Mitsubishi m70 руководство по параметрам

Introduction

This manual is a guide for using the MITSUBISHI CNC M700V/M70V 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 M700V/M70V Series Instruction Manual ………… IB-1500922

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».

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.

The following sings indicate prohibition and compulsory.

The meaning of each pictorial sing is as follows.

DANGER

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

WARNING

When the user may be subject to fatalities or major injuries if handling is mistaken.

CAUTION

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

This sign indicates prohibited behavior (must not do).

For example, indicates «Keep fire away».

This sign indicated a thing that is pompously (must do).

For example, indicates «it must be grounded».

CAUTION

CAUTION

rotated object

CAUTION HOT

Danger

Electric shock risk

Danger

explosive

Prohibited

Disassembly is

prohibited

KEEP FIRE AWAY

General instruction

Earth ground

Mitsubishi CNC is designed and manufactured solely for applications to machine tools to be used for industrial

purposes.

Do not use this product in any applications other than those specified above, especially those which are

substantially influential on the public interest or which are expected to have significant influence on human lives or

properties.

Not applicable in this manual.

1. Items related to operation

If the operation start position is set in a block which is in the middle of the program and the program is

started, the program before the set block is not executed. Please confirm that G and F modal and

coordinate values are appropriate. If there are coordinate system shift commands or M, S, T and B

commands before the block set as the start position, carry out the required commands using the MDI, etc.

If the program is run from the set block without carrying out these operations, there is a danger of

interference with the machine or of machine operation at an unexpected speed, which may result in

breakage of tools or machine tool or may cause damage to the operators.

Under the constant surface speed control (during G96 modal), if the axis targeted for the constant surface

speed control moves toward the spindle center, the spindle rotation speed will increase and may exceed

the allowable speed of the workpiece or chuck, etc. In this case, the workpiece, etc. may jump out during

machining, which may result in breakage of tools or machine tool or may cause damage to the operators.

For Safe Use

DANGER

WARNING

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.

2. Items related to operation

Before starting actual machining, always carry out graphic check, dry run operation and single block

operation to check the machining program, tool compensation amount, workpiece compensation amount

and etc.

If the workpiece coordinate system offset amount is changed during single block stop, the new setting will

be valid from the next block.

Turn the mirror image ON and OFF at the mirror image center.

If the tool compensation amount is changed during automatic operation (including during single block

stop), it will be validated from the next block or blocks onwards.

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.

CAUTION

Disposal

(Note) This symbol mark is for EU countries only.

This symbol mark is according to the directive 2006/66/EC Article 20 Information for end-

users and Annex II.

Your MITSUBISHI ELECTRIC product is designed and manufactured with high quality materials and

components which can be recycled and/or reused.

This symbol means that batteries and accumulators, at their end-of-life, should be disposed of

separately from your household waste.

If a chemical symbol is printed beneath the symbol shown above, this chemical symbol means that the

battery or accumulator contains a heavy metal at a certain concentration. This will be indicated as

follows:

Hg: mercury (0,0005%), Cd: cadmium (0,002%), Pb: lead (0,004%)

In the European Union there are separate collection systems for used batteries and accumulators.

Please, dispose of batteries and accumulators correctly at your local community waste collection/

recycling centre.

Please, help us to conserve the environment we live in!

Trademarks

MELDAS, MELSEC, EZSocket, EZMotion, iQ Platform, MELSOFT, GOT, CC-Link, CC-Link/LT and CC-Link

IE are either trademarks or registered trademarks of Mitsubishi Electric Corporation in Japan and/or other

countries.

Ethernet is a registered trademark of Xerox Corporation in the United States and/or other countries.

Microsoft and Windows are either trademarks or registered trademarks of Microsoft Corporation in the

United States and/or other countries.

CompactFlash and CF are either trademarks or registered trademarks of SanDisk Corporation in the United

States and/or other countries.

UNIX is a registered trademark of The Open Group in the United States and/or other countries.

Intel and Pentium are either trademarks or registered trademarks of Intel Corporation in the United States

and/or other countries.

Other company and product names that appear in this manual are trademarks or registered trademarks of the

respective companies.

( /Japanese)

( A)

Handling of our product

(English)

This is a class A product. In a domestic environment this product may cause radio interference in which case the

user may be required to take adequate measures.

( /Korean)

(A )

.

CONTENTS

1 Control Axes ……………………………………………………………………………………………………………………………… 1

1.1 Coordinate Words and Control Axes ……………………………………………………………………………………….. 2 1.2 Coordinate Systems and Coordinate Zero Point Symbols ………………………………………………………….. 3

2 Least Command Increments ………………………………………………………………………………………………………. 5

2.1 Input Setting Unit …………………………………………………………………………………………………………………. 6 2.2 Input Command Increment Tenfold …………………………………………………………………………………………. 7 2.3 Indexing Increment ………………………………………………………………………………………………………………. 8

3 Program Formats ………………………………………………………………………………………………………………………. 9

3.1 Program Format …………………………………………………………………………………………………………………. 10 3.2 File Format ………………………………………………………………………………………………………………………… 14 3.3 Optional Block Skip …………………………………………………………………………………………………………….. 16

3.3.1 Optional Block Skip; / ………………………………………………………………………………………………….. 16 3.3.2 Optional Block Skip Addition ; /n ……………………………………………………………………………………. 18

3.4 G code ……………………………………………………………………………………………………………………………… 20 3.4.1 Modal, unmodal ………………………………………………………………………………………………………….. 20 3.4.2 G Code Lists ……………………………………………………………………………………………………………….. 20

3.5 Precautions Before Starting Machining ………………………………………………………………………………….. 24

4 Pre-read Buffers ………………………………………………………………………………………………………………………. 25

4.1 Pre-read Buffers …………………………………………………………………………………………………………………. 26

5 Position Commands ………………………………………………………………………………………………………………… 27

5.1 Position Command Methods ; G90,G91 …………………………………………………………………………………. 28 5.2 Inch/Metric Conversion ; G20,G21…………………………………………………………………………………………. 30 5.3 Decimal Point Input …………………………………………………………………………………………………………….. 32

6 Interpolation Functions ……………………………………………………………………………………………………………. 37

6.1 Positioning (Rapid Traverse) ; G00……………………………………………………………………………………….. 38 6.2 Linear Interpolation ; G01 …………………………………………………………………………………………………….. 45 6.3 Circular Interpolation ; G02,G03 …………………………………………………………………………………………… 47 6.4 R Specification Circular Interpolation ; G02,G03 ……………………………………………………………………… 52 6.5 Plane Selection ; G17,G18,G19…………………………………………………………………………………………….. 54 6.6 Thread Cutting ……………………………………………………………………………………………………………………. 56

6.6.1 Constant Lead Thread Cutting ; G33………………………………………………………………………………. 56 6.6.2 Inch Thread Cutting ; G33…………………………………………………………………………………………….. 61

6.7 Helical Interpolation ; G17 to G19, G02, G03 ………………………………………………………………………….. 63 6.8 Unidirectional Positioning ; G60…………………………………………………………………………………………….. 70 6.9 Cylindrical Interpolation ; G07.1…………………………………………………………………………………………….. 72 6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113 …………………………………………………….. 79 6.11 Exponential Interpolation ; G02.3,G03.3……………………………………………………………………………….. 86 6.12 Polar Coordinate Command ; G16/G15………………………………………………………………………………… 92 6.13 Spiral/Conical Interpolation ; G02.0/G03.1(Type1), G02/G03(Type2) ……………………………………….. 99 6.14 3-dimensional Circular Interpolation ; G02.4,G03.4………………………………………………………………. 104 6.15 NURBS Interpolation ; G06.2…………………………………………………………………………………………….. 109 6.16 Hypothetical Axis Interpolation ; G07………………………………………………………………………………….. 114

7 Feed Functions ………………………………………………………………………………………………………………………. 117

7.1 Rapid Traverse Rate………………………………………………………………………………………………………….. 118 7.2 Cutting Feedrate ………………………………………………………………………………………………………………. 119 7.3 F1-digit Feed…………………………………………………………………………………………………………………….. 120 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed) ; G94,G95 ………. 123 7.5 Inverse Time Feed ; G93 ……………………………………………………………………………………………………. 127 7.6 Feedrate Designation and Effects on Control Axes ………………………………………………………………… 132 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration ………………………………………………. 137

7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration ………………………………… 142 7.9 Cutting Feed Constant Inclination Acceleration/Deceleration …………………………………………………… 151 7.10 Exact Stop Check ; G09……………………………………………………………………………………………………. 158 7.11 Exact Stop Check Mode ; G61…………………………………………………………………………………………… 162 7.12 Deceleration Check………………………………………………………………………………………………………….. 163

7.12.1 G1 -> G0 Deceleration Check…………………………………………………………………………………….. 165 7.12.2 G1 -> G1 Deceleration Check…………………………………………………………………………………….. 166

7.13 Automatic Corner Override ……………………………………………………………………………………………….. 167 7.14 Tapping Mode ; G63 ………………………………………………………………………………………………………… 172 7.15 Cutting Mode ; G64…………………………………………………………………………………………………………. 173

8 Dwell………………………………………………………………………………………………………………………………………. 175

8.1 Dwell (Time Designation) ; G04 …………………………………………………………………………………………… 176

9 Miscellaneous Functions ……………………………………………………………………………………………………….. 179

9.1 Miscellaneous Functions (M8-digits) ……………………………………………………………………………………. 180 9.2 Secondary Miscellaneous Functions (A8-digits, B8-digits or C8-digits) …………………………………….. 182 9.3 Index Table Indexing …………………………………………………………………………………………………………. 183

10 Spindle Functions …………………………………………………………………………………………………………………. 185

10.1 Spindle Functions…………………………………………………………………………………………………………….. 186 10.2 Constant Surface Speed Control ; G96,G97………………………………………………………………………… 187 10.3 Spindle Clamp Speed Setting ; G92 …………………………………………………………………………………… 189 10.4 Spindle/C Axis Control ……………………………………………………………………………………………………… 191 10.5 Multiple-spindle Control…………………………………………………………………………………………………….. 194

10.5.1 Multiple-spindle Control II ………………………………………………………………………………………….. 195

11 Tool Functions (T command) ………………………………………………………………………………………………… 197

11.1 Tool Functions (T8-digit BCD) …………………………………………………………………………………………… 198

12 Tool Compensation Functions ……………………………………………………………………………………………… 199

12.1 Tool Compensation………………………………………………………………………………………………………….. 200 12.2 Tool Length Compensation/Cancel ; G43/G44 …………………………………………………………………….. 204 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44…………………………………………. 207 12.4 Tool Radius Compensation ; G38,G39/G40/G41,G42…………………………………………………………… 214

12.4.1 Tool Radius Compensation Operation…………………………………………………………………………. 215 12.4.2 Other Commands and Operations during Tool Radius Compensation……………………………… 224 12.4.3 G41/G42 Commands and I, J, K Designation ………………………………………………………………. 234 12.4.4 Interrupts during Tool Radius Compensation ………………………………………………………………. 240 12.4.5 General Precautions for Tool Radius Compensation……………………………………………………… 243 12.4.6 Changing of Compensation No. during Compensation Mode………………………………………….. 244 12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation…………………………………….. 247 12.4.8 Interference Check …………………………………………………………………………………………………… 249 12.4.9 Diameter Designation of Compensation Amount…………………………………………………………… 258 12.4.10 Workpiece Coordinate Changing during Radius Compensation…………………………………….. 260

12.5 3-dimensional Tool Radius Compensation ; G40/G41,G42……………………………………………………. 262 12.6 Tool Radius Compensation for 5-axis Machining ; G40/G41.2,G42.2 ……………………………………… 273 12.7 Tool Position Offset ; G45 to G48 ………………………………………………………………………………………. 283 12.8 Compensation Data Input by Program ; G10……………………………………………………………………….. 291 12.9 Compensation Data Input to Variable by Program ; G11……………………………………………………….. 296 12.10 Inputting the Tool Life Management Data ; G10,G11 ………………………………………………………….. 297

12.10.1 Inputting the Tool Life Management Data by G10 L3 Command ; G10 L3,G11 ……………….. 297 12.10.2 Inputting the Tool Life Management Data by G10 L30 Command ; G10 L30,G11 ……………. 299 12.10.3 Precautions for Inputting the Tool Life Management Data…………………………………………….. 302

13 Program Support Functions …………………………………………………………………………………………………. 303

13.1 Fixed Cycles……………………………………………………………………………………………………………………. 304 13.1.1 Drilling, Spot Drilling ; G81…………………………………………………………………………………………. 308 13.1.2 Drilling, Counter Boring ; G82 …………………………………………………………………………………….. 309 13.1.3 Deep Hole Drilling Cycle ; G83 …………………………………………………………………………………… 310

13.1.3.1 Deep Hole Drilling Cycle…………………………………………………………………………………….. 310 13.1.3.2 Small Diameter Deep Hole Drilling Cycle ……………………………………………………………… 311

13.1.4 Tapping Cycle ; G84 …………………………………………………………………………………………………. 313 13.1.5 Boring ; G85…………………………………………………………………………………………………………….. 324 13.1.6 Boring ; G86…………………………………………………………………………………………………………….. 325 13.1.7 Back Boring ; G87…………………………………………………………………………………………………….. 326 13.1.8 Boring ; G88…………………………………………………………………………………………………………….. 328 13.1.9 Boring ; G89…………………………………………………………………………………………………………….. 329 13.1.10 Stepping Cycle ; G73………………………………………………………………………………………………. 330 13.1.11 Reverse Tapping Cycle ; G74…………………………………………………………………………………… 331 13.1.12 Circular Cutting ; G75 ……………………………………………………………………………………………… 333 13.1.13 Fine Boring ; G76……………………………………………………………………………………………………. 335 13.1.14 Precautions for Using a Fixed Cycle………………………………………………………………………….. 337 13.1.15 Initial Point and R Point Level Return ; G98,G99…………………………………………………………. 340 13.1.16 Setting of Workpiece Coordinates in Fixed Cycle Mode ………………………………………………. 341 13.1.17 Drilling Cycle with High-Speed Retract ………………………………………………………………………. 342 13.1.18 Acceleration/Deceleration Mode Change in Hole Drilling Cycle …………………………………….. 346

13.2 Special Fixed Cycle; G34, G35, G36, G37 ………………………………………………………………………….. 348 13.2.1 Bolt Hole Cycle ; G34………………………………………………………………………………………………… 349 13.2.2 Line at Angle ; G35 …………………………………………………………………………………………………… 350 13.2.3 Arc ; G36…………………………………………………………………………………………………………………. 351 13.2.4 Grid ; G37 ……………………………………………………………………………………………………………….. 352

13.3 Subprogram Control; G22, G23 …………………………………………………………………………………………. 353 13.3.1 Subprogram Call ; G22,G23 ……………………………………………………………………………………… 353 13.3.2 Figure rotation ; G22 I_J_K_………………………………………………………………………………………. 358

13.4 Variable Commands ……………………………………………………………………………………………………….. 361 13.5 User Macro …………………………………………………………………………………………………………………….. 366

13.5.1 User Macro Commands; G65, G66, G66.1, G67, G68(G23)…………………………………………… 366 13.5.2 Macro Call Instruction ………………………………………………………………………………………………. 367

13.5.2.1 Simple Macro Calls ; G65 ………………………………………………………………………………….. 367 13.5.2.2 Modal Call A (Movement Command Call) ; G66……………………………………………………. 370 13.5.2.3 Modal Call B (for Each Block) ; G66.1 …………………………………………………………………. 372 13.5.2.4 G Code Macro Call …………………………………………………………………………………………… 373 13.5.2.5 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call) ……………………. 374 13.5.2.6 Detailed Description for Macro Call Instruction …………………………………………………….. 375

13.5.3 ASCII Code Macro …………………………………………………………………………………………………… 377 13.5.4 Variable…………………………………………………………………………………………………………………… 381 13.5.5 Types of Variables …………………………………………………………………………………………………… 383

13.5.5.1 Common Variables …………………………………………………………………………………………… 383 13.5.5.2 Local Variables (#1 to #33) ………………………………………………………………………………… 384 13.5.5.3 Macro Interface Inputs/Outputs (#1000 to #1035, #1100 to #1135, #1200 to #1295, #1300 to #1395) ……………………… 388 13.5.5.4 Tool Compensation …………………………………………………………………………………………… 395 13.5.5.5 Workpiece Coordinate System Compensation (#5201 — #532n) ………………………………. 396 13.5.5.6 NC Alarm (#3000) …………………………………………………………………………………………….. 397 13.5.5.7 Integrating Time (#3001, #3002) ………………………………………………………………………… 398 13.5.5.8 Suppression of Single Block Stop and Miscellaneous Function Finish Signal Waiting (#3003) ………………………………………….. 398 13.5.5.9 Feed Hold, Feedrate Override, G09 Valid/Invalid (#3004) ……………………………………… 399 13.5.5.10 Message Display and Stop (#3006) …………………………………………………………………… 399 13.5.5.11 Mirror Image (#3007) ………………………………………………………………………………………. 400 13.5.5.12 G Command Modals (#4001-#4021, #4201-#4221) …………………………………………….. 401 13.5.5.13 Other Modals (#4101 — #4120, #4301 — #4320) …………………………………………………… 402 13.5.5.14 Position Information (#5001 — #5160 + n) …………………………………………………………… 403 13.5.5.15 Number of Workpiece Machining Times (#3901, #3902) ……………………………………… 406 13.5.5.16 Coordinate Rotation Parameter …………………………………………………………………………. 406 13.5.5.17 Rotary Axis Configuration Parameters ……………………………………………………………….. 407 13.5.5.18 Reverse Run Information………………………………………………………………………………….. 407 13.5.5.19 Tool Life Management (#60000 — #64700) …………………………………………………………. 408 13.5.5.20 Reading The Parameters (#100000-#100002, #100010) ……………………………………… 413 13.5.5.21 Reading PLC data (#100100-#100103,#100110) ………………………………………………… 416

13.5.5.22 Time Reading Variables (#3001, #3002, #3011, #3012) ………………………………………. 419 13.5.5.23 R Device Access Variables (#50000 — #50749, #51000 — #51749, #52000 — #52749) ………………………………………. 421 13.5.5.24 Read/write of the Workpiece Installation Error Compensation Amounts ………………….. 427

13.5.6 Operation Commands ………………………………………………………………………………………………. 428 13.5.7 Control Commands ………………………………………………………………………………………………….. 433 13.5.8 External Output Commands ; POPEN, PCLOS, DPRNT ………………………………………………. 436 13.5.9 Precautions …………………………………………………………………………………………………………….. 440 13.5.10 Actual Examples of Using User Macros……………………………………………………………………… 442

13.6 G Command Mirror Image ; G50.1,G51.1,G62…………………………………………………………………….. 446 13.7 Corner Chamfering I / Corner Rounding I …………………………………………………………………………… 450

13.7.1 Corner Chamfering I ; G01 X_ Y_ ,C_ ………………………………………………………………………… 450 13.7.2 Corner Rounding I ; G01 X_ Y_ ,R_ …………………………………………………………………………… 452 13.7.3 Corner Chamfering Expansion/Corner Rounding Expansion ………………………………………….. 454 13.7.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding …………………………….. 456

13.8 Corner Chamfering II / Corner Rounding II …………………………………………………………………………. 457 13.8.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_…………………………………………………………… 458 13.8.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_……………………………………………………………… 460 13.8.3 Corner Chamfering Expansion/Corner Rounding Expansion …………………………………………. 462 13.8.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ……………………………. 462

13.9 Linear Angle Command ; G01 X_/Y_ A_/,A_……………………………………………………………………….. 463 13.10 Geometric …………………………………………………………………………………………………………………….. 464

13.10.1 Geometric I ; G01 A_ ………………………………………………………………………………………………. 464 13.10.2 Geometric IB …………………………………………………………………………………………………………. 466

13.10.2.1 Geometric IB (Automatic calculation of two-arc contact) ; G02/G03 P_Q_ /R_………… 467 13.10.2.2 Geometric IB (Automatic calculation of linear — arc intersection) ; G01 A_ , G02/G03 P_Q_H_ ……………………………………………………………………………… 469 13.10.2.3 Geometric IB (Automatic calculation of linear — arc intersection) ; G01 A_ , G02/G03 R_H_………………………………………………………………………………….. 472

13.11 Circular Cutting ; G12,G13………………………………………………………………………………………………. 475 13.12 Parameter Input by Program ; G10 L70, G11.1 ………………………………………………………………….. 477 13.13 Macro Interruption ; ION,IOF……………………………………………………………………………………………. 480 13.14 Tool Change Position Return ; G30.1 — G30.6 ……………………………………………………………………. 488 13.15 Normal Line Control ; G40.1/G41.1/G42.1 (G150/G151/G152) …………………………………………….. 491 13.16 High-accuracy Control ; G61.1,G08………………………………………………………………………………….. 510 13.17 High-speed Machining Mode …………………………………………………………………………………………… 525

13.17.1 High-speed Machining Mode I, II ; G05 P1, G05 P2…………………………………………………….. 525 13.18 High-speed High-accuracy Control ; G05, G05.1………………………………………………………………… 527

13.18.1 High-speed High-accuracy Control I, II ………………………………………………………………………. 527 13.18.2 SSS Control …………………………………………………………………………………………………………… 533

13.19 Spline ; G05.1 Q2/Q0……………………………………………………………………………………………………… 539 13.20 High-accuracy Spline Interpolation ; G61.2………………………………………………………………………… 548 13.21 Scaling ; G50/G51………………………………………………………………………………………………………….. 550 13.22 Coordinate Rotation by Program ; G68.1/G69.1 …………………………………………………………………. 554 13.23 Coordinate Rotation Input by Parameter ; G10 I_ J_/K_………………………………………………………. 562 13.24 3-dimensional Coordinate Conversion ; G68.1/G69.1 …………………………………………………………. 575 13.25 Tool Center Point Control ; G43.4/G43.5 …………………………………………………………………………… 590 13.26 Timing Synchronization Operation ……………………………………………………………………………………. 618

13.26.1 Timing Synchronization Operation (! code) ; !L……………………………………………………………. 618 13.26.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115 ……………… 621 13.26.3 Timing Synchronization Operation with Start Point Designated (Type 2) ; G116 …………….. 623 13.26.4 Timing Synchronization Operation Function Using M codes ; M*** ……………………………….. 625

13.27 Inclined Surface Machining ; G68.2, G68.3 ……………………………………………………………………….. 629 13.27.1 How to Define Feature Coordinate System Using Euler Angles…………………………………….. 630 13.27.2 How to Define Feature Coordinate System Using Roll-Pitch-Yaw angles ……………………….. 632 13.27.3 How to Define Feature Coordinate System Using Three Points in a Plane……………………… 634 13.27.4 How to Define Feature Coordinate System Using Two Vectors …………………………………….. 636 13.27.5 How to Define Feature Coordinate System Using Projection Angles ……………………………… 638 13.27.6 How to Define Feature Coordinate System Using Tool Axis Direction ……………………………. 640 13.27.7 Tool Axis Direction Control ………………………………………………………………………………………. 642 13.27.8 Details of Operation ………………………………………………………………………………………………… 648

13.27.9 Rotary Axis Basic Position Selection …………………………………………………………………………. 652 13.27.10 Relation with Other Functions…………………………………………………………………………………. 658 13.27.11 Precautions………………………………………………………………………………………………………….. 661

13.28 Machining Condition Selection I ; G120.1,G121 …………………………………………………………………. 665 13.29 End Point Error Check Cancellation ; G69…………………………………………………………………………. 670 13.30 Coordinate Read Function ; G14 ……………………………………………………………………………………… 672

14 Coordinate System Setting Functions……………………………………………………………………………………. 675

14.1 Coordinate Words and Control Axes ………………………………………………………………………………….. 676 14.2 Basic Machine, Workpiece and Local Coordinate Systems……………………………………………………. 677 14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Position (Zero point) …………………………………… 678 14.4 Automatic Coordinate System Setting ………………………………………………………………………………… 679 14.5 Basic Machine Coordinate System Selection ; G53 ……………………………………………………………… 681 14.6 Coordinate System Setting ; G92 ………………………………………………………………………………………. 682 14.7 Reference Position (Zero point) Return ; G28,G29……………………………………………………………….. 684 14.8 2nd, 3rd, and 4th Reference Position (Zero point) Return ; G30 …………………………………………….. 688 14.9 Reference Position Check ; G27………………………………………………………………………………………… 691 14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1)……………………………….. 692 14.11 Local Coordinate System Setting ; G52……………………………………………………………………………. 703 14.12 Workpiece Coordinate System Preset ; G92.1 ………………………………………………………………….. 707 14.13 Coordinate System for Rotary Axis…………………………………………………………………………………… 712 14.14 Workpiece Installation Error Compensation ; G54.4……………………………………………………………. 715

15 Protection Function ………………………………………………………………………………………………………………. 729

15.1 Stroke Check Before Travel ; G22.1/G23.1 …………………………………………………………………………. 730

16 Measurement Support Functions ………………………………………………………………………………………….. 733

16.1 Automatic Tool Length Measurement ; G37.1 ……………………………………………………………………… 734 16.2 Skip Function ; G31 ………………………………………………………………………………………………………… 738 16.3 Multi-step Skip Function 1 ; G31.n ,G04 …………………………………………………………………………….. 743 16.4 Multi-step Skip Function 2 ; G31 P ……………………………………………………………………………………. 745 16.5 Speed Change Skip ; G31 Fn ………………………………………………………………………………………….. 747 16.6 Programmable Current Limitation ; G10 L14 ; ……………………………………………………………………… 751

Appendix 1 Program Errors ……………………………………………………………………………………………………….. 753

Appendix 2 Order of G Function Command Priority ……………………………………………………………………. 787

1 Control Axes

MITSUBISHI CNC

2

1.1 Coordinate Words and Control Axes

Function and purpose

X-Y table

X-Y and rotating table

(a) Direction of table movement

(a) Direction of table movement

(b) Direction of table rotation

+Z

+Z +Y

+X

+X +Y

(a)(a)

+Z +Y

+C

+C +Y

+X +X

(a) (b) (a)

M700V/M70V Series Programming Manual (M2/M0 Format)

1.2 Coordinate Systems and Coordinate Zero Point Symbols

3

1.2 Coordinate Systems and Coordinate Zero Point Symbols

The basic machine coordinate system is the coordinate system that expresses the position (tool change

position, stroke end position, etc.) that is specific to the machine.

Workpiece coordinate systems are used for workpiece machining.

Upon completion of the dog-type reference position return, the parameters are referred and the basic machine

coordinate system and workpiece coordinate systems (G54 to G59) are automatically set.

The offset of the basic machine coordinate zero point and reference position is set by a parameter. (Normally,

set by machine manufacturers)

Workpiece coordinate systems can be set with coordinate systems setting functions, workpiece coordinate

offset measurement (additional specification), and etc.

Reference position: A specific position to establish coordinate systems and change tools

Basic machine coordinate zero point: A position specific to machine

Workpiece coordinate zero points (G54 to G59) A coordinate zero point used for workpiece machining

1 Control Axes

MITSUBISHI CNC

4

The local coordinate systems (G52) are valid on the coordinate systems designated by workpiece coordinate

systems 1 to 6.

Using the G92 command, the basic machine coordinate system can be shifted and made into a hypothetical

machine coordinate system. At the same time, workpiece coordinate systems 1 to 6 are also shifted.

Reference position

Basic machine coordinate zero point

Workpiece coordinate zero points

Local coordinate zero point

Offset set by a parameter

Offset set by a program («0» is set when turning the power ON)

G52 Local coordinate system offset (*1)

G54 Workpiece coordinate (G54) system offset (*1)

G55 Workpiece coordinate (G55) system offset

G92 G92 Coordinate system shift

EXT External workpiece coordinate offset

(*1) G52 offset is independently possessed by G 54 to G59 respectively.

G52

G92

G55G54

EXT

G52

5

2

Least Command Increments

2 Least Command Increments

MITSUBISHI CNC

6

2.1 Input Setting Unit

Function and purpose

The input setting units are the units of setting data including tool compensation amounts and workpiece

coordinates compensation.

The program command units are the units of movement amounts in programs.

These are expressed with mm, inch or degree ().

Detailed description

Program command units for each axis and input setting units, common for all axes, are determined by the

setting of parameters as follows.

Precautions

(1) Inch/metric changeover can be handled by either a parameter screen (#1041 I_inch: valid only when the

power is turned ON) or G commands (G20 or G21).

However, the changeover by a G command applies only to the program command units, and not to the

input setting units. Consequently, the tool compensation amounts and other compensation amounts as

well as the variable data should be preset in order to correspond to input setting units.

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

(3) When performing a circular interpolation between the axes whose program command units are different,

the center command (I, J, K) and the radius command (R) are designated by the input setting units. (Use

a decimal point to avoid confusion.)

Parameter Linear axis Rotary axis

()Millimeter Inch

Input setting unit

#1003 iunit = B 0.001 0.0001 0.001

= C 0.0001 0.00001 0.0001

= D 0.00001 0.000001 0.00001

= E 0.000001 0.0000001 0.000001

Program command unit

#1015 cunit = 0 Follow #1003 iunit

= 1 0.0001 0.00001 0.0001

= 10 0.001 0.0001 0.001

= 100 0.01 0.001 0.01

= 1000 0.1 0.01 0.1

= 10000 1.0 0.1 1.0

M700V/M70V Series Programming Manual (M2/M0 Format)

2.2 Input Command Increment Tenfold

7

2.2 Input Command Increment Tenfold

Function and purpose

The program’s command increment can be multiplied by an arbitrary scale with the parameter designation.

This function is valid when a decimal point is not used for the command increment.

The scale is set with the parameter «#8044 UNIT*10».

Detailed description

(1) When running a machining program already created with a 10m input command increment with a CNC

unit for which the command increment is set to 1m and this function’s parameter value is set to «10»,

this function enables the same machining as the original program.

(2) When running a machining program already created with a 1m input command increment with a CNC

unit for which the command increment is set to 0.1m and this function’s parameter value is set to «10»,

this function enables the same machining as the original program.

(3) This function cannot be used for the dwell function G04_X_(P_);.

(4) This function cannot be used for the compensation amount of the tool compensation input.

(5) This function can be used when decimal point type I is valid, but cannot be used when decimal point type

II is valid.

(6) This function cannot be used for a tool shape setting command (in G10L100 format).

Program example (Machining program : programmed with 1=10m)

(CNC unit is 1=1m system)

«UNIT*10» parameter

10 1

X Y X Y

N1 G90 G00 X0 Y0; 0 0 0 0

N2 G91 X-10000 Y-15000; -100.000 -150.000 -10.000 -15.000

N3 G01 X-10000 Y-5000 F500; -200.000 -200.000 -20.000 -20.000

N4 G03 X-10000 Y-10000 J-10000; -300.000 -300.000 -30.000 -30.000

N5 X10000 Y-10000 R10000; -200.000 -400.000 -20.000 -40.000

N6 G01 X20.000 Y20.000 -180.000 -380.000 0.000 -20.000

UNIT*10 ON UNIT*10 OFF

N1

N2

N3

N4

N5

R

-400

-300

-200

-100

W

-100-200-300

N6

N1

N2

N3

N4

N5

R

-40

-30

-20

-10

W

-10-20-30

N6

2 Least Command Increments

MITSUBISHI CNC

8

2.3 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) which limits the command value is set, the rotary axis can only 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, the machine coordinate position at the end

point can only be commanded with the 2-degree increment.

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 parameter is used.

Precautions

(1) When the indexing increment is set, positioning will be conducted in degree unit.

(2) The indexing position is checked with the rotary axis, and is not checked with other axes.

(3) When the indexing increment is set to 2 degrees, the rotary axis is set to the B axis, and the B axis is

moved with JOG to the 1.234 position, an indexing error will occur if «G90B5.» or «G91B2.» is

commanded.

# Item Details Setting range (unit)

2106 Index unit Indexing increment

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

0 to 360()

3 Program Formats

MITSUBISHI CNC

10

3.1 Program Format

A collection of commands assigned to an NC to move a machine is called «program».

A program is a collection of units called «block» which specifies a sequence of machine tool operations.

Blocks are written in the order of the actual movement of a tool.

A block is a collection of units called «word» which constitutes a command to an operation.

A word is a collection of characters (alphabets, numerals, signs) arranged in a specific sequence.

% Block Block Block Block Block Block Block Block Block

%

M700V/M70V Series Programming Manual (M2/M0 Format)

3.1 Program Format

11

Detailed description

Program

A program format looks as follows.

(1) Program start

Input an End Of Record (EOR, %) at the head of a program.

It is automatically added when writing a program on an NC. When using an external device, do not forget

to input it at the head of a program. For details, refer to the description of the file format.

(2) Program No.

Program Nos. are used to classify programs by main program unit or subprogram unit. They are

designated by the address «L» followed by numbers of up to 8 digits. Program Nos. must be written at the

head of programs. A setting is available to prohibit L8000s and L9000s from editing (edit lock). Refer to

the instruction manual for the edit lock.

(Note) The addresses of the program No. and subprogram call No. differ according to the parameter.

The system must be formatted when this parameter is changed.

This manual describes on the assumption that the parameter is set to «0».

(3) Comment

Data between control out «(» and control in «)» is ignored.

Information including program names and comments can be written in.

(4) Program section

A program is a collection of several blocks.

(5) Program end

Input an end of record (EOR, %) at the end of a program.

It is automatically added when writing a program on an NC.

Setting of «#11009 M2 labelO» Address of the program No. Address to call the subprogram

0 L L

1 O A

% L (COMMENT) Block Block Block Block Block Block Block Block

%

(1)

(5)

(2)

(4)

(3)

3 Program Formats

MITSUBISHI CNC

12

Block and word

[Block]

A block is a least command increment, consisting of words.

It contains the information which is required for a tool machine to execute a specific operation. One block unit

constitutes a complete command.

The end of each block is marked with an End of Block (EOB, expressed as «;» for the sake of convenience).

[Word]

A word consists of a set of an alphabet, which is called an address, and numerals (numerical information).

Meanings of the numerical information and the number of significant digits of words differ according to an

address.

The major contents of a word are described below.

(1) Sequence No.

A «sequence No.» consists of the address «N» followed by numbers of up to 6 digits (Normally 3 or 4

digits). It is used as an index when searching a necessary block in a program (as branch destination and

etc.).

It does not affect the operation of a tool machine.

(2) Preparatory functions (G code, G function)

«Preparatory function (G code, G function)» consists of the address G followed by numbers of 2 or 3

digits (it may include 1 digit after the decimal point). G codes are mainly used to designate functions,

such as axis movements and setting of coordinate systems. For example, G00 executes a positioning

and G01 executes a linear interpolation.

(3) Coordinate words

«Coordinate words» specify the coordinate position and movement amounts of tool machine axes. They

consist of an address which indicates each axis of a tool machine followed by numerical information (+ or

— signs and numerals).

X, Y, Z, U, V, W, A, B and C are used as address. Coordinate positions and movement amounts are

specified by either «incremental value commands» or «absolute value commands».

(4) Feed Functions (F functions)

«Feed Functions (F functions)» designate the speed of a tool relative to a workpiece. They consist of the

address F followed by numbers.

(a) Alphabet (address) (n) Numerals

EOB

Word Word Word… ;Word

(a) (n)

N___ G__ X__ Z__ F__ ;

( 1) ( 2) ( 3) ( 4) EOB

M700V/M70V Series Programming Manual (M2/M0 Format)

3.1 Program Format

13

Main program and subprograms

Fixed sequences or repeatedly used parameters can be stored in the memory as subprograms which can

then be called from the main program when required.

If a command is issued to call a subprogram while a main program is being executed, the subprogram will be

executed. And when the subprogram is completed, the main program will be resumed.

Refer to the description of subprogram control for the details of the execution of subprograms.

(MP) Main program (S1) Subprogram 1 (S2) Subprogram 2

L0010;

G22L1000;

G22L2000;

M02;

L1000;

G23;

(MP) (S1)

L2000;

G23;

(S2)

3 Program Formats

MITSUBISHI CNC

14

3.2 File Format

Function and purpose

Program file can be created using NC edit screen and PC.

It can be input/output between NC memory and an external I/O device. Hard discs stored in NC unit are

regarded as an external I/O device. For the details of input/output method, refer to the instruction manual.

Program file format differs depending on the device which creates the program.

Detailed description

Devices available for input/output

Devices which can input/output program files are as follows.

Program file format

The file format for each external I/O device is as follows.

(1) NC memory (Creates program on NC)

External I/O device M700VW M700VS M70V

NC memory

HD (internal hard disc) — —

Serial

Memory card (front IC card)

DS (NC control unit side compact flash) — —

FD — —

USB memory — —

Ethernet

End of record (EOR, %) The end of record (EOR, %) is automatically added. It does not need to be input purposely.

Program No. (L No.) Not necessary.

File transfer

When multiple programs within the NC memory are transferred to an external device as serial, they will be integrated into one file in the external device. When a file containing multiple programs in an external device is transferred to NC memory as serial, it will be divided into one file per one program.

(COMMENT) ; G28XYZ ;

M02 ; %

M700V/M70V Series Programming Manual (M2/M0 Format)

3.2 File Format

15

(2) External device (except for serials, such as memory card, DS, FD, USB memory)

(3) External device (serial)

[Single program] [Multiple programs]

End of record (EOR, %)

The first line (from % to LF, or CR LF) will be skipped. Also, the content after the second % will not be transferred. «%» must be included in the first line because if not, the necessary information when transferring a file to an NC memory cannot be transferred.

Program No. (L No.) L No. before (COMMENT) will be ignored and the file name will be given the priority.

File transfer

Transfer and check of multiple programs between external devices, except for serial <_> serial, are not available. When a file containing multiple programs in an external device is transferred to NC memory as serial, it will be divided into one file per one program. When transferring divided programs one by one from an external device, which is not serial, (multiple programs) to an NC memory, the head program name can be omitted like «(COMMENT)» only when the transferring destination file name is designated to the file name field of device B.

Program name Program name should be designated with up to 32 alphanumeric characters (29 characters for a multi-part system program).

End of block (EOB, When the I/O parameter «CR output» is set to «1», EOB becomes CRLF.

End of record (EOR, %)

The first line (from % to LF, or CR LF) will be skipped. Also, the content after the second % will not be transferred. «%» must be included in the first line because if not, the necessary information when transferring a file to an NC memory cannot be transferred.

File transfer

Transfer and check of multiple programs between external devices, except for serial <_> serial, are not available. When transferring a file as serial, the head program name can be omitted like «(COMMENT)» only when the transferring destination file name is designated to the file name field of device B.

Program name Program name should be designated with up to 32 alphanumeric characters (29 characters for a multi-part system program).

End of block (EOB, When the I/O parameter «CR output» is set to «1», EOB becomes CRLF.

CRLF

(COMMENT) CRLF

G28 XYZ CRLF

: : M02 CRLF

% ^Z

CRLF

CRLF

G28 XYZ CRLF

: : M02 CRLF

L101(COMMENT1) CRLF

: M02 CRLF

% ^Z

L100(COMMENT)

LF

L100(COMMENT) LF

G28 XYZ LF

: : M02 LF

%

%

3 Program Formats

MITSUBISHI CNC

16

3.3 Optional Block Skip

3.3.1 Optional Block Skip; /

Function and purpose

This function selectively ignores a section of a machining program from a «/» (slash code) to the end of the

block.

Detailed description

Provided that the optional block skip switch is ON, a section of a machining program from a «/» to the end of

the block are ignored. They are executed if the switch is OFF.

Parity check is valid regardless of whether the optional block skip switch is ON or OFF.

When, for instance, all blocks are to be executed for one workpiece but specific blocks are not to be executed

for another workpiece, one machining program can be used to machine different parts by inserting the «/» into

those specific blocks.

Program example

(1) When the parameter «#1274 ext10/bit4» is set to «0» and the parameter «#1226 aux10/bit1» is set to «0»:

A «/» placed in the middle of a block is always interpreted as a division instruction regardless of the

optional block skip signal state being ON or OFF.

(2) When the parameter «#1274 ext10/bit4» is set to «0» and the parameter «#1226 aux10/bit1» is set to «1»:

A «/» placed in a bracketed («[ ]») expression is interpreted as a division instruction.

As for a «/» that appears in any other contexts, the section of the block following the «/» will be skipped if

the optional skip signal is ON, and the «/» itself will be ignored if the optional skip signal is OFF.

— Operation example of a case when optional block skip signal is ON:

— Operation example of a case when optional block skip signal is OFF:

G00 X0. Z0.;

#101 = [ 100. / 4 ] ; Sets «25.» to #101. (As the result of execution of a division instruction)

G00 Z[ 100. / 4 ] ; Moves Z axis to «25.». (As the result of execution of a division instruction)

#102 = 100. / #101 ; Sets «4.» to #102. (As the result of execution of a division instruction)

M30 ;

G00 X0. Z0.;

#101 = [ 100. / 4 ] ; Sets «25.» to #101. (As the result of execution of a division instruction)

G00 X100. / Z200. ; Moves X axis to «100. «. No Z axis movements made. (As the result of skipping the section of the block after «/»)

G00 Z[ 100. / 4 ] ; Moves Z axis to «25.». (As the result of execution of a division instruction)

#102 = 100. / #101 ; Sets «100.» to #102. (As the result of skipping the section of the block after «/»)

M30 ;

G00 X0. Z0.;

#101 = [ 100. / 4 ] ; Sets «25.» to #101. (As the result of execution of a division instruction)

G00 X100. / Z200. ; Moves X axis to «100.» and Z axis to «200.». (As the result of ignoring «/»)

G00 Z[ 100. / 4 ] ; Moves Z axis to «25.». (As the result of execution of a division instruction)

#102 = 100. / #101 ; Program error «P242 = not defined at vrble set» occurs. (As the result of ignoring «/»)

M30 ;

M700V/M70V Series Programming Manual (M2/M0 Format)

3.3 Optional Block Skip

17

(3) When the parameter «#1274 ext10/bit4» is set to «1»:

When a «/» is placed in a bracketed expression or when an expression that includes a «/» is on the right

side of an equation, the «/» is interpreted as a division instruction.

As for a «/» that appears in any other contexts, the section of the block following the «/» will be skipped if

the optional skip signal is ON, and the «/» itself will be ignored if the optional skip signal is OFF.

— Operation example of a case when optional block skip signal is ON:

— Operation example of a case when optional block skip signal is OFF:

Precautions

(1) When the parameter «#1274 ext10/bit4» is set to «0» and parameter «#1226 aux10/bit1» is set to «0»», put

the «/» code for optional block skip at the beginning of a block. If it is placed inside the block, it is

assumed as a user macro, a division instruction.

(Example)

N20 G1 X25. /Z25. ; ……….NG (User macro, a division instruction; a program error results.)

/N20 G1 X25. Z25. ; ……….OK

When parameter «#1274 ext10/bit4» = «0» and parameter «#1226 aux10/bit1» = «1», a «/» placed in the

middle of a block functions as a starting point of the optional skip. To use a «/» as a division instruction,

bracket (enclose in square brackets) the formula containing a slash code.

(2) A space immediately followed by a «/» at the very beginning of a block is always regarded as equal to a «/

» at the head of a block regardless of the value set in parameter «#1226 aux10/bit1».

(3) The optional block skip is processed immediately before the pre-read buffer.

Consequently, it is not possible to skip up to the block which has been read into the pre-read buffer.

(4) This function is valid even during a sequence 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.

G00 X0. Z0.;

#101 = [ 100. / 4 ] ; Sets «25.» to #101. (As the result of execution of a division instruction)

G00 X100. / Z200. ; Moves X axis to «100.». No Z axis movements made. (As the result of skipping the section of the block after «/»)

G00 Z[ 100. / 4 ] ; Moves Z axis to «25.». (As the result of execution of a division instruction)

#102 = 100. / #101 ; Sets «4.» to #102. (As the result of execution of a division instruction)

M30 ;

G00 X0. Z0.;

#101 = [ 100. / 4 ] ; Sets «25.» to #101. (As the result of execution of a division instruction)

G00 X100. / Z200. ; Moves X axis to «100.» and Z axis to «200.». (As the result of ignoring «/»)

G00 Z[ 100. / 4 ] ; Moves Z axis to «25.». (As the result of execution of a division instruction)

#102 = 100. / #101 ; Sets «4.» to #102. (As the result of execution of a division instruction)

M30 ;

3 Program Formats

MITSUBISHI CNC

18

3.3.2 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 n signal is turned ON. For a block with the «/n» code inside the block (not at the head of the

block), the program is operated according to the value of the parameter «#1226 aux10/bit1» setting.

When the optional block skip n signal is OFF, the block with «/n» is executed.

Program example

(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 G90 G81 X50. Z-20. R3. F100 ;

/5 N3 X30. ;

N4 X10. ;

N5 G80 ;

M02 ;

Part 1 Optional block skip 5 signal ON

Part 2 Optional block skip 5 signal OFF

N4 N2 N2N3N4

M700V/M70V Series Programming Manual (M2/M0 Format)

3.3 Optional Block Skip

19

(2) When two or more «/n» codes are commanded at the head of the same block, the block will be ignored if

either of the optional block skip n signals corresponding to the command is ON.

(3) When the parameter «#1226 aux10/bit1» is «1»and two or more «/n» are commanded inside the same

block, the commands following «/n» in the block are ignored if either of the optional block skip n signals

corresponding to the command is ON.

N01 G90 Z3. M03 S1000 ; (a) Optional block skip 1 signal ON (Optional block skip 2.3 signal OFF) N01 -> N08 -> N09 -> N10 -> N11 -> N12

/1/2 N02 G00 X50. ;

/1/2 N03 G01 Z-20. F100 ;

/1/2 N04 G00 Z3. ;

/1 /3 N05 G00 X30. ; (b) Optional block skip 2 signal ON (Optional block skip 1.3 signal OFF) N01 -> N05 -> N06 -> N07 -> N11 -> N12

/1 /3 N06 G01 Z-20. F100 ;

/1 /3 N07 G00 Z3. ;

/2/3 N08 G00 X10. ; (c) Optional block skip 3 signal ON (Optional block skip 1.2 signal OFF) N01 -> N02 -> N03 -> N04 -> N11 -> N12

/2/3 N09 G01 Z-20. F100 ;

/2/3 N10 G00 Z3. ;

N11 G28 X0 M05 ;

N12 M02 ;

N01 G91 G28 X0.Y0.Z0.; N03 block will operate as follows. (a) Optional block skip 1 signal ON Optional block skip 2 signal OFF «Y1. Z1.» is ignored. (b) Optional block skip 1 signal OFF Optional block skip 2 signal ON «Z1.» is ignored.

N02 G01 F1000;

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

N04 M30;

3 Program Formats

MITSUBISHI CNC

20

3.4 G code 3.4.1 Modal, unmodal

G codes define the operation modes of each block in programs.

G codes can be modal or unmodal command.

Modal commands always designate one of the G codes in the group as the NC operation mode. The

operation mode is maintained until a cancel command is issued or other G code among the same group is

commanded.

An unmodal command designates the NC operation mode only when it is issued. It is invalid for the next

block.

3.4.2 G Code Lists

G code Group Function Section

00 01 Positioning 6.1

01 01 Linear interpolation 6.2

02 01

Circular interpolation CW (clockwise) R-specified circular interpolation CW Helical interpolation CW Spiral/Conical interpolation CW (type 2)

6.3 6.4 6.7 6.13

03 01

Circular interpolation CCW (counterclockwise) R-specified circular interpolation CCW Helical interpolation CCW Spiral/Conical interpolation CCW (type 2)

6.3 6.4 6.7 6.13

02.1 01 Spiral/Conical interpolation CW (type1) 6.13

03.1 01 Spiral/Conical interpolation CCW (type1) 6.13

02.3 01 Exponential function interpolation positive rotation 6.11

03.3 01 Exponential function interpolation negative rotation 6.11

02.4 01 3-dimensional circular interpolation 6.14

03.4 01 3-dimensional circular interpolation 6.14

04 00 Dwell 8.1

05 00 High-speed machining mode High-speed high-accuracy control II

13.17 13.18

05.1 00 High-speed high-accuracy control I Spline

13.18 13.19

06.2 01 NURBS interpolation 6.15

07 00 Hypothetical axis interpolation 6.16

07.1 107

21 Cylindrical interpolation 6.9

08 00 High-accuracy control 13.16

09 00 Exact stop check 7.10

10 00 Compensation data input by program Parameter input by program Parameter coordinate rotation input

12.8 13.12 13.23

11.1 00 Cancel (Compensation data input by program, Parameter input by program)

13.12

11.1 00 Program compensation data input to variable 12.9

12 00 Circular cut CW (clockwise) 13.11

13 00 Circular cut CCW (counterclockwise) 13.11

12.1 112

21 Polar coordinate interpolation ON 6.10

* 13.1 113

21 Polar coordinate interpolation cancel 6.10

14 00 Coordinate data read 13.30

* 15 18 Polar coordinate command OFF 6.12

16 18 Polar coordinate command ON 6.12

17 02 Plane selection X-Y 6.5

18 02 Plane selection Z-X 6.5

M700V/M70V Series Programming Manual (M2/M0 Format)

3.4 G code

21

19 02 Plane selection Y-Z 6.5

20 06 Inch command 5.2

21 06 Metric command 5.2

22 00 Subprogram call / figure rotation ON 13.3

23 00 Subprogram return / figure rotation cancel 13.3

22.1 04 Stroke check before travel ON 15.1

23.1 04 Stroke check before travel cancel 15.1

24

25

26

27 00 Reference position check 14.9

28 00 Reference position return 14.7

29 00 Start position return 14.7

30 00 2nd to 4th reference position return 14.8

30.1 00 Tool change position return 1 13.14

30.2 00 Tool change position return 2 13.14

30.3 00 Tool change position return 3 13.14

30.4 00 Tool change position return 4 13.14

30.5 00 Tool change position return 5 13.14

30.6 00 Tool change position return 6 13.14

31 00 Skip Multi-step skip function 2

16.2 16.4

31.1 00 Multi-step skip function 1-1 16.3

31.2 00 Multi-step skip function 1-2 16.3

31.3 00 Multi-step skip function 1-3 16.3

32

33 01 Thread cutting 6.6

34 00 Special fixed cycle (bolt hole circle) 13.2

35 00 Special fixed cycle (line at angle) 13.2

36 00 Special fixed cycle (arc) 13.2

37 00 Special fixed cycle (grid) 13.2

37.1 00 Automatic tool length measurement 16.1

38 00 Tool radius compensation vector designation 12.4

39 00 Tool radius compensation corner arc 12.4

* 40 07 Tool radius compensation cancel 3-dimentional tool radius compensation cancel Tool radius compensation for 5-axis machining cancel

12.4 12.5 12.6

41 07 Tool radius compensation left 3-dimentional tool radius compensation left

12.4 12.5

42 07 Tool radius compensation right 3-dimentional tool radius compensation right

12.4 12.5

* 40.1 150

15 Normal line control cancel 13.15

41.1 151

15 Normal line control left ON 13.15

42.1 152

15 Normal line control right ON 13.15

41.2 07 Tool radius compensation for 5-axis machining (left) 12.6

42.2 07 Tool radius compensation for 5-axis machining (right) 12.6

43 08 Tool length compensation 12.2

*44 08 Tool length compensation cancel Tool length compensation in the tool axis direction Tool center point control cancel

12.2 12.3 13.25

43.1 08 Tool length compensation along the tool axis ON 12.3

43.4 08 Tool center point control type 1 13.25

43.5 08 Tool center point control type 2 13.25

G code Group Function Section

3 Program Formats

MITSUBISHI CNC

22

45 00 Tool position offset (extension) 12.7

46 00 Tool position offset (reduction) 12.7

47 00 Tool position offset (double elongation) 12.7

48 00 Tool position offset (double contraction) 12.7

* 50 11 Scaling cancel 13.21

51 11 Scaling ON 13.21

* 50.1 19 G command mirror image cancel 13.6

51.1 19 G command mirror image ON 13.6

52 00 Local coordinate system setting 14.11

53 00 Basic machine coordinate system selection 14.5

53.1 00 Tool axis direction control (type 1) 13.27

53.6 00 Tool axis direction control (type 2) 13.27

* 54 12 Workpiece coordinate system 1 selection 14.10

55 12 Workpiece coordinate system 2 selection 14.10

56 12 Workpiece coordinate system 3 selection 14.10

57 12 Workpiece coordinate system 4 selection 14.10

58 12 Workpiece coordinate system 5 selection 14.10

59 12 Workpiece coordinate system 6 selection 14.10

54.1 12 Workpiece coordinate system selection 48 / 96 sets extended 14.10

54.4 27 Workpiece installation error compensation 14.14

60 00 Unidirectional positioning 6.8

61 13 Exact stop check mode 7.11

61.1 13 High-accuracy control 1 ON 13.16

61.2 13 High-accuracy spline interpolation 13.20

62 19 G command mirror image 13.6

63 13 Tapping mode 7.14

* 64 13 Cutting mode 7.15

65 00 User macro call 13.5.1

66 14 User macro modal call A 13.5.1

66.1 14 User macro modal call B 13.5.1

* 67 14 User macro modal call cancel 13.5.1

68 00 Subprogram return 13.5.1

69 00 End point error check cancellation 13.29

68.1 16 Coordinate rotation by program ON / 3-dimensional coordinate conversion mode ON

13.22 13.24

68.2 16 Inclined surface machining command 13.27

68.3 16 Inclined surface machining command (Define using tool axis direction)

13.27

* 69.1 16 Coordinate rotation by program cancel / 3-dimensional coordinate conversion mode OFF / Inclined surface machining command cancel

13.22 13.24 13.27

70 09 User fixed cycle

71 09 User fixed cycle

72 09 User fixed cycle

73 09 Fixed cycle (step) 13.1.10

74 09 Fixed cycle (reverse tap) 13.1.11

75 09 Fixed cycle (circle cutting cycle) 13.1.12

76 09 Fixed cycle (fine boring) 13.1.13

77 09 User fixed cycle

78 09 User fixed cycle

79 09 User fixed cycle

* 80 09 Fixed cycle cancel 13.1

81 09 Fixed cycle (drill/spot drill) 13.1.1

82 09 Fixed cycle (drill/counter boring) 13.1.2

83 09 Fixed cycle (deep drilling/small-diameter deep-hole drilling) 13.1.3

G code Group Function Section

M700V/M70V Series Programming Manual (M2/M0 Format)

3.4 G code

23

Precautions

(1) Codes marked with * are codes that must be or are selected in the initial state.

The codes marked with are codes that should be or are selected in the initial state by the

parameters.

(2) If two or more G codes from the same code are commanded, the latter G code will be valid.

(3) This G code list is a list of conventional G codes. Depending on the machine, movements that differ

from the conventional G commands may be included when called by the G code macro. Refer to

the Instruction Manual issued by the tool builder.

(4) Whether the modal is initialized or not depends on each reset input.

(a) «Reset 1»

The modal is initialized when the reset initial parameter «#1151 rstinit» turns ON.

(b) «Reset 2» and «Reset & rewind»

The modal is initialized when the signal is input.

(c) Resetting when emergency stop is canceled

Follows «Reset 1».

(d) When modal is automatically reset at the start of individual functions such as reference position

return.

Follows «Reset & rewind».

84 09 Fixed cycle (tapping) 13.1.4

85 09 Fixed cycle (boring) 13.1.5

86 09 Fixed cycle (boring) 13.1.6

87 09 Fixed cycle (back boring) 13.1.7

88 09 Fixed cycle (boring) 13.1.8

89 09 Fixed cycle (boring) 13.1.9

90 03 Absolute value command 5.1

91 03 Incremental command value 5.1

92 00 Coordinate system setting / Spindle clamp speed setting 14.6

92.1 00 Workpiece coordinate system pre-setting 14.12

93 05 Inverse time feed 7.5

94 05 Feed per minute (Asynchronous feed) 7.4

95 05 Feed per revolution (Synchronous feed) 7.4

96 17 Constant surface speed control ON 10.2

97 17 Constant surface speed control OFF 10.2

* 98 10 Fixed cycle Initial level return 13.1.15

99 10 Fixed cycle R point level return 13.1.15

100 — 225 00 User macro (G code call) Max. 10 13.5.2

120.1 00 Machining condition selection I 13.28

121 00 Machining condition selection I cancel 13.28

CAUTION

1. The commands with «no value after G» will be handled as «G00».

G code Group Function Section

3 Program Formats

MITSUBISHI CNC

24

3.5 Precautions Before Starting Machining

CAUTION

1. 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.

2. Before starting actual machining, always carry out graphic check, dry run operation and single block operation

to check the machining program, tool compensation amount, workpiece offset amount and etc.

4 Pre-read Buffers

MITSUBISHI CNC

26

4.1 Pre-read Buffers

Function and purpose

During automatic processing, the contents of one block ahead are normally pre-read so that program analysis

processing is conducted smoothly. However, during tool radius compensation, a maximum of 5 blocks are

pre-read for the intersection point calculation including interference check.

Detailed description

The specifications of pre-read buffers in 1 block are as follows:

(1) The data of 1 block is stored in this buffer.

(2) When comments and the optional block skip function is ON, the data extending from the «/» (slash) code

up to the EOB code are not read into the pre-read buffer.

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

(4) When the single block function is ON during continuous operation, the pre-read buffer stores the next

block’s data and then stops operation.

(5) The way to prohibit the M command which operates the external controls from pre-reading, and to make

it to recalculate, is as follows:

Identify the M command which operates the external controls by a PLC, and turn on the «recalculation

request» on PLC output signal. (When the «recalculation request» is turned ON, the program that has

been pre-read is recalculated.)

Precautions

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

validation/invalidation of the external control signals including optional block skip, 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 for the program pre-read with the buffer register.

5 Position Commands

MITSUBISHI CNC

28

5.1 Position Command Methods ; G90,G91

Function and purpose

By using the G90 and G91 commands, it is possible to execute the next coordinate commands using absolute

values or incremental values.

The R-designated circle radius and the center of the circle determined by I, J, K are always incremental value

commands.

Command format

G90/G91 X__ Y__ Z__ __ ;

G90 Absolute command

G91 Incremental command

X,Y,Z, Coordinate values ( is the additional axis.)

M700V/M70V Series Programming Manual (M2/M0 Format)

5.1 Position Command Methods ; G90,G91

29

Detailed description

(1) Regardless of the current position, in the absolute value mode, it is possible to move to the position of

the workpiece coordinate system that was designated in the program.

(2) For the next block, the last G90/G91 command that was given becomes the modal.

(3) Since multiple commands can be issued in the same block, it is possible to command specific addresses

as either absolute values or incremental values.

(4) When the power is turned ON, it is possible to select whether you want absolute value commands or

incremental value commands with the #1073 I_Absm parameter.

(5) Even when commanding with the manual data input (MDI), it will be treated as a modal from that block.

N1 G90 G00 X0 Y0 ; In the incremental value mode, the current position is the start point (0), and the movement is made only the value determined by the program, and is expressed as an incremental value. N2 G90 G01 X200. Y50. F100 ; N2 G91 G01 X200. Y50. F100 ; Using the command from the 0 point in the workpiece coordinate system, it becomes the same coordinate command value in either the absolute value mode or the incremental value mode.

Tool

(G90) N3 X100. Y100. ;

The axis moves to the workpiece coordinate system X = 100.mm and Y = 100.mm position.

(G91) N3 X-100. Y50. ;

The X axis moves to -100.mm and the Y axis to +50.0mm as an incremental value, and as a result X moves to 100.mm and Y to 100.mm.

N4 G90 X300. G91 Y100. ; The X axis is treated in the absolute value mode, and with G90 is moved to the workpiece coordinate system 300.mm position. The Y axis is moved +100.mm with G91. As a result, Y moves to the 200.mm position. In terms of the next block, G91 remains as the modal and becomes the incremental value mode.

300.200.

200.

100 N1

100. N2

W X

Y

300.200.

200.

100.

N3

W X

Y

100.

300.200.100.

N4

W X

Y

100.

200.

5 Position Commands

MITSUBISHI CNC

30

5.2 Inch/Metric Conversion ; G20,G21

Function and purpose

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

Command format

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. It is invalid for rotation axes.

Output unit, command unit and setting unit

The counter, parameter setting and display unit are determined by parameter «#1041 I_inch». The movement/

speed command will be displayed as metric units when «#1041 I_inch» is ON during the G21 command mode.

The internal unit metric data of the movement/speed command will be converted into an inch unit and

displayed when «#1041 I_inch» is OFF during the G20 command mode. The command unit for when the

power is turned ON and reset is decided by combining the parameters «#1041 I_inch», «#1151 rstint» and

«#1210 RstGmd/bit5».

NC axis

PLC axis

G20; … Inch command

G21; … Metric command

Item

Initial inch OFF (metric internal unit)

#1041 I_inch=0

Initial inch ON (inch internal unit)

#1041 I_inch=1

G21 G20 G21 G20

Movement/speed command Metric Inch Metric Inch

Counter display Metric Metric Inch Inch

Speed display Metric Metric Inch Inch

User parameter setting/display Metric Metric Inch Inch

Workpiece/tool offset setting/display Metric Metric Inch Inch

Handle feed command Metric Metric Inch Inch

Item #1042 pcinch=0 (metric) #1042 pcinch=1 (inch)

Movement/speed command Metric Inch

Counter display Metric Inch

User parameter setting/display Metric Inch

M700V/M70V Series Programming Manual (M2/M0 Format)

5.2 Inch/Metric Conversion ; G20,G21

31

Precautions

(1) The parameter and tool data will be input/output with the unit set by «#1041 I_inch».

If «#1041 I_inch» is not found in the parameter input data, the unit will follow the unit currently set to NC.

(2) The unit of read/write used in PLC window is fixed to metric unit regardless of a parameter and G20/G21

command modal.

(3) A program error (P33) will occur if G20/G21 command is issued in the same block as following G codes.

Command in a separate block.

— G05 (High-speed machining mode)

— G7.1 (Cylindrical Interpolation)

— G12.1 (Polar coordinate interpolation)

5 Position Commands

MITSUBISHI CNC

32

5.3 Decimal Point Input

Function and purpose

This function enables to input decimal points. It assigns the decimal point in millimeter or inch units for the

machining program input information that defines the tool paths, distances and speeds.

Use the parameter «#1078 Decpt2» to select whether minimum input command increment (type I) or zero point

(type II) to apply to the least significant digit of data without a decimal point.

Detailed description

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

machining programs. (Note, only after G51)

(2) In decimal point input type I and type II, the values of the data commands without the decimal points are

shown in the table below.

(3) The valid addresses for the decimal points are X, Y, Z, U, V, W, A, B, C, I, J, K, E, F, P, Q, and R.

However, P is valid only during scaling. For details, refer to the list.

(4) In decimal point command, the valid range of command value is as shown below. (Input command unit

cunit = 10)

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

(6) While the smallest decimal point command is validated, the smallest unit for a command without a

decimal point designation is the smallest command input unit set in the specifications (1m, 10m,

etc.) or mm can be selected. This selection can be made with parameter «#1078 Decpt2».

(7) Decimal point commands for decimal point invalid addresses are processed as integer data only and

everything below the decimal point is ignored. Addresses which are invalid for the decimal point are D, H,

L, M, N, O, S and T. All variable commands, however, are treated as data with decimal points.

(8) «Input command increment tenfold» is applied in the decimal point type I mode, but not in the decimal

point type II mode.

Command Command unit Type I Type II

X1;

cunit=10000 1000

(m, 10-4inch,10-3)

1 (mm, inch, )

cunit= 1000 100 1

cunit= 100 10 1

cunit= 10 1 1

Movement command (linear)

Movement command (rotary)

Feedrate Dwell

Input unit [mm]

-99999.999 to 99999.999 -99999.999 to

99999.999

0.001 to 10000000.000

0 to 99999.999 Input unit

[inch] -9999.9999 to 9999.9999

0.0001 to 1000000.0000

M700V/M70V Series Programming Manual (M2/M0 Format)

5.3 Decimal Point Input

33

Decimal point input I, II and decimal point command validity

Decimal point input I and II will result as follows when decimal points are not used in an address which a

decimal point command is valid. Whether an address is valid or invalid for the decimal point command is

shown in the table below.

Both decimal point input I and II will produce the same result when a command uses a decimal point.

(1) Decimal point input I

The least significant digit of command data matches the command unit.

(Example) When «X1» is commanded in 1m system, the same result occurs as for an «X0.001»

command.

(2) Decimal point input II

The least significant digit of command data matches the command unit.

(Example) When «X1» is commanded in 1m system, the same result occurs as for an «X1.» command.

-Addresses used, validity of decimal point commands-

Address Decimal Point

Command Application Remarks

A

Valid Coordinate position data

Invalid Revolving table

Invalid Miscellaneous function code

Valid Angle data

Invalid Data settings, axis numbers (G10)

Invalid Subprogram call : program No. (label O)

B

Valid Coordinate position data

Invalid Revolving table

Invalid Miscellaneous function code

C

Valid Coordinate position data

Invalid Revolving table

Invalid Miscellaneous function code

Valid Corner chamfering amount ,C

D

Invalid Compensation numbers (tool position, tool radius)

Valid Automatic tool length measurement: deceleration distance d

Invalid Data setting: byte type data

Invalid Subprogram storing device number ,D

E Valid

Inch thread: number of ridges, precision thread: lead

Valid Dwell time at hole bottom of fixed cycle (label L, O)

F

Valid Feedrate, automatic tool length measurement speed

Valid Thread lead

Valid Number of Z axis pitch in synchronous tap

G Valid Preparatory function code

H

Invalid Tool length compensation number

Invalid Sequence numbers in subprograms (label L, O)

Invalid Subprogram return destination sequence No. (label L, O)

Invalid Parameter input by program: bit type data

Invalid Basic spindle selection

I

Valid Arc center coordinates, center of figure rotation (incremental)

Valid Tool radius compensation vector components

Valid Hole pitch in the special fixed cycle

Valid Circle radius of cut circle (increase amount)

Valid G0/G1 imposition width, drilling cycle G0 imposition width ,I

Valid Stroke check before travel: lower limit coordinates

5 Position Commands

MITSUBISHI CNC

34

J

Valid Coordinates for arc center and center of figure rotation (incremental)

Valid Tool radius compensation vector components

Valid Special fixed cycle’s hole pitch or angle

Valid G0/G1 imposition width, drilling cycle G1 imposition width

Valid Stroke check before travel: lower limit coordinates

K

Valid Coordinates for arc center and center of figure rotation (incremental)

Valid Tool radius compensation vector components

Invalid Number of holes of the special fixed cycle

Invalid Number of drilling cycle repetitions

Valid Stroke check before travel: lower limit coordinates

L

Invalid Subprogram call program No. (label L)

Invalid Tool compensation data input by program/workpiece offset input: type selection

L2, L20, L10, L11 L12, L13,

Invalid Parameter input by program: data setting selection L70

Invalid Parameter input by program: 2-word type data 4 bytes

Invalid Program No. (label L)

Invalid Tool life data

M Invalid Miscellaneous function codes

N Invalid Sequence numbers

Invalid Parameter input by program: data numbers

O Invalid Program numbers

P

Invalid/Valid Dwell time Parameter

Invalid Subprogram program call: program No.

Invalid/Valid Dwell at tap cycle hole base Parameter

Invalid Number of holes of the special fixed cycle

Invalid Amount of helical pitch

Invalid Offset number (G10)

Invalid Constant surface speed control axis number

Invalid Parameter input by program: broad classification number

Invalid Multi-step skip function 2 signal command

Invalid Subprogram return destination sequence No.

Invalid 2nd, 3rd, 4th reference position return number

Valid Scaling magnification

Invalid High-speed mode type

Invalid Type of the coordinate to be read

Invalid Transmission source compensation No. of program compensation data input to variable

Invalid Extended workpiece coordinate system No.

Invalid Tool life data group No.

Invalid Machining purpose

Q

Valid Cut amount of deep hole drill cycle

Valid Shift amount of back boring

Valid Shift amount of fine boring

Invalid Minimum spindle clamp speed

Valid Starting shift angle for screw cutting

Invalid Tool life data management method

Invalid Machining condition

Address Decimal Point

Command Application Remarks

M700V/M70V Series Programming Manual (M2/M0 Format)

5.3 Decimal Point Input

35

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

Program example

(1) Program example of decimal point valid address

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 123mm command. It will not be 123m.

R

Valid R-point in the fixed cycle

Valid R-specified arc radius

Valid Corner R arc radius ,R

Valid Offset amount (G10)

Invalid Synchronous tap/asynchronous tap changeover

Valid Automatic tool length measurement: deceleration distance r

Valid Rotation angle

Invalid Skip acceleration/deceleration time constant

S

Invalid Spindle function codes

Invalid Maximum spindle clamp speed

Invalid Constant surface speed control: surface speed

Invalid Parameter input by program: word type data 2 bytes

T Invalid Tool function codes

U Valid Coordinate position data

V Valid Coordinate position data

W Valid Coordinate position data

X Valid Coordinate position data

Valid Dwell time

Y Valid Coordinate position data

Z Valid Coordinate position data

Program example Decimal point command 1 Decimal point

command 2 When 1 = 1mm When 1 = 1m When 1 = 10m

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

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

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

X123.450 mm X12345.000 mm

#111=123 #112=5.55 X#111 Y#112

X123.000 mm Y5.550 mm

X123.000 mm Y5.550 mm

X123.000 mm Y5.550 mm

#113=#111+#112 (addition)

#113=128.550 #113=128.550 #113=128.550

#114=#111-#112 (subtraction)

#114=117.450 #114=117.450 #114=117.450

#115=#111*#112 (multiplication)

#115=682.650 #115=682.650 #115=682.650

#116=#111/#112 #117=#112/#111 (division)

#116=22.162 #117=0.045

#116=22.162 #117=0.045

#116=22.162 #117=0.045

Address Decimal Point

Command Application Remarks

5 Position Commands

MITSUBISHI CNC

36

37

6

Interpolation Functions

6 Interpolation Functions

MITSUBISHI CNC

38

6.1 Positioning (Rapid Traverse) ; G00

Function and purpose

This command is accompanied by coordinate words and performs high-speed positioning of a tool, from the

present point (start point) to the end point specified by the coordinate words.

Command format

The command addresses are valid for all additional axes.

Detailed description

(1) Positioning will be performed at the rapid traverse rate set in the parameter «#2001 rapid».

(2) G00 command belongs to the 01 group and is modal. When G00 command is successively issued, the

following blocks can be specified only by the coordinate words.

(3) In the G00 mode, acceleration and deceleration are always carried out at the start point and end point of

the block. Before advancing to the next block, a commanded deceleration or an in-position check is

conducted at the end point to confirm that the movement is completed for all the moving axes in each

part system.

(4) G functions (G72 to G89) in the 09 group are cancelled (G80) by the G00 command.

G00 X__ Y__ Z____,I__ ; … Positioning (Rapid Traverse)

X, Y, Z, Coordinate values ( is the additional axis.) An absolute position or incremental position is indicated based on the state of G90/G91 at that time.

,I In-position width. 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

CAUTION

1. The commands with «no value after G» will be handled as «G00».

M700V/M70V Series Programming Manual (M2/M0 Format)

6.1 Positioning (Rapid Traverse) ; G00

39

Tool path

Whether the tool moves along a linear or non-linear path can be selected by the parameter «#1086 G0Intp».

The positioning time does not change according to the path.

(1) Linear path: When the parameter «#1086 G0Intp» is set to «0»

In positioning, a tool follows the shortest path which connects the start point and the end point. The

positioning speed is automatically calculated so that the shortest distribution time is obtained in order

that the commanded speeds for each axis do not exceed the rapid traverse rate.

When, for instance, the X-axis and Y-axis rapid traverse rates are both 9600mm/min;

G91 G00 X-300000 Y200000 ; (With an input setting unit of 0.001mm)

The tool will follow the path shown in the figure below.

(2) Non-linear path: When the parameter «#1086 G0Intp» is set to «1»

In positioning, the tool will move along the path from the start point to the end point at the rapid traverse

rate of each axis.

When, for instance, the X-axis and Y-axis rapid traverse rates are both 9600mm/min;

G91 G00 X-300000 Y200000 ; (With an input setting unit of 0.001mm)

The tool will follow the path shown in the figure below.

(S) Start point (E) End point (fx) Actual X axis rate (fy) Actual Y axis rate

(S) Start point (E) End point (fx) Actual X axis rate (fy) Actual Y axis rate

300

(mm)

(E)

(S)

fy=6400mm/min

Y

X 20

0

fx=9600mm/min

300

(mm)

(E)

(S)

fy=9600mm/min

Y

X

20 0

fx=9600mm/min

6 Interpolation Functions

MITSUBISHI CNC

40

Program example

Precautions for deceleration check

There are two methods for the deceleration check; commanded deceleration method and in-position check

method. Select a method with the parameter «#1193 inpos».

A block with an in-position width command performs an in-position check with a temporarily changed in-

position width. (Programmable in-position width command)

The deceleration check method set in basic specification parameter «#1193 inpos» is used for blocks that do

not have the in-position width command.

During cutting feed and when the error detection is ON, the in-position check is forcibly carried out.

* Following descriptions are for the case of rapid traverse. For G01, interpret the parameters into suitable

ones.

(S) Start point (E) End point

G91 G00 X-270. Y300. Z150. ;

Rapid traverse (G00)

#1193 inpos

0 1

,I command No

Commanded deceleration method (Commanded deceleration check which varies according to the type of acceleration/deceleration, set in «#2003 smgst» bit3-0)

In-position check method (In-position check by «#2077 G0inps», «#2224 SV024»)

Yes In-position check method (In-position check by «,I», «#2077 G0inps», «#2224 SV024»)

Cutting feedrate (G01)

#1193 inpos

0 1

,I command No

Commanded deceleration method (Commanded deceleration check which varies according to the type of acceleration/deceleration, set in «#2003 smgst» bit7-4)

In-position check method (In-position check by «#2078 G1inps», «#2224 SV024»)

Yes In-position check method (In-position check by «,I», «#2078 G1inps», «#2224 SV024»)

mm

( — 120,+200,+300)

(+150, — 100,+150)

X

Z

Y

+300

+150

+200+150

-100 — 120

(S)

(E)

M700V/M70V Series Programming Manual (M2/M0 Format)

6.1 Positioning (Rapid Traverse) ; G00

41

Commanded deceleration method 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 set in the

parameter «#2003 smgst».

(1) Linear acceleration/linear deceleration

(2) Exponential acceleration/linear deceleration

(3) Exponential acceleration/exponential deceleration (Primary delay)

The time required for the deceleration check is the longest among the deceleration check times of each axis

determined by the acceleration/deceleration mode and time constants of the axes commanded

simultaneously.

(Ts) Acceleration/deceleration time constant

(Td) Deceleration check time: Td = Ts + (0 to 7ms)

(Ts) Acceleration/deceleration time constant

(Td) Deceleration check time: Td = 2 Ts + (0 to 7ms)

(Ts) Acceleration/deceleration time constant

(Td) Deceleration check time: Td = 2 Ts + (0 to 7ms)

Ts

Td

G00 Xx1; G00 Xx2;

Td Ts

G00 Xx1; G00 Xx2;

2Ts

Ts

Td

G00 Xx1; G00 Xx2;

6 Interpolation Functions

MITSUBISHI CNC

42

In-position check method 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.

The confirmation of the remaining distance should be done with the imposition width.

The bigger one of the servo parameter «#2224 SV024» or G0 in-position width «#2077 G0inps» (For G01, in-

position width «#2078 G1inps»), will be adapted as the in-position width.

G0 deceleration pattern

The in-position width LR indicates the remaining distance from the previous block at the start of the next block

(shaded area of the figure above).

(TR) Rapid traverse acceleration and deceleration time constant

(LR) In-position width

G00 Xx1 ; G00 Xx2 ;

LR

2TR

TR

M700V/M70V Series Programming Manual (M2/M0 Format)

6.1 Positioning (Rapid Traverse) ; G00

43

The purpose of the rapid traverse deceleration check is to minimize the positioning time. The bigger the

setting value for the in-position width, the shorter the time is, but the remaining distance of the previous block

at the start of the next block also becomes larger, and this could become an obstacle in the actual processing

work.

The check for the remaining distance is done at set intervals. Accordingly, it may not be possible to get the

effect of time reduction for positioning as in-position width setting value.

(1) In-position check by the G0inps: When SV024 < G0inps (Stop is judged at A in the figure)

(2) In-position check using SV024: When G0inps < SV024 (Stop is judged at A in the figure)

(a) Command to motor (b) Outline of motor movement

(a) Command to motor (b) Outline of motor movement

SV024

(a)

(b)

G0inps

A

G0inps

(a)

(b)

SV024

A

6 Interpolation Functions

MITSUBISHI CNC

44

Programmable in-position width command

This command commands the in-position width for the positioning command from the machining program.

Execution of the next block starts after confirming that the position error amount of the positioning (rapid

traverse: G00) command block is less than the in-position width issued in this command.

The bigger one of in-position width (SV024, G0inps (For G01, G1inps)) with parameter or in-position width

specified by program will be adapted as the in-position width.

When there are several movement axes, the system confirms that the position error amount of each

movement axis in each part system is less than the in-position width issued in this command before executing

the next block.

The differences of In-position check

The differences between the in-position check with parameter and with programmable command are as

follows:

(1) In-position check with parameter

After completing deceleration of the command system (A), the servo system’s position error amount and

the parameter setting value (in-position width) are compared.

(2) In-position check with programmable command («,I» address command)

After starting deceleration of the command system (A), the position error amount and commanded in-

position width are compared.

G00 X_ Y_ Z_ ,I_ ;

X,Y,Z Positioning coordinate value of each axis

,I In-position width

(a) Servo machine position (b) Command (c) In-position width (Servo system position error amount) (Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = Ts + (0 to 7ms)

(a) Servo machine position (b) Command (c) In-position width (Error amount between command end point and machine position) (Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = Ts + (0 to 7ms)

Ts

Td

(a) (b)

(c)

A

G00 Xx1;

Ts

Td

(a) (b)

(c)

A

G00 Xx1;

M700V/M70V Series Programming Manual (M2/M0 Format)

6.2 Linear Interpolation ; G01

45

6.2 Linear Interpolation ; G01

Function and purpose

This command is accompanied by coordinate words and a feedrate command. It makes the tool move

(interpolate) linearly from its current position to the end point specified by the coordinate words at the speed

specified by address F. In this case, the feedrate specified by address F always acts as a linear speed in the

tool nose center advance direction.

Command format

Detailed description

(1) G01 command is a modal command in the 01 group. When G01 command is issued in succession, it can

only be issued with coordinate words in subsequent blocks.

(2) The feedrate for a rotary axis is commanded by /min (decimal point position unit). (F300=300/min)

(3) The G functions (G72 to G89) in the 09 group are cancelled (G80) by the G01 command.

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.

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

G01 X__ Y__ Z__ __ F__ ,I__ ; … Linear interpolation

X,Y,Z, Coordinate values ( is the additional axis.) An absolute position or incremental position is indicated based on the state of G90/G91 at that time.

F Feedrate (mm/min or /min)

,I In-position width. 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

G01 X_ Y_ Z_ F_ ,I_ ;

X,Y,Z Linear interpolation coordinate value of each axis

F Feedrate

,I In-position width

6 Interpolation Functions

MITSUBISHI CNC

46

Program example

(Example) Cutting in the sequence of P1 -> P2 -> P3 -> P4 -> P1 at 300mm/min feedrate.

However, P0 -> P1 is for tool positioning.

G91 G00 X20. Y20. ; P0 -> P1

G01 X20. Y30. F300 ; P1 -> P2

X30. ; P2 -> P3

X-20. Y-30. ; P3 -> P4

X-30. ; P4 -> P1

P4 P1

P0

P3P2

20

30

20 20 30

Y

X

(mm)

M700V/M70V Series Programming Manual (M2/M0 Format)

6.3 Circular Interpolation ; G02,G03

47

6.3 Circular Interpolation ; G02,G03

Function and purpose

Command format

G02 X__ Y__ I__ J__ F__ ; … Circular interpolation : Clockwise (CW)

G03 X__ Y__ I__ J__ F__ ; … Circular interpolation : Counterclockwise (CCW)

X,Y End point

I,J Arc center

F Feedrate

6 Interpolation Functions

MITSUBISHI CNC

48

Detailed description

(1) For the arc command, the arc end point coordinates are assigned with addresses X, Y (or Z, or parallel

axis X, Y, Z), and the arc center coordinate value is assigned with addresses I, J (or K).

Either an absolute value or incremental value can be used for the arc end point coordinate value

command, but the arc center coordinate value must always be commanded with an incremental value

from the start point.

The arc center coordinate value is commanded with a program command unit. Caution is required for

the circular command of an axis for which the program command unit (#1015 cunit) differs. Command

with a decimal point to avoid confusion.

(2) G02 (G03) is a modal command of the 01 group. When G02 (G03) command is issued continuously, the

next block and after can be commanded with only coordinate words.

The circular rotation direction is distinguished by G02 and G03.

G02 Clockwise (CW)

G03 Counterclockwise (CCW)

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

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

(a) Plane selection : Is there an arc parallel to one of the XY, ZX or YZ planes?

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

(c) Circular end point coordinates : Given by addresses X, Y, Z

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

(e) Feedrate : Given by address F

G17(X-Y) plane G18(Z-X) plane G19(Y-Z) plane

X

Z

Y G3

G3 G3

G2 G2

G2

Y

X

G02

G03

G02

G03

X

Z

G02

G03

Y

Z

M700V/M70V Series Programming Manual (M2/M0 Format)

6.3 Circular Interpolation ; G02,G03

49

Plane selection

The arc exists in the following three planes (refer to the figure in the Detailed description), and are selected

by the following method.

XY plane

G17; Command with a (plane selection G code)

ZX plane

G18; Command with a (plane selection G code)

YZ plane

G19; Command with a (plane selection G code)

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 operated up to the end point coordinate value only for that

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»

G90 X0 Y0 ; N1 G02 X20. I10. F500 ; … (a) N2 G00 X0 ; N3 G02 X20. F500 ; … (b) M02 ;

(a) The circular interpolation (G02) is executed because there is a center command.

(b) The linear interpolation (G01) is executed because there is no center and radius command.

N1

N3

200

6 Interpolation Functions

MITSUBISHI CNC

50

Program example

(Example 1)

(Example 2)

(S) Start point (E) End point (J) Circle center

G02 J50. F500; Circle command

(S) Start point (E) End point (J) Arc center

G91 G02 X50.Y50. J50. F500; 3/4 command

F = 500mm/min

+Y

+X

J = 50mm

Y

X

(S) / (E)

(J)

F = 500mm/min

+Y

+X

J = 50mm X50Y50mm

(J)

Y

X

(E)

(S)

M700V/M70V Series Programming Manual (M2/M0 Format)

6.3 Circular Interpolation ; G02,G03

51

Precautions

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

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

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

#1084 RadErr Parameter value 0.100 Start point radius=5.000 End point radius=4.899 ErrorR=0.101 (S) Start point (CP) Center (E) End point (SR) Start point radius (ER) End point radius (AL) Alarm stop

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

#1084 RadErr Parameter value 0.100 Start point radius=5.000 End point radius=4.900 ErrorR=0.100 (S) Start point (CP) Center (E) End point (SR) Start point radius (ER) End point radius (SI) Spiral interpolation

(G91) G02 X9.899 I5. ;

R (S)

(AL)

(SR) (ER)

(CP) (E)

(G91) G02 X9.9 I5. ;

R

(SI)

(E)(CP) (S)

(SR) (ER)

6 Interpolation Functions

MITSUBISHI CNC

52

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, J, K)

designation, these commands can also be issued by directly designating the circular radius R.

Command format

The arc radius is commanded with a program command unit. Caution is required for the arc command of an

axis for which the program command unit (#1015 cunit) 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.

The following condition must be met with an R-specified arc interpolation command:

Where L is the line from the start point to the end point. If an R specification and I, J, (K) specification are

given at the same time in the same block, the circular command with the R specification takes precedence. In

the case of a full-circle command (where the start and end points coincide), an R specification circular

command will be completed immediately even if it is issued and no operation will be executed. An I, J, (K)

specification circular command should therefore be used in such a case.

G02 X__ Y__ R__ F__ ; … R specification circular interpolation Clockwise (CW)

G03 X__ Y__ R__ F__ ; … R specification circular interpolation Counterclockwise (CCW)

X X axis end point coordinate

Y Y axis end point coordinate

R Arc radius

F Feedrate

(S) Start point (E) End point

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

L

r

R < 0

(S)

R > 0

(E)

L 12 r

M700V/M70V Series Programming Manual (M2/M0 Format)

6.4 R Specification Circular Interpolation ; G02,G03

53

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, «the midpoint of segment connecting the start and end points» is

compensated as the circular center, because the required semicircle is not obtained by calculation error in R

specification circular interpolation.

Set the setting value to the parameter «#11028 Tolerance Arc Cent (Tolerable correction value of arc center

error)».

(Example) «#11028 Tolerance Arc Cent» = «0.000 (mm)»

Calculation error margin compensation allowance value: 0.002 mm

Segment connecting the start and end points: 10.000

N3: Radius 2 = 10.002 «Error 0.002 -> Compensate»

N5: Radius 2 = 10.004 «Error 0.004 -> Do not compensate»

Therefore, this example is shown in the above figure.

Program example

(Example 1)

(Example 2)

(Example 3)

(Example 4)

Setting value Tolerance value

Setting value < 0 0(Center error will not be interpolated)

Setting value = 0 2 minimum setting increment

Setting value > 0 Setting value

G90 X0 Y0 ; N1 G02 X10. R5.000; N2 G0 X0; …(a) N3 G02 X10. R5.001; N4 G0 X0; …(b) N5 G02 X10. R5.002; N6 G0 X0; M02 ;

(a) Compensate the center coordinate: Same as N1 path

(b) Do not compensate the center coordinate: Slightly inside N1 path

G02 Xx1 Yy1 Rr1 Ff1 ; XY plane R-specified arc

G03 Zz1 Xx1 Rr1 Ff1 ; ZX plane R-specified arc

G02 Xx1 Yy1 Ii1 Jj1 Rr1 Ff1 ; XY plane R-specified arc (When the R specification and I, J, (K) specification are contained in the same block, the circular command with the R specification takes precedence.)

G17 G02 Ii1 Jj1 Rr1 Ff1 ; XY plane This is an R-specified arc, but as this is a circle command, it will be completed immediately.

0 10

N1, N3

N5

6 Interpolation Functions

MITSUBISHI CNC

54

6.5 Plane Selection ; G17,G18,G19

Function and purpose

The plane to which the movement of the tool during the circle interpolation (including helical cutting) and tool

radius compensation command belongs is selected.

If the 3 basic axes and the parallel axes corresponding to these basic axes are entered as parameters, the

commands can select the plane composed of any 2 axes which are not parallel axes. If a rotary axis is

registered as a parallel axis, the commands can select the plane containing the rotary axis.

The plane selection is as follows:

— Plane that executes circular interpolation (including helical cutting)

— Plane that executes tool radius compensation

— Plane that executes fixed cycle positioning

Command format

X, Y and Z indicate each coordinate axis or the parallel axis.

Detailed description

Parameter entry

Table 1 Examples of plane selection parameter entry

As shown in the above example, the basic axis and its parallel axis can be registered.

The basic axis can be an axis other than X, Y and Z.

Axes that are not registered are irrelevant to the plane selection.

G17 ; … Plane selection X-Y

G18 ; … Plane selection Z-X

G19 ; … Plane selection Y-Z

#1026-1028base_I,J,K #1029-1031aux_I,J,K

I X U

J Y

K Z V

M700V/M70V Series Programming Manual (M2/M0 Format)

6.5 Plane Selection ; G17,G18,G19

55

Plane selection system

In Table 1,

I is the horizontal axis for the G17 plane or the vertical axis for the G18 plane

J is the vertical axis for the G17 plane or the horizontal axis for the G19 plane

K is the horizontal axis for the G18 plane or the vertical axis for the G19 plane

In other words,

G17 ….. IJ plane

G18 ….. KI plane

G19 ….. JK plane

(1) Axis addresses assigned in the same block as the plane selection (G17, G18, G19) command determine

which of the basic axes or parallel axes are to be in the actual plane selected.

For the parameter entry example in Table 1.

G17 X__Y__ ; XY plane

G18 X__V__ ; VX plane

G18 U__V__ ; VU plane

G19 Y__Z__ ; YZ plane

G19 Y__V__ ; YV plane

(2) The plane will not changeover at a block where a plane selection G code (G17, G18, G19) is not

commanded.

G17 X__Y__ ; XY plane

Y__Z__ ; XY plane (plane does not change)

(3) If the axis address is omitted in the block where the plane selection G code (G17, G18, G19) is

commanded, it is assumed that the axis addresses of the 3 basic axes have been omitted.

For the parameter entry example in Table 1.

G17 ; XY plane

G17 U__ ; UY plane

G18 U__ ; ZU plane

G18 V__ ; VX plane

G19 Y__ ; YZ plane

G19 V__ ; YV plane

(4) When the axis address is commanded to the same block as the plane selection G code (G17, G18, G19),

the commanded axes will travel.

(5) The axis command that does not exist in the plane determined by the plane selection G code (G17, G18,

G19) is irrelevant to the plane selection.

For the parameter entry example in Table 1.

G17 U__Z__ ;

If the above is commanded, the UY plane will be selected, and Z will move regardless of the plane.

(6) When the basic axes or their parallel axes are duplicated and assigned in the same block as the plane

selection G code (G17, G18, G19), the plane is determined in the order of basic axes, and then parallel

axes.

For the parameter entry example in Table 1.

G17 U__Y__W__ ;

If the above is commanded, the UY plane will be selected, and W will move regardless of the plane.

(Note 1) When the power is turned ON or when the system is reset, the plane set by the parameter «#1025

I_plane» is selected.

6 Interpolation Functions

MITSUBISHI CNC

56

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, and tapered thread-cutting. Multiple

thread screws, etc., can also be machined by designating the thread cutting angle.

Command format

Normal lead thread cutting

Precision lead thread cutting

G33 Z__(X__ Y____ ) F__ Q__ ;

Z (X Y ) Thread end point

F Lead of long axis (axis which moves the most) direction

Q Thread cutting start shift angle (0.001 — 360.000)

G33 Z__(X__ Y____ ) E__ Q__ ;

Z (X Y ) Thread end point

E Lead of long axis (axis which moves most) direction

Q Thread cutting start shift angle (0.001 — 360.000)

M700V/M70V Series Programming Manual (M2/M0 Format)

6.6 Thread Cutting

57

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 «#8156

Fine thread cut E» is set to «1» for precision lead designation.)

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

Thread cutting metric input

(t) Tapered thread section 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.

Input setting unit B (0.001mm)

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

Least Command Increments 1(=0.001) (1.=1.000)

1(=0.0001) (1.=1.0000)

1(=1.00) (1.=1.00)

Command range 0.001 — 999.999

0.0001 — 999.9999

0.03 — 999.99

Input setting unit C (0.0001mm)

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

Least Command Increments 1(=0.0001) (1.=1.0000)

1(=0.00001) (1.=1.00000)

1(=1.000) (1.=1.000)

Command range 0.0001 — 999.9999

0.00001 — 999.99999

0.026 — 222807.017

Input setting unit D (0.00001mm)

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

Least Command Increments 1(=0.00001) (1.=1.00000)

1(=0.000001) (1.=1.000000)

1(=1.0000) (1.=1.0000)

Command range 0.00001 — 999.99999

0.000001 — 999.999999

0.0255 — 224580.0000

Input setting unit E (0.000001mm)

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

Least Command Increments 1(=0.000001) (1.=1.000000)

1(=0.0000001) (1.=1.0000000)

1(=1.00000) (1.=1.00000)

Command range 0.000001 — 999.999999

0.0000001 — 999.9999999

0.02541 — 224719.00000

LZ

Z

XLX

a

(t)

6 Interpolation Functions

MITSUBISHI CNC

58

Thread cutting inch input

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

maximum cutting feedrate.

(3) The constant surface speed control function should not be used for taper thread cutting commands or

scrolled thread cutting commands.

(4) The spindle rotation speed should be kept constant throughout from the rough cutting until the finishing.

(5) If the feed hold function is employed during thread cutting to stop the feed, the thread ridges will lose

their shape. For this reason, feed hold does not function during thread cutting. Note that this is valid from

the time the thread cutting command is executed to the time the axis moves.

If the feed hold switch is pressed during thread cutting, block stop will occur at the end point of the block

following the block in which thread cutting is completed (no longer G33 mode).

(6) The converted cutting feedrate is compared with the cutting feed clamp rate when thread cutting starts,

and if it is found to exceed the clamp rate, an operation error will occur.

(7) In order to protect the lead during thread cutting, a cutting feedrate which has been converted may

sometimes exceed the cutting feed clamp rate.

(8) An illegal lead is normally produced at the start of the thread and at the end of the cutting because of

servo system delay and other such factors.

Therefore, it is necessary to command a thread length which is determined by adding the illegal lead

lengths to the required thread length.

(9) The spindle rotation speed is subject to the following restriction :

1 <= R <= Maximum feedrate/Thread lead

Where R <= Tolerable speed of encoder (r/min)

R: Spindle rotation speed (r/min)

Thread lead = mm or inches

Maximum feedrate= mm/min or inch/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.

Input setting unit B (0.0001inch)

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

Least Command Increments 1(=0.0001) (1.=1.0000)

1(=0.00001) (1.=1.00000)

1(=1.000) (1.=1.000)

Command range 0.0001 — 39.3700

0.00001 — 39.37007

0.025 — 9999.999

Input setting unit C (0.00001inch)

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

Least Command Increments 1(=0.00001) (1.=1.00000)

1(=0.000001) (1.=1.000000)

1(=1.0000) (1.=1.0000)

Command range 0.00001 — 39.37007

0.000001 — 39.370078

0.0255 — 9999.9999

Input setting unit D (0.000001inch)

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

Least Command Increments 1(=0.000001) (1.=1.000000)

1(=0.0000001) (1.=1.0000000)

1(=1.00000) (1.=1.00000)

Command range 0.000001 — 39.370078

0.0000001 — 39.3700787

0.02541 — 9999.99999

Input setting unit E (0.0000001inch)

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

Least Command Increments 1(=0.0000001) (1.=1.0000000)

1(=0.00000001) (1.=1.00000000)

1(=1.000000) (1.=1.000000)

Command range 0.0000001 — 39.3700787

0.00000001 — 39.37007873

0.025401 — 9999.999999

M700V/M70V Series Programming Manual (M2/M0 Format)

6.6 Thread Cutting

59

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

rotation.

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

ignored.

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

(G94).

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

cutting.

(14) When a thread cutting is commanded during tool radius compensation, the compensation is temporarily

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 (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 synchronization signal of the rotary encoder

and starts movement.

Make sure to carry out timing synchronization operation between part systems before issuing a thread

cutting command with multiple part systems. For example, when using the 1-spindle specifications with

two part 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

synchronization signal causing an illegal operation.

(18) The thread cutting start shift angle is not modal. If there is no Q command with G33, this will be handled

as «Q0».

(19) The automatic handle interrupt/interruption is valid during thread cutting.

(20) If a value exceeding 360.000 is command in G33 Q, a program error (P35) will occur.

(21) G33 cuts one row with one cycle. To cut two rows, change the Q value, and issue the same command.

6 Interpolation Functions

MITSUBISHI CNC

60

Program example

N110 G90 G0 X-200. Y-200. S50 M3 ; The spindle center is positioned to the workpiece center, and the spindle rotates in the forward direction.N111 Z110. ;

N112 G33 Z40. F6.0 ; The first thread cutting is executed. Thread lead = 6.0mm

N113 M19 ; Spindle orientation is executed with the M19 command.

N114 G0 X-210. ; The tool is evaded in the X axis direction.

N115 Z110. M0 ; The tool rises to the top of the workpiece, and the program stops with M00. Adjust the tool if required.

N116 X-200. ; M3 ;

Preparation for second thread cutting is done.

N117 G04 X5.0 ; Command dwell to stabilize the spindle rotation if necessary.

N118 G33 Z40. ; The second thread cutting is executed.

Z

X Y

X

10 50 10

M700V/M70V Series Programming Manual (M2/M0 Format)

6.6 Thread Cutting

61

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

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 the parameter «#8156 Fine thread cut E» to «0».)

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

(4) See Section «Constant lead thread cutting» for other details.

G33 Z__ (X_ Y_ _) E__ Q__ ; … Inch thread cutting

Z (X Y ) End point of thread cutting

E Number of ridges per inch in direction of long axis (axis which moves most) (decimal point command can also be assigned)

Q Thread cutting start shift angle, 0 to 360

6 Interpolation Functions

MITSUBISHI CNC

62

Program example

Thread lead ….. 3 threads/inch (= 8.46666 …)

When programmed with 1= 10 mm, 2=10 mm using metric input

N210 G90 G0 X-200. Y-200. S50 M3 ;

N211 Z110. ;

N212 G91 G33 Z-70. E3.0 ; (First thread cutting)

N213 M19 ;

N214 G90 G0 X-210. ;

N215 Z110. M0 ;

N216 X-200. ; M3 ;

N217 G04 X2.0 ;

N218 G91 G33 Z-70. ; (Second thread cutting)

Z

XY

X

1 50.0mm

2

M700V/M70V Series Programming Manual (M2/M0 Format)

6.7 Helical Interpolation ; G17 to G19, G02, G03

63

6.7 Helical Interpolation ; G17 to G19, 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.

3-dimentional path XY plane path (projection path)

(a) Program command path

(b) XY plane projection path in command program

(S) Start point

(E) End point

X

Y

Z

(a)

(b)

(S)

(E) j

Y

X

i

(E)

(S)

6 Interpolation Functions

MITSUBISHI CNC

64

Command format

Either an absolute value or incremental value can be used for the arc end point coordinate value command

and the linear axis end point coordinate value command, but the arc center coordinate value must always be

commanded with an incremental value from the start point.

The arc center coordinate value and arc radius value are commanded with a program command unit. Caution

is required for the helical interpolation command of an axis for which the program command unit (#1015 cunit)

differs.

Command with a decimal point to avoid confusion.

G17/G18/G19 G02/G03 X__ Y__ Z__ I__ J__ P__ F__ ; … Helical interpolation command (Specify arc center)

G17/G18/G19 G02/G03 X__ Y__ Z__ R__ F__ ; … Helical interpolation command (Specify radius (R))

G17/G18/G19 Arc plane (G17: X-Y plane, G18: Z-X plane, G19: Y-Z plane)

G02/G03 Arc rotation direction (G02: clockwise, G03: counterclockwise)

X, Y Arc end point coordinates

Z Linear axis end point coordinates

I, J Arc center coordinates

P Number of pitches

R Arc radius

F Feedrate

M700V/M70V Series Programming Manual (M2/M0 Format)

6.7 Helical Interpolation ; G17 to G19, G02, G03

65

Detailed description

Speed designation during the helical interpolation

Normally, the helical interpolation speed is designated with the tangent speed F’ including the 3rd axis

interpolation element as shown in the lower drawing. However, when designating the arc plane element

speed, the tangent speed F on the arc plane is commanded as shown in the upper drawing.

The NC automatically calculates the helical interpolation tangent speed F’ so that the tangent speed on the

arc plane is F.

The arc plane element speed designation and normal speed designation can be selected with the parameter.

(S) Start point

(E) End point

#1235 set07/bit0 Meaning

1 Arc plane element speed designation is selected.

0 Normal speed designation is selected.

Y

Z

X

F’

F

Y

X (S)

(E)

(S)

(E)

6 Interpolation Functions

MITSUBISHI CNC

66

Normal speed designation

(1) This command should be issued with a linear axis (multiple axes can be commanded) that does not

contain a circular axis in the circular interpolation command combined.

(2) For feedrate F, command the X, Y and Z axis composite element directions speed.

(3) Pitch L is obtained with the following expression.

xs, ys are the start point coordinates from the arc center

xe, ye are the end point coordinates from the arc center

(4) If pitch No. is 0, address P can be omitted.

(Note) The pitch No. P command range is 0 to 9999.

The pitch No. designation (P command) cannot be made with the R-specified arc.

(S) Start point (E) End point

Y

X

e

s

P

2

1

Z

L

Z

Y

X

(E)

(S)

L =

= e — s = tan — 1 — tan — 1 ( )0 < 2 ysye

xsxe

(2 P + )/2 Z

M700V/M70V Series Programming Manual (M2/M0 Format)

6.7 Helical Interpolation ; G17 to G19, G02, G03

67

(5) Plane selection

The helical interpolation arc plane selection is determined with the plane selection mode and axis

address as for the circular interpolation. For the helical interpolation command, the plane where circular

interpolation is executed is commanded with the plane selection G code (G17, G18, G19), and the 2

circular interpolation axes and linear interpolation axis (axis that intersects with circular plane) 3 axis

addresses are commanded.

XY plane circular, Z axis linear

Command the X, Y and Z axis addresses in the G02 (G03) and G17 (plane selection G code) mode.

ZX plane circular, Y axis linear

Command the X, Y and Z axis addresses in the G02 (G03) and G18 (plane selection G code) mode.

YZ plane circular, X axis linear

Command the X, Y and Z axis addresses in the G02 (G03) and G19 (plane selection G code) mode.

The plane for an additional axis can be selected as with circular interpolation.

UY plane circular, Z axis linear

Command the U, Y and Z axis addresses in the G02 (G03) and G17 (plane selection G code) mode.

In addition to the basic command methods above, the command methods described in the following

program example can be used. Refer to the section «Plane Selection; G17,G18,G19» for the arc planes

selected with these command methods.

Arc plane element speed designation

If arc plane element speed designation is selected, the F command will be handled as modal data in the same

manner as the normal F command. This will also apply to the following G01, G02 and G03 commands.

(Example)

When the arc plane element speed designation is selected, only the helical interpolation speed command is

converted to the speed commanded with the arc plane element. The other linear and arc commands operate

as normal speed commands.

(1) The actual feedrate display (Fc) indicates the tangent element of the helical interpolation.

(2) The modal value speed display (FA) indicates the command speed.

(3) The speed data acquired with API functions follows the Fc and FA display.

(4) This function is valid only when feed per minute (asynchronous feed:G94) is selected. If feed per

revolution (synchronous feed: G95) is selected, the arc plane element speed will not be designated.

(5) The helical interpolation option is required to use this function.

G17 G91 G02 X10. Y10. Z-4. I10. F100 ; Helical interpolation at speed at which arc plane element is F100

G01 X20. ; Linear interpolation at F100

G02 X10. Y-10. Z4. J10. ; Helical interpolation at speed at which arc plane element is F100

G01 Y-40. F120; Linear interpolation at F120

G02 X-10. Y-10. Z-4. I-10. ; Helical interpolation at speed at which arc plane element is F120

G01 X-20. ; Linear interpolation at F120

6 Interpolation Functions

MITSUBISHI CNC

68

Program example

(Example 1)

(Note) If pitch No. is 0, address P can be omitted.

(Example 2)

(Example 3)

G17 ; XY plane

G03 Xx1 Yy1 Zz1 Ii1 Jj1 P0 Ff1; XY plane arc, Z axis linear

G17 ; XY plane

G02 Xx1 Yy1 Zz1 Rr1 Ff1; XY plane arc, Z axis linear

G17 G03 Uu1 Yy1 Zz1 Ii1 Jj1 P2 Ff1; UY plane arc, Z axis linear

z1

Z

Y

X

z1 r1

Z

Y

X

z1

Z

Y

U

M700V/M70V Series Programming Manual (M2/M0 Format)

6.7 Helical Interpolation ; G17 to G19, G02, G03

69

(Example 4)

(Note) If the same system is used, the standard axis will perform circular interpolation and the additional

axis will perform linear interpolation.

(Example 5)

(Note) Two or more axes can be designated for the linear interpolation axis.

G18 G03 Xx1 Uu1 Zz1 Ii1 Kk1 Ff1; ZX plane arc, U axis linear

G18 G02 Xx1 Uu1 Yy1 Zz1 Ii1 Jj1 Kk1 Ff1; ZX plane arc, U axis, Y axis linear (The J command is ignored)

u1

z1

x1

Z

XU

6 Interpolation Functions

MITSUBISHI CNC

70

6.8 Unidirectional Positioning ; G60

Function and purpose

The G60 command can position the tool at a high degree of precision without backlash error by locating the

final tool position from a constant direction.

Command format

Detailed description

(1) The creep distance for the final positioning as well as the final positioning direction is set by parameter.

(2) After the tool has moved at the rapid traverse rate to the position separated from the final position by an

amount equivalent to the creep distance, it moves to the final position in accordance with the rapid

traverse setting where its positioning is completed.

G60 X__ Y__ Z__ __; … Unidirectional positioning

Additional axis

(S) Start point

(E) End point

(ST) Stop once

(PP) Positioning position

(FD) Final advance direction

(CD) G60 creep distance

G60a

G60 — a

+-

(PP)

(S)

(E)

(ST)

(S)

(FD)

(CD)

M700V/M70V Series Programming Manual (M2/M0 Format)

6.8 Unidirectional Positioning ; G60

71

(3) The above positioning operation is performed even when Z axis commands have been assigned for Z

axis cancel and machine lock. (Display only)

(4) When the mirror image function is ON, the tool will move in the opposite direction as far as the

intermediate position due to the mirror image function but the operation within the creep distance during

its final advance will not be affected by mirror image.

(5) The tool moves to the end point at the dry run speed during dry run when the G0 dry run function is valid.

(6) Feed during creep distance movement with final positioning can be stopped by resetting, emergency

stop, interlock, feed hold and rapid traverse override zero.

The tool moves over the creep distance at the rapid traverse setting. Rapid traverse override is valid.

(7) Unidirectional positioning is not performed for the drilling axis during drilling fixed cycles.

(8) Unidirectional positioning is not performed for shift amount movements during the fine boring or back

boring fixed cycle.

(9) Normal positioning is performed for axes whose creep distance has not been set by parameter.

(10) Unidirectional positioning is always a non-interpolation type of positioning.

(11) When the same position (movement amount of zero) has been commanded, the tool moves back and

forth over the creep distance and is positioned at its original position from the final advance direction.

(12) Program error (P61) will occur when the G60 command is assigned with an NC system which has not

been provided with this particular specification.

6 Interpolation Functions

MITSUBISHI CNC

72

6.9 Cylindrical Interpolation ; G07.1

Function and purpose

This function develops a shape on the side of a cylinder (shape in a cylindrical coordinate system) into a

plane. When the developed shape is programmed as the plane coordinates, it will be converted into a linear

axis movement and rotary axis movement in the cylindrical coordinates to conduct a contour control when

machining.

As programming can be carried out to the developed shape of the side of the cylinder, this is effective for

machining cylindrical cams, etc. When programmed with the rotary axis and its orthogonal axis, grooves and

other shapes can be machined on the side of the cylinder.

Command format

G07.1 C__ ; … Cylindrical interpolation mode start/cancel

C Cylinder radius value (When rotary axis name is «C») — Radius value 0: Cylindrical interpolation mode start — Radius value = 0: Cylindrical interpolation mode cancel

r

B

Z

X Y

0

360

2 r

M700V/M70V Series Programming Manual (M2/M0 Format)

6.9 Cylindrical Interpolation ; G07.1

73

Detailed description

(1) The coordinate commands in the interval from the start to cancellation of the cylindrical interpolation

mode will be the cylindrical coordinate system.

(2) G107 can be used instead of G07.1.

(3) Command G07.1 is an independent block. A program error (P33) will occur if this command is issued in

the same block as other G codes.

(4) Program the rotary axis with an angle degree.

(5) Linear interpolation or circular interpolation can be commanded during the cylindrical interpolation mode.

Note that the plane selection command must be issued just before the G07.1 block.

(6) The coordinate commands can be both an absolute command or incremental command.

(7) Tool radius compensation can be applied on the program command. Cylindrical interpolation will be

executed to the path after it has gone through a tool radius compensation.

(8) Command the tangent speed on the developed cylinder by F. F is in mm/min or inch/min unit.

Cylindrical interpolation accuracy

In the cylindrical interpolation mode, the movement amount of the rotary axis commanded with an angle is

converted into distance on a circle periphery, and after calculating the linear and circular interpolation

between the other axes, the amount is converted into an angle again.

Thus, the actual movement amount may differ from the commanded value such as when the cylinder radius is

small. Note that the gap generated by this will not be cumulated.

Related parameters

#1516 mill_ax (Milling axis name)

#8111 Milling Radius

#1267 ext03/bit0 (G code type)

#1270 ext06/bit7 (Handling of C axis coordinate during cylindrical interpolation)

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)

6 Interpolation Functions

MITSUBISHI CNC

74

Plane selection

The axis used for cylindrical interpolation must be set with the plane selection command. (Note)

Use parameters (#1029, #1030 and #1031) to set which parallel axis corresponds to the rotary axis.

The circular interpolation and tool radius compensation, etc., can be designated on that plane.

The plane selection command is set immediately before or after the G07.1 command. If a movement

command is issued without this command, a program error (P485) will occur.

When the axis address is commanded while selecting the plane, the axis will travel. To prevent the axis from

traveling, command the address with the incremental value.

(Note) Depending on the model or version, the Z-C plane (Y-Z cylindrical plane) will be automatically

selected with G07.1 and G19.

The circular interpolation and tool radius compensation, etc., can be designated on that plane.

(Example)

G19 Z0. C0. ; …………….. Plane selection command for cylindrical interpolation, and 2-axis command of Z axis and C axis for interpolation

G07.1 C100. ; …………….. Cylindrical interpolation start

:

G07.1 C0 ; …………….. Cylindrical interpolation cancel

Basic coordinate system X,Y,Z

Cylindrical coordinate system C , Y , Z (Rotary axis is X axis’ parallel axis) #1029

Cylindrical coordinate system X , C , Z (Rotary axis is Y axis’ parallel axis) #1030

Cylindrical coordinate system X , Y , C (Rotary axis is Z axis’ parallel axis) #1031

Basic coordinate system X,Y,Z

Cylindrical coordinate system

G17

Y

X

G18

Z

X

G19

Y

Z

G18

Z

C

G17

C

Y

G19

C

Z

G17

X

C

G18

C

X

G19

Y

C

G17

Y

X

G18

Z

X

G19

Y

Z

Z

C

G19

M700V/M70V Series Programming Manual (M2/M0 Format)

6.9 Cylindrical Interpolation ; G07.1

75

Program example

#1029 aux_I

#1030 aux_J C

#1031 aux_K

N01 G28 XZC ;

N02 T020 ;

N03 G97 S100 M23 ;

N04 G00 X50. Z0. ;

N05 G94 G01 X40. F100. ;

N06 G19 C0 Z0 ; …………. Plane selection command for cylindrical interpolation and two axes command for interpolation

N07 G07.1 C20. ; …………. Cylindrical interpolation start

N08 G41 ;

N09 G01 Z-10. C80. F150 ;

N10 Z-25. C90. ;

N11 Z-80. C225 ;

N12 G03 Z-75.C270. R55. ;

N13 G01 Z-25 ;

N14 G02 Z-20.C280. R80. ;

N15 G01 C360. ;

N16 G40 ;

N17 G07.1 C0 ; …………. Cylindrical interpolation cancel

N18 G01 X50. ;

N19 G0 X100. Z100. ;

N20 M25 ;

N21 M30 ;

50

100

150

200

250

300

350

-20-40-60-80

C

Z

N09N10

N11

N12 N13

N14

N15

(mm)

6 Interpolation Functions

MITSUBISHI CNC

76

Relation with other functions

Circular interpolation

(1) Circular interpolation between the rotary axis and linear axis is possible during the cylindrical

interpolation mode.

(2) An R specification command can be issued with circular interpolation. (I, J and K cannot be designated.)

Tool radius compensation

The tool radius can be compensated during the cylindrical interpolation mode.

(1) Command the plane selection in the same manner as circular interpolation.

When using tool radius compensation, start up/cancel the compensation in the cylindrical interpolation

mode.

(2) A program error (P485) will occur if G07.1 is commanded during tool radius compensation.

(3) If the G07.1 command is issued with no movement command after the tool radius compensation 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.

Cutting feed per minute (asynchronous feed)

(1) The feed per minute (asynchronous) mode is forcibly set when the cylindrical interpolation mode is

started.

(2) When the cylindrical interpolation mode is canceled, the feed per revolution (synchronous) will return to

the state before the cylindrical interpolation mode was started.

Constant surface speed control

(1) A program error (P485) will occur if G07.1 is commanded in the constant surface speed control mode

(G96).

Miscellaneous functions

(1) The miscellaneous function (M) and 2nd miscellaneous function can be issued in the cylindrical

interpolation mode.

(2) The S command in the cylindrical interpolation mode specifies the rotary tool’s rotation speed instead of

the spindle rotation speed.

M700V/M70V Series Programming Manual (M2/M0 Format)

6.9 Cylindrical Interpolation ; G07.1

77

Tool length compensation

(1) Program error (P481) will occur if tool length compensation is performed in the cylindrical interpolation

mode.

(2) Complete the tool compensation operation (movement of tool length and wear compensation amount)

before executing the cylindrical interpolation.

If the tool compensation operation is not completed when the cylindrical interpolation start command is

issued, the followings will occur:

— The machine coordinate will not change even if G12.1 is executed.

— The workpiece coordinate will change to that of the post tool length compensation when G07.1 is

executed.

(Even if the cylindrical interpolation is canceled, this workpiece coordinate will not be canceled. )

F command during cylindrical interpolation

As for the F command during cylindrical interpolation mode, whether to use the previous F command depends

on the previous mode of the feed per minute command (G94/G98) or feed per rotation command (G95/G99).

(1) When G94 (G98) is commanded just before G07.1

If there is no F command in the cylindrical interpolation, the previous F command feedrate will be used.

After the cylindrical interpolation mode is canceled, the F command feedrate set at the start of the

cylindrical interpolation mode or the last F command feedrate set during cylindrical interpolation will

continue to be the feedrate.

(2) When G95 (G99) is commanded just before G07.1

The previous F command feedrate cannot be used during cylindrical interpolation, thus a new F

command must be issued.

After the cylindrical interpolation mode is canceled, the feedrate will return to the state before the

cylindrical interpolation mode was started.

When there is no F command in G07.1

When F is commanded in G07.1

:

:

G43 H12 ; … Tool length compensation before cylindrical interpolation -> Valid

G0 X100. Z0. ;

G19 Z C ;

G07.1 C100. ;

:

G43 H11 ; … Tool length compensation in cylindrical interpolation mode -> Program error

:

G07.1 C0 ;

Previous mode No F command After G07.1 is canceled

G94 (G98) Previous F is used <-

G95 (G99) Program error (P62) F just before G07.1 is used

Previous mode With F command After G07.1 is canceled

G94 (G98) Commanded F is used <-

G95 (G99) 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

MITSUBISHI CNC

78

Restrictions and precautions

(1) The following G code commands can be used during the cylindrical interpolation mode.

A program error will occur if a G code other than those listed above is commanded during cylindrical

interpolation.

(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 during cylindrical interpolation has not

completed the reference position return.

(4) Tool radius compensation must be canceled before canceling the cylindrical interpolation mode.

(5) When the cylindrical interpolation mode is canceled and switched to the cutting mode, the plane selected

before the cylindrical interpolation will be restored.

(6) Program cannot be restarted (program restart) when the block is in the cylindrical interpolation.

(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.

G code Details

G00 Positioning

G01 Linear interpolation

G02 Circular interpolation (CW)

G03 Circular interpolation (CWW)

G04 Dwell

G09 Exact stop check

G40-42 Tool radius compensation

G61 Exact stop mode

G64 Cutting mode

G65 Macro call (simple call)

G66 Macro modal call (modal call)

G66.1 Macro modal call (block call per macro)

G67 Macro modal call cancel (modal call cancel)

G80-89 Fixed cycle for drilling

G90/91 Absolute/incremental value command

G94 Asynchronous feed

G98 Hole drilling cycle initial return

G99 Hole drilling cycle R point return

M700V/M70V Series Programming Manual (M2/M0 Format)

6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113

79

6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113

Function and purpose

This function converts the commands programmed with the orthogonal coordinate axis into linear axis

movement (tool movement) and rotary axis movement (workpiece rotation), and controls the contour.

The plane that uses the linear axis as the plane’s 1st orthogonal axis, and the intersecting hypothetical axis as

the plane’s 2nd axis (hereafter «polar coordinate interpolation plane») is selected. Polar coordinate

interpolation is carried out on this plane. The workpiece coordinate system zero point is used as the

coordinate system zero point during polar coordinate interpolation.

This is effective for cutting a notch in a linear line to the external diameter of the workpiece, for cutting cam

shafts and etc.

Command format

(a) Linear axis

(b) Rotation axis (hypothetical axis)

(c) Polar coordinate interpolation plane (G17 plane)

G12.1; … Polar coordinate interpolation mode start

G13.1; … Polar coordinate interpolation mode cancel

X

C

Z

(c)

(a)

(b)

6 Interpolation Functions

MITSUBISHI CNC

80

Detailed description

(1) The coordinate commands in the interval from the start to cancellation of the polar coordinate

interpolation mode will be the polar coordinate interpolation.

(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 other G codes.

(4) Linear interpolation or circular interpolation can be commanded during the polar coordinate interpolation

mode.

(5) The coordinate commands can be both an absolute command or incremental command.

(6) Tool radius compensation can be applied on the program command. Polar coordinate interpolation will

be executed to the path after it has gone through a tool radius compensation.

(7) Command the tangent speed in the polar coordinate interpolation plane (orthogonal coordinate system)

by F. F is in mm/min or inch/min unit.

(8) When the G12.1/G13.1 command is issued, the deceleration check is executed.

Plane selection

The linear axis and rotary axis used for polar coordinate interpolation must be set beforehand with

parameters.

(1) Determine the deemed plane for carrying out polar coordinate interpolation with the parameter (#1533) of

the linear axis used for polar coordinate interpolation.

(2) A program error (P485) will occur if the plane selection command (G17 to G19) is issued during the polar

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 when the parameter (#1533) is blank (no setting).

Related parameters

#1516 mill_ax (Milling axis name)

#1517 mill_c (Milling interpolation hypothetical axis name)

#8111 Milling Radius

#1533 millPax (Pole coordinate linear axis name)

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)

#1533 setting value Deemed plane

X G17 (XY plane)

Y G19 (YZ plane)

Z G18 (ZX plane)

Blank (no setting) G17 (XY plane)

M700V/M70V Series Programming Manual (M2/M0 Format)

6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113

81

Program example

Hypothetical C axis

Hypothetical C axis

Tool

Path after tool radius compensation

Program path

: :

N01 G17 G90 G0 X40.0 C0 Z0; Setting of start position

N02 G12.1; Polar coordinate interpolation mode: Start

N03 G1 G42 X20.0 F2000; Actual machining start

N04 C10.0; N05 G3 X10.0 C20.0 R10.0;

N06 G1 X-20.0; Shape program

N07 C-10.0;

N08 G3 X-10.0 C-20.0 I10.0 J0; (Follows orthogonal coordinate values on X-C hypothetical axis plane.)

N09 G1 X20.0; N10 C0; N11 G40 X40.0;

N12 G13.1; Polar coordinate interpolation mode: Cancel

: : M30 ;

X

Z

C

N04

N05N06

N07

N08 N09

N10

N01 N02 N11

N03

C

X

6 Interpolation Functions

MITSUBISHI CNC

82

Relation with other functions

Program commands during polar coordinate interpolation

(1) The program commands in the polar coordinate interpolation mode are issued by the orthogonal

coordinate value of the linear axis and rotary axis (hypothetical axis) on the polar coordinate interpolation

plane.

The axis address of the rotary axis (C) is specified as the axis address for the plane’s 2nd axis

(hypothetical axis) command.

The command unit is not deg (degree). The same unit (mm or inch) as used for the command by the axis

address of the plane’s 1st axis (linear axis) will be used.

(2) The hypothetical axis coordinate value will be set to «0» when G12.1 is commanded. In other words, the

position where G12.1 is commanded will be interpreted as angle = 0, and the polar coordinate

interpolation will start.

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).

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 when the parameter (#1533) is blank (no setting).

Tool radius compensation

The tool radius can be compensated during the cylindrical interpolation mode.

(1) Command the plane selection in the same manner as polar coordinate interpolation.

When conducting tool radius compensation, it must be started up and canceled during the polar

coordinate interpolation mode.

(2) A program error (P485) will occur if polar coordinate interpolation is executed during tool radius

compensation.

(3) If the G12.1 and G13.1 commands are issued with no movement command after the tool radius

compensation is canceled, the position of the axis in the G12.1 and G13.1 commands block is

interpreted as the position applied after the tool radius compensation is canceled and the following

operations are performed.

Cutting asynchronous feed

(1) The asynchronous mode is forcibly set when the polar coordinate interpolation mode is started.

(2) When the polar coordinate interpolation mode is canceled, the synchronous mode will return to the state

before the polar coordinate interpolation mode was started.

(3) A program error (P485) will occur if G12.1 is commanded in the constant surface speed control mode

(G96).

#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)

M700V/M70V Series Programming Manual (M2/M0 Format)

6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113

83

Miscellaneous functions

(1) The miscellaneous function (M) and 2nd miscellaneous function can be issued in the polar coordinate

interpolation mode.

(2) The S command in the polar coordinate interpolation mode specifies the rotary tool’s rotation speed

instead of the spindle rotation speed.

Tool length compensation

(1) Program error (P481) will occur if tool length compensation is performed in the polar coordinate

interpolation mode.

(2) Complete the tool compensation operation (movement of tool length and wear compensation amount)

before executing the polar coordinate interpolation.

If the tool compensation operation is not completed when the polar coordinate interpolation start

command has been issued, the followings will occur:

— Machine coordinate will not change even if G12.1 is executed.

— When G12.1 is executed, the workpiece coordinate will change to that of the post tool length

compensation.

(Even if the polar coordinate interpolation is canceled, this workpiece coordinate will not be canceled. )

:

G43 H12 ; … Tool length compensation before polar coordinate interpolation -> Valid

G0 X100. Z0. ; G12.1; :

G43 H11 ; … Tool length compensation in polar coordinate interpolation mode -> Program error

: G13.1;

6 Interpolation Functions

MITSUBISHI CNC

84

F command during polar coordinate interpolation

As for the F command during polar coordinate interpolation mode, whether to use the previous F command

depends on the previous mode of the feed per minute command (G94/G98) or feed per rotation command

(G95/G99).

(1) When G94 (G98) is commanded just before G12.1

If there is no F command in the polar coordinate interpolation, the previous F command feedrate will be

used.

After the polar coordinate interpolation mode is canceled, the F command feedrate set at the start of the

polar coordinate interpolation mode or the last F command feedrate set during polar coordinate

interpolation will continue to be the feedrate.

(2) When G95 (G99) is commanded just before G12.1

The previous F command feedrate cannot be used during polar coordinate interpolation. A new F

command must be issued.

The feedrate after the polar coordinate interpolation mode is canceled will return to the state before the

polar coordinate interpolation mode was started.

[When there is no F command in G12.1]

[When F is commanded in G12.1]

Hole drilling axis in the fixed cycle for drilling command

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

with the linear axis parameter (# 1533).

Shift amount in the G76 (fine boring) or G87 (back boring) command

Shift amount in the G76 (fine boring) or G87 (back boring) command during the polar coordinate interpolation

is determined with the linear axis parameter (#1533).

Previous mode No F command After G13.1

G94 (G98) Previous F is used <-

G95 (G99) Program error (P62) F just before G12.1 is used

Previous mode With F command After G13.1

G94 (G98) Commanded F is used <-

G95 (G99) Commanded F is used *1 F just before G12.1 is used

*1) Moves with the feed per minute command during G12.1.

#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)

#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)

M700V/M70V Series Programming Manual (M2/M0 Format)

6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113

85

Restrictions and precautions

(1) The following G code commands can be used during the polar coordinate interpolation mode.

A program error (P481) may occur if a G code other than those listed above is commanded during polar

coordinate interpolation.

(2) Program cannot be restarted (program restart) when the block is in the cylindrical interpolation.

(3) Before commanding polar coordinate interpolation, set the workpiece coordinate system so that the

center of the rotary axis is at the coordinate system zero point. Do not change the coordinate system

during the polar coordinate interpolation mode. (G50, G52, G53, relative coordinate reset, G54 to G59,

etc.)

(4) The feedrate during polar coordinate interpolation will be the interpolation speed on the polar coordinate

interpolation plane (orthogonal coordinate system).

(The relative speed with the tool will vary according to the polar coordinate conversion.)

When passing near the center of the rotary axis on the polar coordinate interpolation plane (orthogonal

coordinate system), the rotary axis side feedrate after polar coordinate interpolation will be very high.

(5) The axis movement command outside of the plane during polar coordinate interpolation will move

unrelated to the polar coordinate interpolation.

(6) The current position displays during polar coordinate interpolation will all indicate the actual coordinate

value. However, the «remaining movement amount» indicates the movement amount on the polar

coordinate input plane.

(7) The polar coordinate interpolation mode is canceled when the power is turned ON or reset.

(8) A program error (P484) will occur if any axis commanded during polar coordinate interpolation has not

completed the reference position return.

(9) Tool radius compensation must be canceled before canceling the polar coordinate interpolation mode.

(10) When the polar coordinate interpolation mode is canceled and switched to the cutting mode, the plane

selected before the polar coordinate interpolation will be restored.

(11) A program error (P486) will occur if the polar coordinate interpolation command is issued during the

mirror 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.

(13) During polar coordinate interpolation, if X axis moveable range is controlled in the plus side, X axis has to

be moved to the plus area that includes «0» and above before issuing the polar coordinate interpolation

command. If X axis moveable range is controlled in the minus side, X axis has to be moved to the minus

area that does not include «0» before issuing the polar coordinate interpolation command.

G code Details

G00 Positioning

G01 Linear interpolation

G02 Circular interpolation (CW)

G03 Circular interpolation (CWW)

G04 Dwell

G09 Exact stop check

G40-42 Tool radius compensation

G61 Exact stop mode

G64 Cutting mode

G65 Macro call (simple call)

G66 Macro modal call (modal call)

G66.1 Macro modal call (block call per macro)

G67 Macro modal call cancel (modal call cancel)

G80-89 Fixed cycle for drilling

G90/91 Absolute/incremental value command

G94 Asynchronous feed

G98 Hole drilling cycle initial return

G99 Hole drilling cycle R point return

6 Interpolation Functions

MITSUBISHI CNC

86

6.11 Exponential Interpolation ; G02.3,G03.3

Function and purpose

Exponential function interpolation changes the rotary axis into an exponential function shape in respect to the

linear axis movement.

At this time, the other axes carry out linear interpolation between the linear axis.

This allows a machining of a taper groove with constant torsion angle (helix angle) (uniform helix machining of

taper shape).

This function can be used for slotting or grinding a tool for use in an end mill, etc.

— Uniform helix machining of taper shape

— Relation of linear axis and rotary axis

Torsion angle : J1 = J2 = J3

A : A axis (rotary axis)

X : X axis (linear axis)

A : A axis (rotary axis)

X : X axis (linear axis)

* : {B, C… constant}

J1 J2 J3

(G02.3/G03.3)

(G00)

(G01) (G01)

A

Z

X

X=B(eCA-1)

A

X *

M700V/M70V Series Programming Manual (M2/M0 Format)

6.11 Exponential Interpolation ; G02.3,G03.3

87

Command format

(Note 1) Designate the end point of the linear axis specified by parameter «#1514 expLinax» and the axis that

carries out linear interpolation between that axis.

If the end point on of the rotary axis designated with parameter «#1515 expRotax» is specified,

linear interpolation without exponential function interpolation will take place.

(Note 2) The command unit is as follows.

The command range is -89 to +89.

A program error (P33) will occur if there is no address I or J command.

A program error (P35) will occur if the address I or J command value is 0.

(Note 3) The command unit is as follows.

The command range is a positive value that does not include 0.

A program error (P33) will occur if there is no address R command.

A program error (P35) will occur if the address R command value is 0.

(Note 4) The command unit and command range is the same as the normal F code. (Command as per

minute feed. )

Command the composite feedrate that includes the rotary axis.

The normal F modal value will not change by the address F command.

A program error (P33) will occur if there is no address F command.

A program error (P35) will occur if the address F command value is 0.

(Note 5) The command unit is as follows.

The command unit and command range is the same as the normal F code.

Command the composite feedrate that includes the rotary axis.

The normal F modal value will not change by the address Q command.

The axis will interpolate between the initial speed (F) and end speed (Q) in the CNC according to

the linear axis.

If there is no address Q command, interpolation will take place with the same value as the initial

feedrate (address F command). (The start point and end point feedrates will be the same.)

A program error (P35) will occur if the address Q command value is 0.

G02.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ; … Forward rotation interpolation (modal)

G03.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ; … Negative rotation interpolation (modal)

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 feedrate (Note 4)

Q Feedrate at end point (Note 5)

K Command will be ignored.

Setting unit #1003 = B #1003 = C #1003 = D #1003 = E

(Unit = ) 0.001 0.0001 0.00001 0.000001

Setting unit #1003 = B #1003 = C #1003 = D #1003 = E Unit

Metric system 0.001 0.0001 0.00001 0.000001 mm

Inch system 0.0001 0.00001 0.000001 0.0000001 inch

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

6 Interpolation Functions

MITSUBISHI CNC

88

— Example of uniform helix machining of taper shape

Detailed description

Relational expression of exponential function

The exponential function relational expression of the linear axis (X) and rotary axis (A) in the G02.3/G03.3

command is defined in the following manner.

X() = r1 * (e/D — 1) / tan(i1) …(linear axis (X) movement (1))

A() = (-1) * 360 * / (2) …(rotary axis (A) movement)

However,

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 rotary axis’ start point

The rotary axis’ rotation angle () is as follows according to expression (1).

= D * 1n(X * tan(i1) / r1) + 1

A : A axis (rotary axis)

X : X axis (linear axis)

x0 : linear axis start point

i1

j1 x1x0

r1

ZZ

A X

M700V/M70V Series Programming Manual (M2/M0 Format)

6.11 Exponential Interpolation ; G02.3,G03.3

89

Machining example

— Uniform helix machining of taper shape

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 with linear axis (X axis))

X() : Absolute value from X axis (linear axis) start point

A() : Absolute value from A axis (rotary axis) start point

r1 : Exponential function interpolation constant value (address R command)

r2 : Workpiece left edge radius

x2 : X axis (linear axis) position at 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 feedrate (address F command)

q1 : Feedrate 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)

The taper gradient angle (i1) and torsion angle (j1) are set by the command address I and J, respectively.

Note that if the shape is a reverse taper shape, the taper gradient angle (i1) is issued as a negative value.

The torsion direction () is changed by the G code. (Forward rotation when G02.3 is commanded, negative

rotation when G03.3 is commanded)

The above settings allow uniform helix machining of a taper shape (or reverse taper shape).

i1

j1 x1x0 x2

p1

r1r2

z1

z2 z0 A

X