (while the axis is moving from the initial point to point R), the hole drilling axis does not move.
Tapping cycle
Tapping cycle currently being executed
G84 (Forward tapping cycle) G74 (Reverse tapping cycle)
G00 G90 X100. Y50. Z0.; ,Q1000; Selected point (Machining start point) S1000 M03; (*1) G84 R-20. Z-100. F800 P500 ,R0; G80; M05; ,Q0; : M30; N1000 M04; Reverses the spindle to perform asynchronous tapping retract. (*2) N1010 G26 G91 Z5.; Pulls up the hole drilling axis to "5" ("-15" for the absolute command) as
the incremental command from point R. (*3) N1020 M05; Spindle stop (*2) N1030 G26 X0. Y0. Z0. F1000; The second and subsequent G26 commands operate as the selected-
point return command. M99;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
615 IB-1501278-P
When performing tapping successively at multiple hole drilling positions, specify the machining start point and ma- chining end point at each hole drilling position. If the machining start point and machining end point are collectively specified for one hole drilling position, tapping is performed from the first step each time retraction start is executed. Therefore, tapping is also performed at the hole drilling position at which machining has already ended.
[Example to apply program-based retraction to the cycle with continuous tapping processes] G00 G90 X0. Y0. Z0.; ,Q1000; G84 Z-100. F1 S1000 ,R1; (*3) ,Q0; (*2) ,Q1000; (*2) X10.; ,Q0; (*2) ,Q1000; (*2) X20.; (*1) ,Q0; G80; M30; N1000; : M99;
(*1) If program-based retraction is performed during tapping at this hole drilling position, tapping is restarted at this hole drilling position after the retraction program was ended.
(*2)(*3) When both commands ",Q1000" and ",Q0" are not issued for each command of hole drilling position, the block to be executed will return to the hole drilling position indicated with (*3) after the retraction program ends.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
616IB-1501278-P
: Enabled, : Disabled
Combinations of G commands while retraction is executed
G code Group Operation G code Group Operation
G00 01 G30.1 00 G01 01 G30.2 00 G02 01 G30.3 00 G03 01 G30.4 00 G02.1 01 G30.5 00 G03.1 01 G30.6 00 G02.3 01 G31 00 G03.3 01 G31.1 00 G02.4 01 G31.2 00 G03.4 01 G31.3 00 G04 00 G33 01 G05 00 G34 00 G05.1 00 G35 00 G06.2 01 G36 00 G07 00 G37 00 G07.1 G107
21 G37.1 00 G38 00
G08 00 G39 00 G09 00 G40 07 G10 00 G41 07 G11 00 G42 07 G12 00 G40.1 15 G13 00 G41.1 15 G12.1 G112
21 G42.1 15 G43 08
G13.1 G113
21 G44 08 G43.1 08
G15 18 G43.4 08 G16 18 G43.5 08 G17 02 G45 00 G18 02 G46 00 G19 02 G47 00 G20 06 G48 00 G21 06 G49 08 G22 04 G50 11 G23 04 G51 11 G27 00 G50.1 19 G28 00 G51.1 19 G29 00 G52 00 G30 00 G53 00
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
617 IB-1501278-P
(1) If emergency stop occurs during synchronous control, a synchronization error between the reference axis and synchronized axis is not corrected in the slide-movement process after an emergency stop is released. To use the synchronous control function, the "automatic correction of synchronization error at servo-ON" must be en- abled. (This setting depends on the MTB specifications (parameter "#1281 ext17/bit3").)
(2) The fixed-cycle modal calling is not performed in the machining interruption program. In addition, the fixed cycle (G code group 9) cannot be commanded. (If commanded, a program error (P728) occurs.)
(3) The macro modal calling is not performed in the machining interruption program. In addition, the macro modal call (G code group 14) cannot be commanded. (If commanded, a program error (P728) occurs.)
G code Group Operation G code Group Operation
G54 12 G75 09 G55 12 G76 09 G56 12 G77 09 G57 12 G78 09 G58 12 G79 09 G59 12 G80 09 G54.1 12 G81 09 G60 00 G82 09 G61 13 G83 09 G61.1 13 G84 09 G61.2 13 G85 09 G62 13 G86 09 G63 13 G87 09 G63.1 13 G88 09 G63.2 13 G89 09 G64 13 G90 03 G65 00 G91 03 G66 14 G92 00 G66.1 14 G92.1 00 G67 14 G93 05 G68 16 G94 05 G69 16 G95 05 G70 09 G96 17 G71 09 G97 17 G72 09 G98 10 G73 09 G99 10 G74 09 G100 - G225 00
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
15 Program Support Functions
618IB-1501278-P
16
619 IB-1501278-P
Multi-part System Control
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
620IB-1501278-P
16Multi-part System Control 16.1 Timing Synchronization Operation
16.1.1 Timing Synchronization Operation (! code) !n (!m ...) L
The multi-axis, multi-part system complex control CNC system can simultaneously run multiple machining programs independently. The synchronization-between-part systems function is used in cases when, at some particular point during operation, the operations of 1st and 2nd part systems are to be synchronized or in cases when the operation of only one part system is required. When timing synchronization is executed in the 1st part system ($1) and the 2nd part system ($2), operations will be as follows.
CAUTION
When programming a multi-part system, carefully observe the movements caused by other part systems' pro-
grams.
Function and purpose
Simultaneous and independent operation
Timing synchronization operation
Simultaneous and independent operation
Timing synchronization operation
2nd part system operation only 1st part system waiting
Timing synchronization operation
Simultaneous and independent operation
Command format
!n (!m ...) L_ ;
!n, !m, ... Timing synchronization operation (!) and part system No. (n:1 - number of part system that can be used) Follows the settings of the parameter "#19419 Timing sync system" if part system num- ber is omitted.
L Timing Synchronization Operation No. 0 to 9999
% %
$1 $2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
621 IB-1501278-P
(1) Timing synchronization between part systems during automatic operation If !n L__ is commanded from a part system (i), operation of the part system i program will wait until !i L_ is com- manded from the part system n program. When !i L_ is commanded, the programs for the two part systems will start simultaneously. Timing synchronization between 2 part systems
(2) The timing synchronization operation command is normally issued alone in a block. However, if a movement command or M, S or T command is issued in the same block, whether to synchronize after the movement com- mand or M, S or T command or to execute the movement command or M, S or T command after synchronization will depend on the MTB specifications (#1093 Wmvfin).
#1093 Wmvfin 0 : Wait before executing movement command. 1 : Wait after executing movement command.
(3) If there is no movement command in the same block as the timing synchronization operation, when the next block movement starts, synchronization may not be secured between the part systems. To synchronize the part sys- tems when movement starts after waiting, issue the movement command in the same block as the timing syn- chronization operation.
(4) The L command is the timing synchronization identification No. The same Nos. are waited but when they are omitted, the Nos. are handled as L0.
(5) "SYN" will appear in the operation status section during timing synchronization operation. The timing synchroni- zation operation signal will be output to the PLC I/F.
(6) In a timing synchronization operation, other part system to be waited for is specified but the own part system can be specified with the other part system.
(7) The timing synchronization operation of a specific part system can be ignored depending on the MTB specifica- tions. Operation will be determined by the combination of the timing synchronization operation ignore signal and pa- rameter "#1279 ext15/bit0". For setting combination, refer to "Time synchronization when timing synchronization ignore is set". For the specifications of the machine you are using, see the instructions issued by the MTB.
Detailed description
!nL1 ;
!iL1;
Pi1 Pn1
Pi2 Pn2
Pi1 Pi2
Pn1 Pn2
$i
$n
$i $n
waiting...
Simultaneously start
Timing synchronization
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
622IB-1501278-P
(1) When the M code can be used, both the M code and ! code can be used. (2) While the timing synchronization operation M code is valid, if one part system is standing by with an M code, an
alarm will occur if there is a ! code timing synchronization operation command in the other part system. (3) While the timing synchronization operation M code is valid, if one part system is standing by with a ! code, an
alarm will occur if there is an M code timing synchronization operation command in the other part system. (4) When macro interruption is carried out in a part system waiting, the part system can stop while waiting even if
the conditions for time synchronization are met. In this case, you will be able to continue the program, ignoring the timing synchronization with timing synchronization operation ignore signal. For details, contact the MTB.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
623 IB-1501278-P
16.1.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115
The part system can wait for the other part system to reach the start point before starting itself. The start point can be set in the middle of a block.
Function and purpose
Command format
!n L__ G115 X__ Y__ Z__ ;
!n Timing synchronization operation (!) and part system No. (n:1 - number of part sys- tem that can be used) Part systems follow the settings of the parameter "#19419 Timing sync system" if the number is omitted.
L Timing Synchronization Operation No. 0 to 9999 (It will be regarded as "L0" when omitted.)
G115 G command X Y Z Start point
(Command by axis and workpiece coordinate value)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
624IB-1501278-P
(1)Designate the start point using the workpiece coordinates of the other part system (ex. $2).
(2)The start point check is executed only for the axis designated by G115. (Example) !L2 G115 X100. ; Once the other part system reaches X100, the own part system (ex. $1) will start. The other axes are not checked.
(3)The other part system starts first when timing synchronization operation is executed.
(4)The own part system waits for the other part system to move and reach the designated start point, and then starts.
(5) When the start point designated by G115 is not on the next block movement path of the other part system, the own part system starts once all the designated axis of the other part system has reach the designated start point.
(6) After waiting, if the start point cannot be obtained with movement command of the other timing synchronization block, the operations depend on the MTB specifications (parameter "#1229 set01/bit5").
(a) When the parameter is ON Wait till the own part system reaches the start point by moving after the next block.
(b) When the parameter is OFF When the next block finishes moving, the own part system will start.
Detailed description
Timing synchronization Designated start point
Movement Designated start point Actual start point
$1
$2 !1
!1
$1
$2
!2 G115
!2 G115
G00 X...
G00 X...
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
625 IB-1501278-P
(7)The timing synchronization status continues when the G115 command has been duplicated between part sys- tems. (Operations will not restart.)
(8) The single block stop function does not apply for the G115 block.
(9) A program error (P32) will occur if an address other than an axis is designated in G115 command block.
(10) In the timing synchronization operation, other part system to be waited for is specified but the own part system can be specified with the other part system.
(11) The timing synchronization operation of a specific part system can be ignored depending on the MTB specifi- cations. Operation will be determined by the combination of the timing synchronization operation ignore signal (PLC signal) and parameter "#1279 ext15/bit0". For setting combination, refer to "Time synchronization when timing synchronization ignore is set". For the specifications of the machine you are using, see the instructions issued by the MTB.
(1) Parameter "#1093 Wmvfin" that selects the timing of the timing synchronization operation and commands on the same block does not work for the start point command block (G115/G116). After synchronization. the start point check will be executed by G115/G116.
(2) Be careful about the timing when interrupting during the time synchronization of G115/G116. For example, as- sume interruption with the macro interrupt type 1 while a part system is waiting for time synchronization with G116. In this case, if there is a movement command or MSTB command in the interrupt program, the program will continue after the interrupt program completes without waiting for the start point.
(3)The L command is the timing synchronization identification No. The same Nos. are waited but when they are omit- ted, the Nos. are handled as L0.
Timing synchronizing
Precautions
$1 !2 G115
!1 G115$2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
626IB-1501278-P
16.1.3 Timing Synchronization Operation with Start Point Designated (Type 2) ; G116
The own part system can make the other part system to wait until it reaches the start point. The start point can be set in the middle of a block.
Function and purpose
Command format
!n L__ G116 X__ Y__ Z__ ;
!n Timing synchronization operation (!) and part system No. (n:1 - number of part sys- tem that can be used) Part systems follow the settings of the parameter "#19419 Timing sync system" if the number is omitted.
L Timing Synchronization Operation No. 0 to 9999 (It will be regarded as "L0" when omitted.)
G116 G command X Y Z Start point
(Command by axis and workpiece coordinate value)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
627 IB-1501278-P
(1)Designate the start point using the workpiece coordinates of the own part system (ex. $1).
(2)The start point check is executed only for the axis designated by G116. (Example) !L1 G116 X100. ; Once the own part system reaches X100, the other part system (ex. $2) will start. The other axes are not checked.
(3)The own part system starts first when timing synchronization operation is executed.
(4)The other part system waits for the own part system to move and reach the designated start point, and then starts.
(5) When the start point designated by G116 is not on the next block movement path of own part system, the other part system starts once all the designated axes of the own part system has reach the designated start point.
(6) If the start point cannot be obtained with the movement of the own part system to the next block, the operations depend on the MTB specifications (parameter "#1229 set01/bit5").
(a) When the parameter is ON The own part system will have a program error (P511) before moving.
(b) When the parameter is OFF When the next block finishes moving, the other part system will start.
(7)The timing synchronization status continues when the G116 command has been duplicated between part sys- tems. (Operations will not restart.)
Detailed description
Timing synchronization Designated start point
Movement Designated start point Actual start point
Timing synchronizing
$1
$2
$1
$2
!2 G116 G00 X...
G00 X...
!1
!1
!2 G116
$1 !2 G116
!1 G116$2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
628IB-1501278-P
(8) The single block stop function does not apply for the G116 block.
(9) A program error (P32) will occur if an address other than an axis is designated in G116 command block.
(10) In the timing synchronization operation, other part system to be waited for is specified but the own part system can be specified with the other part system.
(11) The timing synchronization operation of a specific part system can be ignored depending on the MTB specifi- cations. Operation will be determined by the combination of the timing synchronization operation ignore signal (PLC signal) and parameter "#1279 ext15/bit0". For setting combination, refer to "Time synchronization when timing synchronization ignore is set". For the specifications of the machine you are using, see the instructions issued by the MTB.
Refer to "Start point designation timing synchronization (Type 1) ; G115".
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
629 IB-1501278-P
16.1.4 Timing Synchronization Operation Function Using M codes ; M***
The timing synchronization operation function between part systems is conventionally commanded with the "!" code, but by using this function, the part systems can be waited with the M code commanded in the machining program. If the timing synchronization operation M code is commanded in either part system during automatic operation, the system will wait for the same M code to be commanded in the other part system before executing the next block. The timing synchronization operation M code is used to control the timing synchronization operation between the 1st part system and 2nd part system. Whether the timing synchronization operation M code can be used depends on the MTB specifications.
M code used for timing synchronization depends on the MTB specifications (parameter "#1310 WtMmin)", "#1311 WtMmax").
Function and purpose
Command format
M*** ;
*** Timing synchronization operation M code
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
630IB-1501278-P
(1) When the timing synchronization operation M code is commanded in the machining program, the two part sys- tems will be waited and operation will start in the commanded block. If the timing synchronization operation M code is commanded in either part system during automatic operation, the system will wait for the same M code to be commanded in the other part system before executing the next block.
(2) When the timing synchronization operation M code has been commanded in one part system, and the part sys- tem is standing by for waiting, an alarm will occur if a different M code is commanded in the other part system.
Detailed description
Simultaneous and independent operation on part system 1 and 2 Timing synchronization
In simultaneous and independent operation
M101 Waiting As M101 is commanded in part system 1, part sys- tem 2 starts operation.
M102 Waiting
As M102 is commanded in part system 2, part sys- tem 1 and 2 start operation.independently. Simultaneous and independent operation
M102 Waiting
M101 Waiting
Simultaneous and independent op- eration
M100 Waiting Alarm (Operation stops)
P11
$1
P12
P14
M100 ;
M101 ; M102 ;
M30 ;
P21
$2
P22
P23
P24
M100 ;
M101 ;
M102 ;
M30 ;
P11 P12 P14
P21 P22 P24P23
$1
$2
$1
M100 ;
M101 ;
P11 P21
P22P12
$2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
631 IB-1501278-P
(3) The part systems are waited with the M code following the parameters below. These settings depend on the MTB specifications. Refer to these settings. For details, refer to the specifications of your machine. (a) M code range designation parameter (M code minimum value <= M code <= M code maximum value)
This function is invalid if either parameter is set to "0". The timing synchronization operation M code cannot be used if the M code maximum value is smaller than the minimum value. When the timing synchronization operation M code is valid, both the M code and ! code can be used for timing synchronization operation.
(b) Timing synchronization operation method parameters
Depending on the timing synchronization operation method selection parameter and timing synchronization operation ignore signal combination, the timing synchronization operation will be determined by the param- eters, regardless of the command format ("!" code and M code). This parameter requires the CNC to be turned OFF after the settings. Turn the power OFF and ON to enable the parameter settings.
Refer to "Timing Synchronization Operation (! code);!n (!m ...) L".
# Item Details Setting range
1310 WtMmin Timing syn- chronization M code ABS. MIN.
The minimum value of the M code. If the setting value is "0", the timing synchronization operation M code will be ignored.
0, 100 ~ 99999999
1311 WtMmax Timing syn- chronization M code ABS. MAX.
The maximum value of the M code. If the setting value is "0", the timing synchronization operation M code will be ignored.
0, 100 ~ 99999999
# Item Details Setting range
1279 (PR)
ext15 (bit0)
Method for timing syn- chronization operation be- tween part systems
Select an operation for timing synchronization opera- tion between part systems. 0: If one of the part systems is not in automatic opera- tion, ignore the timing synchronization operation and execute the next block. 1: Operate according to the timing synchronization op- eration ignore signal. If the timing synchronization operation ignore signal is "1", the timing synchronization operation will be ig- nored. If "0", the part systems will be waited.
0 / 1
# Item Details Setting range
1093 Wmvfin Method for timing syn- chronization operation be- tween part systems
Parameter to designate the timing synchronization op- eration between part systems method when using multi-part systems. When there is a movement command in the timing synchronization operation (!, M) block: 0 : Wait before executing movement command. 1 : Wait after executing movement command.
0 / 1
Relation with other functions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
632IB-1501278-P
For precautions for time synchronization, also refer to "Timing Synchronization (!code);!n (!m ...) L"
(1) During timing synchronization operation with the M code, always command the M code alone in a block. (2) While standing by after commanding the timing synchronization operation M code in one part system, an alarm
will occur if a different M code is commanded in the other part system. Operation will stop in both part systems. (3) The timing synchronization operation (! code, M code) in the machining program can be ignored with the timing
synchronization operation ignore signal. (This depends on the MTB specifications. ) Operation with a single part system is possible without deleting the timing synchronization operation (! code, M code) in the machining pro- gram.
(4) Unlike other M codes, the timing synchronization operation M code does not output code signals and strobe sig- nals.
(5) When the M code can be used, both the M code and ! code can be used. (6) While the timing synchronization operation M code is valid, if one part system is standing by with an M code, an
alarm will occur if there is a ! code timing synchronization operation command in the other part system. (7) While the timing synchronization operation M code is valid, if one part system is standing by with a ! code, an
alarm will occur if there is an M code timing synchronization operation command in the other part system. (8) If there is a timing synchronization operation with M code after the 3rd part system, an alarm will occur. (9) The G115 and G116 commands cannot be used when waiting with the M code. (10) If the M code command Nos. are overlapped, the order of priority will be M code macro, M command synchro-
nous tapping, timing synchronization operation M code and normal M code. (11) "SYN" will appear in the operation status section during timing synchronization operation. (12) When the timing synchronization operation between part systems and single block operation are used simulta-
neously, the next block stands by until the cycle start signal is input in the part system in which the single block mode is ON. Therefore, the operation may stop at the block without the timing synchronization operation code of the part system in which the single block is OFF, where it is not supposed to stop initially.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
633 IB-1501278-P
16.1.5 Timing Synchronization When Timing Synchronization Ignore Is Set
Turning on the timing synchronization operation ignore signal makes it possible to ignore the timing synchronization operation of that part system. With a 2-part system, if the timing synchronization operation ignore signal of the other part system is ON, timing synchronization is not executed. In the following section, a 3-part system is used as an example to make it easier to understand the functions.
This signal is also used in the following functions.
Timing synchronization (! code, M code) Start point timing synchronization (G115, G116) Balance cut (G15) Lathe system only
(1) For sub part system control function, refer to "16.3 Sub Part System Control".
The following operation diagram gives an example of ! code.
(1) A case that "Ignores the timing synchronization with a part system not in automatic operation"
Function and purpose
Timing synchronization operation ignore signal (PLC signal)
OFF ON
Parameter (#1279 ext15/bit0)
0 (1) Ignores the timing synchronization with a part system not in automatic operation 1 (2) Does not ignore the timing synchroniza-
tion regardless of whether or not a part sys- tem is in automatic operation (the timing synchronization is executed until the condi- tions for timing synchronization are estab- lished.)
(3) Ignores the timing synchronization re- gardless of whether or not a part system is in automatic operation (ignores the timing synchronization command for the part sys- tem with the timing synchronization ignore signal ON and the timing synchronization operation for that part system)
Note
!n !m L _ ;
$i
$n
Pi1
Pi2
Pi1 Pi2
Pm1
Pm2
!i !n L _ ;
$m Pm1 Pm2
$i $n $m
waiting...
Start simultaneously
Ignore timing synchronization
Simultaneously start after timing synchronization block
(Not in automatic operation)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
634IB-1501278-P
(2) A case that "Does not ignore the timing synchronization regardless of whether or not in automatic operation"
A: When timing synchronization operation between part systems (parameter "#1279 ext15/bit0" = 1), the timing synchronization status continues until the conditions for timing synchronization are established.
B: Part system n is automatically started. If the conditions for timing synchronization are established, the next block will start.
!n !m L 1 ;
Pi1
Pn1
Pi2 Pn2
Pi1 Pi2
Pn1 Pn2
Pm1
Pm2
!i !m L 1 ;
!i !n L 1 ;
!n !m L 1 ;
Pi1 Pm1
!i !n L 1 ;
Pm1
A B
Pm2
$i $n $m
$i $n $m
$i
$n
$m
waiting...
waiting...
Start the $n program.
Timing synchronization Timing synchronization
Timing synchronization
Necessarily conduct timing synchronization
(Automatic start)
Automatic start
Simultaneously start after timing synchronization
block
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
635 IB-1501278-P
(3) A case that "Ignores the timing synchronization regardless of whether or not in automatic operation"
!n !m L 1 ;
!i !n L 1 ;
!i !m L1 ;
!n !m
!i !m
!i !n
Pi1
Pi2 Pn2
Pn1
Pi1 Pi2
Pm1
Pm2
Pm1
Pn1 Pn2
$i $n $m
$i
$n
$m
waiting...
Timing synchronization
Ignore timing synchronization
Timing synchronization operation ignore signal ON
$i and $n start simultaneously in the next block after timing synchronization.
$m timing synchronization
ignore signal Part system m is in the timing synchronization ignore state, so timing synchronization is not conducted.
Part system m does not conduct timing synchronization.
Ignore timing synchronization with part system m.
Timing synchronization
Ignore timing synchronization
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
636IB-1501278-P
16.2 Mixed Control 16.2.1 Arbitrary Axis Exchange ; G140, G141, G142
With this function, an arbitrary axis can be exchanged freely across part systems. The machining can be freer in the multiple part systems by exchanging an axis that can be commanded for machin- ing programs in each part system. This makes it possible to perform operations which are not possible with regular axis configurations: for instance, tools which are provided only on the 1st part system can be used for machining on the 2nd part system.
This chapter illustrates an example based on the placements of the basis axes below.
Refer to "Programming Manual Lathe System" for details of the arbitrary axis exchange.
(1) When performing arbitrary axis exchange with M80 typeA and M80W, set the parameter "#1431 Ax_Chg" to "1". If the arbitrary axis exchange command is issued while the parameter is "0", a program error (P39) occurs. This function is available in the following software version. M80 TypeA, M80W: E1 version or later M800 Series: B1 version or later (depends on the MTB specifications.)
Returns the control right of the axis, exchanged by the previous arbitrary axis exchange command (G140) in the commanded part system, to the state before the axis exchange.
Returns the control right of the axis, exchanged by the arbitrary axis exchange command (G140) in the commanded part system, to the power-ON state.
Function and purpose
X axis Y axis Z axis C axis
1st part system ($1) X1 Y1 Z1 - 2nd part system ($2) X2 Y2 - C2
Command format
When commanding the arbitrary axis exchange
G140 command address = axis address ... ;
Command Address It is a command address used in a movement or other command after arbitrary axis exchange command (G140). Designate the command address with one alphabetical character set to parame- ters ("#12071 adr_abs[1]" to "#12078 adr_abs[8]") .
Axis address Set the axis name for arbitrary axis exchange. Designate the command with two alphanumeric characters set to the parameter "#1022 axname2".
When returning the exchanged axis
G141; Arbitrary axis exchange return
G142; Reference axis arrange return
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
637 IB-1501278-P
There are two methods for axis exchange operations with arbitrary axis exchange command (G140). The methods for your machine depends on the MTB specifications (parameter "#1434 G140Type2").
(1) Operation example of the method for exchanging all axes ("#1434 G140Type2"=0) Below is the control axis of each part system when running the following machining programs (1st part system, 2nd part system)
Detailed description
Arbitrary axis exchange command (G140)
Method Operation
Method for exchanging all axes ("#1434 G140Type2" = 0)
Designates axes to be used in the part system with a command address. The command addresses axes that are not designated will be released as uncon- trol axes.
Method for exchanging com- mand axes ("#1434 G140Type2" = 1)
Designates axes to be used in the part system with a command address. The command addresses axes that are not designated will maintain the current state.
$1 $2 Control axes Uncontrol
axes Machining program Machining program $1 $2
X Y Z X Y C
G140 X=X1 Y=Y1 Z=Z1; G00 X10.; G01 X5. F1; :
(a) G140 X=X2 Y=Y2 C=C2; G00 X20.; G01 X15. F2; :
(d)
X1 Y1 Z1 X2 Y2 C2 -
G140 X=X1 Y=Y2; G00 Y25.; G01 X8. F2; :
(b)
X1 Y2 -
X2 - C2 Y1,Z1
G140 Y=Z1; G00 Y10.; G01 Y8. F0.05; :
(e)
- Z1 - Y1,X2,C2
G140 X=X1 Y=Y1 Z=Z1; G00 X20. Y15.; G01 X15. F5; :
(c)
X1 Y1 Z1
- - - X2,Y2,C2
G140 X=X2 Y=Y2 C=C2; G00 X0; :
(f) X2 Y2 C2 -
1st part system ($1) (a),(c) Declares the use of X1 axis, Y1 axis and Z1 axis. (b) Declares the use of X1 axis and Y2 axis.
The control right of Y2 axis shifts to the 2nd part system from the 1st part sys- tem. Y1 axis, exchanged for Z1 axis and Y2 axis which were not designated, will be an uncontrol axis.
2nd part system ($2) (d),(f) Declares the use of X2 axis, Y2 axis and C2 axis. (e) Declares the use of Z1 axis.
X2 axis and C2 axis which were not designated will be uncontrol axes.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
638IB-1501278-P
(2) Operation example of the method for exchanging command axes ("#1434 G140Type2"=1) Below is the control axis of each part system when running the following machining programs (1st part system, 2nd part system)
"Unavailable state of axis exchange" indicates a "condition in which a target axis for axis exchange is not available for exchange because the designated target axis for axis exchange is being used by other part systems or for other reasons" through the arbitrary axis exchange command (G140), the arbitrary axis exchange return command (G141), the reference axis arrange return command (G142). When the conditions for unavailable state of axis exchange fall through, no axis exchange mode will be cancelled. It will be cancelled when a "reset" signal or emergency stop is entered.
$1 $2 Control axes Uncontrol
axes Machining program Machining program $1 $2
X Y Z X Y C
G140 X=X1 Y=Y1 Z=Z1; G00 X10.; G01 X5. F1; :
(a) G140 X=X2 Y=Y2 C=C2; G00 X20.; G01 X15. F2; :
(d)
X1 Y1 Z1 X2 Y2 C2 -
G140 Y=Y2; G00 Y25.; G01 X8. F2; :
(b)
X1 Y2 Z1
X2 - C2 Y1
G140 Y=Y1; G00 Y10.; G01 Y8. F0.05; :
(e)
X2 Y1 C2 -
G140 Y=Y1 ; G00 X20. Y15.; G01 X15. F5; :
(c)
X1 Y1 Z1
X2 - C2 Y2
G140 X=X2 Y=Y2 C=C2; G00 X0; :
(f) X2 Y2 C2 -
1st part system ($1) (a) Declares the use of X1 axis, Y1 axis and Z1 axis. (b) Declares the use of Y2 axis.
The control right of Y2 axis shifts to the 2nd part system from the 1st part sys- tem. Y1 axis which was exchanged for Y2 axis will be an uncontrol axis.
(c) Declares the use of Y1 axis. The control right of Y1 axis shifts to the 2nd part system from the 1st part sys- tem. Y2 axis which was exchanged for Y1 axis will be an uncontrol axis.
2nd part system ($2) (d) Declares the use of X2 axis, Y2 axis and C2 axis. (e) Declares the use of Y1 axis. (f) Declares the use of X2 axis, Y2 axis and C2 axis.
Unavailable state of axis exchange
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
639 IB-1501278-P
16.3 Sub Part System Control 16.3.1 Sub Part System Control I; G122
This function activates and operates any non-operating part system (sub part system) in the multi-part system. Sub part system control I can be used in the same manner as calling subprogram in a non-operating part system. An auxiliary axis machining program can be controlled in the sub part system by commanding Sub part system control I (G122) from the main part system. In the usage example below, the tool positioning starts to the machining start point at the same time (time T1) as the start of gantry retract by using Sub part system control I (G145) in the flow from feeding the workpiece to moving to cut start position in order to reduce the cycle time. Select whether main part system or sub part system for each part system in Sub part system control I. When using a part system as a sub part system, by setting the operation mode to "Sub part system I operation mode" with the PLC signal and commanding sub part system control I (G122) from an operating part system, it is possible to activate the part system in the sub part system I operation mode as a sub part system.
The following describes the meanings of the terms used in this chapter.
The examples below shows many part systems to provide an easy-to-understand explanation. The actually avail- able number of part systems depends on your machine's specifications.
Function and purpose
Term Meaning
Main part system Indicates a part system located on the uppermost stream side of a sub part system call flow.
Sub part system Indicates a part system activated by the sub part system activation command. Calling part system Indicates a part system that issued the sub part system activation command.
($1)
T1 T2
T1 T2
T2:
T1:
($2)
($1)
(1) Feed the workpiece
(1)Feed the workpiece
Wait for completion of sub part system
(4)Move to cut start position
(2)Clamp the workpiece
(2) Clamp the workpiece
(3) Retract gantry
(3)Retract gantry
(4) Move to cut start position
Machining process when Sub part system control is OFF
Machining process when Sub part system control is ON
Main part system
Time when gantry retract is started
Time when gantry retract is completed Sub part system
Main part system
Sub part system starts Time
Time
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
640IB-1501278-P
(1) This function can be used in multi-part systems of two or more part systems. (2) In order to activate a sub part system using the sub part system control I command, the following conditions must
be satisfied. There are enabling conditions that are only applicable to the M80 series.
[Condition 1] This condition must be satisfied only for the M80 series/C80 series. The number of sub part systems has been set in the base common parameter "#1483 SBS1_sys num" (the num- ber of part systems in sub part system I).
(a) Part systems as many as the number specified in #1483, counted from the end of the valid part system (the part system for which "#1001 SYS_ON" is set to "1"), will be reserved as sub part systems.
(b) If the number of sub part systems or main part systems exceeds the maximum number defined in the system specifications, an MCP alarm (Y05 1483) will occur.
(c) (M80 series only) If the values set for "#1483 SBS1_sys num" and "#1474 SBS2_sys num" are both "1" or more, an MCP alarm (Y05 1483) will occur.
[Condition 2] The identification No. (B command value) used to activate a sub part system has been set in the base common parameter "#12049 SBS_no" (sub part system I identification No.) for sub part systems.
(a) If an identification No. that is not set in the parameter "#12049 SBS_no" is specified when the sub part system control I command is issued, a program error (P650) (sub part system identification No. illegal) will occur.
[Condition 3] The PLC signal SBSM (Sub part system I operation mode) of the sub part system is set to "1".
(a) In a part system operating the sub part system I operation mode, the operation mode appears as "SUB" in the part system display of the operation screen.
(b) If the sub part system control I command is issued to a part system that is not operating the sub part system I operation mode, an operation error (M01 1111) will occur. However, while the operation error (M01 1111) is occurring, the operation can be started by setting SBSM to "1".
Enabling conditions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
641 IB-1501278-P
(1) G145 is ignored in a sub part system activated in the parallel control method (D1 command).
Command format
Call sub part system
G122 A__P__Q__K__D__B__H__ (argument);
G122
A Program No. (1 to 99999999 or 100010000 to 199999998)
point command is valid))
Complete sub part system
M99; (command in sub part system side)
Cancel the standby status for completion of sub part system (command in the sub part system side when the D0 command is issued)
G145;
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
642IB-1501278-P
This function can be used in multi-part systems of two or more part systems. Main part system and sub part system are switched according to the MTB specifications.
(*1) When the parameter "#1253 set25/bit0" is set to "1", the command range is "100010000 to 199999989".
(*2) If a sub part system ends by M99 or the end sequence No., resetting processing is performed automatically in the sub part system.
Detailed description
Description of each address
Address Meaning Command range (unit)
Remarks
A Program No. 1 to 99999999 or 100010000 to 199999998 (*1)
Program No. or file name of the machining program oper- ating in the sub part system. Programs in an external device cannot be designated. If address A and
time, precedence is given to address A. If designation of the program is omitted, the machining
program defined by the MTB will be used (parameter "#12050 SBS_pro").
File name of the program
Up to 32 charac- ters.
P Start sequence No.
1 to 99999999 Sequence No. to start the machining program operating in the sub part system. If there is no command, the operation will start from the
head of the machining program. Q End sequence No. 1 to 99999999 Sequence No. to end the machining program operating in
the sub part system. If there is no command, the program will run up to "M99".
K Number of repeti- tions
1 to 9999 The number of times to repeat the machining program for continuous operation in the sub part system. If there is no command, the program will only run once.
(No repetition) D Synchronous con-
trol 0 / 1 Validity of synchronous control
0: The next block is processed after the sub part system operation completes. 1: The next block is processed at the same time as the start of a sub part system operation. If there is no command, it is handled in the same manner as 0 is designated.
B Sub part system identification No.
1 to 7 Identification No. used for timing synchronization with sub part system, etc. The sub part system to be activated is designated by an
identification No. The correspondence between identifi- cation No. and part system No. depends on the MTB specifications (parameter "#12049 SBS_no"). If there is no command, it is handled in the same manner
as 1 is designated. H Sub part system
reset type (*2) 0 / 1 0: The G command modal is maintained by the reset when
a sub part system is complete. 1: The G command modal is initialized by the reset when a sub part system is complete. If there is no command, it is handled in the same manner
as 0 is designated. (Argument) Argument of a sub
part system local variable
Setting range of lo- cal variable (Decimal point command is possi- ble.)
Argument is passed to the sub part system as a local vari- able (level 0). However, addresses A, B, D, G, H, K, O, P, and Q cannot be used as an argument. For the correspondence between address and variable
number, refer to the following table.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
643 IB-1501278-P
(1) Addresses can be designated in an arbitrary order. (2) Addresses which do not need to be designated can be omitted. (3) Local variables in a sub part system are initialized every time the sub part system is activated. Default value is
model, refer to the list.
(1) The operation mode of sub part systems is used as "sub part system I operation mode". If the memory mode/ MDI mode and the sub part system I operation mode are entered at the same time, the stop code (T01 0108) will be generated.
(2) In a part system operating the sub part system I operation mode, the operation mode appears as "SUB" in the part system display of the operation screen. If an alarm or warning occurs in a sub part system, the part system No. appears as "SUB" in the alarm/warning message of the operation screen.
(3) If the sub part system control I command is issued to a part system that is not operating the sub part system I operation mode, an operation error (M01 1111) will occur.
Correspondence of argument designation address and variable number in sub part system
Argument designa- tion address
Variable number in sub part system
Argument designa- tion address
Variable number in sub part system
A - N #14 B - O - C #3 P - D - Q - E #8 R #18 F #9 S #19 G - T #20 H - U #21 I #4 V #22 J #5 W #23 K - X #24 L #12 Y #25 M #13 Z #26
Operation mode of a sub part system
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
644IB-1501278-P
When issuing the sub part system control I command, designate the sub part system identification No. with com- mand address B. (When there is no B command, it will be handled as the B1 command.) The sub part system iden- tification No. and the sub part system No. to be called depend on the MTB specifications. (Parameter "#12049 SBS_no")
(Example 1) and (Example 2) show the operations when parameters are set as shown below. The available number of part systems depends on your machine's specifications.
(Example 1) If the B command is omitted, $5 corresponding to B1 will be activated.
(Example 2) Sub part system identification No. (the part system No. to be activated and correspondence) can be specified with the B command.
Activation part system of a sub part system
#12049 SBS_no Sub part system I identification No.
$1 $2 $3 $4 $5 $6 $7 $8 0 0 0 0 1 2 3 4
Calling part system ($1) Sub part system ($5)
Calling part system ($1) Sub part system ($7)
: : G122 A100 D0; : :
: : : M99;
: : G122 A100 D0 B3; : :
: : : M99;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
645 IB-1501278-P
When issuing the sub part system control I command, designate the program No. or program name to be operated in the sub part system with command address A or
(*1) If the program of the part system No. for the sub part system is empty, the program of the 1st part system ($1) will be operated. If the program of the 1st part system is also empty, a program error (P461) will occur.
(1) If program is managed for each part system
(2) If program is commonly managed between part systems
Operation program of a sub part system
:
:
M99;
:
: G122 A100 D0 B3 :
$1
$2
$3
$4
$5
$6
$7
$8
O100 - $7
O1 - $1
O100 Caller part system ($1)
$7 is assumed to be started by B3 command.
Sub part system ($7)
When $7 is blank, $1 data will be called.
:
:
M99;
:
:
G122 A100 D0 B3
: O100
O1 O100 Calling part system ($1)
Sub part system ($7)
$7 is assumed to be started by B3 command.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
646IB-1501278-P
If "0" is designated for command address D when the sub part system control I command is issued, or if command address D is omitted, the calling part system will wait for the called sub part system to complete (to M99 or the end sequence No.) before starting the next block. Meanwhile, if the completion wait cancel command (G145) is issued in a sub part system while the calling part sys- tem is in the sub part system completion standby state, the machine will shift to a parallel processing mode. The following shows the operation and the activation timing of each part system.
Sub part system activation with the completion wait method (D=0)
Calling part system
Sub part system
Calling part system
Sub part system
: Completion wait
O1 O2
G00 X100.;
O100 O200
M99;
G145;
M99; G00 X100.;
G122 A100 D0 B1; G122 A200 D0 B1; :
: : :
:
: :
:
:
Calling part system Calling part system
Sub part system Sub part system(a) Start (c) Start
(d) Waiting canceled
(e) Completion(b) Completion
Completion wait Completion wait
(a) (b)
O100
O1
O200
O2 (c) (e)(d)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
647 IB-1501278-P
If "1" is designated for command address D when the sub part system control I command is issued, the following blocks of the calling part system and the first and the following blocks of the sub part system will be operated in parallel. The following shows the operation and the activation timing of each part system.
Multiple sub part systems can be activated in parallel during separate processes by calling from a single part system. The number of sub part systems to be processed simultaneously depends on the model. The following shows the operation and the activation timing of each part system.
Activation of a sub part system with parallel processing mode (D=1)
Calling part system
Sub part system
Activation of multiple sub part systems
Calling part system
Sub part system 1
Sub part system 2
: Completion wait
G122 A100 D1 B1; :
:
:: :
G00 X100.;
O1
O100
M99;
Calling part system
Sub part system(a) Start
(b) Completion
(a) (b)
O100
O1
O1
O200
G00 X100.;
M99;
O100
M99;
G122 A100 D1 B1;
G122 A200 D0 B2; :
: :
: : :
:
:
Sub part system 1
Calling part system
(Parallel processing method)
(Completion wait method)
(a) Start
Completion wait
(b) Start
(d) Completion
(c) Completion
Sub part system 2
(a) (c)
O100
O1
O200
(b) (d)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
648IB-1501278-P
A sub part system can be activated from another sub part system. The number of sub part systems to be processed simultaneously depends on the model. The following shows the operation and the activation timing of each part system.
Activate a sub part system from another sub part system
Calling part system
Sub part system 1
Sub part system 2
: Completion wait
O1
O100
O200
M99;
M99;
G00 X100.;
G122 A100 D0 B1;
G122 A200 D0 B2;
:
: :
: :
: :
:
Calling part system
Completion wait Completion wait
(a) Start
(d) Completion
(c) Completion
(b) Start
Sub part system 1
Sub part system 2
(a) (c)
O100
O1
O200
(b) (d)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
649 IB-1501278-P
If G122 is commanded while a sub part system is being activated, using the same identification No. (B command), the machine will wait for the earlier sub part system to complete activation, before activating the next sub part sys- tem.
In the following example, the machining start timing is accelerated by controlling auxiliary axis with a sub part system and operating the main part system and the sub part system in parallel. The tool positioning starts to the machining start point at the same time (time T1) as the start of gantry retract by using sub part system completion wait cancel command (G145) in the flow from mounting the workpiece to moving to cut start position, after feeding and mounting the workpiece with the gantry, in order to reduce the cycle time. (The machine configuration below is a sample only.)
Sub part system activation command to a sub part system being activated
Calling part system 1
Calling part system 2
Sub part system
: Completion wait : Standby
Operation example
[Axis configuration] Main part system ($1) : X1 axis, Z1 axis => Tool Sub part system ($2) : X2 axis, Z2 axis => Workpiece feed gantry
[Machining process] (a) Feed the workpiece (b) Clamp the workpiece (c) Retract the gantry (d) Move to cut start position
O1 O2
G00 X-20.;
O100
M99;
M99;
O200G00 X100.;
(b)
:
: :
:
: : :
G122 A100 D0 B1;
G122 A200 D1 B1;
: : :
: : :
Calling part system 1
(a) Start
(c) Completion
(e) Completion
(d) Start Wait for vacancy of
sub part system
Completion wait
Sub part system
Calling part system 2
(Identification No. 1)
(a)
O1
O100 O200
O2
(b) (c) (d) (e)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
650IB-1501278-P
(1) Machining process when sub part system control is OFF
After the gantry is retracted, cut start position is determined.
(2) Machining process when sub part system control is ON
Processes after "(c) Retract gantry" and "(d) Move to cut start position" will be operated in parallel.
Main part system ($1) O1 : G140 X=X2 Z=Z2; ... (a) G00 X50.; G00 Z20.; M20; ... (b) G00 X0. Z0. ; ... (c) G140: Arbitrary axis exchange command (Lathe system only) G141; G141: Arbitrary axis exchange return command (Lathe system only) G00 X30. Z-15.; ... (d) M20 : M code of workpiece mounting G01 Z-20. F10.; :
Main part system ($1)
Time
Time when gantry retract is started Time when gantry retract is completed
Main part system ($1) Sub part system ($2)
M20 : M code of workpiece mounting
Sub part system ($2)
Main part system ($1)
Time
Activation of a sub part system Start of gantry retract Completion of retract
: Completion wait
(a) (b) (c) (d)
O1 O100 : : G122 A100 D0 B1; G00 X30. Z-15.; ... (d) G01 Z-20. F10.; : :
G00 X50.; ... (a) G00 Z20.; M20; ... (b) G145; G00 X0. Z0.; ... (c) : M99;
(a) (b) (c)
(d)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
651 IB-1501278-P
While a sub part system is under control, timing synchronization between part systems can be issued with the "![Part system No.]" command. To synchronize timing between a main part system and a sub part system, or between sub part systems, it is also possible to designate a sub part system identification No. (B command) as shown below. However, the number of part systems that can be used is limited by the specifications.
For example, to synchronize timing with the calling part system, command "![0]". Note that, designate the calling part system with "![0]", not the main part system. (Example 1) and (Example 2) shown below are examples of the timing synchronization operation between the main part system ($3), sub part system 1 ($5, identification No. 1), and sub part system 2 ($6, identification No. 2).
(Example 1) Timing synchronization by designating a part system No.
(Example 2) Timing synchronization by designating a sub part system identification No.
Relationship with other functions
Timing synchronization with sub part system
![Sub part system identification No.]
Main part system ($3) Sub part system 1 ($5) Sub part system 2 ($6)
Timing synchronization with 5th and 6th part systems
Timing synchronization with 3rd and 6th part systems
Timing synchronization with 3rd and 5th part systems
Main part system ($3) Sub part system 1 ($5, identi- fication No. 1)
Sub part system 2 ($6, identifi- cation No. 2)
Timing synchronization with the following part system Sub part system of identifi-
cation No. 1 Sub part system of identifi-
cation No. 2
Timing synchronization with the following part system Calling part system ($3) Sub part system of identifi-
cation No. 2
Timing synchronization with the following part system Calling part system ($3) Sub part system of identifica-
tion No. 1
: G122 A100 D1 B1; G122 A200 D1 B2; : !5!6; G00 X100.; : :
: : : : !3!6; : : :
: : : : !3!5; : : :
: G122 A100 D1 B1; G122 A200 D1 B2; : ![1]![2]; G00 X100.; :
: : : : ![0]![2]; : :
: : : : ![0]![1]; : :
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
652IB-1501278-P
Timing synchronization operation ignore signal
Whether to ignore the "![Sub part system identification No.]" command or not depends on the MTB specifications. (Setting of parameter "#1279 ext15/bit0" and the following PLC signals)
With the sub part system control I, axes that belong to the sub part system when the sub part system is activated can be controlled. To change the axis to be controlled, exchange axes (to transfer the control rights of the specified axis from other part systems to the own part system) with the arbitrary axis exchange return command (G140).
If the tool No. is changed (T command) in the program run of a sub part system, the T code data will be changed for the sub part system only. The T code data will not be changed for the main part system or other sub part systems.
When an axis in the main part system, for which the tool compensation has been commanded, is moved to a sub part system with the arbitrary axis exchange or other operation, the tool compensation will be maintained. Also, when an axis (*1) in a sub part system, for which tool compensation has been commanded, is moved to the main part system or another sub part system with the arbitrary axis exchange operation, tool compensation will be main- tained. Whether the arbitrary axis exchange function is available depends on the specifications of your machine tool.
(*1) If tools are managed for each part system, the offset data to be referenced when the tool compensation com- mand is issued in a sub part system is used as setting values for the sub part system. (The setting value of the main part system will not be referenced.)
#1279 ext15/bit0
PLC signal for ignor- ing timing synchroni- zation between part
systems
Operation
If the other part system is being ac- tivated as a sub part system
If the other part system is not being activated as a sub part system
0
ON The timing synchronization operation is ignored when activation of a sub part system is completed for the other part system.
Program error (P35)
OFF
1 ON Ignore the timing synchronization op-
eration.
OFF Execute the timing synchronization operation between part systems.
Arbitrary axis exchange control
Tool functions
Tool compensation
Main part system ($1) Sub part system ($2)
G140: Arbitrary axis exchange command G141: Arbitrary axis exchange return command
O1
: G28 Z0 T01; ...(a) G90 G92 Z0; G43 Z50. H01; ...(b) G01 Z-500. F500; : G122 A100 D0 B1; G00 X10. Z50.; ...(e) :
O100
G140 X=X1; G28 X0 T02; ...(c) G90 G92 X0; G43 X10. H02; ...(d) G01 X-100. F500; :
G141; M99;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
653 IB-1501278-P
L(N_$M) indicates the compensation amount of compensation No. N in the Mth part system.
The sub part system control I command does not affect nesting in user macros and subprograms. It can be com- manded from a subprogram nested at the deepest level.
(1) If the NC reset signal is input to the main part system, the operation of the main part system will be reset and end immediately. However, the operation of sub part systems will continue. The reset operation of the sub part system follows the NC reset signal of the sub part system.
(2) If the NC reset signal is input to an operating sub part system, the operation of the sub part system will end im- mediately. Therefore, if the calling part system is in the sub part system completion standby state, the sub part system is reset, and at the same time, the calling part system cancels the standby state, and the following block will be executed.
If both of the following conditions (1) and (2) are satisfied, the buffer correction is disabled. (The buffer correction window will not open even if the program correction key is pressed.)
(1) The next block is G122 command (including "macro statement + G122 command"). (2) The program designated by G122 is the same as that of the calling part system.
The completion wait time of the sub part system control I command (G122) will not be added to the machining time computation for the main part system.
If the restart search from the block of the G122 command is attempted, a program error (P49) will occur.
T code data Compensation amount
$1 $3 Z1 X1 (a) 1 - : : (b) 1 - L(01_$1) : (c) 1 2 L(01_$1) : (d) 1 2 L(01_$1) L(02_$3) (e) 1 2 L(01_$1) L(02_$3)
User macro
Resetting
Buffer correction
O100 : G00 Z50.; Buffer correction possible G00 X100.; Buffer correction impossible G122 A100 P77 D0 B1; Designated program is the program (O100) of its own part system G00 Y30.; Buffer correction possible : N77 : Program operated in sub part system M99;
Machining time computation
Program restart
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
16 Multi-part System Control
654IB-1501278-P
If the sub part system control I (G122) is commanded during the following G command modal, a program error (P652) will occur.
User macro modal call (G66, G66.1) Fixed cycle modal High-speed machining mode (G05P1, G05P2) High-speed high-accuracy control (G05.1Q1, G05P10000, G05P20000)
The sub part system control I (G122) is ignored at the reverse run or the forward run after the reverse run. Because the sub part systems are in a mode in which reverse run is prohibited, reverse run cannot be carried out in sub part systems.
(1) The sub part system control I command (G122) is a G code that must be issued alone. If another G code is com- manded in the same block, a program error (P651) or (P32) occurs. If another G code is commanded before G122 (for example, when "G00 G122" is commanded), a program
error (P651) occurs. If another G code is commanded after G122 (for example, when "G122 G00" is commanded), a program
error (P32) occurs. (2) While the sub part system I operation mode is in operation, even if the sub part system is not being activated,
automatic operation cannot be started with the automatic operation start signal (ST). The stop code (0146) will be generated. However, when a sub part system is being activated, automatic operation is started with the au- tomatic operation start signal (ST).
(3) If a sub part system identification No. of its own part system is designated for the B command with the sub part system control I command (G122), a program error (P650) will occur.
(4) The PLC signal of the sub part system references the state of the sub part system. (The signal state of the main part system will not be taken over.)
(5) Parameters per part system of the sub part system follow the setting in the sub part system. Therefore, param- eters must also be set in the sub part system.
(6) If the sub part system completion wait cancel command (G145) is issued in the main part system, a program error (P34) occurs.
(7) The following operations are performed in the M80 series/C80 series. These parameter settings depend on the MTB specifications. Activation of a sub part system is only possible in sub part systems that are reserved using the parameter
"#1483 SBS1_sys num". If the sub part system activation command is issued to a main part system (*1), an operation error (M01 1111) occurs. (*1) This refers to a case in which the sub part system I operation mode is established (SBSM: ON) using the
PLC signal before G122 is commanded. Operation searches cannot be carried out in sub part systems that are reserved using the parameter "#1483
SBS1_sys num". (M80 series only) If the values set for the parameters "#1483 SBS1_sys num" and "#1474 SBS2_sys num"
are both "1" or more, an MCP alarm (Y05 1483) will occur.
Illegal modal of a sub part system control I command
Manual arbitrary reverse run
Precautions
17
655 IB-1501278-P
High-speed High-accuracy Control
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
656IB-1501278-P
17High-speed High-accuracy Control 17.1 High-speed Machining Mode
17.1.1 High-speed Machining Mode I, II; G05 P1, G05 P2
This function runs a machining program for which a freely curved surface has been approximated by fine segments at high speed. A higher fine segment processing capability leads to a faster cutting speed, resulting in a shorter cycle time and a better machining surface quality. The high-speed high-accuracy control I/II/III enable not only the high-speed machining mode but also the high-ac- curacy control mode. Use the high-speed high-accuracy control I/II/III for machining which needs to make an edge at a corner or reduce an error from an inner route of curved shape. This function can be used simultaneously for up to two part systems depending on the MTB specifications. kBPM, the unit for the fine segment processing capability, is an abbreviation of "kilo blocks per minute" and refers to the number of machining program blocks that can be processed per minute. In the main text, the axis address refers to the address of an axis that exits on the machine. It corresponds to the address designated in the parameters "#1013 axname" and "#1014 incax". These parameter settings depend on the MTB specifications.
G01 block fine segment processing capability for 1 mm segment (unit: kBPM)
(1) The above performance applies under the following conditions. 6-axis system (including spindle) or less 1-part system 3 axes or less commanded simultaneously in G01 The block containing only the axis name and movement amount (Macro and variable command are not in-
cluded.) In the "G61.1" high-accuracy control mode or cutting mode (G64) During tool radius compensation cancel (G40) (only in the high-speed machining mode II) When the above conditions are not satisfied, the given feedrate may not be secured.
(2) The performance in the table may vary depending on the combination with other functions.
Function and purpose
For one part system
Mode Command Maximum feedrate when 1 mm segment G01 block is executed (kBPM)
M850/M830 M80W M80 C80
Type A Type B
High-speed machin- ing mode I
G05 P1 33.7 33.7 33.7 16.8 33.7
High-speed machin- ing mode II
G05 P2 168 67.5 67.5 67.5 67.5
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
657 IB-1501278-P
G01 block fine segment processing capability for 1 mm segment (unit: kBPM)
(*1) This system cannot be used for this model.
(*2) There are no high-speed machining mode II specifications.
(1) The above performance applies under the following conditions. 3 axes commanded simultaneously in G01 The block containing only the axis name and movement amount (Macro and variable command are not in-
cluded.) Tool radius compensation cancel (G40) mode When the above conditions are not satisfied, the given feedrate in the table may not be secured.
(2) The performance in the table may vary depending on the combination with other functions. (3) The number of part systems and axes that can be used depends on the specifications of your machine tool.
Multi-part system (high-speed machining mode II)
Specified num- ber of part sys- tems (#8040 = 1)
Maximum feedrate when 1 mm segment G01 block is executed (kBPM)
M850/M830 M80
Type A Type B
1-part system 1 part system 168 67.5 67.5 2-part system 1 part system only 100 67.5 67.5
Two part systems simultaneously
67.5 33.7 33.7
4-part system Up to 16 axes
1 part system only - (*1) - (*1) - (*1) Two part systems simultaneously
- (*1) - (*1) - (*1)
5 part systems or more or 17 axes or more
1 part system only - (*1) - (*1) - (*1) Two part systems simultaneously
- (*1) - (*1) - (*1)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
658IB-1501278-P
In addition to the G05 P0 command, the high-speed machining mode I is canceled when the high-speed machining mode II (G05 P2) is commanded. In reverse, the high-speed machining mode II is canceled when the high-speed machining mode I (G05 P1) is com- manded.
Command G05 alone in a block. A program error (P33) occurs if a movement or other command is additionally is- sued in a G05 command block. A program error (P33) also occurs if there is no P command in a G05 command. In addition to cancel the high-speed machining mode II, a G05 P0 command is also used to cancel the high-speed high-accuracy control II/III. Refer to "17.3 High-speed High-accuracy Control" for details.
(1) The override, maximum cutting speed clamp, single block operation, dry run, manual interruption and graphic trace and high-accuracy control mode are valid even during the high-speed machining mode I/II. For a part system that uses the high-speed machining mode II, "1" must be set for the parameter "#8040 High- SpeedAcc". By default, the high-speed machining mode II can only be used in the first part system.
(2) When using the high-speed machining mode II, setting to eliminate the speed fluctuation at the seams between the arc and the straight line, or between arcs depends on the MTB specifications (parameter "#1572 Cirorp/ bit1").
(3) Combination with high-accuracy control The high-speed machining mode and high-accuracy control can be used simultaneously by taking the following steps: (a) Set "1" for the parameter "#8040 High-SpeedAcc". (b) Command "G05 P2" and "G08 P1" or "G61.1" from the machining program. The parameter "#8040 High-SpeedAcc" can be set to "1" for up to two part systems. If "0" is set for all part sys- tems, the first and second part systems can use the high-speed machining mode and high-accuracy control si- multaneously.
Also refer to the following for the description of each function: High-accuracy control: "17.2 High-accuracy Control" Simultaneous usage of the high-speed machining mode and high-accuracy control: "17.3 High-speed High-
accuracy Control"
Command format
High-speed machining mode I ON
G05 P1 ;
High-speed machining mode II ON
G05 P2 ;
High-speed machining mode I/II OFF
G05 P0 ;
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
659 IB-1501278-P
(4) If the variable command, variable operation command, or macro control statement is commanded while high- speed machining mode II is valid, the fine segment processing capability decreases. However, only when the variable commands and variable four-basic-arithmetic operation commands shown below are issued following the axis address or the F address of the cutting feedrate command, the fine segment processing capability does not decrease. (a) Referencing common variables or local variables
Common variables or local variables can be referenced (example: X#500, Y#1, Z##100, A#[#101], etc.). (b) Four basic arithmetic rule
Four basic arithmetic rule (+, -, *, /) operations are available, and also the operation priority can be designated using parentheses ( ) ([#500 + 1.0] * #501, etc.).
If a common variable or local variable is referenced using the variable number operated with a macro operation instruction, a program error (P282) may occur. In this case, set the operated value to the variable before refer- encing the variable.
(5) If geometric command is programmed while high-speed machining mode II is active, a program error (P33) oc- curs.
Example that causes an error F#[FIX[100.1]]; Example that does not cause an error #500 = FIX[100.1] ;
F#[#500] ;
Program example
High-speed machining mode I
G28 X0. Y0. Z0. ; G91 G00 X-100. Y-100. ; G01 F10000 ; G05 P1 ; High-speed machining mode I ON : X0.1 Y0.01 ; X0.1 Y0.02 ; X0.1 Y0.03 ; : G05 P0 ; High-speed machining mode I OFF M30 ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
660IB-1501278-P
Column A: Operation when the combination function is commanded while the high-speed machining mode II is en- abled Column B: Operation when the high-speed machining mode II (G05P2) is commanded while the combination func- tion is enabled : The high-speed machining mode II and the additional function are both enabled : The high-speed machining mode II is temporarily canceled, while the additional function is enabled x: Alarm generation (the text in parentheses refers to the number of the program error to be generated) -: No combination : Others
Relationship with other functions
Relationship between the high-speed machining mode II and G code functions
Group G code Function name A B
0 G04 Dwell - G05P0 High-speed machining mode II OFF
High-speed high-accuracy control II OFF High-speed high-accuracy control III OFF
(*1) (*2)
G05P2 High-speed machining mode II ON (*3) (*3) G05P10000 High-speed high-accuracy control II ON (*4) (*2) G05P20000 High-speed high-accuracy control III ON (*5) (*6) G05.1Q0 High-speed high-accuracy control I OFF
Spline interpolation OFF (*3) (*2)
G05.1Q1 High-speed high-accuracy control I ON (*7) (*2) G05.1Q2 Spline interpolation ON (*12) (*12) G07 Hypothetical axis interpolation (*12) (*12) G08P0 High-accuracy control OFF (*3) (*2) G08P1 High-accuracy control ON (*8) (*8) G09 Exact stop check - G10 I_J_ G10 K_
Parameter coordinate rotation input (*12) - (*12)
G10 L2 Compensation data input by program - G10 L70 G10 L50
Parameter input by program -
G27 Reference position check - G28 Reference position return - G29 Start position return - G30 2nd to 4th reference position return - G30.1 - G30.6 Tool exchange position return - G31 Skip
Multi-step skip 2 -
G31.1 - G31.3 Multi-step skip - G34 - G36 G37.1
Special fixed cycle -
G37 Automatic tool length measurement - G38 Tool radius compensation vector designation - G39 Tool radius compensation corner circular command -
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
661 IB-1501278-P
0 G52 Local coordinate system setting - G53 Machine coordinate system selection - G60 Unidirectional positioning - G65 User macro simple call (*9) (*10) G92 Coordinate system setting - G92.1 Workpiece coordinate system preset (*12) - (*12) G122 Sub part system control I (P652)
(*12) (*11)(*12)
G144 Sub part system control II (P652) (*12)
(*11)(*12)
1 G00 Positioning G01 Linear interpolation G02 G03
Circular interpolation
G02.1 G03.1
Spiral interpolation (*12) (*12)
G02.3 G03.3
Exponential interpolation (*12) (*12)
G02.4 G03.4
3-dimensional circular interpolation (*12) (*12)
G06.2 NURBS interpolation (*12) (*12) G33 Thread cutting
2 G17 - G19 Plane selection 3 G90 Absolute command
G91 Incremental command 4 G22 Stroke check before travel ON
G23 Stroke check before travel OFF 5 G93 Inverse time feed (*12) (*12)
G94 Asynchronous feed (feed per minute) G95 Synchronous feed (feed per revolution)
6 G20 Inch command G21 Metric command
7 G40 Tool radius compensation cancel G41 G42
Tool radius compensation
8 G43 G44
Tool length offset
G43.1 Tool length compensation along the tool axis (*12) (*12) G43.4 G43.5
Tool center point control (*12) (*12)
G49 Tool length offset cancel 9 G80 Fixed cycle cancel
Group 9 Other than G80
Fixed cycle
10 G98 Fixed cycle initial level return G99 Fixed cycle R point return
11 G50 Scaling cancel G51 Scaling ON
12 G54 - G59 G54.1
Workpiece coordinate system selection
Group G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
662IB-1501278-P
(*1) Disables the high-speed machining mode II.
(*2) Enables the high-speed machining mode II.
(*3) High-speed machining mode II continues.
(*4) Enables the high-speed high-accuracy control II.
(*5) Enables the high-speed high-accuracy control III.
(*6) High-speed high-accuracy control III continues.
(*7) Enables the high-speed high-accuracy control I.
(*8) Enables the high-speed machining mode II and high-accuracy control.
(*9) Enables the high-speed machining mode II in a macro program.
(*10) Enables the high-speed machining mode II if G05P2 is commanded in a macro program.
(*11) Enables the high-speed machining mode II if G05P2 is commanded in a sub part system.
13 G61 Exact stop check mode G61.1 High-accuracy control G61.2 High-accuracy spline (*12) (*12) G61.4 Spline interpolation 2 (*12) (*12) G62 Automatic corner override G63 Tapping mode G64 Cutting mode
14 G66 G66.1
User macro modal call
G67 User macro modal call Cancel
15 G40.1 Normal line control cancel G41.1 G42.1
Normal line control (P29)(*12) (P29)(*12)
16 G68 Coordinate rotation by program ON 3-dimensional coordinate conversion ON (P922) (P921)
G68.2 G68.3
Inclined surface machining command (*12) (*12)
G69 Coordinate rotation cancel 3-dimensional coordinate conversion OFF
17 G96 Constant surface speed control ON G97 Constant surface speed control OFF
18 G15 Polar coordinate command OFF G16 Polar coordinate command ON
19 G50.1 Mirror image OFF G51.1 Mirror image ON
21 G07.1 Cylindrical interpolation (P34) (P481) G12.1 Polar coordinate interpolation ON (P34) (P481) G13.1 Polar coordinate interpolation OFF
27 G54.4P0 Workpiece installation error compensation cancel G54.4 P1 - P7
Workpiece installation error compensation (*12) (*12)
Group G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
663 IB-1501278-P
(*12) In M80 Type B, the following program errors occur depending on the G codes.
Column A: Operation when the additional function is commanded while the high-speed machining mode II is enabled Column B: Operation when the high-speed machining mode II (G05P2) is commanded while the additional function is enabled : The high-speed machining mode II and the additional function are both enabled : The high-speed machining mode II is temporarily canceled, while the additional function is enabled x: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination : Others
(*1) Enables the high-speed machining mode II in a subprogram.
(*2) Enables the high-speed machining mode II if G05P2 is commanded in a subprogram.
(*3) Enables timing synchronization.
(*4) Enables the high-speed machining mode II in a MTB program.
(*5) Enables the high-speed machining mode II if G05P2 is commanded in a MTB program.
(*6) Enables the high-speed machining mode II in an interrupt program.
(*7) Enables the high-speed machining mode II if G05P2 is commanded in an interrupt program.
(*8) Disables the high-speed machining mode II in a figure rotation subprogram.
(*9) The high-speed machining mode II is disabled even if G05P2 is commanded in a figure rotation subprogram.
(*10) In M80 Type B, the following program error occurs depending on the function type.
G code Program error G code Program error
G05.1Q2, G92.1, G122, G61.2, G61.4
P39 G10 I_J_/G10 K_ P260 G06.2 P550
G144, G54.4 P1 - P7 P34 G93 P124 G07 P80 G41.1, G42.1 P900 G02.1, G03.1 P73 G43.1 P930 G02.3, G03.3 P611 G43.4, G43.5 P940 G02.4, G03.4 P76 G68.2, G68.3 P950
Relationship between the high-speed machining mode II and functions other than G codes
Function name A B
SSS ON - Mirror image by parameter setting ON - Mirror image by external input ON - Coordinate rotation by parameter - Subprogram call (M98) (*1) (*2) Figure rotation (M98 I_J_K_) (*8)(*10) (*9)(*10) Timing synchronization between part systems (*3) - Machine tool builder macro (*4) (*5) Macro interruption (*6) (*7) Corner chamfering/Corner rounding - Linear angle command - Geometric command (P33) - Chopping Fairing/Smooth fairing ON Optional block skip -
Function Program error
Figure rotation (M98 I_J_K_) P250
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
664IB-1501278-P
(1) If "G05 P1(P2)" is commanded when the high-speed machining mode I/(II) specifications are not provided, a pro- gram error (P39) occurs.
(2) The automatic operation process has priority in high-speed machining mode I/II, and as a result, the screen dis- play may slow down.
(3) The speed will decelerate once at the G05 command block, so turn ON and OFF when the tool separates from the workpiece.
(4) When carrying out operations in high-speed machining mode I/II by communication or tape mode, the machining speed may be suppressed depending on the program transmission speed limit.
(5) Command G05 alone in a block. (6) A decimal point is invalid for the P address in the G05 command block. (7) The P addresses, which are valid in the G05 command block, are P0, P1 and P2 only.
If other P addresses are commanded, a program error (P35) occurs. If there is no P command, a program error (P33) occurs.
(8) The machining speed may be suppressed depending on the number of characters in one block.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
665 IB-1501278-P
17.2 High-accuracy Control 17.2.1 High-accuracy Control ; G61.1, G08
Machining errors caused by delays in control systems can be inhibited. This function is useful for machining which needs to make an edge at a corner or reduce an error from an inner route of curved shape. In high-accuracy control, acceleration/deceleration is performed not to cause machining error by pre-reading blocks and acceleration/decel- eration is automatically performed according to a machining shape so that the machining error is inhibited with min- imizing an extension of machining time.
Commands to enable high-accuracy control are as follows: High-accuracy control command (G08P1/G61.1) High-speed high-accuracy control I command (G05.1Q1) High-speed high-accuracy control II/III command (G05P10000/G05P20000) High-accuracy spline interpolation command (G61.2)
This function uses the following functions to minimize the increase in machining time while reducing the shape error.
(1) Acceleration/deceleration before interpolation (2) Optimum speed control (3) Vector accuracy interpolation (4) Feed forward (5) S-pattern filter control In the main text, the axis address refers to the address of an axis that exits on the machine. It corresponds to the address designated in the parameters "#1013 axname" and "#1014 incax". These parameter settings depend on the MTB specifications.
Function and purpose
High-accuracy control OFF
NC command NC command
Machining program commanded shape
Machining program commanded shape Machining program commanded shape
Machining program commanded shape
Corner shape
Curve shape
High-accuracy control ON
NC command
NC command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
666IB-1501278-P
High-accuracy control can be canceled with either command regardless of the command that has enabled the con- trol.
(1) After "G08 P1" is commanded, G code group 13 is automatically switched to the G61.1 modal. If the high-accuracy control mode is canceled by the "G08 P0" command, G code group 0 is switched to the "G08P0" modal and G code group 13 becomes the "commanded mode".
Command format
High-accuracy control valid
G61.1 ;
or, G08 P1;
High-accuracy control invalid
G08 P0;
or, G command in G code group 13 except G61.1
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
667 IB-1501278-P
(1) Feedrate command F is clamped with the "#2110 Clamp (H-precision)" (Cutting feed clamp speed for high-ac- curacy control mode) set with the parameter.
(2) Rapid traverse rate enables "#2109 Rapid(H-precision)" (Rapid traverse rate during high-accuracy control mode) set by the parameter.
(3) When the "#2109 Rapid(H-precision)" is set to "0", the movement follows "#2001 rapid" (rapid traverse rate) set by the parameter. Also, when "#2110 Clamp (H-precision)" is set to "0", the speed will be clamped with "#2002 clamp" (Cutting clamp speed) set with parameter.
(4) The modal holding state of the high-accuracy control mode depends on the MTB specifications (combination of the parameters "#1151 rstint" (reset initial) and "#1148 I_G611" (initial high-accuracy)).
Hold: Modal hold
ON: Switches to the high-accuracy control mode
As for G61.1, the mode is switched to the high-accuracy mode, even if the other modes (G61 to G64) are valid.
OFF: The status of the high-accuracy control mode is OFF.
Detailed description
Parameters Default state Resetting
Reset initial (#1151)
Initial high-ac- curacy (#1148)
Power ON Reset 1 Reset 2 Reset & rewind
OFF OFF OFF Hold OFF ON OFF OFF ON ON Hold ON ON ON
Parameters Emergency stop Emergency stop cancel
Reset initial (#1151)
Initial high-ac- curacy (#1148)
Emergency stop switch or exter- nal emergency stop
Emergency stop switch or exter- nal emergency stop
OFF OFF Hold Hold ON OFF OFF ON Hold Hold ON ON
Parameters Block interrup- tion
Block stop NC alarm OT
Reset initial (#1151)
Initial high-ac- curacy (#1148)
Mode change- over (automatic/
manual) or
feed hold
Single block Servo alarm H/W OT
OFF OFF Hold ON
OFF ON
ON
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
668IB-1501278-P
Acceleration/deceleration control is carried out for the movement commands to suppress the impact and to smooth out the velocity waveform when the machine starts or stops moving. However, if high-accuracy control is disabled, the corners at the block seams are rounded, and path errors occur regarding the command shape because accel- eration/deceleration is performed after interpolation. In the high-accuracy control function mode, acceleration/deceleration is carried out before interpolation to solve the above problems. This acceleration/deceleration before interpolation enables machining with a faithful path to the commanded shape of the machining program. Furthermore, the acceleration/deceleration time can be reduced because the constant-gradient acceleration/decel- eration is performed for the acceleration/deceleration before interpolation.
(1) Basic patterns of acceleration/deceleration control in linear interpolation commands
Acceleration/deceleration before interpolation
Acceleration/deceleration waveform pattern
Normal mode (a) Because of the acceleration/deceleration that controls the acceleration time to achieve the commanded speed at a con- stant level (acceleration/deceleration with fixed time constant), the acceleration/de- celeration becomes more gentle as the command speed becomes slower (the ac- celeration/deceleration time does not change).
(b) The time to achieve the commanded speed (G1tL) can be set independently for each axis. Note, however, that an arc shape will be distorted if the time constant differs among the base axes.
G1tL: G1 time constant linear (MTB-specified parameter #2007)
High-accuracy con- trol mode
(F) Resultant speed (T) Time
(a) Because of the acceleration/deceleration that controls the acceleration time to achieve the maximum speed (G1bF) set by a parameter at a constant level (con- stant-gradient type linear acceleration/de- celeration), the acceleration/deceleration time is reduced as the command speed becomes slower.
(b) Only one acceleration/deceleration time constant (common for each axis) exists in a system.
G1bF: Maximum speed (MTB-specified parameter #1206) G1btL: Time constant (MTB-specified parameter #1207)
fying the gradient of the acceleration/ deceleration time. The actual cutting feed maximum speed is clamped by the "#2002 clamp" value.
clamp
G1tL
(T)
(F)
clamp
G1btL/2
G1bF
G1bF/2
G1btL
(T)
(F)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
669 IB-1501278-P
(2) Path control in circular interpolation commands When commanding circular interpolation with the conventional "acceleration/deceleration after interpolation" control method, the path itself that is output from the NC to the servo runs further inside the commanded path, and the circle radius becomes smaller than that of the commanded circle. This is due to the influence of the smoothing course droop amount for NC internal acceleration/deceleration.
With the pre-interpolation acceleration/deceleration control method, the path error is eliminated and a circular path faithful to the command results, because interpolation is carried out after the acceleration/deceleration con- trol. Note that the tracking lag due to the position loop control in the servo system is not the target here.
The following shows a comparison of the circle radius reduction error amounts for the conventional "acceleration/ deceleration after interpolation" control and pre-interpolation acceleration/deceleration control in the high-accu- racy control mode.
If an arc is commanded by a machining program as shown above, the error R occurs for the commanded shape on the actual tool path. In the normal mode (acceleration/deceleration after interpolation), R is caused by ac- celeration/deceleration of NC and lag of servo system. High-accuracy control (acceleration/deceleration before interpolation), however, can eliminate errors caused by acceleration/deceleration of NC. By additionally using the feed forward control, it is also possible to reduce errors caused by lag of servo system.
The compensation amount of the circle radius reduction error (R) is theoretically calculated as shown in the following table.
Ts: Acceleration/deceleration time constant in the NC (s) Tp: Servo system position loop time constant (s) (inverse number to "#2203 PGN1") Kf: Feed forward coefficient Kf = fwd_g / 1000 (fwd_g: #2010 Feed forward gain)
Machining program commanded shape
Actual tool path
R: Commanded radius (mm) R: Circle radius reduction error amount (mm) F: Cutting feedrate (mm/min)
"Acceleration/deceleration after interpolation" control (normal mode)
"Pre-interpolation acceleration/deceleration" control (high-accuracy control mode)
Linear acceleration/deceleration
Exponential function acceleration/deceleration
Linear acceleration/deceleration
(a) Because the item Ts can be ignored by using the
pre-interpolation acceleration/deceleration con- trol method, the radius reduction error amount can be reduced.
(b) Item Tp can be negated by making Kf = 1.
R
R
F
R = Ts 2 + Tp2 1 12
1 2R
F 60
2
R = Ts2 + Tp2 1 2R
F 60
2
R = Tp2 1 - Kf 2 1 2R
F 60
2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
670IB-1501278-P
When "#1205 G0bdcc" (G0 pre-interpolation acceleration/deceleration) is "1", pre-interpolation acceleration/decel- eration is also enabled for rapid traverse movement. In this case, acceleration/deceleration control is performed so that the acceleration rate of each axis does not exceed the gradient determined by parameters "#2001 rapid" (rapid traverse rate) and "#2004 G0tL" (G0 time constant (linear)).
(a) Velocity waveform of pre-interpolation acceleration/deceleration
(b) Velocity waveform of acceleration/deceleration after interpolation
(c) Gradient of pre-interpolation acceleration/deceleration
(F) Speed
(T) Time
When the gradient of each axis is different, the most moderate gradient among them is used in pre-interpolation acceleration/deceleration. Because acceleration/deceleration control is performed with a constant gradient, the positioning time for a G00 fine- segment block is reduced.
(1) When "#1086 G0Intp" (G00 non-interpolation) is "1", acceleration/deceleration after interpolation is applied to G00.
(2) When "#8090 SSS ON" is "1", pre-interpolation acceleration/deceleration is applied to G00 regardless of the set- ting in "#1205 G0bdcc" (Acceleration and deceleration before G0 interpolation).
(3) When "#1569 SfiltG0" (G00 soft acceleration/deceleration filter) is set to a value other than "0", cycle time may become longer when pre-interpolation acceleration/deceleration is applied to linear acceleration/deceleration than when acceleration/deceleration after interpolation is applied.
(a) Velocity waveform of pre-interpolation acceleration/deceleration
(b) Velocity waveform of acceleration/deceleration after interpolation
(F) Speed
(T) Time
Rapid traverse pre-interpolation acceleration/deceleration
(F)
(T)
(a)
(b)
(c) #2001
#2004
Note
(F)
(T)
(a)
(b)
#2001
#2004 #1569
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
671 IB-1501278-P
When the moving direction is changed on the corner, arc, etc., acceleration rate corresponding to the amount of change and the feedrate is generated. When the acceleration rate is large, there is a possibility of machine vibration and it may leave stripes on the machining surface. In the high-accuracy control mode, the deceleration control (optimum speed control) is performed to keep the gen- erated acceleration rate under the allowance that has been designed with the parameter so that the problem men- tioned above can be solved. The optimum speed control suppresses the machine vibration and enables highly accurate machining while minimizing the extension of cycle time.
Corner deceleration Consists of optimum corner deceleration and axis-specific acceleration tolerance control.
Arc speed clamp Controls deceleration so that the combined acceleration rate on an arc is kept below the tolerable acceleration rate common to all axes. This can suppress path errors (circle radius reduction error amount) on an arc to a certain level.
(1) Optimum corner deceleration Highly accurate edge machining can be achieved by controlling deceleration so that the combined acceleration rate at the seam between blocks is kept under the tolerable acceleration rate common to all axes, which is de- termined by "#1206 G1bF" (maximum speed), "#1207 G1btL" (time constant), and accuracy coefficient. When entering in a corner, optimum speed for the corner (optimum corner speed) is calculated from the angle with the next block (corner angle) and the tolerable acceleration rate common to all axes. The machine decelerates to the speed in advance, and then accelerates back to the command speed after passing the corner.
Optimum speed control
When a corner with the corner angle is passed at speed F, the acceleration rate F occurs according to and F.
The corner speed F is controlled so that F generated above does not exceed the tol- erable acceleration rate common to all ax- es. The speed pattern is as shown on the left.
Y axis F : Speed before entering the corner
F : Speed after passing the corner
F : Acceleration rate at the corner
X axis
F0 =
F0x2
F0y2
F0x2 + F0y2
Time
Resultant speed
X-axis speed
Time
Time
Y-axis speed
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
672IB-1501278-P
Optimum corner deceleration is not carried out when blocks are smoothly connected, because deceleration is not necessary. The criteria for whether the connection is smooth or not can be designated by the machining pa- rameter "#8020 DCC ANGLE". If the corner angle is equal to or less than the corner deceleration angle, the con- nection is judged to be smooth and optimum corner deceleration is not carried out. The edge accuracy can be further improved by setting a greater accuracy coefficient. A greater accuracy coef- ficient, however, reduces the optimum corner speed, which may increase the cycle time. Setting a negative ac- curacy coefficient can increase the optimum corner speed and reduce the cycle time. As shown below, different accuracy coefficients can be used depending on the parameter "#8021 COM- P_CHANGE", and the tolerable acceleration rate common to all axes can be obtained with the following formula:
The corner speed V0 can be maintained at more than a certain speed so that the corner speed does not drop too far. Set "#2096 crncsp (corner deceleration minimum speed)" for each axis, and make a resultant speed so that the moving axis does not exceed this setting.
Note that the speed is controlled with the optimum corner deceleration speed in the following cases. When the combined corner deceleration speed is equal to or less than the optimum corner deceleration
speed When the corner deceleration minimum speed parameter setting for the moving axes is set to "0" for even
one axis.
#8021 COMP CHANGE Accuracy coefficient used
0 #8019 R COMP 1 #8022 CORNER COMP
Speed is not clamped Speed is clamped
(a) Corner deceleration speed (b) Clamp value according to X axis (c) Y axis setting value (d) X axis setting value
= G1bF (mm/min) / 60
100G1btL (ms) / 1000 Tolerable acceleration rate
for all axes (mm/s2)
100 - R COMP
V
(a)
(b)
(c)
(a)
(d)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
673 IB-1501278-P
(2) Axis-specific acceleration tolerance control (optimum acceleration control) The acceleration rate to be generated at a seem between blocks is evaluated for each axis to control decelera- tion so that the seam is passed at the optimum speed. This enables highly accurate edge machining. The optimum deceleration speed is calculated so that the acceleration rate of each axis to be generated at the seam is equal to or less than the tolerable acceleration rate for each axis, which is determined by "#2157 G1bFx" (maximum speed for each axis), "#2158 G1btLx" (time constant for each axis), and the accuracy coefficient. The machine decelerates to the speed in advance, and then accelerates back to the command speed after passing the corner. This control enables deceleration at an appropriate speed for the characteristics of each axis even when ma- chine vibrations may easily occur due to a low tolerable acceleration rate for a specific axis (rotary axis). This means that the deceleration speed can be raised at a corner where acceleration rate is generated only for an axis with a high tolerable acceleration rate, leading to a reduced cycle time. If acceleration rate is generated for the X axis (linear axis) as shown in Figure (a) below or for the C axis (rotary axis) as shown in Figure (b), the corner speed F is controlled so that the acceleration rate to be generated at the X or C axis does not exceed the tolerable acceleration rate for the X or C axis, respectively. If the tolerable ac- celeration rate for the X axis is higher than that for the C axis, a higher deceleration speed can be used for a path where acceleration rate is generated only for the X axis than where acceleration rate is generated only for the C axis. In this case, the speed patterns are as shown in Figures (c) and (d) below:
F0 =
F0x2
F0x2
F0c2
F0x2 + F0c2 F0 = F0x2 + F0y2
F0c2
F : Speed before entering the corner
(a) Corner shape which generates the acceleration rate on X axis (linear axis)
Controls the acceleration rate generated on X axis to be the X-axis tolerable acceleration rate or less.
Controls the acceleration rate generated on C axis to be the C-axis tolerable acceleration rate or less.
(b) Corner shape which generates the acceleration rate on C axis (rotary axis)
(c) Speed pattern which generates the acceleration rate on X axis (linear axis)
(d) Speed pattern which generates the acceleration rate on C axis (rotary axis)
F : Speed after passing the corner F : Speed before entering the corner
F : Speed after passing the cornerF :
Acceleration rate at the corner
X axis X axis F : Acceleration rate at the corner
Time Time
Time
Time
Time
Time
Resultant speed
X-axis speed
Resultant speed
X-axis speed
C-axis speed C-axis speed
C axis C axis
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
674IB-1501278-P
Deceleration is not carried out when blocks are smoothly connected (when the acceleration rate to be generated for each axis is equal to or lower than the tolerable acceleration rate for each axis). The edge accuracy can be further improved by setting a greater accuracy coefficient. A greater accuracy coefficient, however, reduces the optimum corner speed, which may increase the cycle time. Setting a negative accuracy coef- ficient can increase the optimum corner speed and reduce the cycle time. As shown below, different accuracy coefficients can be used depending on the parameter "#8021 COM- P_CHANGE". Also, the tolerable acceleration rate can be adjusted for each axis using "#2159 compx" (accuracy coefficient for each axis), and the tolerable acceleration rate for each axis can be obtained with the following formula. It is necessary, however, to set the same tolerable acceleration rate for all base axes because an arc shape is dis- torted if it differs among them. If G1bFx is "0" (not set), the tolerable acceleration rate is calculated using "#2001 rapid" (rapid traverse rate). And if G1btLx is "0" (not set), the tolerable acceleration rate is calculated using "#2004 G0tL" (G0 time constant (linear)). If G1bFx and G1btLx are 0 for all base axes, the tolerable acceleration rate for the base axes are unified to the lowest one.
#8021 COMP CHANGE Accuracy coefficient used
0 #8019 R COMP 1 #8022 CORNER COMP
= G1bFx (mm/min) / 60
100 100G1btLx (ms) / 1000
100 - compx Tolerable acceleration rate
for each axes (mm/s2)
100 - R COMP
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
675 IB-1501278-P
(3) Arc speed clamp During circular interpolation, even when moving at a constant speed, acceleration rate is generated as the ad- vance direction constantly changes. When the arc radius is large enough in relation to the commanded speed, control is carried out at the commanded speed. However, when the arc radius is relatively small, the speed is clamped so that the generated acceleration rate does not exceed the tolerable acceleration/deceleration speed before interpolation, calculated with the parameters.
This allows arc cutting to be carried out at an optimum speed for the arc radius.
The figure below shows the acceleration rate F (mm/s2) for movement at the constant speed F (mm/min) on an arc shape with the radius R (mm). Here, the arc clamp speed F' (mm/min) that makes the acceleration rate
F lower than the tolerable acceleration rate common to all axes Ac (mm/s2) can be obtained with the following formula:
When the above F' expression is substituted with F in the expression for the maximum logical arc radius reduc- tion error amount R, explained in the section "Pre-interpolation acceleration/deceleration", the commanded ra- dius R is eliminated, and R does not rely on R. Here, Tp is the servo system position loop time constant (s) and Kf is the feed forward coefficient. Tp is the inverse number to "#2203 PGN1" (position loop gain) (Tp = 1 / PGN1) and Kf is a ratio of "#2010 fws_g" (feed forward gain) (Kf = fwd_g / 100), both of which depend on the MTB specifications.
In other words, with an arc command to be clamped at the arc clamp speed, in logical terms regardless of the commanded radius R, machining can be carried out with a radius reduction error amount within a constant value. The roundness can be further improved by setting a greater accuracy coefficient. A greater accuracy coefficient, however, reduces the arc clamp speed, which may increase the cycle time. Setting a negative accuracy coeffi- cient can increase the arc clamp speed and reduce the cycle time. As shown below, different accuracy coefficients can be used depending on the parameter "#8021 COM- P_CHANGE", and the tolerable acceleration rate common to all axes can be obtained with the following formula:
F: Commanded speed (mm/min) R: Commanded arc radius (mm) : Angle change per interpolation unit F: Speed change per interpolation unit The tool is fed with the arc clamp speed F' so that F does not exceed the tolerable acceleration rate common to all axes Ac (mm/s2).
R : Arc radius reduction error amount Tp : Position loop gain time constant of servo system Kf : Feed forward coefficient F : Cutting feedrate
#8021 COMP CHANGE Accuracy coefficient used
0 #8019 R COMP 1 #8022 CORNER COMP
#8023 CURVE COMP
F
R
F
F
F
F
F'
F' = G1bF( mm/min)
G1btL(ms)
R*Ac*60
R Tp2 1 - Kf 2 1 2R
F 60
2
Tp2 1 - Kf 2 2
AC
= G1bF (mm/min) / 60
100G1btL (ms) / 1000 Tolerable acceleration rate
for all axes (mm/s2)
100 - R COMP
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
676IB-1501278-P
When a fine segment is commanded and the angle between the blocks is extremely small (when not using optimum corner deceleration), interpolation can be carried out more smoothly using the vector accuracy interpolation.
This function reduces path errors caused by delay of servo systems. Path errors caused by acceleration/decelera- tion of NC can be eliminated by acceleration/deceleration before interpolation, however errors caused by delay of servo systems cannot be eliminated by acceleration/deceleration before interpolation. Therefore, when the arc shape of radius R (mm) is machined at speed F (mm/min) as the figure (a)below, for instance, the lag time occurs between the NC commanded speed and the actual tool speed in amount of the servo system time constant and the path error R (mm) occurs. Feed forward control generates the command value taking the delay of servo systems as shown in figure (b)below so that the path error caused by delay of servo systems can be inhibited.
(a) NC command and actual tool movement during Feed forward control OFF
Vector accuracy interpolation
Vector accuracy interpolation Commanded path
Feed forward control
R R
F
NC commanded speed
NC commanded shape
Actual tool path
Actual tool speed
Delay of servo
Time
Speed
NC commanded shape
Actual tool speed (corresponding to original NC commanded speed)
Actual tool path
NC commanded speed is set forward according to a expected delay. (Feed forward control)
Time
Speed
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
677 IB-1501278-P
(b) NC command and actual tool movement during Feed forward control ON
Here, Tp is the servo system position loop time constant (s) and Kf is the feed forward coefficient. Tp is the in- verse number to "#2203 PGN1" (position loop gain) (Tp = 1 / PGN1) and Kf is a ratio of "#2010 fws_g" (feed forward gain) (Kf = fwd_g / 100), both of which depend on the MTB specifications.
Combination with the smooth high gain (SHG) control function
Feed forward control can inhibit path errors more effectively by increasing the feed forward coefficient. In some cases, however, the coefficient cannot be increased because a greater coefficient may cause machine vibra- tions. In this case, use this function together with the smooth high gain (SHG) control function to stably compen- sate path errors caused by lag of servo system. To enable the SHG control, it is also necessary to set "#2204 PGN2" (position loop gain 2) and "#2257 SHGC SHG" (control gain) in addition to "#2203 PGN1" (position loop gain 1), all of which depend on the MTB specifi- cations. By enabling the SHG control, it is possible to inhibit path errors, for example, for an arc shape equiva- lently as with conventional control (SHG control OFF) using the equivalent feed forward gain fwd_g as shown in the following formula. This means that setting fwd_g = 50 (%) for the SHG control is as effective as setting fwd_g = 100 (%) for conventional control in inhibiting path errors.
=R F 2R 60 1
Tp 1 - Kf
fwd _ g' = 100 100 2
fwd _ g 1 1 - 1 -
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
678IB-1501278-P
S-pattern filter (soft acceleration/deceleration filter) is the function that inhibits the machine vibration by smoothing a velocity waveform. There are following types of S-pattern filters:
G01/G00 S-pattern filter G01/G00 jerk filter S-pattern filter 2
(1) G01/G00 S-pattern filter This function inhibits the machine vibration by smoothing a velocity waveform generated by constant-gradient linear acceleration/deceleration. Constant-gradient linear acceleration/deceleration generates continuous velocity waveforms, but makes the ac- celeration rate discontinuous. As a result, machine vibrations may easily occur when there are discontinuities in acceleration rate, which may cause scratches or streaks on the machining surface. The S-pattern filter can make the velocity waveform even smoother and eliminate acceleration rate discontinuities to inhibit machine vibra- tions. The S-pattern filter does not impair machining accuracy because it makes the combined speed smoother before interpolation. A greater S-pattern filter time constant, however, may increases the cycle time. To the S-pattern filter time constant, "#1568 SfiltG1" is applied during cutting feed (G01) or "#1569 SfiltG0" during rapid traverse (G00), each of which can be set in the range of 0 to 200 (ms).
(2) G01/G00 jerk filter The jerk filter function inhibits machine vibrations by eliminating jerk discontinuities when the S-pattern filter alone cannot inhibit such vibrations. Through the S-pattern filter, continuous velocity waveforms can be obtained up to acceleration rate, but jerk dis- continuities remain. The jerk filter further filters the velocity waveform smoothed by the S-pattern filter to smooth jerk as well to inhibit machine vibrations. The jerk filter does not impair machining accuracy because it makes the combined speed smoother before interpolation. To the jerk filter time constant, "#12051 Jerk_filtG1" is applied during cutting feed (G01) or "#12052 Jerk_filtG0" during rapid traverse (G00), each of which can be set in the range of 0 to 50 (ms). Even if a jerk filter time con- stant is set, the S-pattern filter time constant is the time to achieve the target acceleration rate. As a result, the time constant for S-pattern filter processing is "S-pattern filter time constant" - "Jerk filter time constant". If the jerk filter time constant is the same as or greater than the S-pattern filter time constant, an MCP alarm (Y51 0030) will occur.
S-pattern filter control
Time
S-pattern filter 2
Interpolation (axis distribution)
Constant-gradient linear acceleration/ deceleration
Resultant speed
Resultant speed
Resultant speed
Time Time Time
Axis speed
Time
Time
Axis speed
Time
Axis speed
Axis speed
Jerk filter
Smoothing velocity waveform of constant-gradient linear acceleration/deceleration
Making velocity waveform of S-pattern filter even smoother
Smoothing each axis speed after interpolation
S-pattern filter
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
679 IB-1501278-P
(3) S-pattern filter 2 This function inhibits machine vibrations by smoothing slight speed fluctuation caused when the combined speed is distributed to each axis element. S-pattern filter 2 can inhibit machine vibrations by smoothing slight speed fluctuation on each axis. The function, however, may impair machining accuracy because it filters each axis speed after interpolation. A greater S-pat- tern filter 2 time constant, however, may increases the cycle time. To the S-pattern filter 2 time constant, "#1570 Sfilt2" is applied, which can be set in the range of 0 to 200 (ms).
(4) How to adjust parameters (a) The table below shows typical initial values for each filter time constant. If your machine's natural angular
frequency fn (Hz) is known, vibrations can be inhibited effectively by setting the vibration period Tn (ms) ob- tained with the following formula for the S-pattern filter time constant:
(b) If vibrations cannot be inhibited properly with the above initial values, increase the S-pattern filter time con- stant. Or, decrease the S-pattern filter time constant to reduce the cycle time.
(c) If vibrations occur at a corner or other section and stripes remain on the machining surface even after the S- pattern filter time constant is increased, increase the S-pattern filter 2 time constant. The maximum S-pattern filter 2 time constant, however, should be 20 to 25 ms because a greater S-pattern filter 2 time constant may impair machining accuracy.
(d) If high-frequency machine vibrations remain even after the S-pattern filter/S-pattern filter 2 are applied, set the jerk filter time constant.
If a shorter cycle time has a priority over the machining accuracy, it is possible to inhibit vibrations at a corner by reducing the corner accuracy coefficient to increase the corner deceleration speed and increasing the S-pattern filter 2 time constant.
Tsfilt: S-pattern filter time constant Tjerk: Jerk filter time constant
S-pattern filter Jerk filter S-pattern filter
(SfiltG1/SfiltG0) (Jerk_filtG1/Jerk_filtG0) (Sfilt2)
50ms 0ms 10ms
Tsfilt - Tjerk Tsfilt
Tjerk
Constant-gradient linear acceleration/deceleration
Machine vibration is likely to occur
S-pattern filter Jerk filter
Time
Speed
Acceleration rate
Jerk
Jerk Jerk
Acceleration rate Acceleration rateTime Time
Time
Time
Time
Time
Time
Time
Speed Speed
=Tn fn
1000 (ms)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
680IB-1501278-P
(1) The modal must be set as shown below when commanding G08 P1/G61.1.
(*1) These functions can be commanded if the axis-specific acceleration tolerance control (optimum acceleration control) or variable-acceleration pre-interpolation acceleration/deceleration specification is valid.
(2) A program error will occur if high-accuracy control is commanded in the following modes. During milling -> Program error (P481) (*2) During cylindrical interpolation -> Program error (P481) (*2) During polar coordinate interpolation -> Program error (P481) (*2) During normal line control -> Program error (P29)
(3) A program error will occur if the following commands are issued during the high-accuracy control mode. Milling -> Program error (P126) (*2) Cylindrical interpolation -> Program error (P126) (*2) Polar coordinate interpolation -> Program error (P126) (*2) Normal line control -> Program error (P29) (*2) An error will not occur if the axis-specific acceleration tolerance control (optimum acceleration control) or
variable-acceleration pre-interpolation acceleration/deceleration specification is valid.
Relationship with other functions
Function G code
Cylindrical interpolation cancel (*1) G07.1 Polar coordinate interpolation cancel (*1) G15 Normal line control cancel G40.1 Programmable mirror image OFF G50.1 Mirror image with settings Cancel Mirror image with signals Cancel No macro modal call G67 Feed per revolution cancel G94 Constant surface speed control mode cancel G97 Interruption type macro mode cancel M97
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
681 IB-1501278-P
The table below shows operations when following high-accuracy control-related commands are combined:
Operation when high-accuracy control-related G commands are combined
G61.1, G8P1 : High-accuracy control G64 : Cutting mode G61 : Exact stop check mode G62 : Automatic corner override G63 : Tapping mode G61.2 : High-accuracy spline interpolation G08P0 : High-accuracy control cancel (cutting mode) G05.1Q1 : High-speed high-accuracy control I G05.1Q2 : Spline interpolation G05P2 : High-speed machining mode II G05P10000 : High-speed high-accuracy control II G05P20000 : High-speed high-accuracy control III
A B Operation when B is commanded during A command
G61.1/G08P1 G61.1 Continues high-accuracy control. G61,G62,G63,G64 Cancels high-accuracy control and operates in the commanded mode. G61.2 Operates in the high-accuracy spline interpolation mode. G8P1 Continues high-accuracy control. G8P0 Cancels high-accuracy control. (Changes G code group 13 to G64.) G05.1Q1 Operates in the high-speed high-accuracy control I mode. G05.1Q2 A program error (P34) will occur. G05P2 Operates in high-accuracy control + high-speed machining mode II. G05P10000 Operates in the high-speed high-accuracy control II mode. G06.2 A program error (P34) will occur.
G61.2 G61.1 Operates in the high-accuracy control mode. G61,G62,G63,G64 Operates in the commanded mode. G61.2 Continues high-accuracy spline interpolation. G08P1 Operates in the high-accuracy control mode. G08P0 A program error (P29) will occur. G05.1Q1 A program error (P29) will occur. G05.1Q2 A program error (P34) will occur. G05P2 Operates in high-accuracy spline interpolation + high-speed machining
mode II. G05P10000 A program error (P29) will occur. G06.2 A program error (P34) will occur.
G05.1Q1 G61.1 Continues the high-speed high-accuracy control I mode. G64 Continues the high-speed high-accuracy control I mode. G61,G62,G63 Operates in the high-speed high-accuracy control I + commanded mode. G61.2 A program error (P29) will occur. G08P1 Continues the high-speed high-accuracy control I mode. G08P0 Continues the high-speed high-accuracy control I mode. G05.1Q1 Continues the high-speed high-accuracy control I mode. G05.1Q2 A program error (P34) will occur. G05P2 Operates in the high-speed machining mode II. G05P10000 A program error (P34) will occur. G06.2 A program error (P34) will occur.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
682IB-1501278-P
The acceleration rate of either the cutting feed (G01) or the rapid traverse (G00) can be used for the rapid traverse (G00) in the high-accuracy control mode during the tool center point control, workpiece installation error compensa- tion, or inclined surface machining command. Which acceleration rate is used depends on the MTB specifications (parameter "#1250 set22/bit3").
Normally, the acceleration rate of the cutting feed (G01) is used and the acceleration rate in the route direction be- comes constant. If the acceleration rate of the rapid traverse (G00) is used, the acceleration rate can be changed to suit the responsiveness of the moving axis, and also the cycle time can be reduced compared to that of the cutting feed (G01). The figure below shows the relationship between parameters and speed waveforms (when the respon- siveness of the linear axis is higher than that of the rotary axis).
(a) Acceleration rate of rapid traverse (G00)
(b) Acceleration rate of cutting feed (G01)
When at least one of the functions shown in the table below is commanded, positioning is performed with the accel- eration rate of the rapid traverse (G00) in the following conditions:
(1) The parameter "#1250 set22/bit3" is set to "1". (2) SSS control is being executed.
If the above conditions are not satisfied, the system runs with the acceleration rate of the cutting feed (G01).
G05P10000 G61.1 Continues the high-speed high-accuracy control II mode. G64 Continues the high-speed high-accuracy control II mode. G61,G62,G63 Operates in the high-speed high-accuracy control II + commanded
mode. G61.2 A program error (P29) will occur. G08P1 Continues the high-speed high-accuracy control II mode. G08P0 Continues the high-speed high-accuracy control II mode. G05.1Q1 A program error (P34) will occur. G05.1Q2 Operates in the high-speed high-accuracy control II mode + spline inter-
polation G05P2 Operates in the high-speed machining mode II. G05P10000 Continues the high-speed high-accuracy control II mode. G06.2 Operates in the NURBS interpolation mode.
Rapid traverse acceleration rate switching during tool center point control, workpiece installation error com- pensation, or inclined surface machining command
Resultant speed
Time
During tool center point control
Function Instruction (G code)
Tool center point control G43.4, G43.5 Workpiece installation error compensation G54.4 Inclined surface machining command G68.2, G68.3
A B Operation when B is commanded during A command
N2 N1
(a) #1250/bit3=1
(b) #1250/bit3=0
G43.4 H1 ; N1 G00 C10. ; N2 G00 X10. ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
683 IB-1501278-P
The table below shows the rapid traverse acceleration/deceleration patterns and acceleration rate designation meth- ods under the SSS control. The acceleration rate is calculated based on the designated parameters to perform op- erations. Designate the parameters to determine the rapid traverse acceleration rate, referring to the table below.
(*) When "#2109 Rapid(H-precision)" (rapid traverse rate for high-accuracy control mode) is set to "0", "#2001 rapid" is used.
#1250 bit3
Functions in the table above
Rapid traverse constant-gradi- ent multi-step
acceleration/de- celeration
Acceleration/decel- eration pattern
Acceleration rate designation method
0 Not commanded. Invalid Constant-gradient ac- celeration/decelera- tion
Designated with the parameters "#2001 Rapid" and "#2004 G0tL".
Valid Constant-gradient multi-step accelera- tion/deceleration
Follows the rapid traverse constant-gradi- ent multi-step acceleration/deceleration specifications.
Commanded. Invalid/Valid Constant-gradient ac- celeration/decelera- tion
Designated with the parameters "#1206 G1bF" and "#1207 G1btL".
1 Not commanded. Invalid Constant-gradient ac- celeration/decelera- tion
Designated with the parameters "#2001 Rapid" and "#2004 G0tL".
Valid Constant-gradient multi-step accelera- tion/deceleration
Follows the rapid traverse constant-gradi- ent multi-step acceleration/deceleration specifications.
Commanded. Invalid/Valid Constant-gradient ac- celeration/decelera- tion
Designated with the parameters "#2001 Rapid" and "#2004 G0tL".
Speed
Time
#2109 Rapid(H-precision) (*)
#2001 Rapid, #1206 G1bF
#2004 G0tL, #1207 G1btL #2004 G0tL, #1207 G1btL
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
684IB-1501278-P
The following describes the relationship between the setting values of the parameter "#1250 set22/bit3" and the ap- plied acceleration rate using two operation examples (resultant speed waveform). The major parameters are as fol- lows.
(1) Acceleration/deceleration pattern when "#1250 bit3" is set to "0"
N1: Runs with the acceleration rate calculated from "#2001" and "#2004" of the X axis.
N2-N4: Runs with the acceleration rate calculated from "#1206" and "#1207".
(2) Acceleration/deceleration pattern when "#1250 bit3" is set to "1"
N1: Runs with the acceleration rate calculated from "#2001" and "#2004" of the X axis.
N2-N4: Runs with the acceleration rate calculated from "#2001" and "#2004" of each axis. (Calculate the optimum acceleration rate within the range in which the acceleration of each axis does not exceed the setting.)
Parameters Description Setting value
#1205 G0bdcc G0 acceleration/deceleration before interpo- lation
1
#1206 G1bF Maximum speed (mm/min) 10000 #1207 G1btL Time constant (ms) 500 #8090 SSS ON SSS control ON/OFF 1 #2001 Rapid Rapid traverse rate (X axis) 30000 (C axis) 20000 #2004 G0tL G0 time constant (linear) (X axis) 100 (C axis) 500
Resultant speed G91G61.1; N1 G00 X10.; G43.4 H1; N2 G00 C10.; N3 G00 X10.; N4 G00 X10. C1.;
Time
During tool center point control
Resultant speed G91G61.1; N1 G00 X10.; G43.4 H1; N2 G00 C10.; N3 G00 X10.; N4 G00 X10. C1.;
Time
During tool center point control
N1 N2 N3 N4
N1 N3 N4 N2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
685 IB-1501278-P
(1) The "high-accuracy control" specifications are required to use this function If G61.1 is commanded when there are no specifications, a program error (P123) will occur.
(2) "G08P1" must be commanded alone in a block, which also applies to "G08P0". (3) The high-accuracy control function is internally enabled by the high-speed high-accuracy I/II/III (G5.1Q1/
G5P10000) command. If the high-speed high-accuracy I/II/III is commanded in the high-accuracy control mode, the high-speed high-accuracy I/II/III mode is enabled. Then, if the high-speed high-accuracy I/II/III mode is can- celed, the high-accuracy control mode is restored.
(4) In the high-accuracy control mode, feedrate command F is clamped with the "#2110 Clamp (H-precision)" (Cut- ting feed clamp speed for high-accuracy control mode) set with parameter. When the cutting feed clamp speed for the high-accuracy control mode is 0, however, it is clamped with the "#2002 clamp" cutting clamp speed set by the parameter.
(5) In the high-accuracy control mode, rapid traverse rate conforms to "#2109 Rapid(H-precision)" (Rapid traverse rate during high-accuracy control mode) set by the parameter. When the rapid traverse rate during the high-ac- curacy control mode is set to "0", however, the movement follows "#2001 rapid" set by the parameter.
(6) If the specifications for the multi-part system simultaneous high-accuracy control are not provided, the "#1205 G0bdcc" (G0 pre-interpolation) can be used with only one part system. If the 2nd or later part system is set to the G0 pre-interpolation acceleration/deceleration, an MCP alarm (Y51 0017) will occur.
(7) When there are high-accuracy acceleration/deceleration time constant expansion specifications, the sampling buffer area may be smaller.
(8) The high-accuracy control time constant expansion specifications can only be used for a 1-part system. In a multi-part system, the high-accuracy acceleration/deceleration time constant expansion specifications are dis- abled even when they are set to ON.
(9) For a part system where high-accuracy control is to be commanded, set the number of axes in the part system to 8 or less. If high-accuracy control is commanded for a part system that has 9 or more axes, an operation error (M01 0135) will occur. The error will not occur, however, if the number of axes in the part system excluding the master axis/slave axis is 8 or less during the synchronous control/control axis synchronization between part sys- tems.
(10) Even if the parameter "#1210 RstGmd" (modal G code reset setting) is set to "not to initialize group 13 at reset", group 13 is initialized according to the setting of "#1148 I_G611" (Initial hi-precis) if it is enabled. To retain group 13 at reset, set "#1148 I_G611" to "0". These parameters depend on the MTB specifications.
(11) If the parameter "#1205 G0bdcc" (G0 acceleration/deceleration before interpolation) is set to "1", the value set with the parameter "#2224 SV024" (in-position detection width) will be used as the in-position width. The setting of the parameter "#2077 G0inps" (G0 in-position width) and the programmable in-position check with ",I" address are disabled.
(12) When SSS is enabled, the feedrate is controlled so that it will be the optimum value based on the global path information. This means that the actual feedrate may be different from the speed commanded in the machining program.
(13) When the "Manual/Automatic simultaneous valid n-th axis" signal (Y920) is changed during the execution of the movement blocks for the pre-interpolation acceleration/deceleration, the change will not be enabled immediately even if the axis is not moving. The change is enabled when all the axes in the part system decelerate and stop.
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
686IB-1501278-P
17.2.2 SSS Control
This function runs a machining program that approximates a freely curved surface with fine segment lines at high speed and with high-level accuracy. This function enables machining with less scratches and streaks on the cutting surface compared to the conventional high-accuracy control function.
With conventional high-accuracy control, the angle between two blocks is compared with the corner deceleration angle to determine whether to execute corner deceleration between the blocks. This can cause the speed to sud- denly change between the blocks with an angle close to the corner deceleration angle, resulting in scratches or streaks.
The SSS (Super Smooth Surface) control uses information on not only the angle between two blocks but also global paths to provide optimum speed control that is not significantly affected by minute stepping or waviness. The favor- able effects of this control include a reduction in the number of scratches or streaks on cutting surfaces. The SSS control has the following features:
(1) This function is effective at machining smooth-shaped dies using a fine segment program. (2) This function provides speed control that is not susceptible to errors in paths. (3) Even if corner deceleration is not required, the speed is clamped if the predicted acceleration is high.
(The clamp speed can be adjusted using the parameter "#8092 ClampCoeff".)
The length of the path direction recognized with SSS control can be adjusted with the machining parameter "#8091 reference length". The range is increased as the setting value increases, and the effect of the error is reduced. If the multi-part system simultaneous high-accuracy specification is provided, up to two part systems can be used at the same time.
(1) The use of this function requires the following functions, in addition to the SSS control specifications. Make sure that these specifications are enabled before using this function. High-accuracy control (G61.1/G08P1) High-speed high-accuracy control I (G05.1 Q1) High-speed high-accuracy control II (G05 P10000) High-speed high-accuracy control III (G05 P20000)
Function and purpose
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
687 IB-1501278-P
When the parameters are set as below, each of the following high-accuracy control commands is activated under SSS control.
"#8090 SSS ON" ON
"SSS" is displayed on the modal display screen under SSS control. However "SSS" is not displayed when a command being executed is out of the scope of SSS control.
The clamp speed at a corner and arc can be adjusted using "#8022 CORNER COMP" and "#8023 CURVE COMP" (If "#8021 COMP_CHANGE" is set to "0", use "#8019 R COMP" to adjust the clamp speed at a corner and arc). When "#8096 Deceler. coeff. ON" is set to "1", "#8097 Corner decel coeff" and "#8098 Arc clamp spd coef" become valid during SSS control. Using these parameters, you can use different corner deceleration speeds and clamp speeds at arcs according to whether or not the SSS control is enabled. For parameters #8097 and #8098, respectively, set a percentage ratio to the level of the relevant speed that is ap- plied when the SSS control is disabled.
(Example) When "#8097 Corner decel coeff" is set to 200 (%), the corner deceleration speed that is applied when the SSS control is enabled becomes twice the corner deceleration speed that is applied when the SSS control is disabled.
When setting the parameters, adjust the values within the range in which the machine does not vibrate.
Detailed description
[High-accuracy control] G61.1 ; or G08P1; High-accuracy control ON G08P0; or, G command in group 13 except G61.1 High-accuracy control OFF
[High-speed high-accuracy control I] G05.1 Q1 ; High-speed high-accuracy control I ON G05.1 Q0 ; High-speed high-accuracy control I OFF
[High-speed high-accuracy control II] G05 P10000 ; High-speed high-accuracy control II ON G05 P0 ; High-speed high-accuracy control II OFF
[High-speed high-accuracy control III] G05 P20000 ; High-speed high-accuracy control III ON G05 P0 ; High-speed high-accuracy control III OFF
Adjustment of accuracy coefficient
Parameter Item to be adjusted
#8097 Corner decel coeff Corner deceleration speed to be applied when the SSS con- trol is enabled
#8098 Arc clamp spd coef Arc clamp speed to be applied when the SSS control is en- abled
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
688IB-1501278-P
The standard values of the parameters related to SSS control are shown below.
(1) User parameters
The relationship between each parameter, accuracy and speed is shown below. The accuracy and speed required for machining can be adjusted with these settings. When setting the parameters, adjust the values within the range in which the machine does not vibrate.
(2) Basic specification parameters (depend on the MTB specifications)
(3) Axis specification parameters (depend on the MTB specifications)
Parameter standard values
# Item Standard value
8090 SSS ON 1 8091 StdLength 1.000 8092 ClampCoeff 1 8093 StepLeng 0.005 8094 DccWaitAdd 0 8096 Deceler. coeff. ON 1 8097 Corner decel coeff 300 8098 Arc clamp spd coef 100 8019 R COMP 0 8020 DCC ANGLE 10 8021 COMP CHANGE 1 8022 CORNER COMP 0 8023 CURVE COMP -20 8034 AccClampt ON 0 8036 CordecJudge 0 8037 CorJudgeL 0
Parameter Adjustment target Effect
#8022 CORNER COMP Accuracy at corner section
Large setting = Accuracy increases, speed drops
#8023 CURVE COMP Accuracy at curve section
Large setting = Accuracy increases, speed drops
#8092 ClampCoeff Accuracy at curve section
Large setting = Accuracy drops, speed increases
"#8023".
# Item Standard value
1148 I_G611 Initial high-accuracy 0 1206 G1bf Acceleration/deceleration before interpolation Maximum speed - 1207 G1btL Acceleration/deceleration before interpolation Time constant - 1571 SSSdis SSS control adjustment coefficient fixed value selection 0 1572 Cirorp Arc command overlap 0 1568 SfiltG1 G1 soft acceleration/deceleration filter 0 1569 SfiltG0 G0 soft acceleration/deceleration filter 0 1570 Sfilt2 Soft acceleration/deceleration filter 2 0
# Item Standard value
2010 fwd_g Feed forward gain 70 2068 G0fwdg G00 feed forward gain 70 2096 crncsp Minimum corner deceleration speed 0
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
689 IB-1501278-P
(1) Pre-reading is executed during SSS control, so a program error could occur before the block containing the error is executed.
(2) Buffer correction is not guaranteed during SSS control. (3) If automatic/manual simultaneous or automatic handle feed interrupt are used during SSS control, the machining
accuracy will not be guaranteed. (4) If a fine arc command is issued during SSS control, it may take longer to machine. (5) The same path as single block operation will be used during graphic check. (6) The line under the cutting feedrate and arc command block are subjected to the speed control in the SSS control.
The command blocks that are not subjected to speed control, decelerate first and automatically switch the SSS control ON and OFF.
(7) SSS control is temporarily disabled in the following modal: NURBS interpolation Polar coordinate interpolation Cylindrical interpolation User macro interruption enable (M96) Feed per revolution (synchronous feed) Inverse time feed Constant surface speed control Fixed cycle Hypothetical axis interpolation Automatic tool length measurement Tool length compensation along the tool axis
(8) There are some restrictions for each high-accuracy control. Refer to each section for restrictions. "17.2 High-accuracy Control" "17.3 High-speed High-accuracy Control"
(9) Fairing is disabled during the SSS control.
SSS control parameter
Precautions
[Range for recognizing the shape] #1571 SSSdis #8091 StdLength
[Acceleration/deceleration process] Feedrate
Seam between blocks Clamp speed = theory deceleration speed (after adding accuracy coefficient)#8092 ClampCoeff
Time
#8094 DccWaitAdd Able to wait for deceleration by setting the extra time when the speed feedback does not drop to the clamp speed.
Movement command
[Measure for step] #8093 StepLeng Set the value approximately the same as the CAM path difference (tolerance) for the parameter.
#8093 StepLeng
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
690IB-1501278-P
17.2.3 Tolerance Control
This function obtains the optimum clamp speed for corners or curves based on the designated tolerance to perform operations. It also ensures smooth passing within the tolerance range in corner sections, which suppresses machine vibrations. This means that the clamp speed can be increased to reduce the cycle time. This function allows the machine to operate with the optimum tool path and speed, simply by specifying the toler- ance, so an operator can easily carry out high quality machining. The tolerance refers to the allowable error amount between the path commanded in the machining program and the path output by NC. The validity of this function depends on the MTB specifications. This function also requires the SSS control specifi- cations because it can only be used under SSS control.
This function is enabled when the following conditions are satisfied:
(1) The tolerance control specification is valid. (Based on the MTB specifications.) (2) The parameter "#8090 SSS ON" is set to "1". (3) The parameter "#12066 Tolerance ctrl ON" is set to "1". (*1)(*2) (4) High-accuracy control (G61.1/G08P1), spline interpolation (G61.2/G05.1Q2), spline interpolation 2 (G61.4), or
high-speed high-accuracy control I/II/III (G05.1Q1/G05P10000/G05P20000) is valid. (*1) Even if conditions (1) and (3) are satisfied, an operation error (M01 0139) will occur and the cycle start cannot
be performed automatically if the parameter "#8090 SSS ON" is set to "0". In this case, enable SSS control and reset the alarm to start the cycle automatically.
(*2) A setting error will occur if "1" is set when this specification is invalid.
Function and purpose
Program command path
Path commanded by NC to drive unit
Tool path
Tolerance control: Invalid Tolerance control: Valid
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
691 IB-1501278-P
Set the tolerance with the parameter "#2659 tolerance" or the ",K" address following the G code (G61.1 or G61.4 command). When the setting value is "0", this function runs with "0.01(mm)".
The range of the command value is 0.000 to 100.000. If a value exceeding the range is commanded, a program error (P35) will occur.
The tolerance designated by ",K" is applied to all axes in the part system. When "0" is designated or ",K" is omitted, the program runs based on the value of the parameter "#2659 toler-
ance". The tolerance designated by ",K" is not held after reset. Therefore, if ",K" is not designated in the G61.1 or G61.4
command after reset, the axis runs based on the value of the parameter "#2659 tolerance".
(1) The G61.4 command requires the specifications of spline interpolation 2.
The clamp speed is obtained from the tolerance in the corner or curve section during tolerance control. As the designated tolerance is lower, the axis speed decelerates.
Command format
Tolerance specification
G61.1 or G61.4 ,K__ ;
,K Tolerance (mm)
Detailed description
The axis moves in the designated tolerance range during tolerance control. The tolerance on the corner shape is as shown on the right.
Speed control
Tolerance: High Tolerance: Low Command path
Resultant speed
Time Time
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
692IB-1501278-P
The parameters valid and invalid during tolerance control are as follows. Some parameters depend on the MTB specifications.
(1) Valid parameters
(2) Invalid parameters (Parameters with no setting required)
Parameters valid during tolerance control
No. Parameter name Supplements
1206 G1bF When combining with the variable-acceleration pre-inter- polation acceleration/deceleration or axis-specific accel- eration tolerance control, specify parameters "#2157 G1bFx" and "#2158 G1btLx".
1207 G1btL
1568 SfiltG1 12051 Jerk_filtG1 2659 tolerance
No. Parameter name Supplements
1570 Sfilt2 Ignored even if the value is entered. 2159 compx Ignored even if the value is entered. The clamp speed is
obtained from the tolerance during tolerance control; therefore, parameters for adjusting the clamp speed are not required.
8019 R COMP 8020 DCC ANGLE 8021 COMP CHANGE 8022 CORNER COMP 8023 CURVE COMP 8096 Deceler. coeff. ON 8097 Corner decel coeff 8098 Arc clamp spd coef
Program example
: G91 ; G61.1 ,K0.02; Designate tolerance 0.02 (mm). G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ;
Tolerance: 0.02 (mm)
G61.1 ,K0; Designate tolerance 0 (mm). X-0.1 Z-0.05 ; X-0.1 Z-0.3 ;
Tolerance: Follows parameter "#2659 tolerance".
G64 ; :
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
693 IB-1501278-P
(1) While tolerance control is valid, tolerance control may be canceled temporarily depending on some commands. If tolerance control is canceled temporarily, the axis moves to the commanded position without taking an inner route in a corner section. After this, when a temporary cancel cause is removed, tolerance control restarts. The temporary cancel conditions are as follows: (a) Modal in which the group 1 command is not G01 (linear interpolation) or G02/G03 (circular interpolation). (b) Under single block operation (c) Modal in which SSS control is disabled temporarily (Modal shown below)
NURBS interpolation Polar coordinate interpolation Cylindrical interpolation User macro interruption enable (M96) Feed per revolution (Synchronous feed) Inverse time feed Constant surface speed control Fixed cycle Hypothetical axis interpolation Automatic tool length measurement Tool length compensation along the tool axis Normal line control Unidirectional positioning Exponential interpolation 3-dimensional circular interpolation
(2) The stored stroke limit's prohibited range is determined based on the program command path. As a result, ma- chining may not be stopped even if the command moved inward by tolerance control enters the prohibited range.
(3) If a feed hold signal is turned ON at a corner, machining stops on the program command path. This means that it does not stop at point A in the figure below but at point B.
(4) When the tolerance control is enabled (#12066 = "1"), the maximum value of the fine segment processing capa- bility is 100 kBPM for M800 Series and 67.5 kBPM for M80 Series.
Precautions
Program command path
Path without a feed hold signal
Path when a feed hold signal is turned on at a corner A
B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
694IB-1501278-P
17.2.4 Variable-acceleration Pre-interpolation Acceleration/Deceleration
This function is useful when each axis differs in the characteristics (responsiveness) (4-axis/5-axis machine, etc.). The normal acceleration/deceleration before interpolation performs the acceleration/deceleration by setting accel- eration rate common to all axes. Therefore, if the high responsiveness and low responsiveness coexist in axes, the acceleration rate needs to be set to suit the axis with low responsiveness. On the other hand, the variable-acceleration pre-interpolation acceleration/deceleration can perform the accelera- tion/deceleration by setting diverse acceleration rate to each axis. This means that it is possible to set a higher ac- celeration rate for axes with high responsiveness than before. Therefore, the cycle time can be reduced especially in the indexing machining. (Refer to following figure.) The validity of this function depends on the MTB specifications. This function also requires the SSS control specifi- cations because it can only be used under SSS control.
This function is enabled when the following conditions are satisfied:
(1) The variable-acceleration pre-interpolation acceleration/deceleration specification is valid. (Based on the MTB specifications.)
(2) The MTB-specific parameter has been set (#12060 VblAccPreInt). (*1) (3) Under SSS control (*2)
(*1) A setting error will occur if "1" is set when this specification is invalid.
(*2) The validity of the SSS control function depends on the MTB specifications. To enable SSS control, it is necessary to set the parameter "#8090 SSS ON" to "1" to command high-accu- racy control.
(*3) Even if conditions (1) and (2) are satisfied, an operation error (M01 0136) will occur and the cycle start can- not be performed automatically if the parameter "#8090 SSS ON" is set to "0". In this case, enable SSS con- trol and reset the alarm to start the cycle automatically.
"VAC" is displayed on the operation screen and modal display under variable-acceleration pre-interpolation accel- eration/deceleration.
Function and purpose
Resultant speed Variable-acceleration pre-interpolation acceleration/deceleration
Acceleration/deceleration before inter- polation
Time Rotary axis Linear axis Shortened
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
695 IB-1501278-P
The acceleration rate for each axis is determined in the MTB specifications (parameters "#2157 G1bFx" (maximum speed for each axis) and "#2158 G1btLx" (axis time constant)). For an axis with G1bFx = 0 (not set), the acceleration rate is calculated using "#1206 G1bF" (maximum speed). And for an axis with G1btLx = 0 (not set), the acceleration rate is calculated using "#1207 G1btL" (time constant). Therefore, if G1bFx and G1btLx are 0 (not set) for all axes, the normal acceleration/deceleration before interpolation is performed. The following shows examples of settings.
Set linear axis acceleration rate for "#1206 G1bF" and "#1207 G1btL".
It is assumed that only the acceleration rate for the rotary axis is set for "#2157 G1bFx" and "#2158 G1btLx". ("#1206 G1bF" and "#1207 G1btL" are used by not setting the acceleration rate for the linear axis.)
The figure below shows movements with the above settings.
(1) If only the X axis moves, acceleration/deceleration is performed at the acceleration rate set for the X axis. ... (a)
(2) If only the C axis moves, acceleration/deceleration is performed at the acceleration rate set for the C axis. ... (d)
(3) If both of the X and C axes move, acceleration/deceleration is performed at the optimum acceleration rate cal- culated within the range that the acceleration rate of each axis does not exceed the setting. If the movement of the X axis is dominant ... (b) If the movement of the C axis is dominant ... (c)
Detailed description
#1206 G1bF 10000 (mm/min) #1207 G1btL 100 (ms)
X Y Z C
#2157 G1bFx 0 (not set) 0 (not set) 0 (not set) 10000 (mm/min) #2158 G1btLx 0 (not set) 0 (not set) 0 (not set) 500 (ms)
(b) (c) (d)(a)
Time
Time
Time
Time
Time
Time
Time
Time
Time
Time
Time
Time
Acceleration rate : Large Acceleration rate : Small
Resultant speed Resultant speed Resultant speed Resultant speed
X axis speed X-axis speed X-axis speed
C-axis speed C-axis speedC-axis speed
X axis speed
C-axis speed
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
696IB-1501278-P
(1) Under variable-acceleration pre-interpolation acceleration/deceleration, corner deceleration is realized with the axis-specific acceleration tolerance control. Corner deceleration patterns and acceleration/deceleration patterns are as follows with each parameter setting:
(2) This function can only be used under SSS control. This means that variable-acceleration pre-interpolation accel- eration/deceleration is also disabled during a modal that temporarily disables SSS control. As a result, the tool is under the axis-specific acceleration tolerance control. In this mode, the acceleration rate is determined by "#1206 G1bF" and "#1207 G1btL". Out of #2157 and #2158, set the longer one for #1206 and #1207. (Make a note of the original values and restore them as necessary.) Refer to "17.2.2 SSS Control" for modals that temporarily disable SSS control.
(3) Basically, set the same acceleration rate for base axes I, J, and K. A different acceleration rate causes a distorted shape against an arc command. The figure below shows an example where the acceleration rate in the Y direction is greater than that in the X direction.
Precautions
#12060 VblAccPreInt 0 0 1 1 Variable-acceleration Pre-interpo- lation Acceleration/Deceleration ON #12053 EachAxAccCntrl 0 1 0 1 Axis-specific acceleration toler- ance control ON Corner deceleration pattern Optimum corner
deceleration Axis-specific acceleration tolerance control
Acceleration/deceleration pattern Acceleration/deceleration before interpolation
Variable-acceleration pre-interpo- lation acceleration/deceleration
Actual tool path Machining program commanded shape
X
Y
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
697 IB-1501278-P
17.2.5 Initial High-accuracy Control
If "#1148 I_G611" (Initial high-accuracy) is set by the MTB specifications, high-accuracy control-related functions can be enabled when the power is turned ON. At power ON, the modes set by this parameter are enabled, but each mode can be changed to a different one by commanding as follows in the machining program.
It is impossible, however, to shift to the high-speed high-accuracy control II/high-speed high-accuracy control III mode during the high-speed high-accuracy control I. Likewise, it is also impossible to shift to the high-speed high- accuracy control I mode during the high-speed high-accuracy control II/high-speed high-accuracy control III mode. To shift to either mode, cancel the current high-speed high-accuracy control mode using "G05.1 Q0" or "G05 P0" first and then command the target mode. If any function set by this parameter is not included in your machine's specifications, an available high-accuracy function with a number smaller than the parameter setting is enabled.
#1148 setting value Modes enabled at power ON
0 G08P0/G64 (cutting mode) command 1 G08P1/G61.1 (high-accuracy control mode) command 2 G05.1Q1 (high-speed high-accuracy control I mode) command 3 G05P10000 (high-speed high-accuracy control II mode) command 4 G05P20000 (high-speed high-accuracy control III mode) command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
698IB-1501278-P
17.2.6 Multi-part System Simultaneous High-accuracy
High-accuracy control and high-speed machining mode are available respectively in all part systems, however, the simultaneous usage of high-accuracy control and high-speed machining mode (including High-speed high-accuracy control I/II/III) are available only in part systems which are limited by the parameter "#8040 High-SpeedAcc". While high-accuracy control and high-speed machining mode are available simultaneously in a part system where this pa- rameter is set to "1", a program error (P129) will occur in those where the parameter is set to "0" when commanded. Also, for part systems where "#8040 High-SpeedAcc" is set to "0", "#1148 I_G611" must be set to "0" (Cutting mode when the power is turned ON) or "1" (High-accuracy control mode when the power is turned ON). If the parameter "#1148 I_G611" is set to a value other than "0" and "1", the parameter is regarded as being set to "1". Note that up to two part systems can be set to use high-accuracy control and high-speed machining mode simulta- neously. If three or more part systems are set as such, an MCP alarm (Y51 0032) will occur. If the parameter "#8040 High-SpeedAcc" is set to "0" for all part systems, only the first part system is handled as the one with the parameter set to "1".
Function and purpose
G28 X0 Y0; G08 P1; G05 P2; G91 G01 F3000; : : : : G05P0; G08 P0; M02;
G08P0 G08P1
G08P0
$1 $2
$3 $4
G05P0
G05P2
G05P0
G28 X0 Y0; G08 P1; : G08 P0; G05 P2; : G08 P1; : G08 P0; G05 P0; M02;
G08P0 G08P1
G08P0
G08P1
G05P0
G05P2
G28 X0 Y0; G05 P10000; G91 G01 F3000; X1.; : : : : : G05P0; M02;
G08P0 G08P1
G08P0
G05P0 G05P2
G05P0
G28 X0 Y0; G05 P10000; G91 G01 F3000; X1.; : : : : : G05P0; M02;
G08P0 G08P1
G05P0 G05P2
Up to 2 part systems can be set to "1"
High-speed high-accuracy enabled part system = 1
High-speed high-accuracy enabled part system = 1
High-speed high-accuracy enabled part system = 0
High-speed high-accuracy
High-speed high-accuracy
High-speed high-accuracy enabled part system = 0
(Note) It is limited also in G61.1 command.
Alarm
Alarm
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
699 IB-1501278-P
Although some MTB specifications support the high-accuracy acceleration/deceleration time constant expansion specifications, only one part system can be used. Multi-part systems cannot be used even if the high-accuracy ac- celeration/deceleration time constant expansion specifications are valid. For multi-part systems, "#1207 G1btL" must be set to a value within the setting range that is applicable when there are no high-accuracy acceleration/de- celeration time constant expansion specifications.
Refer to the following chapters for details of each high-accuracy control.
"17.2 High-accuracy Control"
"17.3 High-speed High-accuracy Control"
(1) When "#1148 I_G611" (Initial hi-precis) is enabled, the initial modal state after power ON will be the high-accu- racy control mode. Refer to "17.2.5 Initial High-accuracy Control" for details. In this case, the high-accuracy control mode is enabled if the multi-part system simultaneous high-accuracy specification is provided. Otherwise, the 1st part system enters the high-accuracy control mode, but the 2nd part system enters the cutting mode.
(2) If you use the high-accuracy acceleration/deceleration time constant expansion function together with the multi- part system simultaneous high-accuracy function, an MCP alarm (Y51 0020) will occur. Make sure to disable the high-accuracy acceleration/deceleration time constant extension function when you use the multi-part system simultaneous high-accuracy function.
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
700IB-1501278-P
17.3 High-speed High-accuracy Control
It depends on the MTB specifications whether the modal state at power ON is high-speed high-accuracy control I, II, III, or OFF. It also depends on the specifications whether to hold the modal state at reset. Refer to the specifications of your machine. In the main text, the axis address refers to the address of an axis that exits on the machine. It corresponds to the address designated in the parameters "#1013 axname" and "#1014 incax". These parameter settings depend on the MTB specifications.
17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0
This function runs a machining program that approximates a freely curved surface with fine segments at high speed and with high-level accuracy. This is effective in increasing the speed of machining dies of a freely curved surface. This function is useful for machining which needs to make an edge at a corner or reduce an error from an inner route of curved shape. A higher fine segment processing capability leads to a faster cutting speed, resulting in a shorter cycle time and a better machining surface quality. kBPM, the unit for the fine segment processing capability, is an abbreviation of "kilo blocks per minute" and refers to the number of machining program blocks that can be processed per minute.
The tables (1) to (3) describe the fine segment processing capability while the high-speed high-accuracy control is enabled. The units of values in the tables is kBPM (kilo Blocks Per Minute), which expresses the number of machin- ing program blocks which can be processed per minute. The table (1) shows the maximum values of the fine segment processing capability. The fine segment processing capability may decelerate in the conditions with high processing load as follows: Four or more axes are being commanded at the same time. A macro command or a variable command is included in a command. A compensation function such as the tool radius compensation is used. High-speed processing is selected for the processing cycle of the control unit (the parameter "#1468 ctrl period"
is set to "-1"). A large number of axes are installed. Fine segment processing capability may be lowered when the acceleration rate and speed are set to such values that the time duration to reach the specified speed exceeds the maximum value (5000 ms) of acceleration/deceler- ation time constant before interpolation (parameter "#1207 G1btL").
When the tolerance control is enabled (#12066 = "1"), the maximum value of the fine segment processing capability is 100 kBPM for M800 Series and 67.5 kBPM for M80 Series.
(1) High-speed high-accuracy control I
Function and purpose
Fine segment processing capability
Number of part systems/ number of axes
Number of part sys- tems
M850 / M830 M80
(#8040=1) Type A Type B
1-part system 1 part system 67.5 33.7 33.7 2-part system 1 part system 67.5 33.7 33.7
2 part systems 33.7 16.8 16.8 4-part system 1 part system - (*1) - (*1) - (*1) Up to 16 axes 2 part systems - (*1) - (*1) - (*1) 5 part systems or more or 17 axes or more
1 part system - (*1) - (*1) - (*1) 2 part systems - (*1) - (*1) - (*1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
701 IB-1501278-P
(2) High-speed high-accuracy control II
(3) High-speed high-accuracy control III
(*1) This system cannot be used for this model.
(*2) There are no corresponding high-speed high-accuracy control specifications.
(*3) 100 kBPM for a time constant expansion system or while tool center point control, inclined surface machining, or workpiece installation error compensation is in process.
(*4) 67.5 kBPM for a time constant expansion system or while tool center point control, inclined surface machining, or workpiece installation error compensation is in process. (The time constant expansion system can be used in a system configured with a single part system when the specification is valid.)
(*5) When the fairing is valid (When the parameter "#8033" is set to "1"), and the fairing is executed successively, depending on machining programs, the performance of fine segment execution may decelerate more than the value described in the above table. In the network connection, the value described in the above table may not be guaranteed depending on the state.
High-speed high-accuracy control I, II, III can be used simultaneously in up to two part systems. High-speed high-accuracy control I, II, III can be used in a part system where "1" is set for the parameter "#8040 High-SpeedAcc". A program error occurs (P129) if this is commanded for a part system where "0" is set for the pa- rameter.
If the parameter "#8040 High-SpeedAcc" is set to "0" for all part systems, only the first part system is handled as the one with the parameter set to "1". Also, a part system where the parameter "#1148 Initial hi-precis" is set to "2" to "4" is handled as the one with the parameter "#8040 High-SpeedAcc" set to "1". The parameter "#8040 High-SpeedAcc" can be set to "1" for up to two part systems. If 3 or more part systems are set to "1", an MCP alarm (Y51 0032) occurs. When "1" is set for two part systems, the fine segment processing ca- pability decreases compared to when "1" is set only for one part system.
Number of part systems/ number of axes
Number of part sys- tems
M850 / M830 M80
(#8040=1) Type A Type B
1-part system 1 part system 168 (*3)(*5) 67.5 67.5 2-part system 1 part system 100 67.5 67.5
2 part systems 67.5 33.7 33.7 4-part system 1 part system - (*1) - (*1) - (*1) Up to 16 axes 2 part systems - (*1) - (*1) - (*1) 5 part systems or more or 17 axes or more
1 part system - (*1) - (*1) - (*1) 2 part systems - (*1) - (*1) - (*1)
Number of part systems/ number of axes
Number of part sys- tems
M850 / M830 M80
(#8040=1) Type A Type B
1-part system 1 part system 270 (*3)(*5) 135 (*4) - (*2) 2-part system 1 part system 168 135 - (*2)
2 part systems 100 67.5 - (*2) 4-part system 1 part system - (*1) - (*1) - (*2) Up to 16 axes 2 part systems - (*1) - (*1) - (*2) 5 part systems or more or 17 axes or more
1 part system - (*1) - (*1) - (*2) 2 part systems - (*1) - (*1) - (*2)
High-speed high-accuracy control simultaneously for two part systems
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
702IB-1501278-P
(1) The high-speed high-accuracy mode II and III cannot be used at the same time. (2) These commands are valid regardless of the parameter "#1267 ext03/bit0" setting if the specifications are avail-
able. (3) High-speed high-accuracy control III can also be used by setting a parameter instead of a G code.
If the parameter "#8131 High speed/accu 3" is set to "1", the high-speed high-accuracy control II command can be handled as the III command. This also enables the high-speed high-accuracy control III mode in the machin- ing program using "G05P10000". Likewise, the G05P2 command issued during a high-accuracy control mode can be handled as the high-speed high-accuracy control III command. Furthermore, by setting "#1148 Initial hi-precis" to "4", the high-speed high-accuracy control III mode can be set as the initial modal state after power ON.
(1) The high-speed high-accuracy control I / II / III can be used during tape, MDI, SD card or memory modes. (2) The override, maximum cutting speed clamp, single block operation, dry run, handle interrupt and graphic trace
are valid even during the high-speed high-accuracy control I / II / III modal. (3) The machining speed may drop depending on the number of characters in one block. (4) The high-speed high-accuracy control I / II / III function automatically turns the high-accuracy control mode ON.
For high-accuracy control function, refer to "17.3 High-speed High-accuracy Control". (5) Turn the tool radius compensation command ON and OFF during the high-speed high-accuracy control I/II/III
mode. If the high-speed high-accuracy control I/II/III mode is turned OFF without turning the tool radius compensation OFF, a program error (P34) will occur.
(6) Turn the high-speed high-accuracy control I / II / III mode OFF before commanding data other than those that can be commanded.
(7) When using the high-speed high-accuracy control II / III mode, it is necessary to set the parameter "#1572 Cirorp" to eliminate the speed fluctuation at the seams between arc and straight line or arc and arc. This parameter, however, depends on the MTB specifications.
(8) Feedrate command F is clamped with the "#2110 Clamp (H-precision)" (Cutting feed clamp speed for high-ac- curacy control mode) set with parameter.
(9) Rapid traverse rate enables "#2109 Rapid(H-precision)" (Rapid traverse rate during high-accuracy control mode) set by the parameter.
(10) When the "#2109 Rapid(H-precision)" is set to "0", the movement follows "#2001 rapid" (rapid traverse rate) set by the parameter. Also, when "#2110 Clamp (H-precision)" is set to "0", the speed will be clamped with "#2002 clamp" (Cutting clamp speed) set with parameter.
Command format
G05.1 Q1 ; High-speed high-accuracy control I ON
G05.1 Q0 ; High-speed high-accuracy control I OFF
G05 P10000 ; High-speed high-accuracy control II ON
G05 P20000 ; High-speed high-accuracy control III ON
G05 P0 ; High-speed high-accuracy control II/III OFF
Detailed description
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
703 IB-1501278-P
To enable each high-speed high-accuracy control function, it is necessary to satisfy the following conditions respec- tively:
(1) The specification of each function is valid. (*1) (2) Each function is in a valid modal state. (Refer to "Relationship with other functions".) (3) Each function is enabled by one of the following procedures: Command each in the machining program. (*2) Set each for the parameter "#1148 Initial hi-precis". (The modal at power ON corresponds to each high-
speed high-accuracy control function.)
(*1) The following conditions are additionally required to enable high-speed high-accuracy control III. The time constant expansion system is invalid. The SSS control specifications are valid, and the parameter "#8090 SSS ON" is set to "1". If high-speed high-accuracy control III is commanded when the SSS control mode is set to OFF, high-speed high-accuracy control II is enabled. (However, this is available only when the conditions defined in "Relationship with other functions" are satisfied.)
(*2) High-speed high-accuracy control III is also enabled by the following commands. (However, this is available only when the conditions defined in "Relationship with other functions" are satisfied.) While the parameter "#8131 High speed/accu 3" is set to "1", command "G05 P10000" (high-speed high-accu- racy control II) is issued from the machining program. Alternatively, command "G05 P2" (high-speed machining mode II) is issued during high-accuracy control.
(*3) When the parameter "#1148 Initial hi-precis" is set to "3" (high-speed high-accuracy control II) and the param- eter "#8131 High speed/accu 3" to "1" ("High speed/accu 3" is valid), the initial modal state after power ON changes to the high-speed high-accuracy control II mode.
(*4) However, when the parameter "#1074 Initial sync feed" is set to "1", the modal state changes to the high-speed high-accuracy control II mode.
Enabling conditions
#1148 setting
High-speed high-accuracy control I 2 High-speed high-accuracy control II 3 (*3) High-speed high-accuracy control III 4 (*4)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
704IB-1501278-P
(1) Relationship between the high-speed high-accuracy control I and the other G code functions Column A: Operation when the additional function is commanded while the high-speed high-accuracy control I is enabled Column B: Operation when the high-speed high-accuracy control I (G05.1Q1) is commanded while the addition- al function is enabled : The high-speed high-accuracy control I and the additional function are both enabled : The high-speed high-accuracy control I is temporarily canceled, while the additional function is enabled : Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination : Others
Relationship with other functions
Relationship between the high-speed high-accuracy control I and other functions
Group G code Function name A B
0 G04 Dwell - G05P0 High-speed machining mode II OFF
High-speed high-accuracy control II OFF High-speed high-accuracy control III OFF
(P34) (*2)
G05P2 High-speed machining mode II ON (*4) (*2) G05P10000 High-speed high-accuracy control II ON (P34) (P34) G05P20000 High-speed high-accuracy control III ON (P34) (P34) G05.1Q0 High-speed high-accuracy control I OFF
Spline interpolation OFF (*1) (*2)
G05.1Q1 High-speed high-accuracy control I ON (*3) (*3) G05.1Q2 Spline interpolation ON (P34) (*10) (P34) (*10) G07 Hypothetical axis interpolation (*10) (*10) G08P0 High-accuracy control OFF (*3) (*2) G08P1 High-accuracy control ON (*3) (*2) G09 Exact stop check - G10 I_J_ G10 K_
Parameter coordinate rotation input (*10) - (*10)
G10 L2 Compensation data input by program - G10 L70 G10 L50
Parameter input by program -
G27 Reference position check - G28 Reference position return - G29 Start position return - G30 2nd to 4th reference position return - G30.1- G30.6
Tool exchange position return -
G31 Skip Multiple-step skip 2
-
G31.1- G31.3
Multi-step skip -
G34-G36 G37.1
Special fixed cycle -
G37 Automatic tool length measurement - G38 Tool radius compensation vector designation - G39 Tool radius compensation corner circular com-
mand -
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
705 IB-1501278-P
0 G50.2/G250 Tool spindle synchronization IB (spindle-spin- dle, polygon)/IIC (spindle-NC Axis, polygon) cancel
G51.2/G251 Tool spindle synchronization IB (spindle-spin- dle, polygon) ON
Tool spindle Synchronization IC (spindle-NC Axis, polygon) ON
G52 Local coordinate system setting - G53 Machine coordinate system selection - G60 Unidirectional positioning - G65 User macro simple call (*5) (*6) G92 Coordinate system setting - G92.1 Workpiece coordinate system preset (*10) - (*10) G113.1 Spindle synchronization OFF G114.1 Spindle synchronization ON G114.2 Tool spindle synchronization IA (spindle-spin-
dle, polygon mode)
G114.3 Tool spindle synchronization II (hobbing) G122 Sub part system control I (P652) (*10) (*7)(*10) G144 Sub part system control II (P652) (*10) (*7)(*10)
1 G00 Positioning G01 Linear interpolation G02 G03
Circular interpolation When SSS is enabled: When SSS is disabled:
When SSS is enabled: When SSS is disabled:
G02.1 G03.1
Spiral interpolation (*10) (*10)
G02.3 G03.3
Exponential interpolation (*10) (*10)
G02.4 G03.4
3-dimensional circular interpolation (*10) (*10)
G06.2 NURBS interpolation (P34) (*10) (P34) (*10) G33 Thread cutting
2 G17-G19 Plane selection 3 G90 Absolute command
G91 Incremental command 4 G22 Stroke check before travel ON
G23 Stroke check before travel OFF 5 G93 Inverse time feed (P125) (*10) (P125) (*10)
G94 Asynchronous feed (feed per minute) G95 Synchronous feed (feed per revolution)
6 G20 Inch command G21 Metric command
7 G40 Tool radius compensation cancel G41 G42
Tool radius compensation (P29)
Group G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
706IB-1501278-P
(*1) Disables the high-speed high-accuracy control I.
(*2) Enables the high-speed high-accuracy control I.
(*3) High-speed high-accuracy control I continues.
(*4) Enables the high-speed machining mode II.
(*5) Enables the high-speed high-accuracy control I in a macro program.
8 G43 G44
Tool length offset (P29)
G43.1 Tool length compensation along the tool axis (*10) (P29) (*10) G43.4 G43.5
Tool center point control (*10) (P29) (*10)
G49 Tool length offset cancel 9 G80 Fixed cycle cancel
Group 9 Other than G80
Fixed cycle
10 G98 Fixed cycle initial level return G99 Fixed cycle R point return
11 G50 Scaling cancel G51 Scaling ON (P34)
12 G54-G59 G54.1
Workpiece coordinate system selection
13 G61 Exact stop check mode (*8) (*9) G61.1 High-accuracy control (*3) (*2) G61.2 High-accuracy spline (P29) (*10) (P29) (*10) G61.4 Spline interpolation 2 (*10) (*10) G62 Automatic corner override (*3) (*2) G63 Tapping mode (*3) (*2) G64 Cutting mode (*3) (*2)
14 G66 G66.1
User macro modal call (*5) (*6)
G67 User macro modal call cancel 15 G40.1 Normal line control cancel
G41.1 G42.1
Normal line control (P29) (*10) (P29) (*10)
16 G68 Coordinate rotation by program ON 3-dimensional coordinate conversion ON
G68.2 G68.3
Inclined surface machining command (*10) (*10)
G69 Coordinate rotation cancel 17 G96 Constant surface speed control ON
G97 Constant surface speed control OFF 18 G15 Polar coordinate command OFF
G16 Polar coordinate command ON (P34) (P34) 19 G50.1 Mirror image OFF
G51.1 Mirror image ON (P34) 21 G07.1 Cylindrical interpolation (P485)
G12.1 Polar coordinate interpolation ON (P485) G13.1 Polar coordinate interpolation OFF
27 G54.4P0 Workpiece installation error compensation can- cel
G54.4 P1-P7
Workpiece installation error compensation (*10) (*10)
Group G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
707 IB-1501278-P
(*6) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in a macro program.
(*7) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in a sub part system.
(*8) Enables the exact stop check mode.
(*9) Exact stop check mode continues.
(*10) In M80 Type B, the following program errors occur depending on the G codes. G code Program error G code Program error
G05.1Q2, G92.1, G122, G61.2, G61.4
P39 G10 I_J_/G10 K_ P260 G06.2 P550
G144, G54.4 P1-P7 P34 G93 P124 G07 P80 G41.1, G42.1 P900 G02.1, G03.1 P73 G43.1 P930 G02.3, G03.3 P611 G43.4, G43.5 P940 G02.4, G03.4 P76 G68.2, G68.3 P950
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
708IB-1501278-P
(2) Relationship between the high-speed high-accuracy control I and functions other than G codes Column A: Operation when the additional function is commanded while the high-speed high-accuracy control I is enabled Column B: Operation when the high-speed high-accuracy control I (G05.1Q1) is commanded while the addition- al function is enabled : The high-speed high-accuracy control I and the additional function are both enabled : The high-speed high-accuracy control I is temporarily canceled, while the additional function is enabled : Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination : Others
(*1) Enables the high-speed high-accuracy control I in a subprogram.
(*2) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in a subprogram.
(*3) Enables timing synchronization.
(*4) Enables the high-speed high-accuracy control I in a MTB program.
(*5) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in a MTB program.
(*6) Enables the high-speed high-accuracy control I in an interrupt program.
(*7) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in an interrupt program.
(*8) Disables the high-speed high-accuracy control I in a figure rotation subprogram.
(*9) The high-speed high-accuracy control I is disabled even if G05.1Q1 is commanded in a figure rotation sub- program.
(*10) In M80 Type B, the following program error occurs depending on the function type.
Function name A B
SSS ON - Mirror image by parameter setting ON - (P34) Mirror image by external input - (P34) Coordinate rotation by parameter - Subprogram call (M98) (*1) (*2) Figure rotation (M98 I_J_K_) (*8)(*10) (*9)(*10) Timing synchronization between part systems (*3) - MTB macro (*4) (*5) Macro interruption (*6) (*7) PLC interruption (*6) (*7) Corner chamfering/Corner R - Linear angle command - Geometric command - Chopping Optional block skip -
Function Program error
Figure rotation (M98 I_J_K_) P250
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
709 IB-1501278-P
(1) Relationship between the high-speed high-accuracy control II and G code functions Column A: Operation when the additional function is commanded while the high-speed high-accuracy control II is enabled Column B: Operation when the high-speed high-accuracy control II (G05P10000) is commanded while the ad- ditional function is enabled : The high-speed high-accuracy control II and the additional function are both enabled : The high-speed high-accuracy control II is temporarily canceled, while the additional function is enabled : Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination : Others
Relationship between the high-speed high-accuracy control II and other functions
Group G code Function name A B
0 G04 Dwell - G05P0 High-speed machining mode II OFF
High-speed high-accuracy control II OFF High-speed high-accuracy control III OFF
(*1) (*2)
G05P2 High-speed machining mode II ON (*4) (*2) G05P10000 High-speed high-accuracy control II ON (*3) (*3) G05P20000 High-speed high-accuracy control III ON (*2) (*2) G05.1Q0 High-speed high-accuracy control I OFF
Spline interpolation OFF (*3) (*2)
G05.1Q1 High-speed high-accuracy control I ON (P34) (P34) G05.1Q2 Spline interpolation ON (*8) (*8) G07 Hypothetical axis interpolation (*8) (*8) G08P0 High-accuracy control OFF (*3) (*2) G08P1 High-accuracy control ON (*3) (*2) G09 Exact stop check - G10 I_J_ G10 K_
Parameter coordinate rotation input (*8) - (*8)
G10 L2 Compensation data input by program - G10 L70 G10 L50
Parameter input by program -
G27 Reference position check - G28 Reference position return - G29 Start position return - G30 2nd to 4th reference position return - G30.1- G30.6
Tool exchange position return -
G31 Skip Multiple-step skip 2
-
G31.1- G31.3
Multi-step skip -
G34-G36 G37.1
Special fixed cycle -
G37 Automatic tool length measurement - G38 Tool radius compensation vector designa-
tion -
G39 Tool radius compensation corner circular command
-
G50.2/G250 Tool spindle synchronization IB (spindle- spindle, polygon)/IIC (spindle-NC Axis, polygon) cancel
G51.2/G251 Tool spindle synchronization IB (spindle- spindle, polygon) ON
Tool spindle Synchronization IC (spindle- NC Axis, polygon) ON
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
710IB-1501278-P
0 G52 Local coordinate system setting - G53 Machine coordinate system selection - G60 Unidirectional positioning - G65 User macro simple call (*5) (*6) G92 Coordinate system setting - G92.1 Workpiece coordinate system preset (*8) - (*8) G113.1 Spindle synchronization OFF G114.1 Spindle synchronization ON G114.2 Tool spindle synchronization IA (spindle-
spindle, polygon mode)
G114.3 Tool spindle synchronization II (hobbing) G122 Sub part system control I (P652) (*8) (*7)(*8) G144 Sub part system control II (P652) (*8) (*7)(*8)
1 G00 Positioning G01 Linear interpolation G02 G03
Circular interpolation
G02.1 G03.1
Spiral interpolation (*8) (*8)
G02.3 G03.3
Exponential interpolation (*8) (*8)
G02.4 G03.4
3-dimensional circular interpolation (*8) (*8)
G06.2 NURBS interpolation (*8) (*8) G33 Thread cutting
2 G17-G19 Plane selection 3 G90 Absolute command
G91 Incremental command 4 G22 Stroke check before travel ON
G23 Stroke check before travel OFF 5 G93 Inverse time feed (*8) (*8)
G94 Asynchronous feed (feed per minute) G95 Synchronous feed (feed per revolution)
6 G20 Inch command G21 Metric command
7 G40 Tool radius compensation cancel G41 G42
Tool radius compensation
8 G43 G44
Tool length offset
G43.1 Tool length compensation along the tool axis
(*8) (*8)
G43.4 G43.5
Tool center point control (*8) (*8)
G49 Tool length offset cancel 9 G80 Fixed cycle cancel
Group 9 Other than G80
Fixed cycle
10 G98 Fixed cycle initial level return G99 Fixed cycle R point return
11 G50 Scaling cancel G51 Scaling ON
Group G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
711 IB-1501278-P
(*1) Disables the high-speed high-accuracy control II.
(*2) Enables the high-speed high-accuracy control II.
(*3) High-speed high-accuracy control II continues.
(*4) Enables the high-speed machining mode II.
(*5) Enables the high-speed high-accuracy control II in a macro program.
(*6) Enables the high-speed high-accuracy control II if G05P10000 is commanded in a macro program.
(*7) Enables the high-speed high-accuracy control II if G05P10000 is commanded in a sub part system.
(*8) In M80 Type B, the following program errors occur depending on the G codes.
12 G54-G59 Workpiece coordinate system selection G54.1
13 G61 Exact stop check mode G61.1 High-accuracy control (*3) (*2) G61.2 High-accuracy spline (P29) (*8) (P29) (*8) G61.4 Spline interpolation 2 (*8) (*8) G62 Automatic corner override G63 Tapping mode G64 Cutting mode (*3) (*2)
14 G66 G66.1
User macro modal call
G67 User macro modal call cancel 15 G40.1 Normal line control cancel
G41.1 G42.1
Normal line control (P29) (*8) (P29) (*8)
16 G68 Coordinate rotation by program ON 3-dimensional coordinate conversion ON (P922) (P921)
G68.2 G68.3
Inclined surface machining command (*8) (*8)
G69 Coordinate rotation cancel 17 G96 Constant surface speed control ON
G97 Constant surface speed control OFF 18 G15 Polar coordinate command OFF
G16 Polar coordinate command ON 19 G50.1 Mirror image OFF
G51.1 Mirror image ON 21 G07.1 Cylindrical interpolation (P34) (P481)
G12.1 Polar coordinate interpolation ON (P34) (P481) G13.1 Polar coordinate interpolation OFF
27 G54.4P0 Workpiece installation error compensation cancel
G54.4 P1-P7
Workpiece installation error compensation (*8) (*8)
G code Program error G code Program error
G05.1Q2, G92.1, G122, G61.2, G61.4
P39 G10 I_J_/G10 K_ P260 G06.2 P550
G144, G54.4 P1-P7 P34 G93 P124 G07 P80 G41.1, G42.1 P900 G02.1, G03.1 P73 G43.1 P930 G02.3, G03.3 P611 G43.4, G43.5 P940 G02.4, G03.4 P76 G68.2, G68.3 P950
Group G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
712IB-1501278-P
(2) Relationship between the high-speed high-accuracy control II and functions other than G codes Column A: Operation when the additional function is commanded while the high-speed high-accuracy control II is enabled Column B: Operation when the high-speed high-accuracy control II (G05P10000) is commanded while the ad- ditional function is enabled : The high-speed high-accuracy control II and the additional function are both enabled : The high-speed high-accuracy control II is temporarily canceled, while the additional function is enabled : Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination : Others
(*1) Enables the high-speed high-accuracy control II in a subprogram.
(*2) Enables the high-speed high-accuracy control II if G05P10000 is commanded in a subprogram.
(*3) Enables timing synchronization.
(*4) Enables the high-speed high-accuracy control II in a MTB program.
(*5) Enables the high-speed high-accuracy control II if G05P10000 is commanded in a MTB program.
(*6) Enables the high-speed high-accuracy control II in an interrupt program.
(*7) Enables the high-speed high-accuracy control II if G05P10000 is commanded in an interrupt program.
(*8) Disables the high-speed high-accuracy control II in a figure rotation subprogram.
(*9) The high-speed high-accuracy control II is disabled even if G05P10000 is commanded in a figure rotation subprogram.
(*10) In M80 Type B, the following program error occurs depending on the function type.
Function name A B
SSS ON - Mirror image by parameter setting ON - Mirror image by external input - Coordinate rotation by parameter - Subprogram call (M98) (*1) (*2) Figure rotation (M98 I_J_K_) (*8)(*10) (*9)(*10) Timing synchronization between part systems (*3) - MTB macro (*4) (*5) Macro interruption (*6) (*7) PLC interruption (*6) (*7) Corner chamfering/Corner R - Linear angle command - Geometric command - Chopping Fairing/smooth fairing ON Optional block skip -
Function Program error
Figure rotation (M98 I_J_K_) P250
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
713 IB-1501278-P
(1) Relationship between the high-speed high-accuracy control III and G code functions Column A: Operation when the additional function is commanded while the high-speed high-accuracy control III is enabled Column B: Operation when the high-speed high-accuracy control III (G05P20000) is commanded while the ad- ditional function is enabled : The high-speed high-accuracy control III and the additional function are both enabled : The high-speed high-accuracy control III is temporarily canceled, while the additional function is enabled : Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination : Others
Relationship between the high-speed high-accuracy control III and other functions
Group G code Function name A B
0 G04 Dwell - G05P0 High-speed machining mode II OFF
High-speed high-accuracy control II OFF High-speed high-accuracy control III OFF
(*1) (*2)
G05P2 High-speed machining mode II ON (*8) (*2) G05P10000 High-speed high-accuracy control II ON (*3) (*2) G05P20000 High-speed high-accuracy control III ON (*3) (*3) G05.1Q0 High-speed high-accuracy control I OFF
Spline interpolation OFF (*3) (*2)
G05.1Q1 High-speed high-accuracy control I ON (P34) (P34) G05.1Q2 Spline interpolation ON (*4) G07 Hypothetical axis interpolation G08P0 High-accuracy control OFF (*4) (*2) G08P1 High-accuracy control ON (*4) (*2) G09 Exact stop check - G10 I_J_ G10 K_
Parameter coordinate rotation input -
G10 L2 Compensation data input by program - G10 L70 G10 L50
Parameter input by program -
G27 Reference position check - G28 Reference position return - G29 Start position return - G30 2nd to 4th reference position return - G30.1- G30.6
Tool exchange position return -
G31 Skip Multiple-step skip 2
-
G31.1- G31.3
Multi-step skip -
G34-G36 G37.1
Special fixed cycle -
G37 Automatic tool length measurement - G38 Tool radius compensation vector designation - G39 Tool radius compensation corner circular com-
mand -
G50.2/G250 Tool spindle synchronization IB (spindle-spindle, polygon)/IIC (spindle-NC Axis, polygon) cancel
G51.2/G251 Tool spindle synchronization IB (spindle-spindle, polygon) ON
Tool spindle Synchronization IC (spindle-NC Ax- is, polygon) ON
G52 Local coordinate system setting -
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
714IB-1501278-P
0 G53 Machine coordinate system selection - G60 Unidirectional positioning - G65 User macro simple call (*5) (*6) G92 Coordinate system setting - G92.1 Workpiece coordinate system preset - G113.1 Spindle synchronization OFF G114.1 Spindle synchronization ON G114.2 Tool spindle synchronization IA (spindle-spindle,
polygon mode)
G114.3 Tool spindle synchronization II (hobbing) G122 Sub part system control I (P652) (*7) G144 Sub part system control II (P652) (*7)
1 G00 Positioning G01 Linear interpolation G02 G03
Circular interpolation
G02.1 G03.1
Spiral interpolation (*4)
G02.3 G03.3
Exponential interpolation (P34)
G02.4 G03.4
3-dimensional circular interpolation (P34)
G06.2 NURBS interpolation - G33 Thread cutting (*4)
2 G17-G19 Plane selection 3 G90 Absolute command
G91 Incremental command 4 G22 Stroke check before travel ON (*4)
G23 Stroke check before travel OFF 5 G93 Inverse time feed (*4)
G94 Asynchronous feed (feed per minute) G95 Synchronous feed (feed per revolution) (*4)
6 G20 Inch command G21 Metric command
7 G40 Tool radius compensation cancel (*9) G41 G42
Tool radius compensation (*4)
8 G43
G44
Tool length offset
G43.1 Tool length compensation along the tool axis (*4) G43.4 G43.5
Tool center point control (*4)
G49 Tool length offset cancel 9 G80 Fixed cycle cancel
Group 9 Other than G80
Fixed cycle (*4)
10 G98 Fixed cycle initial level return G99 Fixed cycle R point return
11 G50 Scaling cancel G51 Scaling ON (*4)
12 G54-G59 Workpiece coordinate system selection G54.1
Group G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
715 IB-1501278-P
(*1) Disables the high-speed high-accuracy control III.
(*2) Enables the high-speed high-accuracy control III.
(*3) High-speed high-accuracy control III continues.
(*4) Enables the high-speed high-accuracy control II.
(*5) Enables the high-speed high-accuracy control III in a macro program.
(*6) Enables the high-speed high-accuracy control III if G05P20000 is commanded in a macro program.
(*7) Enables the high-speed high-accuracy control III if G05P20000 is commanded in a sub part system.
(*8) Enables the high-speed machining mode II.
(*9) When the parameter "#1271 ext07/bit4" is set to "1", the compensation vector is retained until positioning is commanded even after the cancel command (G40) has been issued for the tool radius compensation. This condition enables the high-speed high-accuracy control II. When the compensation vector is set to "0" in accordance with the positioning command, the high-speed high-accuracy control III is enabled.
13 G61 Exact stop check mode (*4) (*4) G61.1 High-accuracy control (*4) (*2) G61.2 High-accuracy spline (P29) (P29) G61.4 Spline interpolation 2 (*4) (*4) G62 Automatic corner override (*4) (*4) G63 Tapping mode (*4) (*4) G64 Cutting mode (*4) (*2)
14 G66 G66.1
User macro modal call (*4)
G67 User macro modal call cancel 15 G40.1 Normal line control cancel (P29)
G41.1 G42.1
Normal line control (P29) (*4)
16 G68 Coordinate rotation by program ON (*4) (*4) 3-dimensional coordinate conversion ON (P922) (P921)
G68.2 G68.3
Inclined surface machining command (*4)
G69 Coordinate rotation cancel 17 G96 Constant surface speed control ON
G97 Constant surface speed control OFF 18 G15 Polar coordinate command OFF
G16 Polar coordinate command ON (*4) 19 G50.1 Mirror image OFF
G51.1 Mirror image ON (*4) 21 G07.1 Cylindrical interpolation (P34) (P481)
G12.1 Polar coordinate interpolation ON (P34) (P481) G13.1 Polar coordinate interpolation OFF
27 G54.4P0 Workpiece installation error compensation can- cel
G54.4P1-P7 Workpiece installation error compensation (*4)
Group G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
716IB-1501278-P
(2) Relationship between the high-speed high-accuracy control III and functions other than G codes Column A: Operation when the additional function is commanded while the high-speed high-accuracy control III is enabled Column B: Operation when the high-speed high-accuracy control III (G05P20000) is commanded while the ad- ditional function is enabled : The high-speed high-accuracy control III and the additional function are both enabled : The high-speed high-accuracy control III is temporarily canceled, while the additional function is enabled : Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination : Others
(*1) Enables the high-speed high-accuracy control II.
(*2) Enables the high-speed high-accuracy control III in a subprogram.
(*3) Enables the high-speed high-accuracy control III if G05P20000 is commanded in a subprogram.
(*4) Enables timing synchronization.
(*5) Enables the high-speed high-accuracy control III in a MTB program.
(*6) Enables the high-speed high-accuracy control III if G05P20000 is commanded in a MTB program.
(*7) Enables the high-speed high-accuracy control III in an interrupt program.
(*8) Enables the high-speed high-accuracy control III if G05P20000 is commanded in an interrupt program.
(*9) Disables the high-speed high-accuracy control III in a figure rotation subprogram.
(*10) The high-speed high-accuracy control III is disabled even if G05P20000 is commanded in a figure rotation subprogram.
Function name A B
SSS ON - SSS OFF - (*1) Mirror image by parameter setting ON - Mirror image by external input - Coordinate rotation by parameter - Subprogram call (M98) (*2) (*3) Figure rotation (M98 I_J_K_) (*9) (*10) Timing synchronization between part systems (*4) - MTB macro (*5) (*6) Macro interruption (*7) (*8) PLC interruption (*7) (*8) Corner chamfering/Corner R - Linear angle command - Geometric command - Chopping Fairing/smooth fairing ON (*1) (*1) Optional block skip (*1) -
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
717 IB-1501278-P
17.3.2 Fairing
This function is an additional function when the high-speed high-accuracy control II or III mode is ON If there is a protrusion in a path (zigzagging path) in a machining program generated with a CAM, etc., this function can be used to eliminate the protruding path smaller than the setting value so that the protruding path is smoothly connected with the previous and the next paths. This function is valid only for continuous linear commands (G01).
If there is any protruding path after fairing, fairing is repeated.
Function and purpose
Related parameter Contents
#8033 Fairing ON 0: Fairing invalid 1: Execute fairing for the protruding block. 2: Smooth fairing valid
#8029 Fairing L Execute fairing for the shorter block than this setting value.
Before fairing After fairing Path before/after fairing execution
Before fairing After first fairing After final fairing Path in repetitive fairing executions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
718IB-1501278-P
17.3.3 Smooth Fairing
This function is an additional function when the high-speed high-accuracy control II or III mode is ON A path can be smoothen by compensating commanded positions of a machining program. This function is useful when executing a fine segment program to machine smoothly at low speed or a rough ma- chining program with long segment to machine smoothly. This function is enabled while high-speed high-accuracy control II or III is ON or while high-accuracy control is ON in high-speed machining mode II, and performs compensation on consecutive G01 command during this time. The validity of this function depends on the MTB specifications. To use this function, the high-speed high-accuracy control II or III specification, or the high-speed machining mode II and high-accuracy control specifications are re- quired.
(1) High-speed high-accuracy control III functions as high-speed high-accuracy control II while smooth fairing is ON.
Faring and smooth faring differ as follows:
Function and purpose
Fairing Smooth fairing
Operation Eliminating blocks shorter than designated length
Compensating commanded positions across multiple blocks
Usage Eliminating minute steps to occur at fillet and other sections Eliminating noises on commanded paths
Smooth machining at low speed for a fine segment program Smooth machining for a rough machining
program
Note
G90 G00 X0.271 Y0.161; G01; N01 X0.319 Y0.249; N02 X0.415 Y0.220; N03 X0.475 Y0.299; N04 X0.566 Y0.256; N05 X0.638 Y0.325; N06 X0.720 Y0.268; N07 X0.803 Y0.325; N08 X0.875 Y0.256; N09 X0.965 Y0.299; N10 X1.026 Y0.220; N11 X1.122 Y0.249; N12 X1.169 Y0.161;
N01 N03
N11
N05 N09N07
N02 N04 N06 N08
N10 N12
Commanded position
Commanded position
Tool path Tool pathCommanded position
Compensated position
Commanded path
Smooth fairing OFF Smooth fairing ON
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
719 IB-1501278-P
When a minute step exists on a commanded path, for instance, the path after compensation differs between fairing and smooth fairing as follows:
Refer to "Relationship with other functions" for the relationship between smooth fairing and other functions.
To enable smooth fairing, it is necessary for the following conditions to be satisfied respectively:
(a) The smooth fairing specification is set to ON. (b) One of the following modes is set to ON. G05 P20000 (*1) G05 P10000 G05 P2 and the high-accuracy function (G61.1/G08P1 or G61.2) are used simultaneously.
(c) At least one of the following conditions is satisfied. The parameter "#8033 Fairing ON" is set to "2". The G05 P20000, R1/G05 P10000, R1/G05 P2, or R1 command is issued.
(*1) This command functions as G05 P10000 while smooth fairing is ON.
Detailed description
Enabling conditions
G90 G00 X0 Y0;
G01;
N01 X0.100 Y0.000;
N02 X0.200 Y0.000;
N03 X0.300 Y0.000;
N04 X0.400 Y0.000;
N05 X0.500 Y0.000;
N06 X0.500 Y0.010;
N07 X0.600 Y0.010;
N08 X0.700 Y0.010;
N09 X0.800 Y0.010;
N10 X0.900 Y0.010;
N01 N02 N03 N04 N05 N06
N07 N08 N09 N10
Commanded position
Path after compensation
Eliminates blocks shorter than designated length.
Compensates commanded positions in blocks around a step.
Commanded path
Path after compensation by fairing
Path after compensation by smooth fairing
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
720IB-1501278-P
Two methods are available to enable smooth fairing: "G05 Pp,Rr command" and parameter "#8033 Fairing ON" ((c) of the enabling conditions).
Relationship between ",R" address and parameter "#8033 Fairing ON"
: Smooth fairing ON, : Fairing ON, X: Both OFF
(1) When the ",R" address is set to the G05 command, the operation shown in the table below is performed regard- less of the setting value of the parameter "#8033".
(2) The ",R" address is unmodal information. The ",R" address value designated by previous G05 command is not inherited to the next and subsequent G05 commands. Each time the G05 command is issued, the fairing function is switched as shown in the table above.
(3) To switch smooth fairing and fairing, insert the G05P0; command between them. If this switching is commanded without inserting the G05P0 command, a program error (P560) will occur.
Enabling smooth fairing
Parameter "#8033 Fairing ON"
0 1 2
Both OFF Fairing ON Smooth fairing ON
G05 P20000 G05 P10000 G05 P2 Command
No ,R ,R0 ,R1
Smooth fairing ON G05 P20000, R1 G05 P10000, R1 G05 P2, R1
Smooth fairing is ON regardless of the set- ting value of the parameter "#8033".
G05 P20000, R0 G05 P10000, R0 G05 P2, R0
Both fairing and smooth fairing are OFF regardless of the setting value of the pa- rameter "#8033".
G05 P0,Rr (r=0,1) G05 P1,Rr (r=0,1)
Program error (P33)
Smooth fairing OFF G05 P20000,Rr (r=0,1) G05 P10000,Rr (r=0,1) G05 P2,Rr (r=0,1) G05 P1,Rr (r=0,1) G05 P0,Rr (r=0,1)
Program error (P39)
Machining program Operation
N01 G05 P10000, R1; ... In this period, the program runs with G05 P10000, R1. N02 G05 P0; N03 G05 P10000; The ",R" address of the N01 G05 command is not inherited.
... In this period, the program runs with G05 P10000 (without the ",R" ad- dress).
N04 G05 P0;
Machining program Operation
N01 G05 P10000, R1; Set the parameter "#8033" to "1". ... In this period, the program runs with smooth fairing. N03 G05 P10000; Issuing this command switches to fairing, which causes an error.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
721 IB-1501278-P
(4) To enable smooth fairing without setting the ",R" address to the G05 command, set the parameter "#8033 Fairing ON" to "2". The following operation is performed.
An operation example is as follows. (In this figure, symbol indicates the compensated position, and symbol indicates the commanded position.)
(1) Smooth fairing smoothens the path by compensating the positions designated by successive G01 commands. This function recognizes the paths before and after each commanded position, and compensates commanded positions that cause a path to become unsmooth.
: Compensated position
: Commanded position
G05 P20000 G05 P10000 G05 P2
Smooth fairing ON
G05 P1 G05 P0 Both fairing and smooth fairing are OFF
Details of Operation
[Commanded path] (indicated by dashed lines) G90 G00 X0.322 Y0.234; G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.798 Y0.399; N06 X0.900 Y0.343; N07 X1.003 Y0.399; N08 X1.095 Y0.328; N09 X1.205 Y0.367; N10 X1.284 Y0.282; N11 X1.399 Y0.304; N12 X1.465 Y0.207;
[Path after compensation] (indicated by solid lines) The smooth parts are not targeted for compensation.
Only the unsmooth parts are compensated.
NO1
NO2 NO3
NO5 NO6 NO8NO7
NO9 NO10
NO11 NO12
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
722IB-1501278-P
(2) The path recognition range is determined by the parameter "#8038 Path recog. range". Determine the setting value to include multiple G01 commands in the path recognition range. When the setting value is "0", the range is set to "1.0 (1 mm)". When the path recognition range is set to 0.5 mm:
(3) The upper limit of the compensation distance can be determined so that the compensated position does not de- viate from the commanded position significantly. Designate this upper limit in the parameter "#8039 Comp. range limit". Ordinarily, designate the tolerance that is designated when generating the machining program with CAM. When the setting value is "0", the range is set to "0.005 (5 microns)". (a) When the compensation distance tolerance is high:
(b) When the compensation distance tolerance is low:
G90 G00 X0.322 Y0.234; G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.800 Y0.369; N06 X0.900 Y0.423; N07 X1.000 Y0.369; N08 X1.099 Y0.357; N09 X1.198 Y0.338; N10 X1.294 Y0.311; N11 X1.388 Y0.276; N12 X1.478 Y0.234;
The path is recognized in the range of 0.5 mm forward and 0.5 mm backward of the commanded position.
G90 G00 X0.322 Y0.234; G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.800 Y0.369; N06 X0.900 Y0.423; N07 X1.000 Y0.369; N08 X1.099 Y0.357; N09 X1.198 Y0.338; N10 X1.294 Y0.311; N11 X1.388 Y0.276; N12 X1.478 Y0.234;
G90 G00 X0.322 Y0.234; G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.800 Y0.369; N06 X0.900 Y0.423; N07 X1.000 Y0.369; N08 X1.099 Y0.357; N09 X1.198 Y0.338; N10 X1.294 Y0.311; N11 X1.388 Y0.276; N12 X1.478 Y0.234;
0.1mm 0.1mm 0.1mm
0.1mm 0.1mm
0.1mm 0.1mm
0.1mm 0.1mm 0.1mm
0.11mm 0.11mm
NO6 NO7
Compensation range tolerance
Desirable compen- sation position
Actual compensa- tion position
Compensation range tolerance
Desirable compen- sation position
Actual compensa- tion position
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
723 IB-1501278-P
(4) While smooth fairing is ON, the modal or mode status is changed, and smooth fairing may be set to OFF. While smooth fairing is OFF, the commanded position is not compensated, and the axis moves as commanded. For details on the modal or mode status that causes smooth fairing to be set to OFF, refer to "Relationship with other functions".
(5) While smooth fairing is ON, it may be canceled temporarily depending on commands when: there is a block that contains only a sequence number; the modal status of the absolute/incremental command is changed by the G90 or G91 command; and the movement command is issued to an axis other than the three basic axes.
If a command that triggers a temporary cancel is inserted, the axis moves to the commanded position once. For the list of commands that trigger a temporary cancel, refer to "Relationship with other functions".
While smooth fairing is OFF, the axis moves to the commanded posi- tion.
G90 G00 X0.0 Y0.0; G01; N01 G01 X0.039 Y0.077; N02 G01 X0.139 Y0.080; N03 G01 X0.172 Y0.174; N04 G01 X0.271 Y0.161; N05 G01 X0.319 Y0.249; N06 G02 X1.122 Y0.249 R0.5; N07 G01 X1.169 Y0.161; N08 G01 X1.268 Y0.174; N09 G01 X1.301 Y0.080; N10 G01 X1.401 Y0.077; N11 G01 X1.441 Y0.000;
Compensation restarts from the block in which the enabling conditions are satisfied again.
G90 G00 X0.322 Y0.234; G90 G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.798 Y0.399; N06 X0.900 Y0.343; N07; N08 X1.003 Y0.399; N09 X1.095 Y0.328; N10 X1.205 Y0.367; N11 X1.284 Y0.282; N12 X1.399 Y0.304; N13 X1.465 Y0.207;
If a block that triggers a temporary cancel is inserted, the axis moves to the com- manded position once.
NO6
Valid Invalid Valid
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
724IB-1501278-P
(1) Relationship between smooth fairing and other G code functions
Relationship with other functions
A Shows if smooth fairing is valid or not when the G code function on the left is enabled. (valid): Compensates for the commanded position. (invalid): Does not compensate the commanded position.
B Shows operation when the G code on the left is commanded together with a movement command (XYZ address command)(*) while smooth fairing is ON. (continuation): Compensates for the commanded position. (temporary cancel): Temporarily suspends compensation to move to the commanded position.
Temporary cancel for blocks with no movement commands (example: the block where G90 is com- manded alone).
G code group
G code Function name A B
0 G05 High-speed machining mode/high-speed high-accuracy control
(*1) -
G08 High-accuracy control G command in group 0 except the above -
1 G01 Linear interpolation G command in group 1 except the above
2 G17/G18/G19 Plane selection (*2) 3 G90/G91 Absolute command/incremental command (*2) 4 G23 Stroke check before travel OFF
G command in group 4 except the above 5 G94 Asynchronous feed (feed per minute)
G command in group 5 except the above 6 G20/G21 Inch/Metric command 7 G40 Tool radius compensation cancel/3-dimensional tool radius
compensation cancel
G41/G42 Tool radius compensation/3-dimensional tool radius com- pensation
G command in group 7 except the above 8 G43/G44 Tool length offset + /tool length offset -
G43.1 Tool length compensation along the tool axis G49 Tool length offset cancel
G command in group 8 except the above 9 G80 Fixed cycle cancel
G command in group 9 except the above 10 G98/G99 Fixed cycle initial level return/R point level return 11 G50 Scaling cancel
G command in group 11 except the above 12 G54-G59/G54.1 Workpiece coordinate system selection 13 G61.1 High-accuracy control ON
G61.2 High-accuracy spline G command in group 13 except the above
14 G67 User macro modal call cancel G command in group 14 except the above
15 G40.1/G150 Normal line control cancel G command in group 15 except the above
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
725 IB-1501278-P
(*1) (valid) for G05P2/G05P10000/G05P20000 and X (invalid) for the others.
(*2) (continuation) if the modal state does not change before and after the command and X (temporary cancel) otherwise.
(*3) (Valid) for G54.4P0 and X (invalid) for the others.
(2) Relationship between smooth fairing and functions other than G codes
(*1) When there is a block containing only EOB, compensation is not temporarily canceled. However, in such a case, the path slightly changes compared to when there are no blocks containing only EOB.
(*2) PLC interruption is not allowed during high-speed high-accuracy control II/III.
16 G69 Coordinate rotation cancel/3-dimensional coordinate con- version cancel
G command in group 16 except the above 17 G96/G97 Constant surface speed control ON/OFF 18 G15 Polar coordinate command OFF
G command in group 18 except the above 19 G50.1 Mirror image by G code OFF
G command in group 19 except the above 21 G13.1/G113 Cylindrical interpolation/polar coordinate interpolation OFF
G command in group 21 except the above 27 G54.4 Workpiece installation error compensation (*3)
A Shows if smooth fairing is valid or not when the function on the left is enabled. (valid): Compensates for the commanded position. (invalid): Does not compensate the commanded position.
B Shows operation when the function on the left is commanded while smooth fairing is ON. (continuation): Compensates for the commanded position. (temporary cancel): Temporarily suspends compensation to move to the commanded position.
Function other than G code A B
Block containing only EOB(;) - (*1) Block containing only comment - Block containing only sequence number - Block containing only MSTB command - Block containing only F command - If there is an axis movement command for other than three base axes - Block without movement command - During single block operation Subprogram call (M98 P_) Figure rotation subprogram call (M98 P_I_J_K_) Macro interruption (M96, UIT) User macro simple call User macro modal call MTB macro PLC interruption (PIT) (*2) Coordinate rotation by parameter (G10 I_J_/K_) Mirror image by parameter setting (#8211 Mirror image) Mirror image with PLC signals ON
G code group
G code Function name A B
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
726IB-1501278-P
The table below shows which fairing functions are enabled according to the combination of the parameter "#8033 Fairing ON" setting and G command:
: Smooth fairing ON, : Fairing ON, X: Both OFF
"#8033 Fairing ON"
0 1 2
Both OFF Fairing ON Smooth fairing ON
G05 P0 G61.1 G61.2
G05 P2 G61.1 G61.2
G05 P10000 G05 P20000
G5.1 Q0 G5.1 Q2
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
727 IB-1501278-P
17.3.4 Cutting Speed Clamp with Acceleration Rate Judgment
This function is an additional function when the high-speed high-accuracy control II mode is ON. The cutting feed clamp speed during the high-speed high-accuracy control II / III mode, when the following param- eter is set to "1", is clamped so that the acceleration rate generated by each block movement does not exceed the tolerable value. This function clamps the speed optimally even at a section where "angle change at each block is small but entire curvature is large" such as shown below. The tolerable value of the acceleration rate is calculated from the parameter "#1206 G1bF" and "#1207 G1btL" set- ting values. (Tolerable acceleration rate = #1206/#1207)
(*1) When a speed is set in "#2109 Clamp(H-precision)", clamp is executed at that speed. When the setting value is "0", clamp is executed with "#2002 clamp".
Function and purpose
Related parameter Details
#8034 AccClampt ON 0 : Clamp the cutting speed with parameter "#2002 clamp" (*1) or the corner deceleration function.
1 : Clamp the cutting speed with acceleration rate judgment.
If the tool moves along the large curvature section without deceler- ation, a large acceleration rate is generated resulting in a path error by curving inward.
Speed control by curvature
R
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
728IB-1501278-P
17.3.5 High-speed Mode Corner Deceleration
This function is an additional function when high-speed high-accuracy control II mode is ON. During high-accuracy control, if the angle between the adjacent blocks in the machining program is large, this func- tion, conventionally, automatically decelerates the machining so that the acceleration rate generated when passing through the corner is maintained within the tolerable value. If a fine block is inserted at the corner section in the machining program generated with the CAM, etc., the corner passing speed will not match the periphery. This can affect the machining surface. In the corner deceleration in the high-speed mode, even when this type of fine block is inserted, the corner will be judged from a vantage point by setting the below parameter. The fine block is excluded at the judgment of an angle, but is not excluded from the actual movement command.
(a) When"#8036 CordecJudge" is set to "1", corner deceleration is realized without an influence of fine blocks.
Function and purpose
Related parameter Details
#8036 CordecJudge 0 : Judge the corner from the angle of the neighboring block. 1 : Judge the corner from the angle of the neighboring block, excluding
the minute blocks. #8027 CorJudgeL Exclude shorter block than this setting value.
High-speed mode corner deceleration
(a)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
729 IB-1501278-P
17.3.6 Precautions on High-speed High-accuracy Control
(1) The validity of each high-speed high-accuracy control function depends on the MTB specifications. If any of the above is commanded when the corresponding specification is not available on the machine, a program error (P39) will occur.
(2) The machining speed may drop depending on the number of characters in one block. (3) Feedrate command F is clamped with the "#2110 Clamp (H-precision)" (Cutting feed clamp speed for high-ac-
curacy control mode) set with the parameter. (4) The rapid traverse rate conforms to "#2109 Rapid(H-precision)" (Rapid traverse rate during high-accuracy con-
trol mode) set with the parameter. (5) When "#2109 Rapid(H-precision)" (high-accuracy control mode rapid traverse rate) is set to "0", however, the
movement follows "#2001 rapid" (Rapid traverse rate) set with the parameter. Also, when "#2110 Clamp (H-pre- cision)" (Cutting feed clamp speed for high-accuracy control mode) is set to "0", the speed will be clamped with "#2002 clamp" (Cutting clamp speed) set with parameter.
(6) The automatic operation processing has priority in the high-speed high-accuracy control I/II/III modal, so the screen display, etc., may be delayed.
(7) The speed will decelerate once at the high-speed high-accuracy control I command (G05.1 Q1), high-speed high-accuracy control I OFF command (G05.1 Q0), high-speed high-accuracy control II command (G05P10000), high-speed high-accuracy control III command (G05P20000), and high-speed high-accuracy control II/III OFF command (G05P0), so turn ON and OFF when the tool separates from the workpiece.
(8) When carrying out high-speed high-accuracy control I/II operation during tape mode, the machining speed may be suppressed depending on the program transmission speed and the number of characters in one block.
(9) If "#1205 G0bdcc" (G0 acceleration/deceleration before interpolation) is set to "1", the value set with the param- eter "#2224 SV024 INP" (in-position detection width) will be used as the in-position width. "#2077 G0inps" (G0 in-position width) and the ",I" command (programmable in-position check) are disabled.
(10) When the fairing is valid (#8033 = "1"), if consecutive fairing is executed by the machining program, the fine segment processing capability may become lower than that in the tables (1) to (3) of "Fine segment processing capability" in "17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/ P0".
(11) When the "Manual/Automatic simultaneous valid n-th axis" signal (Y920) is changed during the execution of the movement blocks for the pre-interpolation acceleration/deceleration, the change will not be enabled immediately even if the axes are not moving. The change will be enabled when all the axes in the part system decelerate and stop.
(*1) "III" is a function only for the machining center.
(1) If the variable command, variable operation command, or macro control statement is commanded while high- speed high-accuracy control II/III is enabled, the fine segment processing capability may decelerate. However, only when the variable commands and variable four-basic-arithmetic operation commands shown below are is- sued following the axis address or the F address of the cutting feedrate command, the fine segment processing capability does not decelerate. (a) Referencing common variables or local variables
Common variables or local variables can be referenced (example: X#500, Y#1, Z##100, A#[#101], etc.). (b) Four basic arithmetic rule
Four basic arithmetic rule (+, -, *, /) operations are available, and also the operation priority can be designated using parentheses ( ) ([#500 + #501] * #502, etc.).
If a common variable or local variable is referenced using the variable number operated with a macro operation instruction, a program error (P282) may occur. In this case, set the operated value to the variable before refer- encing the variable.
Precautions
Common precautions on high-speed high-accuracy control I/II/III
Common precautions on high-speed high-accuracy control II/III (*1)
Example that causes an error F#[FIX[100.1]]; Example that does not cause an error #500 = FIX[100.1] ;
F#[#500] ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
730IB-1501278-P
(1) Command "G05.1Q0 ;" after turning the tool radius compensation OFF. If "G05.1Q0;" is commanded without turning the tool radius compensation OFF, a program error (P29) will occur.
(2) "G05.1Q1;" must be commanded alone in a block, which also applies to "G05.1Q0;". If a sequence number other than "N" is commanded, a program error (P33) will occur.
(3) A program error (P33) will occur if the G05.1 command block does not contain a Q command. (4) If the high-speed high-accuracy control I command is issued in the high-speed high-accuracy control II modal, a
program error (P34) will occur. (5) To command the high-speed high-accuracy control I during cylindrical interpolation, command "G05.1 Q0" before
canceling cylindrical interpolation (G07.1 C0) to cancel high-speed high-accuracy control I. When cylindrical in- terpolation is canceled during the high-speed high-accuracy control I, the program error (P485) occurs.
(1) "G05P10000;" must be commanded alone in a block, which also applies to "G05P0;". If a sequence number other than "N" is commanded, the program error (P33) will occur.
(2) A program error (P33) will occur if the G05 command block does not contain a P command. (3) The fairing function is valid for the continuous linear command (G01). Fairing is not possible in the case below.
(4) In a single block mode, operation stops at the end point of each block. (5) When using the high-speed high-accuracy control II mode, set the parameter "#1572 Cirorp/bit0" to "1" to elimi-
nate the speed fluctuation at the seams between the arc and the straight line, or between arcs. (6) A program error (P33) will occur if the geometric command is issued during the high-speed high-accuracy control
II. (7) If the high-speed high-accuracy control II command is issued in the high-speed high-accuracy control I modal, a
program error (P34) will occur. (8) A program error (P922) will occur if 3-dimensional coordinate conversion is issued during the high-speed high-
accuracy control II. (9) A program error (P921) will occur if the high-speed high-accuracy control II is commanded during 3-dimensional
coordinate conversion.
Precautions on high-speed high-accuracy control I
Precautions on high-speed high-accuracy control II
G02
G01 G02
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
731 IB-1501278-P
(1) "G05P20000;" must be commanded alone in a block, which also applies to "G05P0;". If a sequence number other than "N" is commanded, a program error (P33) will occur.
(2) A program error (P33) will occur if the G05 command block does not contain a P command. (3) A program error (P33) will occur if the geometric command is issued during the high-speed high-accuracy control
III. (4) If the high-speed high-accuracy control III command is issued in the high-speed high-accuracy control I modal,
a program error (P34) will occur. (5) If the high-speed high-accuracy control II mode is valid when high-speed high-accuracy control III is commanded,
follow the precautions on high-speed high-accuracy control II. (6) High-speed high-accuracy control III can be enabled by commanding the G code from the machining program.
(a) High-speed high-accuracy control III command with the high-speed high-accuracy control III enable condi- tions satisfied If all modal conditions in each G code group and each mode condition shown in "Relationship with other func- tions" (*1) are satisfied when "G05P20000;" is commanded, the high-speed high-accuracy control III mode is enabled, and "G05P20000" is displayed on the modal screen. If conditions are not satisfied after "G05P20000;" has been commanded, the high-speed high-accuracy control III mode is enabled, however, the fine segment processing capability may decelerate.
(*1) For details, refer to "Relationship with other functions" in "17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0".
(*2) High-speed high-accuracy control III is enabled, but the fine segment processing capability described in the tables (1) to (3) of "Fine segment processing capability" in "17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0" may decelerate.
(*3) When the parameter "#1271 ext07/bit4" is "1", the tool radius compensation vector is retained until the positioning command is issued even after the cancel command (G40). In this state, high-speed high-ac- curacy control II is enabled. When the compensation vector changes to "0" by the positioning command, the high-speed high-accuracy control III is enabled.
(b) High-speed high-accuracy control III command with no high-speed high-accuracy control III enabling condi- tions satisfied If the conditions shown in "Relationship with other functions" (*1) are not satisfied when "G05P20000;" is com- manded, the high-speed high-accuracy control II mode is enabled, and "G05P10000" is displayed on the modal screen. In this case, even if all the conditions shown in "Relationship with other functions" (*1) are sat- isfied after "G05P20000;" has been commanded, the high-speed high-accuracy control III mode is not en- abled. To enable the high-speed high-accuracy control III mode, command "G05P20000;" again.
(7) A program error (P922) will occur if 3-dimensional coordinate conversion is issued during the high-speed high- accuracy control III.
(8) A program error (P921) will occur if the high-speed high-accuracy control III is commanded during 3-dimensional coordinate conversion.
Precautions on high-speed high-accuracy control III
Machining program Enable conditions for high-speed high-accuracy control III
Enable mode
G05 P20000; High-speed high-accuracy control III command
Enabling conditions are satisfied. G05P20000
G41 XxYyDd; Tool radius compensation ON Enabling conditions are not satisfied. G05P20000 (*2) G40 XxYy; Tool radius compensation OFF Enabling conditions are satisfied. G05P20000
Machining program Enable conditions for high- speed high-accuracy con-
trol III
Enable mode
G41 XxYyDd; Tool radius compensation ON Enabling conditions are not satisfied. G05P10000G05 P20000; High-speed high-accuracy control
III command G40 XxYy; Tool radius compensation OFF Enabling conditions are satis-
fied. G05P10000
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
732IB-1501278-P
17.4 Spline Interpolation ; G05.1 Q2/Q0
This function automatically generates a spline curve that passes through a sequence of points commanded by the fine segment machining program, and interpolates the path along this curve. This enables high-speed and high-ac- curacy machining to be achieved.
There are two types of spline interpolation command format: G61.2 and G05.1Q2. Both formats can be used regard- less of the parameter "#1267 ext03/bit0" setting if the spline interpolation specifications are available to the machine. This section describes the G05.1Q2 command. For G61.2, refer to "17.6 High-accuracy Spline Interpolation ; G61.2".
The G05.1Q2 command can be issued when the machining parameter "#8025 SPLINE ON" is set to "1" in the high- speed high-accuracy control function II or III mode. The following explanation is limited to the spline function in the high-speed high-accuracy control function II or III mode.
(1) High-speed high-accuracy control III functions as high-speed high-accuracy control II while spline interpolation is ON.
Conditions under which the command can be issued and functions that are valid during a specific modal differ be- tween G61.2 and G05.1Q2.
(*1) The validity of the high-speed high-accuracy control II or III function depends on the MTB specifications. A program error (P34) will occur if the conditions under which the command can be issued are not satisfied.
(*2) The spline interpolation smoothly connects a sequence of points commanded by program. As a result, the glossy machining surface can be obtained, and the machining time can be reduced because the frequency of the corner deceleration decreases compared with conventional linear interpolation.
Function and purpose
Difference between G61.2 and G05.1Q2
Command format Conditions under
which the command can be issued
Functions that become valid
Spline interpolation Fairing High-accuracy con- trol
(*2) (*3) (*4)
G61.2 None Valid Valid Valid G05.1 Q2 When the system is
in the high-speed high-accuracy control II or III mode and "#8025 SPLINE ON" is set to "1" (*1)
Valid Can be turned ON and OFF using "#8033 Fairing ON"
Valid (Because the system is in the high-speed high-accuracy control II or III mode)
G61.2/G05.1Q2
G64/G61.1
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
733 IB-1501278-P
(*3) Super-fine blocks often included in the data generated with CAM are deleted. Such a super-fine block may scratch the machining surface, and increase machining time because of acceleration/deceleration. This function prevents these problems.
(*4) The following shows the functions and their operations included in the high-accuracy control described in this section.
The validity of the SSS control function depends on the MTB specifications.
Functions of high-accuracy control
Contents
Acceleration/deceleration before interpolation (Constant-gradient acceleration/deceleration, S-pat- tern filter)
The process is the same as that performed in the high-accuracy control mode (G61.1/G08P1).
Optimum corner deceleration As is done in the high-accuracy control mode (G61.1/G08P1), optimum corner deceleration is performed at points where the angle between blocks exceeds the spline cancel angle or points at the boundary between G01 and G00, because spline interpolation is temporarily canceled to make corners.
Arc speed clamp (For spline in- terpolation, curvature speed clamp)
Clamp speed is calculated based on the spline curvature radius. The pro- cess for arc blocks is the same as that performed in the high-accuracy control mode (G61.1/G08P1).
Curvature radius speed clamp Clamp speed is calculated based on the spline curvature radius. Arc entrance/exit deceleration control
The process for arc blocks is the same as that performed in the high-ac- curacy control mode (G61.1/G08P1).
SSS Control Optimum speed control is performed so that the process is not affected by steps or reverse runs.
Feed forward control The process is the same as that performed in the high-accuracy control mode (G61.1/G08P1).
Command format
Spline interpolation mode ON
G05.1 Q2 X0 Y0 Z0 ;
Spline interpolation mode OFF
G05.1 Q0;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
734IB-1501278-P
Normally, once the spline function is activated, one curve is generated by smoothly connecting all points until it is canceled. However, if a corner edge should be created, or if the segment length is long and spline interpolation should not to be carried out, the function can be canceled temporarily with the parameters.
(1) Cancel angle If the angle of two consecutive blocks exceeds the value set in parameter "#8026 CANCEL ANG.", the spline function will be temporarily canceled, and optimum corner deceleration will be applied. When this parameter is not set (=0), the spline interpolation will be constantly applied. The corner deceleration angle of the high-accu- racy control function is valid during the temporary cancellation, and the optimum corner deceleration will be ap- plied.
(Example 1) Cancel angle = 60
(Example 2) Cancel angle = 0
If a smooth section becomes a corner, increase the "CANCEL ANG.". If "CANCEL ANG." >= "DCC ANGLE", the axis will decelerate at all corners where the angle is larger than
the "CANCEL ANG." . If the "CANCEL ANG." < "DCC ANGLE", corner deceleration will not be applied if the corner angle is equal
to or less than "DCC ANGLE" even if the spline interpolation is canceled.
Detailed description
Temporary cancellation of spline interpolation
Programmed command Spline interpolation path
Programmed command Spline interpolation path
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
735 IB-1501278-P
(2) Fine segment length If the movement amount in a block is longer than the parameter "#8030 MINUTE LENGS", the spline function will be temporarily canceled, and the linear interpolation will be executed. When this parameter is not set (= 0), the fine segment length will be 1mm. When the segment length in a block > fine segment length (#8030 MINUTE LENGS), the linear interpolation will be executed.
If the fine segment length is set to "-1", the spline interpolation will not be canceled according to the block length.
(3) When a block without movement exists If a block without movement exists during the spline function is operating, the spline interpolation will be canceled temporarily. Note that blocks containing only ";" will not be viewed as a block without movement.
(4) When a block markedly longer than other blocks exists in spline function Given that the i-th block length is Li in the spline interpolation mode and if the following condition is met, the block will be interpreted as a linear section, and the spline interpolation mode will be temporarily canceled: Li > Li-1 x 8 or Li > Li+1 x 8 However, if the parameter "#8030 MINUTE LENGS" is set to "-1", the mode will not be canceled.
Linear interpolation
Block without movement
Li > Li-1 8 or Li > Li + 1 8
Li+1Li - 1
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
736IB-1501278-P
Normally, once the spline function is enabled, one curve is generated by connecting all points smoothly until the function is canceled. But if the spline curve shape should be corrected, the spline curve shape can be corrected with the parameters.
(1) Chord error of block containing inflection point When changing the CAD curve data into fine segments with the CAM, normally, the tolerance (chord error) of the curve is approximated in segments that are approx. 10m. If there is an inflection point in the curve, the length of the block containing the inflection point may lengthen. (Because the tolerance is applied at both ends near the inflection point.) If the block lengths with this block and the previous and subsequent blocks are unbal- anced, the spline curve in this block may have a large error in respect to the original curve. At sections where the tolerance (chord error) of the fine segment block and spline curve in a block containing this type of inflection point, if the chord error in the corresponding section is larger than the value set in parameter (#8027 Toler-1), the spline curve shape is automatically corrected so that the error is within the designated value. However, if the maximum chord error of the corresponding section is more than five times larger than the param- eter "#8027" setting value, the spline function will be temporarily canceled.
The curve is corrected only in the corresponding block.
The corrections are carried out under the following conditions for each block in the spline interpolation mode.
When the above conditions are satisfied, the spline curve will be corrected so that the error between P3-P4 in Fig. 2 is within the designated value.
Spline interpolation curve shape correction
There is an inflection point in the spline curve, and the maximum error of the spline curve and linear block is larger than parameter "#8027". (Distance between P3-P4 in Fig. 1)
Tolerance (chord error) Spline curve
Inflection point
Fine segment
Fig. 1 Spline curve before error correction
P6 P5
P4
P7
P0
P1
P2 P3
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
737 IB-1501278-P
In parameter "#8027 Toler-1", set the tolerance when developed into fine segments with the CAM. Set a smaller value if the expansion (indentation) is apparent due to the relationship with the adjacent cutting paths.
(2) Chord error of block not containing inflection point Even in blocks that do not contain an inflection point, if the block lengths are not matched, the tolerance of the spline curve may increase. The curve may also expand due to the effect of relatively short blocks. At sections where the tolerance (chord error) between the fine segment block and spline curve in a block without an inflection point becomes large, if the chord error in the corresponding section is larger than the value set in parameter (#8028 Toler-2), the spline curve shape is automatically corrected so that the error is within the des- ignated value. However, if the maximum chord error of the corresponding section is more than five times larger than the parameter "#8028" setting value, the spline function will be temporarily canceled.
The curve is corrected only in the corresponding block.
The corrections are carried out under the following conditions for each block in the spline interpolation mode.
When the above conditions are satisfied, the spline curve will be corrected so that the error between P2-P3 in Fig. 4 is within the designated value.
Chord error designated in the parameter "Toler"
Spline curve before correction
Spline curve after correction
Fig. 2 Spline curve after error correction
There is no inflection point in the spline curve, and the maximum error of the spline curve and linear block is larger than parameter "#8028". (Distance between P2-P3 in Fig. 3)
Spline curve
Fine segment
Tolerance (chord error)
Fig. 3 Spline curve before error correction
P3
P4
P1
P2 P3
P4
P5
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
738IB-1501278-P
In parameter "Toler-2", set the tolerance when developed into fine segments with the CAM.
The commanded speed F for the spline function during a segment linear arc will be the speed commanded in the previously set modal. However, if the axis is fed with the same speed, excessive acceleration rate may occur at the sections where the curvature is large (where curvature radius is small) as shown below. Thus, the speed clamp will be applied.
With the spline function, the high-accuracy control function is always valid. Thus, even if the curvature changes such as in this curve, the speed will be clamped so that the tolerable value for pre-interpolation acceleration/deceleration, which is calculated with the parameters, is not exceeded. The clamp speed is set for each block, and the smaller of the curvature radius Rs at the curve block start point and the curvature radius Re at the end point of the block will be used as the main curvature radius R. Using this main curvature radius R, the clamp speed F' will be calculated with expression (1). The smaller of this clamp speed F' and the commanded speed F will be incorporated for the actual feedrate. This allows cutting with an adequate feedrate corresponding the curvature radius along the entire curve.
Chord error designated in the parameter "Toler-2" Spline curve before correction
Spline curve after correction
Fig. 4 Spline curve after error correction
Curvature speed clamp
(a) Curvature small (b) Acceleration rate small (c) Acceleration rate large (d) Curvature large F: Feed command speed (mm/min)
Change of acceleration rate by curvature
Rs : Block start point curvature radius (mm) Re : Block end point curvature radius (mm) R : Block main curvature radius (mm) (smaller one of Rs and Re) V : Tolerable value of pre-interpolation acceleration/deceleration F : Clamp speed (mm/min)
G1bF : Target pre-interpolation acceleration/decelera- tion G1btL : Acceleration/deceleration time to reach the tar- get speed Ks: Accuracy coefficient
P1
P2 P3
P4
P5
(c)F
F
(a)
(b)
(d)
Rs
Re
F'
V = G1bF(mm/min)
G1btL(ms)
F' = R V 60 1000 (1) 100- Ks
100
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
739 IB-1501278-P
(1) The spline function carries out spline interpolation when the following conditions are all satisfied. If the following conditions are not satisfied, the spline function will be canceled once, and the judgment whether to carry out new spline from the next block will be made. It is the movement only of three axes set to the basic axes I, J and K. When the block length is smaller than the value of the machining parameter "#8030 MINUTE LENGS". When the movement amount is not 0. When one of the following modes is entered.
G01: Linear interpolation, G40: Tool compensation cancel, G64: Cutting mode, G80: Fixed cycle cancel, G94: Feed per minute
When only an axis commanded with G05.1Q2 is commanded. A single block is not being executed.
(2) Graphic check will draw the shape of when the spline interpolation OFF. (3) During the spline function mode, the command to the axis must be issued after G05.1 Q2 in the same block. For
example, if the X axis and Y axis are to be commanded in the spline function mode, command "G05.1 Q2 X0 Y0;". The command block containing an axis not designated with this command (G05.1 Q2 X0 Y0) in the spline function mode will carry out linear interpolation instead of spline interpolation.
(4) If G05.1 Q2 is commanded when not in the high-speed high-accuracy control function II or III mode, the program error (P34) will occur.
(5) If the machining parameter "#8025 SPLINE ON" is "0" in the high-speed high-accuracy control function II or III mode and G05.1 Q2 is commanded, the program error (P34) will occur.
(6) Up to three axes set as the basic axes I, J and K can be commanded for the spline function.
Refer to "Relationship with other functions" in "17.2 High-accuracy Control".
(1) If this function are not provided and "G05.1 Q2" is commanded, the program error (P39) will occur. (2) Even if "-1" is set for parameter "#8030 MINUTE LENGS", the spline function will be temporarily canceled by the
cancel conditions (cancel angle, non-movement block, excessive chord error, etc.) other than the block length. (3) "G05.1 Q2" must be commanded alone in a block, which also applies to "G05.1 Q0".
A program error (P33) will occur if it is not commanded alone in a block. (4) The program error (P33) will occur if the G05.1 command block does not contain a Q command. (5) A program error (P34) will occur if the number of axis in the part system does not exceed 3.
Program example
: G91; G05 P10000; High-speed high-accuracy control function II mode ON : G05.1 Q2 X0 Y0 Z0; Spline interpolation mode ON G01 X1000 Z-300 F1000; X1000 Z-200; Y1000; X-1000 Z-50; X-1000 Z-300; G05.1 Q0; Spline interpolation mode OFF : G05 P0 ; High-speed high-accuracy control function II mode OFF :
Relationship with other functions
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
740IB-1501278-P
17.5 Spline Interpolation 2; G61.4
This function automatically generates a curve that smoothly passes through within the tolerable error range. The tool is able to move along the curve, providing smooth machining. This function allows the machine to operate with the optimum tool path and speed, simply by specifying the toler- ance, so an operator can easily attain high quality machining. This function also requires the tolerance control specifications because it can only be used under tolerance control. The tolerance refers to the allowable error amount between the path commanded in the machining program and the path output by NC.
When spline interpolation 2 is used in combination with tool center point control, spline interpolation 2 is performed with 5 axes. It generates a curve that passes through the tool center point points smoothly within the tolerance, with the rotary axis angle also within the tolerance. The tool moves along the curve.
This function is enabled when the following conditions are satisfied:
(1) SSS control is enabled. (2) Tolerance control is valid. (3) The specifications of spline interpolation 2 are valid. (4) "G61.4" is commanded from the machining program. (*1)(*2) (5) (When spline interpolation 2 is performed using 5 axes) Tool center point control command "G43.4" or "G43.5"
is given from within a machining program. (*3) (*1) If G61.4 is commanded while tolerance control is invalid, a program error (P34) occurs.
(*2) If G61.4 is commanded while the specifications of spline interpolation 2 are not defined, a program error (P39) occurs.
(*3) If G43.4 or G43.5 is given while the tool center point control specification is not provided, a program error (P39) occurs. For details on spline interpolation 2 using 5 axes, refer to "Behavior under tool center point control" in "Details of operation".
Function and purpose
Tolerance
Commanded position
Tool path
Tolerance of rotary axis
Commanded position
Tolerance of linear axis
Tool path
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
741 IB-1501278-P
Spline interpolation 2 mode with command G61.4 will be cancelled by designating any one of G code group 13.
G61 (Exact stop check mode) G61.1 (High-accuracy control mode) G61.2 (Spline interpolation command) G62 (Automatic corner override) G63 (Tapping mode) G64 (Cutting mode) G08P1 (High-accuracy control mode start) G08P0 (High-accuracy control mode end)
Designate the tolerance using one of the following methods. Designate the tolerance using the parameter "#2659 tolerance". When the setting is "0", the tolerance is han-
dled as "0.01 (mm)" for a linear axis, or "0.01 (deg)" for a rotary axis. Designate the numeric value following the ",K" address in the G61.4 command for a linear axis, and following
the ",R" address in the G61.4 command for a rotary axis. (a) The tolerance range is 0.000 to 100.000 (mm), or 0.000 to 100.000 (deg). If a value exceeding the range is
commanded, a program error (P35) will occur. (b) The tolerance designated by ",K" is applied to all the linear axes in the part system.
The tolerance designated by ",R" is applied to all the rotary axes in the part system. (c) When "0" is set to ",K" or ",R" or when ",K" or ",R" is omitted, the program runs using the setting value of the
parameter "#2659 tolerance" as the tolerance. (d) The tolerance designated by ",K" or ",R" is not held after reset. Therefore, if ",K" or ",R" is not designated in the
G61.4 command after reset, the setting value of the parameter "#2659 tolerance" is enabled. [Program example]
Command format
Spline interpolation 2 mode ON
G61.4 (,K__) (,R__);
,K Tolerance (mm) (For linear axis) ,R Tolerance (deg) (For rotary axis)
Detailed description
Tolerance specification method
: G91 ; G61.4 ,K0.02; Designate tolerance 0.02 (mm). G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ;
Tolerance: 0.02 (mm)
G61.4 ,K0; Designate the tolerance 0 [mm]. X-0.1 Z-0.05 ; X-0.1 Z-0.3 ;
Tolerance: Follows parameter "#2659 tolerance".
G64 ; :
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
742IB-1501278-P
Spline interpolation 2 interpolates a command point row of the machining program with a smooth curve. The follow- ing figures show the command points and paths.
During spline interpolation 2, the control generates a smooth curve within the specified tolerance (tolerable error) and moves the tool along the generated path. Illustrated below are the tolerances for a corner or curved shape.
The interpolated path varies depending on the tolerance as shown below.
Details of operation
Basic operations
Program command point Program command path
Interpolated path
[For corner] [For curve]
For corner For curve
Tolerance: High
Tolerance: Low
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
743 IB-1501278-P
Spline interpolation 2 can be used together with tool center point control (G43.4/G43.5). When all the conditions be- low are satisfied, spline interpolation 2 is performed using five axes. During G61.4 mode During tool center point control The G01 command in SSS control mode was issued. Spline interpolation 2, coupled with tool center point control, generates a smooth curve along the tool center point points within the tolerance (tolerable error) and moves the tool along the curve. The tool posture is also controlled smoothly within the specified rotary axis angle tolerance to generate a smooth curve.
The points to note when tool center point control is used together with spline interpolation 2 are as follows:
(1) The tool center point control specification is needed to enable the tool center point control. (2) Tool center point control is enabled only when "Joint interpolation method" is selected in "#7910 SLCT_INT_-
MODE" (Interpolation method selection). If "Single axis rotation interpolation method" is selected, the program error (P29) occurs.
(3) The rotary axis prefiltering function cannot be used together. (4) Any G code that is unavailable under tool center point control cannot be commanded.
[Program example]
Behavior under tool center point control
Tool end position Tool angle
Y axis Rotary axis 2
X axis Rotary axis 1
: G91 ; G43.4 H1; Tool center point control ON G61.4 ; Spline interpolation 2 mode ON G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ; X-0.1 Z-0.05 ; X-0.1 Z-0.3 ;
Spline interpolation 2 mode using 5 axes
G61.1 ; Spline interpolation 2 mode OFF G43.9; :
Tool center point control OFF
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
744IB-1501278-P
While spline interpolation 2 is enabled, it may be canceled temporarily depending on commands. If spline interpolation 2 is canceled temporarily, the axis moves to the commanded position. After this, when a tem- porary cancel cause is removed, spline interpolation 2 restarts.
The temporary cancel conditions are as follows.
(1) The group 1 modal is not G01, G02, or G03. (2) The block has a G code other than G90, G91, G01, G02, or G03 commanded. (3) The block has M (miscellaneous function command value), S (spindle command rotation speed), T (tool com-
mand value), or B (2nd miscellaneous function command value) designated. (4) Under single block operation (For details, refer to "Single Block Operation".) (5) Modal in which SSS control is disabled temporarily (Modal shown below)
Temporary cancel
NURBS interpolation Polar coordinate interpolation Cylindrical interpolation User macro interruption enable (M96) Feed per revolution (synchronous feed) Inverse time feed Constant surface speed control Fixed cycle 3-dimensional coordinate conversion Hypothetical axis interpolation Automatic tool length measurement Tool length compensation along the tool axis Normal line control Unidirectional positioning Exponential interpolation 3-dimensional circular interpolation
Path without temporary cancel
Block without movement by temporary cancel
Path without temporary cancel
Block with movement by temporary cancel
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
745 IB-1501278-P
Feed hold allows a deceleration stop in the middle of a curve. However, no interrupt operation can be performed. If the mode is switched to the manual mode or MDI mode during the feed hold, an operation error (M01 0180) will occur and the interrupt operation will be prohibited. After the program has been stopped by the feed hold, the movement on the curve can be restarted by the cycle start. The tool path specified just after the program has restarted is different from that specified when the program is not stopped by the feed hold, and the tool passes an area near the program-commanded shape.
During single block operation, spline interpolation 2 is canceled temporarily. In this period, linear interpolation is car- ried out at the commanded position. If single block is set to ON during continuous operation, the currently processed block stops on a curve, and the next and subsequent blocks stop on the commanded points.
Feed hold
Program commanded shape
NC commanded shape (Not stopped by the feed hold) NC commanded shape (Stopped by the feed hold)
Single block operation
(a) Sets the single block signal ON.
(b) Block stop on curve (e) Restarts spline interpolation 2.
(d) Sets the single block signal OFF.
(c) Block stop at commanded position
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
746IB-1501278-P
Spline interpolation 2 and smooth fairing can be used together. A spline interpolation 2 curve is generated along the points that are compensated by smooth fairing. If spline interpolation 2 is used together with tool center point control, smooth fairing is disabled.
Spline interpolation 2 and tool radius compensation can be combined. A spline curve is generated along the path for which the radius is compensated.
Spline interpolation 2 and high-speed high-accuracy control III can be combined. However, the fine segment pro- cessing capacity is limited. Spline interpolation 2 used in combination with tool center point control cannot be used together with high-speed high-accuracy control III.
Spline interpolation 2 (G61.4) and spline interpolation (G61.2/G05.1Q2) cannot be combined. The following differences are between spline interpolation 2 (G61.4) and spline interpolation (G61.2/G05.1Q2).
(*1) The axis passes through the commanded points at the start and end points.
The following shows differences between the spline interpolation 2 path and spline interpolation path.
Relationship with other functions
Smooth fairing
Compensation by smooth fairing Smooth fairing OFF
Smooth fairing ON
Tool radius compensation
High-speed high-accuracy control III
Spline interpolation
Feature of spline curve Parameter for adjusting the curve shape
Spline interpolation 2 (G61.4)
Passes near the commanded points. (*1)
#2659 tolerance
Spline interpolation (G61.2/G05.1Q2)
Passes on the commanded points. #8026 CANCEL ANG. #8027 Toler-1 #8028 Toler-2 #8029 FairingL #8030 MINUTE LENGS #8033 Fairing ON
Spline interpolation 2 Spline interpolation
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
747 IB-1501278-P
Inclined surface machining is available when tool center point control is used together with spline interpolation 2. Workpiece installation error compensation cannot be used together with spline interpolation 2 even when tool center point control is enabled. The points to note when tool center point control is used together with spline interpolation 2 are as follows:
(1) If G61.4 is given during inclined surface machining in any mode other than tool center point control mode, the operation is performed in the G61.1 mode. G61.4 mode is activated after tool center point control command is given.
(2) Any G code that is unavailable under inclined surface machining cannot be commanded. [Program example]
[Relationship between spline interpolation 2 and each function]
Inclined surface machining command and workpiece installation error compensation
: G68.2 X45. Y-50. I0. J32. K0. Inclined surface machining command ON G53.1 G43.4 H1; Tool center point control ON G61.4 ; Spline interpolation 2 mode ON G01 X0.Y0. F1000 ; Z0. X50. Y50. ; Y0. ; X0. ;
Spline interpolation 2 mode using 5 axes
G61.1 ; Spline interpolation 2 mode OFF G49; Tool center point control OFF G69 Inclined surface machining command OFF
G code Function name When the G codes shown on the left are commanded while spline
interpolation 2 is enabled
When spline interpolation 2 is en- abled while the functions shown
on the left are enabled
G43.4 G43.5
Tool center point control Operation is performed in spline in- terpolation 2 mode using five axes.
Operation is performed in spline in- terpolation 2 mode using five axes.
G68.2 G68.3
Inclined surface machin- ing command
Under tool center point control, the program error (P952) oc- curs. While tool center point control is
disabled, the operation with G61.1 commanded is carried out.
While tool center point control is enabled, spline interpolation 2 operation using five axes is car- ried out. While tool center point control is
disabled, the operation with G61.1 commanded is carried out.
G54.4 P1 to P7
Workpiece installation error compensation
Program error (P546) Program error (P546)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
748IB-1501278-P
(1) The graphic check drawing is not carried out during spline interpolation 2 (the period from G61.4 to the cancel command).
(2) PLC interrupt is not available during spline interpolation 2. If an PLC interrupt is performed during spline interpo- lation 2, the operation error (M01 0180) will occur.
(3) When the arrangement at the commanded point of the adjacent path of the machining program generated from CAM is different extremely, the tool center path generated by spline interpolation may not be aligned with the adjacent path. In this case, reduce the setting value of the parameter "#2659 tolerance" (tolerance amount) or the commanded value of the ",K" address. You can move the tool center path closer to the machining program path. However, the cycle time becomes longer.
(*1) The commanded point is not arranged.
(*2) The arrangement interval between the commanded points is different extremely.
Precautions
(a) When the tolerance amount is large (b) When the tolerance amount is small
There is a position at which the commanded point is not arranged in the adjacent path.
The block segment length of the ad- jacent path is different extremely.
Program command point Program path Tool center path
(*1) (*1)
(*2) (*2)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
749 IB-1501278-P
17.6 High-accuracy Spline Interpolation ; G61.2
This function automatically generates a spline curve that passes through a sequence of points commanded by the fine segment machining program, and interpolates the path along this curve. This enables high-speed and high-ac- curacy machining to be achieved. This function has two functions; fairing function to delete unnecessary fine blocks, and spline interpolation function to connect smoothly a sequence of points commanded by the program. The high-accuracy control function G61.1 is also valid. The high-accuracy spline Interpolation is valid only for the first part system. G61.2 cannot be commanded in the 2nd part system even when the multi-part system simultaneous high-accuracy specifications are available. There are two types of spline interpolation command format: G61.2 and G05.1Q2. Both formats can be used regard- less of the parameter "#1267 ext03/bit0" setting if the spline interpolation specifications are available to the machine. This section describes the G61.2 command. For information about differences between G05.1Q2 and G61.2 or fea- tures of spline interpolation, refer to "17.4 Spline Interpolation ; G05.1 Q2/Q0".
The "G61.2" high-accuracy spline interpolation mode is canceled when any of the functions of G code group 13 is commanded.
(1) Fairing Refer to "17.3.2 Fairing".
(2) Spline interpolation Refer to "Detailed description" of "17.4 Spline Interpolation ; G05.1 Q2/Q0".
Function and purpose
Command format
Spline mode ON
G61.2 X__ Y__ Z__ F__ ; or G61.2 ;
X X axis end point coordinate Y Y axis end point coordinate Z Z axis end point coordinate F Feedrate
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
750IB-1501278-P
(1) The spline interpolation is available when the following conditions are all satisfied. If the following conditions are not satisfied, the spline function will be canceled once, and the judgment whether to carry out new spline from the next block will be made. It is the movement only of three axes set to the basic axes I, J and K. When the block length is smaller than the value of the machining parameter "#8030 MINUTE LENGS". When the movement amount is not 0. The group 1 command is G01 (linear interpolation). Operation in fixed cycle modal It is not during hypothetical axis interpolation mode. It is not during 3-dimensional coordinate conversion modal. It is not in a single block mode.
(2) The spline function is a modal command of group 13. This function is valid from G61.2 command block. (3) The spline function is canceled by group 13 commands (G61 to G64). (4) The spline function is canceled by NC reset 2, reset & rewind, NC reset 1 (the setting which does not hold modal
when NC is reset) or power ON/OFF.
(1) If this function are not provided and G61.2 is commanded, the program error (P39) will occur. (2) Even if "-1" is set for parameter "#8030 MINUTE LENGS", the spline function will be temporarily canceled by the
cancel conditions (cancel angle, non-movement block, excessive chord error, etc.) other than the block length. (3) Graphic check will draw the shape of when the spline interpolation OFF. (4) A program error (P34) will occur if the number of axis in the part system does not exceed 3.
Program example
: G91 ; G61.2 ; Spline interpolation mode ON G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ; X-0.1 Z-0.05; X-0.1 Z-0.3; G64 ; Spline interpolation mode OFF :
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
751 IB-1501278-P
17.7 Machining Condition Selection I ; G120.1, G121
After initializing the machining condition parameter groups with the machining condition selection I function, the ma- chining condition parameter groups can be switched by G code command. Switching is also possible on the "Machining cond" (selecting) screen. In that case, however, the machining condi- tions selected on the screen are applied to all part systems.
(1) G120.1 and G121 commands are unmodal commands of G code group 0. (2) Switching of the machining condition parameter group using the G120.1 or G121 command is only applied to the
commanded part system. (3) G120.1 must be commanded alone in a block, which also applies to G121. If it is not commanded alone in a
block, a program error (P33) will occur. (4) Address P in G120.1 command cannot be omitted. If omitted, a program error (P33) will occur. (5) Address Q in G120.1 command can be omitted. If omitted, it will be handled as "Q1 (condition 1)" is commanded. (6) When address P and Q in G120.1 command is commanded with a decimal point, the digit after the decimal point
is ignored. (7) If other than "0 to 3" is set to address P in G120.1 command or other than "1 to 3" is set to address Q, a program
error (P35) will occur. (8) When address P is set to "0" and address Q is omitted or set between "1" and "3" in G120.1 command, it will be
switched to the reference parameter. (9) It will be switched to the machining condition parameter group selected in "Machining cond" (selecting) screen
by the G121 command.
Function and purpose
Command format
Machining condition selection I
G120.1 P_ Q_ ;
P Machining purpose 0: Reference parameter 1: Usage 1 2: Usage 2 3: Usage 3
Q Condition 1: Condition 1 2: Condition 2 3: Condition 3
When omitted, Q1 will be applied
Machining condition selection I cancel
G121;
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
752IB-1501278-P
(10) When the emergency stop and reset (reset 1, reset 2, and reset & rewind) are performed while running the ma- chining program whose machining condition parameter group is switched by G120.1 command, it will be switched to the selected condition parameter group machining in "Machining cond" (selecting) screen.
(11) Because the parameters are switched after being decelerated by G120.1 and G121 commands, the workpiece may be damaged. Make sure to keep the tool away from the workpiece when commanding G120.1 and G121.
(12) When the machining condition parameter group is switched by G120.1 command more than once, the param- eter group commanded last becomes valid.
(13) It is switched to the selected machining condition parameter group in the "Machining cond" (selecting) screen by program end (M02 and M30).
(14) If G120.1 and G121 are commanded without initializing the machining condition parameter group, a program error (P128) will occur.
"Machining cond" (setting) screen
The displayed machining condition parameter group is switched depending on whether tolerance control is enabled or disabled (parameter "#12066 Tolerance ctrl ON").
Program example
High-accuracy setting
(for finishing machining)
Standard setting (for medium
finishing machining)
High-speed setting
(for rough cutting machining)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
753 IB-1501278-P
(1) When "Application1" and "Condition1" from the machining condition parameter group are selected in "Machining cond" (selecting) screen before running the program.
N1 G91 G28 Z0; Machining condition parameters Operate with (machining usage 1/ condition 1)
N2 G28 X0 Y0; N3 G90 G54 G00 X2. Y2.; N4 G43 H1 Z50.; N5 G90 G01 Z-5. F3000; N6 M3 S10000; N7 F2000; N8 G05 P10000; N9 G01 X2.099 Y1.99; N10 X2.199 Y1.990; : N1499 G05 P0; N1500 G91 G28 Z0; N1501 G28 X0 Y0; N1502 M5; N1503 G120.1 P1 Q3; ... The machining condition parame-
ter groups are switched. N1504 G90 G54 G00 X2. Y2.; Machining condition parameters
Operate with (machining usage 1/ condition 3)
N1505 G43 H1 Z50.; N1506 G90 G01 Z-8. F3000; N1507 M3 S10000; N1508 F1200; N1509 G05 P10000; N1510 G01 X2.099 Y1.997; N1511 X2.199 Y1.990; : N2999 G05 P0; N3000 G91 G28 Z0; N3001 G28 X0 Y0; N3002 M5; N3003 M30; ... Return to the selected machining
condition parameter group in "Ma- chining cond" (selecting) screen at the program end.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
17 High-speed High-accuracy Control
754IB-1501278-P
(1) G code modal that cause a program error when commanding G120.1 and G121 are listed below.
(1) Because the parameters are switched after being decelerated once G120.1 or G121 is commanded, the work- piece may be damaged. Make sure to keep the tool away from the workpiece when commanding G120.1 and G121.
(2) It is switched to the reference parameter by turning the power ON again. (3) When G120.1 and G121 are commanded, parameters are switched when smoothing for NC axes in all part sys-
tems become "0". (4) The machining condition parameter group neither set the parameter setting from the program by G10 command
nor read the parameters by system variables (from #100000). (5) If the machining condition parameters are switched, the setting values of the parameters "#2010 fwd_g" and
"#2659 tolerance" are identical for all the NC axes in the switched part system. (6) The machining condition parameters are not switched for the operation search. The machining condition param-
eters are switched for the restart search. (7) When the following conditions are satisfied simultaneously, the variable-acceleration pre-interpolation accelera-
tion/deceleration is disabled automatically. The operation error (M01 0136) is not displayed. Variable-acceleration pre-interpolation acceleration/deceleration is ON. SSS control has been switched from ON to OFF by machining condition selection I.
Relationship with other functions
G code Function Program error when G120.1 and G121 are commanded
G02.3, G03.3 Exponential interpolation P128 G06.2 NURBS interpolation P32 G07.1 Cylindrical interpolation P128 G12.1 Polar coordinate interpolation P128 G10 Parameter input by program P421
Tool compensation input by pro- gram
G33 Thread cutting P128 G38 Tool radius compensation (vector
designation) P128
G39 Tool radius compensation (corner arc)
P128
G41, G42 Tool radius compensation P128 3-dimensional tool radius compen- sation
G41.1/G151 Normal line control Left P128 G42.1/G152 Normal line control Right P128 G43 Tool length compensation (+) P128 G44 Tool length compensation (-) P128 G43.1 Tool length compensation along
the tool axis P128
G43.4, G43.5 Tool center point control P942 G66, G66.1 User macro (modal call A, B) P128 G68.2, G68.3 Inclined surface machining P951 G73/G74/G76/G81/G82/G83/ G84/G85/G86/G87/G88/G89
Fixed cycle P33 (When G120.1 command is is- sued) P128 (When G121 command is is- sued)
Precautions
18
755 IB-1501278-P
Advanced Multi-Spindle Control Function
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
756IB-1501278-P
18Advanced Multi-Spindle Control Function 18.1 Spindle Synchronization
In a machine having two or more spindles, this function controls the rotation speed and phase of one spindle (refer- ence spindle) in synchronization with the rotation of the other spindle (synchronized spindle). This function provides, for example, an effect that re-grasps the workpiece grasped by the 1st spindle to the 2nd spindle while maintaining the rotation speed of the 1st spindle to reduce the cycle time by the 1st spindle decelera- tion time and the 2nd spindle acceleration time in the next process during re-grasping. Furthermore, this function carries out turning or phase control while grasping both edges of a longer workpiece using the 1st and 2nd spindles, preventing a twist or bow from occurring in the workpiece under machining and enabling the machining accuracy. The spindle synchronous multi-step acceleration/deceleration of the reference spindle is applied to the acceleration/ deceleration of the spindle-synchronization relation spindle under spindle synchronization. (Only for C80 series) The following control methods are available. Which mode is valid depends on the MTB specifications (parameter "#1300 ext36/bit7"). This section describes spindle synchronization control I that is executed with G commands.
Spindle synchronization I The designation of the synchronized spindle and start/stop of the synchronization are executed by commanding G codes in the machining program.
Spindle synchronization II The selections of the synchronized spindle and synchronization start, etc., are controlled from PLC based on the MTB specifications. Refer to the instruction manual issued by the MTB for details.
Function and purpose
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
757 IB-1501278-P
18.1.1 Spindle Synchronization I; G114.1
With the spindle synchronization I, the designation of the spindle and start/stop of the synchronization are executed by commanding G codes in the machining program.
This function cannot be combined with the following spindle synchronization functions while it is active. An operation error (M01 1005) occurs. Spindle synchronization I Spindle synchronization II Tool spindle synchronization IA Tool spindle synchronization IB (IC) Tool spindle synchronization II
(*1) This command changes the phase shift amount of the synchronized spindle of two spindles which have already synchronized by spindle synchronization command.
The spindle synchronization ON (G114.1) command designates the reference spindle and synchronized spindle, and synchronizes the two designated spindles. By commanding the phase shift amount of synchronized spindle, the phases of the reference spindle and synchronized spindle can be aligned.
Function and purpose
Command format
Spindle synchronization command
G114.1 H__ D__ R__ A__ ; Spindle synchronization start command
G114.1 D__ R__ ; Phase shift amount change during spindle synchronization (*1) [C80]
H Reference spindle specification D Synchronized spindle specification R Phase shift amount of synchronized spindle A Spindle synchronization acceleration/deceleration time constant
Address Meaning Command range (unit)
Remarks
H Reference spindle speci- fication Select the number or name of the spindle to be used as the reference spindle from the two spin- dles to be synchronized. (*1)
For spindle number: 1 to n (n: Maximum number of available spindles) For spindle name: 1 to 9
If a value exceeding the command range or spin- dle No. without specifications is commanded, a program error (P35) will occur. If there is no command, a program error (P33)
will occur. If an analog-connected spindle is commanded, a
program error (P700) will occur. (*2)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
758IB-1501278-P
(*1) There are two spindle command methods: spindle number method and spindle name method. Command with the spindle names, only when all spindles are set with the spindle name parameter (#3077 Sname) (from 1 to 9). For others, command with the spindle number. These settings depend on the MTB spec- ifications.
(*2) The available spindle type and connection method depend on the specifications of your machine tool.
D Synchronized spindle specification Select the number or name of the spindle to be synchronized with the ref- erence spindle from the two spindles to be syn- chronized. (*1)
For spindle number: 1 to n or -1 to -n (n: Maximum number of available spindles) For spindle name: 1 to 9 or -1 to -9
If a value exceeding the command range is com- manded, a program error (P35) occurs. If there is no command, a program error (P33)
will occur. If the same spindle as that commanded for the
reference spindle selection is designated, a pro- gram error (P33) will occur. The rotation direction of the synchronized spindle
in respect to the reference spindle is command- ed with the D sign. If an analog-connected spindle is commanded, a
program error (P700) will occur. (*2) R Phase shift amount of
synchronized spindle Set the shift amount from the synchronized spin- dle's reference position ("one rotation" signal).
0 to 359.999 () or 0 to 359999 (* 10-3)
If a value exceeding the command range is com- manded, a program error (P35) occurs. The commanded shift amount will be effective in
the clockwise direction of the reference spindle. Minimum resolution of commanded shift amount
Semi-close case (Gear ratio: 1:1 only) 360/4096 []
Full-close case (360/4096) * K [] (K: Gear ratio of spindle and encoder)
If there is no R command, phase alignment will not be carried out.
A Spindle synchronization acceleration/decelera- tion time constant Command the accelera- tion/deceleration time constant for when the spindle synchronization command rotation speed changes. (Command this to accel- erate or decelerate at a speed slower than the time constant set in the parameters.)
0.001 to 9.999 (s) or 1 to 9999 (ms)
If a value exceeding the command range is com- manded, a program error (P35) occurs. If the commanded value is smaller than the ac-
celeration/deceleration time constant set with the parameters, the value set in the parameters will be applied.
Address Meaning Command range (unit)
Remarks
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
759 IB-1501278-P
(1) An axis that involves any travel cannot be put in the same block as the Spindle synchronization cancel command. Doing so causes the program error (P33) when the cancel command is issued, which causes automatic opera- tion to pause.
Spindle synchronization cancel (G113.1) cancels the synchronous state of the two spindles rotating in synchroniza- tion with the spindle synchronization command.
(1) The rotation speed and rotation direction of the reference spindle and synchronized spindle during spindle syn- chronization are the rotation speed and rotation direction commanded for the reference spindle. Note that the rotation direction of the synchronized spindle can be reversed from the reference spindle through the program.
(2) The reference spindle's rotation speed and rotation direction can be changed during spindle synchronization. (3) If spindle stop is commanded for the synchronized spindle during spindle synchronization, the synchronized spin-
dle rotation will stop. (4) The rotation speed command (S command) and constant surface speed control are invalid for the synchronized
spindle during spindle synchronization. Note that the modal is updated, so these will be validated when the spin- dle synchronization is canceled.
(5) The constant surface speed can be controlled by issuing a command to the reference spindle even during spindle synchronization.
Canceling spindle synchronization
G113.1;
Detailed description
Rotation speed and rotation direction
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
760IB-1501278-P
(1) When rotation synchronization control (command with no R address) is commanded with the G114.1 command, the synchronized spindle rotating at an arbitrary rotation speed will accelerate or decelerate to the rotation speed commanded beforehand for the reference spindle, and will enter the rotation synchronization state.
(2) If the reference spindle's commanded rotation speed is changed during the rotation synchronization state, ac- celeration/deceleration will be carried out while maintaining the synchronization state following the spindle ac- celeration/deceleration time constants set in the parameters, and the commanded rotation speed will be achieved.
(3) In the rotation synchronization state, the reference spindle can be controlled at a constant surface speed even when two spindles are grasping one workpiece.
(4) The following type of operation will take place.
Rotation synchronization
M23 S2=750 ; Forward rotate the 2nd spindle (synchronized spindle) at 750 r/min (speed command). (a)
: M03 S1=1000 ; Forward rotate the 1st spindle (reference spindle) at 1000 r/min (speed command). (b) : G114.1 H1 D-2 ; Synchronize the 2nd spindle (synchronized spindle) with the 1st spindle (reference spin-
dle) by reverse run. (c) : S1=500 ; Change the rotation speed of the 1st spindle (reference spindle) to 500 r/min. (d) : G113.1; Cancel the spindle synchronization. (e)
Rotation speed (r/min) Forward rotation
Reference spindle
Synchronized spindle
Time
Reverse rotation
1000
750
500
0
- 500
- 750
- 1000
(a) (b) (c) (d) (e)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
761 IB-1501278-P
(1) When phase synchronization (command with R address) is commanded with the G114.1 command, the synchro- nized spindle rotating at an arbitrary rotation speed will accelerate or decelerate to the rotation speed command- ed beforehand for the reference spindle, and will enter the rotation synchronization state. Then, the phase is aligned so that the rotation phase commanded with the R address is reached, and the phase synchronization state is entered.
(2) If the reference spindle's commanded rotation speed is changed during the phase synchronization state, accel- eration/deceleration will be carried out while maintaining the synchronization state following the spindle acceler- ation/deceleration time constants set in the parameters, and the commanded rotation speed will be achieved.
(3) In the phase synchronization state, the reference spindle can be controlled at the constant surface speed even when two spindles are grasping one workpiece.
(4) The following type of operation will take place.
(*1) Phase synchronization is performed with the step alignment method (without acceleration/deceleration) when "#3130 syn_spec/bit1" = "0", and with the multi-step acceleration/deceleration method (described lat- er) when "#3130 syn_spec/bit1" = "1".
Phase synchronization
M23 S2=750 ; Forward rotate the 2nd spindle (synchronized spindle) at 750 r/min (speed command). (a) : M03 S1=1000 ; Forward rotate the 1st spindle (reference spindle) at 1000 r/min (speed command). (b) : G114.1 H1 D-2 R0; Synchronize the 2nd spindle (synchronized spindle) with the 1st spindle (reference spin-
dle) by reverse run. (c) Shift the phase of synchronized spindle by the value commanded with "R". (d)
: S1=500 ; Change the rotation speed of the 1st spindle (reference spindle) to 500 r/min. (e) : G113.1; Cancel the spindle synchronization. (f)
Rotation speed (r/min) Forward rotation
Reference spindle
Synchronized spindle
Time
Reverse rotation
1000
750
500
- 500
- 750
- 1000 (d) (*1)
(a)
0
(b) (c) (e) (f)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
762IB-1501278-P
(1) When the "phase shift amount change during spindle synchronization" command (G114.1 D_ R_) is issued to change the phase shift amount of the spindle, for which the rotation or phase has already synchronized by the G114.1 command, the phase is aligned so that the rotation phase commanded with the R address is reached, and the phase synchronization state is entered. The following type of operation will take place.
(*1) Phase synchronization is performed with the step alignment method when "#3130 syn_spec/bit1" = "0", and with the multi-step acceleration/deceleration method (described later) when "#3130 syn_spec/bit1" = "1".
Operation when the "phase shift amount change during spindle synchronization" command is issued [C80]
N01 M23 S2=750; Forward rotate the 2nd spindle (synchronized spindle) at 750 r/min (speed command). (a)
: N10 M03 S1=1000; Forward rotate the 1st spindle (reference spindle) at 1000 r/min (speed com-
mand). (b) : N20 G114.1 H1 D-2 Rxx; Synchronize the 2nd spindle (synchronized spindle) with the 1st spindle (refer-
ence spindle) by reverse run. (c) : Shift the phase of synchronized spindle by the value commanded with "R". (d) N25 Mzz; Wait until phase synchronization is completed. : (An M code is used to check the completion of spindle phase synchronization) N30 G114.1 D2 Ryy; Shift the phase of the 2nd spindle (synchronized spindle) by the value com-
manded with "R". (e) : N40 S1=500; Change the rotation speed of the 1st spindle (reference spindle) to 500 r/min.
(f) : N50 G113.1; Cancel the spindle synchronization. (g)
Rotation speed (r/min) Forward rotation
Reference spindle
Synchronized spindle
Time
Reverse rotation
1000
750
500
- 500
- 750
- 1000 (d) (*1)
(a)
0
(b) (c) (f) (g)
(e) (*1)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
763 IB-1501278-P
(2) The operation to be performed when the "phase shift amount change during spindle synchronization" command (G114.1 D_ R_) is issued varies depending on conditions, for example, whether spindle synchronization has started.
(*1) Spindle synchronization start command
(*2) Command to change the phase shift amount during spindle synchronization
The spindle phase shift amount calculation function obtains and saves the phase difference of the reference spindle and synchronized spindle by turning the "PLC" signal ON when the phase synchronization command is executed. When the phase is positioned to the automatically saved phase difference before executing the phase synchroniza- tion control command, phases can be aligned easier when re-grasping profile materials.
[Saving the phase difference between reference spindle and synchronized spindle]
(1) Set a profile material in the reference spindle. (2) Set the profile material in the synchronized spindle. (3) Turn the "phase shift calculation request" signal (SSPHM) ON. (4) Input a rotation command, with 0 speed, for the reference spindle and synchronized spindle.
nal. (8) Stop both spindles. (9) Turn the "phase shift calculation request" signal OFF.
Phase shift amount (When "start" command (*1) is issued)
State in which the spindle synchroniza- tion "start" command is not executed.
"R" is omitted. (G114.1 H_ D_)
"R" is specified. (G114.1 H_ D_ R_)
Phase shift amount (When "change"
command (*2) is is- sued)
"R" is omitted. Unchanged as spec- ified when the start command (*1) is is- sued.
The phase remains unchanged with the shift amount speci- fied when the start command (*1) is is- sued.
(Program error (P33)) (G114.1 D_)
"R" is specified. The phase shift is carried out in accor- dance with the change command (*2).(G114.1 D_ R_)
Spindle synchronization phase shift amount calculation function
Reference spindle Synchronized spindle : Saved phase difference
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
764IB-1501278-P
[Automatic phase alignment of reference spindle and synchronized spindle]
(1) Turn the "phase offset request" signal ON. (2) Issue the phase synchronization command (with R command).
the spindle synchronization phase shift calculation function. The state in which the phase shift amount of syn- chronized spindle, designation R value, is "0", is the same as the reference state (state obtained with "phase shift calculation request" signal).
Reference spindle Synchronized spindle (a) Phase difference (b) Phase alignment
M6; M15; G113; M3 S1=0 M24 S2=0;
G114.1 H1 D-2;
S1=3000; M77; S1=0; G04X_; G113;
Phase shift calculation request signal (SSPHM, PLC CNC)
Reference spindle chuck close M code
Synchronized spindle chuck close M code
Example of operation macro Automatic operation start (ST, PLC CNC)
Spindle rotation speed synchronization complete signal (FSPRV, CNC PLC)
Saving the phase difference between reference spindle and synchronized
spindle is completed
NC reset
Spindle synchronization complete check M code
Reference spindle forward run command (M3) Reference spindle reverse run command (M24)
(b) (a)
G114.1 H1 D-2 R_; M77; Phase offset request signal (SSPHF, PLC CNC)
Spindle phase synchronization complete signal (FSPRH, CNC PLC)
Spindle synchronization complete check M code
Phase alignment between reference spindle and synchronized spindle is
completed
Machining program example
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
765 IB-1501278-P
Acceleration/deceleration time constants for up to eight steps can be selected according to the spindle rotation speed for the acceleration/deceleration during spindle synchronization. The acceleration/deceleration in each step is as follows.
Time required from minimum rotation speed to maximum rotation speed in each step = [Time constant without multi-step acceleration/deceleration] * [magnification of time constant in each step] * [Rate of rotation speed width in each step respect to rotation speed width up to limit rotation speed]
(1) When the "A" address is designated at G114.1 command, the time is obtained with the "A" address instead of "spt" in the formula below.
Time required for spindle to rotate with the rotation speed set in "sptc 1" from stopped state (a) = spt * sptc1 / slimit Time required for spindle to reach the rotation speed set in "sptc2" from the speed of "sptc1" (b) = spt * spdiv1 * (sptc2 - sptc1) / slimit Time required for spindle to reach the rotation speed set in "sptc3" from the speed of "sptc2" (c) = spt * spdiv2 * (sptc3 - sptc2) / slimit Time required for spindle to reach the rotation speed set in "sptc4" from the speed of "sptc3" (d) = spt * spdiv3 * (sptc4 - sptc3) / slimit Time required for spindle to reach the rotation speed set in "sptc5" from the speed of "sptc4" (e) = spt * spdiv4 * (sptc5 - sptc4) / slimit Time required for spindle to reach the rotation speed set in "sptc6" from the speed of "sptc5" (f) = spt * spdiv5 * (sptc6 - sptc5) / slimit Time required for spindle to reach the rotation speed set in "sptc7" from the speed of "sptc6" (g) = spt * spdiv6 * (sptc7 - sptc6) / slimit Time required for spindle to reach the rotation speed set in "slimit" from the speed of "sptc7" (h) = spt * spdiv7 * (slimit - sptc7) / slimit
To decrease the number of acceleration/deceleration steps during spindle synchronization, set one of the following for the unnecessary step. Magnification for time constant changeover speed (spdiv7 to spdiv1) = 0 (or 1) Spindle synchronous multi-step acceleration/deceleration changeover speed (sptc7 to sptc1) = Limit rotation
speed (slimit) or higher
Multi-step acceleration/deceleration
Rotation speed (r/min)
Time (ms)
Note
slimit
sptc7
sptc6
sptc5
sptc4
sptc3
sptc2
sptc1
(a) (b) (c) (d) (e) (f) (g) (h) spt
0
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
766IB-1501278-P
The spindle orientation is carried out with the spindle orientation command for the reference spindle while the spindle synchronization status remains kept. The spindle orientation command is ignored for the synchronized spindle. The multi-step orientation command or indexing command is also enabled.
The "spindle orientation command" signal (ORC) for the reference spindle in the C axis mode is ignored during spindle synchronization. However, if the spindle position control command (C axis mode switch command) is issued during spindle orientation, the mode is switched to the C axis mode.
The "spindle orientation" signal operation depends on the MTB specifications. Refer to the instruction manual issued by the MTB for details.
Gear switching is enabled while the reference spindle is in the spindle mode. Gear switching is disabled while the reference spindle is in the C axis mode or in process of spindle orientation.
Switching to the C axis mode or the spindle orientation cannot be carried out during gear switching. After gear switching has been completed, the mode is switched to the C axis mode.
The reference position return operation at C axis mode switch command for the reference spindle and the spin- dle override in the C axis mode are invalid.
The cutting feed override or rapid traverse override of the NC axes is valid in the C axis mode. The spindle override is invalid while the reference spindle is in process of spindle orientation or spindle indexing.
The maximum clamp rotation speed specified with the address S following G92 is valid for the reference or syn- chronized spindle.
The minimum clamp rotation speed specified with the address Q following G92 is valid for the reference spindle, but invalid for the synchronized spindle. If the rotating spindle is set to the synchronized spindle at the minimum clamp rotation speed, the minimum rotation speed clamp is canceled, and the spindle rotates at the command- ed rotation speed. If the spindle synchronization control state is canceled, the minimum clamp rotation speed is enabled.
The synchronous tap spindle cannot be commanded as the reference spindle or synchronized spindle of the spindle synchronization I. If such a command is issued, an operation error (M01 1007) occurs, causing the automatic operation to be paused.
You cannot command a synchronous tapping that uses the reference spindle or synchronized spindle of spindle synchronization I. If such a command is issued, an operation error (M01 1139) occurs, causing the automatic operation to be paused.
The spindle-mode rotary axis cannot be commanded for the reference spindle or synchronized spindle of spindle synchronization I/II, tool spindle synchronization IA (spindle-spindle, polygon), or tool spindle synchronization IB (spindle-spindle, polygon). If such a command is issued, an operation error (M01 1024) occurs, causing the auto- matic operation to be paused.
Relationship with other functions
"Spindle orientation" signal (ORC)
Switching the spindle gear
Spindle override
Spindle clamp speed setting
Synchronous tapping cycle
Spindle-mode rotary axis control
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
767 IB-1501278-P
(1) The spindle rotating with spindle synchronization control will stop when emergency stop is applied. (2) The rotation speed clamp during spindle synchronization will follow the smaller clamp value set for the reference
spindle or synchronized spindle. (3) Orientation of the reference spindle and synchronized spindle is not possible during the spindle synchronization
mode. To carry out orientation, cancel the spindle synchronization mode first. (4) The rotation speed command (S command) is invalid for the synchronized spindle during the spindle synchroni-
zation mode. However, the modal will be updated, therefore this command will be validated when spindle syn- chronization is canceled.
(5) The constant surface speed control is invalid for the synchronized spindle during the spindle synchronization mode. However, the modal will be updated, therefore this command will be validated when spindle synchroniza- tion is canceled.
(6) The rotation speed command (S command) and constant surface speed control for the synchronized spindle will be validated when spindle synchronization is canceled. Thus, the synchronized spindle may carry out different operations when this control is canceled.
(7) If the phase difference is not obtained with the "phase shift calculation request" signal and the phase synchroni- zation command is executed by turning the "phase offset request" signal ON, the phase shift amount will not be calculated correctly.
(8) The spindle Z phase encoder position parameter "#3035 sppst" is invalid when using the spindle synchronization phase shift amount calculation function. (It is ignored.) The spindle Z phase encoder position parameter "#3035 sppst" is valid when the "phase offset request" signal is OFF.
(9) If the phase synchronization command (command with R address) is issued while the "phase shift calculation request" signal is ON, an operation error (1106) occurs.
(10) If the "phase shift calculation request" signal is ON and the reference spindle or synchronized spindle is rotation while rotation synchronization is commanded, an operation error (1106) occurs.
(11) If the phase synchronization command R0 (
(12) If a value other than the phase synchronization command R0 (
(13) The "phase offset request" signal will be ignored when the "phase shift calculation request" signal is ON. (14) The phase difference of the reference spindle and synchronized spindle saved in the NC is valid only when the
"phase shift calculation" signal is ON and for the combination of the reference spindle selection (H_) and syn- chronized spindle selection (D_) commanded with the rotation synchronization command (no R address). For example, if the phase difference between reference spindle and synchronized spindle is saved as "G114.1 H1 D-2 ;", the saved phase difference will be valid only when the "phase offset request" signal is ON and "G114.1 H1 D-2 R*** ;" is commanded. If "G114.1 H2 D-1 R*** ;" is commanded in this case, the phase shift amount will not be calculated correctly.
(15) The phase difference between reference spindle and synchronized spindle saved in the NC is held until the next spindle synchronous phase shift calculation (rotation synchronization command is completed with the "phase shift calculation request" signal ON).
(16) When the spindle synchronization commands are being issued with the PLC I/F method (#1300 ext36/bit7 OFF), a program error (P610) occurs if the spindle synchronization is commanded with G114/G113.1.
(17) When the spindle-mode servo is used for the reference spindle or the synchronized spindle, the spindle param- eter "#13003 SP003" (PGS) and spindle-mode servo parameter "#52203 SV003" (PGN) must be set to the same value between the reference and synchronized spindles. (These settings depend on the MTB specifications.)
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
768IB-1501278-P
(1) To enter the rotation synchronization mode while the reference spindle and synchronized spindle are chucking the same workpiece, turn the reference spindle and synchronized spindle rotation commands ON before turning the spindle synchronization mode ON.
(2) To chuck the same workpiece with the reference spindle and synchronized spindle in the phase synchronization mode, align the phases before chucking.
(3) (Only for M8 series) When the spindle synchronization control is commanded and if the "start" signal of the syn- chronized spindle is not input, turn the servo ON for the synchronized spindle and accelerate or decelerate the spindle rotation up to the commanded speed of the reference spindle. Whether the linear acceleration/deceler- ation or multi-step acceleration/deceleration is used as the acceleration/deceleration depends on the MTB spec- ifications (parameter "#1255 set27/bit6"). However, when the synchronized spindle is the spindle-mode servo, multi-step acceleration/deceleration is ap- plied regardless of the parameter setting.
Cautions on programming
CAUTION
Do not make the synchronized spindle rotation command OFF with one workpiece chucked by the reference
spindle and synchronized spindle during the spindle synchronization mode. Failure to observe this may cause
the synchronized spindle stop, and hazardous situation.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
769 IB-1501278-P
18.1.2 Spindle Position Control (Spindle/C Axis Control) under Spindle Synchronization Control
This function enables the spindle position control (spindle/C axis control) by the reference spindle in spindle syn- chronization control mode. The reference spindle can be controlled as the rotary axis while the spindle synchronization status remains kept, and also positioning or interpolation with another NC axis is enabled by issuing the position command (movement command) in the same way as for the NC axis. There are two methods: PLC signal method and program command method to switch the spindle and rotary axis during spindle synchronization control. The method that is applied for switching depends on the MTB specifications (parameter "#3129 cax_spec/bit0"). This section describes the program command method. In this manual, the state to control an axis as a spindle is referred to as "spindle mode", and the state to control an axis as a rotary axis as "C axis mode". For details about the spindle position control (spindle/C axis control) function, refer to "10.4 Spindle Position Control (Spindle/C Axis Control)". This section also describes considerations to perform the spindle position control (spindle/C axis control) under spin- dle synchronization, and the status of various PLC signals and restrictions. The status, control method, and opera- tion of the PLC signal depend on the MTB specifications.
Function and purpose
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
770IB-1501278-P
The machining program switches the reference spindle to the C axis mode with G00 command, and to the spindle mode with S command. The C axis servo OFF signal (*SVFn) must be kept ON while the program command method is selected. When the program command method is selected, switching operation is performed only with the reference position return type. The following shows the C axis switching sequence under spindle synchronization.
the spindle mode, the spindle is directly located at the position commanded by the reference spindle while the synchronous status remains kept.
(2) Only the G00 command is valid to switch the mode. If the C axis movement is commanded with the G code other than G00, it causes a program error (P430).
(3) The spindle position control (spindle/C axis control) axis must be commanded with the absolute position ad- dress or absolute command (G90). If the incremental position address or incremental command (G91) is used, it causes a program error (P32).
(4) In the switching specifications, only the reference position return type (equivalent to "#3106 zrn_typ/bit8" = 0) is valid, and the direction to return from the rotation mode to the reference position follows the rotation direction (equivalent to "#3106 zrn_typ/bitB" = 1). The direction to return from the spindle stop state to the reference position ("#3106 zrn_typ/bitA-bit9") and interpolation mode selection ("#3106 zrn_typ/bitD-bitE ") follow the appropriate parameters.
[C axis mode switching conditions] (1) The C axis servo OFF signal (*SVFn) of the reference spindle is set to ON when switching is commanded. (2) The spindle rotation speed synchronization completion signal (FSPRV) is set ON for rotation synchronization,
and the spindle phase synchronization completion signal (FSPPH) is set ON for phase synchronization.
(SRI) ON and the S command. (2) The switching is performed with the startup of the spindle forward run signal (SRN) or the spindle reverse run
signal (SRI). [Spindle mode switching condition]
(1) The C axis servo OFF signal (*SVFn) of the reference spindle is set to ON and the C axis selection signal (CMD) is set to OFF when switching is commanded.
Detailed description
Program command method
G114.1 H1 D2 G00 C0 S1000 M3G00 C90.
NC->PLC
NC->PLC
PLC->NC
PLC->NC
Spindle mode Spindle mode
In spindle synchronization
C axis mode
(Parameter) Spindle/C axis reference position
return speed
FSPRV Spindle rotation speed
synchronization completed
*SVFn Servo OFF
RDYn Servo ready
Start of spindle forward run (reverse run)
time
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
771 IB-1501278-P
dle mode. (2) In the spindle mode, the axis does not run as a spindle even if the forward run command (SRN) or reverse
run command (SRI) is executed. (3) In the C axis mode, an operation error (M01 0005) occurs if the movement command is executed. In the servo
OFF mode, switching follows the setting of the spindle specification parameter "#1064 svof " (error correc- tion).
If the C axis mode selection command is issued until the spindle synchronization completion signal (spindle rotation speed synchronization completion (FSPRV) for rotation synchronization and spindle phase synchronization comple- tion (FSPPH) for phase synchronization (FSPPH)) is set ON after the spindle synchronization command has been issued, the mode is switch to the C axis mode after the spindle synchronization completion signal has been set ON. The following shows the C axis mode selection command from after the spindle synchronization command has been issued to before the spindle synchronization is completed.
C axis mode selection command in spindle synchronization incomplete state
M3 S1=500 M23 S2=0 MG114.1 H1 D-2 R0
NC->PLC
NC->PLC
PLC->NC
time
Spindle mode C axis mode
In spindle synchronization
Wait for the completion of spindle synchronization.
Phase alignment (at R command)
Reference spindle (S1) Synchronized spindle (S2)
Spindle/C axis control status
FSPPH Spindle rotation speed
synchronization completed
*SVFn Servo OFF
RDYn Servo ready
M: C axis switching command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
772IB-1501278-P
The spindle synchronization is canceled while the reference spindle remains set in the C axis mode by issuing the spindle synchronization cancel command in the C axis mode or axis stop state. The following shows the spindle synchronization cancel operation in the C axis mode.
(1) If the spindle is stopped by feed hold or cutting override zero during C axis movement, the spindle synchroniza- tion control is canceled with the spindle synchronization cancel command.
(2) If the C axis is in process of movement when the spindle synchronization cancel command is issued, it causes an operation error (M01 1135), and the spindle synchronization cancel operation is not completed. When the movement of the C axis is completed and the C axis is set to the smoothing zero, the operation error is canceled, and the spindle synchronization cancel operation is completed.
(1) When a spindle that is not in the spindle synchronization state is set in the C axis control mode, if the spindle synchronization command is issued using the spindle as the reference spindle, it causes an operation error (M01 1026).
Spindle synchronization cancel in C axis mode
Spindle synchronization command using the spindle in the C axis mode as the reference spindle
M G113G00 C100.G114.1 H1 D-2 G00 C200. M24 S2=2000
NC->PLC
NC->PLC
PLC->NC
PLC->NC
Spindle mode C axis mode
In spindle synchronization
Synchronized with reference spindle Spindle control
Reference spindle
FSPRV Spindle rotation speed
synchronization completed
*SVFn Servo OFF
RDYn Servo ready
SRI Start of spindle reverse run
(Synchronized spindle)
Reference spindle (S1) Synchronized spindle (S2)
Synchronized spindle
Spindle synchroni- zation
M: C axis switching command
time
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
773 IB-1501278-P
When the reference spindle is in the C axis control state, the synchronized spindle synchronizes with the reference spindle in the spindle control state without being setting in the C axis control state.
(1) The upper limit of the rotation speed in the C axis mode is controlled by the rapid traverse rate (#2001 rapid) or cutting feed clamp speed (#2002 clamp) of the C axis set to the axis specification parameter; therefore, the ro- tation speed of the spindle motor may exceed the highest spindle rotation speed depending on the setting of the C axis rapid traverse rate or clamp speed. The rapid traverse speed (#2001 rapid) and cutting feed clamp speed (#2002 clamp) of the C axis must not be below the highest spindle rotation speed (#3001 slimt1 to #3004 slimt4) of the reference or synchronized spindle (which depends on the MTB specifications).
C axis rapid traverse rate (/min) Highest spindle rotation speed (r/min) 360()
(2) If the spindle in the C axis mode is set to the reference or synchronized spindle, it causes an operation error (M01 1026). When the control mode at power-on is set to the C axis mode, switch it to the spindle mode once to com- mand the spindle synchronization, and switch it to the C axis mode again. The control mode at power-on depends on the MTB specifications (parameter "#3129 cax_spec/bit2").
(3) If the C axis servo OFF signal (*SVFn) of the synchronized spindle is set to ON during spindle synchronization, it causes an operation error (M01 1026).
Relationship with other functions
Function that can be commanded by the spindle position control (spindle/C axis control) under spindle syn- chronization control
Contents of command Operation
C axis selection command OFF The reference spindle is switched to the C axis mode, but the synchronized spin- dle is kept in the synchronous state.
Spindle synchronization cancel command (G113.1)
Cancels the spindle synchronization control. If the spindle synchronization cancel command is issued during movement of the
C axis, it causes an operation error (M01 1135), and the spindle synchronization is not canceled. When the operation error is canceled after the C axis has stopped, the spindle synchronization control is also canceled.
Emergency stop When the spindle is set in the emergency stop state, the spindle synchronization control is canceled immediately. If emergency stop occurs in the C axis mode, the reference or synchronized
spindle decelerates and stops based on the parameter (spindle parameter "#13056 SP056 EMGt " deceleration time constant at emergency stop) that is set to each spindle.
Tool center point control (G43.4)
When the reference spindle is in C axis mode, the functions shown on the left can be commanded. If the function shown on the left is commanded when the reference spindle is in
spindle mode, a program error (P934) or operation error (M01 0186) occurs. Inclined surface machining command (G68.2) 3-dimensional tool radius com- pensation (Tool's vertical-direc- tion compensation) (G41.2/G42.2/G40) Workpiece installation error compensation (G54.4) 3-dimensional manual feed Rotation center error compen- sation
Cautions on spindle position control under spindle synchronization control
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
774IB-1501278-P
18.2 Tool Spindle Synchronization I 18.2.1 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon) ; G114.2, G113.1
In a machine having a rotary tool axis and having a spindle controlled as the workpiece axis, polygon machining between spindles can be carried out by controlling the rotation of the workpiece axis in synchronization with the ro- tary tool axis rotation.
This function cannot be combined with the following spindle synchronization functions while it is active. An operation error (M01 1005) occurs. Spindle synchronization I Spindle synchronization II Tool spindle synchronization IA Tool spindle synchronization IB (IC) Tool Spindle Synchronization II
(1) An axis address that involves any travel cannot be put in the same block as for the tool spindle synchronization IA cancel command. Doing so causes the program error (P33) when the cancel command is issued, which caus- es automatic operation to pause.
Function and purpose
Command format
Tool spindle synchronization IA (Spindle-spindle, polygon mode) ON
G114.2 H__ D__ E__ L__ R__ ;
H Rotary tool axis selection (Reference spindle) D Workpiece axis selection (Synchronized spindle) E Rotary tool axis rotation ratio designation L Workpiece axis rotation ratio designation R Phase shift amount of synchronized spindle
Tool spindle synchronization IA (Spindle-spindle, polygon mode) OFF
G113.1 ;
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
775 IB-1501278-P
Tool spindle synchronization IA ON (G114.2) command sets the polygon machining mode that rotates the two axes in synchronization with differing speeds by designating the rotary tool axis and workpiece axes and the rotation ratio (Number of the rotary tool gear teeth and workpiece corners) of the two designated spindles (spindle and spindle). Tool spindle synchronization IA OFF (G113.1) cancels the synchronous state of two synchronously rotating spindles using the spindle synchronization command.
(*1) There are two spindle command methods: spindle number method and spindle name method. Command with the spindle names, only when all spindles are set with the spindle name parameter (#3077 Sname) (from 1 to 9). For others, command with the spindle number. These settings depend on the MTB spec- ifications.
(*2) The available spindle type and connection method depend on the specifications of your machine tool.
Explanation of address
Address Meaning Command range (unit)
Remarks
H Rotary tool axis selec- tion Command the spindle number or spindle name of the rotary tool axis from multiple spindles. (*1)
Spindle number: 1 to n (n: Maximum num- ber of available spin- dles) Spindle name: 1 to 9
If a value exceeding the command range is command- ed, a program error (P35) will occur. If there is no command, a program error (P33) will oc-
cur. If the same value as the D command is commanded, a
program error (P33) will occur. If an analog-connected spindle is selected, a program
error (P700) will occur. (*2) D Workpiece axis selection
Commands the spindle number or spindle name of the workpiece axis of two spindles. (*1)
Spindle number: 1 to n or -1 to -n (n: Maximum num- ber of available spin- dles) Spindle name: 1 to 9 or -1 to -9
If a value exceeding the command range is command- ed, a program error (P35) will occur. If there is no command, a program error (P33) will oc-
cur. The rotation direction of the workpiece axis in respect
to the rotary tool axis is commanded with the D sign. If the same value as the H command is commanded, a
program error (P33) will occur. If an analog-connected spindle is selected, a program
error (P700) will occur. (*2) E Rotary tool axis rotation
ratio designation Set the rotation ratio (Number of rotary tool gear teeth) of the rotary tool axis.
1 to 999 If a value exceeding the command range is command- ed, a program error (P35) will occur. If there is no command, the rotation ratio will be inter-
preted as 1.
L Workpiece axis rotation ratio designation Set the rotation ratio (number of workpiece corners) of the work- piece axis.
1 to 999 If a value exceeding the command range is command- ed, a program error (P35) will occur. If there is no command, the rotation ratio will be inter-
preted as 1.
R Phase shift amount of synchronized spindle Set the shift amount from the synchronized spin- dle's reference position ("one rotation" signal).
0 to 359.999 () If a value exceeding the command range is command- ed, a program error (P35) will occur. The commanded shift amount will be applied in the
clockwise direction in respect to the spindle. Minimum resolution of commanded shift amount
Semi-close case 360/4096 []
Full-close case (360/4096) * K [] (K: Gear ratio of spindle and encoder)
If there is no R command, phase alignment will not be carried out.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
776IB-1501278-P
The rotary tool axis and workpiece axis rotation speed and rotation direction during tool spindle synchronization IA command are as follows.
(1) The rotation speed and rotation direction of the rotary tool axis are the rotation speed commanded with the S command and the rotation direction commanded with the M command, etc., for the spindle selected as the rotary tool axis.
(2) The workpiece axis rotation speed is determined by the number of the rotary tool gear teeth workpiece corners commanded with G114.2.
(3) The workpiece axis rotation direction is determined by the sign of the address D commanded with G114.2. In other words, when the "D" sign is "+", the workpiece axis rotates in the same direction as the rotary tool axis, and when "-", the workpiece axis rotates in the reverse direction of the rotary tool axis.
(4) After tool spindle synchronization IA is commanded, the relation of the rotary tool axis and workpiece axis rotation is held in all automatic or manual operation modes until spindle synchronization cancel (G113) is commanded, the "spindle synchronization cancel" signal is input, or reset (reset 1, reset 2, reset & rewind) is executed when "#1239 set11/bit3" is set to "1". Even during feed hold, the rotary tool axis and workpiece axis synchronization state is held.
(1) Even if the forward run command and reverse run command are not issued to the workpiece axis when the tool spindle synchronization IA mode is commanded, the workpiece axis starts rotation synchronously with the rotary tool axis if the rotation command is issued to the rotary tool axis.
(2) The rotation command (S command) and constant surface speed control are invalid in respect to the workpiece axis during the tool spindle synchronization IA mode. Note that the modal will be updated, so these will be effec- tive after the spindle synchronization is canceled.
(3) If the rotation speed commanded to the workpiece axis exceeds the maximum rotation speed of the rotary tool axis or the maximum clamp speed designated by address S following G92, the workpiece axis rotation speed is clamped to prevent the rotation speed from exceeding those maximum speeds.
Detailed description
Rotary axis and rotation direction
Sw: Workpiece axis rotation speed (r/min) Sh: Rotary tool axis rotation speed (r/min) E: Rotary tool axis rotation ratio (Number of rotary tool gear teeth) L: Workpiece axis rotation ratio (Number of workpiece corners)
Spindle operation for spindle-spindle polygon
Sw = E LSh *
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
777 IB-1501278-P
(1) Acceleration/deceleration time constants for up to eight steps can be selected according to the spindle rotation speed for the acceleration/deceleration during spindle-spindle polygon machining. The acceleration/deceleration in each step is as follows. Time required from minimum rotation speed to maximum rotation speed in each step = [Time constant without multi-step acceleration/deceleration] * [magnification of time constant in each step] * [Rate of rotation speed width in each step respect to rotation speed width up to limit rotation speed]
Time required to rotate to sptc1 set rotation speed from stopped state (a) = spt * sptc1 / slimit Time required to reach sptc2 set rotation speed from sptc1 (b) = spt * spdiv1 * (sptc2 - sptc1) / slimit Time required to reach sptc3 set rotation speed from sptc2 (c) = spt * spdiv2 * (sptc3 - sptc2) / slimit Time required to reach sptc4 set rotation speed from sptc3 (d) = spt * spdiv3 * (sptc4 - sptc3) / slimit Time required to reach sptc5 set rotation speed from sptc4 (e) = spt * spdiv4 * (sptc5 - sptc4) / slimit Time required to reach sptc6 set rotation speed from sptc5 (f) = spt * spdiv5 * (sptc6 - sptc5) / slimit Time required to reach sptc7 set rotation speed from sptc6 (g) = spt * spdiv6 * (sptc7 - sptc6) / slimit Time required to reach slimit set rotation speed from sptc7 (h) = spt * spdiv7 * (slimit - sptc7) / slimit
To decrease the number of acceleration/deceleration steps, set one of the followings for the unnecessary step. Magnification for time constant changeover speed (spdiv7 to spdiv1) = 0 (or 1) Spindle synchronous multi-step acceleration/deceleration changeover speed (sptc7 to sptc1) = Limit rota-
tion speed (slimit) or higher (2) The rotary tool axis accelerates/decelerates linearly according to the spindle synchronous acceleration/deceler-
ation time constant (spt) setting value of the spindle selected as the rotary tool axis and workpiece axis, which- ever is larger.
(3) If the rotary tool axis command rotation speed is changed during spindle synchronization, the axis will accelerate/ decelerate to the commanded rotation speed according to the spindle acceleration/deceleration set in the pa- rameters while maintaining the synchronized state.
Multi-step acceleration/deceleration control
Rotation speed (r/min)
Time (ms)
slimit
sptc7
sptc6
sptc5
sptc4
sptc3
sptc2
sptc1
0 (a) (b) (c) (d) (e) (f) (g) (h)
spt
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
778IB-1501278-P
(1) If the tool spindle synchronization IA command (with R designation) is commanded with the G114.2 command, the synchronized spindle rotating at an arbitrary rotation speed will accelerate or decelerate to the rotation speed following the reference spindle and synchronized spindle rotation ratio command, and the spindle synchroniza- tion state will be entered. The spindles will then enter the spindle synchronization state. After that, the phases will be aligned to realize the rotation phase commanded with the R address.
(2) The spindle synchronization phase shift amount is commanded as the shift amount from the synchronized spin- dle's (workpiece axis) reference position ("one rotation" signal). There is not the shift amount in respect to the reference spindle (rotary tool axis).
If the spindle-mode rotary axis is commanded for the reference spindle or synchronized spindle of spindle synchro- nization I/II, tool spindle synchronization IA (spindle-spindle, polygon), or tool spindle synchronization IB (spindle- spindle, polygon), an operation error (M01 1024) occurs.
Tool spindle synchronization IA is not available during tool center point control. A program error (P942) occurs. How- ever, the tool center point control command can be issued during tool spindle synchronization IA.
Tool spindle synchronization IA is not available during execution of the inclined surface machining command. A pro- gram error (P951) occurs. However, the inclined surface machining command can be issued during tool spindle syn- chronization IA.
(1) Always command G114.2 alone in a block. (2) Do not issue S command in the same block as G114.2. (3) The tool spindle synchronization IA (spindle-spindle, polygon) mode cannot be commanded during the spindle
synchronization mode commanded with G114.*. An operation error (M01 1005) will occur. (4) If spindle-spindle polygon machining is commanded while the "phase shift calculation request" signal SSPHM is
ON, an operation error (M01 1106) will occur. (5) Tool spindle synchronization IA (G114.2) cannot be executed using the spindle that is used in the synchronous
tapping. An operation error (M01 1007) will occur. Also, the synchronous tapping cannot be commanded using the spindle which is used in G114.2 command. An operation error (M01 1139) will occur.
(6) When the spindle/C axis is used for the spindle-spindle polygon machining cannot be executed by designating the C axis mode spindle with the G114.2 command. An operation error (M01 1026) will occur.
(7) After G114.2 is commanded, the cutting feed block will not start until synchronization is established. Operation will stop with an operation error (M01 1033).
Phase alignment control
Relationship with other functions
Spindle-mode rotary axis control
Tool center point control
Inclined surface machining
Precautions
Precautions for programming
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
779 IB-1501278-P
(1) Make sure that the rotation ratio of spindle (and rotary tool axis spindle) actual rotation speed and encoder rota- tion speed has the following relation. Spindle rotation speed/encoder rotation speed = "n" ("n" is an integer of "1" or more) If this relationship is not established, the encoder's reference position will not stay at a constant position on the spindle, and thus the phase (position) will deviate with each phase alignment command. Note that even in this case, as shown below, if the number of rotary tool gear teeth (Number of workpiece cor- ners) is equivalent to the rotation ratio, the blade and workpiece phase (position) will not deviate. (Rotary tool axis spindle rotation speed * Number of rotary tool gear teeth) /encoder rotation speed = "n" ("n" is an integer of "1" or more)
(2) During phase alignment control, phase alignment is carried out following each spindle encoder's reference posi- tion. Thus, if the positional relation of the workpiece and reference position (rotary tool and reference position) devi- ates when the power is turned OFF/ON or when the tool is changed, etc., the phase will deviate.
Restrictions regarding phase alignment control
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
780IB-1501278-P
18.2.2 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon) ; G51.2/G50.2 or G251/G250
In a machine having a workpiece axis and having a spindle controlled as the rotary tool axis, polygon machining between spindles can be carried out by controlling the rotation of the rotary tool axis in synchronization with the work- piece axis rotation. Tool spindle synchronization IB and tool spindle synchronization IC are switched depending on the setting of the parameter (#1501).
This function is valid when the G code system is 1.
This function cannot be combined with the following spindle synchronization functions while it is active. An operation error (M01 1005) occurs. Spindle synchronization I Spindle synchronization II Tool spindle synchronization IA Tool spindle synchronization IB (IC) Tool Spindle Synchronization II
(1) An axis address that involves any travel cannot be put in the same block as the tool spindle synchronization IB mode cancel command. Doing so causes the program error (P33) when the cancel command is issued, which causes automatic operation to pause.
Function and purpose
#1501 polyax = 0 : Tool spindle synchronization IB Other than 0 : Tool spindle synchronization IC
Command format
Tool spindle synchronization IB (Spindle-spindle, polygon mode) ON (or G251)
G51.2 H__D__P__Q__R__ ;
H Workpiece axis selection (Reference spindle) D Rotary tool axis selection (Synchronized spindle) P Workpiece axis rotation ratio designation Q Rotary tool axis rotation ratio designation R Phase shift amount of synchronized spindle
Tool spindle synchronization IB (Spindle-spindle, polygon mode) Cancel (or G250)
G50.2 ;
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
781 IB-1501278-P
Tool spindle synchronization IB ON (G51.2) command sets the polygon machining mode that rotates the two axes in synchronization with differing speeds by designating the rotary tool axis and workpiece axes and the rotation ratio (Number of the rotary tool gear teeth and workpiece corners) of the two designated spindle (spindle and spindle). Tool spindle synchronization IB OFF (G50.2) command cancels the synchronous state of rotating two spindles by the tool spindle synchronization command. The spindle-spindle polygon machining mode is also canceled in the following cases. Power OFF Emergency stop Reset (reset 1, reset 2, reset & rewind)
(only when #1239 set11/bit3 = 1) "Spindle-spindle polygon machining cancel" signal Spindle synchronization cancel command (G113.1) "Spindle synchronization cancel" signal (SPSYC) The detail of each address of the command format is as follows.
(*1) There are two spindle command methods: spindle number method and spindle name method. Command with the spindle names, only when all spindles are set with the spindle name parameter (#3077 Sname) (from 1 to 9). For others, command with the spindle number. These settings depend on the MTB spec- ifications.
(*2) The available spindle type and connection method depend on the specifications of your machine tool.
Detailed explanation of command format
Address Meaning Command range (unit)
Remarks
H Workpiece axis selection Command the spindle number of the workpiece axis. (*1)
Spindle No.: 1 to n (n: Maximum number of available spindles) Spindle name: 1 to 9
If a value exceeding the command range is com- manded, a program error (P35) will occur. If the same value as the D command is command-
ed, a program error (P33) will occur. If an analog-connected spindle is selected, a pro-
gram error (P33) will occur. (*2) If this address is omitted, the spindle number or spin-
dle name specified in the parameter is designated. D Rotary tool axis selection
Command the spindle number of the rotary tool axis. (*1)
Spindle No.: 1 to n (n: Maximum num- ber of available spin- dles) Spindle name: 1 to 9
If a value exceeding the command range is com- manded, a program error (P35) will occur. If the same value as the H command is command-
ed, a program error (P33) will occur. If an analog-connected spindle is selected, a pro-
gram error (P33) will occur. (*2) If this address is omitted, the spindle number or spin-
dle name specified in the parameter is designated. P Workpiece axis rotation ra-
tio designation Set the rotation ratio (num- ber of workpiece corners) of the workpiece axis.
1 to 999 If a value exceeding the command range is com- manded, a program error (P35) will occur.
Q Rotary tool axis rotation ratio designation Command the rotary tool axis rotation ratio (number of tool teeth).
1 to 999 -1 to -999
If a value exceeding the command range is com- manded, a program error (P35) will occur. If a negative "-" sign is commanded, the rotary tool
axis will rotate in the direction opposite to the work- piece axis.
R Phase shift amount of syn- chronized spindle Command the shift amount designation from the reference position ("one rotation" signal) of the rotary tool axis spindle.
0 to 359.999 () If a value exceeding the command range is com- manded, a program error (P35) will occur. The commanded shift amount will be applied in the
clockwise direction in respect to the spindle. Minimum resolution of commanded shift amount
Semi-close case 360/4096 [] Full-close case (360/4096) * K [] ) (K: Gear ratio of spindle and encoder) If there is no R command, the phase will be handled
as R0. (only when #1239 set11/bit4 = 0)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
782IB-1501278-P
The workpiece axis and rotary tool axis rotation speed and rotation direction during spindle-spindle polygon machin- ing are as follows.
(1) The workpiece axis rotation speed and rotation direction are rotation speed commanded with the S command and the rotation direction commanded with the M command, etc., for the spindle selected as the workpiece axis.
(2) The rotary tool axis rotation speed is determined by the number of the rotary tool teeth and number of workpiece corners commanded with G51.2/G251.
(3) The rotary tool axis rotation direction is determined by the sign of the rotary tool axis selection Q commanded with G51.2/G251. In other words, if the Q sign is "+", the rotary tool axis will rotate in the same direction as the workpiece axis. If the Q sign is "-", the rotary tool axis will rotate in the reverse direction of workpiece axis.
(4) After tool spindle synchronization IB (G51.2/G251) is commanded, the relationship between the workpiece axis and rotary tool axis rotation is held until tool spindle synchronization IB cancel (G50.2/G250) is commanded, the "spindle-spindle polygon machining cancel" signal is input, or until the "reset or emergency stop" signal is input. Even at feed hold, the workpiece axis and rotary tool axis synchronization states are held.
(1) When the tool spindle synchronization IB mode is commanded, even if neither the forward run nor reverse run command is input for the rotary tool axis, the rotary tool axis will start rotating.
(2) If spindle stop is commanded to a rotary tool axis during the tool spindle synchronization IB mode (when the "spindle stop" signal is ON), the rotary tool axis will stop rotating even if the workpiece axis is rotating.
(3) The rotation command (S command) and constant surface speed control are invalid in respect to the rotary tool axis during the tool spindle synchronization IB mode. Note that the modal is updated, so these will be validated when the spindle-spindle polygon machining is canceled.
(4) If the rotation speed commanded to the workpiece axis exceeds the maximum rotation speed of the rotary tool axis or the maximum clamp speed designated by address S following G92, the workpiece axis rotation speed is clamped to prevent the rotation speed from exceeding those maximum speeds.
(1) Acceleration/deceleration of the workpiece axis will be carried out linearly according to the spindle synchroniza- tion acceleration/deceleration time constant (parameter "#3049 spt") of the spindle selected as the workpiece axis.
(2) By setting the spindle synchronization multi-step acceleration/deceleration time constant changeover speed lev- els 1 to 7 (parameters "#3054 sptc1" to "#3060 sptc7") and the scale for the time constant changeover speed (parameters "#3061 spdiv1" to "#3067 spdiv7"), the acceleration/deceleration time can be changed in up to eight steps.
(3) If the workpiece axis command rotation speed is changed during spindle synchronization state, the commanded speed will be reached by accelerating or decelerating according to the spindle acceleration/deceleration set in the parameters while maintaining the synchronized state.
Detailed description
Rotary axis and rotation direction
Sw: Rotary tool axis rotation speed (r/min) Sh: Workpiece axis rotation speed (r/min) P: Workpiece axis rotation ratio (Number of workpiece corners) Q: Rotary tool axis rotation ratio (Number of rotary tool gear teeth)
Operation for polygon machining with rotary tool axis
Acceleration/deceleration control
Sw = Q PSh *
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
783 IB-1501278-P
(1) If the tool spindle synchronization IB command (R is treated as "0" when there is no R command) is commanded with G51.2/G251, the workpiece axis spindle rotating at an arbitrary rotation speed will accelerate/decelerate to the rotation speed following the rotation ratio command of the workpiece axis spindle and the spindle synchro- nization state will be entered. The spindles will then enter the spindle synchronization state. After that, the phases will be aligned to realize the rotation phase commanded with the R address.
(2) The spindle synchronization phase shift amount is commanded the shift amount from the rotary tool axis spin- dle's reference position ("one rotation" signal). This is not the shift amount for the workpiece axis.
Tool spindle synchronization IB cannot be executed using the spindle-mode rotary axis. An operation error (M01 1024) will occur.
Tool spindle synchronization IB is not available during tool center point control. A program error (P942) occurs. How- ever, the tool center point control command can be issued during tool spindle synchronization IB.
Tool spindle synchronization IB is not available during execution of the inclined surface machining command. A pro- gram error (P951) occurs. However, the inclined surface machining command can be issued during tool spindle syn- chronization IB.
Phase alignment control
Relationship with other functions
Spindle-mode rotary axis control
Tool center point control
Inclined surface machining
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
784IB-1501278-P
(1) Make sure that the spindle (and workpiece axis spindle) actual rotation speed and encoder rotation speed's ro- tation ratio has the following relation. Spindle rotation speed/encoder rotation speed = "n" ("n" is an integer of 1 or more) If this relationship is not established, the encoder's reference position will not stay at a constant position on the spindle, and thus the phase (position) will deviate with each phase alignment command. Note that even in this case, as shown below, if the number of workpiece corners (number of rotary tool teeth) corresponds to the rotation ratio, the phase (position) of the blade and workpiece will not deviate. (Workpiece axis spindle rotation speed * Number of workpiece teeth) /encoder rotation speed = "n" ("n" is an integer of "1" or more)
(2) During phase alignment control, the phase are aligned to the reference position of each spindle's encoder. Thus, if the position relation of the workpiece and reference position (workpiece and reference position) deviates when the power is turned ON/OFF or the tool is replaced, etc., the phase will deviate.
(1) G51.2 (G251) must be commanded alone in a block, which also applies to G50.2 (G250). (2) The R command can be omitted when entering the tool spindle synchronization IB mode, but the P and Q com-
mands must always be issued. A program error (P33) will occur if there are not the P and Q commands. (3) To change the P, Q or R modal value in the tool spindle synchronization IB mode, command G51.2/G251 again.
In this case, R can be commanded alone. However, if either P or Q is also changed, always command P and Q again.
(4) Commands can be issued to each part system, but two or more part systems cannot be used simultaneously. The part system commanded first will be valid, and an operation error (M01 1005) will occur for that commanded last.
(5) The spindle No. designated in the parameters will be used if D_H_ is omitted from the G51.2/G251 command. (6) A program error (P610) will occur if the workpiece axis No. (#1518) and rotary tool axis No. (#1519) are the same
as the value set in the parameters. A program error (P33) will occur if the spindle is connected in analog mode. (These parameters depend on the MTB specifications.)
(7) After G51.2/G251 was commanded, the cutting feed block will not start until synchronization is established. (An operation error (M01 1033) will occur, and the program stops.)
(8) Tool spindle synchronization IB (G51.2/G251) machining cannot be executed by designating the spindle which is used in the synchronous tapping. An operation error (M01 1007) will occur. Also, the synchronous tapping can- not be commanded using a spindle which is used in G51.2/G251 command. An operation error (M01 1139) will occur.
(9) If the rotary tool axis number or workpiece axis number is changed in the tool spindle synchronization IB mode, a program error (P33) will occur.
Precautions
Restrictions regarding phase alignment control
Precautions for programming
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
785 IB-1501278-P
18.2.3 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon) ; G51.2/G50.2 or G251/G250
This function controls so that the workpiece (spindle) and tool (rotary tool axis) are synchronously rotating with the commanded ratio to conduct polygon machining. This function is available for machining of square-head bolts, bolt heads of hexagon-head bolts, or hexagon nuts. Tool spindle synchronization IB and tool spindle synchronization IC are switched depending on the setting of the parameter (#1501).
This function cannot be combined with the following spindle synchronization functions while it is active. An operation error (M01 1005) occurs. Spindle synchronization I Spindle synchronization II Tool spindle synchronization IA Tool spindle synchronization IB (IC) Tool Spindle Synchronization II
In addition to the G50.2 command, the tool spindle synchronization IC mode is also canceled in the following cases. Power OFF Emergency stop Reset (reset 1, reset 2, reset & rewind)
Function and purpose
Command format
Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon mode) ON (or G251)
G51.2 P__ Q__ ;
P,Q Spindle and rotary tool axis rotation ratio (P__:Q__) P : Spindle Q : Rotary tool axis Command range : Integer value between 1 and 200, -1 and -200 Rotation direction : Designate with a sign ("+" for forward rotation, whereas "-" for reverse rotation).
Tool spindle synchronization IC (spindle-NC axis, polygon) cancel (or G250)
G50.2 ;
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
786IB-1501278-P
The rotary tool axis depends on the setting of the base specification parameter "#1501 polyax".
(1) The spindle rotation direction during the polygon machining mode is determined by the P command sign and the spindle parameter "#3106 zrn_typ/bit7" (synchronous tap command polarity).
(2) The rotation direction of the rotary tool axis during the polygon machining mode is determined by the Q command sign and the base specifications parameters "#1018 CCW".
Detailed description
Details of operation
S1000 ; The spindle rotation speed (workpiece rotation speed) is commanded. G51.2 P1 Q2 ; :
The polygon machining mode is entered with the G51.2 command. The spindle and rotary tool axis start rotating, and control is applied so that the spindle rotation speed and tool axis rotation speed are the commanded ratio (P:Q).(Cutting into workpiece)
: G50.2 ; The polygon machining mode between the spindle and rotary tool axis is canceled
by the G50.2 command, and the spindle and rotary tool axis rotation stop.
Rotation direction
P command sign #3106 zrn_typ/bit7 Rotation direction
(+) 0 CW (+) 1 CCW (-) 0 CCW (-) 1 CW
Q command sign #1018 CCW Rotation direction
(+) 0 CW (+) 1 CCW (-) 0 CCW (-) 1 CW
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
787 IB-1501278-P
If the spindle-mode rotary axis is changed to the servo axis mode while tool spindle synchronization IC is executed using the spindle-mode rotary axis as the polygon spindle, an operation error (M01 1024) occurs. Also, if tool spindle synchronization IC is commanded using the spindle-mode rotary axis of servo axis mode as the polygon axis, an operation error (M01 1024) occurs.
If the spindle/C axis is changed to the C axis mode while tool spindle synchronization IC is executed using the spin- dle/C axis as the polygon-related spindle, an operation error (M01 1026) occurs. Also, if tool spindle synchronization IC is commanded using the spindle/C axis in the C axis mode as the polygon-related spindle, an operation error (M01 1026) occurs.
When tool spindle synchronization IC is commanded while the high-speed high-accuracy control is valid or when high-speed high-accuracy control is commanded during tool spindle synchronization IC, high-speed high-accuracy control is temporarily canceled, and tool spindle synchronization IC is executed preferentially.
The arbitrary axis exchange command (G140), arbitrary axis exchange return command (G141), or reference axis arrange return command (G142) cannot be issued in the part system for tool spindle synchronization IC. A program error (P501) occurs. However, tool spindle synchronization IC using the arbitrary axis exchange axis can be com- manded.
The rotary tool axis of tool spindle synchronization IC cannot be commanded as the axis to be replaced. Doing so triggers the arbitrary axis exchange disable state.
The 3-dimensional coordinate conversion cannot be commanded in the part system for tool spindle synchronization IC. A program error (P922) occurs. Also, tool spindle synchronization IC cannot be commanded during 3-dimensional coordinate conversion. A program error (P921) occurs.
Tool spindle synchronization IC is not available during tool center point control. A program error (P942) occurs. The tool center point control command can be issued during tool spindle synchronization IC.
expected operation by the tool center point control command during tool spindle synchronization IC.
Tool spindle synchronization IC is not available during execution of the inclined surface machining command. A pro- gram error (P951) occurs. Also, the inclined surface machining command cannot be issued during tool spindle syn- chronization IC. A program error (P952) occurs.
Relationship with other functions
Spindle-mode rotary axis control
Spindle position control (Spindle/C axis control)
High-speed high-accuracy Control
Arbitrary axis exchange control
3-dimensional coordinate conversion
Tool center point control
Inclined surface machining command
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
788IB-1501278-P
(1) The tool spindle synchronization IC specifications must be provided to use this function. If "G51.2/G251" or "G50.2/G250" is commanded without the specifications, a program error (P39) will occur.
(2) G51.2 (G251) must be commanded alone in a block, which also applies to G50.2 (G250). If the G51.2/G251 (G50.2/G250) command and G code of group 0 are commanded in the same block, the
G code commanded last in the block will have the priority. If the G51.2/G251 (G50.2/G250) command and G code other than a group 0 code are commanded in the
same block, a program error (P33) will occur. (3) While in the polygon machining mode, a movement command cannot be issued in the machining program for an
NC axis set as the rotary tool axis. If a movement command is issued to the rotary tool axis during the polygon machining mode, the program error (P32) will occur.
(4) The NC axis set as the rotary tool axis can be used as a feed axis in modes other than the polygon machining mode.
(5) The following functions are invalid for the rotary tool axis during the polygon machining mode. Override Feed hold Stored stroke limit
(6) The spindle rotation speed can be changed with the S command even during the polygon machining mode. The spindle override and spindle rotation speed clamp are also valid. If the spindle rotation speed is changed, the rotary tool axis rotation speed will also change so that the spindle and rotary tool axis established the P:Q ratio.
(7) The forward run/reverse run commands are invalid for the spindle when the polygon machining mode is in effect. (8) If the feedrate for the rotary tool axis exceeds the rapid traverse rate (axis specifications parameters "#2001 rap-
id") when the polygon machining mode is in effect, the speed will be clamped at the rapid traverse rate. If the rotary tool axis is clamped at the rapid traverse rate, the spindle speed will also be set to lower than the command speed so that the spindle and rotary tool axis establish the P:Q ratio.
(9) The position loop gain for the rotary tool axis will be the value set in the axis specifications parameters "#2017 tap_g" during the polygon machining mode. The position loop gain for the spindle will be the spindle parameters "#13002 PGN" setting value.
(10) To perform polygon machining, set the parameter "#8213 rotary axis type" to "0" or "1". (11) The following functions cannot be used simultaneously with polygon machining. Synchronous tapping Thread cutting
(12) If an axis other than the rotary tool axis reaches the stroke end during the polygon machining mode, the axis other than the rotary tool axis will stop moving, but the rotary tool axis and spindle rotation will not stop.
(13) If the rotary tool axis reaches the stroke end during the polygon machining mode, the rotary tool axis and spindle rotation will stop, and the movement of axes other than the rotary tool axis will also stop.
(14) If the spindle specifications parameter "#3106 zrn_typ/bit4" is set to "0", the polygon machining will start after the spindle returns to the zero point. (This parameter setting depends on the MTB specifications.)
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
789 IB-1501278-P
18.3 Tool Spindle Synchronization II 18.3.1 Tool Spindle Synchronization II (Hobbing) ; G114.3/G113
This function is to cut the gear with hob (hob cutter). A spur gear can be machined by synchronizing and rotating the hob axis and the workpiece axis in a constant ratio. A helical gear can be machined by compensating the workpiece axis according to the gear torsion angle for the Z axis movement.
By synchronizing and rotating the hob axis and the workpiece axis in a constant rotation ratio, a gear is machined so that the cutter is engaged with gear.
In this manual, the hob axis and the workpiece axis are defined as follows:
Hob axis : Rotary tool axis on which a hob is mounted Workpiece axis : Rotary axis on which a workpiece is mounted Hob threads : Number of the screw paths created by cutter part on hob. Usually this is 1 row.
This function cannot be combined with the following spindle synchronization functions while it is active. An operation error (M01 1005) occurs. Spindle synchronization I Spindle synchronization II Tool spindle synchronization IA Tool spindle synchronization IB (IC) Tool Spindle Synchronization II
Function and purpose
Spur gears Helical gears
(a) Hob (b) Gear
(a)
(b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
790IB-1501278-P
(1) An axis address that involves any travel cannot be put in the same block as the tool spindle synchronization II cancel command. Doing so causes the program error (P33) when the cancel command is issued, which causes automatic operation to pause.
Command format
Tool spindle synchronization II (hobbing) ON (for spur gear)
G114.3 H__ D__ E__ L__ R__ ;
H Hob axis selection D Workpiece axis selection E Hob axis rotation ratio designation L Workpiece axis rotation ratio designation R Workpiece axis phase shift amount
Tool spindle synchronization II (hobbing) ON (for helical gear)
G114.3 H__ D__ E__ L__ P__ Q__ R__ ;
H Hob axis selection D Workpiece axis selection E Hob axis rotation ratio designation L Workpiece axis rotation ratio designation P Gear torsion angle designation Q Module or diametral pitch designation R Workpiece axis phase shift amount
Tool spindle synchronization II (hobbing) OFF
G113.1 ;
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
791 IB-1501278-P
Tool spindle synchronization II ON (G114.3 for spur gear) is set as the hobbing mode for the spur gears that syn- chronously rotates two axes at different speeds by designating the hob axis and workpiece axis and designating the rotation ratio (number of hob threads and number of gear teeth) for the two designated axes.
Tool spindle synchronization II ON (G114.3 for helical gears) is set as the hobbing mode for the helical gears by designating the gear torsion angle and module or diametral pitch.
Tool spindle synchronization II OFF (G113.1) cancels the synchronous state of the hob axis and workpiece axis ro- tating in synchronization with the tool spindle synchronization II (hobbing) command.
Detailed explanation of format
Address Meaning Command range (unit)
Remarks
H Hob axis selection Command the spindle number of the hob axis. (*1)
Spindle No.: 1 to n (n: Maximum num- ber of available spin- dles) Spindle name: 1 to 9
If there is no command, a program error (P33) will occur. If an analog-connected spindle is selected, a program
error (P33) will occur. If disconnected spindle No. is designated, a program er-
ror (P35) will occur. D Workpiece axis selection
Command the rotation number of the workpiece axis.
-9 to -1, 1 to 9 1 to 8 Axis No. (in part system) 9: C axis
If there is no command, a program error (P33) will occur. The rotation direction of the workpiece axis in respect to
the hob axis is commanded with the D sign. If the D sign is "+", the workpiece axis will rotate in the
forward direction when the hob axis rotates in the for- ward direction. If the D sign is "-", the workpiece axis will rotate in the reverse direction when the hob axis ro- tates in the forward direction.
If the axis specified as the workpiece axis is not a rotary axis, a program error (P33) will occur.
If C axis is selected when there is no C axis, a program error (P33) will occur.
E Hob axis rotation ratio designation Command the hob axis rotation ratio (hob threads).
0 to 999 If there is no command, the rotation ratio will be inter- preted as 1.
If E0 is commanded, the workpiece axis will stop (syn- chronized with the Z axis for a helical gear). (*2)
L Workpiece axis rotation ratio designation Command the workpiece axis rotation ratio (num- ber of gear teeth).
1 to 999 If there is no command, the rotation ratio will be inter- preted as 1.
(For G code lists 6 and 7)
If L0 is commanded, the workpiece axis will stop (syn- chronized with the Z axis for a helical gear). (*6)
The rotation direction of the workpiece axis in respect to the hob axis is commanded with the L sign. L sign = "+": When the hob axis rotates forward, the workpiece axis also rotates forward. L sign = "-": When the hob axis rotates forward, the workpiece axis rotates backward.
R Workpiece axis phase shift amount Command the amount to shift from the workpiece axis reference position to synchronize with the hob axis reference position.
0 to 359999 (0 to 359.999) Decimal point input possible (*3)
The commanded shift amount will be applied in the workpiece axis counter's positive direction.
If there is no R command, phase alignment will not be carried out.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
792IB-1501278-P
(*1) If a value exceeding the command range is commanded, a program error (P35) will occur.
(*2) When address E = 0 is commanded, the workpiece axis will not rotate. Do not use this except for special cutting (cutting of only part of the gears, etc.).
(*3) The range which can be set depends on the input setting unit (parameter "#1003 iunit"). (Example) When the input setting unit is 0.000001, the range is 0 to 359.999999.
(*4) If the decimal point input is OFF, the available setting range varies according to the input setting unit (parameter "#1003 iunit"). When the input setting unit is 0.000001, the range is -89000000 to 89000000.
(*5) If the decimal point input is OFF, the available setting range varies according to the input setting unit (parameter "#1003 iunit"). When the input setting unit is 0.000001, the range is as follows. 100000 to 250000000 in metric system 1000000 to 2500000000 in inch system
(*6) When address L = 0 is commanded, the workpiece axis will not rotate. Do not use this except for special cutting (cutting of only part of the gears, etc.).
P Gear torsion angle des- ignation Command the torsion angle for the helical gear.
-89000 to 89000 (-89.000 to 89.000) Decimal point input possible (*4)
If there is no P command, or if P0 is commanded, a spur gear will be machined.
To move the Z axis in the plus direction after entering the hobbing mode, command the direction that the work- piece axis is twisted. P sign: when it is +, + direction P sign: when it is -, - direction
Q Module designation Command the normal module for helical gear. When inch input, com- mand the diametral pitch.
Metric input Module designation 100 to 25000 0.1 to 25. (0.1 to 25 mm) Inch input Diametral pitch des- ignation 1000 to 250000 0.1 to 25. (0.1 to 25inch-1) Decimal point input possible (*5)
If there is no Q command for helical gear (when P is des- ignated), a program error (P33) will occur.
For spur gear (when P is not designated, or P0 is com- manded), the Q command will be ignored.
Address Meaning Command range (unit)
Remarks
C
Z
C
Z
P
P
P
P
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
793 IB-1501278-P
The rotation ratio and the number of hob threads can be changed without stopping the hob axis or the workpiece axis during tool spindle synchronization II (hobbing) mode.
(1) Each address can be omitted in the G114.3 command in the tool spindle synchronization II (hobbing) mode. If the address is omitted, modal value of the last command is used. (Example) When changing only the workpiece axis rotation ratio (the modal value of the previous command is used for items other than the workpiece axis rotation ratio.) G114.3 L50;
(2) If the followings are issued, a program error (P33) will occur. (a) When R command (workpiece axis phase shift amount) is issued. (b) When the hob axis number and workpiece axis number are changed (c) When other than "0" is commanded by E command in E=0 state, or "0" is commanded by E command in E0
state. (3) The workpiece axis rotation speed may be changed by rotation ratio. At this time, the acceleration/deceleration
time constant follows the hobbing workpiece axis time constant (parameter "#2195 hob_tL"). (4) "Spindle rotation speed synchronization completion" signal is turned OFF by changing the rotation ratio. This sig-
nal is turned ON when the workpiece axis rotation speed reaches the prescribed range for hob axis rotation speed after completing the rotation ratio change.
(5) The hob axis rotation speed cannot be changed while the rotation ratio is changed (during workpiece axis accel- eration/deceleration). If the rotation command is issued for hob axis during the rotation ratio change, the com- manded rotation speed is applied after completing the rotation ratio speed change.
(6) The helical gear machining by Z axis movement does not be executed while the rotation ratio is changed (during workpiece axis acceleration/deceleration). The helical gears machining is executed after completing the rotation ratio change.
(7) The phase of hob axis and workpiece axis during rotation ratio changing (during workpiece axis acceleration/ deceleration) or after changing is not warrantable. A phase cannot be aligned with gears machining of the last command.
(8) The "Hob axis delay (advance) monitoring", "Compensation control by workpiece axis" and "The workpiece axis feed forward control" are invalid while the rotation ratio is changed (during workpiece axis acceleration/deceler- ation). These functions are valid after finishing the rotation ratio change.
Detailed description
Rotation ratio change during tool spindle synchronization II (hobbing) mode
G114.3 E__ L__ P__ Q__ ; Rotation ratio change
E Hob axis rotation ratio designation L Workpiece axis rotation ratio designation P Gear torsion angle designation Q Module or diametral pitch designation
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
794IB-1501278-P
The rotation speed and rotation direction of the hob axis and workpiece axis during tool spindle synchronization II (hobbing) are as follows.
(1) The rotation speed and rotation direction of hob axis are the rotation speed commanded with the S command and the rotation direction commanded with the M command, etc., for the spindle selected as the hob axis.
directions of the machine coordinate system of the workpiece axis. (2) The workpiece axis rotation speed is determined by the hob threads specified using the hobbing mode command
and the number of gear teeth.
Sw : Workpiece axis rotation speed (r/min) Sh: Hob axis rotation speed (r/min) E: Hob axis rotation ratio (number of hob threads) L: Workpiece axis rotation ratio (number of gear teeth)
(3) The workpiece axis rotation direction is as follows. The workpiece axis rotation direction is determined by the sign of the workpiece axis selection "D" commanded with the hobbing mode command. In other words, when the "D" sign is "+", the workpiece axis will rotate in the same direction as the hob axis, and when the "D" sign is "-", the workpiece axis will rotate in the direction opposite to the hob axis.
(4) After tool spindle synchronization II (hobbing) was commanded, the relationship between the hob axis and work- piece axis rotation is held in all operation modes of automatic and manual modes until spindle synchronization cancel (G113.1) is commanded or until the "spindle synchronization cancel" signal is input. Even during reset or feed hold, the hob axis and workpiece axis synchronization state is held.
Rotation speed and rotation direction
When the sign of D command is + When the sign of D command is -
(a) Hob axis: Forward rotation (c) Workpiece axis: + direction (b) Hob axis: Reverse rotation (d) Workpiece axis: - direction
(a)
(c) (d)
(a)
(b)
(d) (c)
(b)
Sw = E LSh *
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
795 IB-1501278-P
(1) When the hobbing mode is commanded during hob axis rotation, the workpiece axis accelerates up to the speed required in synchronization with the hob axis according to the hobbing workpiece axis time constant (#2195 hob_tL) using the constant-gradient acceleration/deceleration control. Then rotates in synchronization with hob axis.
(2) The "axis selection" signal and in "axis motion" signal of the workpiece axis are not output during the tool spindle synchronization II (hobbing) mode.
(3) If a manual movement command is issued to the workpiece axis during the tool spindle synchronization II (hob- bing) mode, the manual movement will be superimposed on the workpiece axis movement with tool spindle syn- chronization. In this case, the "axis selection" signal and in "axis motion" signal of workpiece axis will be output. Note that, if the movement command is issued in the manual reference position return mode, an operation error (0005) occurs. An automatic movement command can be issued to the workpiece axis during the tool spindle synchronization II (hobbing) mode. Refer to "(2) Command compensation" in "Compensation control by workpiece axis" for de- tails of the command to the workpiece axis.
(4) During the tool spindle synchronization II (hobbing) mode, the operations in respect to the "input" signals of ex- ternal deceleration, interlock and machine lock for workpiece axis are as follows.
(5) If a "servo OFF" signal is input for the workpiece axis during the Tool spindle synchronization II (hobbing) mode, the tool spindle synchronization II (hobbing) is canceled because synchronization cannot be maintained.
(6) The workpiece axis rotation speed is determined according to the hob axis rotation speed, so designate the hob axis rotation speed so that the workpiece axis cutting clamp speed is not exceeded.
(7) The C axis counter on each screen will be updated as shown below during the tool spindle synchronization II (hobbing) mode. (a) When the workpiece axis is a rotary-type rotary axis
The axis will rotate in the 0.000 to 359.999 range in the normal manner.
(b) When the workpiece axis is a linear-type rotary axis (all coordinate values linear type) The axis will rotate in the 360 range including the machine coordinate position and workpiece coordinate position when hobbing starts.
(c) When the workpiece axis is a linear-type rotary axis (workpiece coordinate values linear type) The axis will rotate in the 360 range including the workpiece coordinate position when hobbing starts.
(Example)
(8) If the hobbing command is issued before the workpiece axis completes zero point return, a program error (P430) will occur.
(1) The hob axis will carry out multi-step acceleration/deceleration with the spindle synchronization acceleration/de- celeration time constant (spt) set for the spindle selected as the hob axis.
Workpiece axis control
Interlock Machine lock External de- celeration
Movement by the hobbing function Invalid Invalid Invalid Movement by manual command Valid for manual interlock Valid for manual machine
lock Valid
Automatic compensation by incre- mental command
Valid for automatic interlock Valid for automatic machine lock
Valid
Coordinate value when the hobbing starts Rotation range
125.000 750.500 -252.200
() () ()
0.000 to 359.999 720.000 to 1079.999 -360.000 to -0.001
() () ()
Acceleration/deceleration control
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
796IB-1501278-P
To carry out phase alignment during hobbing, the spindle encoder commanded to the hob axis must have a Z phase and satisfy the following conditions.
When the zero point of hob axis is not established by the hob axis rotation after turning the power ON or the spindle gear changeover, carry out phase alignment by following operations. (The zero point of the hob axis is established within the range of (a) - (b) in the figure.)
(1) When tool spindle synchronization II (with R command) is specified using the hobbing mode command , the ro- tary axis commanded as the workpiece axis will enter the spindle synchronization II (hobbing) control state.
(2) The hob axis will start rotation at the Z phase detection speed (parameter "#3109 zdetspd") set in the parameters with the first S command issued for the hob axis after the hobbing control state is entered. At this time, the workpiece axis will reach the rotation speed following the rotation ratio command for the hob axis and workpiece axis. If this command rotation speed is 0 (r/min), the hob axis will not start rotating, and instead will wait for the next S command.
(3) The hob axis and workpiece axis phases will be aligned in this state. (4) After the phases are aligned, the hob axis will accelerate/decelerate to the rotation speed commanded with the
S command. The workpiece axis will accelerate/decelerate to the rotation speed obtained based on the hob axis rotation speed allowing for the hob axis and workpiece axis rotation ratio, and will enter the synchronized state.
When the zero point of hob axis has already been established, the zero point of hob axis establishment is omitted. Thus, the process finishes fast compared with the case that the zero point of hob axis is not established.
(1) When tool spindle synchronization II (with R command) is specified using the hobbing mode command , the ro- tary axis commanded as the workpiece axis will enter the spindle synchronization II (hobbing) control state.
(2) The hob axis rotation speed follows the Z phase detection speed (parameter "#3109 zdetspd") set in the param- eters with the first S command issued for the hob axis after entering the hobbing control state. If this command rotation speed is 0 (r/min), the workpiece axis will not start rotating, and instead will wait for the next S command.
(3) Phase alignment is carried out when the hob axis is stopped and the workpiece axis is rotating. (4) After the phases are aligned, the hob axis will accelerate/decelerate to the rotation speed commanded with the
S command. The workpiece axis will accelerate/decelerate to the rotation speed obtained based on the hob axis rotation speed allowing for the hob axis and workpiece axis rotation ratio, and will enter the synchronized state.
Phase alignment control (Machine configuration that the phase alignment is possible)
Control system Gear ratio conditions
Semi-closed control Spindle side gear : Motor side gear = 1 : 1 Full-closed control Spindle end : Encoder end = 1 : 1 Control system Gear ratio conditions
Phase alignment control (Operation when the zero point of hob axis is not established)
Phase alignment control (Operation when the zero point of hob axis is established)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
797 IB-1501278-P
(1) Automatic compensation The workpiece axis is controlled while constantly allowing for hob axis delay (advance) caused by disturbance, etc. This is especially effective in increasing the workpiece accuracy during heavy cutting. Automatic compen- sation is validated with parameters. When the amount of the compensation added to the workpiece axis by hobbing conditions etc. changes greatly and rapidly, a servo alarm might occur for the workpiece axis. In that case, with the compensation amount through the primary delay filter, this enables the compensation amount fluctuation to further smoothen. However, the more widely the primary delay time constant is set, the more the effect of the compensation decreases, so the effect of the workpiece accuracy might not improve. [Spindle NC parameter] (Machine parameter)
#3130 syn_spec/bit0: Tool spindle synchronization II (hobbing) automatic compensation selection 0 (OFF): No compensation 1 (ON): Hob axis delay (advance) is compensated with workpiece axis.
#3134 sphtc: Tool spindle synchronization II (hobbing) automatic compensation primary delay time constant 0: Primary delay filter control invalid 1 to 32768: Primary delay filter time constant setting unit (ms)
(2) Command compensation Errors in the cutting workpiece shape caused by insufficient machine rigidity, etc., are compensated for with the workpiece axis command in the machining program. (a) Command the workpiece axis compensation amount as an incremental position. (b) Command the workpiece axis compensation amount direction in the workpiece axis rotation direction using
a "+" command, and in the direction opposite the workpiece axis rotation using a "-" command. (c) When the movement command is issued with an absolute position for the workpiece axis during the Tool spin-
dle synchronization II (hobbing) mode, a program error (P32) will occur.
A feedforward control can be issued for the hob axis and the workpiece axis during the tool spindle synchronization II (hobbing) mode.
(1) The hob axis feedforward control is controlled according to hob axis feedforward gain (parameter "#3135 sf- wd_g").
(2) The workpiece axis feedforward control is controlled according to hob axis feedforward gain (parameter "#3135 sfwd_g") for the workpiece axis rotation contents of the hob axis rotation. The feedforward control is controlled according to workpiece axis feedforward gain (#2155 hob_fwd_g) for the helical compensation of the Z axis movement.
The hobbing mode command and hobbing cancel mode command can be issued during hob axis rotation.
(1) When the hobbing mode command is issued during hob axis rotation, the rotary axis designated as workpiece axis accelerates up to the speed according to the hob and workpiece axes' rotation ratio command. This accel- eration follows the hobbing workpiece axis time constant (parameter "#2195 hob_tL") and uses the constant- gradient acceleration/deceleration control. If the setting of hobbing workpiece axis time constant is outside the setting range, set the maximum value in the range.
(2) After the workpiece axis finishes acceleration, phase alignment is carried out between hob and workpiece axes if the hobbing mode command contains R command.
(3) Synchronization is established after phase alignment is completed. (4) If the hobbing cancel mode command is issued during hob axis rotation, the workpiece axis decelerates and
stops. This deceleration follows the hobbing workpiece axis time constant (parameter "#2195 hob_tL"), and uses the constant-gradient acceleration/deceleration. If the setting of hobbing workpiece axis time constant is outside the setting range, set the maximum value in the range.
Compensation control by workpiece axis
Feedforward control during tool spindle synchronization II (hob machining) mode
Tool spindle synchronization II (hobbing) command during hob axis rotation
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
798IB-1501278-P
Operating retract during hobbing mode prevents a destruction of the work when hobbing is interrupted. When "Hob retract request" signal is input during hobbing mode, the control can retract the axis designated by pa- rameter. Retract operation can also be carried out when a program error or operation error occurs.
(1) The retract operation is carried out when "Hob retract request" signal (YCDE) is turned ON during hobbing mode. However, the retract operation is not performed while the "hob retract complete" signal is ON. Also, after the operation has been completed, the tool is separated from the workpiece by the retract amount in hobbing mode; therefore, hob cutting is not performed properly.
(2) Retract operation can also be carried out when a program error or operation error occurs during hobbing mode. Specify whether to enable or disable a retract by alarm with the parameter "#19406" (Hob retract ON at alarm). However, if the parameter "#19406" (Hob retract ON at alarm) is enabled, a retract by alarm is not carried out when the "hob alarm retract inhibit" signal (YCDF) is turned ON.
(3) Retract is carried out in automatic operation mode. But when it is in automatic mode, retract can also be per- formed when not in automatic operation. (The hob axis and workpiece axis do not stop.)
(4) After the retract operation is completed, automatic operation pause. When performing retract operation in automatic operation, retract operation can be interrupted by turning ON "Automatic operation pause" signal. But when performing retract in a mode other than automatic operation, retract will not be interrupted by turning ON "Automatic operation pause" signal. If the retract operation is interrupted by automatic operation pause or by switching the operation mode (automatic to manual), retract will not be resumed even when you activate automatically after the interruption. However, if a new retract factor occurs after automatic operation has been started, the retract operation is performed by the specified amount.
(5) No retract operation is performed during manual operation mode. (6) The movement amount in the retract operation is determined by either the parameter "#8219 Hob retract amt 1"
or "#8220 Hob retract amt 2", which is specified by the "hob retract amount selection" signal (YB20). If the retract amount of all axes are set to "0", retract operation and automatic operation pause are not carried out.
(7) The parameters "#8219 Hob retract amt 1" and "#8220 Hob retract amt 2" are handled as radius values. (8) Retract speed is set for each axis in the parameter "#8221 Hob retract speed". (9) The "In hob retract" signal (XCAE) is ON during the retract operation. This signal is turned ON by either a retract
triggered by an alarm or a retract triggered by the "hob retract request" signal. (10) When the retract operation is completed, "Hob retract complete" signal (XCAF) turns ON. This signal is turned
ON by either a retract triggered by an alarm or a retract triggered by the "hob retract request" signal. (11) When retract is performed, acceleration and deceleration are carried out based on the travel command's accel-
eration/deceleration mode. However, when the parameter "#19407 Hob ret ac/dc OFF" is set to "1", step-wise acceleration/deceleration is carried out. When the parameter "#19407 Hob ret ac/dc OFF" is set to "1", and retract speed is relatively fast, a servo alarm (excessive error etc.) may occur.
(12) Retract is not carried out for axes that are in movement. (13) If mirror image is set for the retract axis, mirror image will be reflected on the retract operation. Therefore, the
retract is carried out in the direction opposite to the setting. (14) Machine lock is enabled for the retract axis. (15) Automatic interlock is enabled for the retract axis. When not in automatic operation, automatic interlock is en-
abled for retract axis.
Retract during Hobbing Mode
"Hob retract request" signal (HOBRTR) or program error/operation error
Hob axis travel speed
Hob retract speed (#8220)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
799 IB-1501278-P
(16) Cutting feed override or rapid traverse override is not reflected on the retract axis. (17) External deceleration is enabled for the retract axis. (18) Dry run is disabled for the retract axis. (19) Pre-interpolation acceleration/deceleration is disabled for a retract axis. Acceleration/deceleration after interpo-
lation is applied instead. (20) Retract can be performed for an axis that is under synchronization control. Retraction for a master axis causes
the slave axis to move. (21) Retract can be performed for an axis that is under inclined axis control. In accordance with the inclined axis'
movement, the reference axis moves by the compensation amount.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
800IB-1501278-P
(1) The synchronous tapping spindle cannot be commanded as the hob spindle of tool spindle synchronization II (hobbing). The operation error (M01 1007) will occur, which causes automatic operation to pause.
(2) The synchronous tapping cannot be commanded using the hob axis in tool spindle synchronization II (hobbing). The operation error (M01 1139) will occur, which causes automatic operation to pause.
(1) The tool spindle synchronization II (hobbing) mode cannot be commanded during spindle synchronization I, spin- dle synchronization II, or tool spindle synchronization IA/IB (spindle-spindle, polygon) ON. An operation error (M01 1005) occurs.
(2) Spindle synchronization I, spindle synchronization II, or tool spindle synchronization IA/IB (spindle-spindle, poly- gon) cannot be commanded during tool spindle synchronization II (hobbing) mode. An operation error (M01 1005) occurs.
(1) Even if the "reset" signal is input, the tool spindle synchronization II (hobbing) maintains synchronization. How- ever, the synchronization is canceled at emergency stop.
(1) The arbitrary axis exchange command (G140), arbitrary axis exchange return command (G141) or reference axis arrange return command (G142) cannot be issued in the part system where the tool spindle synchronization II (hobbing) is being performed. A program error (P501) will occur. However, hobbing that uses the axis in arbitrary axis exchange mode is possible.
(2) The workpiece axis of tool spindle synchronization II (hobbing) cannot be commanded as the axis exchange tar- get. Doing so triggers the arbitrary axis exchange disable state.
(1) If door interlock I or door interlock II is turned ON during the tool spindle synchronization II (hobbing) mode, tool spindle synchronization II (hobbing) will be canceled because synchronization cannot be maintained.
Tool spindle synchronization II (hobbing) cannot be executed using the spindle-mode rotary axis as the hob axis. An operation error (M01 1024) will occur. However, tool spindle synchronization II (hobbing) can be executed using the spindle-mode rotary axis as the work- piece axis.
(1) The 3-dimensional coordinate conversion cannot be commanded in the part system for tool spindle synchroni- zation II (hobbing). A program error (P922) will occur.
(2) Tool spindle synchronization II (hobbing) cannot be commanded during 3-dimensional coordinate conversion. A program error (P921) will occur.
Relationship with other functions
Synchronous tapping cycle
Spindle synchronization I, Spindle synchronization II, Tool spindle synchronization IA/IB (spindle-spindle, polygon)
NC reset, Emergency Stop
Arbitrary axis exchange command (G140), arbitrary axis exchange return command (G141), reference axis arrange return command (G142)
Door interlock I / Door interlock II
Spindle-mode rotary axis control
3-dimensional coordinate conversion
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
801 IB-1501278-P
When tool spindle synchronization II (hobbing) is commanded while the high-speed high-accuracy control is valid or when high-speed high-accuracy control is commanded during tool spindle synchronization II (hobbing), high-speed high-accuracy control is temporarily canceled, and tool spindle synchronization II (hobbing) is executed preferential- ly.
(1) Tool spindle synchronization II (hobbing) is not available during tool center point control. A program error (P942) will occur.
(2) The tool center point control command can be issued during tool spindle synchronization II (hobbing).
(1) Tool spindle synchronization II (hobbing) is not available during execution of the inclined surface machining com- mand. A program error (P951) will occur.
(2) The inclined surface machining command cannot be issued during tool spindle synchronization II (hobbing). A program error (P952) will occur.
(1) When cutting helical gear, correct cutting feed will not be possible in the synchronous feed mode, so always cut in the asynchronous feed mode.
(2) To carry out phase alignment when machining a helical gear, phase alignment will not be carried out correctly if the Z axis is moving, so always carry out phase alignment control when the Z axis is stopped.
(3) The linear-type rotary axis for the absolute position system cannot be used as the hobbing workpiece axis. If used, the absolute position detection alarm (Z70 0002) will occur after the power was turned OFF and ON.
(4) If hobbing control is carried out using the linear-type rotary axis as the hob axis, the current value will be illegal when the hobbing is canceled. In this case, preset the counter after canceling hob machining.
(5) If the hob axis rotation ratio is set to "0", phase alignment will not be carried out. Even if the workpiece axis phase shift amount is commanded, it is ignored.
(6) When "Hob axis delay (advance) allowable angle" (parameter "#3133 spherr") is "0", "Hob axis delay excess" (X18B3) is not output.
(7) During acceleration/deceleration of hob axis, "Hob axis delay angle" (R6516) and "Maximum hob axis delay an- gle" (R6517) are not updated.
(8) When the maximum hob axis delay (advance) angle (R6516) exceeds the hob axis delay (advance) allowable angle (parameter "#3133 spherr"), CNC only outputs the "delay excess" signal (X18B3). For information about how to take an action, contact the MTB representative.
(9) G00 of G01 command for the workpiece axis from the machining program should be an incremental command. When an absolute command is issued, program error (P32) occurs.
(10) Always set the position loop gain of the hob axis and the workpiece axis to the same value. If different values are set, the machining accuracy is not warrantable.
(11) Do not command hobbing (tool spindle synchronization II) during synchronous control of the workpiece axis (C1 axis) and rear workpiece axis (C2 axis). When hobbing is commanded during synchronous control, rear work- piece axis (C2 axis) and workpiece axis (C1 axis) will not operate in synchronization (because this does not trig- ger an alarm), and this may twist the workpiece.
piece axis (C1 axis) can be carried out. (12) Command the hobbing mode with the workpiece axis stopped. When hobbing is commanded while the work-
piece axis is rotating, hobbing mode turns ON after the stop of the workpiece axis was confirmed.
High-speed High-accuracy Control
Tool center point control
Inclined surface machining command
Precautions and restrictions
Hob axis : #13003 SP003 , #13036 SP036/bit4 Workpiece axis (NC axis) : #2203 SV003 , #2204 SV004 , #2257 SV057 Workpiece axis (Spindle/C axis) : #13002 SP002 , #13035 SP035/bitC
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
802IB-1501278-P
18.4 Multiple Spindle Synchronization Set Control [C80]
By this function, multiple sets of spindle synchronization I control can be performed simultaneously. Spindle synchronization I cannot be combined with spindle synchronization II. This section describes spindle synchronization I.
[Ref] indicates "reference axis" or "reference spindle". [Sync] indicates "synchronized axis" or "synchronized spindle". This is also applied to spindle synchronization II.
(*1) The synchronized spindle of the 1st set overlaps with that of the 2nd set.
(*2) The reference spindle of the 1st set overlaps with the synchronized spindle of the 2nd set. Or the synchronized spindle of the 1st set overlaps with the reference spindle of the 2nd set.
(*3) The reference spindle or synchronized spindle of the 1st or 2nd set overlaps with the synchronous tap spindle.
(1) This function can be applied to a lathe system equipped with two or more spindles. (2) The validity of this function depends on the MTB specifications. (Parameter "#1440 multi_sp_syn")
If this function is invalid, multiple spindle synchronization commands cannot be issued. (If two or more spindle synchronization commands are issued, the operation error (M01 1005) occurs, which causes automatic opera- tion to pause.)
Function and purpose
List of available combinations
G114.1: Spindle synchronization I command G84: Synchronous tapping
Spindle synchronization command for the 2nd set
Spindle synchronization command for the 1st set
[Ref] [Sync] G114.1 S1 [Ref] - S2 [Sync]
G84 S1
G114.1 S3 S4 S1 S4 (*3) S3 S2 (*1) S2 S3 (*2) S3 S1 (*2) (*3)
G84 S1 (*3) (*3) S2 (*3) S3
Enabling conditions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
803 IB-1501278-P
For details about the command format to start each function, refer to the relevant function's section.
(1) Command to cancel all synchronization modes Cancels all the synchronized sets. The format varies depending on the MTB specifications (parameter "#1242 set14/bit6). [When "#1242 set14/bit6" = 0]
If one set of spindle synchronization is active, G113.1 (without D_ command) is able to cancel the spindle synchronization control. However, if two or more sets of Spindle synchronization are active, the command causes the operation error (M01 1135) to occur.
[When "#1242 set14/bit6" = 1]
If "G113.1 D0;" is commanded, a program error (P35) occurs.
(2) Spindle synchronization I cancel command
(*1) There are two types of spindle designation methods: Spindle number method and spindle name method. When any name (1 to 9) is set to the spindle name parameter "#3077 Sname" of all the spindles, the spindle name method takes effect. In other cases, the spindle number is used.
(*2) Spindle synchronization I can be canceled by the G113.1 D_ command regardless of whether the multiple spindle synchronization set control is valid or invalid.
Command format
Canceling Spindle Synchronization
G113.1 D0; Cancels all the currently executed spindle synchronization I commands.
G113.1 ;
G113.1 D_;
Address Meaning of address Command range Remarks
D Synchronization axis to be can- celed
Spindle No.: 1 to num- ber of spindles Spindle name: 1 to 9
If the command range is exceed- ed, the program error (P35) will occur. If you specify a non-existent
spindle, the program error (P35) occurs. If you specify a spindle that is not
under synchronization, the oper- ation error (M01 005) occurs. If there is no address D, the syn-
chronization status of all spindle synch sets is cancelled.
Specify the number or name of the spindle that serves as the syn- chronized spindle in the Spindle synchronization I. (*1)
Note
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
804IB-1501278-P
The function combination table in the operation example shows each function as follows.
G114.1: Spindle synchronization I command G84: Synchronous tap
(1) If there is no overlap among the spindles of each spindle synchronization set, the multiple synchronization sets can be controlled simultaneously. Example: Combinations when the commanded reference spindle or synchronized spindle is not included in other control sets
(2) If the reference spindle of one spindle synchronization set overlaps with that of another synchronization set, the operation error (M01 1005) occurs. Note, however, that the reference spindle in spindle synchronization mode can be commanded as that for spindle synchronization in another synchronization set. Example: Combinations when the reference spindle of the 2nd set is controlled as the reference spindle of an-
other set (When S1 is duplicated as the reference spindle)
(3) If the synchronized spindle to be controlled in each spindle synchronization set overlaps with that of another syn- chronization set, an operation error (M01 1005) occurs.
(4) If the reference spindle of one spindle synchronization set overlaps with the synchronized spindle of another syn- chronization set, the operation error (M01 1005) occurs.
Operation example
Spindle synchronization com- mand for the 2nd set
Spindle synchronization command for the 1st set
G114.1 (S1-S2)
G114.1 (S3-S4)
S1, S2, S3, S4: S command name C1, C3: Name of rotary axis
Spindle synchronization com- mand for the 2nd set
Spindle synchronization command for the 1st set
G114.1 (S1-S2)
G114.1 (S1-S3)
S1,S2,S3,S4: S command name C1, C3: Name of rotary axis
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
805 IB-1501278-P
[M800/M80]
Spindle synchronization II does not support the multiple spindle synchronization set control. Thus, output the PLC output signal of the 1st spindle regardless of whether the multiple spindle synchronization set control is valid or in- valid.
[C80]
(1) Multiple spindle synchronization set control can be used with spindle synchronization II. However, Spindle syn- chronous control I and II cannot be used simultaneously.
(2) For Spindle synchronous control II, if the parameter "#1440 multi_sp_syn" is set to "0", the synchronization is performed by using the setting value of the 1st spindle of the PLC interface. In this case, the values set to spin- dles other than the 1st spindle are not used.
In the following cases, the operation error will occur, which causes automatic operation to pause.
(1) A synchronous tapping spindle cannot be commanded as the reference spindle of Spindle synchronization I. (Operation error (M01 1007))
(2) A synchronous tapping spindle cannot be commanded as the synchronized spindle of Spindle synchronization I. (Operation error (M01 1007))
(3) You cannot command a synchronous tapping that uses the reference spindle of spindle synchronization I mode. (Operation error (M01 1139))
(4) You cannot command a synchronous tapping that uses the synchronized spindle of spindle synchronization I mode. (Operation error (M01 1139))
(1) If any of the following commands is issued to a spindle for which the cancel operation is being processed by the (G113.1) command or the spindle synchronization/superimposition cancel signal (SPSYC), the operation error (M01 1005) occurs. Spindle synchronization Note that the commanded spindle synchronization operation starts after the cancel process is completed.
(2) If the cancel command (G113.1D_) is issued to the spindle that is not under synchronous control, an operation error (M01 1005) occurs.
(3) If the "spindle synchronization/superimposition cancel" signal (SPSYC) turns ON for a spindle that is not under synchronization control, the control ignores the cancel signal.
(4) An axis that involves any travel cannot be put in the same block as the spindle synchronization cancel command (G113.1). Doing so causes a program error (P33) when the spindle synchronization cancel command is issued, which causes automatic operation to be paused.
Relationship with other functions
Spindle synchronization II
Synchronous tapping cycle
Precautions
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
18 Advanced Multi-Spindle Control Function
806IB-1501278-P
19
807 IB-1501278-P
Advanced Machining Control
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
808IB-1501278-P
19Advanced Machining Control 19.1 Tool Position Compensation; G43.7/G49
The position compensation of a turning tool is executed when turning is performed in a machine of machining center system. Use of the tool position compensation enables the three base axes (X, Y and Z axes) to be compensated from the tool base position (base point). To set the compensation amount of the three base axes, switch the tool compensation display type to tool compen- sation type III. The validity of this parameter depends on the MTB specifications (parameter "#1046 T-ofs disp type").
The tool position compensation function is valid for machining center compensation type II. This setting depends on the MTB specifications (parameter "#1037 cmdtyp").
The valid range of the compensation No. will differ according to the specifications (No. of compensation sets). If the commanded compensation No. exceeds the specification range, the program error (P170) will occur. The H address can be omitted. If omitted, the previously specified compensation No. is used.
(1) Do not omit the H address. If the H address is omitted, an unintended operation may be performed by the H address that is input using a command other than G43.7.
(2) Even if the H command is issued alone in a block, the compensation amount corresponding to the compensation No. does not become valid. The compensation amount designated by the previous command is applied contin- uously.
(3) If G43.7 is commanded with a type other than tool compensation type II of the machining center, the program error (P39) will occur.
Function and purpose
Command format
Tool position compensation start
G43.7 H__;
H Compensation No. (H0 cancels tool position compensation.)
Tool position compensation cancel
G49;
X(+)
Z(+)
Y(+)
Y axis tool compen- sation amount (base axis J)
X axis tool compensation amount (base axis I)
Z axis tool compensation amount (base axis K)
Base position (base point)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
809 IB-1501278-P
The tool position compensation function compensates the tool position for the axis specified in the parameter using the offset specified by the compensation No. The three base axes are determined by the following parameters.
#1026 base_I (Base axis I) #1027 base_J (Base axis J) #1028 base_K (Base axis K)
Detailed description
Three base axes
Differences between tool length compensation and tool position compensation
[Tool length compensation (G43/G44)] [Tool position compensation (G43.7)]
The H address is used to compensate only one axis.
The H address is used to compensate three axis directions.
Z
X
Z(+)
Y(+)
X(+)
Base position (Base point)
X axis direction compensation amount
Y axis direction compen- sation amountTool length compen-
sation amount
Z axis direction compensation amount
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
810IB-1501278-P
When G43.7 is commanded in the program, tool position compensation is enabled, and the axis moves using the coordinate position, which is obtained by adding the compensation amount specified by the compensation No. to the end point coordinates specified in the movement command of the block, as the end point. This process is executed regardless of the absolute command or incremental command. Then, the compensation amount is added to the end point coordinates specified in the program until tool position compensation is canceled with a G49 command. Even except when the power is turned ON, G49 mode is set after M02 and M30 have been executed or after reset- ting has been performed.
When no movement command is included in the same block as for G43.7 or G49, the operation depends on the MTB specifications
(parameter "#1247 set19/bit0" (Movement by tool length offset)). For details, refer to "Movement by tool length com- pensation".
(1) The compensation No. commanded in the same block as G43.7 will be valid for the following modals.
(2) When G43.7 is further commanded in G43.7 mode, the compensation is applied by the tool compensation amount commanded later.
(3) When the H command is issued alone in a block during G43.7 modal, the compensation amount in modal mode is applied continuously.
Start-up and cancel operations
For absolute command N1 G91 G28 X0 Y0 Z0 ; N2 G00 G90 ; N3 G43.7 X-20. Y0. Z-40. H01 ; N4 Z-80. N5 G01 X-50. F500 ;
For incremental command N1 G91 G28 X0 Y0 Z0 ; N2 G00 G91 ; N3 G43.7 X-20. Y0. Z-40. H01 ; N4 Z-40. N5 G01 X-30. F500 ;
Compensation No.
G43.7 Hh1 ; :
Used as the tool compensation amount of (lh1).
G49;
:
Tool length compensation is canceled.
G43.7; :
Used again as the tool compensation amount of (lh1).
G43.7 Hh1 ; :
Used as the tool compensation amount of (lh1).
G43.7 Hh2 ; :
Used as the tool compensation amount of (lh2).
G43.7 Hh1 ; :
Used as the tool compensation amount of (lh1).
G43.7 Hh2 ; :
Used as the tool compensation amount of (lh2).
Hh3 ; :
The compensation amount designated in (lh2) is applied continuously.
N3
N4
N5
R
Program path
Workpiece
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
811 IB-1501278-P
If the reference position return operation is performed, the tool length compensation amount is canceled when the reference position return is completed. However, for the manual high-speed reference position return, the axis can be returned to the coordinates that are shifted by the tool length compensation amount again when the axis is moved after it has reached the reference position, using the parameter. (Parameter "#8122 Keep G43 MDL M-REF")
(Example 1) Automatic reference position return operation
(Example 2) Manual dog-type reference position return operation (The same operation is also performed when "#8122" is set to "0" and manual high-speed reference position return is valid.)
(Example 3) When "#8122" is set to "1" and manual high-speed reference position return is valid:
The movement is commanded to the G53 machine coordinate system, the axis will move to the machine position when the tool compensation amount is canceled. If the movement command is issued first after G53, the axis returns to the coordinates that are shifted by the tool length compensation amount.
Tool compensation cancel at reference position return operation
Automatic reference po- sition return (G28/G30)
Manual reference position return
Dog type High-speed type
When the axis reached the reference position:
Cancel Cancel Cancel
When the axis moves af- ter the above:
Cancel Cancel #8122 = 0: Cancel #8122 = 1: Reactivates tool length compensation amount that is ap- plied before the axis reaches the reference position.
G43.7 Xx1 Zz1 Hh1 ; : G28 Xx2 Zz2 ; Canceled when reference position is reached. (Same as when G49 is command-
ed.) G01 Xx3 Zz3 Ff3 ; :
Performs the same operation as that in G49 mode.
G43.7 Xx1 Zz1 Hh1 ; : (Interrupted by manual dog-type reference po- sition return.)
Canceled when reference position is reached.
G01 Xx2 Zz2 Ff2 ; :
Performs the same operation as that in G49 mode.
G43.7 Xx1 Zz1 Hh1 ; : (Interrupted by manual high-speed reference position return.)
Canceled when reference position is reached.
G01 Xx2 Zz2 Ff2 ; :
The end point is set for the coordinates that are shifted by the compensation amount specified by compensation No. h1.
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
812IB-1501278-P
When there is no movement command in the same block as for the G43.7 or G49 command, whether the axis moves to the current position by the specified compensation amount when the G43.7 command block is executed is deter- mined depending on the MTB specifications (parameter "#1247 set19/bit0").
(1) For the G49 command, command it at a safe position where the tool does not interfere with the machine in con- sideration of the compensation canceling operation. When the parameter "#1247 set19/bit0" is set to "0", the axis moves to the position where the compensation was canceled even though there is no axis command in the G49 command block.
Movement by tool length compensation
G43.7/G49 Not move by the compensation amounts (#1247 set19/bit0 = 1)
Moves by the compensation amounts (#1247 set19/bit0 = 0)
Without move- ment commands
(*1) Not moved. (*2) Not moved. If tool position compensation is commanded alone in a block, the axis does not move, but the tool compensation amount is applied to the program position counter.
(*3) Movement by (+) compensation amount (*4) Movement by (-) compensation amount If the tool position compensation is command- ed alone in a block, the axis moves by the tool length compensation amount.
With movement commands
(*3) Movement by (+) compensation amount (*4) Movement by (-) compensation amount If the tool position compensation and axis movement command are issued in the same block, the axis moves to the end point that is obtained by adding the tool length compensation amount to the movement command.
G00 Xx Yy Zz ; G43.7 H1 ; (*1)
G49 ; (*2)
(*1)
(*2)
G00 Xx Yy Zz ; G43.7 H1 ; (*3)
G49 ; (*4)
(*3)
(*4)
G00 Xx Yy Zz ; G43.7 H1 X10.; (*3)
G49 X5. ; (*4)
(*3)
(*4)
Note
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
813 IB-1501278-P
Relationship with other functions
Relationship between tool position compensation command and G code function
Column A : Operation to be performed when the tool position compensation command (G43.7/G49) and an- other G command are issued to the same block
Column B : Operation to be performed when another command is issued in G43.7 mode Column C : Operation to be performed when G43.7 is commanded in non-G43.7 mode : Can be executed. - : The G43.7 command is ignored. P(xx) : The program error will occur.
Modal group
G code Function A B C
0/1 G04 Dwell P45 (*1) G05 High-speed high-accuracy II P33 G05.1 High-speed high-accuracy I P34 P34 G07 Hypothetical axis interpolation P33 G08 High-accuracy control P33 G10 Parameter input by program / Com-
pensation data input by program P45 (*1)
G11 Parameter input by program cancel - G12/G13 Circular cut P32 (H command
only)
G27 Reference position check P45 (*1) G28 Reference position return P45 (*1) (*5) G29 Start position return P45 (*1) G30 2nd to 4th reference position return P45 (*1) G30.1 - G30.6 Tool exchange position return - G37 Automatic tool length measurement P801 P801 G52 Local coordinate system setting P45 (*1) G53 Machine coordinate system selection P45 (*1) G53.1/G53.6 Tool axis direction control P953 G65 User macro simple call P231 (*1) G115/G116 Start point timing synchronization P32 G120.1/G121 Machining condition selection I P33 G122 Activate sub part system I P651, P32 (*2)
1 G02/G03 Circular interpolation P33 (*1) G2.3/G3.3 Exponential interpolation P33 G2.4/G3.4 3-dimensional circular interpolation P75 P75 P75 G06.2 NURBS interpolation P33 P32
7 G41.2/G42.2 3-dimensional tool radius compensa- tion (Tool's vertical-direction compen- sation)
P163 P162
8 G43 Tool length compensation (+) (*3) P801 P801 G43.1 Tool length compensation along the
tool axis ON (*3) P801 P930
G43.4/G43.5 Tool center point control (*3) P941 P942 G44 Tool length compensation (-) (*3) P801 P801 G49 Tool length compensation cancel (*3)
9 G73 - G76 G81 - G89
Fixed cycle for drilling P801 P801
14 G66 User macro modal call - (*4)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
814IB-1501278-P
(*1) When the parameter "#1241 set13" is set to "1", G43.7 is ignored.
(*2) If G122 or G144 is called before G43.7, the program error (P651) will occur. If it is called after G43.7, the pro- gram error (P32) will occur.
(*3) When "G43.7 G43 H1;" is commanded, the G43 commanded later is enabled.
(*4) Only the modal is updated.
(*5) If the reference position return (G28) is commanded during the G43.7 modal, the G43.7 modal is canceled when the return is completed.
When the compensation by tool position compensation command G43.7/ G49 is applied to the circular movement axis, compensation movement is superimposed with circular movement if the axis moves by the specified compen- sation amount in the circular command block.
16 G68 3-dimensional coordinate conversion mode ON
P923
G68.2/G68.3 Inclined surface machining command P954 19 G50.1 G command mirror image cancel P801
G51.1 G command mirror image ON P801 P801 P801 21 G7.1/G107 Cylindrical interpolation P33 P481
G12.1/G112 Polar coordinate interpolation ON P33 P481 G13.1/G113 Polar coordinate interpolation cancel P33
27 G54.4 Workpiece installation error compen- sation
P546 P546
Circular interpolation
Modal group
G code Function A B C
X
Z
Uncompensated path
Path compensated by tool position compensa- tion
Z axis tool compensation amount (Reference axis K)
Circular movement amount
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
815 IB-1501278-P
19.2 Tool Length Compensation Along the Tool Axis; G43.1/G49
(1) Changes in the tool length compensation in the tool axis direction and compensation amount The tool length can be compensated for in the tool axis direction even when the rotary axis rotates and the tool axis direction becomes other than the Z axis direction. By using this function, and setting the deviation between the tool length amount set in the program and the actual tool length as the compensation amount, a more flexible program can be created. This is especially valid for programs in which many axis movement commands are present.
The tool length compensation amount in the tool axis direction can be changed by rotating the manual pulse gen- erator when the tool length compensation amount in the tool axis direction is being changed during the tool length compensation in the tool axis direction mode.
(2) Machine configuration The compensation using the tool length compensation in the tool axis direction function is applied to the direction of the tool tip axis (rotary axis).
As for the axes that determine the compensation direction, a combination of the C axis (spindle) for Z axis rota- tion and the A axis for X axis rotation or B axis for Y axis rotation is designated using a parameter.
Function and purpose
Axis A or B Axis B or C Axis A or B
(d) Rotation center (e) Tool (f) Axis direction (compensation direction) (g) Workpiece
Y
Z
X
A B
C
A
B
C (d)
(e)
(f)
A/B
(g)
(d)
(e)
(f)
(g)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
816IB-1501278-P
(1) G43, G44 and G43.1 are in the same G code group. Therefore, it is not possible to designate more than one of these commands simultaneously for compensation. G49 is used to cancel the G43, G44 and G43.1 commands.
(2) If the G43.1 command is designated when the specification for the tool length compensation in the tool axis di- rection is not provided, the program error (P930) will occur.
(3) If reference position has not been completed for any of the X, Y, Z, A or B and C axes in the G43.1 block, the program error (P430) will occur. However, the error does not apply to the following cases. When mechanical axes have been selected
The error does not apply to the A, B and C axes. When "1" has been set for the "#2031 noref" zero point return parameter
The error does not apply to the axis for which "noref" is set to "1" because it is considered that the reference position return of the axis has already completed.
Command format
Tool length compensation along the tool axis ON
G43.1 X__ Y__ Z__ H__ ;
Tool length compensation cancel
G49 X__ Y__ Z__ ;
X, Y, Z Movement data H Tool length compensation No.
(If the compensation No. exceeds the specification range, a program error (P170) will occur.)
Detailed description
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
817 IB-1501278-P
(1) When the following conditions have been met, the handle movement amount is added to the tool length com- pensation amount in the tool axis direction by rotating the manual pulse generator. When the operation mode is MDI, memory or tape operation mode and the state is "during single block
stop", "during feed hold" or "during cutting feed movement". Note that compensation amount cannot be changed during error or warning.
During tool length compensation in the tool axis direction (G43.1). In the tool length compensation amount in the tool axis direction changing mode (YC92/1). In the tool handle feed & interruption mode (YC5E/1). The 3rd axis (tool axis) is selected for the handle selection axis.
(2) The change amount is canceled when the compensation No. is changed.
The coordinate value in the tool length compensation amount in the tool axis direction change mode operates in the same manner as that when the manual ABS is ON, regardless of manual ABS switch (YC28) or base axis specification parameter "#1061 intabs". If compensation amount is changed during continuous operation, single block stop, or feed hold, the compen-
sation amount will be effective immediately in the next block.
When changing compensation amount, the compensation amount corresponding to the actual compensation No. will be changed. However, when executing the NC reset or tool length compensation in the direction of tool axis cancel (G49), the compensation amount will be returned to the original.
Changing the amount of tool length compensation in the tool axis direction
(Example) When changing compensation amount during continuous operation.
(Example) When changing compensation amount during single block stop.
(a) Compensation amount before change (b) Changed compensation amount (c) Path after compensation (d) Program path (e) Single block stop
Note
(a)
(b)
(c)
(d)
(a)
(b) (c)
(d)
(b)
(e)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
818IB-1501278-P
The vectors representing the tool length compensation in the tool axis direction are as follows.
(1) When the A and C axes are set as the rotary axes: Vx = L * sin(A) * sin(C) Vy = -L * sin(A) * cos(C) Vz = L * cos(A)
(2) When the B and C axes are set as the rotary axes: Vx = L * sin(B) * cos(C) Vy = L * sin(B) * sin(C) Vz = L * cos(B)
Vx, Vy, Vz: Tool length compensation along the tool axis vectors for X, Y and Z axes L: Tool length compensation amount (1h) A, B, C: Rotation angle (machine coordinate position) of A, B and C axes
(3) Rotary axis angle command The value used for the angle of the rotary axis (tool tip axis) differs according to the type of rotary axis involved. When servo axes are used: The machine coordinate position is used for the rotation angles of the A, B and C axes.
When mechanical axes are used: Instead of the machine coordinate position of the axes, the values read out from the R registers (R2628 to R2631) are used for the rotation angles of the A, B and C axes.
Tool length compensation in the tool axis direction is cleared in the following cases.
(1) When manual reference position return is completed. (2) When reset 1, reset 2 or reset & rewind has been executed. (3) When the G49 command has been designated. (4) When the offset No. 0 command has been executed. (5) When NC reset has been executed with "1" set for the basic system parameter "#1151 rstint". (6) When the G53 command is designated while the compensation status is still established, the compensation is
temporarily canceled, and the tool moves to the machine position designated by G53.
Tool length compensation in the tool axis direction vector
(a) Path after tool length compensation in the tool axis direction (b) G43.1 command (c) Program path (d) G49 command
Compensation amount resetting
(c)
(d)
(a)
(b)
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
819 IB-1501278-P
Example of arc machining
Shown below is an example of a program for linear -> arc -> arc -> linear machining using the B and C rotary axes on the ZX plane.
Program example
Machining program N01 G91 G28 X0 Y0 Z0 ; Compensation amount H01
= 50 mm N02 G28 B0 C0 ; N03 G90 G54 G00 X400. Y0 ; N04 Z-150. ; N05 B90. ; B axis: 90 N06 G18 ; N07 G43.1 X250. H01 ; Tool length compensation in
the tool axis direction ON N08 G01 Z0 F200 ; N09 G02 X0 Z250. I-250. K0 B0 ; Top right arc, B axis: 0 N10 G02 X-250. Z0 I0 K-250. B-90. ; Bottom right arc, B axis: -90 N11 G01 Z-150. ; N12 G00 G49 X-400. ; Tool length compensation in
the tool axis direction OFF N13 G91 G28 B0 C0 ; N14 G28 X0 Y0 Z0 ; N15 M02 ;
Tool with no compensation
Program path
Path after compensation
N07
N08 N09 H01 = 50mm
N10
N11
N12
X
Z
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
820IB-1501278-P
(1) A program error (P931) will occur if 3-dimensional coordinate conversion is carried out during tool length com- pensation in the tool axis direction.
(2) A program error (P921) will occur if the tool length is compensated for in the tool axis direction during 3-dimen- sional coordinate conversion.
(3) A program error (P923) will occur if the tool length compensation in the tool axis direction is commanded in the same block as the 3-dimensional coordinate conversion.
(1) A program error (P931) will occur if a command from G27 to G30 is issued during tool length compensation in the tool axis direction.
(1) Reference position return of orthogonal axis Tool length compensation along the tool axis will be canceled, as well as the dog-type reference position return and the high-speed reference position return.
Relationship with other functions
Relationship with 3-dimensional coordinate conversion
Relationship with automatic reference position return
Relationship with manual reference position return
N1 G90 G00 G54 X0 Y0 Z0 ; Positioning to the workpiece origin
N2 G00 A45. ; Rotating the rotary axis by 45
N3 G43.1 H1 ; Tool length compensation along the tool axis ON
N4 G19 G03 Y-5.858 Z-14.142 J14.142 K-14.142 A90. ; Circular cutting
Manual dog-type reference position return (a)
N5 G00 Y0. ; N6 Z0. ; : :
N5 G00 Y0. ; Positioning to the position where tool length compen- sation along the tool axis was canceled.
N6 Z0. ; Positioning to the position where tool length compen- sation along the tool axis was canceled.
: :
N2
N3
N4
(a)
N1 45
Z
Y M
W
Z
Y M
W
N6
N5
M800/M80/E80/C80 Series Programming Manual (Machining Center System) (2/2)
19 Advanced Machining Control
821 IB-1501278-P
(2) Reference position return of rotary axis Tool length compensation along the tool axis will be canceled, as well as the dog-type reference position return and the high-speed reference position return.
If you want to find out how the C80 Series Mitsubishi Electric works, you can view and download the Mitsubishi Electric M800, M80, E80, C80 Programming Manual v2 on the Manualsnet website.
Yes, we have the Programming Manual for Mitsubishi Electric C80 Series as well as other Mitsubishi Electric manuals. All you need to do is to use our search bar and find the user manual that you are looking for.
The Programming Manual should include all the details that are needed to use a Mitsubishi Electric C80 Series. Full manuals and user guide PDFs can be downloaded from Manualsnet.com.
The best way to navigate the Mitsubishi Electric M800, M80, E80, C80 Programming Manual v2 is by checking the Table of Contents at the top of the page where available. This allows you to navigate a manual by jumping to the section you are looking for.
This Mitsubishi Electric M800, M80, E80, C80 Programming Manual v2 consists of sections like Table of Contents, to name a few. For easier navigation, use the Table of Contents in the upper left corner.
You can download Mitsubishi Electric M800, M80, E80, C80 Programming Manual v2 free of charge simply by clicking the “download” button in the upper right corner of any manuals page. This feature allows you to download any manual in a couple of seconds and is generally in PDF format. You can also save a manual for later by adding it to your saved documents in the user profile.
To be able to print Mitsubishi Electric M800, M80, E80, C80 Programming Manual v2, simply download the document to your computer. Once downloaded, open the PDF file and print the Mitsubishi Electric M800, M80, E80, C80 Programming Manual v2 as you would any other document. This can usually be achieved by clicking on “File” and then “Print” from the menu bar.