Mitsubishi C80 Machining Center System Programming Manual PDF

Introduction

This manual describes the information for programming on Mitsubishi Electric CNC. Improper handling can cause unexpected malfunctions. To use this device correctly, be sure to read this manual before use.

Supported models of this manual are as follows:

Abbreviations for model names used in this manual are as follows:

To safely use this CNC unit, thoroughly study the "Precautions for Safety" before use. Be sure to keep this manual on hand so that users can refer to it at any time. Also refer to the manuals on "Manual List" as necessary.

Notes on reading this manual

(1) The description concerning "signals" in this manual refers to information transmission between a machine and PLC or between CNC and PLC. The method on controlling the signals (ON/OFF) differs depending on the machine. Refer to the manual issued by the machine tool builder (MTB).

(2) 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 this manual. Confirm the specifications for your machine with the manual issued by the MTB.

Details described in this manual In this manual, the following abbreviations might be used.

L system: Lathe system M system: Machining center system MTB: Machine tool builder

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-081194ENG Outline of hardware such as part names, external dimensions,

installation, wiring, maintenance, etc. of GOTs

GOT2000 Series Users Manual (Utility)

SH-081195ENG Outline of utilities such as screen display setting, operation

method, etc. of GOTs

GOT2000 Series Users Manual (Monitor)

SH-081196ENG Outline of each monitor function of GOTs

GOT2000 Series Connection Manual (Mitsubishi Electric Products)

SH-081197ENG Outline of connection types and connection method between

GOT and Mitsubishi Electric connection devices

GT Designer3 (GOT2000) Screen Design Manual

SH-081220ENG 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-0800004 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 or registered trademarks of PROFIBUS User Organization.

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.

BiSS is a registered trademark of iC-Haus GmbH.

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 .................................................................................................................................... 84 6.11 Polar Coordinate Interpolation; G12.1, G13.1/G112, G113.................................................................................. 86 6.12 Exponential Interpolation; G02.3, G03.3............................................................................................................... 94 6.13 Polar Coordinate Command; G16 ...................................................................................................................... 101 6.14 Spiral/Conical Interpolation; G02.1/G03.1 (Type 1), G02/G03 (Type 2)............................................................. 108 6.15 3-dimensional Circular Interpolation; G02.4, G03.4............................................................................................ 112 6.16 NURBS Interpolation; G06.2............................................................................................................................... 118 6.17 Hypothetical Axis Interpolation; G07................................................................................................................... 124 6.18 Involute Interpolation; G02.2/G03.2.................................................................................................................... 126

7 Feed Functions......................................................................................................................................... 139 7.1 Rapid Traverse Rate............................................................................................................................................. 140

7.1.1 Rapid Traverse Rate .................................................................................................................................... 140 7.1.2 G00 Feedrate Command (,F Command) ..................................................................................................... 141

7.2 Cutting Feedrate ................................................................................................................................................... 145 7.3 F1-digit Feed......................................................................................................................................................... 146 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed); G94,G95 .............................. 148 7.5 Inverse Time Feed; G93 ....................................................................................................................................... 150 7.6 Feedrate Designation and Effects on Control Axes.............................................................................................. 155 7.7 Selection of Axis (Axes) for Feedrate Command; G130....................................................................................... 160 7.8 Rapid Traverse Constant-gradient Acceleration/Deceleration.............................................................................. 164 7.9 Rapid Traverse Constant-gradient Multi-step Acceleration/Deceleration ............................................................. 170 7.10 Cutting Feed Constant-gradient Acceleration/Deceleration................................................................................ 178 7.11 Exact Stop Check; G09 ...................................................................................................................................... 186 7.12 Exact Stop Check Mode; G61 ............................................................................................................................ 190 7.13 Deceleration Check ............................................................................................................................................ 191

7.13.1 Deceleration Check.................................................................................................................................... 191 7.13.2 Deceleration Check When Movement in the Opposite Direction Is Reversed ........................................... 199

7.14 Rapid Traverse Block Overlap; G0.5 P1............................................................................................................. 202 7.14.1 Rapid Traverse Block Overlap for G00; G0.5 ............................................................................................ 204 7.14.2 Rapid Traverse Block Overlap for G28 ...................................................................................................... 214

7.15 Automatic Corner Override ................................................................................................................................. 216 7.15.1 Automatic Corner Override ; G62............................................................................................................... 223 7.15.2 Inner Arc Override...................................................................................................................................... 224

7.16 Tapping Mode; G63 ............................................................................................................................................ 225 7.17 Cutting Mode; G64.............................................................................................................................................. 226

8 Dwell.......................................................................................................................................................... 227 8.1 Dwell (Time-based Designation); G04.................................................................................................................. 228

9 Miscellaneous Functions ........................................................................................................................ 231 9.1 Miscellaneous Functions (M8-Digits) .................................................................................................................... 232 9.2 2nd Miscellaneous Functions (A8-digits, B8-digits or C8-digits)........................................................................... 236 9.3 Index Table Indexing ............................................................................................................................................ 237

10 Spindle Functions .................................................................................................................................. 243 10.1 Spindle Functions ............................................................................................................................................... 244 10.2 Constant Surface Speed Control; G96, G97 ...................................................................................................... 245 10.3 Spindle Clamp Speed Setting; G92 .................................................................................................................... 252 10.4 Spindle Position Control (Spindle/C Axis Control) .............................................................................................. 254 10.5 Spindle Speed Fluctuation Detection; G162/G163 ............................................................................................. 263

11 Tool Functions (T command)................................................................................................................ 271 11.1 Tool Functions (T8-digit BCD) ............................................................................................................................ 272

12 Tool Compensation Functions ............................................................................................................. 273 12.1 Tool Compensation............................................................................................................................................. 274

12.1.1 Tool Compensation .................................................................................................................................... 274 12.1.2 Number of Tool Offset Sets Allocation to Part Systems............................................................................. 278

12.2 Tool Length Compensation/Cancel; G43, G44 / G49 ......................................................................................... 280 12.3 Tool Radius Compensation; G38,G39/G40/G41,G42 ........................................................................................ 287

12.3.1 Tool Radius Compensation Operation ....................................................................................................... 288 12.3.2 Other Commands and Operations during Tool Radius Compensation...................................................... 297 12.3.3 G41/G42 Commands and I, J, K Designation ............................................................................................ 307 12.3.4 Interrupts during Tool Radius Compensation............................................................................................. 313 12.3.5 General Precautions for Tool Radius Compensation................................................................................. 315 12.3.6 Changing of Compensation No. during Compensation Mode.................................................................... 316 12.3.7 Start of Tool Radius Compensation and Z Axis Cut in Operation .............................................................. 319 12.3.8 Interference Check..................................................................................................................................... 321 12.3.9 Diameter Designation of Compensation Amount ....................................................................................... 331 12.3.10 Workpiece Coordinate Changing during Radius Compensation.............................................................. 333

12.4 Tool Nose Radius Compensation (for Machining Center System) ..................................................................... 335 12.5 3-dimensional Tool Radius Compensation; G40/G41, G42................................................................................ 338 12.6 Tool Position Offset; G45 to G48........................................................................................................................ 350

13 Fixed Cycle ............................................................................................................................................. 359 13.1 Fixed Cycles ....................................................................................................................................................... 360

13.1.1 Drilling, Spot Drilling; G81 .......................................................................................................................... 364 13.1.2 Drilling, Counter Boring; G82 ..................................................................................................................... 365 13.1.3 Deep Hole Drilling Cycle; G83 ................................................................................................................... 366

13.1.3.1 Deep Hole Drilling Cycle ................................................................................................................... 366 13.1.3.2 Small Diameter Deep Hole Drilling Cycle.......................................................................................... 368

13.1.4 Tapping Cycle; G84 ................................................................................................................................... 371 13.1.5 Boring; G85................................................................................................................................................ 386 13.1.6 Boring; G86................................................................................................................................................ 387 13.1.7 Back Boring; G87....................................................................................................................................... 388 13.1.8 Boring; G88................................................................................................................................................ 392 13.1.9 Boring; G89................................................................................................................................................ 393 13.1.10 Stepping Cycle; G73 ................................................................................................................................ 394 13.1.11 Reverse Tapping Cycle; G74................................................................................................................... 396 13.1.12 Circular Cutting; G75................................................................................................................................ 398 13.1.13 Fine Boring; G76...................................................................................................................................... 400 13.1.14 Thread Milling Cycle; G187...................................................................................................................... 402 13.1.15 Punchtap Cycle ........................................................................................................................................ 406 13.1.16 Precautions for Using a Fixed Cycle ........................................................................................................ 419 13.1.17 Initial Point and R Point Level Return; G98, G99..................................................................................... 421 13.1.18 Setting of Workpiece Coordinates in Fixed Cycle Mode.......................................................................... 422 13.1.19 Drilling Cycle High-Speed Retract............................................................................................................ 423 13.1.20 Acceleration/Deceleration Mode Change in The Fixed Cycle for Drilling................................................. 427

13.2 Special Fixed Cycle ............................................................................................................................................ 429 13.2.1 Bolt Hole Cycle; G34.................................................................................................................................. 430 13.2.2 Line at Angle; G35 ..................................................................................................................................... 431 13.2.3 Arc; G36..................................................................................................................................................... 432 13.2.4 Grid; G37.1................................................................................................................................................. 433

13.3 Fixed Cycle for Turning Machining ..................................................................................................................... 435 13.3.1 Longitudinal Cutting Cycle; G174............................................................................................................... 436 13.3.2 Thread Cutting Cycle; G175....................................................................................................................... 439 13.3.3 Face Cutting Cycle; G176.......................................................................................................................... 443

14 Macro Functions .................................................................................................................................... 447 14.1 Subprogram Control; M98, M99, M198 .............................................................................................................. 448

14.1.1 Subprogram Call; M98, M99 ...................................................................................................................... 448 14.1.2 Subprogram Call; M198 ............................................................................................................................. 454 14.1.3 Figure Rotation; M98 I_J_K_ ..................................................................................................................... 455

14.2 Variable Commands ........................................................................................................................................... 458 14.3 User Macro ......................................................................................................................................................... 463 14.4 Macro Call Instructions ....................................................................................................................................... 464

14.4.1 Simple Macro Calls; G65 ........................................................................................................................... 464 14.4.2 Modal Call A (Movement Command Call) ; G66 ....................................................................................... 468 14.4.3 Modal Call B (for Each Block); G66.1 ........................................................................................................ 470 14.4.4 G Code Macro Call..................................................................................................................................... 472 14.4.5 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call) .................................................... 474 14.4.6 Detailed Description for Macro Call Instruction .......................................................................................... 476 14.4.7 Handling the Macro Call Command [C80].................................................................................................. 478 14.4.8 ASCII Code Macro ..................................................................................................................................... 482

14.5 Variables Used in User Macros .......................................................................................................................... 486 14.5.1 Common Variables..................................................................................................................................... 488 14.5.2 Local Variables (#1 to #33) ........................................................................................................................ 489 14.5.3 System Variables ....................................................................................................................................... 492

14.6 User Macro Commands...................................................................................................................................... 493 14.6.1 Operation Commands ................................................................................................................................ 493 14.6.2 Control Commands .................................................................................................................................... 498 14.6.3 External Output Commands; POPEN, PCLOS, DPRNT............................................................................ 504 14.6.4 Precautions ................................................................................................................................................ 508 14.6.5 Actual Examples of Using User Macros..................................................................................................... 510

14.7 Macro Interruption; M96, M97............................................................................................................................. 514

15 Program Support Functions ................................................................................................................. 525 15.1 Corner Chamfering I/Corner Rounding I ............................................................................................................. 526

15.1.1 Corner Chamfering I ; G01 X_ Y_ ,C ......................................................................................................... 526 15.1.2 Corner Rounding I ; G01 X_ Y_ ,R_........................................................................................................... 528 15.1.3 Corner Chamfering Expansion/Corner Rounding Expansion..................................................................... 530 15.1.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ..................................................... 532

15.2 Corner Chamfering II/Corner Rounding II ........................................................................................................... 533 15.2.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_....................................................................................... 533 15.2.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_ .......................................................................................... 535 15.2.3 Corner Chamfering Expansion/Corner Rounding Expansion..................................................................... 536 15.2.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ..................................................... 536

15.3 Linear Angle Command; G01 X_/Y_ A_/,A_....................................................................................................... 537 15.4 Geometric I; G01 A_ ........................................................................................................................................... 538 15.5 Geometric IB....................................................................................................................................................... 540

15.5.1 Geometric IB (Automatic Calculation of Contact Point of Two Circular Arcs); G02/G03 P_Q_ /R_........... 541 15.5.2 Geometric IB (Automatic Calculation of Intersection Point between Line And Circular Arc) ;

G01 A_ , G02/G03 P_Q_H_ ...................................................................................................................... 543 15.5.3 Geometric IB (Automatic Calculation of Contact Point between Line And Circular Arc) ;

G01 A_ , G02/G03 R_H_........................................................................................................................... 546 15.6 Mirror Image by G code ; G50.1,G51.1 .............................................................................................................. 548 15.7 Normal Line Control; G40.1/G41.1/G42.1 (G150/G151/G152)........................................................................... 552 15.8 Manual Arbitrary Reverse Run Prohibition ; G127.............................................................................................. 572 15.9 Data Input by Program........................................................................................................................................ 578

15.9.1 Parameter Input by Program; G10 L70, G11 ............................................................................................. 578 15.9.2 Compensation Data Input by Program (Tool Compensation Amount) ; G10 L10/L11/L12/L13, G11 ........ 580 15.9.3 Compensation Data Input by Program (Workpiece Offset Amount) ; G10 L2/L20, G11............................ 583 15.9.4 Compensation Data Input by Program (Turning Tool) ; G10 L12/L13, G11............................................... 587 15.9.5 Tool Shape Input by Program; G10 L100, G11.......................................................................................... 589 15.9.6 R-Navi Data Input by Program; G10 L110/L111, G11, G68.2, G69........................................................... 592

15.10 Tool Life Management ...................................................................................................................................... 596 15.10.1 Inputting the Tool Life Management Data by G10 L3 Command; G10 L3, G11 ...................................... 596 15.10.2 Inputting the Tool Life Management Data by G10 L30 Command; G10 L30, G11 .................................. 599 15.10.3 Precautions for Inputting the Tool Life Management Data....................................................................... 602 15.10.4 Allocation of the Number of Tool Life Management Sets to Part Systems .............................................. 603

15.11 Interactive Cycle Insertion; G180...................................................................................................................... 605 15.11.1 Interactive Cycle Insertion........................................................................................................................ 605 15.11.2 Interactive Macro...................................................................................................................................... 608

15.12 Axis Name Extension........................................................................................................................................ 609 15.13 Machining Interruption [C80]; G26.................................................................................................................... 615

16 Multi-part System Control ..................................................................................................................... 631 16.1 Timing Synchronization Operation...................................................................................................................... 632

16.1.1 Timing Synchronization Operation (! code) !n (!m ...) L ............................................................................. 632 16.1.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115 ...................................... 635 16.1.3 Timing Synchronization Operation with Start Point Designated (Type 2) ; G116 ...................................... 638 16.1.4 Timing Synchronization Operation Function Using M codes ; M*** ........................................................... 641 16.1.5 Timing Synchronization When Timing Synchronization Ignore Is Set........................................................ 645

16.2 Mixed Control...................................................................................................................................................... 648 16.2.1 Arbitrary Axis Exchange ; G140, G141, G142 ........................................................................................... 648

16.3 Sub Part System Control .................................................................................................................................... 651 16.3.1 Sub Part System Control I; G122.............................................................................................................. 651

16.4 Loader Control Part System ............................................................................................................................... 667

17 High-speed High-accuracy Control ...................................................................................................... 671 17.1 High-speed Machining Mode .............................................................................................................................. 672

17.1.1 High-speed Machining Mode I, II; G05 P1, G05 P2................................................................................... 672 17.2 High-accuracy Control ........................................................................................................................................ 681

17.2.1 High-accuracy Control ; G61.1, G08 .......................................................................................................... 681 17.2.2 SSS Control ............................................................................................................................................... 702 17.2.3 Tolerance Control....................................................................................................................................... 706 17.2.4 Variable-acceleration Pre-interpolation Acceleration/Deceleration ............................................................ 710 17.2.5 Initial High-accuracy Control ...................................................................................................................... 713 17.2.6 Multi-part System Simultaneous High-accuracy ........................................................................................ 714

17.3 High-speed High-accuracy Control ..................................................................................................................... 716 17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0.................. 716 17.3.2 Fairing ........................................................................................................................................................ 733 17.3.3 Smooth Fairing........................................................................................................................................... 734 17.3.4 Cutting Speed Clamp with Acceleration Rate Judgment ........................................................................... 743 17.3.5 High-speed Mode Corner Deceleration...................................................................................................... 744 17.3.6 Precautions on High-speed High-accuracy Control ................................................................................... 745

17.4 Spline Interpolation ; G05.1 Q2/Q0..................................................................................................................... 748 17.5 Spline Interpolation 2; G61.4 .............................................................................................................................. 756 17.6 High-accuracy Spline Interpolation ; G61.2 ........................................................................................................ 765 17.7 Machining Condition Selection I ; G120.1, G121................................................................................................ 767

18 Advanced Multi-Spindle Control Function .......................................................................................... 771 18.1 Spindle Synchronization ..................................................................................................................................... 772

18.1.1 Spindle Synchronization I; G114.1............................................................................................................. 773 18.1.2 Spindle Position Control (Spindle/C Axis Control) under Spindle Synchronization Control ....................... 785

18.2 Tool Spindle Synchronization I ........................................................................................................................... 790 18.2.1 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon) ; G114.2, G113.1 ........................................ 790 18.2.2 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon) ; G51.2/G50.2 or G251/G250 ..................... 796 18.2.3 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon) ; G51.2/G50.2 or G251/G250 .................... 801

18.3 Tool Spindle Synchronization II .......................................................................................................................... 805 18.3.1 Tool Spindle Synchronization II (Hobbing) ; G114.3/G113 ........................................................................ 805

18.4 Multiple Spindle Synchronization Set Control [C80] ........................................................................................... 818

19 Advanced Machining Control ............................................................................................................... 823 19.1 Tool Position Compensation; G43.7/G49 ........................................................................................................... 824 19.2 Tool Length Compensation Along the Tool Axis; G43.1/G49 ............................................................................. 831 19.3 Tool Center Point Control; G43.4, G43.5/G49.................................................................................................... 838

19.3.1 Circular Command in Tool Center Point Control (G43.4/G43.5)................................................................ 870 19.4 Inclined Surface Machining; G68.2, G68.3/G69 ................................................................................................. 874

19.4.1 How to Define Feature Coordinate System Using Euler Angles ................................................................ 876 19.4.2 How to Define Feature Coordinate System Using Roll-Pitch-Yaw Angles................................................. 878 19.4.3 How to Define Feature Coordinate System Using Three Points in a Plane ............................................... 880 19.4.4 How to Define Feature Coordinate System Using Two Vectors ................................................................ 882 19.4.5 How to Define Feature Coordinate System Using Projection Angles ........................................................ 884 19.4.6 Define by Selecting the Registered Machining Surface ............................................................................. 886 19.4.7 How to Define Feature Coordinate System Using Tool Axis Direction ...................................................... 887 19.4.8 Tool Axis Direction Control; G53.1/G53.6 .................................................................................................. 889 19.4.9 Details of Inclined Surface Machining Operation ....................................................................................... 897 19.4.10 Rotary Axis Basic Position Selection ....................................................................................................... 902 19.4.11 Relationship between Inclined Surface Machining and Other Functions ................................................. 908 19.4.12 Precautions for Inclined Surface Machining............................................................................................. 913

19.5 3-dimensional Tool Radius Compensation (Tool's Vertical-direction Compensation); G40/G41.2, G42.2......... 916 19.6 Workpiece Installation Error Compensation; G54.4............................................................................................ 927 19.7 Rotation Center Error Compensation (Precautions for Creating a Machining Program) .................................... 940 19.8 Applicable Machines........................................................................................................................................... 944

20 Coordinate System Setting Functions ................................................................................................. 947 20.1 Coordinate Words and Control Axes .................................................................................................................. 948 20.2 Types of Coordinate Systems............................................................................................................................. 949

20.2.1 Basic Machine, Workpiece and Local Coordinate Systems....................................................................... 949 20.2.2 Machine Zero Point and 2nd, 3rd, 4th Reference Position (Zero Point) .................................................... 950 20.2.3 Automatic Coordinate System Setting ....................................................................................................... 951 20.2.4 Coordinate System for Rotary Axis ............................................................................................................ 952

20.3 Basic Machine Coordinate System Selection; G53 ............................................................................................ 955 20.4 Coordinate System Setting; G92 ........................................................................................................................ 958 20.5 Local Coordinate System Setting; G52............................................................................................................... 960 20.6 Workpiece Coordinate System Selection and Extended Workpiece Coordinate System Selection;

G54 to G59, G54.1 ............................................................................................................................................. 964 20.7 Workpiece Coordinate System Preset; G92.1 .................................................................................................... 972 20.8 Workpiece Position Offset for Rotary Axis ; G54.2 ............................................................................................. 977 20.9 3-dimensional Coordinate Conversion; G68/G69 ............................................................................................... 989 20.10 Coordinate Rotation by Program; G68/G69.................................................................................................... 1007 20.11 Coordinate Rotation Input by Parameter; G10 I_ J_/K_ ................................................................................. 1016 20.12 Scaling; G50/G51 ........................................................................................................................................... 1033 20.13 Reference Position (Zero Point) Return; G28, G29 ........................................................................................ 1037

20.14 2nd, 3rd, and 4th Reference Position (Zero Point) Return ; G30.................................................................... 1041 20.15 Tool Change Position Return; G30.1 - G30.6................................................................................................. 1044 20.16 Reference Position Check; G27 ..................................................................................................................... 1047

21 Protection Function ............................................................................................................................. 1049 21.1 Stroke Check before Travel; G22/G23 ............................................................................................................. 1050

21.1.1 Stroke Check before Travel in Stored Stroke Limit Area ......................................................................... 1052 21.2 Enable Interfering Object Selection Data; G186............................................................................................... 1055

22 Measurement Support Functions ....................................................................................................... 1059 22.1 Automatic Tool Length Measurement; G37 ...................................................................................................... 1060 22.2 Skip Function; G31 ........................................................................................................................................... 1064 22.3 Multi-step Skip Function 1; G31.n, G04............................................................................................................ 1070 22.4 Multi-step Skip Function 2; G31 P .................................................................................................................... 1072 22.5 Speed Change Skip; G31 Fn............................................................................................................................ 1074 22.6 Torque Limitation Skip; G160 ........................................................................................................................... 1078 22.7 Programmable Current Limitation; G10 L14 ..................................................................................................... 1082

23 System Variables ................................................................................................................................. 1083 23.1 System Variables List ....................................................................................................................................... 1084 23.2 System Variables (G Command Modal) ........................................................................................................... 1086 23.3 System Variables (Non-G Command Modal) ................................................................................................... 1087 23.4 System Variables (Modal Information at Macro Interruption) ........................................................................... 1088 23.5 System Variables (Tool Information) ................................................................................................................ 1090 23.6 System Variables (Tool Compensation) ........................................................................................................... 1098 23.7 System Variables (Tool Life Management)....................................................................................................... 1099 23.8 System Variables (Workpiece Coordinate Offset) ............................................................................................ 1104 23.9 System Variables (Workpiece Position Offset Amount for Rotary Axis) ........................................................... 1105 23.10 System Variables (Extended Workpiece Coordinate Offset) .......................................................................... 1106 23.11 System Variables (External Workpiece Coordinate Offset) ............................................................................ 1107 23.12 System Variables (Position Information)......................................................................................................... 1108 23.13 System Variables (Alarm) ............................................................................................................................... 1112 23.14 System Variables (Message Display and Stop).............................................................................................. 1113 23.15 System Variables (Cumulative Time) ............................................................................................................. 1114 23.16 System Variables (Time Read Variables)....................................................................................................... 1115 23.17 System Variables (Machining Information) ..................................................................................................... 1117 23.18 System Variables (Reverse Run Information) ................................................................................................ 1118 23.19 System Variables (Number of Workpiece Machining Times) ......................................................................... 1118 23.20 System Variables (Mirror Image) .................................................................................................................... 1118 23.21 System Variables (Coordinate Rotation Parameter)....................................................................................... 1119 23.22 System Variables (Rotary Axis Configuration Parameter).............................................................................. 1120 23.23 System Variables (Normal Line Control Parameter)....................................................................................... 1121 23.24 System Variables (Parameter Reading) ......................................................................................................... 1122 23.25 System Variables (Workpiece Installation Error Compensation Amount)....................................................... 1126 23.26 System Variables (Macro Interface Input (PLC -> NC)).................................................................................. 1127 23.27 System Variables (Macro Interface Output (NC -> PLC))............................................................................... 1133 23.28 System Variables (R Device Access Variables) ............................................................................................. 1139 23.29 System Variables (PLC Data Reading) .......................................................................................................... 1145 23.30 System Variables (Interfering Object Selection) ............................................................................................. 1149 23.31 System Variables (ZR Device Access Variables) [C80] ................................................................................. 1152 23.32 System Variables (NC Data Reading/Writing with API Section and Sub-section Nos. Input/Output by Program) [M8] ... 1154

24 Appx.1: Fixed Cycles ........................................................................................................................... 1157

25 Appx.2: Command Value Range Lists ............................................................................................... 1163

1

1 IB-1501277-Q

Control Axes

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

1 Control Axes

2IB-1501277-Q

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-Q

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-Q

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-Q

Minimum Command Unit

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

2 Minimum Command Unit

6IB-1501277-Q

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-Q

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-Q

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-Q

Program Formats

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

3 Program Formats

10IB-1501277-Q

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-Q

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-Q

[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-Q

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-Q

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-Q

(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-Q

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-Q

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-Q

(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-Q

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-Q

(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-Q

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-Q

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-Q

* 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-Q

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-Q

(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-Q

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-Q

Pre-read Buffer

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

4 Pre-read Buffer

28IB-1501277-Q

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-Q

Position Commands

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

5 Position Commands

30IB-1501277-Q

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-Q

(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-Q

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-Q

(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-Q

(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-Q

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-Q

(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-Q

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-Q

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-Q

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-Q

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-Q

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-Q

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-Q

(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-Q

6

45 IB-1501277-Q

Interpolation Functions

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

6 Interpolation Functions

46IB-1501277-Q

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-Q

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-Q

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-Q

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-Q

(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-Q

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-Q

(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-Q

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-Q

(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-Q

(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-Q

(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-Q

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-Q

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-Q

(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-Q

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-Q

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-Q

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-Q

Thread cutting metric input

Thread cutting inch input

It is not possible to assign a lead where the feedrate as converted into feed per minute exceeds the max- 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-Q

(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 (1 and 2) 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) Whether dry run is valid or invalid for thread cutting depends on the MTB settings. (When the parameter "#1279 ext15/bit4" is "1", the dry run is invalid. However, when the "Spindle OFF mode" signal (YCD3) is ON, the dry run is valid regardless of the parameter setting, and depends on the "Dry run" signal (YC15).) When the dry run is valid, the feedrate based on the 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. However, when the thread cutting override is valid, only the spindle override can be changed.

(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) In the thread cutting command, the part systems wait for the single rotation synchronization signal of the rotary encoder before starting movement. When the thread cutting is commanded for one spindle from multiple part systems, each part system waits for the encoder single rotation synchronization signal before starting thread cutting; therefore, the timing synchroni- zation operation between part systems is not required.

(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-Q

(1) For multiple spindle control II, do not change the encoder selection signal during the thread cutting. If it is changed, the thread ridges will lose their shape because the tool cannot be fed at the correct feedrate.

(2) When the thread cutting is commanded while the following parameters are set, the thread cutting start timing change is valid. (This depends on the MTB specifications.)

"#13227 SP227 bitF-C" is "4". (The proximity switch signal detection is valid.) "#3025 enc-on" is "2". (The spindle encoder is serially connected.) "#3127 SPECSP/bit4" is "1". (The thread cutting start timing change is "Start thread cutting after receiving an

external signal".)

(3) During the following functions, the thread cutting start timing change is invalid. During the following functions, the thread cutting command starts thread cutting after waiting for the Z phase signal from the encoder.

Multi-part system simultaneous thread cutting cycle I (G76.1) Two-part system simultaneous thread cutting cycle II (G76.2) Spindle synchronization control I (G114.1) Spindle synchronization control II Guide bushing spindle synchronization Spindle superimposition control (G164)

(4) When the thread cutting start timing change is valid, do not use the thread recutting function. Even if the thread recutting function is used while the thread cutting start timing change is valid, the lead cannot be guaranteed.

Precautions

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-Q

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-Q

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-Q

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-Q

(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-Q

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. J-10. ; 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-Q

(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. "P" command range is 0 to 9999. 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-Q

(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-Q

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-Q

(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-Q

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-Q

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-Q

(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-Q

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-Q

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-Q

(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.)

(3) An arc is drawn on the developed surface of the cylinder in the circular interpolation, thus the calculation is per- formed with the C axis unit in millimeters (mm).

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.

Relationship with other functions

Circular interpolation

N1 G18 Z-5.C0.; Perform positioning at Z-5 mm, C0 degrees. (The parameter "#1029 aux_I" is "C".)

N2 G07.1 C100.; Start cylindrical interpolation mode of radius 100 mm.

N3 G02 Z-15. R5.; Perform circular interpolation of radius 5 mm to Z-15 mm.

[mm]

N3 block (circular interpolation of radius 5 mm)

Tool radius compensation/tool nose radius compensation

Miscellaneous functions

-(2 100)

-5

-5 0 Z

Z

C -15

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

6 Interpolation Functions

81 IB-1501277-Q

(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.

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

82IB-1501277-Q

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

83 IB-1501277-Q

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

84IB-1501277-Q

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

85 IB-1501277-Q

(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

86IB-1501277-Q

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

87 IB-1501277-Q

(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.

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).

#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

88IB-1501277-Q

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

89 IB-1501277-Q

(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

90IB-1501277-Q

(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.)

Operations vary depending on whether the synchronous feed during polar coordinate interpolation is valid or invalid.

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" is set to "0"):

Only the asynchronous feed is valid during the polar coordinate interpolation mode. If synchronous feed (G95) is commanded during polar coordinate interpolation, the program error (P481) occurs. The operation when the polar coordinate interpolation mode is started or canceled varies depending on the feed mode that is active before the polar coordinate interpolation mode is started.

(a) If the feed mode before start is the asynchronous feed (G94)

The previous feed mode (asynchronous feed) and F command feedrate are used when the polar coordinate

interpolation mode is started or canceled.

(b) If the feed mode before start is the synchronous feed (G95)

The asynchronous feed is forcibly set and the feedrate is canceled when the polar coordinate interpolation

mode is started.

Set the feedrate with an F command after the polar coordinate interpolation mode is started. The program

error (P62) occurs if the F command is not designated.

When the polar coordinate interpolation mode is canceled, the feed mode (synchronous feed) and feedrate

before polar coordinate interpolation start are restored.

(2) When the synchronous feed is valid ("#1293 ext29/bit0" is set to "1"):

Both the synchronous and asynchronous feed are valid during the polar coordinate interpolation mode. The feed mode and feedrate remain unchanged and take over the previous state when the polar coordinate in- terpolation mode is started or canceled.

Changes in the feed mode before and after polar coordinate interpolation mode

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 -> Program error

: G13.1 ;

Feed mode and F command before and after polar coordinate interpolation mode

#1293 ext29/bit0

Changes in feed mode and feedrate

Before start At start At cancel

0 Asynchronous feed Asynchronous feed Feedrate just before start

Asynchronous feed Feedrate just before cancel

Synchronous feed Asynchronous feed Feedrate is "0" (cancel)

Synchronous feed Feedrate before the polar coordi- nate interpolation is started

1 Asynchronous feed Asynchronous feed Feedrate just before start

Feed mode just before cancel Feedrate just before cancel

Synchronous feed Synchronous feed Feedrate just before start

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

6 Interpolation Functions

91 IB-1501277-Q

Hole drilling axis in the fixed cycle for drilling command during the polar coordinate interpolation is determined with

the linear axis parameter (# 1533).

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.

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)

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

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

6 Interpolation Functions

92IB-1501277-Q

[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).

(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

93 IB-1501277-Q

(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

94IB-1501277-Q

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

95 IB-1501277-Q

(*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

96IB-1501277-Q

(*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

97 IB-1501277-Q

[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

98IB-1501277-Q

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

99 IB-1501277-Q

(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

100IB-1501277-Q

(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

101 IB-1501277-Q

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

102IB-1501277-Q

(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

103 IB-1501277-Q

(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

104IB-1501277-Q

(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

105 IB-1501277-Q

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

106IB-1501277-Q

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

107 IB-1501277-Q

(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

108IB-1501277-Q

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

109 IB-1501277-Q

(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

110IB-1501277-Q

(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

111 IB-1501277-Q

(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

112IB-1501277-Q

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

113 IB-1501277-Q

(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

114IB-1501277-Q

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

115 IB-1501277-Q

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

116IB-1501277-Q

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

117 IB-1501277-Q

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

118IB-1501277-Q

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

119 IB-1501277-Q

(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

120IB-1501277-Q

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

121 IB-1501277-Q

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

122IB-1501277-Q

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

123 IB-1501277-Q

(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

124IB-1501277-Q

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

125 IB-1501277-Q

(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

126IB-1501277-Q

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

127 IB-1501277-Q

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

128IB-1501277-Q

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

129 IB-1501277-Q

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

130IB-1501277-Q

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

131 IB-1501277-Q

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

132IB-1501277-Q

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

133 IB-1501277-Q

[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

134IB-1501277-Q

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

135 IB-1501277-Q

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

136IB-1501277-Q

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

137 IB-1501277-Q

(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

138IB-1501277-Q

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

139 IB-1501277-Q

Feed Functions

M800/M80/E80/C80 Series Programming Manual (Machining Center System) (1/2)

7 Feed Functions

140IB-1501277-Q

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

141 IB-1501277-Q

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

142IB-1501277-Q

(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

143 IB-1501277-Q

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

144IB-1501277-Q

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

145 IB-1501277-Q

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

146IB-1501277-Q

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

147 IB-1501277-Q

(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

148IB-1501277-Q

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

149 IB-1501277-Q

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) Even in the machine lock status, the feedrate in feed per revolution follows the issued F command.

(5) Under dry run conditions, feed per minute applies and movement results at the manual feedrate (mm/min or inch/ min).

(6) The feed mode in the following cases follows the modal (G94/G95).

Tapping cycle (G84) Reverse tapping cycle (G74)

(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

150IB-1501277-Q

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

151 IB-1501277-Q

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

152IB-1501277-Q

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

153 IB-1501277-Q

(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

154IB-1501277-Q

(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

155 IB-1501277-Q

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

156IB-1501277-Q

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

157 IB-1501277-Q

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

158IB-1501277-Q

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

159 IB-1501277-Q

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

160IB-1501277-Q

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

161 IB-1501277-Q

(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

162IB-1501277-Q

(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

163 IB-1501277-Q

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

164IB-1501277-Q

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

165 IB-1501277-Q

[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

166IB-1501277-Q

(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

167 IB-1501277-Q

(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.

When "#2598" is "0", use "#2004".# When "#2599" is "0", use "#2005". The time constant switched by the "Rapid traverse time constant: Switchover request" signal is only the

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

168IB-1501277-Q

(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

169 IB-1501277-Q

(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

170IB-1501277-Q

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

171 IB-1501277-Q

(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

172IB-1501277-Q

(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

173 IB-1501277-Q

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

174IB-1501277-Q

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

175 IB-1501277-Q

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

176IB-1501277-Q

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

177 IB-1501277-Q

(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

178IB-1501277-Q

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

179 IB-1501277-Q

(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

180IB-1501277-Q

[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

181 IB-1501277-Q

[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

182IB-1501277-Q

[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

183 IB-1501277-Q

(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