Mitsubishi M700 Lathe System Programming Manual PDF

MELDAS is registered trademarks of Mitsubishi Electric Corporation. Other company and product names that appear in this manual are trademarks or registered trademarks of the respective companies.

Introduction This manual is a guide for using the MITSUBISHI CNC 700/70 Series. Programming is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study the "Precautions for Safety" on the following page to ensure safe use of this NC unit. Details described in this manual

CAUTION

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 option functions are added.

Refer to the specifications issued by the machine tool builder before starting 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 possible. Please confirm the specifications before use.

General precautions (1) Refer to the following documents for details on handling MITSUBISHI CNC 700/70 Series Instruction Manual ................................. IB-1500042

Precautions for Safety Always read the specifications issued by the machine tool builder, this manual, related manuals and attached documents before 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".

When the user may be subject to imminent fatalities or major injuries if handling is mistaken. When the user may be subject to fatalities or major injuries if handling is mistaken. When the user may be subject to injuries or when physical damage may occur if handling is mistaken.

Note that even items ranked as " CAUTION", may lead to major results depending on the situation. In any case, important information that must always be observed is described.

DANGER

Not applicable in this manual.

WARNING

Not applicable in this manual.

CAUTION

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 option functions are added. Refer to the specifications issued by the machine tool builder before starting 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 possible. Please confirm the specifications before use.

DANGER

WARNING

CAUTION

CAUTION

2. Items related to operation Before starting actual machining, always carry out dry run operation to confirm the machining program, tool offset amount and workpiece offset amount, 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 synchronous spindle rotation command OFF with one workpiece chucked by the basic spindle and synchronous spindle during the spindle synchronization. Failure to observe this may cause the synchronous spindle stop, and hazardous situation.

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.

CONTENTS

1. Control Axes ................................................................................................................................. 1 1.1 Coordinate Words and Control Axes ........................................................................................ 1 1.2 Coordinate Systems and Coordinate Zero Point Symbols ....................................................... 2

2. Least Command Increments........................................................................................................ 3 2.1 Input Setting Units .................................................................................................................... 3 2.2 Indexing Increment ................................................................................................................... 5

3. Data Formats................................................................................................................................. 6 3.1 Tape Codes .............................................................................................................................. 6 3.2 Program Formats...................................................................................................................... 9 3.3 Tape Memory Format ............................................................................................................. 12 3.4 Optional Block Skip ................................................................................................................ 12

3.4.1 Optional Block Skip; / ....................................................................................................... 12 3.4.2 Optional Block Skip Addition ; /n ...................................................................................... 13

3.5 Program/Sequence/Block Nos.; O, N ..................................................................................... 15 3.6 Parity H/V ............................................................................................................................... 16 3.7 G Code Lists........................................................................................................................... 17 3.8 Precautions before Starting Machining................................................................................... 23

4. Buffer Register............................................................................................................................ 24 4.1 Input Buffer ............................................................................................................................. 24 4.2 Pre-read Buffers ..................................................................................................................... 25

5. Position Commands ................................................................................................................... 26 5.1 Incremental/Absolute Value Commands ................................................................................ 26 5.2 Radius/Diameter Commands ................................................................................................. 27 5.3 Inch/Metric Conversion; G20, G21 ......................................................................................... 28 5.4 Decimal Point Input ................................................................................................................ 30

6. Interpolation Functions.............................................................................................................. 34 6.1 Positioning (Rapid Traverse); G00 ......................................................................................... 34 6.2 Linear Interpolation; G01 ........................................................................................................ 41 6.3 Circular Interpolation; G02, G03............................................................................................. 44 6.4 R Specification Circular Interpolation; G02, G03.................................................................... 49 6.5 Plane Selection; G17, G18, G19 ............................................................................................51 6.6 Thread Cutting........................................................................................................................ 53

6.6.1 Constant Lead Thread Cutting; G33 ................................................................................ 53 6.6.2 Inch Thread Cutting; G33................................................................................................. 58 6.6.3 Continuous Thread Cutting .............................................................................................. 60 6.6.4 Variable Lead Thread Cutting; G34.................................................................................. 61 6.6.5 Circular Thread Cutting; G35, G36................................................................................... 64

6.7 Helical Interpolation; G17, G18, G19, and G02, G03 ............................................................. 68 6.8 Milling Interpolation; G12.1..................................................................................................... 71

6.8.1 Selecting Milling Mode ..................................................................................................... 73 6.8.2 Milling Interpolation Control and Command Axes ............................................................ 74 6.8.3 Selecting a Plane during the Milling Mode ....................................................................... 76 6.8.4 Setting Milling Coordinate System ................................................................................... 78 6.8.5 Preparatory Functions ...................................................................................................... 80 6.8.6 Switching from Milling Mode to Turning Mode; G13.1...................................................... 85 6.8.7 Feed Function .................................................................................................................. 85 6.8.8 Program Support Functions ............................................................................................. 85 6.8.9 Miscellaneous Functions .................................................................................................. 86 6.8.10 Tool Offset Functions ..................................................................................................... 87 6.8.11 Interference Check....................................................................................................... 103

6.9 Cylindrical Interpolation; G07.1 (6 and 7 only in G code list)................................................ 111 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112, G113 (Only 6, 7 in G code list) ........ 119

6.11 Exponential Interpolation; G02.3, G03.3 ............................................................................ 126

7. Feed Functions ......................................................................................................................... 132 7.1 Rapid Traverse Rate ............................................................................................................ 132 7.2 Cutting Feed Rate ................................................................................................................ 132 7.3 F1-digit Feed ........................................................................................................................ 133 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed); G94, G95135 7.5 Feed Rate Designation and Effects on Control Axes ........................................................... 137 7.6 Thread Cutting Mode............................................................................................................ 141 7.7 Automatic Acceleration/Deceleration.................................................................................... 142 7.8 Rapid Traverse Constant Inclination Acceleration/Deceleration .......................................... 143 7.9 Speed Clamp........................................................................................................................ 145 7.10 Exact Stop Check; G09 ...................................................................................................... 146 7.11 Exact Stop Check Mode ; G61 ........................................................................................... 149 7.12 Deceleration Check ............................................................................................................ 150

7.12.1 G1 -> G0 Deceleration Check ...................................................................................... 152 7.12.2 G1 -> G1 Deceleration Check ...................................................................................... 153

7.13 Automatic Corner Override ; G62 ....................................................................................... 154 7.14 Tapping Mode ; G63........................................................................................................... 159 7.15 Cutting Mode ; G64 ............................................................................................................ 159

8. Dwell .......................................................................................................................................... 160 8.1 Per-second Dwell ; G04........................................................................................................ 160

9. Miscellaneous Functions ......................................................................................................... 162 9.1 Miscellaneous Functions (M8-digits BCD)............................................................................ 162 9.2 2nd Miscellaneous Functions (A8-digits, B8-digits or C8-digits) .......................................... 164 9.3 Index Table Indexing ............................................................................................................ 165

10. Spindle Functions................................................................................................................... 167 10.1 Spindle Functions (S2-digits BCD) ..... During Standard PLC Specifications..................... 167 10.2 Spindle Functions (S6-digits Analog) ................................................................................. 167 10.3 Spindle Functions (S8-digits).............................................................................................. 168 10.4 Constant Surface Speed Control; G96, G97 ...................................................................... 169 10.5 Spindle Clamp Speed Setting; G92.................................................................................... 170 10.6 Spindle/C Axis Control........................................................................................................ 171 10.7 Spindle Synchronization ..................................................................................................... 174

10.7.1 Spindle Synchronization Control I ................................................................................ 175 10.7.2 Spindle Synchronization II............................................................................................ 185 10.7.3 Precautions for Using Spindle Synchronization Control............................................... 190

10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon); G114.2 ............................... 192 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon);

G51.2 (Only 6 and 7 in G code list) .................................................................................... 200 10.10 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon);

G51.2 (Only 6 and 7 in G code list) .................................................................................... 208 10.11 Tool Spindle Synchronization II (Hobbing) ; G114.3 ........................................................ 211 10.12 Multiple-spindle Control .................................................................................................... 226

10.12.1 Multiple-spindle Control I (multiple spindle command)............................................... 227 10.12.2 Multiple-spindle Control I (spindle selection command) ............................................. 228 10.12.3 Multiple-spindle Control II........................................................................................... 231

11. Tool Functions ........................................................................................................................ 234 11.1 Tool Functions (T8-digits BCD) .......................................................................................... 234

12. Tool Offset Functions............................................................................................................. 235 12.1 Tool Offset .......................................................................................................................... 235

12.1.1 Tool Offset Start ........................................................................................................... 236 12.1.2 Expanded Method at Starting Tool Offset .................................................................... 238

12.2 Tool Length Offset .............................................................................................................. 240 12.3 Tool Nose Wear Offset ....................................................................................................... 242

12.4 Tool Nose Radius Compensation; G40, G41, G42, G46.................................................... 243 12.4.1 Tool Nose Point and Compensation Directions............................................................ 245 12.4.2 Tool Nose Radius Compensation Operations .............................................................. 249 12.4.3 Other Operations during Tool Nose Radius Compensation ......................................... 267 12.4.4 G41/G42 Commands and I, J, K Designation .............................................................. 275 12.4.5 Interrupts during Tool Nose Radius Compensation ..................................................... 280 12.4.6 General Precautions for Tool Nose Radius Compensation.......................................... 282 12.4.7 Interference Check....................................................................................................... 283

12.5 Compensation Data Input by Program; G10, G11.............................................................. 288 12.6 Tool Life Management II..................................................................................................... 291

12.6.1 Counting the Tool Life .................................................................................................. 294

13. Program Support Functions ..................................................................................................296 13.1 Fixed Cycles for Turning Machining ................................................................................... 296

13.1.1 Longitudinal Cutting Cycle; G77................................................................................... 297 13.1.2 Thread Cutting Cycle; G78........................................................................................... 299 13.1.3 Face Cutting Cycle; G79 .............................................................................................. 302

13.2 Fixed Cycle for Turning Machining (MITSUBISHI CNC special format) ............................. 305 13.3 Compound Type Fixed Cycle for Turning Machining ......................................................... 306

13.3.1 Longitudinal Rough Cutting Cycle; G71 ....................................................................... 307 13.3.2 Face Rough Cutting Cycle; G72................................................................................... 323 13.3.3 Formed Material Rough Cutting Cycle; G73 ................................................................ 325 13.3.4 Finishing Cycle; G70 .................................................................................................... 329 13.3.5 Face Cut-off Cycle; G74............................................................................................... 330 13.3.6 Longitudinal Cut-off Cycle; G75 ................................................................................... 332 13.3.7 Compound Thread Cutting Cycle; G76 ........................................................................ 334 13.3.8 Precautions for Compound Type Fixed Cycle for Turning Machining; G70 to G76 ..... 338

13.4 Compound Type Fixed Cycle for Turning Machining (MITSUBISHI CNC special format) . 341 13.5 Fixed Cycle for Drilling; G80 to G89 ................................................................................... 346

13.5.1 Face Deep Hole Drilling Cycle 1; G83 (Longitudinal deep hole drilling cycle 1; G87).. 354 13.5.2 Face Tapping Cycle; G84 (Longitudinal tapping cycle; G88)

/ Face Reverse Tapping Cycle; G84.1 (Longitudinal reverse tapping cycle; G88.1)...... 355 13.5.3 Face Boring Cycle; G85 (Longitudinal boring cycle; G89) ........................................... 359 13.5.4 Deep Hole Drilling Cycle 2; G83.2................................................................................ 359 13.5.5 Fixed Cycle for Drilling Cancel; G80 ............................................................................ 362 13.5.6 Precautions When Using a Fixed Cycle for Drilling...................................................... 362

13.6 Fixed Cycle for Drilling; G80 to G89 (MITSUBISHI CNC special format) ........................... 364 13.6.1 Initial Point and R Point Level Return; G98, G99 ......................................................... 383 13.6.2 Setting of Workpiece Coordinates in Fixed Cycle Mode .............................................. 384

13.7 Subprogram Control; M98, M99, M198 .............................................................................. 385 13.7.1 Calling Subprogram with M98 and M99 Commands.................................................... 385 13.7.2 Calling Subprogram with M198 Commands................................................................. 390

13.8 Variable Commands ........................................................................................................... 391 13.9 User Macro ......................................................................................................................... 396

13.9.1 User Macro Commands; G65, G66, G66.1, G67 ......................................................... 396 13.9.2 Macro Call Instruction................................................................................................... 397 13.9.3 ASCII Code Macro .......................................................................................................405 13.9.4 Variables ...................................................................................................................... 410 13.9.5 Types of Variables........................................................................................................ 412 13.9.6 Operation Commands .................................................................................................. 450 13.9.7 Control Commands ...................................................................................................... 456 13.9.8 External Output Commands ......................................................................................... 459 13.9.9 Precautions .................................................................................................................. 461

13.10 Mirror Image for Facing Tool Posts .................................................................................. 463 13.11 Corner Chamfering/Corner Rounding I............................................................................. 473

13.11.1 Corner Chamfering ",C_" (or "I_", "K_", "C_") ........................................................... 473 13.11.2 Corner Rounding ",R_" (or "R_") ................................................................................ 475

13.11.3 Corner Chamfering/Corner Rounding Expansion....................................................... 477 13.11.4 Interrupt during Corner Chamfering/Corner Rounding ............................................... 479

13.12 Corner Chamfering/Corner Rounding II............................................................................ 481 13.12.1 Corner Chamfering ",C_" (or "I_", "K_", "C_") ........................................................... 481 13.12.2 Corner Rounding ",R_" (or "R_") ................................................................................ 484 13.12.3 Corner Chamfering/Corner Rounding Expansion....................................................... 485 13.12.4 Interrupt during Corner Chamfering/Corner Rounding ............................................... 485

13.13 Linear Angle Command.................................................................................................... 486 13.14 Geometric ......................................................................................................................... 487

13.14.1 Geometric I................................................................................................................. 487 13.14.2 Geometric IB .............................................................................................................. 490

13.15 Parameter Input by Program; G10, G11........................................................................... 504 13.16 Macro Interruption ............................................................................................................ 506 13.17 Tool Change Position Return; G30.1 to G30.5................................................................. 514 13.18 Balance Cut; G15, G14 .................................................................................................... 517 13.19 Synchronizing Operation between Part Systems ............................................................. 521

13.19.1 Synchronization Standby Code (! code)..................................................................... 521 13.19.2 Start Point Designation Synchronizing (Type 1); G115.............................................. 524 13.19.3 Start Point Designation Synchronization (Type 2); G116........................................... 526 13.19.4 Synchronization Function Using M Codes ................................................................. 528

13.20 2-part System Synchronous Thread Cutting Cycle .......................................................... 531 13.20.1 Parameter Setting Command..................................................................................... 531 13.20.2 2-part System Synchronous Thread Cutting Cycle I; G76.1 ...................................... 532 13.20.3 2-part System Synchronous Thread Cutting Cycle II; G76.2 ..................................... 535

13.21 2-part System Simultaneous Thread-cutting Cycle (MELDAS special format)................. 539

14. Coordinate System Setting Functions.................................................................................. 541 14.1 Coordinate Words and Control Axes .................................................................................. 541 14.2 Basic Machine, Workpiece and Local Coordinate Systems ............................................... 542 14.3 Machine Zero Point and 2nd Reference Position (Zero point) ........................................... 543 14.4 Automatic Coordinate System Setting................................................................................ 544 14.5 Basic Machine Coordinate System Selection; G53 ............................................................ 545 14.6 Coordinate System Setting; G92 ........................................................................................ 546 14.7 Reference Position (Zero point) Return; G28, G29 ............................................................ 547 14.8 2nd, 3rd, and 4th Reference Position (Zero point) Return; G30......................................... 551 14.9 Reference Position Collation; G27 ..................................................................................... 554 14.10 Workpiece Coordinate System Setting and Offset; G54 to G59 (G54.1).......................... 555 14.11 Local Coordinate System Setting; G52 ............................................................................ 561 14.12 Workpiece Coordinate System Preset; G92.1.................................................................. 562 14.13 Coordinate System for Rotary Axis .................................................................................. 567

15. Protection Function................................................................................................................ 570 15.1 Chuck Barrier/Tailstock Barrier; G22, G23 ......................................................................... 570 15.2 Stored Stroke Limit ............................................................................................................. 575

16. Measurement Support Functions.......................................................................................... 577 16.1 Automatic Tool Length Measurement; G37........................................................................ 577 16.2 Skip Function; G31 ............................................................................................................. 581 16.3 Multiple-step Skip Function; G31.n, G04............................................................................ 587 16.4 Multiple-step Skip Function 2; G31..................................................................................... 589 16.5 Speed Change Skip............................................................................................................ 592 16.6 Programmable Current Limitation....................................................................................... 595

Appendix 1. Parameter Input by Program N No. Correspondence Table............................... 596 Appendix 2. Program Error......................................................................................................... 599 INDEX............................................................................................................................................. X-1

1. Control Axes 1.1 Coordinate Words and Control Axes

1

1. Control Axes 1.1 Coordinate Words and Control Axes

Function and purpose

In the case of a lathe, the axis parallel to the spindle is known as the Z axis and its forward direction is the direction in which the turret moves away from the spindle stock while the axis at right angles to the Z axis is the X axis and its forward direction is the direction in which it moves away from the Z axis, as shown in the figure below.

Spindle stock

Tailstock

Tool

Turret +X +Y

+Z

Coordinate axes and polarities

Since coordinates based on the right hand rule are used with a lathe, the forward direction of the Y axis in the above figure which is at right angles to the X-Z plane is downward. It should be borne in mind that an arc on the X-Z plane is expressed as clockwise or counterclockwise as seen from the forward direction of the Y axis. (Refer to the section on circular interpolation.)

G54

G52

G58

G55

G59

G30

G28 +X

(+Y)

+Z

Spindle nose

Machine zero point

Workpiece zero points (G54 to G59)

Local coordinate system (Valid in G54 to G59)

2nd reference position

Reference position

Relationship between coordinates

1. Control Axes 1.2 Coordinate Systems and Coordinate Zero Point Symbols

2

1.2 Coordinate Systems and Coordinate Zero Point Symbols

Function and purpose

: Reference position

: Machine coordinate origin

: Workpiece coordinate zero points (G54 to G59)

Upon completion of the reference position return, the parameters are referred to and automatically set for the basic machine coordinate system and workpiece coordinate systems (G54 to G59). The basic machine coordinate system is set so that the first reference position is at the position designated by the parameter from the basic machine coordinate zero point (machine zero point).

X1

X3

+X

+Z

Z1

X2 Z2

Hypothetical machine coordinate system (shifted by G92)

Workpiece coordinate system 1 (G54)

Workpiece coordinate system 2 (G55)

Workpiece coordinate system 5 (G58)

Workpiece coordinate system6 (G59) Z 3

1st reference position

Machine zero point Basic machine coordinate system

Local coordinate system (G52)

The local coordinate system (G52) is valid on the coordinate systems designated by the commands for the workpiece coordinate systems 1 to 6. Using the G92 command, the basic machine coordinate system can be shifted and made the hypothetical machine coordinate system. At the same time, workpiece coordinate systems 1 to 6 are also shifted.

2. Least Command Increments 2.1 Input Setting Units

3

2. Least Command Increments 2.1 Input Setting Units

Function and purpose

The input setting units are, as with the compensation amounts, the units of setting data used in common for all axes. The command units are the movement amounts in the program which are commanded with MDI inputs or command tape. These are expressed with mm, inch or degree () units. With the parameters, the command units are decided for each axis, and the input setting units are decided commonly for all axes.

Linear axis Parameters

Millimeter Inch Rotation axis

()

#1003 iunit = B 0.001 0.0001 0.001 = C 0.0001 0.00001 0.0001 = D 0.00001 0.000001 0.00001

Input setting unit

= E 0.000001 0.0000001 0.000001 #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

Command unit

= 10000 1.0 0.1 1.0

(Note 1) Inch/metric changeover is performed in either of 2 ways: conversion from the parameter screen (#1041 I_inch: valid only when the power is turned ON) and conversion using the G command (G20 or G21).

However, when a G command is used for the conversion, the conversion applies only to the input command increments 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 to correspond to inches or millimeters.

(Note 2) The millimeter and inch systems cannot be used together.

(Note 3) During circular interpolation on an axis where the input command increments are different, the center command (I, J, K) and the radius command (R) can be designated by the input setting units. (Use a decimal point to avoid confusion.)

2. Least Command Increments 2.1 Input Setting Units

4

Detailed description

(1) Units of various data

These input setting units determine the parameter setting unit, program command unit and the external interface unit for the PLC axis and handle pulse, etc. The following rules show how the unit of each data changes when the input setting unit is changed. This table applies to the NC axis and PLC axis.

Input setting unit Data Unit

system Setting value 1m (B) 0.1m (C) 10nm (D) 1nm (E)

20000 (mm/min) 20000 20000 20000 20000Milli- metre Setting range 1 to 999999 1 to 999999 1 to 999999 1 to 999999

2000 (inch/min) 20000 20000 20000 20000

Speed data Example: rapid Inch

Setting range 1 to 999999 1 to 999999 1 to 999999 1 to 999999 123.123 (mm) 123.123 123.1230 123.12300 123.123000Milli-

metre Setting range 99999.999 99999.9999 99999.99999 99999.999999 12.1234 (inch) 12.1234 12.12340 12.123400 12.1234000

Position data Example: SoftLimit+ Inch

Setting range 9999.9999 9999.99999 9999.999999 9999.9999999 1 (m) 2 20 200 2000Milli-

metre Setting range 9999 9999 9999 9999 0.0001 (inch) 2 20 200 2000

Interpolation unit data Inch

Setting range 9999 9999 9999 9999 (2) Program command

The program command unit follows the above table. If the data has a decimal point, the number of digits in the integer section will remain and the number of digits in the decimal point section will increase as the input setting unit becomes smaller. When setting data with no decimal point, and which is a position command, the data will be affected by the input setting increment and input command increment. For the feed rate, as the input setting unit becomes smaller, the number of digits in the integer section will remain the same, but the number of digits in the decimal point section will increase.

2. Least Command Increments 2.2 Indexing Increment

5

2.2 Indexing Increment

Function and purpose

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).

Detailed description

When the indexing increment (parameter) for limiting the command value is set, the rotary axis can be positioned 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, only command with the

2-degree increment are possible.

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)

The following axis specification parameters are used.

# Item Contents Setting range (unit)

2106 Index unit Indexing increment

Set the indexing increment to which the rotary axis can be positioned.

0 to 360 ( )

Precautions

When the indexing increment is set, degree increment positioning takes place. The indexing position is checked with the rotary axis, and is not checked with other axes. 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 "G91B5." is commanded.

3. Data Formats 3.1 Tape Codes

6

3. Data Formats 3.1 Tape Codes

Function and purpose

The tape command codes used for this controller are combinations of alphabet letters (A, B, C, ... Z), numbers (0, 1, 2, ... 9) and signs (+, -, /, ...). These alphabet letters, numbers and signs are referred to as characters. Each character is represented by a combination of 8 holes which may, or may not, be present. These combinations make up what is called codes. This controller uses the ISO code (R-840).

(Note 1) If a code not given in the "Table of tape codes" is assigned during operation, a program

error (P32) will result.

(Note 2) For the sake of convenience, a " ; " has been used in the CNC display to indicate the End of Block (EOB/LF) which separates one block from another. Do not use the " ; " key, however, in actual programming but use the keys in the following table instead.

CAUTION " ; " "EOB" and " % " "EOR" are explanatory notations. The actual code is "Line feed" and "%". (ISO code (R-840)

Detailed description

(1) Use the keys in the following table for programming.

EOB/EOR keys and displays Code used

Key used ISO Screen display

End of Block LF or NL ; End of Record % %

(2) Significant data section (label skip function)

All data up to the first EOB ( ; ), after the power has been turned ON or after operation has been reset, are ignored during automatic operation based on tape, memory loading operation or during a search operation. In other words, the significant data section of a tape extends from the character or number code after the initial EOB ( ; ) code after resetting to the point where the reset command is issued.

3. Data Formats 3.1 Tape Codes

7

(3) Control out, control in

When the ISO code is used, all data between control out "(" and control in ")" (or ";") are ignored, although these data appear on the setting and display unit. Consequently, the command tape name, No. and other such data not directly related to control can be inserted in this section. This information (except (B) in the "Table of tape codes") will also be loaded, however, during tape loading. The system is set to the "control in" mode when the power is turned ON.

L C S L F RG0 0 X - 8 5 0 0 0 Y - 6 4 0 0 0 ( CUT T ERPRE T URN ) F

Operator information print-out example

Information in this section is ignored and nothing is executed.

Example of ISO code

(4) EOR (%) code

Generally, the End of Record code is punched at both ends of the tape. It has the following functions: (a) Rewind stop when rewinding tape (with tape rewinder) (b) Rewind start during tape search (with tape rewinder) (c) Completion of loading during tape loading into memory

(5) Tape preparation for tape operation (with tape rewinder)

2m

10cm %

2m

10cm %; ;;;

Initial block Last block

..

If a tape rewinder is not used, there is no need for the 2-meter dummy at both ends of the tape and for the head EOR (%) code.

3. Data Formats 3.1 Tape Codes

8

ISO code (R-840) Feed holes

8 7 6 5 4 3 2 1 Channel No.

1 2

3 4

5 6

7 8

9 0

A B

C D

E F G H

I J K

L M N

O P

Q R S

T U V

W X Y Z

+ - .

, / %

LF (Line Feed) or NL ( (Control Out)

) (Control In) :

# * = [ ]

! $

SP (Space) CR(Carriage Return) BS (Back Space)

HT (Horizontal Tab) &

(Apostrophe) ;

< >

? @

DEL (Delete)

NULL DEL (Delete)

(A)

(B)

Under the ISO code, LF or NL is EOB and % is EOR. The (A) codes are stored on tape but an error results (except when they are used in the comment section) during operation. The (B) codes are non-working codes and are always ignored. (Parity V check is not executed.)

Table of tape codes

3. Data Formats 3.2 Program Formats

9

3.2 Program Formats

Function and purpose

The prescribed arrangement used when assigning control information to the controller is known as the program format, and the format used with this controller is called the "word address format".

Detailed description

(1) Word and address

A word is a collection of characters arranged in a specific sequence. This entity is used as the unit for processing data and for causing the machine to execute specific operations. Each word used for this controller consists of an alphabet letter and a number of several digits. (A + or - sign may be attached to the head of a number.)

Alphabet (address)

Word

Numerals

Word configuration

*

The alphabet letter at the head of the word is the address. It defines the meaning of the numerical information which follows it. For details of the types of words and the number of significant digits of words used for this controller, refer to "Format details".

(2) Blocks

A block is a collection of words. It includes the information which is required for the machine to execute specific operations. One block unit constitutes a complete command. The end of each block is marked with an EOB (End of Block) code.

(3) Programs

A program is a collection of several blocks.

3. Data Formats 3.2 Program Formats

10

Metric command Inch command Rotary axis

(Metric command) Rotary axis

(Inch command) Program No. 08 Sequence No. N6 Preparatory function G3/G21

0.001() mm/ 0.0001 inch X+53 Z+53 +53 X+44 Z+44 +44 X+53 Z+53 +53 X+53 Z+53 +53

0.0001() mm/ 0.00001 inch X+54 Z+54 +54 X+45 Z+45 +45 X+54 Z+54 +54 X+54 Z+54 +54

0.00001() mm/ 0.000001 inch X+55 Z+55 +55 X+46 Z+46 +46 X+55 Z+55 +55 X+55 Z+55 +55

Movement axis

0.000001() mm/ 0.0000001 inch X+56 Z+56 +56 X+47 Z+47 +47 X+56 Z+56 +56 X+56 Z+56 +56

0.001() mm/ 0.0001 inch I+53 K+53 R+53 I+44 K+44 R+44 I+53 K+53 R+53 I+44 K+44 R+44

(Note 5) 0.0001() mm/ 0.00001 inch I+54 K+54 R+54 I+45 K+45 R+45 I+54 K+54 R+54 I+45 K+45 R+45

(Note 5) 0.00001() mm/ 0.000001 inch I+55 K+55 R+55 I+46 K+46 R+46 I+55 K+55 R+55 I+46 K+46 R+46

(Note 5)

Arc and cutter radius

0.000001() mm/ 0.0000001 inch I+56 K+56 R+56 I+47 K+47 R+47 I+56 K+56 R+56 I+47 K+47 R+47

(Note 5) Dwell 0.001(sec.) X+53/P+8

0.001() mm/ 0.0001 inch

F62(Feed per minute) F44(Feed per revolution)

F53(Feed per minute) F26(Feed per revolution)

F63(Feed per minute) F43(Feed per revolution)

F44(Feed per minute) F34(Feed per revolution)

(Note 6)

0.0001() mm/ 0.00001 inch

F63(Feed per minute) F45(Feed per revolution)

F54(Feed per minute) F27(Feed per revolution)

F64(Feed per minute) F44(Feed per revolution)

F55(Feed per minute) F35(Feed per revolution)

(Note 6)

0.00001() mm/ 0.000001 inch

F64(Feed per minute) F46(Feed per revolution)

F55(Feed per minute) F28(Feed per revolution)

F65(Feed per minute) F45(Feed per revolution)

F56(Feed per minute) F36(Feed per revolution)

(Note 6)

Feed function

0.000001() mm/ 0.0000001 inch

F65(Feed per minute) F47(Feed per revolution)

F56(Feed per minute) F29(Feed per revolution)

F66(Feed per minute) F46(Feed per revolution)

F57(Feed per minute) F37(Feed per revolution)

(Note 6) Tool offset T1/T2 Miscellaneous function (M) M8 Spindle function (S) S8 Tool function (T) T8 2nd miscellaneous function A8/B8/C8 Subprogram P8 H5 L4

0.001() mm/ 0.0001 inch R+53 Q53 P8 L4

0.0001() mm/ 0.00001 inch R+54 Q54 P8 L4

0.00001() mm/ 0.000001 inch R+55 Q55 P8 L4

Fixed cycle

0.000001() mm/ 0.0000001 inch R+56 Q56 P8 L4

(Note 1) indicates the additional axis address, such as A, B or C.

(Note 2) The number of digits check for a word is carried out with the maximum number of digits of that address.

(Note 3) Numerals can be used without the leading zeros.

3. Data Formats 3.2 Program Formats

11

(Note 4) The meanings of the details are as follows :

Example 1 : 08 : 8-digit program No. Example 2 : G21 : Dimension G is 2 digits to the left of the decimal point, and 1 digit to the right. Example 3 : X+53 : Dimension X uses + or - sign and represents 5 digits to the left of the

decimal point and 3 digits to the right. For example, the case for when the X axis is positioned (G00) to the 45.123 mm position in the absolute value (G90) mode is as follows :

G00 X45.123 ; 3 digits below the decimal point 5 digits above the decimal point, so it's +00045, but the leading zeros and the mark (+) have been omitted. G0 is possible, too.

(Note 5) If an arc is commanded using a rotary axis and linear axis while inch commands are being used, the degrees will be converted into 0.1 inches for interpolation.

(Note 6) While inch commands are being used, the rotary axis speed will be in increments of 10 degrees. Example : With the F1. (Feed per minute) command, this will become the 10 degrees/minute

command.

(Note 7) The decimal places below the decimal point are ignored when a command, such as an S command, with an invalid decimal point has been assigned with a decimal point.

(Note 8) This format is the same for the value input from the memory, MDI or setting and display unit.

(Note 9) Command the program No. in an independent block. Command the program NO. in the head block of the program.

3. Data Formats 3.3 Tape Memory Format

12

3.3 Tape Memory Format

Function and purpose

(1) Storage tape and significant sections (ISO, EIA automatic judgment)

Both ISO and EIA tape codes can be stored in the memory in the same way as tape operation. After resetting, ISO/EIA is automatically judged by the EOB code at the head. The interval to be stored in the memory is from the next character after the head EOB to the EOR code after resetting. The significant codes listed in the "Table of tape code" in Section 3.1 "Tape codes", in the above significant section are actually stored into the memory. All other codes are ignored and are not stored. The data between control out "(" and control in ")" are stored into the memory.

3.4 Optional Block Skip 3.4.1 Optional Block Skip; /

Function and purpose

This function selectively ignores specific blocks in a machining program which starts with the "/" (slash) code.

Detailed description

(1) Provided that the optional block skip switch is ON, blocks starting with the "/" code 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 block are not to be executed for another workpiece, the same command tape can be used to machine different parts by inserting the "/" code at the head of those specific blocks.

Precautions for using optional block skip

(1) 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 G1 X25. /Z25. ; ..........NG (User macro, a division instruction;

a program error results.) /N20 G1 X25. Z25. ; ..........OK (2) Parity checks (H and V) are conducted regardless of the optional block skip switch position. (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 No. search. (5) All blocks with the "/" code are also input and output during tape storing and tape output,

regardless of the position of the optional block skip switch.

3. Data Formats 3.4 Optional Block Skip

13

3.4.2 Optional Block Skip Addition ; /n

Function and purpose

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.

Detailed description

The block with "/n" (slash) code is skipped when the "/n" is programmed to the head of the block and the optional block skip signal is turned ON. For the block with the "/n" code inside the block (not the head of block), the program is operated according to the value of the parameter "#1226 aux10/bit1" setting. When the optional block skip signal is OFF, the block with "/n" is executed.

Example of program

(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. N1 G54; N2 G90G81X50. Z-20. R3. F100; /5 N3 X30.; N4 X10.; N5 G80; M02;

Part 1 the optional block skip 5 signal ON

Part 2 the optional block skip 5 signal OFF

N4 N2 N2 N3 N4

3. Data Formats 3.4 Optional Block Skip

14

(2) When two or more "/n" codes are commanded to the head of the same block, the block is

ignored if either of the optional block skip signal corresponding to the command is ON.

N01 G90 Z3. M03 S1000; /1/2 N02 G00 X50.; /1/2 N03 G01 Z-20. F100; /1/2 N04 G00 Z3.; /1 /3 N05 G00 X30.; /1 /3 N06 G01 Z-20. F100; /1 /3 N07 G00 Z3.; /2/3 N08 G00 X10.; /2/3 N09 G01 Z-20. F100; /2/3 N10 G00 Z3.; N11 G28 X0 M05; N12 M02;

(a) Optional block skip 1 signal ON (Optional block skip 2, 3 signals OFF)

N01 -> N08 -> N09 -> N10 -> N11 -> N12 (b) Optional block skip 2 signal ON

(Optional block skip 1, 3 signals OFF) N01 -> N05 -> N06 -> N07 -> N11 -> N12 (c) Optional block skip 3 signal ON

(Optional block skip 1, 2 signals OFF) N01 -> N02 -> N03 -> N04 -> N11 -> N12

(3) When the parameter "#1226 aux10/bit1" is "1", when 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 signal corresponding to the command is ON.

N01 G91 G28 X0.Y0.Z0.;

N02 G01 F1000;

N03 X1. /1 Y1. /2 Z1.;

N04 M30;

(a) When the optional block skip 1 signal is ON and the optional block skip 2 signal is OFF, "Y1. Z1." is ignored

(b) When the optional block skip 1 signal is

OFF and the optional block skip 2 signal is ON, "Z1." is ignored.

3. Data Formats 3.5 Program/Sequence/Block Nos.; O, N

15

3.5 Program/Sequence/Block Nos.; O, N

Function and purpose

These Nos. are used for monitoring the execution of the machining programs and for calling both machining programs and specific stages in machining programs.

(1) Program Nos. are classified by workpiece correspondence or by subprogram units, and they are designated by the address "O" followed by a number with up to 8 digits.

(2) Sequence Nos. are attached where appropriate to command blocks which configure machining programs, and they are designated by the address "N" followed by a number with up to 6 digits.

(3) Block Nos. are automatically provided internally. They are preset to zero every time a program No. or sequence No. is read, and they are counted up one at a time unless program Nos. or sequence Nos. are commanded in blocks which are subsequently read. Consequently, all the blocks of the machining programs given in the table below can be determined without further consideration by combinations of program Nos., sequence Nos. and block Nos.

Monitor display Machining program

Program No. Sequence No. Block No. O12345678 (DEMO, PROG) ; 12345678 0 0 N100 G00 G90 X120. Z100. ; 12345678 100 0 G94 S1000 ; 12345678 100 1 N102 G71 P210 Q220 I0.2 K0.2 D0.5 F600 ; 12345678 102 0 N200 G94 S1200 F300 ; 12345678 200 0 N210 G01 X0 Z95. ; 12345678 210 0 G01 X20. ; 12345678 210 1 G03 X50. Z80. K15. ; 12345678 210 2 G01 Z55. ; 12345678 210 3 G02 X80. Z40. I15. ; 12345678 210 4 G01 X100. ; 12345678 210 5 G01 Z30. ; 12345678 210 6 G02 Z10. K15. ; 12345678 210 7 N220 G01 Z0 ; 12345678 220 0 N230 G00 X120. Z150. ; 12345678 230 0 N240 M02 ; 12345678 240 0 % 12345678 240 0

3. Data Formats 3.6 Parity H/V

16

3.6 Parity H/V

Function and purpose

Parity check provides a mean of checking whether the tape has been correctly perforated or not. This involves checking for perforated code errors or, in other words, for perforation errors. There are two types of parity check: Parity H and Parity V.

(1) Parity H

Parity H checks the number of holes configuring a character and it is done during tape operation, tape input and sequence No. search. A parity H error is caused in the following cases. (a) ISO code

When a code with an odd number of holes in a significant data section has been detected. (b) EIA code

When a code with an even number of holes in a significant data section has been detected.

(Example 1) Parity H error example (For ISO codes)

This character causes a parity H error.

When a parity H error occurs, the tape stops following the alarm code.

(2) Parity V A parity V check is done during tape operation, tape input and sequence No. search when the I/O PARA #9n15 (n is the unit No.1 to 5) parity V check function is set to "1". It is not done during memory mode. A parity V error occurs in the following case: when the number of codes from the first significant code to the EOB (;) in the significant data section in the vertical direction of the tape is an odd number, that is, when the number of characters in one block is odd. When a parity V error is detected, the tape stops at the code following the EOB (;).

(Note 1) Among the tape codes, there are codes which are counted as characters for parity

and codes which are not counted as such. For details, refer to the "Table of tape code" in Section 3.1 "Tape codes".

(Note 2) Any space codes which may appear within the section from the initial EOB code to the address code or "/" code are counted for parity V check.

3. Data Formats 3.7 G Code Lists

17

3.7 G Code Lists Function and purpose

G codes include the six G code lists 2, 3, 4, 5, 6 and 7. One list is selected by setting in parameter "#1037 cmdtyp".

cmdtyp G code list 3 List 2 4 List 3 5 List 4 6 List 5 7 List 6 8 List 7

G functions are explained using the G code list 3.

(Note 1) A program error (P34) will result if a G code that is not in the Table of G code lists is commanded.

(Note 2) An alarm will result if a G code without additional specifications is commanded.

Table of G code lists

G code list 2 3 4 5 6 7

Group Function Section

G00 G00 G00 G00 G00 G00 01 Positioning 6.1 G01 G01 G01 G01 G01 G01 01 Linear interpolation 6.2

G02 G02 G02 G02 G02 G02 01 Circular interpolation CW / Helical interpolation CW

6.3 6.4 6.7

G03 G03 G03 G03 G03 G03 01 Circular interpolation CCW / Helical interpolation CCW

6.3 6.4 6.7

G02.3 G02.3 G02.3 G02.3 G02.3 G02.3 01 Exponential interpolation CW 6.11 G03.3 G03.3 G03.3 G03.3 G03.3 G03.3 01 Exponential interpolation CCW 6.11 G04 G04 G04 G04 G04 G04 00 Dwell 8.1

G07.1 G107

G07.1 G107 19 Cylindrical interpolation 6.9

G09 G09 G09 G09 G09 G09 00 Exact stop check 7.10

G10 G10 G10 G10 G10 G10 00 Parameter/Compensation data input by program/ Tool life management data registration

12.5 13.15

G11 G11 G11 G11 G11 G11 00 Program parameter input / Tool life management data registration mode cancel

12.5 13.15

G12.1 G112

G12.1 G112 19 Polar coordinate interpolation ON 6.10

G13.1 G113

G13.1 G113 19 Polar coordinate interpolation cancel 6.10

G12.1 G12.1 G12.1 G12.1 19 Milling interpolation ON 6.8 *G13.1 *G13.1 *G13.1 *G13.1 19 Milling interpolation cancel 6.8 *G14 *G14 *G14 *G14 18 Balance cut OFF 13.18 G15 G15 G15 G15 18 Balance cut ON 13.18

3. Data Formats 3.7 G Code Lists

18

G code list 2 3 4 5 6 7

Group Function Section

G16 G16 G16 G16 02 Milling interpolation plane selection Y-Z cylindrical plane 6.8.3

G17 G17 G17 G17 G17 G17 02 Plane selection X-Y 6.5 G18 G18 G18 G18 G18 G18 02 Plane selection Z-X 6.5 G19 G19 G19 G19 G19 G19 02 Plane selection Y-Z 6.5 G20 G20 G20 G20 G20 G20 06 Inch command 5.3 G21 G21 G21 G21 G21 G21 06 Metric command 5.3 G22 G22 G22 G22 04 Barrier check ON 15.1 *G23 *G23 *G23 *G23 04 Barrier check OFF 15.1

G22 G22 00 Soft limit ON 15.2 G23 G23 00 Soft limit OFF 15.2

G27 G27 G27 G27 G27 G27 00 Reference position return check 14.9 G28 G28 G28 G28 G28 G28 00 Automatic reference position return 14.7 G29 G29 G29 G29 G29 G29 00 Return from reference position 14.7 G30 G30 G30 G30 G30 G30 00 2nd, 3rd and 4th reference position return 14.8

G30.1 G30.1 G30.1 G30.1 G30.1 G30.1 00 Tool change position return 1 13.17 G30.2 G30.2 G30.2 G30.2 00 Tool change position return 2 13.17 G30.3 G30.3 G30.3 G30.3 00 Tool change position return 3 13.17 G30.4 G30.4 G30.4 G30.4 00 Tool change position return 4 13.17 G30.5 G30.5 G30.5 G30.5 00 Tool change position return 5 13.17

G31 G31 G31 G31 G31 G31 00 Skip function/Multiple-step skip function 2 16.2

16.4 G31.1 G31.1 G31.1 G31.1 G31.1 G31.1 00 Multiple-step skip function 1-1 16.3 G31.2 G31.2 G31.2 G31.2 G31.2 G31.2 00 Multiple-step skip function 1-2 16.3 G31.3 G31.3 G31.3 G31.3 G31.3 G31.3 00 Multiple-step skip function 1-3 16.3

G32 G33 G32 G33 G32 G33 01 Thread cutting 6.6.1

6.6.2 G34 G34 G34 G34 G34 G34 01 Variable lead thread cutting 6.6.4 G35 G35 G35 G35 G35 G35 01 Circular thread cutting CW 6.6.5 G36 G36 G36 G36 G36 G36 01 Circular thread cutting CCW 6.6.5

G37 G37 G36/G37 G36/G37 G36/G37 G37.1 G37.2

G36/G37 G37.1 G37.2

00 Automatic tool length measurement 16.1

*G40 *G40 *G40 *G40 *G40 *G40 07 Tool nose R compensation cancel 12.4 G41 G41 G41 G41 G41 G41 07 Tool nose R compensation left 12.4 G42 G42 G42 G42 G42 G42 07 Tool nose R compensation right 12.4

G46 G46 G46 G46 G46 G46 07 Tool nose R compensation (direction automatically selected) ON 12.4

3. Data Formats 3.7 G Code Lists

19

G code list 2 3 4 5 6 7

Group Function Section

G43.1 G43.1 G43.1 G43.1 G43.1 G43.1 20 1st spindle control mode 10.12.2 G44.1 G44.1 G44.1 G44.1 G44.1 G44.1 20 Selected spindle control mode 10.12.2 G47.1 G47.1 G47.1 G47.1 G47.1 G47.1 20 All spindles simultaneous control mode 10.12.2

G50 G92 G50 G92 G50 G92 00 Spindle clamp speed setting Coordinate system setting

10.5 14.6

*G50.2 *G50.2 *G50.2 *G50.2 11 Scaling cancel G51.2 G51.2 G51.2 G51.2 11 Scaling ON

G50.2 G250

G50.2 G250 00 Polygon machining mode cancel

(spindle-tool axis synchronization) 10.9

G51.2 G251

G51.2 G251 00 Polygon machining mode ON

(spindle-tool axis synchronization) 10.9

G52 G52 G52 G52 G52 G52 00 Local coordinate system setting 14.11

G53 G53 G53 G53 G53 G53 00 Basic machine coordinate system selection 14.5

*G54 *G54 *G54 *G54 *G54 *G54 12 Workpiece coordinate system selection 1 14.10 G55 G55 G55 G55 G55 G55 12 Workpiece coordinate system selection 2 14.10 G56 G56 G56 G56 G56 G56 12 Workpiece coordinate system selection 3 14.10 G57 G57 G57 G57 G57 G57 12 Workpiece coordinate system selection 4 14.10 G58 G58 G58 G58 G58 G58 12 Workpiece coordinate system selection 5 14.10 G59 G59 G59 G59 G59 G59 12 Workpiece coordinate system selection 6 14.10

G54.1 G54.1 G54.1 G54.1 G54.1 G54.1 12 Workpiece coordinate system 48 sets expanded 14.10

G61 G61 G61 G61 G61 G61 13 Exact stop check mode 7.11

G62 G62 G62 G62 G62 G62 13 Automatic corner override 7.13 G63 G63 G63 G63 G63 G63 13/19 Tapping mode 7.14 *G64 *G64 *G64 *G64 *G64 *G64 13/19 Cutting mode 7.15 G65 G65 G65 G65 G65 G65 00 User macro call 13.9.1 G66 G66 G66 G66 G66 G66 14 User macro modal call A 13.9.1

G66.1 G66.1 G66.1 G66.1 G66.1 G66.1 14 User macro modal call B 13.9.1 *G67 *G67 *G67 *G67 *G67 *G67 14 User macro modal call cancel 13.9.1 G68 G68 G68 G68 15 Mirror image for facing tool posts ON 13.10 G69 G69 G69 G69 15 Mirror image for facing tool posts OFF 13.10

G68 G68 15 Mirror image for facing tool posts ON or balance cut mode ON 13.10

*G69 *G69 15 Mirror image for facing tool posts OFF or balance cut mode cancel 13.10

G70 G70 G70 G70 G70 G70 09 Finishing cycle 13.3.4 G71 G71 G71 G71 G71 G71 09 Longitudinal rough cutting cycle 13.3.1 G72 G72 G72 G72 G72 G72 09 Face rough cutting cycle 13.3.2 G73 G73 G73 G73 G73 G73 09 Formed material rough cutting cycle 13.3.3 G74 G74 G74 G74 G74 G74 09 Face cut-off cycle 13.3.5 G75 G75 G75 G75 G75 G75 09 Longitudinal cut-off cycle 13.3.6 G76 G76 G76 G76 G76 G76 09 Compound thread cutting cycle 13.3.7

3. Data Formats 3.7 G Code Lists

20

G code list 2 3 4 5 6 7

Group Function Section

G76.1 G76.1 G76.1 G76.1 G76.1 G76.1 09 2-part system synchronous thread-cutting cycle (1) 13.20.2

G76.2 G76.2 G76.2 G76.2 G76.2 G76.2 09 2-part system synchronous thread-cutting cycle (2) 13.20.3

G90 G77 G90 G77 G90 G77 09 Longitudinal cutting fixed cycle 13.1.1 G92 G78 G92 G78 G92 G78 09 Thread cutting fixed cycle 13.1.2 G94 G79 G94 G79 G94 G79 09 Face cutting fixed cycle 13.1.3

*G80 *G80 *G80 *G80 *G80 *G80 09 Fixed cycle for drilling cancel 13.5

13.5.5 13.6

G81 G81 G81 G81 G81 G81 09 Fixed cycle (drill/spot drilling) 13.6 G82 G82 G82 G82 G82 G82 09 Fixed cycle (drill/counter boring) 13.6 G79 G83.2 G79 G83.2 G79 G83.2 09 Deep hole drilling cycle 2 13.5.4

G83 G83 G83 G83 G83 G83 09 Deep hole drilling cycle (Z axis)/ Small-diameter deep-hole drilling cycle

13.5 13.5.1

G83.1 G83.1 G83.1 G83.1 G83.1 G83.1 09 Stepping cycle 13.6

G84 G84 G84 G84 G84 G84 09 Tapping cycle (Z axis) 13.5

13.5.2

G85 G85 G85 G85 G85 G85 09 Boring cycle (Z axis) 13.5

13.5.3

G87 G87 G87 G87 G87 G87 09 Deep hole drilling cycle (X axis) 13.5

13.5.1

G88 G88 G88 G88 G88 G88 09 Tapping cycle (X axis) 13.5

13.5.2

G89 G89 G89 G89 G89 G89 09 Boring cycle (X axis) 13.5

13.5.3 G84.1 G84.1 G84.1 G84.1 G84.1 G84.1 09 Reverse tapping cycle (Z axis) 13.5.2 G84.2 G84.2 G84.2 G84.2 G84.2 G84.2 09 Synchronous tapping cycle 13.6 G88.1 G88.1 G88.1 G88.1 G88.1 G88.1 09 Reverse tapping cycle (X axis) 13.5.2

G50.3 G92.1 G50.3 G92.1 G50.3 G92.1 00 Workpiece coordinate preset 14.12 G96 G96 G96 G96 G96 G96 17 Constant surface speed control ON 10.4 G97 G97 G97 G97 G97 G97 17 Constant surface speed control OFF 10.4 G98 G94 G98 G94 G98 G94 05 Feed per minute (Asynchronous feed) 7.4 G99 G95 G99 G95 G99 G95 05 Feed per revolution (Synchronous feed) 7.4

G90 G90 G90 03 Absolute value command 5.1 G91 G91 G91 03 Incremental value command 5.1

G98 G98 G98 10 Fixed cycle initial return 13.6

13.6.1 G99 G99 G99 10 Fixed cycle R point return 13.6.1

3. Data Formats 3.7 G Code Lists

21

G code list 2 3 4 5 6 7

Group Function Section

G113 G113 G113 G113 00 Spindle synchronization cancel Polygon machining (spindle-spindle synchronization) mode cancel

10.7 10.8

G114.1 G114.1 G114.1 G114.1 00 Spindle synchronization 10.7.1

G114.2 G114.2 G114.2 G114.2 00 Polygon machining (spindle-spindle synchronization) mode ON 10.8

G114.3 G114.3 G114.3 G114.3 00 Tool spindle synchronization II (Hobbing) 10.11

G115 G115 G115 G115 G115 G115 00 Start point designation synchronization Type 1 13.19.2

G116 G116 G116 G116 G116 G116 00 Start point designation synchronization Type 2 13.19.3

G117 G117 G117 G117 G117 G117 00 Miscellaneous function output during axis movement

(Note 1) A () symbol indicates the G code to be selected in each group when the power is turned ON or when a reset is executed to initialize the modal.

(Note 2) A () symbol indicates the G code for which parameters selection is possible as an initialization status when the power is turned ON or when a reset is executed to initialize the modal. Note that inch/metric changeover can only be selected when the power is turned ON.

(Note 3) A () symbol indicates a function dedicated for multi-part system. (Note 4) If two or more G codes from the same group are commanded, the last G code will be

valid. (Note 5) 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 machine tool builder.

(Note 6) Whether the modal is initialized differs for each reset input.

(1) "Reset 1" The modal is initialized when the reset initialization parameter (#1151 rstinit) is ON.

(2) "Reset 2 "and "Reset and Rewind" The modal is initialized when the signal is input.

(3) Reset at emergency stop release Conforms to "Reset 1".

(4) When an automatic reset is carried out at the start of individual functions, such as reference position return.

Conforms to "Reset and Rewind".

3. Data Formats 3.7 G Code Lists

22

(Note 7) Precautions for 6 and 7 in G code lists

(1) G68 and G69 When both the mirror image for facing tool posts option and balance cut option are valid,

G68 and G69 will be handled as the command to turn the mirror image for facing tool posts ON and OFF.

(The mirror image for facing tool posts has the priority.) (2) G36 G36 is used for the two functions, automatic tool length measurement and circular

thread cutting (CCW). The applied function follows the parameter "#1238 set10/bit0" (circular thread cutting) setting.

When "#1238 set10/bit0" is set to 0

G code Function G35 Circular thread cutting clockwise rotation (CW) G36 Automatic tool length measurement X G37 Automatic tool length measurement Z

When "#1238 set10/bit0" is set to 1

G code Function G35 Circular thread cutting clockwise rotation (CW) G36 Circular thread cutting counterclockwise rotation (CCW) G37 Automatic tool length measurement Z

CAUTION The commands with "no value after G" will be handled as "G00".

3. Data Formats 3.8 Precautions before Starting Machining

23

3.8 Precautions before Starting Machining

Precautions before 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 consider the machining conditions.

Before starting actual machining, always carry out dry run operation to confirm the machining program, tool offset amount and workpiece offset amount, etc.

4. Buffer Register 4.1 Input Buffer

24

4. Buffer Register 4.1 Input Buffer

Function and purpose

When the pre-read buffer is empty during a tape operation or RS-232C operation, the contents of the input buffer are immediately transferred to the pre-read buffers, and provided that the data stored in the input buffer do not exceed 250 4 characters, the following data (Max. 250 characters) are read and loaded into the input buffer. This buffer is designed to eliminate the operational delay originating in the readout time of the tape reader and to smooth out the block joints. The pre-reading effects are lost, however, when the block execution time is shorter than the tape readout time of the following block.

(Buffer size: 250 5 characters)

Input buffer

Memory

MDI data

Keyboard

Tape

Mode switching

Analysis processing Max. 5 execution blocks

Pre-read buffer 5

Buffer 4

Arithmetic processing

(Note) Data equivalent to 1 block are stored in 1 pre-read buffer.

Buffer 3 Buffer 2

Buffer 1

The input buffer has a memory capacity of 250 5 characters (including the EOB code).

(1) The contents of the input buffer register are updated in 250-character units.

(2) Only the significant codes in the significant data section are read into the input buffer.

(3) When codes (including "(" and ")") are sandwiched in the control in or control out mode and the optional block skip function is ON, the data extending from the "/" (slash) code up to the EOB code are read into the input buffer.

(4) The input buffer contents are cleared with resetting.

(Note 1) The input buffer size (250 characters) differs according to the model.

4. Buffer Register 4.2 Pre-read Buffers

25

4.2 Pre-read Buffers Function and purpose

During automatic processing, the contents of 1 block are normally pre-read so that program analysis processing is conducted smoothly. However, during nose R compensation, a maximum of 5 blocks are pre-read for the intersection point calculation including interference check. The specifications of the data in 1 block are as follows: (1) The data of 1 block are stored in this buffer.

(2) Only the significant codes in the significant data section are read into the pre-read buffer.

(3) When codes are sandwiched in the control in and control out, 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.

(4) The pre-read buffer contents are cleared with resetting.

(5) When the single block function is ON during continuous operation, the pre-read buffer stores the following block data and then stops operation.

Other precautions

(1) Depending on whether the program is executed continuously or by single blocks, the timing of

the valid/invalid for the external control signals for the optional block skip and others will differ.

(2) If the external control signal such as optional block skip is turned ON/OFF with the M command, the external control operation will not be effective on the program pre-read with the buffer register.

(3) According to the M command that operates the external controls, it prohibits pre-reading, and the recalculation is as follows:

The M command that commands the external controls is distinguished at the PLC, and the "recalculation request" for PLC NC interface table is turned ON.

(When the "recalculation request" is ON, the program that has been pre-read is reprocessed.)

5. Position Commands 5.1 Incremental/Absolute Value Commands

26

5. Position Commands 5.1 Incremental/Absolute Value Commands

Function and purpose

There are 2 methods of issuing tool movement amount commands: the incremental value method and the absolute value method. The incremental value method applies for coordinates of a point which is to be moved and it issues a command using the distance from the present point; on the other hand, the absolute value method issues a command using the distance from the coordinate zero point. The following figure shows what happens when the tool is moved from point P1 to point P2.

Workpiece coordinate zero point

Spindle

X axis

Z axis

Z W P1

P2

U 2

X

Incremental and absolute value commands

Incremental value commands and absolute value commands for the X axis and Z axis are identified by address when parameter "#1076 AbsInc" is set to 1, and identified by G code (G90/ G91) when set to 0. Similarly, even with additional axes (C axis or Y axis), they are differentiated by addresses, or G code.

Command method Remarks X axis Address X Z axis Address Z

Absolute value

C/Y axis Address C/Y X axis Address U Z axis Address W

Incremental value

C/Y axis Address H/V

Set correspondence between addresses and axes into "#1013 axname" and "#1014 incax".

Absolute and incremental values can be used together in the same block.

(Example)

X W ; Incremental value command for Z axis Absolute value command for X axis

(Note 1) When parameter "#1076 AbsInc" is 1, and H is used for the incremental command

address, address H of blocks in M98, G114.2, and G10 L50 modal will be handled as the parameter of each command, and the axis will not be moved.

5. Position Commands 5.2 Radius/Diameter Commands

27

5.2 Radius/Diameter Commands

Function and purpose

The cross sections of workpieces machined on a lathe are circular, and the diameter or radius value of those circles can be used for movement commands in the X-axis direction. A radius command will move the tool by the commanded amount only, but a diameter command will move the tool both in the X-axis direction by an amount equivalent to one-half the commanded amount only and in the Z-axis direction by the commanded amount only. This system permits radius or diameter commands to be issued, depending on the parameter (#1019 dia) setting. The figure below shows the command procedure when the tool is to be moved from point P1 to point P2.

Spindle

Workpiece coordinate zero point

P1

P2

r2

r1

X axis

Z axis

X command U command Remarks Radius Diameter Radius Diameter

X = r1 X = 2r1 U = r2 U = 2r2

Even when a diameter command has been selected, only the U command can be made a radius command by parameter "#1077 radius".

Radius and diameter commands

Precautions and Restrictions

(1) In the above example, the tool moves from P1 to P2 in the minus direction of the X axis and so

when an incremental value is issued, the minus sign is given to the numerical value being commanded.

(2) In this manual, diameter commands are used in descriptions of both the X and U axes for the sake of convenience.

5. Position Commands 5.3 Inch/Metric Conversion

28

5.3 Inch/Metric Conversion; G20, G21

Function and purpose

The commands can be changed between inch and metric with the G20/G21 command.

Command format

G20/G21; G20 Inch command G21 Metric command

Detailed description

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 and it is meaningless for rotation axes.

Output unit, command unit and setting unit

The counter or parameter setting and display unit is determined by parameter "#1041 I_inch". For the movement/speed command, the followings will be resulted: 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".

NC axis

Initial inch OFF (metric internal unit)

#1041 I_inch=0

Initial inch ON (inch internal unit)

#1041 I_inch=1 Item

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

PLC axis

Item #1042 pcinch=0 (metric)

#1042 pcinch=1 (inch)

Movement/ speed command Metric Inch

Counter display Metric Inch User parameter setting/display Metric Inch

5. Position Commands 5.3 Inch/Metric Conversion

29

Precautions

(1) The parameter and tool data will be input/output with the "#1041 I_inch" setting unit.

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 command modal.

(3) A program error (P33) will occur if G20/G21 command is issued in the same block as following G code. Command in a separate block. G7.1 (Cylindrical Interpolation) G12.1 (Polar coordinate interpolation)

5. Position Commands 5.4 Decimal Point Input

30

5.4 Decimal Point Input

Function and purpose

This function enables the decimal point to be input. It assigns the decimal point in millimeter or inch units for the machining program input information that defines the tool paths, distances and speeds. A parameter "#1078 Decpt2" selects whether minimum input command increment (type I) or zero point (type II) is to apply for the least significant digit of data without a decimal point.

Detailed description

(1) The decimal point command is valid for the distances, angles, times and speeds in machining

programs.

(2) Refer to the table rising the "Addresses used and valid/invalid decimal point commands" for details on the valid addresses for the decimal point commands.

(3) In decimal point command, the valid range of command value is as shown below (for input command increment cunit=10).

Movement command

(linear)

Movement command

(rotary) Feed rate Dwell

Input unit [mm]

-99999.999 to 99999.999

0. 001 to 10000000.000

Input unit [inch]

-9999.9999 to 9999.9999

-99999.999 to 99999.999 0. 0001 to

1000000.0000

0 to 99999.999

(4) The decimal point command is valid even for commands defining the variable data used in

subprograms.

(5) Decimal point commands for decimal point invalid addresses are processed as integer data only and everything below the decimal point is ignored. Addresses which are invalid for the decimal point are D, H, L, M, N, O, P, S and T. All variable commands, however, are treated as data with decimal points.

Precautions

(1) If an arithmetic operator is inserted, the data will be handled as data with a decimal point.

(Example1) G00 X123+0 ; This is the X axis command 123mm command. It will not be 123m.

5. Position Commands 5.4 Decimal Point Input

31

Example of program

(1) Example of program for decimal point valid address

Decimal point command 1 Specification division Program example When 1 = 1m When 1 = 10m

Decimal point command 2 When 1 = 1mm

G0 X123.45 (decimal points are all mm points)

X123.450mm X123.450mm X123.450mm

G0 X12345 X12.345mm (last digit is 1m unit)

X123.450mm X12345.000mm

#111 = 123, #112 = 5.55 X#111 Z#112

X123.000mm, Z5.550mm

X123.000mm, Z5.550mm

X123.000mm, Z5.550mm

#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

Decimal point input I, II and decimal point command validity

In the table on the next page, decimal point input I and II result in the following for commands in which a decimal point is not used in an address where a decimal point command is valid. Both decimal point input I and II become the same for commands using a decimal point.

(1) Decimal point input I

The lowest order digit of command data matches the command unit. (Example) When "X1" is commanded in 1m system, the same result occurs as for an

"X0.001" command.

(2) Decimal point input II The lowest order digit of command data matches the command unit. (Example) When "X1" is commanded in 1m system, the same result occurs as for an "X1."

command.

5. Position Commands 5.4 Decimal Point Input

32

Addresses used, validity of decimal point commands

Add- ress

Decimal point

command Application Re-

marks

Valid Coordinate position data Invalid 2nd miscellaneous function

code

Valid Angle data Invalid MRC program No. Invalid Parameter input by

program, axis No.

Valid Deep hole drilling cycle (2) Safety distance

A

Valid Spindle synchronous acceleration/deceleration time constant

Valid Coordinate position data B Invalid 2nd miscellaneous function

code

Valid Coordinate position data Invalid 2nd miscellaneous function

code

Valid Corner chamfering amount ,C Valid Program tool offset input

Nose R compensation amount (incremental)

C

Valid Chamfering width (slitting cycle)

Valid Automatic tool length measurement, deceleration range d

Invalid Parameter input by program, byte type data

D

Invalid Synchronous spindle No. at spindle synchronization

Valid Inch threads Precision thread lead

E

Valid Corner cutting feed rate

Valid Feed rate F Valid Thread lead

G Valid Preparatory function code Valid Coordinate position data

Invalid Sequence Nos. in subprograms

Invalid Parameter input by program, bit type data

Invalid Selection of linear - arc intersection (geometric)

H

Invalid Basic spindle No. at spindle synchronization

Valid Circular center coordinates Valid Nose R compensation/ tool

radius compensation vector components

Valid Deep hole drilling (2) First cut amount

I

Valid G0/G1 in-position width Hole drilling cycle G0 in-position width

,I

(Note 1) Decimal points are all valid in user macro arguments.

Add- ress

Decimal point

command Application Re-

marks

Valid Circular center coordinates Valid Nose R compensation/ tool

radius compensation vector components

Invalid Deep hole drilling (2) Dwell at return point

J

Invalid Hole drilling cycle G1 in-position width

,J

Valid Circular center coordinates Valid Nose R compensation/tool

radius compensation vector components

Invalid Hole machining cycle Number of repetitions

Valid Deep hole drilling cycle (2) Second and subsequent cut amounts

K

Valid Thread lead increase/ decrease amount (variable lead thread cutting)

Invalid Subprogram Number of repetitions

Invalid Program tool compensation input type selection

L2 L10 L11

Invalid Parameter input by program, selection

L70

Invalid Parameter input by program, two-word type data

4 bytes

Invalid Synchronization

L

Invalid Tool life data M Invalid Miscellaneous function

codes

Invalid Sequence Nos. N Invalid Parameter input by program,

data No.

O Invalid Program Nos. Invalid Dwell time Invalid Subprogram call program

Nos.

Invalid 2nd, 3rd and 4th reference position No.

Invalid Constant surface speed control, axis No.

Invalid MRC finishing shape start sequence No.

Valid Cut-off cycle shift amount/cut amount

Invalid Compound thread cutting cycle, number of cutting passes, chamfering, tool nose angle

Valid Compound thread cutting cycle Thread height

P

Invalid Program tool compensation input compensation No.

5. Position Commands 5.4 Decimal Point Input

33

Add- ress

Decimal point

command Application Re-

marks

Invalid Parameter input by program, section No.

Valid Coordinate position data Invalid Skip signal command Valid Arc center coordinates

(absolute value) (geometric)

Invalid Subprogram return destination sequence No.

Invalid Extended workpiece coordinate system No.

P

Invalid Tool life data group No. Invalid Minimum spindle clamp

rotation speed

Invalid MRC finishing shape end sequence No.

Valid Cut-off cycle Cut amount/shift amount

Valid Compound thread cutting cycle Minimum cut amount

Valid Compound thread cutting cycle First cut amount

Valid Deep hole drilling cycle 1 Cut amount of each pass

Invalid Program tool compensation input Hypothetical tool nose point No.

Invalid Deep hole drilling cycle (2) Dwell at cut point

Valid Arc center coordinates (absolute value) (geometric)

Valid Thread cutting start shift angle

Q

Invalid Tool life data management method

Valid R-designated arc radius Valid Corner rounding circular

radius ,R

Valid Automatic tool length measurement, deceleration range r

Valid MRC longitudinal/face escape amount

Invalid MRC shaping division No. Valid Cut-off cycle, return

amount

Valid Cut-off cycle, escape amount

Valid Compound thread cutting cycle, finishing allowance

Valid Compound thread cutting cycle/turning cycle, taper difference

R

Valid Hole drilling cycle/deep hole drilling cycle (2), distance to R point

(Note 1) Decimal points are all valid in user macro arguments.

Add- ress

Decimal point

command Application Re-

marks

Valid Program tool compensation input/nose R compensation amount

Valid Coordinate position data Valid Rough cutting cycle

(longitudinal) (face) pull amount

Valid Synchronous tap/ asynchronous tap changeover

,R

R

Valid Synchronous spindle phase shift amount

Invalid Spindle function codes Invalid Maximum spindle clamp

rotation speed

Invalid Constant surface speed control, surface speed

S

Invalid Parameter input by program, word type data

2 bytes

T Invalid Tool function codes Valid Coordinate position data Valid Program tool compensation

input

Valid Rough cutting cycle (longitudinal) cutting amount

U

Valid Dwell Valid Coordinate position data V Valid Program tool compensation

input

Valid Coordinate position data Valid Program tool compensation

input

W

Valid Rough cutting cycle (face) cutting amount

Valid Coordinate position data Valid Dwell

X

Valid Program tool compensation input

Valid Coordinate position data Y Valid Program tool compensation

input

Valid Coordinate position data Z Valid Program tool compensation

input

6. Interpolation Functions 6.1 Positioning (Rapid Traverse)

34

6. Interpolation Functions 6.1 Positioning (Rapid Traverse); G00

Function and purpose

This command is accompanied by coordinate words. It positions the tool along a linear or non-linear path from the present point as the start point to the end point which is specified by the coordinate words.

Command format

G00 X__/U__ Z__/W__ ; X, U, Z, W Coordinate values

The command addresses are valid for all additional axes.

Detailed description

(1) Once this command has been issued, the G00 mode is retained until it is changed by another

G function or until the G01, G02, G03, G33 or G34 command in the 01 group is issued. If the next command is G00, all that is required is simply that the coordinate words be specified.

(2) In he G00 mode, acceleration and deceleration are always carried out at the start point and end point of the block. After confirming that the current block command is 0, the next block is advanced to after confirming the state of the tracking error of the acceleration/deceleration circuit. The in-position width is set with the parameters.

(3) Any G command (G83 to G89) in the 09 group is cancelled (G80) by the G00 command.

(4) Whether the tool moves along a linear or non-linear path is determined by parameter, but the positioning time does not change.

(a) Linear path................. This is the same as linear interpolation (G01), and the speed is limited by the rapid traverse rate of each axis.

(b) Non-linear path .......... The tool is positioned at the rapid traverse rate independently for each axis.

(5) When no number following the G address, this is treated as G00.

CAUTION The commands with "no value after G" will be handled as "G00".

6. Interpolation Functions 6.1 Positioning (Rapid Traverse)

35

Example of program

Workpiece

Chuck

End point (+100, +150)

(Unit : mm)

+X

+Z

Start point (+180, +300)

Turret

G00 X100000 Z150000 ; Absolute value command G00 U-80000 W-150000 ; Incremental value command

(With an input setting unit of 0.001mm)

Precautions

(Note 1) When the parameter "#1086 G0Intp" is 0, the path along which the tool is positioned is the

shortest path connecting the start and end points. 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 Z-axis rapid traverse rates are both 9600mm/min, the tool will follow the path in the figure below if the following is programmed:

G00 Z-300000 X400000 ; (With an input setting unit of 0.001mm)

End point

(Unit : mm)

Start point

fz

fx

X

Z

300

40 0

Actual X axis rate: 6400 mm/min

Actual Z axis rate: 9600 mm/min

6. Interpolation Functions 6.1 Positioning (Rapid Traverse)

36

(Note 2) When parameter "#1086 G0Intp" is 1, 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 Z-axis rapid traverse rates are both 9600 mm/min, the

tool will follow the path in the figure below if the following is programmed:

G00 Z 300000 X400000 ; (With an input setting unit of 0.001mm)

fz

fx

X

Z

300 40

0

End point

Start point

(Unit : mm)

Actual X axis rate: 9600 mm/min

Actual Z axis rate: 9600 mm/min

6. Interpolation Functions 6.1 Positioning (Rapid Traverse)

37

(Note 3) The rapid traverse rate for each axis with the G00 command differs according to the

individual machine and so reference should be made to the machine specifications manual.

(Note 4) Rapid traverse (G00) deceleration check There are two methods for the deceleration check at rapid traverse; commanded

deceleration method and in-position check method. Select a method with the parameter #1193 inpos.

When inpos = 1

Upon completion of the rapid traverse (G00), the next block will be executed after confirming that the remaining distances for each axis are below the fixed amounts. (Refer to Operation during in-position check.)

The confirmation of the remaining distance should be done with the imposition width, LR . L R is the setting value for the servo parameter "#2224 sv024". The purpose of checking the rapid feed rate is to minimize the time it takes for positioning. The bigger the setting value for the servo parameter "#2224 sv024", the longer the reduced time is, but the remaining distance of the previous block at the starting time of the next block also becomes larger, and this could become an obstacle in the actual processing work. The check for the remaining distance is done at set intervals. Accordingly, it may not be possible to get the actual amount of time reduction for positioning with the setting value sv024.

When inpos = 0 Upon completion of the rapid traverse (G00), the next block will be executed after the

deceleration check time (Td) has elapsed. The deceleration check time (Td) is as follows, depending on the acceleration/deceleration type.

(1) Linear acceleration/linear deceleration......................... Td = Ts +

Ts

Td

Previous block Next block

Ts : Acceleration/deceleration time constant

Td : Deceleration check time Td = Ts + (0 to 14ms)

(2) Exponential acceleration/linear deceleration................ Td = 2 Ts +

2 Ts

Td Ts

Previous block Next block

Ts : Acceleration/deceleration time constant

Td : Deceleration check time Td = 2 Ts + (0 to 14ms)

6. Interpolation Functions 6.1 Positioning (Rapid Traverse)

38

(3) Exponential acceleration/exponential deceleration ...... Td = 2 Ts +

Ts

Td

Previous block Next block

Ts : Acceleration/deceleration time constant

Td : Deceleration check time Td = 2 Ts + (0 to 14ms)

Where Ts is the acceleration time constant, = 0 to 14ms The time required for the deceleration check during rapid traverse is the longest among the

rapid traverse deceleration check times of each axis determined by the rapid traverse acceleration/deceleration time constants and by the rapid traverse acceleration/ deceleration mode of the axes commanded simultaneously.

6. Interpolation Functions 6.1 Positioning (Rapid Traverse)

39

Programmable in-position width command for positioning

This command commands the in-position width for the positioning command from the machining program. G00 X__ Z__ ,I__ ;

In-position width

Positioning coordinate value of each axis

Operation during in-position check

Execution of the next block starts after confirming that the position error amount of the positioning (rapid traverse: G00) command block and the block that carries out deceleration check with the linear interpolation (G01) command is less than the in-position width issued in this command. The in-position width in this command is valid only in the command block, so the deceleration check method set in base specification parameter "#1193 inpos" is used for blocks that do not have the in-position width command. When there are several movement axes, the system confirms that the position error amount of each movement axis in each part system is less than the in-position width issued in this command before executing the next block. The differences of when the in-position check is validated with the parameter (base specification parameter "#1193 inpos" set to 1; refer to next page for in-position width) and when validated with this command are shown below.

The differences of In-position check with parameter

In-position check with ",I" address command In-position check with parameter After starting deceleration of the command system, the position error amount and commanded in-position width are compared.

After starting deceleration of the command system, the servo system's position error amount and the parameter setting value (in-position width) are compared.

Servo Command In-position width (Error amount of command end point and machine position)

Start of in-position check with ",I" address command

Block being executed

Ts

Td

Servo Command In-position width (Servo system position error amount)

Start of in-position check with parameter

Block being executed

Ts Td

Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = Ts + (0 to 14ms)

6. Interpolation Functions 6.1 Positioning (Rapid Traverse)

40

G0/G1 in-position width setting

When the setting value of the servo parameter "#2224 SV024" is smaller than the setting value of the G0 in-position width "#2077 G0inps" and the G1 in-position width "#2078 G1inps", the in-position check is carried out with the G0 in-position width and the G1 in-position width.

In-position check using the "G0inps" value Command to motor

Outline of motor movement

G0 in-position

SV024

A stop is judged here.

In-position check using the "G1inps" value Command to motor

Outline of motor movement

G1 in-position

SV024

A stop is judged here.

When the SV024 value is larger, the in-position check is completed when the error amount is smaller than the SV024 setting value. The in-position check method depends on the method set in the deceleration check parameter.

(Note 1) When the in-position width (programmable in-position check width) is set in the machining program, either the in-position width set with the parameter (SV024, G0inps, G1inps) or that set in the program, whichever larger, is applied when performing an in-position check.

(Note 2) When the SV024 setting value is larger than the G0 in-position width/G1 in-position width, the in-position check is carried out with the SV024 value.

(Note 3) When the error detection is ON, the in-position check is forcibly carried out.

6. Interpolation Functions 6.2 Linear Interpolation

41

6.2 Linear Interpolation; G01

Function and purpose

This command is accompanied by coordinate words and a feed rate command. It makes the tool move (interpolate) linearly from its present position to the end point specified by the coordinate words at the speed specified by address F. In this case, the feed rate specified by address F always acts as a linear speed in the tool nose center advance direction.

Command format

G01 X__/U__ Z__/W__ __ F__ ,I__ ; ("" is an additional axis) X, U, Z, W, F I

Coordinate values Feed rate (mm/min or /min) In-position width. This is valid only in the commanded block. A block that does not contain this address will follow the parameter "#1193 inpos" settings. 1 to 999999 (mm)

X axis

Z axis X

Present position

U / 2

Z W

Command point

Detailed description

Once this command is issued, the mode is maintained until another G function (G00, G02, G03, G33, G34) in the 01 group which changes the G01 mode is issued. Therefore, if the next command is also G01 and if the feed rate is the same all that is required to be done is to specify the coordinate words. If no F command is given in the first G01 command block, program error (P62) results. The feed rate for a rotation axis is commanded by /min (decimal point position unit). (F300 = 300/min) The G functions (G70 to G89) in the 09 group are cancelled (G80) by the G01 command.

6. Interpolation Functions 6.2 Linear Interpolation

42

Example of program

(Example 1)

20.0

50.0

Z axis

Present position

X axis

(Unit: mm)

G01 X50.0 Z20.0 F300 ;

(Example 2) Cutting in the sequence of P1 P2 P3 P4 at 300mm/min feed rate P0 P1 , P4 P0 is for tool positioning.

Turret

240

200

140

100

2209040 230160

P1

P2 P3 P4

P0

+X

+Z

Input setting unit : 0.001mm

(Unit: mm)

G00 X200000 Z40000 ; P0 P1 G01 X100000 Z90000 F300 ; P1 P2 Z160000 ; P2 P3 X140000 Z220000 ; P3 P4 G00 X240000 Z230000 ; P4 P0

6. Interpolation Functions 6.2 Linear Interpolation

43

Programmable in-position width command for linear interpolation

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. G01 X__ Z__ F__ ,I__ ;

In-position width Feed rate Linear interpolation coordinate value of each axis

(Note 1) Refer to section "6.1 Positioning (Rapid Traverse); G00" for details on the in-position check operation.

6. Interpolation Functions 6.3 Circular Interpolation

44

6.3 Circular Interpolation; G02, G03 Function and purpose

These commands serve to move the tool along a circular.

Command format

G02 (G03) X__/U__ Z__/W__ I__ K__ F__ ; G02 Clockwise (CW) G03 Counterclockwise (CCW) X/U Circular end point coordinates, X axis (absolute value of workpiece

coordinate system for X, incremental value from present position for U) Z/W Circular end point coordinates, Z axis (absolute value of workpiece

coordinate system for Z, incremental value from present position for W) I Circular center, X axis (for I, incremental value of X coordinate at center as

seen from start point. Command as radius command.) K Circular center, Z axis (for K, incremental value of Z coordinate at center as

seen from start point) F Feed rate

The circular center coordinate value is commanded with an input setting increment. Caution is required for the arc command of an axis for witch the input command increment differs. Command with a decimal point to avoid confusion.

X

Z KW

U/2

I End point

Start point

Z axis

CenterX axis

6. Interpolation Functions 6.3 Circular Interpolation

45

Detailed description

(1) G02 (or G03) is retained until another G command (G00, G01 or G33) in the 01 group that

changes its mode is issued. The direction of the circular rotation is differentiated by G02 and G03: G02 : Clockwise (CW) G03 : Counterclockwise (CCW)

Turret

Turret +X

+X

+X

+X

+Z

+Z

+Z

CCW(G03)

CCW(G03)

CW(G02)

CW(G02)

Chuck

Work- piece

(2) An arc which extends for more than one quadrant can be executed with a single block command.

(3) The following information is needed for circular interpolation.

(a) Rotation direction :Clockwise (G02) or counterclockwise (G03)

(b) Circular end point coordinates :Given by addresses X, Z, U, W

(c) Circular center coordinates :Given by addresses I, K (incremental value commands)

(d) Feed rate :Given by address F

(4) A program error results when I, K or R is not commanded. Consideration must be given to the sign for I and K since I is the distance in the X-axis direction to the arc center as seen from the start point and K is the distance in the Z-axis direction.

(5) No T commands can be issued in the G2/G3 modal status. A program error (P151) results if a T command is issued in the G2/G3 modal status.

6. Interpolation Functions 6.3 Circular Interpolation

46

Example of program

120.0

20.0

70.0 50.0

50.0

(Unit: mm)

Z axis

X axis

Workpiece coordinate zero point

G2 X120.0 Z70.0 I50.0 F200 ; Absolute value command G2 U100.0 W-50.0 I50.0 F200 ; Incremental value command

6. Interpolation Functions 6.3 Circular Interpolation

47

Change into linear interpolation command

Program error (P33) will occur when the center and radius are not designated at circular command. When the parameter "#11029 Arc to G1 no Cent (Change command from arc to linear when no arc center designation)" is set, the linear interpolation can be applied to terminal coordinates value for only the block. However, a modal is the circular modal. This function is not applied to a circular command by a geometric function. (Example) The parameter "#11029 Arc to G1 no Cent (Change command from arc to linear when no arc center designation)" = "1"

N1

N3

20 0

G90 X0 Y0 ; N1 G02 X20. I10. F500 ; N2 G00 X0 N3 G02 X20. F500 ; M02 ;

(a) (b)

(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.

6. Interpolation Functions 6.3 Circular Interpolation

48

Cautions for circular interpolation

(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 coordinate 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 and K is the same as commanding a 360 arc (perfect circle).

(3) The following occurs when the start and end point radii do not match in a circular command:

(a) Program error (P70) results at the circular start point when error R is greater than the parameter "#1084 RadErr".

G02Z80.K50. ;

R

X

Z

Alarm stop

Start point radius End point radius

Center End point Start point

(b) Spiral interpolation in the direction of the commanded end point results when error R is less than the parameter value.

Spiral interpolation

R

G02Z90.K50. ;

X

Z Start point radius End point

radius

Center Start point

End point

6. Interpolation Functions 6.4 R Specification Circular Interpolation

49

6.4 R Specification Circular Interpolation; G02, G03

Function and purpose

Along with the conventional circular interpolation commands based on the circular center coordinate (I, K) designation, these commands can also be issued by directly designating the circular radius R.

Command format

G02 (G03) X/U__ Z/W__ R__ F__ ; X/U Z/W R F

X-axis end point coordinate Z-axis end point coordinate Circular radius Feed rate

The arc radius is commanded with an input setting increment. Caution is required for the arc command of an axis for which the input command increment differs. Command with a decimal point to avoid confusion.

Detailed description

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 perpendicular 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.

01

02

L

r

Circular path when R sign is minus

End point

Circular path when R sign is plus

Center point

Center point

Start point

The following condition must be met with an R specification circular interpolation command: 1

When L/2 - r > (parameter : #1084 RadErr), an alarm will occur.

Where L is the line from the start point to end point. 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. 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, K specification circular command should therefore be used in such a case.

L 2 r

6. Interpolation Functions 6.4 R Specification Circular Interpolation

50

Example of program

(Example 1)

G03 Zz1 Xx1 Rr1 Ff1 ; R specification circular on Z-X plane

(Example 2)

G02 Xx1 Zz1 Ii1 Kk1 Rr1 Ff1 ; R specification circular on X-Z plane (When the R specification and I, K specification are contained in the same block, the R specification has priority in processing.)

Circular center coordinate compensation

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 segment connecting the start and end points" is compensated as the circular center. Set the setting value to the parameter "#11028 Tolerance Arc Cent (Tolerable correction value of arc center error)". (Ex.) "#11028 Tolerance Arc Cent" = "0.000 (mm)"

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

0 10

N1, N3

N

G90 X0 Y0 ;

N1 G02 X10. R5.000;

N2 G0 X0;

N3 G02 X10. R5.001;

N4 G0 X0;

N5 G02 X10. R5.002;

N6 G0 X0;

M02 ;

(a)

(b)

(a) Compensate the center coordinate: Same as N1 path (b) Do not compensate the center coordinate: Inside path a little than N1 Calculation error margin compensation allowance value: 0.002 mm Segment connecting the start and end paints: 10.000 N3: Radius 2 = 10.002 "Error 0.002 -> Compensate" N5: Radius 2 = 10.004 "Error 0.004 -> Do not compensate" Therefore, this example is shown in the above figure.

6. Interpolation Functions 6.5 Plane Selection

51

6.5 Plane Selection; G17, G18, G19

Function and purpose

These commands are used to select the control plane and the plane on which the circular exists. If the 3 basic axes and the parallel axes corresponding to these basic axes are entered as parameters, the commands can select the plane composed of any 2 axes which are not parallel axes. If a rotation axis is entered as a parallel axis, the commands can select the plane containing the rotation axis. These commands are used to select:

The plane for circular interpolation The plane for nose R compensation

Command format

G17; G18; G19;

(I-J plane selection) (K-I plane selection) (J-K plane selection)

I, J and K indicate each basic axis or parallel axis. When the power is turned ON or when the system is reset, the plane set by the parameters "#1025 I_plane" is selected.

I

J

G02

G03

I

K

G02

G03

K

J

G02

G03

G17 (I-J) plane G18 (K-I) plane G19 (J-K) plane

6. Interpolation Functions 6.5 Plane Selection

52

Parameter entry

#1026 to 1028

base_I, J, K #1029 to 1031

aux_I, J, K I X Y J Y K Z

Plane selection system

This section describes the plane selection for the parameter entry samples shown in Fig. 1.

(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.

(Example)

G17XY; Y

X

G02

G03

G18XZ; X

Z

G02

G03

G19YZ; Z

Y

G02

G03

(2) Plane selection is not performed with blocks in which the plane selection G code (G17, G18, G19) is not assigned.

G18 X_ Z_ ; Z-X plane Y_ Z_ ; Z-X plane (no plane change)

(3) When the axis addresses are omitted in the block containing the plane selection G codes (G17, G18, G19), it is assumed that the axis addresses of the 3 basic axes have been assigned.

G18 ; (Z-X plane = G18 XZ ;)

(4) 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.

G18 XYZ ; The Z-X plane is selected. Therefore, the Y movement is unrelated to the selected plane.

(Note 1) When the "2" in the parameter "#1025 I_plane" is kept ON, the G18 plane is selected

when the power is turned ON or when the system is reset.

Basic axes and parallel axes can be entered in the parameters. The same axis name can be entered in duplication, but when it is assigned in duplication, the plane is determined by plane selection system (4). It is not possible to set axes, which have not been entered, as control axes.

Fig. 1 Examples of plane selection parameter entry

6. Interpolation Functions 6.6 Thread Cutting

53

6.6 Thread Cutting 6.6.1 Constant Lead Thread Cutting; G33

Function and purpose

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, tapered thread-cutting, and continuous thread-cutting.

Straight thread Scrolled thread Continuous thread

F/E

F/E

F/E

Command format

G33 Z/W__ X/U__ F__ Q__ ; (Normal lead thread cutting commands) Z, W, X, U F Q

Thread end point Lead of long axis (axis which moves most) direction Thread cutting start shift angle, 0.001 to 360.000

G33 Z/W__ X/U__ E__ Q__ ; (Precision lead thread cutting commands) Z, W, X, U E Q

Thread end point Lead of long axis (axis which moves most) direction Thread cutting start shift angle, 0.001 to 360.000

Z

Z

U/2

X

Q

One-rotation synchronization signal

Thread cutting start position

W

2 1

1 > Illegal lead at start of thread cutting 2 > Illegal lead at end of thread cutting

X axis

Start point

End point

Z axis

F/E

6. Interpolation Functions 6.6 Thread Cutting

54

Detailed description

(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 "#1229 set 01/bit" is set to "1" for precision lead designation.)

(2) The lead in the long axis direction is commanded for the taper thread lead.

When a < 45, Lead is in Z-axis direction. When a > 45, Lead is in X-axis direction. When a = 45, Lead can be in either Z or X-axis direction.

U/2

W

a

Tapered thread section

X axis

Start point

End point

Z axis

Thread cutting metric input

Input setting unit B (0.001mm) C (0.0001mm)

Command address F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)

Least command increment

1 (=1.000), (1.=1.000)

1 (= 1.00000), (1.=1.00000)

1 (= 1.00), (1.=1.00)

1 (= 1.0000), (1.=1.0000)

1(=1.000000), (1.=1.000000)

1 (= 1.000), (1.=1.000)

Command range

0.001 to 999.999

0.00001 to 999.99999

0.03 to 999.99

0.0001 to 999.9999

0.000001 to 999.999999

0.255 to 999.999

Input

setting unit D (0.00001mm) E (0.000001mm)

Command address F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)

Least command increment

1 (= 1.00000), (1.=1.00000)

1 (= 1.0000000), (1.=1.0000000)

1 (= 1.0000), (1.=1.0000)

1 (= 1.000000), (1.=1.000000)

1 (=1.00000000), (1.=1.00000000)

1 (= 1.00000), (1.=1.00000)

Command range

0.00001 to 999.99999

0.0000001 to 999.9999999

0.2550 to 999.9999

0.000001 to 999.999999

0.00000001 to 999.99999999

0.25500 to 999.99999

6. Interpolation Functions 6.6 Thread Cutting

55

Thread cutting inch input

Input setting unit B (0.0001inch) C (0.00001inch)

Command address F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)

Least command increment

1(=1.0000), (1.=1.0000)

1(=1.000000), (1.=1.000000)

1 (= 1.0000), (1.=1.0000)

1(=1.00000), (1.=1.00000)

1(=1.0000000), (1.=1.0000000)

1(=1.00000), (1.=1.00000)

Command range

0.0001 to 99.9999

0.000001 to 39.370078

0.0255 to 9999.9999

0.00001 to 99.99999

0.0000001 to 39.3700787

0.25401 to 9999.99999

Input

setting unit D (0.000001inch) E (0.0000001inch)

Command address F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)

Least command increment

1 (= 1.000000), (1.=1.000000)

1 (= 1.00000000), (1.=1.00000000)

1 (= 1.000000), (1.=1.000000)

1 (= 1.0000000), (1.=1.0000000)

1 (= 1.000000000), (1.=1.000000000)

1 (= 1.0000000), (1.=1.0000000)

Command range

0.000001 to 99.999999

0.00000001 to 39.37007874

0.025500 to 9999.99999

0.0000001 to 99.9999999

0.000000001 to 39.370078740

0.0255000 to 9999.9999999

(Note 1) It is not possible to assign a lead where the feed rate as converted into feed per minute exceeds the maximum cutting feed rate.

(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 result at the end point of the block following the block in which thread cutting is completed (no longer G33 mode).

(6) The converted cutting feed rate 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 result.

(7) In order to protect the lead during thread cutting, a cutting feed rate 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 system 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 feed rate Thread lead

Where R Tolerable speed of encoder (r/min) R = Spindle rotation speed (r/min) Thread lead = mm or inches Maximum feed rate = mm/min or inch/mm (this is subject to the restrictions imposed by the machine specifications).

(10) A program error (P97) may occur when the result of the expression (9) is R<1 because the thread lead is very large to the highest cutting feedrate.

6. Interpolation Functions 6.6 Thread Cutting

56

(11) Dry run is valid for thread cutting but the feed rate based on dry run is not synchronized with the

spindle rotation. The dry run signal is checked at the start of thread cutting and any switching during thread

cutting is ignored.

(12) Synchronous feed applies for the thread cutting commands even with an asynchronous feed command (G94).

(13) Spindle override and cutting feed override are invalid and the speeds are fixed to 100% during thread cutting.

(14) When a thread cutting command is programmed during nose R compensation, the compensation is temporarily canceled 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 contain 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 (When G33 mode is cancelled) is first executed and then the automatic operation stops. Note that automatic operation is stopped until the G33 command axis starts moving.

(17) The thread cutting command waits for the single rotation sync signal of the rotary encoder and starts movement. Note that carry out synchronization between part systems before issuing a thread cutting command with multiple part systems. For example, when using the 1-spindle specifications with multi-part systems, if one part system issues a thread cutting command during ongoing thread cutting by another part system, the movement will start without waiting for the rotary encoder single rotation sync signal.

(18) The thread cutting start shift angle is not a 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 commanded with 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.

6. Interpolation Functions 6.6 Thread Cutting

57

Example of program

40.0 50.0

90.0

20.0 Z axis

X axis

(Unit: mm)

G33 X90.0 Z40.0 E12.34567 ; Absolute value command G33 U70.0 W-50.0 E12.34567 ; Incremental value command

6. Interpolation Functions 6.6 Thread Cutting

58

6.6.2 Inch Thread Cutting; G33

Function and purpose

If the number of ridges per inch in the long axis direction is assigned in the G33 command, the feed of the tool synchronized with the spindle rotation will be controlled, which means that constant-lead straight thread-cutting and tapered thread-cutting can be performed.

Command format

G33 Z/W__ X/U__ E__ Q__ ; Z,W,X,U E Q

Thread end point Number of ridges per inch in direction of long axis (axis which moves most) (decimal point command can also be assigned) Thread cutting start shift angle, 0.001 to 360.000

Z

Z

U/2

X

Q

One-rotation synchronization signal

Thread cutting start position

W

2 1

1 > Illegal lead at start of thread cutting 2 > Illegal lead at end of thread cutting

X axis

Start point

End point

Z axis

F/E

Detailed description

(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 parameter "#1229 set 01/bit 1" to "0".)

(3) The E command value should be set within the lead value range when the lead is converted.

(4) See Section "6.6.1 Constant lead thread cutting" for other details.

6. Interpolation Functions 6.6 Thread Cutting

59

Example of program

40.0 50.0

90.0

20.0 Z axis

X axis

(Unit: mm)

G33 X90.0 Z40.0 E12.0 ; Absolute value command G33 U70.0 W-50.0 E12.0 ; Incremental value command

6. Interpolation Functions 6.6 Thread Cutting

60

6.6.3 Continuous Thread Cutting Function and purpose

Continuous thread cutting is possible by assigning thread cutting commands continuously. In this way, it is possible to cut special threads whose lead or shape changes.

G33 G33

G33

Command format

G33 Zz1/Ww1 Xx1/Uu1 Ff1/Ee1 Qq1 ; (G33) Zz2/Ww2 Xx2/Uu2 Ff2/Ee2 Qq2 ; (G33) Zz3/Ww3 Xx3/Uu3 Ff3/Ee3 Qq3 ; Zzn, Wwn, Xxn, Uun Ffn/Een Qqn

Thread end point Lead of long axis (axis which moves most) direction Thread cutting start shift angle, 0.001 to 360.000

Detailed description

(1) The first thread cutting block in the continuous thread cutting command waits for the spindle's single rotation synchronization signal before starting thread cutting. From the second and following blocks, movement starts without waiting for the spindle's single rotation synchronization command.

Thus, the thread cutting start shift angle (Q) can be commanded only in the first block. (2) The G33 command can be omitted from the second and following blocks. (3) When commanding continuous thread cutting, command the thread cutting commands in

successive blocks. If a command other than thread cutting is issued, continuous thread cutting will not take place.

Note that if a command that does not involve axis movement (G4 dwell command, MST command, etc.) is commanded between the thread cutting command blocks, whether to wait for the spindle's single rotation synchronization signal after the 2nd block can be selected with the parameters.

# Item Contents Setting range 1270 ext06/

bit6 Set the continuous thread cutting Z phase wait operation. 0: If there is no movement command (MST command, etc.)

between the thread cutting locks, the 2nd block thread cutting waits for the spindle's single rotation synchronization signal before starting movement.

1: Even if there is no movement command (MST command, etc.) between the thread cutting blocks, the 2nd block thread cutting starts movement without waiting for the spindle's single rotation synchronization signal.

0/1

(4) The other matters are the same as uniform lead thread cutting.

6. Interpolation Functions 6.6 Thread Cutting

61

6.6.4 Variable Lead Thread Cutting; G34

Function and purpose

Variable lead thread cutting is enabled by a command specifying a lead increment or decrement amount per turn of the screw.

Command format

G34 X/U__ Z/W__ F/E__ K__ ; X/U Z/W F/E K

Thread end point Standard screw lead Lead increment or decrement amount per turn of the screw

F+3.5K

Non-lead axis

Lead axis

F+2.5K F+1.5K F+0.5K

Lead speed F+4K

F+3K F+2K F+K F

6. Interpolation Functions 6.6 Thread Cutting

62

Detailed description

(1) The command range is as shown below.

Thread cutting metric input

Input setting unit B (0.001mm) C (0.0001mm)

Command address F (mm/rev) E (mm/rev) F (mm/rev) E (mm/rev)

Least command increment

1 (=1.000), (1.=1.000)

1 (= 1.00000), (1.=1.00000)

1 (= 1.0000), (1.=1.0000)

1(=1.000000), (1.=1.000000)

Command range

0.001 to 999.999

0.00001 to 999.99999

0.0001 to 999.9999

0.000001 to 999.999999

Input setting unit D (0.00001mm) E (0.000001mm) B/C/D/E

Command address F (mm/rev) E (mm/rev) F (mm/rev) E (mm/rev)

Least command increment

1 (= 1.00000), (1.=1.00000)

1 (= 1.0000000), (1.=1.0000000)

1 (= 1.000000), (1.=1.000000)

1 (=1.00000000), (1.=1.00000000)

Command range

0.00001 to 999.99999

0.0000001 to 999.9999999

0.000001 to 999.999999

0.00000001 to 999.99999999

K (n mm/rev) n: Number of

pitches Same as F or E (signed)

Thread cutting inch input

Input setting unit B (0.0001inch) C (0.00001inch)

Command address F (inch/rev) E (inch/rev) F (inch/rev) E (inch/rev)

Least command increment

1(=1.0000), (1.=1.0000)

1(=1.000000), (1.=1.000000)

1(=1.00000), (1.=1.00000)

1(=1.0000000), (1.=1.0000000)

Command range

0.0001 to 99.9999

0.000001 to 39.370078

0.00001 to 99.99999

0.0000001 to 39.3700787

Input setting unit D (0.000001inch) E (0.0000001inch) B/C/D/E

Command address F (inch/rev) E (inch/rev) F (inch/rev) E (inch/rev)

Least command increment

1 (= 1.000000), (1.=1.000000)

1 (= 1.00000000), (1.=1.00000000)

1 (= 1.0000000), (1.=1.0000000)

1 (= 1.000000000), (1.=1.000000000)

Command range

0.000001 to 99.999999

0.00000001 to 39.37007874

0.0000001 to 99.9999999

0.000000001 to 39.370078740

K (n inch/rev) n: Number of

pitches Same as F or E (signed)

(2) A positive value of K indicates incremental pitches. Movement amount of one block (n pitches) = (F + K) + (F + 2K) + (F + 3K) + + (F + nK) (3) A negative value of K indicates decremental pitches. Movement amount of one block (n pitches) = (F K) + (F 2K) + (F 3K) + + (F nK)

6. Interpolation Functions 6.6 Thread Cutting

63

(4) A program error will occur if the thread lead is not set correctly.

Error No. Meaning Remedy

P93 Illegal pitch value (1) An invalid value is specified for F/E

or K in a thread cutting command. (2) The last lead goes outside of the F/E

command range.

Specify valid values for F/E and K. (Reference 1)

(Reference 1) Last lead = (F2+2KZ) Number of pitches = (F + last lead)/K Z: Length of lead axis

(5) The other matters are the same as G33. Refer to section "6.6.1 Constant lead thread cutting; G33".

6. Interpolation Functions 6.6 Thread Cutting

64

6.6.5 Circular Thread Cutting; G35, G36

Function and purpose

Circular thread cutting making the longitudinal direction the lead is possible.

Command format

G35(G36) X/U__ Z/W__ { I__ K__

R__ } F/E__ Q__ ;

G35 G36 X/U Z/W I K R F/E Q

Clockwise (CW) Counterclockwise (CCW) Circular end point coordinate, X axis (absolute value of workpiece coordinate system for X, incremental value from present position for U) Circular end point coordinate, Z axis (absolute value of workpiece coordinate system for Z, incremental value from present position for W) Circular center, X axis (incremental value of circular center looking from start point) Circular center, Z axis (incremental value of circular center looking from start point) Arc radius Longitudinal (axis with largest movement amount) direction lead (F.. normal lead thread cutting/E .. precision lead thread, inch thread) Thread cutting start shift angle, 0.000 to 360.000

X axis

Z W End point

U/2

X R

Center

K

Z axis

l

Start point

F/E Circular thread

6. Interpolation Functions 6.6 Thread Cutting

65

Detailed description

(1) A program error (P33) will occur if the start point and end point match or if the arc center angle

is more than 180.

(2) The following will occur if the start point radius and end point radius do not match.

A program error (P70) will occur if the error R is more than parameter "#1084 RadErr" (arc error).

Interpolation will start from the arc center where the start point radius and end point radius match if the error R is less than parameter "#1084 RadErr".

End point radius

End point

Center

Start point radius

Start point Obtained center

R

(3) A program error (P33) will occur if the R_ sign is negative.

(4) A program error (P33) will occur if there is no I_K_ command and R_ command.

(5) The R_ command will have the priority if the I_K_ command and R_ command are issued in the same block.

(6) If the arc center is (0,0), the arc command can be issued for two successive quadrants. A program error (P33) will occur if an arc with more than three quadrants is issued.

Z Z

X

Start point End point

X

When Z axis is long axis

1st and 4th quadrant 2nd and 3rd quadrant

Center

Start point End point

Center

6. Interpolation Functions 6.6 Thread Cutting

66

(7) When the movement amount is equal, the horizontal direction in the selected plane will be the

long axis.

Plane selection Long axis when movement amount is equal G17 (XY plane) I axis G18 (ZX plane) K axis G19 (YZ plane) J axis

(8) G36 is used to command two functions, automatic tool length measurement and circular thread

cutting (CCW). Which function is selected follows parameter "#1238 set10/bit0" (Arc thread cutting).

When #1238 set10/bit0 is set to 0 G code Function

G35 Circular thread cutting clockwise (CW) G36 Automatic tool length measurement X

When #1238 set10/bit0 is set to 1

G code Function G35 Circular thread cutting clockwise (CW) G36 Circular thread cutting counterclockwise (CCW) G37 Automatic tool length measurement Z G37.1 Automatic tool length measurement X G37.2 Automatic tool length measurement Z

(9) If the lead axis and non-lead axis cutting feed rate is faster than the clamp speed when thread

cutting is started, the "M01 operation error 107" will occur, and thread cutting will not start.

(10) During thread cutting, the cutting feed rate may exceed the clamp speed to guarantee the lead. In this case, the error "M01 operation error 107" will appear, but thread cutting will continue. However, if the "cutting feed rate > clamp speed" is established during circular thread cutting commanded in the second or following block of continuous thread cutting, automatic operation will be stopped just before the circular thread cutting command in the 2nd block, and the error "M01 operation error 107" will appear.

(11) Continuous thread cutting is possible by commanding the thread cutting command in succession. This allows special threads in which the leads or shapes change midway to be cut.

The continuous thread cutting command can be issued in the order of arc arc, arc constant lead, and constant lead arc.

(12) Normally, an illegal lead will be cut at the start and end of the threads, due to a delay in the servo system.

Thus, command the required thread length with the illegal thread length added to the start and end.

As another method, command the required thread length as a circular thread (G35/G36), and then command the illegal lead length before and after that command (start and end of thread cutting) as a constant lead thread (G33). (Continuous thread cutting in order of constant lead arc constant lead.)

6. Interpolation Functions 6.6 Thread Cutting

67

Relation with other functions

(1) A program error (P113) will occur if the G35/G36 command is issued to an axis not within the

selected plane.

(2) The thread cutting speed is not synchronized with the spindle rotation when dry run is valid. (The thread pitch is not guaranteed.)

(3) If the dry run switch is turned ON during thread cutting, the dry run signal will be ignored.

(4) If the FEEDHOLD switch is pressed during thread cutting, the block will stop at the end point of the block following that in which thread cutting is completed (when the thread cutting mode is exited).

(5) Circular thread cutting will function normally even during mirror image.

(6) A program error (P201) will occur if the G35/G36 circular thread cutting command is issued in the finish shape program of the compound type fixed cycle for turning machining.

(7) A program error (P385) will occur if thread cutting corner rounding or corner chamfering is commanded during circular thread cutting or the next block.

(8) Geometric and circular thread cutting cannot be commanded simultaneously. If commanded simultaneously, a program error (P395) or program error (P70) will occur.

(9) If thread cutting is commanded during nose R compensation, nose R compensation will be temporarily canceled, and thread cutting will be executed.

(10) Do not issue the circular thread cutting command during constant surface speed control. The thread will not be cut correctly because the spindle rotation speed will change during thread cutting.

Precautions

(1) Spindle override does not function during thread cutting.

(2) A program error (P39) will occur if G35/G36 is commanded when the additional specifications are not provided.

6. Interpolation Functions 6.7 Helical Interpolation

68

6.7 Helical Interpolation; G17, G18, G19, and G02, G03

Function and purpose

This function is for circularly interpolating 2 axes on the selected plane and simultaneously interpolating the other axis linearly in synchronization with the circular motion. When this interpolation is performed with 3 orthogonal axes, the tool will travel helically.

X

Y Z Command program path

Linear interpolation element

Circular interpolation element

Command format

G17 G02 (G03) X/U__ Y/V__ Z/W__ I__ J__ F__ ; G17 G02 (G03) X/U__ Y/V__ Z/W__ R__ F__ ;

G17 Arc plane (G17: X-Y plane, G18: Z-X plane, G19: Y-Z plane) G02 (G03) Arc rotation direction (G02: clockwise, G03: counterclockwise) X/U, Y/V Arc end point coordinates Z/W Linear axis end point coordinates I, J Arc center coordinates R Arc radius F Feed rate

(Note 1) In this manual, the following setting descriptions are used: I axis: X, J axis: Y, K axis: Z

6. Interpolation Functions 6.7 Helical Interpolation

69

Detailed description

The following type of movement will take place when the following type of command is issued.

G17 G02 Xx Yy Zz Ii Jj Ff ;

Y

X

Start point

End point

X

Y Z

X-Y plane path (projected path)

i

j

Command program path

Linear interpolation element

Circular interpolation element

The left drawing shows the process as an exploded view, and the right drawing shows the arc plane from directly above.

6. Interpolation Functions 6.7 Helical Interpolation

70

Example of program

(Example)

G17 G02 X100. Y100. Z100. I-100. J100. F120 ;

Y

X

Start point

End point

X

Y Z

X-Y plane path (projected path)

I-100. J100.

Command program path

Linear interpolation element

Circular interpolation element

(Unit: mm)

The left drawing shows the process as an exploded view, and the right drawing shows the arc plane from directly above. At the start of the block, the axis centers at the point 100mm in the X axis direction and 100mm in the Y axis direction from the workpiece coordinates (start point), and starts cutting at the feed rate 120mm/min while rotating.

Precautions and restrictions

(1) When executing helical interpolation, command another linear axis (several axis can be

commanded) that does not contain the circular interpolation command and arc axis.

(2) Up to the number of simultaneous contouring control axes can be commanded simultaneously.

(3) A command exceeding one rotation cannot be issued. (The circular interpolation command specifications are followed.)

(4) Command the feed rate as the composite speed for each axis.

(5) With helical interpolation, the axis that configures the plane is the circular interpolation axis, and the other axes are the linear interpolation axes.

(6) The corner chamfering or corner R commands that are issued before or after the helical interpolation command block are effective only on the axes contained in the selected plane.

(7) For the parameters and error messages, refer to the materials concerning the circular interpolation (G02,G03).

6. Interpolation Functions 6.8 Milling Interpolation

71

6.8 Milling Interpolation; G12.1

Function and purpose

Milling interpolation is used to perform contouring control by converting commands programmed in an orthogonal coordinate system into movements of a linear axis and rotation axis (workpiece rotation).

C

Z

Y (Hypothetical axis)

X

A G12.1 command is issued to perform milling and a G13.1 command is issued to cancel milling and returns to normal turning.

Command format

G12.1 D__ E__ ; Milling mode ON D Selection of milling hypothetical axis name E Designation of milling interpolation rotation axis

G13.1; Milling mode OFF (Turning mode)

6. Interpolation Functions 6.8 Milling Interpolation

72

Address Meaning of address Command range (unit) Remarks

D Selection of milling hypothetical axis name

0: Y axis 1: Rotation axis

name

If there is no D command, the milling hypothetical axis name will follow parameter (#1517 mill_C).

If only the D command is issued, it will be handled as D0.

A program error (P35) will occur if a value other than 0 or 1 is issued as the numerical command after the D command.

E Designation of milling interpolation rotation axis

G12.1 command system rotation axis command address

If there is no E command, the parameter (#1516 mill_ax) will be followed.

A program error (P33) will occur if only an E command is issued.

A program error (P33) will occur if an axis address is not commanded after "E=".

A program error (P300) will occur if an axis that does not exist in the command system is designated as the rotation axis name.

A program error (P32) will occur if a value is commanded for the rotation axis name.

To issue a program command after the "E= rotation axis name", delimit the "E= rotation axis name" and the other command with a comma (,). A program error (P33) will occur if there is no comma.

The following G codes are used to select milling and set the conditions.

G code Function Remarks G12.1 Milling mode ON Default is G13.1. G13.1 Milling mode OFF G16 Selection of Y-Z cylindrical plane G17 Selection of X-Y plane G19 Selection of Y-Z plane

One of G17, G16, and G19 can be defined as the default (when G12.1 is issued) by the parameter.

G41 Tool radius compensation left Default is G40. G42 Tool radius compensation right

6. Interpolation Functions 6.8 Milling Interpolation

73

G46, G41, G42/G40 (Nose R compensation) G41, G42/G40 (Tool compensation)

6.8.1 Selecting Milling Mode

Detailed description

(1) The G12.1 and G13.1 commands are used to switch between the turning (G13.1) and milling

(G12.1) modes.

(2) These commands are modal and the initial mode effective at power ON is the turning mode.

(3) The following requirements must be satisfied before a G12.1 command is issued. Otherwise, a program error (P485) results.

(a) Nose R compensation has been canceled.

(b) Constant surface speed control has been canceled.

(4) If one of the command axes in the milling mode has not completed reference position return, a program error (P484) results.

(5) The G12.1 command automatically cancels an asynchronous mode F command. Therefore, specify an F value in milling mode.

(Note1) If G12.1 is executed, while no movement command has been given, after nose R compensation is canceled by an independent G40 command, nose R compensation is canceled in the G12.1 block.

(Note2) If the milling interpolation command is issued during the mirror image, a program error (P486) results.

(Note3) When the G12.1 command is issued, the deceleration check is executed.

(Note 4) If a command other than a plane section is issued during the G12.1 command, a program error (P33) will occur.

Machining mode

G13.1 (Turning mode) G12.1 (Milling mode)

G17 (X-Y plane)

G18 (Z-X plane)

G19 (Y-Z plane)

G16 Y-Z cylindrical plane

G17 (X-Y plane)

G19 (Y-Z plane)

6. Interpolation Functions 6.8 Milling Interpolation

74

6.8.2 Milling Interpolation Control and Command Axes

Detailed description

(1) The two orthogonal linear axes (X axis and Z axis) and a rotation axis are used as control axes

for milling interpolation. The rotation axis is selected with the E command. The axis designated with the parameter will be selected if there is no E command.

(2) Three orthogonal linear axes are used as the command axes for milling interpolation. They are the X, Z, and a hypothetical axis.

The hypothetical axis is a hypothetical axis for interpolation which intersects the X and Z axes at right angles. The hypothetical axis name is the control rotation axis name selected with Y or in (1) with the D command. The axis name designated with the parameter will be selected if there is no D command.

Z

X

(Hypothetical axis)

(3) Command axis X for milling is not just the interpolated one of control axis X. It is handled as X in the milling coordinate system when a G12. 1 command is issued.

(4) Whether the position in the milling coordinate system is a diameter command or radius

command is selected with the following parameter.

ParameterDetails 0: Radius command for all axes

#8111 Milling Radius 1: Follows parameter (#1019 dia) for each axis

(Example 1)

X

0 10 Hypothetical axis

N3

10

(Program 1) : : :

N1 G0 X40 ; N2 G12.1 ; (or G12.1 E=C, D0 ;) N3 G1 X10. Y10. F10. ;

: : :

When C axis is used for rotation axis, and "Y" is used for hypothetical axis name

20

(Unit: mm)

6. Interpolation Functions 6.8 Milling Interpolation

75

N3 of program 1 is executed as follows:

X = Mill _ X

Mill _ X Mill _ X

(d) (c)

(b)(a) Mill _ X

X

X X

(Unit: mm)

Program path

Program path

Program path

Program path

Hypothetical axis Hypothetical

axis

Hypothetical axis

Hypothetical axis

1010

Current values X 28.284 (diameter value display) C 45.000

(5) Milling interpolation is also available for a two-control-axis system consisting of one linear axis and one rotation axis. The X axis must be used as the linear axis. The rotation and milling hypothetical axes are selected as shown above. In milling mode, the G17 plane must be selected.

(6) The table below lists the incremental axis names of the hypothetical axis used in milling mode. These axis commands handle radius commands only.

Selected hypothetical axis Absolute axis name Incremental axis name

Y axis Y V Rotation axis (C) Rotation axis name (C) Rotation axis incremental name (H)

(The following description uses Y for the hypothetical axis name and C for the rotation axis name.)

6. Interpolation Functions 6.8 Milling Interpolation

76

6.8.3 Selecting a Plane during the Milling Mode

Function and purpose

A plane selection command decides the plane on which the tool moves for circular interpolation or tool radius compensation in milling mode.

Command format

G17/G19 ; G16 C__ ;

G16 Y-Z cylindrical plane C Cylindrical radius value G17 X-Y plane G19 Y-Z plane

(1) These G commands for plane selection are modal. The G17 plane is automatically selected as the default each time the turning mode is switched to the milling mode by a G12.1 command. When the milling mode is switched back to the turning mode by a G13.1 command, the plane that was selected before the milling mode is entered is restored.

(2) G16 or G19 can also be defined as the default effective when a G12.1 command is issued. A parameter is used for this.

(3) The three planes selected are explained below.

(a) G16 G16 indicates the plane obtained by developing a cylinder with its bottom radius X. This is useful to process the side face of a workpiece.

X

Z

Y

Y-Z cylindrical plane

6. Interpolation Functions 6.8 Milling Interpolation

77

(b) G17

G17 is an X-Y plane in an XYZ orthogonal coordinate system. This is useful to process the end face of a workpiece.

X

Y

Z

X-Y plane

(c) G19

G19 is a Y-Z plane in an XYZ orthogonal coordinate system.

Center of workpiece

X

Y

Z

Y-Z plane

6. Interpolation Functions 6.8 Milling Interpolation

78

6.8.4 Setting Milling Coordinate System

Function and purpose

The coordinate system for the milling mode is set according to the selected plane each time the turning mode (G13.1) is switched to the milling mode by a G12.1 command.

G17 and G19 planes

(1) For the X and Z axes, the current positions are set as radius value on the coordinate value.

(2) The Y axis is decided as the axis which intersects the X and Z axes at right angles. Y=0 is defined in a G12.1 command.

Z

Tool X

Y

(Note1) During the milling mode on the G17 plane, the X axis is operated in the area (positive or negative side) that has existed before issuing the G12.1 command. When you want to control the X axis in the positive side during the milling mode, moving the X axis to the positive area (including 0) is required before issuing the G12.1 command. When you want to control the X axis in the negative side during the milling mode, moving the X axis to the negative area (not including 0) is required before issuing the G12.1 command.

G16 plane

(1) To select a G16 plane, the radius value of a cylinder is specified by "G16 C__ ;". If no radius

value is specified, the current X axis value is used as the radius value to define a cylinder. If no radius value can be defined, a program error (P485) occurs.

(2) As in normal turning mode, the X axis indicates the distance from the center line of the workpiece.

(3) G16 (Y-Z cylindrical plane) is actually the side of a cylinder.

(4) The X axis indicates the distance from the center line of the workpiece. The Y axis indicates the circumference with the radius value of the bottom of a cylinder defined by a G16 command.

6. Interpolation Functions 6.8 Milling Interpolation

79

(5) The zero point of the Y axis is the position where a G12.1 command is issued.

(Example)

: : G12.1 G16 C50. ; : : :

or

: : G12.1 ; G16 C50. ; : :

or

: : G12.1 Ee,Dd ; G16 C50. ; : :

or

: : G12.1 Ee,Dd ; G16 C50. ; : :

Z

X

Y

r

6. Interpolation Functions 6.8 Milling Interpolation

80

6.8.5 Preparatory Functions

Valid G codes in milling mode

Classifi- cation G code Function Classifi-

cation G code Function

G00 Positioning G65 Macro call G01 Linear interpolation G66 Macro modal call A G02 Circular interpolation (CW) G66.1 Macro modal call B G03

Circular interpolation (CCW) G67 Macro modal call cancel

G04 Dwell G09 Exact stop check G80 Hole drilling cycle cancel G83 Deep hole drilling cycle (Z axis) G13.1 Turning mode G84 Tap cycle (Z axis) G85 Boring cycle (Z axis) G87 Deep hole drilling cycle (X axis) G16 Y-Z cylindrical plane selection G88 Tap cycle (X axis)

G17 X-Y plane selection G89 Boring cycle (X axis) G90 Absolute value command G19 Y-Z plane selection G91 Incremental value command G22 Barrier check ON G94 Asynchronous feed G23 Barrier check OFF G98 Hole drilling cycle initial point

return G99 Hole drilling cycle R point return G61 Exact stop mode G40 Tool radius compensation

cancel

G41 Tool radius compensation left G64 Turning mode G42 Tool radius compensation right

: Milling interpolation command : G code effective only in milling mode

(1) If an invalid G code is issued in milling mode, a program error (P481) occurs.

If the milling interpolation is commanded in milling mode, a program error (P481) occurs.

(2) In milling mode, all movement commands are commanded with the coordinate system determined by the selected machining plane. The rotation axis thus cannot be moved by a direct command in milling mode. To perform milling at a specific position of a workpiece, therefore, positioning must have been made in turning mode.

(Example)

: : G0 X100. C180.; Positioning before milling G12.1; (or G12.1 E=C,D0;) G0 X50.; : :

(3) If a command for an axis other than X, Z, and Y (rotation axis) is issued in milling mode, a program error (P481) occurs. The asynchronous tap can be used during the milling mode; however, the synchronous tap must not be commanded.

6. Interpolation Functions 6.8 Milling Interpolation

81

(4) In milling mode, the Y axis can be specified by only four G codes: G00, G01, G02, and G03.

These are called the milling interpolation commands. (5) The G84, G88 synchronous tapping cycles cannot be used during the milling mode.

Positioning (G00)

If a G00 command is issued in milling mode, positioning is made to the specified point on the selected plane at a rapid traverse rate.

G00 X/U__ Y/V__ Z/W__ ;

Linear interpolation (G01)

If a G01 command is issued in milling mode, linear interpolation is made to the specified point on the selected plane at the speed specified by an F speed. (1) G16 mode

Program format

G01 Y/V__ Z/W__ X/U__ F__ ;

Development

Z X

z

y Y

z

y

E

S

S

E

6. Interpolation Functions 6.8 Milling Interpolation

82

(2) G17 mode

Program format

G01 X/U__ Y/V__ Z/W__ F__ ;

A

Z

X

S

Y

x

y

z E

E

(3) G19 mode Program format

G01 Y/V__ Z/W__ X/U__ F__ ;

A Z

X

S

Y

x

y z

E

E

6. Interpolation Functions 6.8 Milling Interpolation

83

Circular interpolation (G02/G03)

If a G02 or G03 command is issued in milling mode, circular interpolation is performed at the specified speed on the selected plane.

(1) G16 mode

G02/G03 Y/V__ Z/W__ J__ K__ F__ ; or G02/G03 Y/V__ Z/W__ R__ F__ ;

G02 Circular interpolation (clockwise) G03 Circular interpolation (counterclockwise) Y/V Circular end point coordinate, Y axis (Y: absolute value, V:

incremental value) Z/W Circular end point coordinate, Z axis (Z: absolute value, W:

incremental value) J/K Circular center incremental value (radius command

incremental value from the start point to the center) R Circular radius F Feed rate

Development

S

(A, Q) E

X Z

Z

(A, Q) k j

Y

S

E

6. Interpolation Functions 6.8 Milling Interpolation

84

(2) G17 mode

G02/G03 X/U__ Y/V__ I__ J__ F__ ; or G02/G03 X/U__ Y/V__ R__ F__ ;

X/U Circular end point coordinate, X axis (X: absolute value, U: incremental value)

Y/V Circular end point coordinate, Y axis (Y: absolute value, V: incremental value)

I/J Circular center incremental value (incremental value from the start point to the center)

R Circular radius F Feed rate

Z

(A, Q)

S

E

X

Q

i

j

A

Y

(3) G19 mode

G02/G03 Y/V__ Z/W__ J__ K__ F__ ; or G02/G03 Y/V__ Z/W__ R__ F__ ;

Y/V Circular end point coordinate, Y axis (Y: absolute value, V: incremental value)

Z/W Circular end point coordinate, Z axis (Z: absolute value, W: incremental value)

J/K Circular center incremental value (incremental value from the start point to the center)

R Circular radius F Feed rate

Z

S

E

Q

X

A

Y k

j

6. Interpolation Functions 6.8 Milling Interpolation

85

6.8.6 Switching from Milling Mode to Turning Mode; G13.1

Detailed description

(1) A G13.1 command is used to cancel the milling mode and return to the turning mode.

(2) The G13.1 command is effective if the following requirement is met. If not, a program error (P485) occurs.

(a) Tool radius compensation has been canceled.

(3) The G13.1 command restores the plane selected before the preceding G12.1 command was issued.

(4) The G13.1 command restores the mode (synchronous or asynchronous) and the F value (if in asynchronous mode) selected before the preceding G12.1 command was issued.

(Note 1) If G13.1 is executed, while no movement command has been given, after cancellation by

an independent G40 command, tool radius compensation is canceled in the G13.1 block. (Note 2) When G13.1 command is issued, the deceleration check is executed. (Note 3) If another command is issued during the G13.1 command, a program error will occur.

6.8.7 Feed Function

Asynchronous cutting feed

An asynchronous feed mode (G94 command) can use F6.3 digits to specify the feed rate per minute in units of 0.001mm/min. The specifiable range is 0.001 to 999999.999mm/min. If the effective speed exceeds the cutting feed clamp speed, it is clamped by that clamp speed.

(Note 1) Whenever the turning mode is switched to the milling mode by a G12.1 command, the F

command modal value is canceled. After mode change, therefore, the feed rate must be set by an F command.

(Note 2) A G12.1 command forces the mode to shift to the asynchronous mode. (Note 3) When the milling mode is canceled by a G13.1 command, both the feed mode and F

command modal value return to the original state before the preceding G12.1 command was issued.

6.8.8 Program Support Functions

Relation with other functions

The following program support functions are effective in milling mode: (1) Linear angle command (2) Variable command (3) Automatic corner chamfering/corner rounding (4) Geometric function (5) Hole drilling cycle (6) Subprogram function (7) User macro

6. Interpolation Functions 6.8 Milling Interpolation

86

6.8.9 Miscellaneous Functions

Relation with other functions

(1) M and B commands can be issued in milling mode.

(2) In milling mode, an S command specifies not the spindle rotation speed but the rotary tool speed.

(3) If a T command is issued in milling mode, a program error (P485) occurs. Before a G12.1 command is issued, therefore, tool selection must be done.

: T1212 ; Specify a T command before a G12.1 command. G0 X100. Z0. ; G12.1 ; (or G12.1 E=C,DO ;) : T1200 ; In milling mode, a T command causes a program error (P485). : G13.1 ;

(4) Complete the tool compensation operation (movement of tool length and wear compensation amount) before executing the milling interpolation. If the tool compensation operation is not completed when the milling interpolation start command has been issued, the followings will be resulted: Machine coordinate is not changed even if G12.1 is executed. The workpiece coordinate is changed to that of the post tool length compensation when G12.1 is executed. (Even if canceling the milling interpolation, this workpiece coordinate will not be canceled.)

(Example) Workpiece coordinate offset (X axis)=20. Tool compensation amount of T0101 (X axis)=100. Setting compensation operation with movement command after T command

: [X axis] [C axis] [X axis] [C axis] G00 X200. C0.; 200. 0. 220. 0. T0101; 200. 0. 220. 0. G12.1; 100. 0. 220. 0. <-The workpiece coordinate system

is shifted (without moving the axis) G01 X50. F1000; 50. 0. 170. 0. :

6. Interpolation Functions 6.8 Milling Interpolation

87

6.8.10 Tool Offset Functions

Tool length offset

(1) In milling mode, tool compensation is performed by adding the tool length offset amount

specified on the cutting coordinates converted from the milling coordinate system.

Tool length offset

Tool position

X X

Y

Y

Y

X : Tool position

Y X

Milling coordinate system Actual tool position

Movement on the milling coordinate system

6. Interpolation Functions 6.8 Milling Interpolation

88

(2) As in (1) on previous page, if the offset amount is different from the actual one, the shape is not

corrected normally.

(a) If the offset amount is larger than tool length:

Example: The actual tool length is 15.0 when tool length X = 20.0

Milling command

Actual shape

Tool movement

Y

X

6. Interpolation Functions 6.8 Milling Interpolation

89

(b) If the offset amount is smaller than tool length:

Example: The actual tool length is 25.0 when tool length X = 20.0

Milling command

Actual shape

Tool movement

X

Y

Tool radius compensation

The workpiece shape can be compensated in the direction of the vector by the radius amount of the tool specified by a G command (G40 to G42) and selected compensation No.

Command format

G40 X__ Y__ ; Tool radius compensation cancel G41 X__ Y__ ; Tool radius compensation (left) G42 X__ Y__ ; Tool radius compensation (right)

(1) A tool radius compensation command must be issued after the milling mode is entered. The tool radius compensation command must be canceled before the turning mode is

restored.

(2) A tool compensation No. must be specified before the milling mode is entered (before a G12. 1 command is issued).

A T command in milling mode causes a program error (P485).

(3) Tool radius compensation is performed on the selected plane.

G17 plane ... XY axes G19 plane G16 plane

YZ axes

6. Interpolation Functions 6.8 Milling Interpolation

90

Tool radius compensation cancel mode

Tool radius compensation is canceled under either of the following conditions: (1) While a G12.1 command is effective

(2) After a compensation cancel command (G40) is issued In the compensation cancel mode, the offset vector is 0 and the tool center path matches the programmed path. A program that contains tool radius compensation must end after the compensation is canceled.

Starting tool radius compensation (startup)

Tool radius compensation starts if all the following requirements are met in compensation cancel mode: (1) A G41 or G42 command is issued.

(2) The tool radius compensation No. is greater than 0 and equal to or less than the maximum compensation No.

(3) The movement command is not a circular command. Whether in continuous or single block operation, compensation always starts after reading three movement command blocks, or if three movement command blocks are not found, up to five continuous blocks. Similarly, in compensation mode, up to five blocks are pre-read for compensation operation.

Control state diagram

Starting to pre-read five blocks

T___; S___; G00___; G41___; G01___; G02___; Machining program

Pre-read buffer

Executed block

G02_; G01_;G41_;G00_;S_; T_;

G02_;G01_;

G02_;G01_;G41_;G00_;S_;T_;

There are two ways of starting tool radius compensation: type A and type B. The type depends on the selection of the control parameter "tool nose compensation type B". This type is used in common with the compensation cancel type. In the following explanatory figure, "S" denotes the single block stop point.

6. Interpolation Functions 6.8 Milling Interpolation

91

Start operation for tool radius compensation

(1) Machining an inside corner

Linear Linear Linear Circular

Tool center path

Program path r = Compensation amount

s

G42

Start point

Program path

Tool center path

Center of circular

Start point

G42

s

r

(2) Machining an outside corner (obtuse angle) (Type A or B can be selected by parameter) [90 < 180]

Linear Linear (Type A) Linear Circular (Type A)

Tool center path

Program path

r = Compensation amount

s

G41

Start point Program path

Tool center path

Center of circular

Start point

G41

s

r

Linear Linear (Type B) Linear Circular (Type B)

Start point

Tool center path

Program path

s

G41

Program path

Tool center path

Center of circular

Start point

G41

s

r

r r r

Intersection Intersection

6. Interpolation Functions 6.8 Milling Interpolation

92

(3) Machining an outside corner (acute angle) (Type A or B can be selected by parameter)

[ < 90]

Linear Linear (Type A) Linear Circular (Type A)

Program path

Tool center path

Center of circular

Start point

G41

s

r

Tool center path

Program path s

r

Start point

G41

Linear Linear (Type B) Linear Circular (Type B)

Program path

Tool center path

Center of circular

Start point

G41

s

r

Tool center path

Program path

s

r

r

Start point

G41

r

6. Interpolation Functions 6.8 Milling Interpolation

93

Operations in compensation mode

Compensation is valid both for positioning and for interpolation commands such as circular and linear interpolation. Even if the same compensation command (G41 or G42) is specified in the compensation mode, the command will be ignored. If four or more blocks not accompanying movement are assigned continuously in the compensation mode, over-cutting or under-cutting will result.

(1) Machining an outside corner

Linear Linear (90 < 180) Linear Circular (0 < < 90)

Program path

Tool center path Intersection

s

Program path

Tool center path

s

r

r

Linear Circular (90 < 180) Linear Circular (0 < < 90)

Program path

Tool center path

Center of circular

s

Program path

Tool center path

s

r

rr r

Center of circular

Circular Linear (90 < 180) Circular Linear (0 < < 90)

Program path

Tool center path

Center of circular

s

Program path

Tool center path

s

r

r

r r

Center of circular

Intersection

6. Interpolation Functions 6.8 Milling Interpolation

94

Circular Circular (90 < 180) Circular Circular (0 < < 90)

r

s

r

s

r r

Program path

Center of circular Center of circular

Tool center path Tool center path

Center of circular

Intersection

Program path

Center of circular

(2) Machining an inside corner

Linear Linear (Obtuse angle) Linear Linear (Obtuse angle)

r r

r

s s

Program path

Tool center path Intersection

Program path

Tool center path

Linear Circular (Obtuse angle) Linear Circular (Obtuse angle)

r

s

r

r

s

Program path

Tool center path Inter- section

Center of circular

Tool center path

Center of circular

Intersection

Program path

Circular Linear (Obtuse angle) Circular Linear (Obtuse angle)

s r

r

s

Program path

Tool center path

Center of circular

Program path

Tool center path Inter- section

Center of circular

Inter- section

6. Interpolation Functions 6.8 Milling Interpolation

95

Circular Circular (Obtuse angle) Circular Circular (Acute angle)

Program path

Tool center path

Center of circular

s

Program path

Tool center path

s

r

r

Center of circular

Center of circular

Intersection

Inter- section

Center of circular

(3) When the arc end point is not on the circular

With a spiral circular command: the area from the arc start point to the end point is interpolated as a spiral arc. With a normal circular command: if the error after compensation is within the parameter value, it is interpolated as a spiral arc.

Program path

Tool center path

Center of circular

s r

End point of circular

Hypothetical circle

r

R

(4) When the inside intersection does not exist In an instance such as that shown in the figure below, the intersection of arcs A and B may cease to exist due to the compensation amount. In such cases, program error (P152) appears, and the tool stops at the end point of the preceding block.

Program path

Tool center path Center of circular A

A

r

B

r

Program error stop

Linear intersecting circulars A and B

6. Interpolation Functions 6.8 Milling Interpolation

96

Tool radius compensation cancel

If either of the following conditions is met in the tool radius compensation mode, the compensation will be canceled. However, the movement command must be a command other than a circular command. If an attempt is made to cancel the compensation by a circular command, program error (P151) results.

(1) A G40 command has been executed.

The cancel mode is established once the compensation cancel command has been read, the 5-block pre-read process is suspended, and 1-block pre-read applies instead.

Tool radius compensation cancel operation

(1) Machining an inside corner

Linear Linear Circular Linear

Program path

Tool center path

End point

s

r = Compensation amount

G40

Program path

Tool center path

Center of circular

s

r

End point

G40

6. Interpolation Functions 6.8 Milling Interpolation

97

(2) Machining an outside corner (obtuse angle) (Type A or B can be selected by parameter) [90 < 180]

Linear Linear (Type A) Circular Linear (Type A)

Program path

Tool center path

End point

s

r = Compensation amount

G40

Program path

Tool center path

Center of circular

s

r

End point

G40

Linear Linear (Type B) Circular Linear (Type B)

Program path

Tool center path

End point

s

G40

Program path

Tool center path

Center of circular

s

r

End point

G40

r r

Intersection

r

Intersection

6. Interpolation Functions 6.8 Milling Interpolation

98

(3) Machining an outside corner (acute angle) (Type A or B elm be selected by parameter)

[ < 90]

Linear Linear (Type A) Circular Linear (Type A)

Program path

Tool center path

End point

s

G40

Program path

Tool center path

Center of circular

s

r

End point

G40

r

Linear Linear (Type B) Circular Linear (Type B)

Program path

Tool center path

End point

s

G40

Program path

Tool center path

Center of circular

s

r

End point

G40

r

r

6. Interpolation Functions 6.8 Milling Interpolation

99

Changing the compensation direction during tool radius compensation

The compensation direction can be changed by changing the compensation command in the compensation mode without the compensation having to be first canceled. However, no change is possible in the compensation start block and the following block.

Linear Linear

Program path

Tool center path

r

G41 G41 G42

r

r

Intersection

If there is no intersection when the compensation direction is changed.

Linear Circular

Program path

Tool center path

r

G41 G42 G41

r

r

G41 G42

r

r

r

6. Interpolation Functions 6.8 Milling Interpolation

100

Circular Circular

Program path

Tool center path

G41

G41 G42

r

Center of circular

Center of circular

G41

G41

G42

r

Linear return

Program path

Tool center path G42

G41

r

G0 block

If there is a block containing a G0 command, the preceding block does not perform intersection operation, the tool comes to the position vertical to the end point, and the G0 block temporarily loses the offset vector. Compensation is not canceled, but instead the tool moves from the intersection vector directly to a point without vector, that is, to the point specified by the program. The offset vector is regenerated by a block containing a G1 command.

N15

N17

N16

N12 N13

N14

Y

X

(Unit: mm)

: : N10 G12.1; N11 G42; N12 G1 Y100..F100; N13 X-100.; N14 G0 Y-100.; N15 G1 X100.; N16 Y0.; N17 G40 G0 X200.; : :

6. Interpolation Functions 6.8 Milling Interpolation

101

Blocks without movement and M commands inhibiting pre-read

The following blocks are known as blocks without movement;

a. M03 ; ............................................M command b. S12 ; .............................................S command c. G04 X500 ; ...................................Dwell d. G10 P01 R50 ;..............................Compensation amount setting e. (G17) Z40 ; ...................................Movement but not on compensation plane f. G90 ;.............................................G code only g. G91 X0 ; .......................................Movement amount 0

M00, M01, M02, and M30 are treated as M codes inhibiting pre-read. ................... Zero movement amount

(1) Blocks without movement commands specified at compensation start If four or more blocks without movement continue or if M command inhibiting pre-read is issued, offset vectors are not generated.

N1 X30. Y60.; N2 G41; N3 G4 X1000; N4 F100; N5 S500; N6 M3; N7 X20. Y50.; N8 X50. Y20.;

Block without movement

N2, 3, 4, 5, 6

N1 N7

(Intersection) N8

(2) Blocks without movement commands specified in compensation mode If four or more blocks without movement do not continue in compensation mode and if no M command inhibiting pre-read is issued, intersection vectors are generated as usual.

N6 G91 X100. Y200.; N7 G04 X P1000; ....... N8 X200.;

Block without movement

N6 N8

Block N7 is executed here.

N6

N7 N8

If four or more blocks without movement continue or if M command inhibiting pre-read is issued, offset vectors are generated perpendicularly at the end point of the preceding block.

This may cause cutting.

N6 X100. Y200.; N7 G4 X1000; N8 F100; N9 S500; N10 M4; N11 X100.;

Block without movement

N6

N6

N11

N7 to 10

N11

No movement

6. Interpolation Functions 6.8 Milling Interpolation

102

(3) Compensation cancel alone

(a) G1 precedes the block containing G40:

N10

N11

N12

Compensation is canceled by a movement command following G40.

(b) G0 precedes the block containing G40:

N20

N21

N22

Compensation is canceled by a G0 command before G40.

(Note) In program (a), if G13.1 is commanded after G40 without a movement command, cancellation is done at block G13.1.

Corner movement

When a multiple number of offset vectors are created at the joints between movement command blocks, the tool will move in a straight line between those vectors. This action is called corner movement. When the vectors do not match, the tool moves in order to turn the corner although this movement belongs to the next block. Consequently, operation in the single block mode will execute the previous block + corner movement as a single block and the remaining joining movement + next block will be executed as a single block in the following operation.

N2

N1 Program path

Center of circular

Stop point in single block mode

r

r Tool center path

This movement and feed rate are under block N2.

: N10 G1 X__ Y__; N11 G40; N12 G0 X__ Y__;

: N20 G1 X__ Y__; N21 G0 X__ Y__; N22 G40;

6. Interpolation Functions 6.8 Milling Interpolation

103

6.8.11 Interference Check

Function and purpose

A tool, whose tool radius has been compensated under the tool radius compensation function by the usual 2-block pre-reading, may sometimes cut into the workpiece. This is known as interference. An interference check is the function which prevents such interference from occurring. The types of interference check are indicated below, and each can be selected for use by parameter.

Function Parameter Operation Interference check alarm function

Rad compen intrf byp : OFF Interference check invalid signal OFF

Operation stops with a program error before execution of the block causing cutting.

Interference check avoiding function

Rad compen intrf byp : ON Interference check invalid signal OFF

The tool path is changed to prevent cutting from occurring.

(Example)

Avoided path

Tool outside diameter

N1 N3

N2

Cutting by N2

(G41)

N1 G90 G1 X50. Y-100. ;

N2 X70. Y-100. ;

N3 X120. Y0 ;

Cutting by N2

(1) With alarm function

An alarm is given before N1 is executed. The buffer correction function can thus be used to change N1 to the following, enabling machining to continue: N1 G1 X20. Y-40.;

(2) With avoidance function

The intersection of N1 and N3 is calculated to create interference avoidance vectors.

6. Interpolation Functions 6.8 Milling Interpolation

104

(4)(3)(2)

(1)

(1)

N1

N3

N2

(4)

(2) (3)

Examples of interference check:

Vector (1) (4) check No interference Vector (2) (3) check No interference Vector (3) (2) check Interference Vectors (3) (2) deleted Vectors (4) (1) deleted As a result of the above processing, vectors (1) (2) (3) , and (4) remain as valid, and operation is done with the path connecting these vectors as the interference avoidance path.

6. Interpolation Functions 6.8 Milling Interpolation

105

Detailed description

(1) Conditions regarded as interference

With three blocks containing movement commands of five pre-read blocks, interference is regarded as occurring if the compensation calculation vectors, which have been created at contact of movement commands, intersect each other.

N1 N3

N2

r

Tool center path

Program path

Vectors intersect here.

(2) Interference check is not available when:

(a) Three blocks containing movement commands cannot be pre-read (three or more blocks of five pre-read blocks do not contain movement commands).

(b) Interference occurs in the fourth or subsequent block containing movement commands.

N1

N3

N2

Program path

Tool center path

No interference check available

N4

N5

N6

(3) Operation during interference avoidance

If the interference avoidance function is available, the tool moves as follows.

N1 N3

N2

Program path Tool center path

6. Interpolation Functions 6.8 Milling Interpolation

106

Program path

Center of circular

Linear movement

N1

N3

N1

N2

r

r

N2

N3

Tool center path when interference check is invalid

Tool center path when interference is avoided

Solid line : Interference avoidance path Broken lines : Interference check invalid

Program path

Tool center path when interference check is invalid

Tool center path when interference is avoided

Program path

Tool center path 2

Tool center path 1

N1

N3

N2

r1

N4

r2

r1 r2

Avoidance vector 2

Avoidance vector 1

N1

N3

N2

Tool center path

Program path

Avoidance vector

Avoidance vector

If all interference avoidance line vectors have been deleted, new avoidance vectors are created to avoid interference as shown in the figure at right.

6. Interpolation Functions 6.8 Milling Interpolation

107

In the figure below, the groove is left uncut.

Nose R center path

Interference avoidance path

Program path

Solid line : Interference avoidance path Broken lines : Interference check invalid path

In the figure below, the tool moves in the opposite direction at N2. After N1 is executed, program error (P153) occurs.

N1

N2 N3

N4

1 2 3 4

Interference check alarm

An interference check alarm occurs under the following conditions.

(1) With the interference check alarm function selected

(a) All vectors are deleted at the end point of the current block. As shown in the figure, if vectors 1 to 4 are all deleted at the end point of the N1 block,

program error (P153) results prior to N1 execution.

N1

2 3

N2 1

N3 4

6. Interpolation Functions 6.8 Milling Interpolation

108

(2) With the interference check avoidance function selected

(a) There are valid vectors at the end point of the following block though all vectors at the end point of the current block were deleted.

(i) In the figure, if N2 interference check is conducted, the N2 end point vectors are all deleted but the N3 end point vectors are regarded as valid.

This causes program error (P153) at the N1 end point.

N1

2 N2 1

N3 43

N4

Alarm stop

(ii) In the figure, the tool moves in the opposite direction at N2. This causes program error (P153) after N1 execution.

N1

N2 N3

N4

1 2 3 4

6. Interpolation Functions 6.8 Milling Interpolation

109

(b) The avoidance vectors cannot be created. As shown in the figure, even when the conditions for creating avoidance vectors are met, it

may still be impossible to create avoidance vectors or the avoidance vectors may interfere with N3. Program error (P153) thus occurs at the N1 end point if the vectors intersect at an angle of 90 or more.

N1

N2

N3

N4

Alarm stop

N1

N2

N3

N4

Alarm stop

Angle of intersection

6. Interpolation Functions 6.8 Milling Interpolation

110

(c) The program advance direction and the advance direction after compensation are

reversed. An interference may be assumed when no interference occurs actually if grooves running

in parallel with narrower width between the two than the tool diameter or a bottom-widened groove is programmed.

Stop

Program path Tool center path

Stop

6. Interpolation Functions 6.9 Cylindrical Interpolation

111

6.9 Cylindrical Interpolation; G07.1 (6 and 7 only in G code list)

Function and purpose

This function develops a shape with a cylindrical side (shape in cylindrical coordinate system) into a plane. When the developed shape is programmed as the plane coordinates, that is converted into the linear axis and rotation axis movement in the cylindrical coordinates and the contour is controlled during machining.

X Hypothetical C

Z

C r

As programming can be carried out with a shape with which the side on the cylinder is developed, this is effective for machining cylindrical cams, etc. When programmed with the rotation axis and its orthogonal axis, slits, etc., can be machined on the cylinder side.

Develop- ment

0

360

2r

6. Interpolation Functions 6.9 Cylindrical Interpolation

112

Command format

G07.1 C__ ; (Cylindrical interpolation mode start/cancel) C Cylinder radius value

Radius value 0: Cylindrical interpolation mode start Radius value = 0: Cylindrical interpolation mode cancel

(Note) The above format applies when the name of the rotation axis is "C". If the name is not "C",

command the name of the rotation axis being used instead of "C". (1) The coordinates commanded in the interval from the start to cancellation of the cylindrical

interpolation mode will be the cylindrical coordinate system. G07.1 C Cylinder radius value; 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)

(2) G107 can be used instead of G07.1.

Detailed description

(1) Command G07.1 in an independent block. A program error (P33) will occur if this command is

issued in the same block as another G code.

(2) Program the rotation axis with an angle degree.

(3) Linear interpolation or circular interpolation can be commanded during the cylindrical interpolation mode. Note that the plane selection command must be issued just before the G07.1 block.

(4) The coordinates can be commanded with either an absolute command or incremental command.

(5) Tool radius compensation can be applied on the program command. Cylindrical interpolation will be executed on the path after tool radius compensation.

(6) Command the segment feed in the cylinder development with F. The F unit is mm/min or inch/min.

(7) Cylindrical interpolation accuracy In the cylindrical interpolation mode, the movement amount of the rotation axis commanded

with an angle is converted on the circle periphery, and after operating 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 error generated at this time is not cumulated.

6. Interpolation Functions 6.9 Cylindrical Interpolation

113

(8) Related parameters

# Item Details Setting range

1516 mill_ax Milling axis name

Set the name of the rotation axis for milling interpolation (polar coordinate interpolation, cylindrical interpolation). Only one of the rotation axes can be set.

A to Z

8111 Milling Radius Select the diameter and radius of the linear axis for milling interpolation (polar coordinate interpolation, cylindrical interpolation). 0: Radius command for all axes 1: Each axis setting (follows #1019 dia diameter

designation axis)

0 / 1

1267 (PR)

ext03 (bit0)

G code type The type of high-speed high-accuracy G code is changed. 0: G61.1 type 1: G8 type

0 / 1

1270 (PR)

ext06 (bit7)

Handle C axis coordinate during cylindrical interpolation

Specify whether the rotary axis coordinate before the cylindrical interpolation start command is issued is kept during the cylindrical interpolation or not. 0: Do not keep 1: keep

0 / 1

(9) Plane selection

The axis used for cylindrical interpolation must be set with the plane selection command. (Note) The correspondence of the rotation axis to an axis' parallel axis is set with the parameters (#1029, #1030, #1031). 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 not set and a movement command is issued, a program error (P485) will occur.

6. Interpolation Functions 6.9 Cylindrical Interpolation

114

(Example)

Basic coordinate system X, Y, Z

Cylindrical coordinate system C, Y, Z (Rotation axis is X axis' parallel axis) #1029

Cylindrical coordinate system X, C, Z (Rotation axis is Y axis' parallel axis) #1030

Cylindrical coordinate system X, Y, C (Rotation axis is Z axis' parallel axis) #1031

G17

Y

X

G18

Z

X

G19

Y

Z

G18

Z

C

G18

C

X

G19

C

Z

G19

Y

C

G17

X

C

G17

C

Y

G19 Z0. C0. ;

G07.1 C100. ;

:

G07.1 C0 ;

(Note) Depending on the model or version, the Z-C plane (Y-Z cylinder plane) will be automatically

selected with G07.1 and G19. The circular interpolation and tool radius compensation, etc., can be designated on that

plane.

G17 G18 G19 Y

X

X

Z

Z

Y

G19

Z

C

Basic coordinate system X, Y, Z

Cylindrical coordinate system

6. Interpolation Functions 6.9 Cylindrical Interpolation

115

Relation with other functions

(1) Circular interpolation

(a) Circular interpolation between the rotation axis and linear axis is possible during the cylindrical interpolation mode.

(b) An R specification command can be issued with circular interpolation. (I, J and K cannot be designated.)

(2) Tool radius compensation The tool radius can be compensated during the cylindrical interpolation mode.

(a) Command the plane selection in the same manner as circular interpolation. When using tool radius compensation, start up and cancel the compensation within the

cylindrical interpolation mode.

(b) A program error (P485) will occur if G07.1 is commanded during tool radius compensation.

(c) If the G07.1 command is issued with no movement command given after the tool radius compensation is canceled, the position of the axis in the G07.1 command block is interpreted as the position applied after the tool radius compensation is canceled and the following operations are performed.

(3) Cutting feed per minute (asynchronous feed)

(a) The feed per minute (asynchronous) mode is forcibly set when the cylindrical interpolation mode is started.

(b) When the cylindrical interpolation mode is canceled, the feed per revolution (synchronous) will return to the state before the cylindrical interpolation mode was started.

(4) Constant surface speed control

(a) A program error (P485) will occur if G07.1 is commanded in the constant surface speed control mode (G96).

(5) Miscellaneous functions

(a) The miscellaneous function (M) and 2nd miscellaneous function can be issued even in the cylindrical interpolation mode.

(b) The S command in the cylindrical interpolation mode issues the rotary tool's rotation speed instead of the spindle rotation speed.

(c) Issue the T command before cylindrical interpolation is started. A program error (P485) will occur if the T command is issued in the cylindrical interpolation mode.

: : T1212 ; ... T command before cylindrical interpolation Valid T0 X100. Z0 ; G19 Z C ; G07.1 C100. ; : T1200 ; ... T command in cylindrical interpolation mode Program error : G07.1 C0 ;

6. Interpolation Functions 6.9 Cylindrical Interpolation

116

(d) Complete the tool compensation movement (movement of tool length and wear compensation amount) before executing the cylindrical interpolation. If the tool compensation movement is not completed when the cylindrical interpolation start command has been issued, the followings will be resulted: Machine coordinate is not changed even if G07.1 is executed. The workpiece coordinate is changed to that of the post tool length compensation when G07.1 is executed. (Even if canceling the cylindrical interpolation, this workpiece coordinate will not be canceled.)

(6) F command during cylindrical interpolation As for the F command in the cylindrical interpolation mode, whether the previous F command

is used or not depends on that the mode just before G07.1 is the feed per minute command (G94) or feed per revolution command (G95).

(a) When G94 is commanded just before G07.1 If there is no F command in the cylindrical interpolation, the previous F command feed rate

will be used. The feed rate after the cylindrical interpolation mode is canceled will remain the F

command feed rate issued when the cylindrical interpolation mode was started or the final F command feed rate set during cylindrical interpolation.

(b) When G95 is commanded just before G07.1 The previous F command feed rate cannot be used during cylindrical interpolation, thus a

new F command must be issued. The feed rate after the cylindrical interpolation mode is canceled will return to that applied

before the cylindrical interpolation mode was started.

When there is no F command in G07.1 Previous mode No F command After G07.1 is canceled G94 Previous F is used G95 Program error (P62) F just before G07.1 is used

When F is commanded in G07.1

Previous mode No F command After G07.1 is canceled G94 Commanded F is used G95 Commanded F is used *1 F just before G07.1 is used

*1) Moves with the feed per minute command during G07.1.

6. Interpolation Functions 6.9 Cylindrical Interpolation

117

Restrictions and precautions

(1) The following G code commands can be used during the cylindrical interpolation mode.

G code Details G00 G01 G02 G03 G04 G09 G22/23 G40-42 G50.2 G61 G64 G65 G66 G66.1 G67 G79-89 G90/91 G94 G98 G99

Positioning Linear interpolation Circular interpolation (CW) Circular interpolation (CWW) Dwell Exact stop check Chuck barrier ON/OFF Tool nose R compensation Polygon machining mode cancel Exact stop check mode Cutting mode Macro call (simple call) Macro modal call A (modal call) Macro modal call B (block call per macro) Macro modal call cancel (modal call cancel) Fixed cycle for drilling Absolute/incremental value command Asynchronous feed Hole drilling cycle initial return Hole drilling cycle R point return

A program error will occur if a G code other than those listed above is commanded during cylindrical interpolation.

(2) The cylindrical interpolation mode is canceled when the power is turned ON or reset.

(3) A program error (P484) will occur if any axis commanded for cylindrical interpolation has not completed reference position return.

(4) Tool radius compensation must be canceled before the cylindrical interpolation mode can be canceled.

(5) When the cylindrical interpolation mode is canceled, the mode will change to the cutting mode, and the plane will return to that selected before cylindrical interpolation.

(6) The program of the block during the cylindrical interpolation cannot be restarted (program restart).

(7) A program error (P486) will occur if the cylindrical interpolation command is issued during the mirror image.

(8) When the cylindrical interpolation mode is started or canceled, the deceleration check is performed.

(9) A program error (P481) will occur if the cylindrical interpolation or the polar coordinate interpolation is commanded during the cylindrical interpolation mode.

(10) The G84 or G88 synchronous tapping cycles cannot be used during cylindrical interpolation mode. The asynchronous tap can be used during cylindrical interpolation mode; however, the synchronous tap must not be commanded.

6. Interpolation Functions 6.9 Cylindrical Interpolation

118

Example of program

#1029 aux_I #1030 aux_J C #1031 aux_K

Command of plane selection for cylindrical interpolation and command of two interpolation axes Cylindrical interpolation start Cylindrical interpolation cancel

N01 G28XZC; N02 T0202; N03 G97S100M23; N04 G00X50.Z0.; N05 G94G01X40.F100.; N06 G19C0Z0; N07 G07.1C20.; N08 G41; N09 G01Z-10.C80.F150; N10 Z-25.C90.; N11 Z-80.C225; N12 G03Z-75.C270.R55.; N13 G01Z-25; N14 G02Z-20.C280.R80.; N15 G01C360. N16 G40; N17 G07.1C0; N18 G01X50.; N19 G0X100.Z100.; N20 M25; N21 M30;

(Unit: mm)

50

100

150

200

250

300

350

-20-40-60-80

C

Z

N09 N10

N11

N12 N13

N14

N15

6. Interpolation Functions 6.10 Polar Coordinate Interpolation

119

6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112, G113 (Only 6, 7 in G code list)

Function and purpose

This function converts the commands programmed with the orthogonal coordinate axis into linear axis movement (tool movement) and rotation 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 carried out on this plane. The workpiece coordinate system zero point is used as the coordinate system zero point during polar coordinate interpolation.

Linear axis

X axis

C axis

Z axis

Rotation axis (hypothetical axis)

Polar coordinate interpolation plane (G17 plane)

This is effective for cutting a notch section on a linear section of the workpiece diameter, and for cutting cam shafts, etc.

6. Interpolation Functions 6.10 Polar Coordinate Interpolation

120

Command format

G12.1 ; Polar coordinate interpolation mode start G13.1 ; Polar coordinate interpolation mode cancel

(1) The coordinates commanded in the interval from the start to cancellation of the polar

coordinate interpolation mode will be the polar coordinate interpolation. 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)

(2) G112 and G113 can be used instead of G12.1 and G13.1.

(3) Command G12.1 and G13.1 in an independent block. A program error (P33) will occur if this command is issued in the same block as another G code.

(4) Linear interpolation or circular interpolation can be commanded during the polar coordinate interpolation mode.

(5) The coordinates can be commanded with either an absolute command or incremental command.

(6) Tool radius compensation can be applied on the program command. Polar coordinate interpolation will be executed on the path after tool radius compensation.

(7) Command the segment feed in the polar coordinate interpolation plane (orthogonal coordinate system) with F. The F unit is mm/min or inch/min.

(8) When the G12.1 and G13.1 commands are issued, the deceleration check is executed.

Detailed description

(1) Plane selection The linear axis and rotation axis used for polar coordinate interpolation must be set beforehand

with the parameters.

(a) Determine the deemed plane for carrying out polar coordinate interpolation with the parameter (#1533) for the linear axis used for polar coordinate interpolation.

#1533 setting value Deemed plane X G17 (XY plane) Y G19 (YZ plane) Z G18 (ZX plane)

Blank (no setting) G17 (XY plane)

(b) A program error (P485) will occur if the plane selection command (G16 to G19) is issued during the polar coordinate interpolation mode.

(Note) Depending on the model or version, parameter (#1533) may not be provided. In this case, the operation will be the same as if the parameter (#1533) is blank (no setting).

6. Interpolation Functions 6.10 Polar Coordinate Interpolation

121

(2) Related parameters

# Item Details Setting range

1516 mill_ax Milling axis name

Set the name of the rotation axis for milling interpolation (polar coordinate interpolation, cylindrical interpolation). Only one of the rotation axes can be set.

A to Z

1517 mill_c Milling interpolation hypothetical axis name

Select the hypothetical axis command name for milling interpolation (polar coordinate interpolation, cylindrical interpolation). 0: Y axis command 1: Command rotation axis name

0 / 1

8111 Milling Radius Select the diameter and radius of the linear axis for milling interpolation. 0: Radius command for all axes 1: Each axis setting (follows #1019 dia diameter

designation axis)

0 / 1

Relation with other functions

(1) Program commands during polar coordinate interpolation

(a) The program commands in the polar coordinate interpolation mode are commanded with the orthogonal coordinate value of the linear axis and rotation axis (hypothetical axis) on the polar coordinate interpolation plane.

The axis address of the rotation axis (C) is commanded as the axis address for the plane's 2nd axis (hypothetical axis) command.

The command unit is not deg (degree), and instead is the same unit (mm or inch) as the command issued with the axis address for the plane's 1st axis (linear axis).

(b) 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.

(2) Circular interpolation on polar coordinate plane The arc radius address for carrying out circular interpolation during the polar coordinate

interpolation mode is determined with the linear axis parameter (#1533). #1533 setting value 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)

The arc radius can also be designated with the R command.

(Note) Depending on the model or version, parameter (#1533) may not be provided. In this case, the operation will be the same as if the parameter (#1533) is blank (no setting).

(3) Tool radius compensation The tool radius can be compensated during the polar coordinate interpolation mode.

(a) Command the plane selection in the same manner as polar coordinate interpolation. When using tool radius compensation, it must be started up and canceled within the polar

coordinate interpolation mode.

(b) A program error (P485) will occur if polar coordinate interpolation is executed during tool radius compensation.

(c) If the G12.1 and G13.1 commands are issued with no movement command given 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 applied after the tool radius compensation is canceled and the following operations are performed.

6. Interpolation Functions 6.10 Polar Coordinate Interpolation

122

(4) Cutting asynchronous feed

(a) The asynchronous mode is forcibly set when the polar coordinate interpolation mode is started.

(b) When the polar coordinate interpolation mode is canceled, the synchronization mode will return to the state before the polar coordinate interpolation mode was started.

(c) A program error (P485) will occur if G12.1 is commanded in the constant surface speed control mode (G96).

(5) Miscellaneous functions

(a) The miscellaneous function (M) and 2nd miscellaneous function can be issued even in the polar coordinate interpolation mode.

(b) The S command in the polar coordinate interpolation mode issues the rotary tool's rotation speed instead of the spindle rotation speed.

(c) Issue the T command before polar coordinate interpolation is started. A program error (P485) will occur if the T command is issued in the polar coordinate interpolation mode.

: : T1212 ; ... T command before polar coordinate interpolation Valid G0 X100. Z0 ; G12.1 ; : T1200 ; ... T command in polar coordinate interpolation mode Program error : G13.1 ;

(d) 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 be resulted: Machine coordinate is not changed even if G12.1 is executed. The workpiece coordinate is changed to that of the post tool length compensation when G12.1 is executed. (Even if canceling the polar coordinate interpolation, this workpiece coordinate will not be canceled.)

6. Interpolation Functions 6.10 Polar Coordinate Interpolation

123

(6) F command during polar coordinate interpolation

As for the F command in the polar coordinate interpolation mode, whether the previous F command is used or not depends on that the mode just before G12.1 is the feed per minute command (G94) or feed per revolution command (G95).

(a) When G94 is commanded just before G12.1 If there is no F command in the polar coordinate interpolation, the previous F command feed rate will be used. The feed rate after the polar coordinate interpolation mode is canceled will remain the F command feed rate issued when the polar coordinate interpolation mode was started or the final F command feed rate set during polar coordinate interpolation. The previous F command feed rate cannot be used during polar coordinate interpolation.

(b) When G95 is commanded just before G12.1 The previous F command feed rate cannot be used during polar coordinate interpolation. A new F command must be issued. The feed rate after the polar coordinate interpolation mode is canceled will return to that applied before the polar coordinate interpolation mode was started.

When there is no F command in G12.1 Previous mode No F command After G13.1 is canceled G94 Previous F is used G95 Program error (P62) F just before G12.1 is used

When F is commanded in G12.1 Previous mode No F command After G13.1 is canceled G94 Commanded F is used G95 Commanded F is used *1 F just before G12.1 is used

*1) Moves with the feed per minute command during G12.1.

(7) Hole drilling axis in the fixed cycle for drilling command during the polar coordinate interpolation Hole drilling axis in the fixed cycle for drilling command during the polar coordinate interpolation is determined with the linear axis parameter (# 1533).

#1533 setting value 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)

6. Interpolation Functions 6.10 Polar Coordinate Interpolation

124

Restrictions and precautions

(1) The following G code commands can be used during the polar coordinate interpolation mode.

G code Details G00 G01 G02 G03 G04 G09 G22/23 G40-42 G61 G64 G65 G66 G66.1 G67 G80-89 G90/91 G94 G98 G99

Positioning Linear interpolation Circular interpolation (CW) Circular interpolation (CWW) Dwell Exact stop check Chuck barrier ON/OFF Tool nose R compensation Exact stop check mode Cutting mode Macro call (simple call) Macro modal call A (modal call) Macro modal call B (block call per macro) Macro modal call cancel (modal call cancel) Fixed cycle for drilling Absolute/incremental value command Asynchronous feed Hole drilling cycle initial return Hole drilling cycle R point return

A program error (P481) may occur if a G code other than those listed above is commanded during polar coordinate interpolation.

(2) The program cannot be restarted (resumed) for a block in polar coordinate interpolation.

(3) Before commanding polar coordinate interpolation, set the workpiece coordinate system so that the center of the rotation axis is at the coordinate system zero point. Do not change the coordinate system during the polar coordinate interpolation mode. (G50, G52, G53, relative coordinate reset, G54 to G59, etc.)

(4) The feed rate during polar coordinate interpolation will be the interpolation speed on the polar coordinate interpolation plane (orthogonal coordinate system).

(The relative speed with the tool will be converted with polar coordinate conversion.) When passing near the center of the rotation axis on the polar coordinate interpolation plane

(orthogonal coordinate system), the rotation axis side feed rate 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 poler coordinate interpolation.

(6) The current position displays during polar coordinate interpolation will all indicate the actual coordinate value. However, the "remaining movement amount" will be the movement amount on the polar coordinate input plane.

(7) The polar coordinate interpolation mode will be canceled when the power is turned ON or reset.

(8) A program error (P484) will occur if any axis commanded for polar coordinate interpolation has not completed reference position return.

(9) Tool radius compensation must be canceled before the polar coordinate interpolation mode can be canceled.

(10) When the polar coordinate interpolation mode is canceled, the mode will change to the cutting mode, and the plane will return to that selected before polar coordinate interpolation.

(11) A program error (P486) will occur if the polar coordinate interpolation command is issued during the mirror image.

(12) A program error (P481) will occur if the cylindrical interpolation or the polar coordinate interpolation is commanded during the polar coordinate interpolation mode.

6. Interpolation Functions 6.10 Polar Coordinate Interpolation

125

(13) The G84 or G88 synchronous tapping cycles cannot be used during pole coordinate interpolation mode. The asynchronous tap can be used during pole coordinate interpolation mode; however, the synchronous tap must not be commanded.

Example of program

Hypothetical C axis

X axis

Z axis

C axis

Hypothetical C axis

C axis

Tool

X axis

N01 N02

N11

N05

N04

N03

N10

N09 N08

N07

N06

Path after tool radius compensation Program path

: : N00 T0101; : : N01 G17 G90 G0 X40.0 C0 Z0; N02 G12.1; N03 G1 G42 X20.0 F2000; N04 C10.0; N05 G3 X10.0 C20.0 R10.0; N06 G1 X-20.0; N07 C-10.0; N08 G3 X-10.0 C-20.0 I10.0 J0; N09 G1 X20.0; N10 C0; N11 G40 X40.0; N12 G13.1; : : M30 ;

Setting of start position Polar coordinate interpolation mode: Start Actual machining start Shape program (Follows orthogonal coordinate values on X-C hypothetical axis plane.) Polar coordinate interpolation mode: Cancel

6. Interpolation Functions 6.11 Exponential Interpolation

126

6.11 Exponential Interpolation; G02.3, G03.3

Function and purpose

Exponential interpolation changes the rotation 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

(Linear axis)

Torsion angle: J1=J2=J3

A axis (Rotation axis)

Z axis

X axis J1 J2 J3

(G02.3/G03.3)

(G00)

(G01) (G01)

Relation of linear axis and rotation axis

A axis (Rotation axis)

"Relation of linear axis and rotation axis"

X=B (eCA-1) {B, C... constant} X axis

(Linear axis)

6. Interpolation Functions 6.11 Exponential Interpolation

127

Command format

G02.3/G03.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 ; G02.3 Forward rotation interpolation G03.3 Negative rotation interpolation X X axis end point (Note 1) Y Y axis end point (Note 1) Z Z axis end point (Note 1) I Angle i1 (Note 2) J Angle j1 (Note 2) R Constant value r1 (Note 3) F Initial feed rate (Note 4) Q Feed rate at end point (Note 5)

(Note 1) Designate the end point of the linear axis designated with parameter (#1514 expLinax) and the axis that carries out linear interpolation between that axis.

If the end point on of the rotation axis designated with parameter (#1515 expRotax) is designated, linear interpolation without exponential interpolation will take place.

(Note 2) The command unit is as follows.

Setting unit #1003 = B #1003 = C #1003 = D #1003 = E (Unit = ) 0.001 0.0001 0.00001 0.000001

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. (Note 3) The command unit is as follows.

Setting unit #1003 = B #1003 = C #1003 = D #1003 = E Unit Metric system 0.001 0.0001 0.00001 0.000001 mm Inch system 0.0001 0.00001 0.000001 0.0000001 inch

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. (Note 4) The command unit and command range is the same as the normal F code. (Command

as a feed per minute.) Command the composite feed rate that includes the rotation 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. (Note 5) The command unit is as follows.

Setting unit #1003 = B #1003 = C #1003 = D #1003 = E Unit Metric system 0.001 0.0001 0.00001 0.000001 mm Inch system 0.0001 0.00001 0.000001 0.0000001 inch

The command unit and command range is the same as the normal F code. Command the composite feed rate that includes the rotation 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 feed rate (address F command). (The start point and end point feed rates will be the same.)

A program error (P35) will occur if the address Q command value is 0.

6. Interpolation Functions 6.11 Exponential Interpolation

128

Example of uniform helix machining of taper shape

i1

j1 x1 x0

r1

Z axis Z axis

A axis

Linear axis ... X axis, rotation axis ... A axis, linear axis (X axis) start point ... x0

Relational expression of exponential function

The exponential function relational expression of the linear axis (X) and rotation axis (A) in the G02.3/G03.3 command is defined in the following manner. X () = r1 (e/D- 1) / tan (i1) (linear axis (X) movement (1)) A () = (-1) 360 / (2) (rotation axis (A) movement) D = tan (j1) / tan (i1) = 0 during forward rotation (G02.3), and = 1 during reverse rotation (G03.3) is the rotation angle (radian) from the rotation axis' start point The rotation axis' rotation angle () is as follows according to expression (1). = D 1n { (X tan (i1) / r1) + 1 }

6. Interpolation Functions 6.11 Exponential Interpolation

129

Machining example

Example of uniform helix machining of taper shape

i1

j1 x1 x0 x2

p1

A axis

r1 r2

z1 z2 z0

X axis

Z axis

Z () = r1 (e/D-1) tan (p1) / tan (i1) + z0 ... (1) X () = r1 (e/D-1) / tan (i1) ... (2) A () = (-1) 360 / (2) D = tan (j1) / tan (i1) Z () Absolute value from zero point of Z axis (axis that linearly interpolates between interval

with linear axis (X axis)) X () Absolute value from X axis (linear axis) start point A () Absolute value from A axis (rotation axis) start point r1 Exponential interpolation constant value (address R command) r2 Workpiece left edge radius x2 X axis (linear axis) position at workpiece left edge 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

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 feed rate (address F command) q1 Feed rate at end point (address Q command) k1 Insignificant data (address K command) According to expressions (1) and (2): Z () = X () tan (p1) + z0 ... (3) According to expression (3), the slot base gradient angle (p1) is determined 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) }

6. Interpolation Functions 6.11 Exponential Interpolation

130

The taper gradient angle (i1) and torsion angle (j1) are each issued with the command address I and J. 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 with 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).

Command and operation

G2.3(Equivalent to G3.3 if j1<0)

X movement direction > 0 X movement direction < 0

i1>0 i1<0 i1>0 i1<0

C om

m an

d

i1

X

Z End point

j1

r1

Start point

-

X

Z +

j1

i1

r1

End point

Start point

X

Z

j1

i1

r1

Start point

End point

End point

Start point

X

Z+ -

j1

i1

r1

O pe

ra tio

n

X

A

X

A

X

A

X

A

M ac

hi ni

ng

pr og

ra m

e xa

m pl

e 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;

G3.3(Equivalent to G2.3 if j1<0)

X movement direction > 0 X movement direction < 0

i1>0 i1<0 i1>0 i1<0

C om

m an

d

End point Start

point

X

Z

j1

i1

r1

End point

Start point

-

X

Z +

j1

r1

Start point

End point

X

Z

j1

i1

r1

End point

Start point

X

Z+ -

j1

i1

r1

O pe

ra tio

n

X A

X

A

X A

X

A

M ac

hi ni

ng

pr og

ra m

e xa

m pl

e 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;

6. Interpolation Functions 6.11 Exponential Interpolation

131

Precautions for programming

(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 rotation axis as 0.

(2) Linear interpolation will take place in the following cases, even if in the G02.3/G03.3 mode. The feed rate 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 rotation axis designated with the parameter (#1515 expRotax) is commanded.

(3) Tool length offset and nose R compensation cannot be used during the G02.3/G03.3 mode. Note that the tool length offset started before interpolation is started before the G02.3/G03.3 mode will normally continue.

(4) A program error (P481) will occur if commands are issued during the polar coordinate interpolation, cylindrical interpolation or milling interpolation modes.

(5) Program error (P612) will occur if commands are issued during the mirror image.

(6) G02.3/G03.3 will function with feed per minute even during the feed per revolution mode.

(7) 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 rotation axis.

7. Feed Functions 7.1 Rapid Traverse Rate

132

7. Feed Functions 7.1 Rapid Traverse Rate

Function and purpose

The rapid traverse rate can be set independently for each axis. The speed range that can be set is 1mm/min to 10000000mm/min. Note that the upper limit speed is limited by the machine specification. Refer to the specifications manual of the machine for the rapid traverse rate settings. Two paths are available during 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 by parameter "#1086 G0Intp". The positioning time is the same in each case.

(Note) Rapid traverse override Override can be applied by an external input signal for both manual and automatic rapid

traverse. There are 2 types which are determined by the PLC specifications. Type 1: Override in 4 steps: 1%, 25%, 50% and 100% Type 2: Override in 1% steps from 0% to 100%.

7.2 Cutting Feed Rate

Function and purpose

This function specifies the feed rate of the cutting commands, and a feed amount per spindle rotation or feed amount per minute is commanded. Once commanded, it is stored in the memory as a modal value. The feed rate modal is cleared to zero only when the power is turned ON. The maximum cutting feed rate is clamped by the cutting feed rate clamp parameter (whose setting range is the same as that for the cutting feed rate). The cutting feed rate is assigned with address F and 8-digit number. The F8 digits are assigned with a decimal point for a 5-digit integer and a 3-digit fraction. The cutting feed rate is valid for the G01, G02, G03, G33 and G34 commands.

Examples (asynchronous feed)

Feed rate G1 X100. Z100. F200 ; 200.0mm/min F200. or F200.000 gives the same rate. F1 X100. Z100. F123.4 ; 123.4mm/min F1 X100. Z100. F56.789 ; 56.789mm/min

Speed range that can be commanded (when input setting unit is 1m)

Command mode Feed rate command range Remarks mm/min 0.001 to 10000000 mm/min inch/min 0.0001 to 1000000 inch/min

/min 0.001 to 10000000 /min

(Note 1) A program error (P62) results when there is no F command in the first cutting command (G01, G02, G03, G33, G34) after the power has been turned ON.

7. Feed Functions 7.3 F1-digit Feed

133

7.3 F1-digit Feed

Function and purpose

By setting the F1-digit feed parameter, the feed rate 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. (The G modal does not change, but the acceleration/deceleration method follows the rapid traverse setting.) When F1 to F5 is assigned, the feed rate set to correspond to the command serves as the command value. The command greater than F6 is considered to be the normal cutting feed rate. The F1-digit command is valid in a G01, G02, G03, G02.1 or G03.1 modal. The F1-digit command can also be used for fixed cycle.

Detailed description

The override function of the feed rate which is set in accordance to the F1-digit is performed by using the first manual handle. The feed rate cannot be changed with the 2nd and 3rd handle. The amount by which the feed rate can be increased or reduced is determined by the following formula.

F = FM

K (number of manual handle pulse generator pulses)

Where "+" means increase, and "" means reduction. K : Operation constant (This is the number of FM divisions, and is the calculated constant of

the increment/decrement speed per scale of the manual handle pulse generator.) This is set with the base specification parameter "#1507 F1_K".

FM : This is the clamp speed of F1 to F5 This is set with the base specification parameter "#1506 F1_FM".

Set the corresponding speed of F1 to F5 with the base specification parameters "#1185 spd_F1" to "#1189 spd_F5" respectively. The increase/reduction range is from "0" to the set value of the parameter "#1506 F1_FM". Operation alarm (104) will occur when the feed rate is 0. (1) Operation method

(a) Make the F1-digit command valid. (Set the base specification parameter "#1079 F1digt" to 1.)

(b) Set FM and K. Setting range K : 1 to 32767 (Base specification parameter "#1507 F1_K") FM : 0 to Fmax (mm/min) (Base specification parameter "#1506 F1_FM")

(c) Set F1 to F5. (Base specification parameter "1185 spd_F1" to "#1189 spd_F5")

7. Feed Functions 7.3 F1-digit Feed

134

(2) Special notes

(a) Use of both the F1-digit command and normal cutting feed rate 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 feed rate command

(b) F1 to F5 are invalid in the G00 mode and the rapid traverse rate is established instead.

(c) If F0 is used in the G02 or G03 mode, a program error (P121) will result.

(d) When F1. to F5. (with decimal point) are assigned, the 1mm/min to 5mm/min direct commands are established instead of the F1-digit command.

(e) When the commands are used with the millimeter or degree units, the feed rate set to correspond to F1 to F5 serves as the assigned speed mm ()/min.

(f) When the commands are used with inch units, one-tenth of the feed rate set correspond to F1 to F5 serves at the assigned speed inch/min.

(g) The number of manual handle pulses is 1 pulse per scale unit regardless of the scaling factor.

(h) During a F1-digit command, the F1-digit number and F1-digit command signal are output as the PLC signals.

(i) Even if F1-digit feed is commanded during feed per revolution (G95), it will be executed as a normal F command (direct numerical value command).

(3) F1-digit and G commands

(a) 01 group G command in same block as F1-digit commands

Executed feed rate Modal display rate G modal G0F0 F0G0 Rapid traverse rate 0 G0

G0F1 F1G0 Rapid traverse rate 1 G0

G1F0 F0G1 Rapid traverse rate 0 G1

G1F1 F1G1 F1 contents 1 G1

(b) F1-digit and unmodal commands may be assigned in the same block. In this case, the unmodal command is executed and at the same time the F1-digit modal command is updated.

(4) Example of arithmetic constant K setting

When the handle scale unit is to be made 10mm/min. FM is made 15000 mm/min:

F = 10 = 15000 K

Therefore, K is 1500. The feed rate is made F (1 to 5) 10 (mm/min) by rotating the handle through one scale unit.

(5) Valid manual handle conditions

The manual handle is valid during cutting feed (F1 to F5), automatic start, F1-digit valid and manual handle valid switch ON at the machine side as well as in the MDI mode, tape mode or memory mode provided that the machine lock (machine lock rapid traverse) or dry run status has not been established. The function cannot be used when the handle specifications have not been provided.

7. Feed Functions 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed)

135

7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed); G94, G95

Function and purpose

Using the G95 command, it is possible to assign the feed amount per rotation with an F code. When this command is used, the rotary encoder must be attached to the spindle.

Command format

G94; G95; G94 Feed per minute (mm/min) (asynchronous feed) G95 Feed per revolution (mm/rev) (synchronous feed)

The G95 command is a modal command and so it is valid until the G94 command (feed per minute) is next assigned.

(1) The F code command range is as follows.

The movement amount per spindle rotation with synchronous feed (feed per revolution) is assigned by the F code and the command range is as shown in the table below.

Metric input

Input setting unit B (0.001mm) C (0.0001mm)

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)

Least command increment

1 (= 1.00), (1. = 1.00)

1 (= 0.0001), (1. = 1.00)

1 (= 1.000), (1. = 1.000)

1 (= 0.00001), (1. = 1.00)

Command range

0.01 to 1000000.00

0.0001 to 9999.9999

0.001 to 1000000.000

0.00001 to 9999.99999

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)

Least command increment

1 (= 1.0000), (1. = 1.0000)

1 (= 0.000001), (1. = 1.00)

1 (= 1.00000), (1. = 1.00000)

1 (= 0.0000001), (1. = 1.00)

Command range

0.0001 to 1000000.0000

0.000001 to 9999.999999

0.00001 to 1000000.00000

0.0000001 to 9999.9999999

7. Feed Functions 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed)

136

Inch input

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)

Least command increment

1 (= 1.000), (1. = 1.000)

1 (= 0.000001), (1. = 1.000)

1 (= 1.0000), (1. = 1.0000)

1 (= 0.0000001), (1. = 1.000)

Command range

0.001 to 100000.000

0.000001 to 99.999999

0.0001 to 100000.0000

0.0000001 to 99.9999999

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)

Least command increment

1 (= 1.00000), (1. = 1.00000)

1 (= 0.00000001), (1. = 1.000)

1 (= 1.000000), (1. = 1.000000)

1 (= 0.000000001), (1. = 1.000)

Command range

0.00001 to 100000.00000

0.00000001 to 99.99999999

0.000001 to 100000.000000

0.000000001 to 99.999999999

(2) The effective speed (actual movement speed of machine) under feed per revolution conditions is given in the following formula (Formula 1).

FC = F N OVR ........... (Formula 1)

Where FC = Effective rate (mm/min, inch/min) F = Commanded speed (mm/rev, inch/rev) N = Spindle rotation speed (r/min) OVR = Cutting feed override

When a multiple number of axes have been commanded at the same time, the effective rate FC in formula 1 applies in the vector direction of the command.

(Note 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 feed per minute speed, appears as the FC on the monitor 1. screen of the setting and display unit.

(Note 2) When the above effective rate exceeds the cutting feed clamp rate, it is clamped at that clamp rate.

(Note 3) If the spindle rotation speed is zero when feed per revolution is executed, operation alarm (105) results.

(Note 4) During machine lock processing, the rate will be 1,000,000 mm/min (or 39,370 inch/min, 1,000,000 /min) regardless of the commanded speed and spindle rotation speed.

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

(Note 6) 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 is executed can be selected by setting parameter "#1074 I_Sync".

7. Feed Functions 7.5 Feed Rate Designation and Effects on Control Axes

137

7.5 Feed Rate Designation and Effects on Control Axes

Function and purpose

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 rotation axes which control rotary movement. The feed rate 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 rotation axes. The displacement amount for each axis is assigned separately for each axis by a value corresponding to the respective axis. The feed rate 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 involved. The assignment of the feed rate is described with the following related items.

When controlling linear axes

Even when only one machine axis is to be controlled or there are two or more axes to be controlled simultaneously, the feed rate which is assigned by the F code functions as a linear speed in the tool advance direction.

(Example) When the feed rate is designated as "f" and linear axes (X and Z) are to be controlled

X

Zz

x P2 (Tool end point)

Speed in this direction is "f"

P1 (Tool start point)

Feed rate for X axis = f

Feed rate for Z axis = f

X

x2 + z2

Z

x2 + z2

When only linear axes are to be controlled, it is sufficient to designate the cutting feed in the program. The feed rate for each axis is such that the designated rate is broken down into the components corresponding to the movement amounts.

7. Feed Functions 7.5 Feed Rate Designation and Effects on Control Axes

138

(Note) When the circular interpolation function is used and the tool is moved along the circumference of an arc by the linear control axis, the rate in the tool advance direction, or in other words the tangential direction, will be the feedrate designated in the program.

x

z

X

Zi

P2

P1

Linear speed is "f"

(Example) When the feed rate is designated as "f" and the linear axes (X and Z) are to be

controlled using the circular interpolation function In this case, the feed rate of the X and Z axes will change along with the tool movement.

However, the combined speed will always be maintained at the constant value "f".

When controlling rotation axes

When rotation axes are to be controlled, the designated feed rate functions as the rotation speed of the rotation 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 feed rate is designated as "f" and rotation axis (C) is to be controlled ("f" units

= /min)

c

r

P2 (Tool end point)

Rotation center

Angular speed is "f"

P1 (Tool start point)

Linear speed is : r f 180

In this case, in order to make the cutting feed (linear speed) in the tool advance direction "fc":

fc = f

Therefore, the feed rate to be designated in the program must be: f = fc

r 180

180 r

7. Feed Functions 7.5 Feed Rate Designation and Effects on Control Axes

139

When linear and rotation axes are to be controlled at the same time

The NC unit proceeds in exactly the same way whether linear or rotation axes are to be controlled. When a rotation axis is to be controlled, the numerical value assigned by the coordinate words (C, H) is the angle and the numerical values assignees by the feed rate (F) are all handled as linear speeds. In other words, 1 of the rotation axis is treated as being equivalent to 1mm of the linear axis. Consequently, when both linear and rotation axes are to be controlled simultaneously, the components for each axis of the numerical values assigned by F will be the same as for section (1) above (applying when linear axes are to be controlled). 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 rotation axis control will change along with the tool movement (their size will not change). This means, as a result, that the combined tool advance direction feed rate with vary along with the tool movement.

(Example) When the feed rate is designated as "f" and linear (X) and rotation (C) axes are to be

controlled simultaneously If the X-axis incremental command value is "x" and the C-axis incremental command

value is "c":

P1

x

fc

c

fc ft

fx

fx

ft r

P2

Size and direction are fixed for fx. Size is fixed for fc but direction varies. Both size and direction vary for ft.

Rotation center

7. Feed Functions 7.5 Feed Rate Designation and Effects on Control Axes

140

X-axis feed rate (linear speed) "fx" and C-axis feed rate (angular speed) "" are expressed as: fx = f ........ (1) = f ........ (2) Linear speed "fc" based on C-axis control is expressed as: fc = ........ (3) If the speed in the tool advance direction at start point P1 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: ftx = rsin ( ) + fx ........ (4) fty = rcos ( ) ................... (5) Where r is the distance between center of rotation and tool (in mm units), and is the angle between the P1 point and the X axis at the center of rotation (in units ). The combined speed "ft" according to formulae (1), (2), (3), (4) and (5) is: ft = ftx2 + fty2 x2 x c rsin ( ) + ( )2 = f x2 + c2 Consequently, feed rate "f" designated by the program must be as follows: x2 + c2 x2 x c rsin ( ) + ( )2 "ft" in formula (6) is the speed at the P1 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.

x x2 + c2

c x2 + c2

r 180

180

180

180

180

180

90

r c 180

180

90

r c 180

f = ft

........... (6)

........... (7)

7. Feed Functions 7.6 Thread Cutting Mode

141

7.6 Thread Cutting Mode

Function and purpose

F7-digit or E8-digit commands for thread leads can be issued for the thread cutting mode (G33, G34, G76, G78 commands). The thread Iead command range is 0.0001 to 999.9999mm/rev (F7 digits) or 0.0001 to 999.99999 mm/rev (E8 digits) (with input unit of m).

Thread cutting metric input

Input setting unit B (0.001mm) C (0.0001mm)

Command address F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)

Least command increment

1 (=1.000), (1.=1.000)

1 (= 1.00000), (1.=1.00000)

1 (= 1.00), (1.=1.00)

1 (= 1.0000), (1.=1.0000)

1(=1.000000), (1.=1.000000)

1 (= 1.000), (1.=1.000)

Command range

0.001 to 999.999

0.00001 to 999.99999

0.03 to 999.99

0.0001 to 999.9999

0.000001 to 999.999999

0.255 to 9999.999

Input

setting unit D (0.00001mm) E (0.000001mm)

Command address F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)

Least command increment

1 (= 1.00000), (1.=1.00000)

1 (= 1.0000000), (1.=1.0000000)

1 (= 1.0000), (1.=1.0000)

1 (= 1.000000), (1.=1.000000)

1 (=1.00000000), (1.=1.00000000)

1 (= 1.00000), (1.=1.00000)

Command range

0.00001 to 999.99999

0.0000001 to 999.9999999

0.2550 to 9999.9999

0.000001 to 999.999999

0.00000001 to 999.99999999

0.25500 to 9999.99999

Thread cutting inch input

Input setting unit B (0.0001inch) C (0.00001inch)

Command address F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)

Least command increment

1(=1.0000), (1.=1.0000)

1(=1.000000), (1.=1.000000)

1 (= 1.0000), (1.=1.0000)

1(=1.00000), (1.=1.00000)

1(=1.0000000), (1.=1.0000000)

1(=1.00000), (1.=1.00000)

Command range

0.0001 to 99.9999

0.000001 to 39.370078

0.0255 to 9999.9999

0.00001 to 99.99999

0.0000001 to 39.3700787

0.25401 to 999.99999

Input

setting unit D (0.000001inch) E (0.0000001inch)

Command address F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)

Least command increment

1 (= 1.000000), (1.=1.000000)

1 (= 1.00000000), (1.=1.00000000)

1 (= 1.000000), (1.=1.000000)

1 (= 1.0000000), (1.=1.0000000)

1 (= 1.000000000), (1.=1.000000000)

1 (= 1.0000000), (1.=1.0000000)

Command range

0.000001 to 99.999999

0.00000001 to 39.37007874

0.025500 to 9999.99999

0.0000001 to 99.9999999

0.000000001 to 39.370078740

0.0255000 to 999.9999999

7. Feed Functions 7.7 Automatic Acceleration/Deceleration

142

7.7 Automatic Acceleration/Deceleration

Function and purpose

The rapid traverse and manual feed acceleration/deceleration pattern is linear acceleration and linear deceleration. Time constant TR can be set independently for each axis using parameters in 1ms steps from 1 to 500ms. The cutting feed (not manual feed) acceleration/deceleration pattern is exponential acceleration/ deceleration. Time constant Tc can be set independently for each axis using parameters in 1ms steps across a range from 1 to 500ms. (Normally, the same time constant is set for all axes.)

With continuous commands

With continuous commands

TR

f

t

TC

f

t TR Td

TC

Rapid traverse acceleration/deceleration Pattern (TR = Rapid traverse time constant) (Td = Deceleration check time)

Cutting feed acceleration/deceleration pattern (Tc = Cutting feed time constant)

With rapid traverse and manual feed, the following block is executed after the command pulse of the present block has become "0" and the tracking error of the acceleration/deceleration circuit has become "0". However, with cutting feed, the following block is executed as soon as the command pulse of the present block becomes "0" although an external signal (error detection) can detect that the tracking error of the acceleration/deceleration circuit has reached "0" and the following block can be executed. When the in-position check has been made valid (selected by parameter "#1193 inpos") during the deceleration check, it is first confirmed that the tracking error of the acceleration/deceleration circuit has reached "0", then it is checked that the position deviation is less than the parameter setting value "#2204 SV024", and finally the following block is executed. It depends on the machine as to whether the error detection function can be activated by a switch or M function and so reference should be made to the instructions issued by the machine tool builder.

7. Feed Functions 7.8 Rapid Traverse Constant Inclination Acceleration/Deceleration

143

7.8 Rapid Traverse Constant Inclination Acceleration/Deceleration

Function and purpose

This function performs acceleration and deceleration at a constant inclination during linear acceleration/deceleration in the rapid traverse mode. Compared to the method of acceleration /deceleration after interpolation, the constant inclination acceleration/deceleration method makes for improved cycle time.

Detailed description

(1) Rapid traverse constant inclination acceleration/deceleration are valid only for a rapid traverse

command. Also, this function is effective only when the rapid traverse command acceleration/deceleration mode is linear acceleration and linear deceleration.

(2) The acceleration/deceleration patterns in the case where rapid traverse constant inclination acceleration/deceleration are performed are as follows.

L

T s T s T d

T

Next block

rapid

rapid : Rapid traverse rate

Ts : Acceleration/deceleration time constant

Td : Command deceleration check time : Acceleration/deceleration inclination T : Interpolation time L : Interpolation distance

T = rapid

L +Ts

Td = Ts + (0~1.7 ms)

= tan-1 rapid

Ts ( )

rapid: Rapid traverse rate Ts: Acceleration/deceleration time constant Td: Command deceleration check time : Acceleration/deceleration inclination T: Interpolation time L: Interpolation distance

L

Ts Td

T

rapid

Next block

= tan-1 rapid Ts

( )

Td = + (0 ~ 1.7 ms) T 2

T = 2 Ts X L / rapid

7. Feed Functions 7.8 Rapid Traverse Constant Inclination Acceleration/Deceleration

144

(3) When 2-axis simultaneous interpolation (linear interpolations) is performed during rapid

traverse constant inclination acceleration and deceleration, the acceleration (deceleration) time is the longest value of the acceleration (deceleration) times determined for each axis by the rapid traverse rate of commands executed simultaneously, the rapid traverse acceleration and deceleration time constant, and the interpolation distance, respectively. Consequently, linear interpolation is performed even when the axes have different acceleration and deceleration time constants.

<2-axis simultaneous interpolation (When linear interpolation is used, Tsx < Tsz, and Lx Lz)>

x Tsx Tsx

Tdx

Lx

Tx

Next block

X axis

Tsz

Lz

Tz

Z axis

rapid X

rapid Z

Z

Tsz Tdz

Next block

When Tsz is greater than Tsx, Tdz is also greater than Tdx, and Td = Tdz in this block.

(4) The program format of G0 (rapid traverse command) when rapid traverse constant inclination acceleration/deceleration are executed is the same as when this function is invalid (time constant acceleration/deceleration).

(5) This function is valid only for G0 (rapid traverse).

7. Feed Functions 7.9 Speed Clamp

145

7.9 Speed Clamp

Function and purpose

This function exercises control over the actual cutting feed rate in which override has been applied to the cutting feed rate command so that the speed clamp value which has been preset independently for each axis is not exceeded. (Note) Speed clamping is not applied to synchronous feed and thread cutting.

7. Feed Functions 7.10 Exact Stop Check

146

7.10 Exact Stop Check; G09

Function and purpose

In order for roundness to be prevented during corner cutting and for machine shock to be alleviated when the tool feed rate changes suddenly, there are times when it is desirable to start the commands in the following block once the in-position state after the machine has decelerated and stopped or the elapsing of the deceleration check time has been checked. The exact stop check function is designed to accomplish this purpose. Whether to control with the deceleration check time or with the in-position state can be selected with the parameter. (Refer to the section "7.12 Deceleration check") The in-position width is set into parameter the servo parameter "#2224 sv024" or "#2077 G0inps", "#2078 G1inps".

Command format

G09 G01 (G02, G03) ;

The exact stop check command G09 has an effect only with the cutting command (G01 to G03) in its particular block.

Example of program

N001 G09 G01 X100.000 F150 ; The commands in the following block are started

once the deceleration check time or in-position state has been checked after the machine has decelerated and stopped.

N002 Z100.000 ;

N002

N001

Fig. 1 Exact stop check result

X axis

Z axis

f (Commanded speed)

Time

N001

N002Without G09

Tool

Solid line indicates speed pattern with G09 command. Broken line indicates speed pattern without G09 command.

With G09

7. Feed Functions 7.10 Exact Stop Check

147

Detailed description

(1) With continuous cutting feed

Ts

Fig. 2 Continuous cutting feed command

Previous block Next block

(2) With cutting feed in-position check

Fig. 3 Block joint with cutting feed in-position check

Ts Ts

Previous block Next block

Lc (in-position width)

In Figs. 2 and 3:

Ts = Cutting feed acceleration/deceleration time constant Lc = In-position width As shown in Fig. 3, the in-position width "Lc" can be set into the servo parameter "#2224 SV024" as the remaining distance (shaded area in Fig. 3) of the previous block when the next block is started. The in-position width is designed to reduce the roundness at the workpiece corners to below the constant value.

Lc Next block

Previous block

To eliminate corner roundness, set the value as small as possible to servo parameter and perform an in-position check or assign the dwell command (G04) between blocks.

7. Feed Functions 7.10 Exact Stop Check

148

(3) With deceleration check

(a) With linear acceleration/deceleration

Ts

Td

Previous block Next block

Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = Ts + ( 0 to 14ms)

(b) With exponential acceleration/deceleration

Ts

Td

Previous block Next block

Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = 2 Ts + ( 0 to 14ms)

(c) With exponential acceleration/linear deceleration

2 x Ts

Td Ts

Previous block Next block

Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = 2 Ts + ( 0 to 14ms)

The time required for the deceleration check during cutting feed is the longest among the cutting feed deceleration check times of each axis determined by the cutting feed acceleration/deceleration time constants and by the cutting feed acceleration/ deceleration mode of the axes commanded simultaneously. (Note 1) To execute exact stop check in a fixed cycle cutting block, insert command G09

into the fixed cycle subprogram.

7. Feed Functions 7.11 Exact Stop Check Mode

149

7.11 Exact Stop Check Mode ; G61

Function and purpose

Whereas the G09 exact stop check command checks the in-position status only for the block in which the command has been assigned, the G61 command functions as a modal. This means that deceleration will apply at the end points of each block to all the cutting commands (G01 to G03) subsequent to G61 and that the in-position status will be checked. G61 is released by automatic corner override (G62), tapping mode (G63), or cutting mode (G64).

Command format

G61 ;

In-position check is executed in the G61 block, and thereafter, the in-position check is executed at the end of the cutting command block is executed until the check mode is canceled.

7. Feed Functions 7.12 Deceleration Check

150

7.12 Deceleration Check

Function and purpose

The deceleration check is a function that determines the method of the check at the completion of the axis movement block's movement. The deceleration check includes the in-position check and commanded speed check method. The G0 and G1 deceleration check method combination can be selected. (Refer to section "Deceleration check combination".) With this function, the deceleration check in the reverse direction of G1 G0 or G1 G1 can be changed by changing the parameter setting.

(1) Types of deceleration check

Commanded speed check With the commanded speed check, the completion of deceleration is judged when the command to the motor is completed.

Deceleration start point

Judges the stop here

Movement of motor

Command to motor

In-position check With the in-position check, the completion of deceleration is judged when the motor moves to the in-position width designated with the parameter.

Deceleration start point

Judges the stop here

G0/G1 in-position width

7. Feed Functions 7.12 Deceleration Check

151

(2) Designating deceleration check

The deceleration check by designating a parameter includes "deceleration check specification type 1" and "deceleration check specification type 2". The setting is selected with the parameter "#1306 InpsTyp".

(a) Deceleration check specification type 1 ("#1306 InpsTyp" = 0) The G0 and G1 deceleration check method can be selected with the base specification

parameter deceleration check method 1 (#1193 inpos) and "deceleration check method 2" (#1223 aux07/bit1).

Parameter Rapid traverse

command Parameter

Other than rapid traverse command (G1 : other than G0 command)

inpos (#1193)

G0XX (G0+G9XX)

AUX07/BIT-1 (#1223/BIT-1)

G1+G9XX G0XX

0 Command

deceleration check 0

Command deceleration check

1 In-position

check 1

In-position check

No deceleration check

(Note 1) XX expresses all commands.

(Note 2) "#1223 aux07" is the part system common parameter.

(b) Deceleration check specification type 2 ("#1306 InpsTyp" = 1) Rapid traverse and cutting in-position are designated with the "#1193 inpos" parameter.

Parameter Command block #1193 Inpos G0 G1+G9 G1

0 Command

deceleration check Command

deceleration check No deceleration

check

1 In-position

check In-position

check No deceleration

check

(Note 1) "#1193 inpos" is the parameter per part system.

(Note 2) "G0" means the rapid traverse, and "G1" means the cutting feed.

7. Feed Functions 7.12 Deceleration Check

152

7.12.1 G1 G0 Deceleration Check Detailed description

(1) In G1 G0 continuous blocks, the parameter "#1502 G0Ipfg" can be changed to change the

deceleration check in the reverse direction.

Same direction Reverse direction

G0Ipfg: 0

G0Ipfg: 1

Command deceleration

Example of program

When there is a deceleration check in the movement of several axes:

(1) G91 G1 X100. Z100. F4000 ; G0 X-100. Z120. ;

A deceleration check is carried out, because the X axis moves in the reverse direction in the program above.

(2) G91 G1 X100. Z-100. F4000 ;

G0 X80. Z100. ; A deceleration check is carried out, because the Z axis moves in the reverse direction in the program above.

(3) G90 G1 X100. Z100. F4000 ;

G0 X80. Z120. ; (When the program start position is X0 Z0) A deceleration check is carried out, because the X axis moves in the reverse direction in the program above.

(4) G91 G1 X100. Z100. F4000 ;

G0 X100. Z100. ; A deceleration check is not carried out, because both the X axis and the Z axis move in the same direction in the program above.

(5) G91 G1 X100. Z80. F4000 ;

G0 X80. ; A deceleration check is not carried out, because the X axis moves in the same direction, and there is no Z axis movement command in the program above.

G1 G0

G1 G0

G0 G1

G0 G1

The acceleration rate is excessive due to the composite speed of G1 and G0.

7. Feed Functions 7.12 Deceleration Check

153

7.12.2 G1 G1 Deceleration Check Detailed description

(1) In G1 G1 continuous blocks, the parameter "#1503 G1Ipfg" can be changed to change the

deceleration check of the reverse direction.

Same direction Reverse direction

G1Ipfg: 0

G1 G1

G1 G1

G1 G1

G1Ipfg: 1

G1 G1

Command deceleration

Example of program

When there is a deceleration check in the movement of several axes:

(1) G91 G1 X100. Z100. F4000 ; G1 X-100. Z120. ;

A deceleration check is carried out, because the X axis moves in the reverse direction in the program above.

(2) G91 G1 X100. Z-100. F4000 ;

G1 X80. Z100. ; A deceleration check is carried out, because the Z axis moves in the reverse direction in the program above.

(3) G90 G1 X100. Z100. F4000 ;

G1 X80. Z120. ; (When the program start position is X0 Z0) A deceleration check is carried out, because the X axis moves in the reverse direction in the program above.

(4) G91 G1 X100. Z100. F4000 ;

G1 X100. Z100. ; A deceleration check is not carried out, because both the X axis and the Z axis move in the same direction in the program above.

(5) G91 G1 X100. Z80. F4000 ;

G1 X80. ; A deceleration check is not carried out, because the X axis moves in the same direction, and there is no Z axis movement command in the program above.

7. Feed Functions 7.13 Automatic Corner Override

154

7.13 Automatic Corner Override ; G62

Function and purpose

With this command, when cutting with tool radius compensation, an override is automatically applied to the feed rate to reduce the load during inside corner cutting or during inside cutting of automatic corner R. Automatic corner override is valid until the nose R compensation cancel (G40), exact stop check mode (G61), tapping mode (G63), or cutting mode (G64) command is issued.

Command format

G62 ;

Machining inside corners

When cutting an inside corner as in Fig. 1, the machining allowance amount increases and a greater load is applied to the tool. To remedy this, override is applied automatically within the corner set range, the feed rate is reduced, the increase in the load is reduced and cutting is performed effectively. However, this function is valid only when finished shapes are programmed.

Ci

Fig. 1

S

workpiece

Machining allowance

Machining allowance Programmed path (finished shape)

Workpiece surface shape

Nose R center path

Tool

: Max. angle at inside corner Ci : Deceleration range (IN)

Deceleration range

(1) (2)

(3)

7. Feed Functions 7.13 Automatic Corner Override

155

(1) Operation

(a) When automatic corner override is not to be applied : When the tool moves in the order of (1) (2) (3) in Fig. 1, the machining allowance at

(3) increases by an amount equivalent to the area of shaded section S and so the tool load increases.

(b) When automatic corner override is to be applied :

When the inside corner angle in Fig. 1 is less than the angle set in the parameter, the override set into the parameter is automatically applied in the deceleration range Ci.

(2) Parameter setting

The following parameters are set into the machining parameters :

# Parameter Parameter setting #8007 OVERRIDE 0 to 100% #8008 MAX. ANGLE 0 to 180 #8009 DSC. ZONE 0 to 99999.999mm or 0 to 3937.000 inches

Refer to the Instruction Manual for details on the setting method.

Automatic corner R

Ci Workpiece

P ro

gr am

m ed

pa

th

M ac

hi ni

ng

al lo

w an

ce

W or

kp ie

ce

su rfa

ce s

ha pe

N

os e

R

ce nt

er p

at h

Corner R section

Machining allowance

Corner R center

(1) The override set in the parameter is automatically applied at the deceleration range Ci and corner R section for inside offset with automatic corner R. (There is no angle check.)

7. Feed Functions 7.13 Automatic Corner Override

156

Application example

(1) Linear - linear corner

Ci

Program

Nose R center

Tool

The override set in the parameter is applied at Ci.

(2) Linear - arc (outside offset) corner

Ci

Program Nose R center

Tool

The override set in the parameter is applied at Ci.

(3) Arc (inside offset) - linear corner

Ci

Program

Nose R center

Tool Tool

The override set in the parameter is applied at Ci. (Note) The deceleration range Ci where the override is applied is the length of the arc with an

arc command.

7. Feed Functions 7.13 Automatic Corner Override

157

(4) Arc (inside offset) - arc (outside offset) corner

N1

Ci

N2 Program

Nose R center

The override set in the parameter is applied at Ci.

Relation with other functions

Function Override at corner Cutting feed override Automatic corner override is applied after cutting feed override

has been applied. Override cancel Automatic corner override is not canceled by override cancel. Speed clamp Valid after automatic corner override Dry run Automatic corner override is invalid. Synchronous feed Automatic corner override is applied to the synchronous feed rate. Thread cutting Automatic corner override is invalid. G31 skip Program error results with G31 command during nose R

compensation. Machine lock Valid Machine lock high speed Automatic corner override is invalid. G00 Invalid G01 Valid G02, G03 Valid

Precautions

(1) Automatic corner override is valid only in the G01, G02, and G03 modes; it is not effective in

the G00 mode. When switching from the G00 mode to the G01 (or G02 or G03) mode at a corner (or vice versa), automatic corner override will not be applied at that corner in the G00 block.

(2) Even if the automatic corner override mode is entered, the automatic corner override will not be applied until the nose R compensation mode is entered.

(3) Automatic corner override will not be applied on a corner where the nose R compensation is started or canceled.

(4) Automatic corner override will not be applied on a corner where the nose R compensation I, K vector command is issued.

7. Feed Functions 7.13 Automatic Corner Override

158

(5) Automatic corner override will not be applied when intersection calculation cannot be executed.

Intersection calculation cannot be executed in the following case. (a) When the movement command block does not continue for four or more times.

(6) The deceleration range with an arc command is the length of the arc.

(7) The inside corner angle, as set by parameter, is the angle on the programmed path.

(8) Automatic corner override will not be applied when the maximum angle in the parameter is set to 0 or 180.

(9) Automatic corner override will not be applied when the override in the parameter is set to 0 or 100.

7. Feed Functions 7.14 Tapping Mode

159

7.14 Tapping Mode ; G63 Function and purpose

The G63 command allows the control mode best suited for tapping to be entered, as indicated below :

1. Cutting override is fixed at 100%. 2. Deceleration commands at joints between blocks are invalid. 3. Feed hold is invalid. 4. Single block is invalid. 5. In-tapping mode signal is output.

G63 is released by the exact stop check mode (G61), automatic corner override (G62), or cutting mode (G64) command.

Command format

G63 ; 7.15 Cutting Mode ; G64 Function and purpose

The G64 command allows the cutting mode in which smooth cutting surfaces are obtained to be established. Unlike the exact stop check mode (G61), the next block is executed continuously with the machine not decelerating and stopping between cutting feed blocks in this mode. G64 is released by the exact stop check mode (G61), high-accuracy control mode (G61.1), automatic corner override (G62), or tapping mode (G63) command.

This cutting mode is established in the initialized status.

Command format

G64 ;

8. Dwell 8.1 Per-second Dwell

160

8. Dwell

The G04 command can delay the start of the next block. 8.1 Per-second Dwell ; G04

Function and purpose

The machine movement is temporarily stopped by the program command to make the waiting time state. Therefore, the start of the next block can be delayed. The waiting time state can be canceled by inputting the skip signal.

Command format

G04 X/U__ ; or G04 P__ ; X, P, U Dwell time

The input command increment for the dwell time depends on the parameter. In addition to the address P and X, the address U (actually, the address corresponding to the X-axis designated with the #1014 incax) can be used. Note that this is invalid when the #1076 AbsInc is set to 0.

Detailed description

(1) When designating the dwell time with X or U, the decimal point command is valid. (2) When designating the dwell time with P, the availability of the decimal point command can be

selected with the parameter (#8112). When the decimal point command is invalid in the parameter setting, the command below the decimal point issued with P is ignored.

(3) When the decimal point command is valid or invalid, the dwell time command range is as follows.

Command range when the decimal point command is valid

Command range when the decimal point command is invalid

0 to 99999.999 (s) 0 to 99999999 (ms) (4) The dwell time setting unit applied when there is no decimal point can be made 1s by setting 1

in the parameter #1078 Decpt2. This is effect only for X, U and P for which the decimal command is valid.

(5) When a cutting command is in the previous block, the dwell command starts calculating the dwell time after the machine has decelerated and stopped. When it is commanded in the same block as an M, S, T or B command, the calculation starts simultaneously.

(6) The dwell is valid during the interlock. (7) The dwell is valid even for the machine lock.

8. Dwell 8.1 Per-second Dwell

161

(8) The dwell can be canceled by setting the parameter #1173 dwlskp beforehand. If the set skip

signal is input during the dwell time, the remaining time is discarded, and the following block will be executed.

Previous block cutting command

Next block

Dwell command

Dwell time

Example of program

Dwell time (s)

#1078 Decpt2 = 0 #1078 Decpt2 = 1 Command DECIMAL

PNT-N DECIMAL

PNT-P DECIMAL

PNT-N DECIMAL

PNT-P G04 X500 ; 0.5 500 G04 X5000 ; 5 5000 G04 X5. ; 5 5 G04 X#100 ; 1000 1000 G04 U500 ; 0.5 500 G04 U5000 ; 5 5000 G04 U5. ; 5 5 G04 U#100 ; 1000 1000 G04 P5000 ; 5 5 5000 G04 P12.345 ; 0.012 12.345 0.012 12.345 G04 P#100 ; 1 1000 1 1000

(Note 1) The above examples are the results under the following conditions. Input setting unit 0.001mm or 0.0001inch #100 = 1000 ; (Note 2) "DECIMAL PNT-P" is a control parameter (#8112). (Note 3) If the input setting unit is 0.0001inch, the X before G04 will be multiplied by 10. For

example for "X5. G04 ;", the dwell time will be 50 seconds. Precautions and restrictions

(1) When using this function, command X or U after G04 in order to make sure that the dwell is

based on X or U.

9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD)

162

9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD)

Function and purpose

The miscellaneous (M) functions are also known as M functions, and they include such numerically controlled machine functions as spindle forward and reverse rotation, operation stop and coolant ON/OFF. These functions are designated by an 8-digit number (0 to 99999999) following the address M with this controller, and up to 4 groups can be commanded in a single block.

(Example) G00 Xx Mm1 Mm2 Mm3 Mm4 ;

When five or more commands are issued, only the last four will be valid. The output signal is an 8-digit BCD code and start signal. The eight commands of M00, M01, M02, M30, M96, M97, M98 and M99 are used as auxiliary commands for specific objectives and so they cannot be used as general auxiliary commands. This therefore leaves 92 miscellaneous functions which are usable as such commands. Reference should be made to the instructions issued by the machine tool builder for the actual correspondence between the functions and numerical values. When the M00, M01, M02, and M30 functions are used, the next block is not read into the pre-read buffer due to pre-read inhibiting. If the M function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which sequence applies.

(1) The M function is executed after the movement command.

(2) The M function is executed at the same time as the movement command. Which of these sequences actually applies depends on the machine specifications.

Processing and completion sequences are required in each case for all M commands except M96, M97, M98 and M99. The 8 M functions used for specific purposes will now be described.

Program stop : M00

When the tape reader has read this function, it stops reading the next block. As far as the NC system's functions are concerned, only the tape reading is stopped. Whether such machine functions as the spindle rotation and coolant supply are stopped or not differs according to the machine in question. Re-start is enabled by pressing the automatic start button on the machine operation board. Whether resetting can be initiated by M00 depends on the machine specifications.

9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD)

163

Optional stop : M01

If the tape reader reads the M01 command when the optional stop switch on the machine operation board is ON, it will stop and the same effect as with the M00 function will apply. If the optional stop switch is OFF, the M01 command is ignored.

(Example)

~

Optional stop switch command is ignored.

N10 G00 X1000 ; N11 M01 ;

Stops at N11 when switch is ON Next command (N12) is executed without stopping at N11 when switch is OFF

N12 G01 X2000 Z3000 F600 ;

~

Program end : M02 or M30

This command is normally used in the final block for completing the machining, and so it is primarily used for tape rewinding. Whether the tape is actually rewound or not depends on the machine specifications. Depending on the machine specifications, the system is reset by the M02 or M30 command upon completion of tape rewinding and any other commands issued in the same block. (Although the contents of the command position display counter are not cleared by this reset action, the modal commands and compensation amounts are canceled.) The next operation stops when the rewinding operation is completed (the in-automatic operation lamp goes off). To restart the unit, the automatic start button must be pressed or similar steps must be taken.

(Note 1) Independent signals are also output respectively for the M00, M01, M02 and M30 commands and these outputs are each reset by pressing the reset key.

(Note 2) M02 or M30 can be assigned by manual data input (MDI). At this time, commands can be issued simultaneously with other commands just as with the tape.

Macro interruption : M96, M97

M96 and M97 are M codes for user macro interruption control. The M code for user macro interruption control is processed internally, and is not output externally. To use M96 and M97 as a miscellaneous function, change the setting to another M code with the parameter (#1109 subs_M and #1110 M96_M, #1111 M97_M).

Subprogram call/completion : M98, M99

These commands are used as the return instructions from branch destination subprograms and branches to subprograms. M98 and M99 are processed internally and so M code signals and strobe signals are not output.

Internal processing with M00/M01/M02/M30 commands

Internal processing suspends pre-reading when the M00, M01, M02 or M30 command has been read. Other tape rewinding operations and the initialization of modals by resetting differ according the machine specifications.

9. Miscellaneous Functions 9.2 2nd Miscellaneous Functions (A8-digits, B8-digits or C8-digits)

164

9.2 2nd Miscellaneous Functions (A8-digits, B8-digits or C8-digits)

Function and purpose

These serve to assign the indexing table positioning and other such functions. In this controller, they are assigned by an 8-digit number from 0 to 99999999 following address A, B or C. The machine tool builder determines which codes correspond to which positions. If the A, B or C function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which sequence applies.

(1) The A, B or C function is executed after the movement command.

(2) The A, B or C function is executed simultaneously with the movement command.

Processing and completion sequences are required for all 2nd miscellaneous functions. The table below given the various address combinations. It is not possible to use an address which is the same for the axis name of an additional axis and 2nd miscellaneous function.

Additional axis name

2nd miscellaneous function A B C

A B C

(Note) When "A" has been assigned as the 2nd miscellaneous function address, the following commands cannot be used.

(1) Linear angle commands (,A can be used.)

(2) Geometric I commands

(3) Deep hole drilling cycle 2 commands

9. Miscellaneous Functions 9.3 Index Table Indexing

165

9.3 Index Table Indexing Function and purpose

Index table indexing can be carried out by setting the index axis. The indexing command only issues the indexing angle to the axis set for indexing. It is not necessary to command special M codes for table clamping and unclamping, thus simplifying the program.

Detailed description

The index table index function carries out operations as follows.

(Example) G00 B90 ;

The axis that was designated as the index axis with parameter "#2076 index x".

(1) Set the "index_x" parameter (#2076) for the axis in which index table indexing will be carried out to "1".

(2) The movement command (either absolute or incremental) for the selected axis is executed with the program command.

(3) An unclamp process are carried out before the axis movement.

(4) The commanded axis movement starts after the unclamp process completes.

(5) The clamp process is carried out after the movement is completed.

(6) The next block is processed after the unclamp process completes.

T10 FIN WAIT 0800 T10 FIN WAIT 0800

B axis movement

Unclamp completed

Unclamp command

G0 B90. ;Program command

9. Miscellaneous Functions 9.3 Index Table Indexing

166

Precautions

(1) Several axes can be set as index table indexing axes.

(2) The movement speed of index table indexing axes follows the feed rate of the modal (G0/G1) at that time.

(3) The unclamp process for the indexing axes is also issued when the index table indexing axes are commanded in the same block as other axes. Thus, the movement of other axes commanded in the same block is not carried out until the unclamp process completes.

Note that the movement of other axes commanded in the same block is carried out for non-interpolation commands.

(4) Index table indexing axes are used as normal rotation axes, but this function performs an unclamp process even for linear axes.

(5) If some error that makes unclamp command OFF occurs during indexing axis movement in automatic operation, the unclamp state will be remained, and the indexing axis will execute a deceleration stop.

Other axes commanded in the same block will also execute a deceleration stop, except for non-interpolation commands.

(6) If the axis movement is interrupted by an interlock, etc., during indexing axis movement, the unclamp state will be remained.

(7) The clamp and unclamp process are not executed when the movement commands of the index table indexing axis are continuous.

Note that the clamp and unclamp process are executed even when the movement commands are continued during single block operation.

(8) Make sure that the command position is at a position where clamping is possible.

10. Spindle Functions 10.1 Spindle Functions (S2-digits BCD)

167

10. Spindle Functions 10.1 Spindle Functions (S2-digits BCD) ..... During Standard PLC Specifications

Function and purpose

The spindle functions are also known simply as S functions and they assign the spindle rotation speed. In this controller, they are assigned with a 2-digit number following the address S ranging from 0 to 99, and 100 commands can be specified. Note that how many of these 100 types can be used, and which value corresponds to the actual rotation speed differs for each machine. Refer to the Instruction Manual issued by the machine tool builder for more details. When a number exceeding 2 digits is assigned, the last 2 digits will be valid. If the S function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which sequence applies.

(1) The S function is executed after the movement command.

(2) The S function is executed simultaneously with the movement command.

Processing and completion sequences are required for all S commands from S00 to S99. 10.2 Spindle Functions (S6-digits Analog)

Function and purpose

When the S6-digits function is added, a 6-digit value (0 to 999999) can be designated after the S code. Other commands conform to the S2-digits function. Always select S command binary output when using this function. In this function, the appropriate gear signal, voltage corresponding to the commanded spindle rotation speed, and start signal are output by the numeric command of the six digits following the S code. Processing and completion sequences are required for all S commands. The analog signal specifications are given below.

(1) Output voltage................. 0 to 10V

(2) Resolution......................... 1/4096 (2-12)

(3) Load conditions. 10k

(4) Output impedance. 220 If the parameters for up to 4 gear stages are set in advance, the gear stage corresponding to the S command will be selected and the gear signal will be output. The analog voltage is calculated in accordance with the input gear signal.

(1) Parameters corresponding to individual gears Limit rotation speed, maximum rotation speed, shift rotation speed and tapping rotation speed

(2) Parameters corresponding to all gears. Orientation rotation speed, minimum rotation speed

10. Spindle Functions 10.3 Spindle Functions (S8-digits)

168

10.3 Spindle Functions (S8-digits)

Function and purpose

These functions are assigned with an 8-digit (0 to 99999999) number following the address S, and one group can be assigned in one block. The output signal is a 32-bit binary data with sign and start signal. Processing and completion sequences are required for all S commands.

10. Spindle Functions 10.4 Constant Surface Speed Control

169

10.4 Constant Surface Speed Control; G96, G97

Function and purpose

These commands automatically control the spindle rotation speed in line with the changes in the radius coordinate values as cutting proceeds in the diametrical direction, and they serve to keep the cutting point speed constant during the cutting.

Command format

G96 S__ P__ ; Constant surface speed ON S P

Surface speed Designation of constant surface speed control axis

G97; Constant surface speed cancel

Detailed description

(1) The constant surface speed control axis is set by parameter (#1181 G96_ax).

0 : Fixed at 1st axis (P command invalid) 1 : 1st axis 2 : 2nd axis 3 : 3rd axis

(2) When the above-mentioned parameter is not zero, the constant surface speed control axis can be designated by address P. (Example) When G96_ax = 1

Program Constant surface speed control axis G96 S100 ; 1st axis G96 S100 P3 ; 3rd axis

(3) Example of selection program and operation

G90 G96 G01 X50. Z100. S200 ;

~

The spindle rotation speed is controlled so that the surface speed is 200m/min.

G97 G01 X50. Z100. F300 S500 ; ~

The spindle rotation speed is controlled to 500 r/min.

M02 ; The modal returns to the initial value.

(4) The spindle subject to control is determined with the following. For multiple-spindle control I (#1300 ext36 bit0 = 0), the spindle is determined by the spindle

selection command in the G group 20. For multiple-spindle control II (#1300 ext36 bit0 = 1), the spindle is determined by the spindle

selection signal (SWS) from the PLC.

10. Spindle Functions 10.5 Spindle Clamp Speed Setting

170

10.5 Spindle Clamp Speed Setting; G92

Function and purpose

The maximum clamp rotation speed of the spindle can be assigned by address S following G92 and the minimum clamp rotation speed by address Q.

Command format

G92 S__ Q__ ; S Q

Maximum clamp rotation speed Minimum clamp rotation speed

Detailed description

Besides this command, parameters can be used to set the rotation speed range up to 4 stages in 1 r/min units to accommodate gear selection between the spindle and spindle motor. The lowest upper limit and highest lower limit are valid among the rotation speed ranges based on the parameters and based on "G92 Ss Qq ;".

Set in the parameter (#1146 Sclamp, #1227 aux11/bit5) whether to carry out rotation speed clamp only in the constant surface speed mode or even when the constant surface speed is canceled. (Note) G92S command and rotation speed clamp operation

Sclamp = 0 Sclamp = 1 aux11/bit5 = 0 aux11/bit5 = 1 aux11/bit5 = 0 aux11/bit5 = 1

In G96 ROTATION SPEED CLAMP COMMAND

ROTATION SPEED CLAMP COMMAND Command

In G97 SPINDLE ROTATION SPEED COMMAND

ROTATION SPEED CLAMP COMMAND

In G96 ROTATION SPEED CLAMP EXECUTION

ROTATION SPEED CLAMP EXECUTION

Operation In G97 NO ROTATION SPEED CLAMP

ROTATION SPEED CLAMP EXECUTION

NO ROTATION SPEED CLAMP

10. Spindle Functions 10.6 Spindle/C Axis Control

171

10.6 Spindle/C Axis Control Function and purpose

This function enables one spindle (MDS-A-SP and later) to also be used as a C axis (rotation axis) by an external signal.

Detailed description

(1) Spindle/C axis changeover

Changeover between the spindle and C axis is done by the C axis SERVO ON signal.

At servo OFF .................Spindle (C axis control not possible) At servo ON ...................C axis (spindle control not possible)

The C axis is in a reference position return incomplete state.

C axis Spindle Spindle Servo ON

Reference position return state Reference position return is incomplete when the Z phase has not been passed. Reference position return is complete when the Z phase has been passed. C axis potion data The NC's internal C axis position data is updated even for the spindle rotation during

spindle control. The C axis coordinate value counter is held during spindle control, and is updated

according to the amount moved during spindle control when the C axis servo READY is turned ON. (The C axis position at servo ON may differ from the position just before the previous servo OFF.)

(2) Changeover timing chart example

2

Recalculation request

Blocks being executed

Reference position return complete status

C axis command (automatic operation)

Spindle forward run/ reverse run start

Servo ON

Servo READY

Motor speed C axis movement

Program error (P430 AXIS NOT RET.)

Reference position return complete

Reference position return complete

OrientationOrientation

Spindle reverse run

Reverse run

2 1

1

Forward run

Spindle forward run

C axis command

Servo ON C axis command C axis command

recalculation

Servo OFF

Spindle reverse run

C axis command

Spindle forward run Spindle reverse run Servo ON Servo OFF Servo ON

Servo ON

Program error because the reference position return is incomplete at this calculation.

Reference position return complete at recalculation

Blocks being calculated

10. Spindle Functions 10.6 Spindle/C Axis Control

172

(Note) For axis commands, the reference position return complete is checked at calculation. Thus, when the C axis servo ON command and C axis command are continuous, the program error (P430) will occur as shown above in 2.

In response to this kind of situation, the following two processes must be carried out on user PC, as shown above in 1.

Input the recalculation request signal with a servo ON command.

Wait for the completion of the servo ON command until the C axis enters a servo READY state.

(3) C axis gain

The C axis gain is changed over (the optimum gain is selected) by the C axis cutting condition. During C axis cutting feed, cutting gain is applied. During other axis' cutting feed (C axis face turning), non-cutting stop gain is applied. Non-cutting gain is applied in all other cases.

Z axis command (other part system)

X axis command (C axis part system)

Selected gain

C axis command

Non-cutting gain

Non-cutting gainNon-cutting gain Cutting stop gain Cutting gain

G1

G1

G1G0

G0

G1

G0

G0

(Note 1) The cutting feed of other part systems does not affect the C axis gain selection.

(Note 2) There are 1st to 3rd cutting gains, which are selected with the ladder. (4) Deceleration check in movement including spindle/C-axis

The deceleration check in a movement command including the spindle/C-axis is as the table described below when the following condition is fulfilled.

When the different values are set for the position loop gain in non-cutting mode (spindle parameter #3203 PGCO) and the position loop gain in cutting mode (spindle parameter #3330 PGC1 to #3333 PGC4).

That is because a vibration and so on occurs in the machine when the gain is changed during the axis movement.

Parameter Rapid traverse

command Parameter

Other than rapid traverse command (G1 : other than G0 command)

Inpos (#1193)

G0XX (G0+G9XX)

AUX07/BIT-1 (#1223/BIT-1)

G1+G9XX (G1+G9XX)

G1 G1

0 Command

deceleration check 0

1 In-position

check 1

In-position check

(Applicable only to SV024)

No deceleration check

(Note 1) When G1 command is issued, the in-position check is performed regardless of the deceleration check parameter.

(Note 2) XX expresses all commands.

10. Spindle Functions 10.6 Spindle/C Axis Control

173

Precautions and Restrictions

(1) The program error (P430) will occur if a C axis command is issued during servo OFF or during

orientation.

(2) Do not execute a servo OFF during a C axis command. The remaining C axis commands will be cleared at servo ON. (If servo OFF is executed during C axis control, the feed will stop and spindle control will

occur.)

(3) If servo ON is executed during spindle rotation, the rotation will stop and C axis control will occur.

(4) Dog-type reference position return is not possible for the C axis. Set the reference position return to the orientation method in the parameters (Spindle base

specifications parameters "#3106 zrn_typ/bit8" = 0), or set the axis to "Axis without reference position (zero point)" (Zero point return parameters "#2031 noref: 1").

10. Spindle Functions 10.7 Spindle Synchronization

174

10.7 Spindle Synchronization

Function and purpose

In a machine having two or more spindles, this function controls the rotation speed and phase of one spindle (basic spindle) in synchronization with the rotation of the other spindle (synchronous spindle). The function is used when the rotation speed of the two spindles must be matched, for example, if a workpiece grasped by the 1st spindle is to be grasped by a 2nd spindle, or if the spindle rotation speed has to be changed when one workpiece is grasped by both the 1st and 2nd spindles. There are two types of spindle synchronization: Spindle synchronization I and Spindle synchronization II.

The spindle synchronization control I

The designation of the synchronous spindle and start/stop of the synchronization are executed by commanding G codes in the machining program.

The spindle synchronization function II

The selections of the synchronized spindle and synchronization start, etc., are all designated from the PLC. Refer to the instruction manual issued by the machine tool builder for details.

Common setting for the spindle synchronization control I and II

When the spindle synchronization control is carried out, the followings must be set.

Chuck close Error temporary cancel Multi-speed acceleration/deceleration

For details, refer to the "10.7.3 Precautions for Using Spindle Synchronization Control".

10. Spindle Functions 10.7 Spindle Synchronization

175

10.7.1 Spindle Synchronization Control I

Function and purpose

With the spindle synchronization control I, the designation of the synchronous spindle and start/stop of the synchronization are executed by commanding G codes in the machining program.

Command format

(1) Spindle synchronization ON (G114.1)

This command designates the basic spindle and synchronous spindle, and synchronizes the two designated spindles. By commanding the synchronous spindle phase shift amount, the phases of the basic spindle and synchronous spindle can be aligned.

G114.1 H__ D__ R__ A__ ; H Basic spindle selection D Synchronous spindle selection R Synchronous spindle phase shift amount A Spindle synchronization acceleration/deceleration time constant

(2) Spindle synchronization cancel (G113)

This command cancels the synchronous state of the two spindles rotating in synchronization with the spindle synchronization command.

G113 ;

Add- ress

Meaning of address

Command range (unit) Remarks

H Basic spindle selection Select the No. of the spindle to be used as the basic spindle from the two spindles.

1 to 6 1: 1st spindle 2: 2nd spindle 3: 3rd spindle 4: 4th spindle 5: 5th spindle 6: 6th spindle

A program error (P35) will occur if a value exceeding the command range or spindle No. without specifications is commanded.

A program error (P33) will occur if there is no command.

A program error (P700) will occur if a spindle not serially connected is commanded.

D Synchronous spindle selection Select the No. of the spindle to be synchronized with the basic spindle from the two spindles.

1 to 6 or -1 to -6 1: 1st spindle 2: 2nd spindle 3: 3rd spindle 4: 4th spindle 5: 5th spindle 6: 6th spindle

A program error (P35) will occur if a value exceeding the command range is commanded.

A program error (P33) will occur if there is no command.

A program error (P33) will occur if the same spindle as that commanded for the basic spindle selection is designated.

The rotation direction of the synchronous spindle in respect to the basic spindle is commanded with the D sign.

A program error (P700) will occur if a spindle not serially connected is commanded.

10. Spindle Functions 10.7 Spindle Synchronization

176

Add- ress

Meaning of address

Command range (unit) Remarks

R Synchronous spindle phase shift amount Command the shift amount from the reference point (one rotation signal) of the synchronous spindle.

0 to 359.999 ( ) or 0 to 35999 ( * 10-3)

A program error (P35) will occur if a value exceeding the command range is commanded.

The commanded shift amount is effective in the clockwise direction of the basic spindle.

If there is no R command, the phases will not be aligned.

A Spindle synchronization acceleration/decele- ration time constant Command the acceleration/decele- ration time constant for when the spindle synchronization command rotation speed changes. (Command this to accelerate or decelerate at a speed slower than the time constant set in the parameters.)

0.001 to 9.999 (s) or 1 to 9999 (ms)

A program error (P35) will occur if a value exceeding the command range is commanded.

If the commanded value is smaller than the acceleration/deceleration time constant set with the parameters, the value set in the parameters will be applied.

Rotation speed and rotation direction

(1) The rotation speed and rotation direction of the basic spindle and synchronous spindle during

spindle synchronization are the rotation speed and rotation direction commanded for the basic spindle. Note that the rotation direction of the synchronous spindle can be reversed from the basic spindle through the program.

(2) The basic spindle's rotation speed and rotation direction can be changed during spindle synchronization.

(3) The synchronous spindle's rotation command is also valid during spindle synchronization. When spindle synchronization is commanded, if neither a forward run command nor reverse

run command is commanded for the synchronous spindle, the synchronization standby state will be entered without starting the synchronous spindle's rotation. If the forward run command or reverse run command is input in this state, the synchronous spindle will start rotation. The synchronous spindle's rotation direction will follow the direction commanded in the program.

If spindle stop is commanded for the synchronous spindle during spindle synchronization (when both the forward run and reverse run commands are turned OFF), the synchronous spindle rotation will stop.

(4) The rotation speed command (S command) and constant surface speed control are invalid for the synchronous spindle during spindle synchronization. Note that the modal is updated, so these will be validated when the spindle synchronization is canceled.

(5) The constant surface speed can be controlled by issuing a command to the basic spindle even during spindle synchronization.

10. Spindle Functions 10.7 Spindle Synchronization

177

Rotation synchronization

(1) When rotation synchronization control (command with no R address) is commanded with the

G114.1 command, the synchronous spindle rotating at an arbitrary rotation speed will accelerate or decelerate to the rotation speed commanded beforehand for the basic spindle, and will enter the rotation synchronization state.

(2) If the basic spindle's commanded rotation speed is changed during the rotation synchronization state, acceleration/deceleration will be carried out while maintaining the synchronization state following the spindle acceleration/deceleration time constants set in the parameters, and the commanded rotation speed will be achieved.

(3) In the rotation synchronization state, the basic spindle can be controlled to the constant surface speed even when two spindles are grasping one workpiece.

(4) Operation will take place in the following manner.

M23 S2=750 ; : M03 S1=1000 ; : G114.1 H1 D-2 ; : S1=500 ; : G113 ;

... Forward rotate 2nd spindle (synchronous spindle) at 750

r/min (speed command) ... Forward rotate 1st spindle (basic spindle) at 1000 r/min

(speed command) ... Synchronize 2nd spindle (synchronous spindle) to 1st

spindle (basic spindle) with reverse run ... Change 1st spindle (basic spindle) rotation speed to 500

r/min ... Cancel spindle synchronization

1000

750

500

0

500

750

1000

2nd spindle (synchronous spindle) forward run

1st spindle (basic spindle) forward run

2nd spindle (synchronous spindle) reverse run synchronization

1st spindle (basic spindle) rotation speed change

Spindle synchronization cancel

Basic spindle Synchronous spindle

Forward run

Reverse run

Rotation speed (r/min)

10. Spindle Functions 10.7 Spindle Synchronization

178

Phase synchronization

(1) When phase synchronization (command with R address) is commanded with the G114.1

command, the synchronous spindle rotating at an arbitrary rotation speed will accelerate or decelerate to the rotation speed commanded beforehand for the basic spindle, and will enter the rotation synchronization state.

Then, the phase is aligned so that the rotation phase commanded with the R address is reached, and the phase synchronization state is entered.

(2) If the basic spindle's commanded rotation speed is changed during the phase synchronization state, acceleration/deceleration will be carried out while maintaining the synchronization state following the spindle acceleration/deceleration time constants set in the parameters, and the commanded rotation speed will be achieved.

(3) In the phase synchronization state, the basic spindle can be controlled to the constant surface speed even when two spindles are grasping one workpiece.

(4) Operation will take place in the following manner.

M23 S2=750 ; : M03 S1=1000 ; : G114.1 H1 D-2 Rxx ; : : S1=500 ; : G113 ;

... Forward rotate 2nd spindle (synchronous spindle) at 750

r/min (speed command) ... Forward rotate 1st spindle (basic spindle) at 1000 r/min

(speed command) ... Synchronize 2nd spindle (synchronous spindle) to 1st

spindle (basic spindle) with reverse run Shift phase of synchronous spindle by R command value

... Change 1st spindle (basic spindle) rotation speed to 500 r/min

... Cancel spindle synchronization

10. Spindle Functions 10.7 Spindle Synchronization

179

1000

750

500

0

500

750

1000

Basic spindle Synchronous spindle

2nd spindle (synchronous spindle) forward run

1st spindle (basic spindle) forward run

2nd spindle (synchronous spindle) reverse run synchronization

1st spindle (basic spindle) rotation speed change

Spindle synchronization cancel

Forward run

Reverse run

Phase alignment

Rotation speed (r/min)

(Note 1) Acceleration/Deceleration at the phase synchronization is the step synchronization method when "#3130 syn_spec/bit1" = "0", the multi-step acceleration/deceleration method when "#3130 syn_spec/bit1" = "1".

10. Spindle Functions 10.7 Spindle Synchronization

180

Spindle synchronization phase shift amount calculation function

The spindle phase shift amount calculation function obtains and saves the phase difference of the basic spindle and synchronous spindle by turning the PLC signal ON when the phase synchronization command is executed. When the phase is positioned to the automatically saved phase difference before executing the phase synchronization control command, phases can be aligned easier when re-grasping profile materials. (1) Saving the basic spindle and synchronous spindle phase difference

(a) Set a profile material in the main spindle (basic spindle).

(b) Set the profile material in the rear spindle.

(c) Turn the phase shift calculation request signal (SSPHM) ON.

(d) Input a rotation command, with 0 speed, for the main spindle (basic spindle) and rear spindle (synchronous spindle).

M3 S1=0 M24 S2 = 0;

(e) Execute the rotation synchronization signal (with no R address command). <Example> G114.1 H1 D-2;

(f) Rotate the main spindle at the speed actually used when re-grasping. S1 = 3000;

(g) Check that the phase difference has been saved by looking at the spindle speed synchronization complete signal.

(h) Stop both spindles.

(i) Turn the phase shift calculation request signal OFF.

Basic spindle Synchronous spindle

: Saved phase difference

Example of operation macro M6; M15; G113; M3 S1=0

M24 S2=0; G114.1 H1 D-2;

S1=3000; M77; S1=0; G4X_; G113;

Automatic operation start (ST, PLC CNC) Phase shift calculation request signal

(SSPHM, PLC CNC)

Spindle rotation speed synchronization complete signal

(FSPRV, CNC PLC)

Basic spindle and synchronous spindle phase difference save complete

Basic spindle chuck close M code

Synchronous spindle chuck close M code Spindle synchronization complete check M code

Basic spindle forward run command (M3) Basic spindle reverse run command (M24)

NC reset

10. Spindle Functions 10.7 Spindle Synchronization

181

(2) Automatic phase alignment of basic spindle and synchronous spindle

(a) Turn the phase offset request signal ON.

(b) Issue the phase synchronization command (with R command). G114.1 H1 D-2 R0;

(c) The phase is aligned by offsetting the phase synchronization command by the phase difference obtained with the spindle synchronization phase shift calculation function. The state in which the synchronous spindle phase shift amount designation R value is 0 is the same as the reference state (state obtained with phase shift calculation request signal).

Basic spindle

Phase alignment

Synchronous spindle

: Phase difference

Machining program example G114.1 H1 D-2 R_; M77; Phase offset request signal (SSPHF, PLC CNC) Spindle phase synchronization

complete signal

(FSPPH, CNC PLC)

Basic spindle and synchronous spindle phase alignment complete

Spindle synchronization complete check M code

10. Spindle Functions 10.7 Spindle Synchronization

182

Multi-step acceleration/deceleration

Acceleration/deceleration time constants for up to eight steps can be selected according to the spindle rotation speed for the acceleration/deceleration during spindle synchronization. The acceleration/deceleration in each step is as follows. Time required from minimum rotation speed to maximum rotation speed in each step

= [Time constant without multi-step acceleration deceleration] * [Magnification of time constant in each step] * [Rate of rotation speed width in each step in respect to rotation speed width up to limit rotation speed]

Time required to rotate to sptc1 set rotation speed from stopped state (a)

= spt (or A command when G114.1 is commanded) * sptc1/slimit Time required to reach sptc2 set rotation speed from sptc1 (b)

= spt (or A command when G114.1 is commanded) * spdiv1 * (sptc2 - sptc1)/slimit Time required to reach sptc3 set rotation speed from sptc2 (c)

= spt (or A command when G114.1 is commanded) * spdiv2 * (sptc3 - sptc2)/slimit Time required to reach sptc4 set rotation speed from sptc3 (d)

= spt (or A command when G114.1 is commanded) * spdiv3 * (sptc4 - sptc3)/slimit Time required to reach sptc5 set rotation speed from sptc4 (e)

= spt (or A command when G114.1 is commanded) * spdiv4 * (sptc5 - sptc4)/slimit Time required to reach sptc6 set rotation speed from sptc5 (f)

= spt (or A command when G114.1 is commanded) * spdiv5 * (sptc6 - sptc5)/slimit Time required to reach sptc7 set rotation speed from sptc6 (g)

= spt (or A command when G114.1 is commanded) * spdiv6 * (sptc7 - sptc6)/slimit Time required to reach sptc8 set rotation speed from sptc7 (h)

= spt (or A command when G114.1 is commanded) * spdiv7 * (slimit - sptc7)/slimit

Rotation speed (r/min)

slimit

sptc7

sptc6

sptc5

sptc4

sptc3

sptc2

sptc1

0

(a) (b) (c) (d) (e) (f) (g) (h) spt Time (ms)

To decrease the number of acceleration/deceleration steps during spindle synchronization, set one of the following for the unnecessary step. Magnification for time constant changeover speed (spdiv7 to spdiv1) = 0 (or 1) Spindle synchronous multi-step acceleration/deceleration changeover speed (sptc7 to sptc1) =

Limit rotation speed (slimit) or higher

10. Spindle Functions 10.7 Spindle Synchronization

183

Cautions on programming

(1) To enter the rotation synchronization mode while the basic spindle and synchronous spindle

are chucking the same workpiece, turn the basic spindle and synchronous spindle rotation commands ON before turning the spindle synchronization mode ON.

$1 (1st part system) $2 (2nd part system) : : M6 ; 1st spindle chuck close : : M25 S2=0 ; 2nd spindle stops at S=0 : : !2 ; !1 ; Synchronization between

part systems M5 S1=0 ; 1st spindle stops at S=0 M15 ; 2nd spindle chuck close : M24 ; 2nd spindle rotation

command ON M3 ; 1st spindle rotation

command ON :

!2 ; !1 ; Synchronization between

part systems : G114.1 H1 D-2 ; Rotation synchronization : : mode ON S1=1500 ; Synchronous rotation at

S=1500 :

: : S1=0 ; G113 ;

Both spindles stop Synchronization mode OFF

(2) To chuck the same workpiece with the basic spindle and synchronous spindle in the phase

synchronization mode, align the phases before chucking.

$1 $2 : : M6 ; 1st spindle chuck close : : : M3 S1=1500 ; 1st spindle rotation

command ON :

: G114.1 H1 D-2 R0 ; Phase synchronization : : mode ON : M24 ; 2nd spindle rotation

command ON : : : M15 ; 2nd spindle chuck close

(Note 1) : :

(Note 1) Close the chuck after confirming that the spindle phase synchronization complete signal (X18AA) has turned ON (phase alignment complete).

CAUTION Do not make the synchronous spindle rotation command OFF with one workpiece chucked by the basic spindle and synchronous spindle during the spindle synchronous mode. Failure to observe this may cause the synchronous spindle stop, and hazardous situation.

10. Spindle Functions 10.7 Spindle Synchronization

184

Precautions and restrictions

(1) The spindle rotating with spindle synchronization will stop when emergency stop is applied. (2) The rotation speed clamp during spindle synchronization will follow the smaller clamp value set

for the basic spindle or synchronous spindle. (3) Orientation of the basic spindle and synchronous spindle is not possible during the spindle

synchronization mode. To carry out orientation, cancel the spindle synchronization mode first. (4) The rotation speed command (S command) is invalid for the synchronous spindle during the

spindle synchronization mode. Note that the modal will be updated, so this will be validated when spindle synchronization is canceled.

(5) The constant surface speed control is invalid for the synchronous spindle during the spindle synchronization mode. Note that the modal will be updated, so this will be validated when spindle synchronization is canceled.

(6) The rotation speed command (S command) and constant surface speed control for the synchronous spindle will be validated when spindle synchronization is canceled. Thus, the synchronous spindle may carry out different operations when this control is canceled.

(7) If the phase difference is not obtained with the phase shift calculation request signal and the phase synchronization command is executed by turning the phase offset request signal ON, the phase shift amount will not be calculated correctly.

(8) The spindle Z phase encoder position parameter (sppst) is invalid when using the spindle synchronous phase shift amount calculation function. (It is ignored)

The spindle Z phase encoder position parameter (sppst) is valid when the phase offset request signal is OFF.

(9) If the phase synchronization command (command with R address) is issued while the phase shift calculation request signal is ON, an operation error (1106) will occur.

(10) If the phase shift calculation request signal is ON and the basic spindle or synchronous spindle is rotation while rotation synchronization is commanded, an operation error (1106) will occur.

(11) If the phase synchronization command R0 ( G114.1 H1 D-2 R0) is commanded while the phase offset request signal is ON, the basic spindle and synchronous spindle phases will be aligned to the phase error of the basic spindle and synchronous spindle saved in the NC memory.

(12) If a value other than the phase synchronization command R0 ( G114.1 H1 D-2 R000) is commanded while the phase offset request signal is ON, the phase error obtained by adding the value commanded with the R address command to the phase difference of the basic spindle and synchronous spindle saved in the NC memory will be used to align the basic spindle and synchronous spindle.

(13) The phase offset request signal will be ignored when the phase shift calculation request signal is ON.

(14) The phase error of the basic spindle and synchronous spindle saved in the NC is valid only when the phase shift calculation signal is ON and for the combination of the basic spindle selection (H_) and synchronous spindle (D_) commanded with the rotation synchronization command (no R address).

For example, if the basic spindle and synchronous spindle phase error is saved as "G114.1 H1 D-2 ;", the saved phase error will be valid only when the phase offset request signal is ON and "G114.1 H1 D_2 R ;" is commanded. If "G114.1 H2 D-1 R ;" is commanded in this case, the phase shift amount will not be calculated correctly.

(15) The basic spindle and synchronous spindle phase difference saved in the NC is held until the next spindle synchronous phase shift calculation (rotation synchronization command is completed with phase shift calculation request signal ON).

(16) When the spindle synchronization commands are being issued with the PLC I/F method (#1300 ext36/bit7 OFF), a program error (P610) will occur if the spindle synchronization is commanded with G114.1/G113.

(17) Always set the "Chuck close". If the "Chuck close" is not set, an excessive load may be applied on the machine or an alarm may occur.

10. Spindle Functions 10.7 Spindle Synchronization

185

10.7.2 Spindle Synchronization II

Function and purpose

For spindle synchronization function II, selection of the synchronized spindle and synchronization start, etc., are all designated from the PLC. Refer to the instruction manual issued by the machine tool builder for details.

Basic spindle and synchronous spindle selection

Select the basic spindle and synchronous spindle for synchronous control from the PLC.

Device No. Signal name Abbrev. Explanation R7016 Basic spindle

selection - Select a serially connected spindle to be

controlled as the basic spindle. (0: 1st spindle) 1: 1st spindle 2: 2nd spindle 3: 3rd spindle 4: 4th spindle 5: 5th spindle 6: 6th spindle (Note 1) Spindle synchronization will not take

place if a spindle not connected in serial is selected.

(Note 2) If "0" is designated, the 1st spindle will be controlled as the basic spindle.

R7017 Synchronous spindle selection

- Select a serially connected spindle to be controlled as the synchronous spindle. (0: 2nd spindle) 1: 1st spindle 2: 2nd spindle 3: 3rd spindle 4: 4th spindle 5: 5th spindle 6: 6th spindle (Note 3) Spindle synchronization will not take

place if a spindle not connected in serial is selected or if the same spindle as the basic spindle is selected.

(Note 4) If "0" is designated, the 2nd spindle will be controlled as the synchronous spindle.

10. Spindle Functions 10.7 Spindle Synchronization

186

Starting spindle synchronization

The spindle synchronization mode is entered by inputting the spindle synchronization signal (SPSYC). The synchronous spindle will be controlled in synchronization with the rotation speed commanded for the basic spindle during the spindle synchronization mode. When the difference of the basic spindle and synchronous spindle rotation speeds reaches the spindle synchronization rotation speed reach level setting value (#3050 sprlv), the spindle rotation speed synchronization complete signal (FSPRV) will be output. The synchronous spindle's rotation direction is designated with the spindle synchronization rotation direction designation as the same as the basic spindle or the reverse direction.

Device No. Signal name Abbrev. Explanation Y18B0 Spindle

synchronization SPSYC The spindle synchronization mode is entered

when this signal turns ON. X18A8 In spindle

synchronization SPSYN1 This notifies that the mode is the spindle

synchronization. X18A9 Spindle rotation

speed synchronization complete

FSPRV This turns ON when the difference of the basic spindle and synchronous spindle rotation speeds reaches the spindle rotation speed reach level setting value during the spindle synchronization mode. This signal turns OFF when the spindle synchronization mode is canceled, or when an error exceeding the spindle rotation speed reach level setting value occurs during the spindle synchronization control mode.

Y18B2 Spindle synchronization rotation direction designation

- Designate the basic spindle and synchronous spindle rotation directions for spindle synchronization. 0: The synchronous spindle rotates in the

same direction as the basic spindle. 1: The synchronous spindle rotates in the

reverse direction of the basic spindle.

10. Spindle Functions 10.7 Spindle Synchronization

187

Spindle phase alignment

Spindle phase synchronization starts when the spindle phase synchronization signal (SPPHS) is input during the spindle synchronization mode. The spindle phase synchronization complete signal is output when the spindle synchronization phase reach level setting value (#3051 spplv) is reached. The synchronous spindle's phase shift amount can also be designated from the PLC.

Device No. Signal name Abbrev. Explanation Y18B1 Spindle phase

synchronization control

SPPHS Spindle phase synchronization starts when this signal is turned ON during the spindle synchronization mode. (Note 1) If this signal is turned ON in a mode

other than the spindle synchronization mode, it will be ignored.

X18AA Spindle phase synchronization complete

FSPPH This signal is output when the spindle synchronization phase reach level is reached after starting spindle phase synchronization.

R7018 Phase shift amount setting

- Designate the synchronous spindle's phase shift amount. Unit: 360/4096

Spindle synchronization signal (Y18B0)

Spindle synchronization complete signal (X18A9)

In spindle synchronization signal (X18A8)

Spindle phase synchronization signal (Y18B1)

Spindle phase synchronization complete signal (X18AA)

Spindle phase synchronization complete ON

(Note 2)

Spindle phase synchronization ON

Spindle synchronization complete ON

Spindle synchronization OFF

Spindle synchronization ON

Spindle synchronization OFF

(Note 2) Turns OFF temporarily to change the rotation speed during phase synchronization.

10. Spindle Functions 10.7 Spindle Synchronization

188

Calculating the spindle synchronization phase shift amount and requesting phase offset

The spindle phase shift amount calculation function obtains and saves the phase difference of the basic spindle and synchronous spindle by turning the PLC signal ON during spindle synchronization. When calculating the spindle phase shift, the synchronous spindle can be rotated with the handle, so the relation of the phases between the spindles can also be adjusted visually. If the spindle phase synchronization control signal is input while the phase offset request signal (SSPHF) is ON, the phases will be aligned using the position shifted by the saved phase shift amount as a reference. This makes aligning of the phases easier when grasping the material that the shape of one end differs from the other end.

Device No. Signal name Abbrev. Explanation Y18B3 Phase shift

calculation request

SSPHM If spindle synchronization is carried out while this signal is ON, the phase difference of the basic spindle and synchronous spindle will be obtained and saved.

Y18B4 Phase offset request

SSPHF If spindle phase synchronization is carried out while this signal is ON, the phases will be aligned using the position shifted by the saved phase shift amount as a basic position.

R6516 Phase difference output

- The delay of the synchronous spindle in respect to the basic spindle is output. Unit: 360/4096 (Note 1) If either the basic spindle or

synchronous spindle has not passed through the Z phase, etc., and the phase cannot be calculated, -1 will be output.

(Note 2) This data is output only while calculating the phase shift or during spindle phase synchronization.

R6518 Phase offset data

- The phase difference saved with phase shift calculation is output. Unit: 360/4096 (Note 3) This data is output only during

spindle synchronization.

Spindle synchronization signal (Y18B0)

Spindle synchronization complete signal (X18A9)

In spindle synchronization signal (X18A8)

Spindle synchronization ON

Phase shift calculation request (Y18B3)

The phase difference in this interval is saved. (The synchronous spindle can be controlled with the handle.)

Spindle synchronization OFF

Phase shift calculation request ON

Phase shift calculation request OFF

(Note 4) The phases cannot be aligned while calculating the phase shift. (Note 5) The synchronous spindle cannot be rotated with the handle when the manual operation

mode is set to the handle mode.

10. Spindle Functions 10.7 Spindle Synchronization

189

Precautions and restrictions

(1) When carrying out spindle synchronization, a rotation command must be issued to both the

basic spindle and synchronous spindle. The synchronous spindle's rotation direction will follow the basic spindle rotation direction and spindle synchronization rotation direction designation regardless of whether a forward or reverse run command is issued.

(2) The spindle synchronization control mode will be entered even if the spindle synchronization control signal is turned ON while the spindle rotation speed command is ON. However, synchronous control will not actually take place. Synchronous control will start after the rotation speed command has been issued to the basic spindle, and then the spindle synchronization complete signal will be output.

(3) The spindle rotating with spindle synchronization will stop when emergency stop is applied.

(4) An operation error will occur if the spindle synchronization signal is turned ON while the basic spindle and synchronous spindle designations are illegal.

(5) The rotation speed clamp during spindle synchronization will follow the smaller clamp value set for the basic spindle or synchronous spindle.

(6) Orientation of the basic spindle and synchronous spindle is not possible during the spindle synchronization. To carry out orientation, turn the spindle synchronization signal OFF first.

(7) The rotation speed command is invalid for the synchronous spindle during the spindle synchronization. The commanded rotation speed will be validated after spindle synchronization is canceled.

(8) The constant surface speed control is invalid for the synchronous spindle during the spindle synchronization.

(9) If the phase offset request signal is turned ON before the phase shift is calculated and then spindle phase synchronization is executed, the shift amount will not be calculated.

(10) The spindle Z-phase encoder position parameters are invalid when phase offset is carried out.

(11) If spindle phase synchronization is started while the phase shift calculation request signal is ON, the error "M01 operation error 1106" will occur.

(12) Turn the phase shift calculation request signal ON when the basic spindle and synchronous spindle are both stopped. If the phase shift calculation request signal is ON while either of the spindles is rotating, the error "M01 operation error 1106" will occur.

(13) The phase shift amount saved in the NC is held until the next phase shift is calculated. (This value is saved even when the power is turned OFF.)

(14) Always set the "Chuck close". If the "Chuck close" is not set, an excessive load may be applied on the machine or an alarm may occur.

10. Spindle Functions 10.7 Spindle Synchronization

190

10.7.3 Precautions for Using Spindle Synchronization Control

Function and purpose

Some PLC signals must be set when spindle synchronization control I or II is used. If these signals are not set, an excessive load or an alarm may occur. Refer to the instruction manual issued by the machine tool builder for details. In this section, each function and the signal are explained.

Chuck close signal

The synchronous spindle side carries out droop compensation while the chuck is opened, and aligns itself with the basic spindle. However, when the chuck is closed, the droop compensation is added, and the synchronization error with the base increases. Droop compensation is prevented with the chuck close signal and the position where the chuck is grasped is maintained with position compensation.

Device No. Signal name Abbrev. Explanation Y18B9 Chuck close - This turns ON when the chuck is closed. When

this signal turns ON, the compensation between the basic spindle and synchronous spindle will change from droop compensation to position compensation.

X18AC Chuck close confirmation

- This turns ON when the chuck close signal is received during the spindle synchronization mode.

Chuck open Chuck closeChuck close

Spindle synchronization signal (Y18B0)

Error temporary cancel (Y18B5)

In spindle synchronization signal (X18A8)

Error canceled

Synchronous spindle chuck

Spindle synchronization complete signal (X18A9)

Basic spindle chuck Chuck close Chuck close Chuck open Chuck close confirmation

Chuck open confirmation

Chuck close (Y18B9)

(Note 1) Use the error temporary cancel only when there is still an error between the spindle and synchronization with the chuck close signal.

10. Spindle Functions 10.7 Spindle Synchronization

191

Error temporary cancel function

When spindle synchronization is carried out while grasping the workpiece with the basic spindle and rotating, if the chuck is closed to grasp the workpiece with the synchronous spindle, the speed will fluctuate due to external factors and an error will occur. If spindle synchronization is continued without compensating this error, the workpiece will twist. This torsion can be prevented by temporarily canceling this error.

Device No. Signal name Abbrev. Explanation Y18B5 Error temporary

cancel SPDRP0 The error is canceled when this signal is ON.

Phase error monitor

The phase error can be monitored during spindle phase synchronization.

Device No. Signal name Abbrev. Explanation R6519 Phase error

monitor - The phase error during spindle phase

synchronization control is output as a pulse unit.

R6520 Phase error monitor (lower limit value)

- The lower limit value of the phase error during spindle phase synchronization control is output as a pulse unit.

R6521 Phase error monitor (upper limit value)

- The upper limit value of the phase error during spindle phase synchronization control is output as a pulse unit.

Multi-speed acceleration/deceleration

Up to eight steps of acceleration/deceleration time constants for spindle synchronization can be selected according to the spindle rotation speed.

Sptc1

Sptc2

Sptc3

(1) (2) (3)

Rotation speed

Time

(1) Time required from stopped state to sptc1 setting rotation speed

spt (sptc1/maximum rotation speed) (2) Time required from sptc1 to sptc2 setting rotation speed spt ((sptc2sptc1)/maximum rotation speed) spdiv1 (3) Time required from sptc2 to sptc3 setting rotation speed spt ((sptc3sptc2)/maximum rotation speed) spdiv2

10. Spindle Functions 10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

192

10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon); G114.2

Function and purpose

In a machine having a rotary tool controlled with a serial connection and having a spindle controlled with a serial connection as the workpiece axis, polygon machining can be carried out by controlling the workpiece axis rotation in synchronized with the rotation of the rotary tool axis. The serial connection control of spindle and rotary tool axis can be carried out with MDS--SP or MDS--SPJ2.

Command format

(1) Tool spindle synchronization IA (Spindle-Spindle, Polygon) ON (G114.2)

This command sets the polygon machining mode that rotates the two axes in synchronized with differing speeds by designating the rotary tool axis and workpiece axes and the rotation ratio (Number of the rotary tool gear teeth and workpiece corners) of the two designated axes (spindle and spindle).

G114.2 H__ D__ E__ L__ R__ ; H Rotary tool axis (Basic spindle) D Workpiece axis (Synchronous spindle) E Rotary tool axis rotation ratio L Workpiece axis rotation ratio R Synchronous spindle phase shift amount

(2) Spindle synchronization cancel (G113)

This command cancels the synchronization state of rotating two spindles by the spindle synchronization command.

G113 ;

Address Meaning of address Command range (unit) Remarks H Rotary tool axis

Of the two spindles, the spindle No. of the select rotation axis.

1 to number of spindles 1: 1st spindle 2: 2nd spindle 3: 3rd spindle 4: 4th spindle

If a value exceeding the command range is commanded, a program error (P35) will occur.

If there is no command, a program error (P33) will occur.

If the same value as the D command is commanded, a program error (P33) will occur.

If a spindle that is not serially connected is selected, a program error (P700) will occur.

10. Spindle Functions 10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

193

Address Meaning of address Command range (unit) Remarks

D Workpiece axis Of the two spindles, select the spindle No. of the workpiece axis.

1 to number of spindles or -1 to - (number of spindles) 1, -1: 1st spindle 2, -2: 2nd spindle 3, -3: 3rd spindle 4, -4: 4th spindle

A program error (P35) will occur if a value exceeding the command range is commanded.

If there is no command, a program error (P33) will occur.

The rotation direction of the workpiece axis in respect to the rotary tool axis is commanded with the D sign.

If the same value as the H command is commanded, a program error (P33) will occur.

If a spindle that is not serially connected is selected, a program error (P700) will occur.

E Rotary tool axis rotation ratio

Set the rotation ratio (Number of rotary tool gear teeth) of the rotary tool axis.

1 to 10 A program error (P35) will occur if a value exceeding the command range is commanded.

If there is no command, the rotation ratio will be interpreted as 1.

L Workpiece axis rotation ratio

Set the rotation ratio (Number of workpiece corners) of the workpiece axis.

1 to 999 A program error (P35) will occur if a value exceeding the command range is commanded.

If there is no command, the rotation ratio will be interpreted as 1.

R Synchronized spindle phase shift amount

Set the shift amount from the synchronized spindle's reference point (one rotation signal).

0 to 359.999 () A program error (P35) will occur if a value exceeding the command range is commanded.

The commanded shift amount is applied in the clockwise direction of the spindle.

If there is no R command, phase alignment will not be carried out.

10. Spindle Functions 10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

194

Rotation axis and rotation direction

The rotary tool axis and workpiece axis rotation speed and rotation direction during tool spindle synchronization IA (Polygon) command are as follows.

(1) The rotation speed and rotation direction of the rotary tool axis are the rotation speed

commanded with the S command and the rotation direction commanded with the M command, etc., for the spindle selected as the rotary tool axis.

(2) The workpiece axis rotation speed is determined by the number of the rotary tool gear teeth workpiece corners commanded with G114.2.

Sw = Sh

Sw : Workpiece axis rotation speed (r/min) Sh : Rotary tool axis rotation speed (r/min) L : Rotary tool axis rotation ratio (Number of rotary tool gear teeth) E : Workpiece axis rotation ratio (Number of workpiece corners)

(3) The workpiece axis rotation direction is determined by the sign of the address D commanded

with G114.2. In other words, when the D sign is "+", the workpiece axis rotates in the same direction as the rotary tool axis, and when "-", the workpiece axis rotates in the reverse direction of the rotary tool axis.

(4) After tool spindle synchronization IA (Polygon) mode is commanded, the relation of the rotary tool axis and workpiece axis rotation is held in all automatic or manual operation modes until spindle synchronization cancel (G113) is commanded, the spindle synchronization cancel signal is input, or reset (reset 1, reset 2, reset & rewind) is executed when "#1239 set11/bit3" is set to 1.

Even during feed hold, the rotary tool axis and workpiece axis synchronization state is held.

Operation for spindle-spindle polygon

The workpiece axis will be controlled in the following manner.

(1) When the spindle synchronization IA (polygon machining) mode is commanded, if neither a

forward run command nor a reverse run command is input for the workpiece axis, the workpiece axis will not start rotating even if the polygon axis is rotating, and instead will wait for synchronization. If a forward run command or reverse run command is input for the workpiece axis in this state, the workpiece axis will start rotation.

(2) If spindle stop is commanded (both forward run command and reverse run command are turned OFF) in respect to the workpiece axis during the spindle synchronization IA (polygon machining) mode, the workpiece axis rotation will stop even when the rotary tool axis is rotating.

(3) The rotation command (S command) and constant surface speed control are invalid in respect to the workpiece axis during the tool spindle synchronization IA (polygon) mode. Note that the modal will be updated, so these will be effective after the spindle synchronization is canceled.

(4) If a rotary tool axis rotation speed that exceeds the workpiece axis maximum rotation speed is commanded, the rotary tool axis rotation speed will be clamped so that the workpiece axis rotation speed does not exceed the workpiece axis maximum rotation speed.

L E

10. Spindle Functions 10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

195

Multi-step acceleration/deceleration control

(1) Acceleration/deceleration time constants for up to eight steps can be selected according to the

spindle rotation speed for the acceleration/deceleration during Spindle-Spindle polygon machining.

The acceleration/deceleration in each step is as follows.

Time required from minimum rotation speed to maximum rotation speed in each step = [Time constant without multi-step acceleration deceleration] * [Magnification of time constant in each step] * [Rate of rotation speed width in each step in respect to rotation speed width up to limit rotation speed]

Time required to rotate to sptc1 set rotation speed from stopped state (a) = spt * sptc1/slimit

Time required to reach sptc2 set rotation speed from sptc1 (b) = spt * spdiv1 * (sptc2 - sptc1)/slimit

Time required to reach sptc3 set rotation speed from sptc2 (c) = spt * spdiv2 * (sptc3 - sptc2)/slimit

Time required to reach sptc4 set rotation speed from sptc3 (d) = spt * spdiv3 * (sptc4 - sptc3)/slimit

Time required to reach sptc5 set rotation speed from sptc4 (e) = spt * spdiv4 * (sptc5 - sptc4)/slimit

Time required to reach sptc6 set rotation speed from sptc5 (f) = spt * spdiv5 * (sptc6 - sptc5)/slimit

Time required to reach sptc7 set rotation speed from sptc6 (g) = spt * spdiv6 * (sptc7 - sptc6)/slimit

Time required to reach sptc8 set rotation speed from sptc7 (h) = spt * spdiv7 * (slimit - sptc7)/slimit

Rotation speed (r/min)

slimit

sptc7

sptc6

sptc5

sptc4

sptc3

sptc2

sptc1

0

(a) (b) (c) (d) (e) (f) (g) (h) spt Time (ms)

To decrease the number of acceleration/deceleration steps, set one of the following for the unnecessary step. Magnification for time constant changeover speed (spdiv7 to spdiv1) = 0 (or 1) Spindle synchronous multi-step acceleration/deceleration changeover speed (sptc7 to sptc1) =

Limit rotation speed (slimit) or higher (2) The rotary tool axis accelerates/decelerates linearly according to the spindle synchronous

acceleration/deceleration time constant (spt) setting value of the spindle selected as the rotary tool axis and workpiece axis, whichever is larger.

(3) If the rotary tool axis command rotation speed is changed during spindle synchronization, the axis will accelerate/decelerate to the commanded rotation speed according to the spindle acceleration/deceleration set in the parameters while maintaining the synchronized state.

10. Spindle Functions 10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

196

Phase alignment control

(1) If the tool spindle synchronization IA command (with R designation) is commanded with the

G114.2 command, the synchronous spindle rotating at an arbitrary rotation speed will accelerate or decelerate to the rotation speed following the basic spindle and synchronous spindle rotation ratio command, and the spindle synchronization state will be entered. After that, the phase will be aligned to match the rotation phase commanded with the R address.

(2) The spindle synchronization phase shift amount is commanded as the shift amount from the synchronous spindle's (workpiece axis) reference point (one rotation signal). There is no shift amount in respect to the basic spindle (rotary tool axis).

(3) If the basic spindle's (rotary tool axis) commanded rotation speed is changed during the spindle synchronization state, acceleration/deceleration will be carried out following the spindle acceleration/deceleration set in the parameters while maintaining the synchronization state, and will reach the commanded rotation speed.

(4) The following type of operation will take place.

M03 S1=0 ;

Txx00 ; M83 S4=500 ;

G114.2 H4 D1 E1 L5 Rxx ;

G113 ;

Carries out forward run (speed command) 1st spindle

(synchronous spindle) Rotary tool selection Carries out forward run (speed command) 4th spindle

(basic spindle) Carries out forward run 1st spindle (synchronous spindle)

and synchronizes with 4th spindle (basic spindle). Shifts synchronous spindle phase by amount of R command value.

Cancels tool-spindle synchronization IA

10. Spindle Functions 10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

197

Time

Cancels Spindle synchronization

Basic spindle

Synchronous spindle

600

<Operation>

Rotation speed

500

400

300

200

100

0

Phase alignment

No. 1 spindle (synchronous spindle) forward run synchronization

No. 4 spindle (basic spindle) forward run

No. 1 spindle (synchronous spindle) forward run

10. Spindle Functions 10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

198

Example of program

M03 S1=0 ; 1st spindle forward run Txx00 ; Rotary tool selection M83 S4=500 ; 4th spindle forward run G00 X40.Z-5. ;

G114.2 H4 D1 E1 L10 R0 ;

Tool spindle synchronization IA (Spindle-Spindle, Polygon mode) ON

Rotary tool axis : 4th spindle Workpiece axis : 1st spindle Number of rotary tool gear teeth : 1 Rotation ratio : Number of workpiece corners as 10 Synchronous spindle phase shift amount : 0

S1 starts rotating by forward run in synchronization with S4. The phase is aligned with shift amount 0. The S1 rotation speed is 50 r/min (S2:S1 = 10:1).

G99 ; Synchronous feed mode selection

G00 X18. ; G01 Z20. F0.1 ; G00 X40. ;

Z-5. ;

1st cut in Z axis feed rate is 0.1mm per workpiece axis rotation

G00 X14. ; G01 Z20. F0.1 ; G00 X40. ;

Z-5. ;

Final cut in Z axis feed rate is 0.1mm per workpiece axis rotation

G113 ;

Spindle synchronization cancel M85 ; 4th spindle stop

M05 ; 1st spindle stop

10. Spindle Functions 10.8 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

199

Precautions for programming

(1) The axis address (X, Z, C) command in the same block as G114.2 will be ignored.

ex. G114.2 X_ ; Ignored.

(2) If a modal is commanded in the same block as G114.2, the modal will be updated. ex. G114.2 G01 ; The group 01 modal is set to G01.

(3) If a miscellaneous command (M, S, T) is commanded in the same block as G114.2, the miscellaneous command will be executed simultaneously with the change to the rotary tool machining mode. ex. G114.2 M03 ; M03 is executed simultaneously with G114.2.

(4) If there is a group 00 G code command in the same block as G114.2, the G code commanded last in the block will have the priority. ex. G114.2 G4 P30 ; G4 P30. is executed.

Precautions and Restrictions

(1) Restrictions regarding phase alignment control

(a) Make sure that the rotation ratio of spindle (and rotary tool axis spindle) actual rotation speed and encoder rotation speed has the following relation.

Spindle rotation speed/encoder rotation speed = n ("n" is an integer of 1 or more)

If this relation is not established, the encoders reference position will not stay at a constant position of the spindle, and thus the phase (position) will deviate with each phase alignment command. Note that even in this case, if the number of rotary tool gear teeth (Number of workpiece corners) is equivalent to the rotation ratio, the blade and workpiece phase (position) will not deviate. (Following relation)

(Rotary tool axis spindle rotation speed Number of rotary tool gear teeth) / encoder rotation speed = n ("n" is an integer of 1 or more)

(b) During phase alignment control, phase alignment is carried out following each spindle encoder's reference position, so if the positional relation of the workpiece and reference position (rotary tool and reference position) deviates when the power is turned OFF/ON or when the tool is changed, etc., the phase will deviate.

(2) If S is commanded in the same block as G114.2, the synchronization speed will be created at

the previous S command until the S command ends, so the spindle speed may fluctuate momentarily. Thus, do not command S in the same block if possible.

(3) Always command G114.2 in an independent block. (4) The tool spindle synchronization 1 (Spindle-Spindle, Polygon) mode cannot be commanded

during the spindle synchronization mode commanded with G114.*. "M01 Operation error 1005" will occur.

(5) If Spindle-Spindle polygon machining is commanded while the phase shift calculation request signal SSPHM is ON, "M01 Operation error 1106" will occur.

(6) Spindle-Spindle polygon machining cannot be executed by designating a spindle being used for synchronous tapping with the G114.2 command. "M01 Operation error 1007" will occur.

(7) When the spindle/C-axis is used for the Spindle-Spindle-spindle polygon machining cannot be executed by designating the C axis mode spindle with the G114.2 command. "M01 Operation error 1026" will occur.

(8) After G114.2 is commanded, the cutting feed block will not start until synchronization is established. Operation will stop with "M01 Operation error 1033".

10. Spindle Functions 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)

200

10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon); G51.2 (Only 6 and 7 in G code list)

Function and purpose

In machines having a serial connection-controlled workpiece axis, and furthermore having a serial connection-controlled spindle as a rotary tool axis, Spindle-Spindle polygon machining can be carried out by controlling the rotation of the rotary tool axis rotation in synchronization with the workpiece axis. The mode can be changed between polygon machining and Spindle-Spindle polygon machining with parameter #1501.

#1501 polyax = 0 : Spindle-Spindle polygon machining Other than 0 : NC axis- spindle polygon machining

The workpiece axis and rotary tool axis can be serially connected and controlled with MDS--SP or MDS--SPJ2. This function is valid when the G code system is 6 or 7.

Command format

(1) Polygon machining mode command

This command designates the rotary tool axis and workpiece axis, and enters the polygon machining mode that enables synchronized rotation of two axes at differing speeds. It does this by designating the rotation ratio (number of rotary tool teeth and workpiece corners) of the two designated spindles (spindle and spindle).

G51.2 H__ D__ P__ Q__ R__ ; Tool spindle synchronization IB (Spindle-Spindle, Polygon mode) ON G51.2 (or G251) H D P Q R

Polygon machining command Workpiece axis selection (Basic spindle) Rotary tool axis selection (Synchronous spindle) Rotary tool axis rotation ratio designation Workpiece axis rotation ratio designation Synchronous spindle phase shift amount

(2) Polygon machining mode cancel command

The synchronous state of the two spindles rotating in synchronization with the tool spindle synchronization command is canceled.

G50.2 ; Tool spindle synchronization IB (Spindle-Spindle, Polygon mode) OFF

The Spindle-Spindle polygon machining mode is also canceled in the following cases. Power OFF Emergency stop Reset (reset 1, reset 2, reset & rewind) (only when #1239 set11/bit3 = 1) Spindle-Spindle polygon machining cancel signal

10. Spindle Functions 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)

201

Address Meaning of address Command range (unit) Remarks H Workpiece axis selection

Command the spindle No. of the workpiece axis.

1 to number of spindles

A program error (P35) will occur if a value exceeding the command range is commanded.

A program error (P33) will occur if the same value as the D command is commanded.

A program error (P33) will occur if a spindle not serially connected is commanded.

The spindle No. set in the parameters will be applied if omitted.

D Rotary tool axis selection Command the spindle No. of the rotary tool axis.

1 to number of spindles

A program error (P35) will occur if a value exceeding the command range is commanded.

A program error (P33) will occur if the same value as the H command is commanded.

A program error (P33) will occur if a spindle not serially connected is commanded.

The spindle No. set in the parameters will be applied if omitted.

P Workpiece axis rotation ratio designation Command the workpiece axis rotation ratio (number of workpiece corners).

1 to 999 A program error (P35) will occur if a value exceeding the command range is commanded.

Q Rotary tool axis rotation ratio designation Command the rotary tool axis rotation ratio (number of tool teeth).

1 to 999 1 to 999

A program error (P35) will occur if a value exceeding the command range is commanded.

If a negative sign is commanded, the rotary tool axis will rotate in the direction opposite the workpiece axis.

R Synchronous spindle phase shift amount designation Command the shift amount from the reference point (one rotation signal) of the rotary tool axis spindle.

0 to 359.999 ( )

A program error (P35) will occur if a value exceeding the command range is commanded.

The commanded shift amount will be applied in the clockwise direction in respect to the spindle.

If there is no R command, the phase will be handled as R0.

(#1239 set11/bit4=0)

10. Spindle Functions 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)

202

Rotation and rotation direction

The workpiece axis and rotary tool axis rotation speed and rotation direction during spindle- spindle polygon machining are as follows.

(1) The workpiece axis rotation speed and rotation direction are rotation speed commanded with

the S command and the rotation direction commanded with the M command, etc., for the spindle selected as the workpiece axis.

(2) The rotary tool axis rotation speed is determined by the number of rotary tool teeth and number of workpiece corners commanded with G51.2.

Sw = Sh Sw : Rotary tool axis rotation speed (r/min) Sh : Workpiece axis rotation speed (r/min) P : Workpiece axis rotation ratio (number of workpiece corners) Q : Rotary tool axis rotation ratio (number of rotary tool teeth)

(3) The rotary tool axis rotation direction is determined by the sign of the rotary tool axis selection Q commanded with G51.2.

If the Q sign is "+", the rotary tool axis will rotate in the same direction as the workpiece axis. If the Q sign is "-", the rotary tool axis will rotate in the direction opposite the workpiece axis.

(4) After Spindle-Spindle polygon machining is commanded, the relation of the workpiece axis and rotary tool axis rotation is held until Spindle-Spindle polygon machining cancel (G50.2) is commanded, the Spindle-Spindle polygon machining cancel signal is input, or until the reset or emergency stop signal is input.

The workpiece axis and rotary tool axis synchronization states are held even at feed hold.

Polygon machining with rotary tool axis

(1) When the Spindle-Spindle polygon machining mode is commanded, even if neither the forward

run nor reverse run command is input for the rotary tool axis, the rotary tool axis will start rotating.

(2) If spindle stop is commanded to a rotary tool axis during the Spindle-Spindle polygon machining mode (when the spindle stop signal is ON), the rotary tool axis will stop rotating even if the workpiece axis is rotating.

(3) The rotation speed command (S command) and constant surface speed control are invalid for the rotary tool axis during the Spindle-Spindle polygon machining mode. Note that the modal is updated, so these will be validated when the Spindle-Spindle polygon machining is canceled.

(4) If a workpiece axis rotation speed that exceeds the rotary tool axis's maximum rotation speed is commanded, the workpiece axis rotation speed will be clamped so that the rotary tool axis rotation does not exceed the rotary tool axis's maximum rotation speed.

Q P

10. Spindle Functions 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)

203

Acceleration/deceleration control

(1) Acceleration/deceleration of the workpiece axis will be carried out linearly according to the

spindle synchronization acceleration/deceleration time constant (spt) of the spindle selected as the workpiece axis.

(2) By setting the spindle synchronization multi-speed acceleration/deceleration time constant changeover speed (spdct1 to 7) and the scale for the time constant changeover speed (spddiv 1 to 7), the acceleration/deceleration time can be changed in up to eight steps.

(3) If the workpiece axis command rotation speed is changed during the spindle synchronization state, the commanded speed will be reached by accelerating or decelerating according to the spindle acceleration/deceleration set in the parameters while maintaining the synchronized state.

Phase alignment control

(1) If the Spindle-Spindle polygon command (R=0 with no R command) is commanded with G51.2,

the workpiece axis spindle rotating at an arbitrary rotation speed will accelerate/ decelerate to the rotation speed following the rotation ratio command of the workpiece axis spindle and rotary tool axis spindle. The spindles will then enter the spindle synchronization state. After that, the phases will be aligned to realize the rotation phase commanded with the R address.

(2) The spindle synchronization phase shift amount commands the shift amount from the rotary tool axis spindle's reference point (one rotation signal). This is not the shift amount for the workpiece axis.

10. Spindle Functions 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)

204

(3) Operation takes place in the following manner.

With phase error (#1239 set11/bit4=0)

. Txx00 ; M03 S100 ; . G51.2 H1 D3 P1 Q5 Rxx ; . . . G50.2 ;

Select rotary tool Forward rotate 1st spindle (workpiece axis) (speed command) Spindle-Spindle polygon command, synchronize 3rd spindle (rotary tool axis) to 1st spindle (workpiece axis spindle) with forward run. Shift synchronous spindle's phase by R command value. Cancel Spindle-Spindle polygon mode

Time

Phase alignment

1st axis (workpiece axis) forward run synchronization

1st spindle (workpiece axis) forward run

G51.2 command spindle-spindle polygon machining start 3rd spindle (rotary tool axis) forward run

Spindle synchronization cancel

Workpiece axis Rotary tool axis

3rd spindle (rotary tool axis) forward run synchronization

Synchronization complete

Rotation speed

600

500

400

300

200

100

0

10. Spindle Functions 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)

205

No phase error (#1239 set11/bit4=1)

. Txx00 ; M03 S100 ; . G51.2 H1 D3 P1 Q5 ; . . . G50.2 ;

Select rotary tool Forward rotate 1st spindle (workpiece axis) (speed command) Spindle-Spindle polygon command, synchronize 3rd spindle (rotary tool axis) to 1st spindle (workpiece axis spindle) with forward run. Cancel Spindle-Spindle polygon mode

600

500

400

300

200

100

0

Time

Synchronization complete

1st spindle (workpiece axis) forward run synchronization

1st spindle (workpiece axis) forward run

G51.2 command spindle-spindle polygon machining start 3rd spindle (rotary tool axis) forward run

Spindle synchronization cancel

Workpiece axis Rotary tool axis

3rd spindle (rotary tool axis) forward run synchronization

Rotation speed

10. Spindle Functions 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)

206

Example of program

. . .

Txx00 ; Select rotary tool M03 S500 ; G00 X40. Z-5. ;

1st spindle forward run

G51.2 H1 D3 P1 Q3 R0 ;

Spindle-Spindle polygon machining mode ON Select 1st spindle as workpiece axis and 3rd spindle as rotary tool axis Designate rotation ratio as one workpiece corner and three rotary tool teeth Designate rotary tool axis spindle phase shift amount as 0.

Start synchronous rotation of S3 to S1 with forward run. Align phases with 0 shift amount. S3 rotation speed is 1500 r/min (S1:S3=1:3)

G99 ; Select synchronous feed mode

G00 X18. ; G01 Z20. F0.1 ; G00 X40. ;

Z-5. ;

If synchronization is not completed, wait to start cutting feed 1st cut

. . . .

G00 X14. ; G01 Z20.F0.1 ; G00 X40. ;

Z-5. ;

Final cut

G50.2 ;

Cancel Spindle-Spindle polygon machining Stop 3rd spindle

M05 ; Stop 1st spindle

. . .

10. Spindle Functions 10.9 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)

207

Cautions for programming

(1) Always command G51.2 and G50.2 in independent blocks.

(2) The R command can be omitted when entering the Spindle-Spindle polygon mode, but the P and Q commands must always be issued. Failure to do so will cause a program error (P33).

(3) To change the P, Q or R modal value while in the Spindle-Spindle polygon mode, command G51.2 again. In this case, R can be commanded independently. However, if either P or Q is also changed, always command P and Q again.

(4) Commands can be issued to each part system, but two part systems cannot be used simultaneously. The part system commanded first will be valid, and the operation error 1005 will occur for that commanded last.

(5) The spindle No. designated in the parameters will be used if D_H_ is omitted from the G51.2 command.

(6) A program error (P610) will occur if the workpiece axis No. (#1518) and rotary tool axis No. (#1519) are the same as the value set in the parameters. Program error (P33) will occur if the spindle is not serially connected.

(7) The cutting feed block will not start until synchronization is established after the G51.2 command. (Operation will stop with the operation error 1033.)

Precautions and restrictions

(1) Limits to phase alignment control

(a) Make sure that the spindle (and workpiece axis spindle) actual rotation speed and encoder rotation speed's rotation ratio has the following relation.

Spindle rotation speed/encoder rotation speed = n (n is an integer higher than 1)

If this relation is not established, the encoder's reference position will not be set at a set spindle position. Thus, the phase (position) will deviate each time the phase alignment command is executed.

Note that even in this case, if the number of workpiece corners (number of rotary tool teeth) corresponds to the rotation ratio, the phase (position) of the blade and workpiece will not deviate. (Following relation)

(Workpiece axis spindle rotation speed number of workpiece teeth)/ encoder rotation speed = n (n is an integer higher than 1)

(b) During phase alignment control, the phases are aligned to the reference position of each spindle's encoder. Thus, if the positional relation of the workpiece and reference position (workpiece and reference position) deviates when the power is turned ON/OFF or the tool is replaced, etc., the phase will deviate.

(c) When the spindle speed is reached, the speed may decelerate momentarily because of phase synchronization separately from the above phase alignment control.

10. Spindle Functions 10.10 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon)

208

10.10 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon); G51.2 (Only 6 and 7 in G code list)

Function and purpose

This function carries out polygon machining by controlling the workpiece (spindle) and tool axis (NC servo axis) to rotate in synchronization at the commanded ratio.

Command format

(1) Polygon machining mode ON

G51.2 P__ Q__ ; Spindle synchronization start (Start of polygon machining mode) P,Q

Spindle and rotary tool axis rotation ratio (P__:Q__) P : Spindle Q : Rotary tool axis Command range : Integer value between 1 and 9, 1 and 9 The rotation direction is designated with a sign. (+) : Forward rotation () : Reverse rotation

(2) Polygon machining mode OFF

G50.2 ; Spindle synchronization cancel (Polygon machining mode cancel)

Explanation of operation

Program Operation

S1000 ; The spindle rotation speed (workpiece rotation speed) is commanded G51.2 P1 Q2 ;

The polygon machining mode is entered with the G51.2 command. The spindle and rotary tool axis start rotating, and control is applied so that the spindle rotation speed and tool axis rotation speed are the commanded ratio (P:Q).

Cutting into workpiece

G50.2 ; The polygon machining mode between the spindle and rotary tool axis is canceled by the G50.2 command, and the spindle and rotary tool axis rotation stop.

The rotary tool axis is designated with the base specifications parameters "#1501 polyax".

Canceling the polygon machining mode

The polygon machining mode is canceled in the following cases.

G50.2 command Power OFF Emergency stop Reset (Reset 1, Reset 2, Reset & Rewind)

10. Spindle Functions 10.10 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon)

209

Rotation direction

(1) The spindle rotation direction during the polygon machining mode is determined by the P command sign and the spindle parameter "#3393 SP193(SPECT)/bit 4 :command polarity".

P command sign #3393 SP193/bit 4 Rotation direction ( + ) 0 CW ( + ) 1 CCW ( - ) 0 CCW ( - ) 1 CW

(2) The rotation direction of the rotary tool axis during the polygon machining mode is determined by

the Q command sign and the base specifications parameters "#1018 CCW".

Q command sign #1018 CCW Rotation direction ( + ) 0 CW ( + ) 1 CCW ( - ) 0 CCW ( - ) 1 CW

Example of program

An example of the program is shown below.

N10 G00 X100. Z20. ; Positioning N20 S1000 ; Spindle (workpiece) rotation speed command N30 G51.2 P1 Q2 ; Spindle/tool axis rotation start

(Spindle rotation speed 1000 [r/min], tool axis rotation speed 2000 [r/min])

N40 G01 X80. F10. ; X axis cut in N50 G04 X2. ; Dwell N60 G00 X100. ; X axis retract N70 G50.2 ; Spindle/tool axis rotation stop

(Note) Always command G51.2 and G50.2 in independent blocks.

10. Spindle Functions 10.10 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon)

210

Precautions

(1) The "spindle synchronization (Polygon)" specifications must be provided to use this function.

If G51.2 or G50.2 is commanded without the specifications, the program error (P39) will occur.

(2) Always command G51.2 and G50.2 in independent blocks. If the G51.2 (G50.2) command and group 0 G code are commanded in the same block, the

G code commanded last in the block will have the priority. If the G51.2 (G50.2) command and G code other than a group 0 code are commanded in

the same block, the program error (P33) will occur.

(3) While in the polygon machining mode, a movement command cannot be issued in the machining program for a servo axis set as the rotary tool axis. If a movement command is issued to the rotary tool axis during the polygon machining mode, the program error (P32) will occur.

(4) The servo axis set as the rotary tool axis can be used as a feed axis in modes other than the polygon machining mode.

(5) The following functions are invalid for the rotary tool axis during the polygon machining mode. Override Feed hold Stored stroke limit

(6) The spindle rotation speed can be changed with the S command even during the polygon machining mode. The spindle override and spindle rotation speed clamp are also valid. If the spindle rotation speed is changed, the rotary tool axis rotation speed will also change so that the spindle and rotary tool axis establish the P:Q ratio.

(7) The forward run/reverse run commands are invalid for the spindle during the polygon machining mode.

(8) If the feed rate for the rotary tool axis exceeds the rapid traverse rate (axis specifications parameters "#2001 rapid") during the polygon machining mode, the speed will be clamped at the rapid traverse rate. If the rotary tool axis is clamped at the rapid traverse rate, the spindle speed will also be set to lower than the command speed so that the spindle and rotary tool axis establish the P:Q ratio.

(9) The position loop gain for the rotary tool axis will be the value set in the axis specifications parameters "#2017 tap_g" during the polygon machining mode. The position loop gain for the spindle will be the spindle parameters "#13002 PGN" setting value.

(10) The following functions cannot be used simultaneously with polygon machining. Synchronous tap Thread cutting

(11) If an axis other than the rotary tool axis reaches the stroke end during the polygon machining mode, the axis other than the rotary tool axis will stop moving, but the rotary tool axis and spindle rotation will not stop.

(12) If the rotary tool axis reaches the stroke end during the polygon machining mode, the rotary tool axis and spindle rotation will stop, and the movement of axes other than the rotary tool axis will also stop.

(13) By setting the spindle basic specifications parameters "#3106 zrn_typ/bit4" to "0", the polygon machining will start after the spindle returns to the zero point.

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

211

10.11 Tool Spindle Synchronization II (Hobbing) ; G114.3

Function and purpose

This function is to cut the gear with hob (hob cutter). A spur gear can be machined by synchronizing and rotating the hob axis and the workpiece axis in a constant ratio. A helical gear can be machined by compensating the workpiece axis according to the gear torsion angle for the Z axis movement.

Spur gears Helical gears

By synchronizing and rotating the hob axis and the workpiece axis in a constant rotation ratio, a gear is machined so that the cutter is engaged with gear.

Hob

Gear

In this manual, the hob axis and the workpiece axis are defined as follows:

Hob axis : Rotary tool axis on which a hob is mounted Workpiece axis : Rotary axis on which a workpiece is mounted Hob threads : Number of the screw paths created by cutter part on hob. Usually this is 1 row.

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

212

Command format

(1) Hobbing mode commands (for spur gear)

The hobbing mode for spur gear in which two axes are synchronously rotated at different speeds is entered by designating the hob axis and workpiece axis, and by designating the rotation ratio (hob threads and number of gear teeth) for the two designated axes.

G114.3 H__ D__ E__ L__ R__ ;

Tool spindle synchronization control II (hobbing mode) ON

H : Hob axis D : Workpiece axis E : Hob axis rotation ratio L : Workpiece axis rotation ratio R : Workpiece axis phase shift amount

(2) Hobbing mode commands (for helical gear)

The hobbing mode for helical gear is entered by additionally designating the gear torsion angle and module or diametrical pitch.

G114.3 H__ D__ E__ L__ P__ Q__ R__ ;

Tool spindle synchronization control II (hobbing mode) ON

H : Hob axis D : Workpiece axis E : Hob axis rotation ratio L : Workpiece axis rotation ratio P : Gear torsion angle Q : Module or diametrical pitch R : Workpiece axis phase shift amount

(3) Hobbing mode cancel command

The synchronous state of the hob axis and workpiece axis rotating in synchronization with the tool spindle synchronous II (hobbing) command is canceled.

G113 ; Tool spindle synchronization II (hobbing)

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

213

Address Meaning of address Command range (unit) Remarks

H Hob axis Set the spindle No. of the hob axis.

1 to 6 If there is no command, a program error (P33) will occur.

If an analog connected spindle is selected, a program error (P33) will occur.

If the spindle No. not connected is designated, a program error (P35) will occur.

D Workpiece axis Set the rotation No. of the workpiece axis.

-9 to -1, 1 to 9 1 to 6 Axis No. (in part system) 9 : C axis

If there is no command, a program error (P33) will occur.

The rotation direction of the workpiece axis in respect to the hob axis is commanded with the D sign.

If the D sign is "+", the workpiece axis will rotate in the forward direction when the hob axis rotates in the forward direction. If the D sign is "-", the workpiece axis will rotate in the reverse direction when the hob axis rotates in the forward direction.

If the axis specified as the workpiece axis is not a rotation axis, a program error (P33) will occur.

If C axis is selected when there is no C axis, a program error (P33) will occur.

E Hob axis rotation ratio Set the hob axis rotation ratio (hob threads).

0 to 999 If there is no command, the rotation ratio will be interpreted as 1.

If E0 is commanded, the workpiece axis will stop (synchronized with the Z axis for a helical gear). (Note 2)

L Workpiece axis rotation ratio Set the workpiece axis rotation ratio (number of gear teeth).

1 to 999 If there is no command, the rotation ratio will be interpreted as 1.

R Workpiece axis phase shift amount Command the amount to shift from the workpiece axis reference point to synchronize with the hob axis reference point.

0 to 359999 (0 to 359.999) Decimal point input possible (Note 3)

The commanded shift amount will be applied in the workpiece axis counter's positive direction.

If there is no R command, phase alignment will not be carried out.

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

214

Address Meaning of address Command range (unit) Remarks

P Gear torsion angle Command the torsion angle for the helical gear.

-89000 to 89000 (-89.000 to 89.000) Decimal point input possible (Note 3)

If there is no P command, or if P0 is commanded, spur gear will be machined.

To move the Z axis in the pulse direction after entering the hobbing mode, command the direction that the workpiece axis is twisted.

P sign Torsion direction of workpiece axis

+ + direction - - direction

P sign : + -C

+Z

P sign : - -C

+Z

P

P

Q Module

Command the normal module for helical gear. When inch input, command the diametrical pitch.

Metric input Module 100 to 25000 0.1 to 25. (0.1 to 25 mm) Inch input Designate diametrical pitch 1000 to 250000 0.1 to 25. (0.1 to 25 inch-1) Decimal point input possible (Note 3)

If there is no Q command for helical gear (when P is designated), a program error (P33) will occur.

For spur gear (when P is not designated, or P0 is commanded), the Q command will be ignored.

(Note 1) If a value exceeding the command range is commanded, a program error (P35) will occur.

(Note 2) When address E = 0 is commanded, the workpiece axis will not rotate. Do not use this except for special cutting (cutting of only part of the gears, etc.).

(Note 3) The range which can be set depends on the input setting unit (parameter "#1003 iunit"). (Example)When the input setting unit is 0.000001, the range is 0 to 359.999999.

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

215

Rotation ratio change during the tool spindle synchronization control II mode

The rotation ratio and the number of hob threads can be changed stopping neither the hob axis nor the workpiece axis during tool spindle synchronization control II (hobbing) mode.

G114.3 E__ L__ P__ Q__

Rotation ratio change

E : Hob axis rotation ratio L : Workpiece axis rotation ratio P : Gear torsion angle Q : Module or diametrical pitch

(1) The G114.3 command during the tool spindle synchronization control II (hobbing) mode can

omit each address. If the address is omitted, modal value of the last command is used. (Example) When changing only the workpiece axis rotation ratio (the modal value of the last command is used excluding L.)

G114.3 L50; (2) If the followings are issued, a program error (P33) will occur.

(a) When R command (workpiece axis phase shift amount) is issued. (b) When the hob axis No. and workpiece axis No. are changed. (c) When other than 0 is commanded by E command in E=0 state, or 0 is commanded by E command in E0 state.

(3) The workpiece axis rotation speed may be changed by changing ratio. Acceleration/deceleration time constant follows spindle multi-step acceleration/deceleration time constant based on spindle rotation region of hob axis calculated in consideration for rotation ratio at workpiece axis rotation speed.

(4) Spindle rotation speed synchronization completion signal is turned OFF by changing the rotation ratio. This signal is turned ON when the workpiece axis rotation speed reaches the prescribed range for hob axis rotation speed after completing the rotation ratio change.

(5) The hob axis rotation speed cannot be changed while the rotation ratio is changed (during workpiece axis acceleration/deceleration). If the rotation command is issued for hob axis during the rotation ratio change, the commanded rotation speed is applied after completing the rotation ratio speed change.

(6) The helical gears machining by Z axis movement do not be executed while the rotation ratio is changed (during workpiece axis acceleration/deceleration). The helical gear machining is executed after completing the rotation ratio change.

(7) The phase of hob axis and workpiece axis during rotation ratio changing (during workpiece axis acceleration/deceleration) or after changing is not warrantable. A phase cannot be aligned with gears machining of the last command.

(8) The "Hob axis delay (advance) monitoring", "Compensation control by workpiece axis" and "The workpiece axis feedforward control " are invalid while the rotation ratio is changed (during workpiece axis acceleration/deceleration). These functions are valid after finishing the rotation ratio change.

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

216

Rotation speed and rotation direction

The rotation speed and rotation direction of hob axis and workpiece axis during tool spindle synchronization control II (hobbing) are as follows. (1) The rotation speed and rotation direction of hob axis are the rotation speed commanded with

the S command and the rotation direction commanded with the M command, etc., for the spindle selected as the hob axis.

When the sign of D command is + When the sign of D command is -

Hob axis : Forward rotation

Workpiece axis : + direction

Workpiece axis : - direction

Hob axis : Reverse rotation

Workpiece axis : - direction

Workpiece axis : + direction

(2) The workpiece axis rotation speed is determined by the number of the rotary tool gear teeth

workpiece corners commanded with G114.2. E Sw = Sh * L

Sw : Workpiece axis rotation speed (r/min) Sh : Hob axis rotation speed (r/min) E : Hob axis rotation ratio (hob threads) L : Workpiece axis rotation ratio (number of gear teeth)

(3) The workpiece axis rotation direction is determined by the sign of the address D commanded

with G114.3. In other words, when the D sign is "+", the workpiece axis will rotate in the same direction as the hob axis, and when "-", the workpiece axis will rotate in the direction opposite the hob axis.

(4) After tool spindle synchronization control II (hobbing) is commanded the relation of the hob axis and workpiece axis rotation is held in all operation modes of automatic and manual modes until spindle synchronization cancel (G113) is commanded or until the spindle synchronization cancel signal is input. Even during reset or feed hold, the hob axis and workpiece axis synchronization state is held.

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

217

Workpiece axis control

(1) The workpiece axis will start rotating in synchronization with the hob axis simultaneously with the commanding of G114.3. Thus, the workpiece axis accelerates rapidly when commanding G114.3 while the hob axis is rotating. So, stop the hob axis to avoid this before G114.3 commanded.

(2) The axis selection signal and in axis motion signal of workpiece axis are not output during the tool spindle synchronization control II (hobbing) mode.

(3) If a manual movement command is issued to the workpiece axis during the tool spindle synchronization control II (hobbing) mode, the manual movement will be superimposed on the workpiece axis movement with tool spindle synchronization. In this case, The axis selection signal and in axis motion signal of workpiece axis will be output. Note that, if the movement command is issued in the manual reference position return mode, an operation error (0005) occurs. An automatic movement command can be issued to the workpiece axis during the tool spindle synchronization control II (hobbing) mode. Refer to "(2) Command compensation" in "Compensation control by workpiece axis" for details of the command to the workpiece axis.

(4) The input signals of external deceleration, interlock and machine lock are following below for the workpiece axis during the tool spindle synchronization control II (hobbing) mode.

Interlock Machine lock External deceleration Movement by the hobbing function

Invalid Invalid Invalid

Movement by manual command

Valid for manual interlock

Valid for manual machine lock

Valid

Automatic compensation by incremental command

Valid for automatic interlock

Valid for automatic machine lock

Valid

(5) If a servo OFF signal is input for the workpiece axis during the tool spindle synchronization control II (hobbing) mode, the tool spindle synchronization control II (hobbing) is canceled because synchronization cannot be maintained.

(6) The workpiece axis rotation speed is determined according to the hob axis rotation speed, so designate the hob axis rotation speed so that the workpiece axis cutting clamp speed is not exceeded.

(7) The C axis counter on each screen will be updated as shown below during the tool spindle synchronization control II (hobbing) mode.

(a) When workpiece axis is a rotary-type rotation axis. The axis will rotate in the 0.000 to 359.999 range in the normal manner.

(b) When workpiece axis is a linear-type rotation axis (all coordinate values linear type) The axis will rotate in the 360 range including the machine coordinate position and workpiece coordinate position when hobbing starts.

(c) When workpiece axis is a linear-type rotation axis (workpiece coordinate value linear type) The axis will rotate in the 360 range including the workpiece coordinate position when hobbing starts.

(Example) Coordinate value when the

hobbing starts Rotation range

125.000 750.500

-252.200

() () ()

0.000 to 359.999 720.000 to1079.999

-360.000 to -0.001

() () ()

(8) If the hobbing command is issued before the workpiece axis completes zero point return, a

program error (P430) will occur.

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

218

Acceleration/deceleration control

(1) The hob axis will carry out multi-step acceleration/deceleration with the spindle synchronization acceleration/deceleration time constant (spt) set for the spindle selected as the hob axis.

Phase alignment control (Machine configuration that the phase alignment is possible)

To carry out phase alignment during hobbing, the spindle detector commanded as the hob axis must have a Z phase and satisfy the following conditions.

Control system Gear ratio conditions Semi-closed control Spindle side gear : moter side gear = 1 : 1 Full-closed control Spindle end : encoder end = 1 : 1

Phase alignment control (Operation when the zero point of hob axis is not established)

When the zero point of hob axis is not established by the hob axis rotation after turning the power ON or the spindle gear changeover, carry out phase alignment by following operation. (The zero point of hob axis is established within the range of (i) - (A) in figure. ) ) (1) When tool spindle synchronization control II (with R command) is commanded with G114.3, the

rotation axis commanded as the workpiece axis will enter the tool spindle synchronization II (hobbing) control state.

(2) The hob axis will start rotation at the Z phase detection speed (parameter "#3109 zdetspd") set in the parameters with the first S command issued for the hob axis after the hobbing control state is entered. At this time, the workpiece axis, will reach the rotation speed following the rotation ratio command for the hob axis and workpiece axis. If this command rotation speed is 0 (r/min), the hob axis will not start rotating, and instead will wait for the next S command.

(3) The hob axis and workpiece axis phases will be aligned in this state.

(4) After the phases are aligned, the hob axis will accelerate/decelerate to the rotation speed commanded with the S command. The workpiece axis will accelerate/decelerate to the rotation speed obtained based on the hob axis rotation speed allowing for the hob axis and workpiece axis rotation ratio, and will enter the synchronized state.

(5) The operation example is as follows.

Txx00; M83 S4=0; : G114.3 H4 D9 E1 L5 R0;

Select the rotary tool. Forward run the fourth spindle (hob axis). (Rotation speed is 0) Hobbing mode (phase alignment at phase difference 0) ON

S4=500; :

Rotate fourth spindle (hob axis) at 500r/min.

(1)

M85; Stop fourth spindle. (2) G113; Cancel hobbing mode. (3)

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

219

600

500

400

300

200

100

0

Hob axis Workpiece axis

Z phase detection speed

Command rotation speed

(1) (A) (2) (3)

Phase alignment control (Operation when the zero point of hob axis is established)

When the zero point of hob axis has already been established, the zero point of hob axis establishment is omitted. Thus, the process finishes fast compared with the case that the zero point of hob axis is not established. (1) When tool spindle synchronization control II (with R command) is commanded with G114.3, the

rotation axis commanded as the workpiece axis will enter the tool spindle synchronization II (hobbing) control state.

(2) The hob axis rotation speed according to the Z phase detection speed (parameter "#3109 zdetspd") set in the parameters is entered with the first S command issued for the hob axis after the hobbing control state. If this command rotation speed is 0 (r/min), the workpiece axis will not start rotating, and instead will wait for the next S command.

(3) When the state of the hob axis stopping and workpiece axis rotating, the phase alignment is carried out.

(4) After the phases are aligned, the hob axis will accelerate/decelerate to the rotation speed commanded with the S command. The workpiece axis will accelerate/decelerate to the rotation speed obtained based on the hob axis rotation speed allowing for the hob axis and workpiece axis rotation ratio, and will enter the synchronized state.

(5) The operation example is as follows.

Txx00; M83 S4=0; : G114.3 H4 D9 E1 L5 R0;

Select the rotary tool. Forward run the fourth spindle (hob axis). (Rotation speed is 0) Hobbing mode (phase alignment at phase difference 0) ON

S4=500; :

Rotate fourth spindle (hob axis) at 500r/min.

(1)

M85; Stop fourth spindle. (2) G113; Cancel hobbing mode. (3)

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

220

600

500

400

300

200

100

0

Hob axis Workpiece axis

Workpiece axis rotation speed based on Z phase detection speed

Command rotation speed

(1) (2) (3)

Compensation control by workpiece axis

(1) Automatic compensation

The workpiece axis is controlled while constantly allowing for hob axis delay (advance) caused by disturbance, etc. This is especially effective in increasing the workpiece accuracy during heavy cutting. Automatic compensation is validated with parameters. When the amount of the compensation added to the workpiece axis by hobbing conditions etc. changes greatly and rapidly, a servo alarm might occur for the workpiece axis. In that case, with the compensation amount through the primary delay filter, this enables the compensation amount fluctuation to further smoothen. However, the more widely the primary delay time constant is set, the more the effect of the compensation decreases, so the effect of the workpiece accuracy might not improve. [Spindle NC parameter] (Machine parameter) #3130 syn_spec/bit0 Tool spindle synchronization II (hobbing) automatic compensation selection OFF : No compensation ON : Hob axis delay (advance) is compensated with workpiece axis #3134 sphtc Tool spindle synchronization II (hobbing) automatic compensation primary delay time constant 0 : Primary delay filter control invalid 1 to 32768 : Primary delay filter time constant Setting unit (ms)

(2) Command compensation

Errors in the cutting workpiece shape caused by insufficient machine rigidity, etc., are compensated with the workpiece axis command in the machining program. (a) Command the workpiece axis compensation amount as an incremental value. (b) Command the workpiece axis compensation amount direction in the workpiece axis

rotation direction using a "+" command, and in the direction opposite the workpiece axis rotation using a "-" command.

(c) When the movement command is issued with absolute value for the workpiece axis during the tool spindle synchronization control II (hobbing) mode, a program error (P32) will occur.

10. Spindle Functions 10.11 Tool Spindle Synchronization II (Hobbing)

221

5

Workpiece axis compensation amount

Shape caused by insufficient rigidity

Command shape

N2 block

N1 block

Z axis

Workpiece axis (C axis) rotation direction

Program G114.3 H1 D9 E1 L10 P30. Q100.; S1 = 100; G94; N1 G01 Z20. F10; N2 G91 G01 Z20.C5.; : : : Workpiece axis

compensation amount

(Ex.)

Feedforward control during tool spindle synchronization II (hobbing) mode

A feed forward control can be issued for the hob axis and the workpiece axis during the tool/spindle synchronization control II (hobbing) mode. (1) The hob axis feedforward control is controlled according to hob axis feedforward gain (#3135

sfwd_g).

(2) The workpiece axis feedforward control is controlled according to hob axis feedforward gain (parameter "#3135 sfwd_g") for the workpiece axis rotation contents of the hob axis rotation. The feedforward control is controlled according to workpiece axis feedforward gain (#2155 hob_fwd_g) for the helical compensation of the Z axis movement.