MITSUBISHI M80, M800 Programming Manual

Page 1

Page 2

Introduction

This manual is a guide for using the MITSUBISHI CNC M800/M80 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

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

Some parameters can be used by end-users and some parameters are set by the MTB according to the specifications. Endusers may not be able to set or change some of the parameters described as "... can be set with the parameter #XXXX" in the main text. Confirm the specifications for your machine with the manual issued by the MTB.

CAUTION

For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by the machine tool builder 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 M800/M80 Series Instruction Manual ............ IB-1501274

(2) Refer to the following documents for details on programming

MITSUBISHI CNC M800/M80 Series Programming Manual

Lathe System (1/2) .................................... IB-1501275

Lathe System (2/2) .................................... IB-1501276

Machining Center System (1/2) ................. IB-1501277

Machining Center System (2/2) ................. IB-1501278

Page 3

Page 4

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".

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. Note that even items ranked as " CAUTION", may lead to major results depending on the situation. In any case, important in-

formation that must always be observed is described. The following sings indicate prohibition and compulsory.

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".

The meaning of each pictorial sing is as follows.

CAUTION

Prohibited

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.

CAUTION

rotated object

Disassembly is

prohibited

CAUTION HOT

KEEP FIRE AWAY

For Safe Use

Danger

Electric shock risk

General instruction

Danger

explosive

Earth ground

DANGER

Not applicable in this manual.

Page 5

WARNING

1. Items related to operation

If the operation start position is set in a block which is in the middle of the program and the program is started, the program before the set block is not executed. Please confirm that G and F modal and coordinate values are appropriate. If there are coordinate system shift commands or M, S, T and B commands before the block set as the start position, carry out the required commands using the MDI, etc. If the program is run from the set block without carrying out these operations, there is a danger of interference with the machine or of machine operation at an unexpected speed, which may result in breakage of tools or machine tool or may cause damage to the operators.

Under the constant surface speed control (during G96 modal), if the axis targeted for the constant surface speed control (normally X axis for a lathe) moves toward the spindle center, the spindle rotation speed will increase and may exceed the allowable speed of the workpiece or chuck, etc. In this case, the workpiece, etc. may jump out during machining, which may result in breakage of tools or machine tool or may cause damage to the operators.

CAUTION

1. Items related to product and manual

For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by the machine tool

builder takes precedence over this manual.

Items not described in this manual must be interpreted as "not possible".

This manual is written on the assumption that all option functions are added. Refer to the specifications issued by the ma-

chine 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 pos-

sible. 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 offset amount, workpiece compensation amount and etc.

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

next block.

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

If the tool offset amount is changed during automatic operation (including during single block stop), it will be validated from

the next block or blocks onwards.

Do not make the synchronized spindle rotation command OFF with one workpiece chucked by the reference spindle and synchronized spindle during the spindle synchronization. Failure to observe this may cause the synchronized spindle stop, and hazardous situation.

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.

Page 6

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 endusers 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!

Page 7

Page 8

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. SD logo and SDHC logo are either registered trademarks or trademarks of LLC. UNIX is a registered trademark of The Open Group in the United States and/or other countries. Intel® and Pentium® are either trademarks or registered trademarks of Intel Corporation in the United States and/or other countries. MODBUS® is either trademark or registered trademark of Schneider Electric USA, Inc. or the affiliated companies in Japan and/or other countries.

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

Page 9

Page 10

本製品の取扱いについて

( 日本語 /Japanese) 本製品は工業用 ( クラス A) 電磁環境適合機器です。販売者あるいは使用者はこの点に注意し、住商業環境以外での使用をお願いいたします。

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.

본 제품의 취급에 대해서

( 한국어 /Korean) 이 기기는 업무용 (A 급 ) 전자파적합기기로서 판매자 또는 사용자는 이 점을 주의하시기 바라며 가정외의 지역에 서 사용하는 것을 목적으로 합니다 .

Page 11

Page 12

Chapter 1 - 14 : Refer to Programming Manual (Machining Center System) (1/2) Chapter 15 and later : Refer to Programming Manual (Machining Center System) (2/2)

1 Control Axes................................................................................................................................................. 1

1.1 Coordinate Words and Control Axes ........................................................................................................................ 2

1.2 Coordinate Systems and Coordinate Zero Point Symbols ....................................................................................... 3

2 Minimum Command Unit............................................................................................................................. 5

2.1 Input Setting Unit ...................................................................................................................................................... 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 .................................................................................................................. 25

4 Pre-read Buffer ........................................................................................................................................... 27

4.1 Pre-read Buffer ....................................................................................................................................................... 28

5 Position Commands .................................................................................................................................. 29

5.1 Position Command Methods ; G90,G91 ................................................................................................................. 30

5.2 Inch/Metric Conversion ; G20,G21 ......................................................................................................................... 32

5.3 Decimal Point Input................................................................................................................................................. 34

6 Interpolation Functions ............................................................................................................................. 39

6.1 Positioning (Rapid Traverse) ; G00 ....................................................................................................................... 40

6.2 Linear Interpolation ; G01 ....................................................................................................................................... 43

6.3 Circular Interpolation ; G02,G03............................................................................................................................ 45

6.4 R Specification Circular Interpolation ; G02,G03.................................................................................................... 50

6.5 Plane Selection ; G17,G18,G19 ............................................................................................................................. 52

6.6 Thread Cutting ........................................................................................................................................................ 54

6.6.1 Constant Lead Thread Cutting ; G33 ............................................................................................................. 54

6.6.2 Inch Thread Cutting ; G33............................................................................................................................. 58

6.7 Helical Interpolation ; G17,G18,G19 and G02,G03 ................................................................................................ 60

6.8 Unidirectional Positioning ....................................................................................................................................... 66

6.8.1 Unidirectional Positioning ; G60..................................................................................................................... 66

6.8.2 Axis-based Unidirectional Positioning ............................................................................................................ 68

6.9 Cylindrical Interpolation ; G07.1.............................................................................................................................. 69

6.10 Circular Cutting ; G12,G13 ................................................................................................................................... 76

6.11 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113................................................................................... 78

6.12 Exponential Interpolation ; G02.3,G03.3............................................................................................................... 85

6.13 Polar Coordinate Command ; G16 ....................................................................................................................... 91

6.14 Spiral/Conical Interpolation ; G02.1/G03.1(Type1), G02/G03(Type2).................................................................. 98

6.15 3-dimensional Circular Interpolation ; G02.4,G03.4............................................................................................ 103

6.16 NURBS Interpolation ; G06.2.............................................................................................................................. 108

6.17 Hypothetical Axis Interpolation ; G07.................................................................................................................. 114

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

7.1 Rapid Traverse Rate............................................................................................................................................. 118

7.1.1 Rapid Traverse Rate.................................................................................................................................... 118

7.1.2 G00 Feedrate Command (,F Command) ..................................................................................................... 119

7.2 Cutting Feed Rate................................................................................................................................................. 123

7.3 F1-digit Feed......................................................................................................................................................... 124

7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed) ; G94,G95 ............................. 127

Page 13

7.5 Inverse Time Feed ; G93...................................................................................................................................... 130

7.6 Feedrate Designation and Effects on Control Axes.............................................................................................. 135

7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration........................................................................... 139

7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration .......................................................... 144

7.9 Cutting Feed Constant Inclination Acceleration/Deceleration............................................................................... 152

7.10 Exact Stop Check ; G09 ..................................................................................................................................... 158

7.11 Exact Stop Check Mode ; G61 ........................................................................................................................... 162

7.12 Deceleration Check ............................................................................................................................................ 163

7.12.1 Deceleration Check.................................................................................................................................... 163

7.12.2 Deceleration Check when Movement in The Opposite Direction Is Reversed........................................... 171

7.13 Rapid Traverse Block Overlap; G0.5 P1............................................................................................................. 173

7.13.1 Rapid Traverse Block Overlap for G00; G0.5 ............................................................................................ 175

7.13.2 Rapid Traverse Block Overlap for G28 ...................................................................................................... 183

7.14 Automatic Corner Override ................................................................................................................................. 185

7.14.1 Automatic Corner Override ; G62............................................................................................................... 191

7.14.2 Inner Arc Override...................................................................................................................................... 192

7.15 Tapping Mode ; G63 ........................................................................................................................................... 193

7.16 Cutting Mode ; G64............................................................................................................................................ 194

8 Dwell.......................................................................................................................................................... 195

8.1 Dwell (Time Designation) ; G04............................................................................................................................ 196

9 Miscellaneous Functions ........................................................................................................................ 199

9.1 Miscellaneous Functions (M8-digits) .................................................................................................................... 200

9.2 Secondary Miscellaneous Functions (A8-digits, B8-digits or C8-digits) ............................................................... 202

9.3 Index Table Indexing ............................................................................................................................................ 203

10 Spindle Functions .................................................................................................................................. 205

10.1 Spindle Functions ............................................................................................................................................... 206

10.2 Constant Surface Speed Control ; G96,G97 ...................................................................................................... 207

10.3 Spindle Clamp Speed Setting ; G92 ................................................................................................................... 213

10.4 Spindle Position Control (Spindle/C Axis Control) .............................................................................................. 215

11 Tool Functions (T command)................................................................................................................ 225

11.1 Tool Functions (T8-digit BCD) ............................................................................................................................ 226

12 Tool Compensation Functions ............................................................................................................. 227

12.1 Tool Compensation............................................................................................................................................. 228

12.1.1 Tool Compensation .................................................................................................................................... 228

12.1.2 Number of Tool Offset Sets Allocation to Part Systems............................................................................. 232

12.2 Tool Length Compensation/Cancel ; G43,G44/G49 ........................................................................................... 234

12.3 Tool Length Compensation in The Tool Axis Direction ; G43.1/G49 .................................................................. 238

12.4 Tool Radius Compensation ; G38,G39/G40/G41,G42 ....................................................................................... 245

12.4.1 Tool Radius Compensation Operation ....................................................................................................... 246

12.4.2 Other Commands and Operations during Tool Radius Compensation...................................................... 255

12.4.3 G41/G42 Commands and I, J, K Designation............................................................................................ 265

12.4.4 Interrupts during Tool Radius Compensation............................................................................................. 271

12.4.5 General Precautions for Tool Radius Compensation................................................................................. 273

12.4.6 Changing of Compensation No. during Compensation Mode ....................................................................274

12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation .............................................................. 277

12.4.8 Interference Check..................................................................................................................................... 279

12.4.9 Diameter Designation of Compensation Amount ....................................................................................... 289

12.4.10 Workpiece Coordinate Changing during Radius Compensation.............................................................. 291

12.5 3-dimensional Tool Radius Compensation ; G40/G41,G42................................................................................ 293

12.6 Tool Position Offset ; G45 to G48....................................................................................................................... 304

13 Fixed Cycle ............................................................................................................................................. 313

13.1 Fixed Cycles ....................................................................................................................................................... 314

13.1.1 Drilling, Spot Drilling ; G81 ......................................................................................................................... 318

13.1.2 Drilling, Counter Boring ; G82 .................................................................................................................... 319

13.1.3 Deep Hole Drilling Cycle ; G83 .................................................................................................................. 320

13.1.3.1 Deep Hole Drilling Cycle ................................................................................................................... 320

13.1.3.2 Small Diameter Deep Hole Drilling Cycle.......................................................................................... 322

13.1.4 Tapping Cycle ; G84 .................................................................................................................................. 325

13.1.5 Boring ; G85............................................................................................................................................... 337

Page 14

13.1.6 Boring ; G86............................................................................................................................................... 338

13.1.7 Back Boring ; G87......................................................................................................................................339

13.1.8 Boring ; G88............................................................................................................................................... 341

13.1.9 Boring ; G89............................................................................................................................................... 342

13.1.10 Stepping Cycle ; G73........................................ .................................. ... .. .................... ............................343

13.1.11 Reverse Tapping Cycle ; G74..................................................................................................................345

13.1.12 Circular Cutting ; G75............................................................................................................................... 347

13.1.13 Fine Boring ; G76..................................................................................................................................... 349

13.1.14 Precautions for Using a Fixed Cycle........................................................................................................351

13.1.15 Initial Point and R Point Level Return ; G98,G99.....................................................................................353

13.1.16 Setting of Workpiece Coordinates in Fixed Cycle Mode................................ .................................. ........ 354

13.1.17 Drilling Cycle High-Speed Retract............................................................................................................ 355

13.1.18 Acceleration/Deceleration Mode Change in Hole Drilling Cycle .............................................................. 359

13.2 Special Fixed Cycle............................................................................................................................................ 361

13.2.1 Bolt Hole Cycle ; G34.................................................................................................................................362

13.2.2 Line at Angle ; G35 .................................................................................................................................... 363

13.2.3 Arc ; G36.................................................................................................................................................... 364

13.2.4 Grid ; G37.1................................................................................................................................................365

14 Macro Functions .................................................................................................................................... 367

14.1 Subprogram Control; M98, M99, M198 ..............................................................................................................368

14.1.1 Subprogram Call ; M98,M99.....................................................................................................................368

14.1.2 Subprogram Call ; M198...........................................................................................................................374

14.1.3 Figure Rotation ; M98 I_J_K_ ....................................................................................................................375

14.2 Variable Commands........................................................................................................................................... 378

14.3 User Macro.........................................................................................................................................................382

14.4 Macro Call Instruction.........................................................................................................................................383

14.4.1 Simple Macro Calls ; G65 ............................... ..................................... .....................................................383

14.4.2 Modal Call A (Movement Command Call) ; G66.......................................................................................387

14.4.3 Modal Call B (for Each Block) ; G66.1 ...................................................................................................... 389

14.4.4 G Code Macro Call.....................................................................................................................................391

14.4.5 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call).................................................... 392

14.4.6 Detailed Description for Macro Call Instruction..........................................................................................394

14.4.7 ASCII Code Macro..................................................................................................................................... 396

14.5 Variables Used in User Macros..........................................................................................................................400

14.5.1 Common Variables..................................................................................................................................... 402

14.5.2 Local Variables (#1 to #33)........................................................................................................................403

14.5.3 System Variable......................................................................................................................................... 406

14.6 User Macro Commands...................................................................................................................................... 407

14.6.1 Operation Commands................................................................................................................................407

14.6.2 Control Commands.................................................................................................................................... 412

14.6.3 External Output Commands ; POPEN, PCLOS, DPRNT..........................................................................415

14.6.4 Precautions................................................................................................................................................419

14.6.5 Actual Examples of Using User Macros..................................................................................................... 421

14.7 Macro Interruption; M96, M97.............................................................................................................................425

15 Program Support Functions ................................................................................................................. 435

15.1 Corner Chamfering I /Corner Rounding I............................................................................................................ 436

15.1.1 Corner Chamfering I ; G01 X_ Y_ ,C .................................................................. ... .................................... 436

15.1.2 Corner Rounding I ; G01 X_ Y_ ,R_........................................................................................................... 438

15.1.3 Corner Chamfering Expansion/Corner Rounding Expansion..................................................................... 440

15.1.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ..................................................... 442

15.2 Corner Chamfering II /Corner Rounding II..........................................................................................................443

15.2.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_.......................................................................................443

15.2.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_.......................................................................................... 445

15.2.3 Corner Chamfering Expansion/Corner Rounding Expansion..................................................................... 446

15.2.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ..................................................... 446

15.3 Linear Angle Command ; G01 X_/Y_ A_/,A_......................................................................................................447

15.4 Geometric ; G01 A_............................................................................................................................................ 448

15.5 Geometric IB....................................................................................................................................................... 450

15.5.1 Geometric IB (Automatic calculation of two-arc contact) ; G02/G03 P_Q_ /R_........................................451

15.5.2 Geometric IB (Automatic calculation of linear - arc intersection) ; G01 A_ , G02/G03 P_Q_H_................ 453

15.5.3 Geometric IB (Automatic calculation of linear - arc intersection) ; G01 A_ , G02/G03 R_H_ ................... 456

15.6 G Command Mirror Image ; G50.1,G51.1 .......................................................................................................... 458

15.7 Normal Line Control ; G40.1/G41.1/G42.1 (G150/G151/G152)..........................................................................462

15.8 Manual Arbitrary Reverse Run Prohibition ; G127.............................................................................................. 481

Page 15

15.9 Data Input by Program........................................................................................................................................ 487

15.9.1 Parameter Input by Program ; G10 L70/L100, G11 ................................................................................... 487

15.9.2 Compensation Data Input by Program ; G10 L2/L10/L11, G11 .................................................................490

15.9.3 Tool Shape Input by Program ; G10 L100, G11......................................................................................... 496

15.9.4 R-Navi Data Input by Program ; G10 L110, G11 ....................................................................................... 499

15.10 Inputting The Tool Life Management Data ; G10,G11...................................................................................... 503

15.10.1 Inputting The Tool Life Management Data by G10 L3 Command ; G10 L3,G11 ..................................... 503

15.10.2 Inputting The Tool Life Management Data by G10 L30 Command ; G10 L30,G11 ................................. 506

15.10.3 Precautions for Inputting The Tool Life Management Data...................................................................... 509

15.10.4 Tool Life Management Set Allocation to Part Systems............................................................................ 510

16 Multi-part System Control ..................................................................................................................... 513

16.1 Timing Synchronization ...................................................................................................................................... 514

16.1.1 Timing Synchronization Operation (! code) !n (!m ...) L ............................................................................. 514

16.1.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115 ...................................... 517

16.1.3 Timing Synchronization Operation with Start Point Designated (Type 2) ; G116 ...................................... 520

16.1.4 Timing Synchronization Operation Function Using M codes ; M*** ...........................................................523

16.1.5 Time Synchronization when Timing Synchronization Ignore Is Set ...........................................................527

16.2 Sub Part System Control .................................................................................................................................... 530

16.2.1 Sub Part System Control I ; G122............................................................................................................. 530

17 High-speed High-accuracy Control ...................................................................................................... 545

17.1 High-speed Machining Mode .............................................................................................................................. 546

17.1.1 High-speed Machining Mode I, II ; G05 P1, G05 P2 .................................................................................. 546

17.2 High-accuracy Control ........................................................................................................................................ 554

17.2.1 High-accuracy Control ; G61.1,G08 ........................................................................................................... 554

17.2.2 SSS Control ............................................................................................................................................... 572

17.2.3 Tolerance Control....................................................................................................................................... 576

17.2.4 Variable-acceleration Pre-interpolation Acceleration/Deceleration ............................................................ 580

17.2.5 Initial High-accuracy Control ...................................................................................................................... 583

17.2.6 Multi-part System Simultaneous High-accuracy ........................................................................................ 584

17.3 High-speed High-accuracy Control ..................................................................................................................... 586

17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0.................. 586

17.3.2 Fairing ........................................................................................................................................................ 602

17.3.3 Smooth Fairing........................................................................................................................................... 603

17.3.4 Acceleration Clamp Speed......................................................................................................................... 612

17.3.5 High-speed Mode Corner Deceleration...................................................................................................... 613

17.3.6 Precautions on High-speed High-accuracy Control ................................................................................... 614

17.4 Spline Interpolation ; G05.1 Q2/Q0..................................................................................................................... 617

17.5 Spline Interpolation 2; G61.4 .............................................................................................................................. 626

17.6 High-accuracy Spline Interpolation ; G61.2 ........................................................................................................ 633

17.7 Machining Condition Selection I ; G120.1,G121................................................................................................. 635

18 Advanced Machining Control ............................................................................................................... 639

18.1 Inclined Surface Machining ; G68.2, G68.3 ........................................................................................................ 640

18.1.1 How to Define Feature Coordinate System Using Euler Angles ................................................................ 642

18.1.2 How to Define Feature Coordinate System Using Roll-Pitch-Yaw Angles................................................. 644

18.1.3 How to Define Feature Coordinate System Using Three Points in a Plane ............................................... 646

18.1.4 How to Define Feature Coordinate System Using Two Vectors ................................................................648

18.1.5 How to Define Feature Coordinate System Using Projection Angles ........................................................ 650

18.1.6 Define by Selecting The Registered Machining Surface............................................................................ 652

18.1.7 How to Define Feature Coordinate System Using Tool Axis Direction ...................................................... 653

18.1.8 Tool Axis Direction Control; G53.1/G53.6.................................................................................................. 654

18.1.9 Details of Inclined Surface Machining Operation ....................................................................................... 660

18.1.10 Rotary Axis Basic Position Selection ....................................................................................................... 664

18.1.11 Relationship with Other Functions ........................................................................................................... 670

18.1.12 Precautions .............................................................................................................................................. 673

19 Coordinate System Setting Functions ................................................................................................. 677

19.1 Coordinate Words and Control Axes .................................................................................................................. 678

19.2 Types of Coordinate Systems............................................................................................................................. 679

19.2.1 Basic Machine, Workpiece and Local Coordinate Systems....................................................................... 679

19.2.2 Machine Zero Point and 2nd, 3rd, 4th Reference Position (Zero Point) .................................................... 680

19.2.3 Automatic Coordinate System Setting ....................................................................................................... 681

19.2.4 Coordinate System for Rotary Axis............................................................................................................ 682

Page 16

19.3 Basic Machine Coordinate System Selection ; G53 ........................................................................................... 685

19.4 Coordinate System Setting ; G92 ....................................................................................................................... 688

19.5 Local Coordinate System Setting ; G52............................................................................................................. 690

19.6 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1)........................................................... 694

19.7 Workpiece Coordinate System Preset ; G92.1.................................................................................................. 704

19.8 3-dimensional Coordinate Conversion ; G68/G69 .............................................................................................. 709

19.9 Coordinate Rotation by Program ; G68/G69....................................................................................................... 727

19.10 Coordinate Rotation Input by Parameter ; G10 I_ J_/K_ .................................................................................. 734

19.11 Scaling ; G50/G51 ............................................................................................................................................ 747

19.12 Reference Position (Zero Point) Return ; G28,G29 .......................................................................................... 751

19.13 2nd, 3rd, and 4th Reference Position (Zero Point) Return ; G30...................................................................... 755

19.14 Tool Change Position Return ; G30.1 - G30.6.................................................................................................. 758

19.15 Reference Position Check ; G27 ...................................................................................................................... 761

20 Protection Function ............................................................................................................................... 763

20.1 Stroke Check before Travel ; G22/G23 .............................................................................................................. 764

21 Measurement Support Functions ......................................................................................................... 767

21.1 Automatic Tool Length Measurement ; G37 ....................................................................................................... 768

21.2 Skip Function ; G31 ........................................................................................................................................... 772

21.3 Multi-step Skip Function 1 ; G31.n, G04............................................................................................................ 777

21.4 Multi-step Skip Function 2 ; G31 P .................................................................................................................... 779

21.5 Speed Change Skip ; G31 Fn............................................................................................................................ 781

21.6 Torque Limitation Skip ; G160 ............................................................................................................................ 785

21.7 Programmable Current Limitation ; G10 L14 ; .................................................................................................... 789

Appendix1 Fixed Cycles............................................................................................................................. 791

Page 17

Page 18

435

IB-1501278-B

Program Support Functions

Page 19

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

15 Program Support Functions

15Program Support Functions

15.1 Corner Chamfering I /Corner Rounding I

Function and purpose

Chamfering at any angle or corner rounding is performed automatically by adding ",C_" or ",R_" to the end of the block to be commanded first among those command blocks which shape the corner with lines only.

15.1.1 Corner Chamfering I ; G01 X_ Y_ ,C

Function and purpose

This chamfers a corner by connecting the both side of the hypothetical corner which would appear as if chamfering is not performed, by the amount commanded by ",C_".

Command format

N100 G01 X__ Y__ ,C__ ;

N200 G01 X__ Y__ ;

,C Length up to chamfering starting point or end point from hypothetical corner

Corner chamfering is performed at the point where N100 and N200 intersect.

Detailed description

(1) The start point of the block following the corner chamfering is the hypothetical corner intersection point.

(2) If there are multiple or duplicate corner chamfering commands in a same block, the last command will be valid.

(3) When both the corner chamfer and corner rounding commands exist in the same block, the latter command is

valid.

(4) Tool compensation is calculated for the shape which has already been subjected to corner chamfering.

(5) When the block following a command with corner chamfering does not contain a linear command, a corner cham-

fering/corner rounding II command will be executed.

(6) Program error (P383) will occur when the movement amount in the corner chamfering block is less than the

chamfering amount.

(7) Program error (P384) will occur when the movement amount in the block following the corner chamfering block

is less than the chamfering amount.

(8) Program error (P382) will occur when a movement command is not issued in the block following the corner cham-

fering I command.

IB-1501278-B

436

Page 20

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

15 Program Support Functions

Program example

X100.0

10.0

Y100.0

(1)

(2)

(a)

(b)

(c)

(1) G91 G01 X100. ,C10.; (2) X100. Y100.;

(a) Chamfering start point (b) Hypothetical corner intersection point (c) Chamfering end point

437

IB-1501278-B

Page 21

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

15 Program Support Functions

15.1.2 Corner Rounding I ; G01 X_ Y_ ,R_

Function and purpose

The hypothetical corner, which would exist if the corner were not to be rounded, is rounded with an arc that has a radius commanded by ",R_" only when configured of linear lines.

Command format

N100 G01 X__ Y__ ,R__ ;

N200 G01 X__ Y__ ;

,R Arc radius of corner rounding

Corner rounding is performed at the point where N100 and N200 intersect.

Detailed description

(1) The start point of the block following the corner rounding is the hypothetical corner intersection point.

(2) When both corner chamfering and corner rounding are commanded in the same block, the latter command will

be valid.

(3) Tool compensation is calculated for the shape which has already been subjected to corner rounding.

(4) When the block following a command with corner rounding does not contain a linear command, a corner cham-

fering/corner rounding II command will be executed.

(5) Program error (P383) will occur when the movement amount in the corner rounding block is less than the R value.

(6) Program error (P384) will occur when the movement amount in the block following the corner rounding block is

less than the R value.

(7) Program error (P382) will occur if a movement command is not issued in the block following the corner rounding.

IB-1501278-B

438

Page 22

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

15 Program Support Functions

Program example

X100.0

Y100.0

(1)

(2)

R10.0

(a)

(b)

(c)

(1) G91 G01 X100. ,R10.; (2) X100. Y100.;

(a) Corner rounding start point (b) Corner rounding end point (c) Hypothetical corner intersection point

439

IB-1501278-B

Page 23

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

15 Program Support Functions

15.1.3 Corner Chamfering Expansion/Corner Rounding Expansion

Function and purpose

Using an E command, the feedrate can be designated for the corner chamfering and corner rounding section. In this way, the corner section can be cut into a correct shape.

Example

F200.

E100.

(G94)

G01Y70.,C30. F200.E100.; X-110.;

F200.

E100.

(G94)

G01Y70.,R30. F200.E100.; X-110.;

F200.

IB-1501278-B

440

Page 24

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

15 Program Support Functions

Detailed description

(G94) G01Y30.,C10. F100.E50.; X-50.,C10.; Y50.,C10.; X-50.;

F100.

E50.

F100.

E50.

(G94)

G01Y30.,C10. F100.E50.; X-50.,C10.; Y50.,C10. E0; X-50.;

(G94)

G01Y30.,C10. F100.; X-50.,C10.; Y50.,C10. E50; X-50.;

(1) The E command is modal. It is also valid for the feed in the next corner chamfering/corner rounding section.

Example

(2) E command modal has separate asynchronous feedrate modal and synchronous feedrate modal functions.

Which one is validated depends on the asynchronous/synchronous mode (G94/G95).

(3) When the E command is 0, or when there has not been an E command up to now, the corner chamfering/corner

rounding section feedrate will be the same as the F command feedrate.

Example

(4) E command modal is not cleared even if the reset button is pressed.

It is cleared when the power is turned OFF. (In the same manner as F commands.)

(5) All E commands except those shown below are at the corner chamfering/corner rounding section feedrate.

- E commands during thread cutting modal

- E commands during thread cutting cycle modal

441

IB-1501278-B

Page 25

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

15 Program Support Functions

15.1.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding

Detailed description

(1) Shown below are the operations of manual interruption during corner chamfering or corner rounding.

With an absolute value command and manual absolute switch ON.

N1 G28 XY; N2 G00 X120.Y20. ; N3 G03 X70. Y70.I-50. ,R20. F100 ; N4 G01 X20. Y20. ;

140.

40.

20. 70.

With an incremental value command and manual absolute switch OFF

N1 G28 XY; N2 G00 X120. Y20. ; N3 G03 X-50. Y50. I-50. ,R20. F100 ; N4 G01 X-50. Y-50.;

140.

40.

20. 70.

120.

(mm)

Interrupt amount

Path in interrupt case

Path in non-interrupt case

(2)With a single block during corner chamfering or corner rounding, the tool stops after these operations are exe-

cuted.

IB-1501278-B

442

Page 26

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

15 Program Support Functions

15.2 Corner Chamfering II /Corner Rounding II

Function and purpose

Corner chamfering and corner rounding can be performed by adding ",C" or ",R" to the end of the block which is commanded first among the block that forms a corner with continuous arbitrary angle lines or arcs.

15.2.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_

Function and purpose

The corner is chamfered by commanding ",C" in the 1st block of the two continuous blocks containing an arc. For an arc, this will be the chord length.

Command format

N100 G03 X__ Y__ I__ J__ ,C__ ;

N200 G01 X__ Y__ ;

,C Length up to chamfering starting point or end point from hypothetical corner

Corner chamfering is performed at the point where N100 and N200 intersect.

Detailed description

(1) If this function is commanded while the corner chamfer or corner rounding command is not defined in the spec-

ifications, it causes a program error (P381).

(2) The start point of the block following the corner chamfering is the hypothetical corner intersection point.

(3) If there are multiple or duplicate corner chamfering commands in a same block, the last command will be valid.

(4) When both corner chamfering and corner rounding are commanded in the same block, the latter command will

be valid.

(5) Tool compensation is calculated for the shape which has already been subjected to corner chamfering.

(6) Program error (P385) will occur when positioning or thread cutting is commanded in the corner chamfering com-

mand block or in the next block.

(7) Program error (P382) will occur when the block following corner chamfering contains a G command other than

group 01 or another command.

(8) Program error (P383) will occur when the movement amount in the block, commanding corner chamfering, is

less than the chamfering amount.

(9) Program error (P384) will occur when the movement amount is less than the chamfering amount in the block

following the block commanding corner chamfering.

(10) Even if a diameter is commanded, it will be handled as a radial command value during corner chamfering.

(11) Program error (P382) will occur when a movement command is not issued in the block following the corner

chamfering II command.

443

IB-1501278-B

Page 27

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

15 Program Support Functions

Program example

(1) Linear - arc

Absolute value command N1 G28 XY; N2 G90 G00 X100. Y100.; N3 G01 X50.Y150.,C20. F100; N4 G02 X0 Y100. I-50. J0; : Relative value command N1 G28 XY; N2 G91 G00 X100. Y100.; N3 G01 X-50.Y50.,C20. F100; N4 G02 X-50. Y-50. I-50. J0; :

(2) Arc - arc

(a)

150.

C20.

100.

100.50.

(mm)

(a) Hypothetical corner intersection point

Absolute value command N1 G28 XY; N2 G91 G00 X140. Y10.; N3 G02 X60.Y50.I0 J100. ,C20. F100; N4 X0 Y30.I-60.J80.; : Relative value command N1 G28 XY; N2 G91 G00 X140. Y10.; N3 G02 X-80.Y40. R100. ,C20. F100; N4 X-60. Y-20. I-60. J80.; :

130.

110.

(a)

50.

C20.

30. N3

10.

(a) Hypothetical corner intersection point

140.60.

(mm)

IB-1501278-B

444

Page 28

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

15 Program Support Functions

15.2.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_

Function and purpose

The corner is rounded by commanding ",R_" in the 1st block of the two continuous blocks containing an arc.

Command format

N100 G03 X__ Y__ I__ J__ ,R__ ;

N200 G01 X__ Y__ ;

,R Arc radius of corner rounding

Corner rounding is performed at the point where N100 and N200 intersect.

Detailed description

(1) If this function is commanded while the corner chamfer or corner rounding command is not defined in the spec-

ifications, it causes a program error (P381).

(2) The start point of the block following the corner rounding is the hypothetical corner intersection point.

(3) When both corner chamfering and corner rounding are commanded in a same block, the latter command will be

valid.

(4) Tool compensation is calculated for the shape which has already been subjected to corner rounding.

(5) Program error (P385) will occur when positioning or thread cutting is commanded in the corner rounding com-

mand block or in the next block.

(6) Program error (P382) will occur when the block following corner rounding contains a G command other than

group 01 or another command.

(7) Program error (P383) will occur when the movement amount in the corner rounding block is less than the R value.

(8) Program error (P384) will occur when the movement amount is less than the R value in the block following the

corner rounding.

(9) Even if a diameter is commanded, it will be handled as a radial command value during corner rounding.

(10) A program error (P382) will occur if a movement command is not issued in the block following corner rounding.

445

IB-1501278-B

Page 29

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

15 Program Support Functions

Program example

80.

30.

100.50.

(a)

(mm)

R10.

80.

30.

100.50.

N4 N3

(a)

(mm)

R10.

(1) Linear - arc

Absolute value command N1 G28 XY; N2 G90 G00 X100. Y30.; N3 G01 X50.Y80.,R10. F100; N4 G02 X0 Y30. I-50.J0; : Relative value command N1 G28 XY; N2 G91 G00 X100. Y30.; N3 G01 X-50.Y50.,R10. F100; N4 G02 X-50. Y-50. I-50.J0; :

(2) Arc - arc

(a) Hypothetical corner intersection point

Absolute value command N1 G28 XY; N2 G90 G00 X100. Y30.; N3 G02 X50.Y80. R50.,R10.F100; N4 X0 Y30. R50.; : Relative value command N1 G28 XY; N2 G91 G00 X100. Y30.; N3 G02 X-50.Y50. I0 J50.,R10.F100; N4 X-50. Y-50. I-50. J0; :

(a) Hypothetical corner intersection point

15.2.3 Corner Chamfering Expansion/Corner Rounding Expansion

For details, refer to "Corner Chamfering I / Corner Rounding" and "Corner Chamfering Expansion / Corner Rounding Expansion".

15.2.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding

For details, refer to "Corner Chamfering I / Corner Rounding" and "Interrupt during Corner Chamfering Interrupt during / Corner Rounding".

IB-1501278-B

446

Page 30

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

15 Program Support Functions

15.3 Linear Angle Command ; G01 X_/Y_ A_/,A_

( x1,y1)

( x2,y2)

Function and purpose

The end point coordinates are automatically calculated by commanding the linear angle and one of the end point coordinate axes.

Command format

N1 G01 Xx1(Yy1) Aa1; N2 G01 Xx2(Yy2) A-a2; (A-a2 can also be set as Aa 3. )

N1 G01 Xx1(Yy1) ,Aa1; N2 G01 Xx2(Yy2) ,A-a2;

This designates the angle and the X or Y axis coordinates. Select the command plane with G17 to G19.

Detailed description

(1) As seen from the + direction of the horizontal axis of the selected plane, the counterclockwise (CCW) direction

is considered to be + and the clockwise direction (CW) -.

(2) Either of the axes on the selected plane is commanded for the end point.

(3) The angle is ignored when the angle and the coordinates of both axes are commanded.

(4) When only the angle has been commanded, this is treated as a geometric command.

(5) The angle of either the start point (a1) or end point (a2) may be used.

(6) This function is valid only for the G01 command; it is not valid for other interpolation or positioning commands.

(7) The range of slope "a" is between -360.000 and 360.000.

When a value outside this range is commanded, it will be divided by 360 (degrees) and the remainder will be commanded. (Example) If 400 is commanded, 40° (remainder of 400/360) will become the command angle.

(8) If an address A is used for the axis name or the 2nd miscellaneous function, use ",A" as the angle.

(9) If "A" and ",A" are commanded in a same block, ",A" will be interpreted as the angle.

(Note) A program error (P33) will occur if this function is commanded during the high-speed machining mode or high-

speed high-accuracy mode.

447

IB-1501278-B

Page 31

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

15 Program Support Functions

15.4 Geometric ; G01 A_

(x2,y2)

(C)

Function and purpose

When it is difficult to calculate the intersection point of two straight lines in a continuous linear interpolation command, the end point of the first straight line will be automatically calculated inside the CNC and the movement command will be controlled, provided that the slope of the first straight line as well as the end point coordinates and slope of the second straight line are commanded. (Note) If the parameter (#1082 Geomet) is set to 0, geometric I will not function.

Command format

N1 G01 Aa1 (A-a2) Ff1; N2 Xx2 Yy2 A-a4 (A-a3) Ff2;

Aa1, A-a2, A-a3, Aa4 Angle

Ff1, Ff2 Feedrate

Xx2, Yy2 Next block end point coordinates

Detailed description

(1) Program error (P396) will occur when the geometric command is not on the selected plane.

(2) As seen from the + direction of the horizontal axis of the selected plane, the counterclockwise (CCW) direction

is considered to be + and the clockwise direction (CW) -.

(3) The range of slope "a" is -360.000 ≤ a ≤ 360.000.

When a value outside this range is commanded, it will be divided by 360 (degrees) and the remainder will be commanded. (Example) If 400. is commanded, 40° (remainder of 400/360) will become the command angle.

(4) The slope of the line can be commanded on either the start or end point side. Whether the commanded slope is

on the start or end point side is identified automatically inside the NC unit.

(5) The end point coordinates of the second block should be commanded with absolute values. If incremental values

are used, program error (P393) will occur.

(6) The feedrate can be commanded for each block.

(7) When the angle where the two straight lines intersect is less than 1°, program error (P392) will occur.

(8) Program error (P396) will occur when the plane is changed in the 1st block and 2nd block.

(9) This function is ignored when address A is used for the axis name or as the 2nd miscellaneous function.

(10) Single block stop is possible at the end point of the 1st block.

(11) Program error (P394) will occur when the 1st and 2nd blocks do not contain the G01 or G33 command.

448

IB-1501278-B

Page 32

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

15 Program Support Functions

Relation with other functions

(x2,y2)

(x1,y1)

(x2,y2)

(x1,y1)

(x2,y2)

(x3,y3)

(x1,y1)

(x2,y2)

(x3,y3)

(x1,y1

)

(1) Corner chamfering and corner rounding can be commanded after the angle command in the 1st block.

(Example 1) N1 Aa1 ,Cc1 ; N2 Xx2 Yy2 Aa2 ;

(Example 2) N1 Aa1 ,Rr1 ; N2 Xx2 Yy2 Aa2 ;

(2) The geometric command I can be issued after the corner chamfering or corner rounding command.

(Example 3) N1 Xx2 Yy2 ,Cc1 ; N2 Aa1 ; N3 Xx3 Yy3 Aa2 ;

(3) The geometric command I can be issued after the linear angle command.

(Example 4) N1 Xx2 Aa1 ; N2 Aa2 ; N3 Xx3 Yy3 Aa3 ;

449

IB-1501278-B

Page 33

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

15 Program Support Functions

15.5 Geometric IB

Function and purpose

With the geometric IB function, the contact and intersection are calculated by commanding an arc center point or linear angle in the movement commands of two continuous blocks (only blocks with arc commands), instead of commanding the first block end point.

(Note) If the parameter (#1082 Geomet) is not set to 2, geometric IB will not function.

Two-arc contact

(??)

Linear - arc (arc - linear) intersection

Linear - arc (arc - linear) contact

(??)

IB-1501278-B

450

Page 34

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

15 Program Support Functions

15.5.1 Geometric IB (Automatic calculation of two-arc contact) ; G02/G03 P_Q_ /R_

Function and purpose

When the contact of two continuous contacting arcs is not indicated in the drawing, it can be automatically calculated by commanding the 1st circular center coordinate value or radius, and the 2nd arc end point absolute value and center coordinate value or radius.

Command format

N1 G02(G03) Pp1 Qq1 Ff1;

N2 G03(G02) Xx2 Yy2 Pp2 Qq2 Ff2;

N1 G02(G03) Pp1 Qq1 Ff1;

N2 G03(G02) Xx2 Yy2 Rr2 Ff2;

N1 G02(G03) Rr1 Ff1;

N2 G03(G02) Xx2 Yy2 Pp2 Qq2 Ff2;

P,Q X and Y axes circular center coordinate absolute value (diameter/radius value com-

mand)The center address for the 3rd axis is commanded with A.

R Arc radius (when a (-) sign is attached, the arc is judged to be 180° or more)

* I and J (X and Y axes arc center coordinate incremental value) commands can be issued instead of P and Q.

1st block arc : Incremental amount from the start point to the center

2nd block arc : Incremental amount from the end point to the center

(p1,q1)

(x2,y2)

(p2,q2)

451

IB-1501278-B

Page 35

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

15 Program Support Functions

Detailed description

Tool path

"Arc error"

(1) Program error (P393) will occur before the 1st block if the 2nd block is not a coordinate absolute value command.

(2) Program error (P398) will occur before the 1st block if there is no geometric IB specification.

(3) Program error (P395) will occur before the 1st block if there is no R (here, the 1st block is designated with P, Q

(I, J)) or P, Q (I, J) designation in the 2nd block.

(4) Program error (P396) will occur before the 1st block if another plane selection command (G17 to G19) is issued

in the 2nd block.

(5) Program error (P397) will occur before the 1st block if two arcs that do not contact are commanded.

(6) The contact calculation accuracy is ±1μm (fractions rounded up).

(7) Single block operation stops at the 1st block.

(8) When I or J is omitted, the values are regarded as I0 and J0. P and Q cannot be omitted.

(9) The error range in which the contact is obtained is set in parameter "#1084 RadErr".

(10) For an arc block perfect circle command (arc block start point = arc block end point), the R designation arc com-

mand finishes immediately, and there is no operation. Thus, use a PQ (IJ) designation arc command.

(11) G codes of the G modal group 1 in the 1st/2nd block can be omitted.

(12) Addresses being used as axis names cannot be used as command addresses for arc center coordinates or arc

radius.

(13) When the 2nd block arc inscribes the 1st block arc and the 2nd block is an R designation arc, the R+ sign be-

comes the inward turning arc command, and the R- sign becomes the outward turning arc command.

R-

R+

IB-1501278-B

452

Page 36

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

15 Program Support Functions

15.5.2 Geometric IB (Automatic calculation of linear - arc intersection) ; G01 A_ , G02/G03 P_Q_H_

H=1

H=0

-a4

-a2

(??)

(p2,q2)

(x2,y2)

(p1,q1)

(x2,y2)

Function and purpose

When the contact point of a shape in which contact between a line and an arc is not indicated in the drawing, it can be automatically calculated by commanding the following program.

Command format (For G18 plane)

N1 G01 Aa1 (A-a2) Ff1;

N2 G02(G03) Xx2 Yy2 Pp2 Qq2 Hh2 Ff2 ;

N1 G02(G03) Pp1 Qq1 Hh1 (,Hh1) Ff1 ;

N2 G1 Xx2 Yy2 Aa3 (A-a4) Ff2 ;

A Linear angle (-360.000° to 360.000°) P,Q X and Y axes circular center coordinate absolute value (diameter/radius value com-

mand)The center address for the 3rd axis is commanded with A.

H (,H) Selection of linear - arc intersection

0: Intersection of the shorter line 1: Intersection of the longer line

* I and J (X and Y axes arc center coordinate incremental value) commands can be issued instead of P and Q.

1st block arc : Incremental amount from the start point to the center

2nd block arc : Incremental amount from the end point to the center

453

IB-1501278-B

Page 37

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

15 Program Support Functions

Detailed description

Tool path

Arc error

N2 G2 Xx2 Yy2 Pp2 Qq2 Ff2 ;

N1 G1 A a1 Ff1;

N1 G1 A –a2 Ff1; N2 G2 Xx2 Yy2 Pp2 Qq2 Ff2 ;

(p2,q2)

-a2

(1) When the 2nd miscellaneous function address is A, the 2nd miscellaneous function is validated and this function

is invalidated.

(2) Program error (P393) will occur before the 1st block if the 2nd block is not a coordinate absolute value command.

(3) Program error (P398) will occur before the 1st block if there is no geometric IB specification.

(4) In case of the 2nd block arc, a program error (P395) will occur before the 1st block if there is no P, Q (I, J) des-

ignation. A program error (P395) will also occur if there is no A designation for the line.

(5) Program error (P396) will occur before the 1st block if another plane selection command (G17 to G19) is issued

in the 2nd block.

(6) Program error (P397) will occur before the 1st block if a straight line and arc that do not contact or intersect are

commanded.

(7) Single block operation stops at the 1st block.

(8) When I or J is omitted, the values are regarded as I0 and J0. P and Q cannot be omitted.

(9) When H is omitted, the value is regarded as H0.

(10) The linear - arc contact is automatically calculated by designating R instead of P, Q (I, J).

(11) The error range in which the intersect is obtained is set in parameter "#1084 RadErr".

(12) As seen from the + direction of the horizontal axis of the selected plane, the counterclockwise (CCW) direction

is considered to be + and the clockwise direction (CW) -.

(13) The slope of the line can be commanded on either the start or end point side. Whether designated slope is the

starting point or the end point will be automatically identified.

(14) When the distance to the intersection from the line and arc is same (as in the figure below), the control by ad-

dress H (short/long distance selection) is invalidated. In this case, the judgment is carried out based on the angle of the line.

(15) The intersect calculation accuracy is ±1μm (fractions rounded up).

(16) In linear - arc intersections, the arc command can only be PQ (IJ) command. When the arc block start point and

arc block end point are the same point, the arc is a perfect circle.

IB-1501278-B

454

Page 38

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

15 Program Support Functions

(17) G codes of the G modal group in the 1st block can be omitted.

(18) Addresses being used as axis names cannot be used as command addresses for angles, arc center coordi-

nates or intersection selections.

(19) When geometric IB is commanded, two blocks are pre-read.

Relationship with other functions

Command Tool path

Geometric IB + corner chamfering

N1 G02 P_ Q_ H_ ; N2 G01 X_ Y_ A_ ,C_ ; G01 X_ Y_ ;

455

IB-1501278-B

Page 39

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

15 Program Support Functions

15.5.3 Geometric IB (Automatic calculation of linear - arc intersection) ; G01 A_ , G02/G03 R_H_

Function and purpose

When the intersection of a shape in which a line and an arc intersect is not indicated in the drawing, it can be automatically calculated by commanding the following program.

Command format (For G18 plane)

N1 G01 Aa1 (A-a2) Ff1;

N2 G03(G02) Xx2 Yy2 Rr2 Ff2;

N1 G03(G02) Rr1 Ff1;

N2 G01 Xx2 Yy2 Aa3 (A-a4) Ff2 ;

A Linear angle (-360.000° to 360.000°) R Circular radius

(??)

-a4

(x2,y2)

(??)

-a2

(x2,y2)

Detailed description

(1) When the 2nd miscellaneous function address is A, the 2nd miscellaneous function is validated and this function

is invalidated.

(2) Program error (P393) will occur before the 1st block if the 2nd block is not a coordinate absolute value command.

(3) Program error (P398) will occur before the 1st block if there is no geometric IB specification.

(4) Program error (P396) will occur before the 1st block if another plane selection command (G17 to G19) is issued

in the 2nd block.

(5) A program error (P397) will occur before the 1st block if a straight line and arc that do not contact are command-

ed.

(6) In case of the 2nd block arc, a program error (P395) will occur before the 1st block if there is no R designation.

A program error (P395) will also occur if there is no A designation for the line.

(7) Single block operation stops at the 1st block.

(8) The linear - arc contact is automatically calculated by designating R instead of P, Q (I, J).

IB-1501278-B

456

Page 40

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

15 Program Support Functions

(9) The error range in which the contact is obtained is set in parameter "#1084 RadErr".

Tool path

Arc error

(10) The line slope is the angle to the positive (+) direction of its horizontal axis. Counterclockwise (CCW) is positive

(+). Clockwise (CW) is negative (-).

(11) The slope of the line can be commanded on either the start or end point side. Whether the commanded slope

is on the start or end point side is identified automatically inside the NC unit.

(12) The intersect calculation accuracy is ±1μm (fractions rounded up).

(13) In linear - arc contact, the arc command can only be an R command. Thus, when the arc block start point = arc

block end point, the arc command finishes immediately, and there will be no operation. (Perfect circle command is impossible.)

(14) G codes of the G modal group 1 in the 1st block can be omitted.

(15) Addresses being used as axis names cannot be used as command addresses for angles or arc radius.

(16) When geometric IB is commanded, two blocks are pre-read.

Relationship with other functions

Command Tool path

Geometric IB + corner chamfering

N1 G03 R_ ; N2 G01 X_ Y_ A_ ,C_ ; G01 X_ Y_ ;

Geometric IB + corner rounding

N1 G03 R_ ; N2 G01 X_ Y_ A_ ,R_ ; G01 X_ Y_ ;

457

IB-1501278-B

Page 41

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

15 Program Support Functions

15.6 G Command Mirror Image ; G50.1,G51.1

(A)

(B)

Function and purpose

When cutting a shape that is symmetrical on the left and right, programming time can be shortened by machining one side and then using the same program to machine the other side. The mirror image function is effective for this. For example, when using a program as shown below to machine the shape on the left side (A), a symmetrical shape (B) can be machined on the right side by applying mirror image and executing the program.

Mirror axis

Command format

Mirror image ON

G51.1 Xx1 Yy1 Zz1

x1, y1, z1 Mirror image center coordinates (Mirror image will be applied regarding this position

as a center)

Mirror image OFF

G50.1 Xx2 Yy2 Zz2

x2, y2, z2 Mirror image cancel axis (The values of x2, y2, z2 will be ignored.)

IB-1501278-B

458

Page 42

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

15 Program Support Functions

Detailed description

(1) At G51.1, command the mirror image axis and the coordinate to be a center of mirror image with the absolute

command or incremental command.

(2) At G50.1, command the axis for which mirror image is to be turned OFF. The values of x2, y2, and z2 will be

ignored.

(3) If mirror image is applied on only one axis of the designated plane, the rotation direction and compensation di-

rection will be reversed for the arc or tool radius compensation and coordinate rotation, etc.

(4) This function is processed on the local coordinate system, so the center of the mirror image will change when

the counter is preset or when the workpiece coordinates are changed.

(5) Reference position return during mirror image If the reference position return command (G28, G30) is executed

during the mirror image, the mirror image will be valid during the movement to the intermediate point, but will not be applied to the movement to the reference point after the intermediate point.

Path on which mirror is applied Mirror center Programmed path

Intermediate point when mirror is applied

Intermediate point

(6) Return from zero point during mirror image If the return command (G29) from the zero point is commanded during

the mirror image, the mirror will be applied to the intermediate point.

(7) The mirror image will not be applied to the G53 command.

459

IB-1501278-B

Page 43

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

15 Program Support Functions

Relationship with other functions

(1) Combination with radius compensation

The mirror image (G51.1) will be processed after the radius compensation (G41, G42) is applied, so the following type of cutting will take place.

Programmed path Path with mirror image applied

Program path

Path with only radius compensation applied

Path with only mirror image applied

Path with mirror image and radius compensation applied

IB-1501278-B

460

Page 44

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

15 Program Support Functions

Precautions

CAUTION

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

If mirror image is not canceled at the mirror center, the absolute value and machine position will deviate as shown below. (This state will last until an absolute value command (positioning with G90 mode) is issued, or a reference position return with G28 or G30 is executed.) The mirror center is set with an absolute value, so if the mirror center is commanded again in this state, the center may be set to an unpredictable position. Cancel the mirror at the mirror center or position with the absolute value command after canceling.

Absolute value (position commanded in program)

Machine position

When moved with the incremental command after mirror cancel

Mirror center

Mirror cancel command

Mirror axis command

461

IB-1501278-B

Page 45

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

15 Program Support Functions

15.7 Normal Line Control ; G40.1/G41.1/G42.1 (G150/G151/G152)

Function and purpose

The C axis (rotary axis) turning will be controlled so that the tool constantly faces the normal line direction in respect to the movement of the axes in the selected plane during program operation. At the block seams, the C axis turning is controlled so that the tool faces the normal line direction at the next block's start point.

C axis center (rotary axis)

Tool end position

C axis turning

During arc interpolation, the rotary axis turning is controlled in synchronization with the operation of the arc interpolation.

Rotation axis center (C axis)

Tool end position

The normal line control I and II can be used according to the C axis turning direction during normal line control. Which method is to be used depends on the MTB specifications (parameter "#1524 C_type").

Normal line control

type

Type I Direction that is 180° or

(#1524 C_type=0)

Type II As a principle, the command-

(#1524 C_type = 1)

Turning direction Turning speed Turning speed in arc inter-

polation

less(shortcut direction)

ed direction

Parameter speed(#1523 C_feed)

Feedrate Speed when the tool nose

Speed when the program path follows the F command

follows the F command

IB-1501278-B

462

Page 46

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

15 Program Support Functions

Command format

(a)

(b)

G40.1 (G150) X__ Y__ F__ ; ... Normal line control cancel

G41.1 (G151) X__ Y__ F__ ; ... Normal line control left ON

G42.1 (G152) X__ Y__ F__ ; ... Normal line control right ON

X X axis end point coordinate Y Y axis end point coordinate F Feedrate

G41.1 Normal line control left side G42.1 Normal line control right side

(a)

(b)

(a) Center of rotation (b) Tool end(b) Tool end

Program path

Tool end path

The normal line control axis depends on the MTB specifications (parameter #1522 C_axis). Normal line control is carried out in respect to the movement direction of the axis which is selecting the plane. G17 plane X-Y axes G18 plane Z-X axes G19 plane Y-Z axes Whether to cancel the normal line control at resetting depends on the MTB specifications (parameter "##1210 RstGmd/ bitE").

463

IB-1501278-B

Page 47

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

15 Program Support Functions

Detailed description

K+

I+

180

270

J+

K+

180

270

Definition of the normal line control angle

The normal line control angle is 0° (degree) when the tool is facing the horizontal axis (+ direction) direction. The counterclockwise direction turning is + (plus), and the clockwise direction turning is - (minus).

G17 plane (I - J axes) ... The axis angle is 0°(degree) when the tool is facing the +I direction.

J+

G18 plane (K - I axes) ...The axis angle is 0°(degree) when the tool is facing the +K direction.

G19 plane (J - K axes) ... The axis angle is 0°(degree) when the tool is facing the +J direction.

180

I+

270

IB-1501278-B

464

Page 48

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

15 Program Support Functions

Normal line control turning operation in respect to movement command

(x2,y2)

(x1,y1)

G41.1

(x2,y2)

(x1,y1)

G41.1

(1) Start up

After the normal line control axis turns to the right angle of the advance direction at the start point of the normal line control command block, the axis which is selecting the plane is moves. Note that the normal line control axis at the start up turns in the direction that is 180° or less (shortcut direction) in both the normal line control type I and II.

N1 G01 Xx1 Yy1 Ff1 ;

N2 G41.1 ; ... Independent block

N3 Xx2 Yy2 ;

N2 is fixed

N1 G01 Xx1 Yy1 Ff1 ;

N2 G41.1 Xx2 Yy2 ; ... Same block

(2) During normal line control mode

(a) Block seam

No tool radius compensation

With tool radius compensation

After the normal line control axis is turned to be at the right angle of the plane selecting movement in the next block, the operation moves to the next block.

Liner - Liner Liner - Arc Arc - Arc

Programmed path

Tool end path

If tool radius compensation is applied, normal line control is carried out along the path to which the tool radius compensation is applied.

Liner - Liner Liner - Arc Arc - Arc

Programmed path

Tool radius compensation path

Tool end path

465

IB-1501278-B

Page 49

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

15 Program Support Functions

(b) During block movement

(x2,y2)

(x1,y1)

G40.1

(x2,y2)

(x1,y1)

G40.1

The normal line control axis angle is kept unchanged during the linear command, and the normal line control axis does not turn. During the arc command, the normal line control axis turns in synchronization with the operation of the arc interpolation.

(3) Cancel

The normal line control axis will not turn, and the plane selecting axis will be moved by the program command.

N1 G01 Xx1 Yy1 Ff1 ;

N2 G40.1 ; ... Independent block

N3 Xx2 Yy2 ;

N2 is fixed

N1 G01 Xx1 Yy1 Ff1 ;

N2 G40.1 Xx2 Yy2 ; ... Same block

IB-1501278-B

466

Page 50

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

15 Program Support Functions

Normal line control temporary cancel

(a)

During normal line control, the turning operation for the normal line control axis is not carried out at the seam between a block and the next block, in which the movement amount is smaller than that set with the parameter (#1535 C_leng).

(1) For liner block;

When the movement amount of the N2 block is smaller than the parameter(#1535 C_leng), the normal line control axis is not turned at the seam between the N1 block and N2 block. It stays the same direction as the N1 block.

N2 block movement amount < Parameter(#1535 C_leng)

(2) For arc block;

When the diameter value of the N2 block is smaller than the parameter(#1535 C_leng), the normal line control axis is not turned at the seam between the N1 block and N2 block. It stays the same direction as the N1 block. During arc interpolation of the N2 block, the normal line control axis does not turn in synchronization with the operation of arc interpolation.

N2 block diameter value < Parameter (#1535 C_leng)

(a) Diameter value

(Note) Since operation fractions are created by calculating the intersection point of two segments, the turning oper-

ation may or may not be carried out when the parameter (#1535 C_leng) and the segment length are equal.

467

IB-1501278-B

Page 51

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

15 Program Support Functions

Normal line control axis turning direction at block seam

0180

270

(a)

(b)

(c)

The normal line control axis turning direction at block seam differs according to the normal line control type I or II. The turning angle is limited by the angle ε set with the parameter (#1521 C_min).

Item Normal line control type I Normal line control type II

Normal line control axis turning direction at block seam

Normal line control axis turning angle at block seam

Direction that is 180° or less. (shortcut direction)

When - | θ | < ε, turning is not performed. θ : Turning angle ε : Parameter (#1521 C_min)

- When the turning angle is 180°, the turning direction is indefinite regardless of the command mode.

[G41.1/G42.1 When the normal line control axis is at 0°]

G41.1 : - direction (CW) G42.1 : + direction (CCW)

When - | θ | < ε, turning is not performed. θ : Turning angle ε : Parameter (#1521 C_min) In the following cases, an operation error (0118) will occur. <For G41.1> ε <= θ < 180° - ε <For G42.1> 180° + ε < θ <= 360° - ε [G41.1 When the normal line control axis is at 0°]

180 -

(e)

0180

(d)

270

[G42.1 When the normal line control axis is at

(c)

(a) Normal line control axis turning (CCW)

0°]

(d)

(b) Normal line control axis turning (CW) (c) No turning

0180

180 +

(c)

(e)

270

IB-1501278-B

468

Page 52

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

15 Program Support Functions

(1) Normal line control type I

0180

270 (-90 )

0180

270 (- 90 )

Normal line control axis turning

angle at block seam: θ

1. -ε < θ <ε

G41.1 G42.1

2. ε <= θ < 180°

3. 180° <= θ <= 360°- ε

0180

360 -

No turning

Shortcut direction

No turning

Shortcut direction

270 (-90 )

469

IB-1501278-B

Page 53

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

15 Program Support Functions

(2)Normal line control type II

0180

270 (-90 )

0180

270 (-90 )

180 -

0180

270 (-90 )

180 +

360 -

0180

270 (-90 )

180 +

Normal line control axis turning

angle at block seam: θ

1. -ε < θ < ε

G41.1 G42.1

2. ε <= θ < 180°- ε

3. 180°-ε <= θ <= 180°+ ε

No turning

Operation error 0118 (Note)

No turning

4. 180°+ ε < θ <= 360°- ε

(Note)If the axis turns into the command direction, it turns inside the workpiece. Therefore, an operation error will

occur.

IB-1501278-B

470

Operation error 0118 (Note)

Page 54

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

15 Program Support Functions

Normal line control axis turning speed

Turning speed at block seam (select from type I or type II)

(1)Normal line control axis turning speed at block seam

(a) Rapid traverse

Normal line control type I Normal line control type II

- Dry run OFF The rapid traverse rate (#2001 rapid) is applied. Normal line control axis turning speed f = Rapid traverse rate * (Rapid traverse override) (° /min)

- Dry run ON The manual feedrate is applied. Normal line control axis turning speed f = Manual feedrate * (Cutting feed override) (° /min)

(Note 1) When the manual override valid is ON, the cutting feed override is valid.

(Note 2) If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be applied.

(Note 3) When the rapid traverse is ON, the dry run is invalid.

- Dry run OFF Normal line control axis turning speed f = F * 180 / (π * R) * (Rapid traverse override) (° /min) For R=0, the following expression is applied. Normal line control axis turning speed f = F * (Rapid traverse override) (° /min) F: Rapid traverse rate (#2001 rapid) (mm/min) R: Parameter (#8041 C-rot.R) (mm) (Length from normal line control axis center to tool nose) (Note 1) If the normal line control axis turning speed exceeds the rapid traverse rate (#2001 rapid), the rapid traverse rate will be applied.

- Dry run ON Normal line control axis turning speed f = F * 180 / (π * R) * (Cutting feed override) (° /min) For R=0, the following expression is applied. Normal line control axis turning speed f = F * (Cutting feed override) (° /min) F: Manual feedrate (mm/min) R: Parameter (#8041 C-rot.R) (mm) (Length from normal line control axis center to tool nose)

(Note 1) When the manual override valid is ON, the cutting feed override is valid.

(Note 2) If the normal line control axis turning speed exceeds the rapid traverse rate (#2001 rapid), the rapid traverse rate will be applied.

(Note 3) When the rapid traverse is ON, the dry run is invalid.

471

IB-1501278-B

Page 55

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

15 Program Support Functions

(b) Cutting feed

Normal line control type I Normal line control type II

- Dry run OFF The normal line control axis turning speed set with the parameter (#1523 C_feed) is applied. Normal line control axis turning speed f = Parameter (#1523 C_feed) * (Cutting feed override) (° /min)

- Dry run ON (Rapid traverse ON) The cutting feed clamp speed (#2002 clamp) is applied. Normal line control axis turning speed f = Cutting feed clamp speed (°/min)

- Dry run ON (Rapid traverse OFF) The manual feedrate is applied. Normal line control axis turning speed f = Manual feedrate * (Cutting feed override) (° /min)

(Note 1) When the manual override valid is ON, the cutting feed override is valid.

(Note 2) If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be applied.

The feedrate at the tool nose is the F command. The normal line control axis turning speed is the normal line control axis speed that follows this F command.

Normal line control axis turning speed f = F * 180 / (π * R) * (Cutting feed override) (° /min) For R=0, the following expression is applied. Normal line control axis turning speed f = F (° /min) F: Feedrate command (mm/min) R: Parameter (#8041 C-rot.R) (mm) (Length from normal line control axis center to tool nose)

(Note 1) If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be applied.

(Note 2) When the dry run is ON, the normal line control axis turning speed is obtained by the same expression as the rapid traverse.

(R)

(F)

(f)

Feedrate command f: Normal line control axis turning speed

=F*180/( *R)

(f)

F: Feedrate command f: Normal line control axis turning speed R: Parameter (#8041 C-rot.R)

IB-1501278-B

472

Page 56

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

15 Program Support Functions

(2)Normal line control axis turning speed during circular interpolation

=F*180/( *(R+r))

(F)

(R)

(r)

(f)

Normal line control type I Normal line control type II

The normal line control axis turning speed is the rotation speed obtained by feedrate F.

Normal line control axis turning speed f = F * 180 / (π * r) (° /min) F : Feed command speed (mm/min) r : Arc radius (mm)

(F)

The feedrate at the tool nose is the F command. The normal line control axis turning speed is the rotation speed that follows this F command.

Normal line control axis turning speed f = F * 180 / (π * (R + r)) (° /min) F : Feed command speed (mm/min) R : Parameter (#8041 C-rot. R) (mm) Length from normal line control axis center to tool nose r : Arc radius (mm)

(r)

(f)

=F*180/( *r)

(Note 1)If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the speed

will be as follows;

- Normal line control axis turning speed = Cutting feed clamp speed.

- Moving speed during arc interpolation = The speed according to the normal line control axis turning speed

473

IB-1501278-B

Page 57

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

15 Program Support Functions

Automatic corner arc insertion function

During normal line control, an arc is automatically inserted at the corner in the axis movement of the plane selection. This function is for the normal line control type I. The radius of the arc to be inserted is set with the parameter (#8042 C-ins.R). This parameter can be read and written using the macro variable #1901. Normal line control is performed also during the interpolation for the arc to be inserted.

Parameter (#8042 C-rot. R)

- The corner arc is not inserted in the following cases: linear and arc, arc and arc, linear and moveless or moveless and linear blocks or when a line is shorter than the radius of the arc to insert.

Corner R is not inserted.

- During the radius compensation, the radius compensation is applied to the path that the corner arc is inserted.

Radius compensation path

Parameter (#8042 C-rot. R)

IB-1501278-B

474

Page 58

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

15 Program Support Functions

- The stop point of the single block and block start interlock is as follows.

Stop point

- The stop point of the cutting start interlock is as follows.

Stop point

475

IB-1501278-B

Page 59

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

15 Program Support Functions

Program example

(0,0)

R10

R15

20.20.

Normal line control type I

Main program O500

G91X0Y0;G28C0; G90G92G53X0Y0; G00G54X25.Y-10.; G03G41.1X35.Y0.R10.F10.; #10=10; WHILE[#10NE0]DO1; M98P501; #10=#10-1; END1; G03X25.Y10.R10.; G40.1; G28X0Y0; M02;

Subprogram O501

G03X8.Y9.R15.; G02X-8.R10.; G03Y-9.R-15.; G02X8.R10.; G03X35.Y0.R15.; M99;

IB-1501278-B

476

Page 60

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

15 Program Support Functions

Normal line control type II

(b)

0.1

10.

(a)

20.

(0,0)

R10

20.

35. 35.

(Example 1)

Main program O500

G91X0Y0; G28 Z0; G28 C0; G90G92G53X0Y0Z0; G00G54G43X35.Y0.Z100.H 1; G00Z3.; G01Z0.1F6000; G42.1 ; M98P1001L510; M98P1002L2; G91G01Y10.Z0.05; G40.1 ; G90G00Z100.; G28X0Y0Z0; M02 ;

Subprogram O1001

G17G91G01Y20.,R10.Z-0.01; X-70.,R10.; Y-40.,R10.; X70.,R10.; Y20.; M99 ;

O1002

G17G91G01Y20.,R10.; X-70.,R10.; Y-40.,R10.; X70.,R10.; Y20.; M99 ;

(Corner chamfering/Corner R specifications are required)

(a) C-axis (b) Tool

477

IB-1501278-B

Page 61

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

15 Program Support Functions

(Example 2)

(b)

0.1

(a)

(0,0)

30. 30.

Main program O2000

G91G28Z0; G28X0Y0; G28 C0; G90G92G53X0Y0Z0; G00G54X30.Y0.; G00Z3.; G41.1G01Z0.1F5000; M98P2001L510; M98P2002L2; G91G01X-30.Z0.05; G40.1 ; G90G00Z100.; G28X0Y0Z0; M02 ;

Subprogram O2001

G17G91G01X-60.Z-0.01; X60.; M99 ;

O2002

G17G91G01X-60.; X60.; M99 ;

(a) C-axis (b) Tool

IB-1501278-B

478

Page 62

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

15 Program Support Functions

Relationship with other functions

Function name Notes

Unidirectional positioning Normal line control is not applied. Helical cutting Normal line control is applied normally. Spiral interpolation The start point and end point are not on the same arc, so normal line control is not

applied correctly.

Exact stop check The operation will not decelerate and stop for the turning movement of the normal

line control axis. Error detect Error detect is not applied to the turning movement of the normal line control axis. OVERRIDE Override is applied to the turning movement by normal line control axis. Coordinate rotation by pro-

gram Scaling Normal line control is applied to the shape after scaling. Mirror image Normal line control is applied to the shape after mirror image. Thread cutting Normal line control is not applied. Automatic reference position

return Start position return Normal line control is not applied to the movement to the intermediate point posi-

High-accuracy control This cannot be commanded during normal line control. The program error (P29)

Spline This cannot be commanded during normal line control. The program error (P29)

High-speed High-accuracy control I/II

Cylindrical interpolation This cannot be commanded during normal line control. The program error (P486)

Workpiece coordinate system offset

Local coordinate system offset

Program restart The program including the normal line control command cannot be restarted. "E98

Dry run The feedrate is changed by the dry run signal even in respect to the turning move-

Chopping The axis cannot be used as the normal line control axis during the chopping com-

Graphic check The section turned by normal line control is not drawn. The axes subject to graphic

G00 non-interpolation Normal line control is not applied.

Normal line control is applied to the shape after coordinate rotation.

Normal line control is not applied.

tion.

If the base specification parameter "#1086 G0Intp" is OFF, normal line control is

applied to the movement from the intermediate point to a position designated in

the program.

will occur.

The normal line control command during high-accuracy control cannot be issued,

either.

The program error (P29) will occur.

will occur.

The normal line control command during spline cannot be issued, either.

The program error (P29) will occur.

This cannot be commanded during normal line control. The program error (P29)

will occur.

The normal line control command during high-speed High-accuracy control I/II

cannot be issued either.

The program error (P29) will occur.

will occur.

The normal line control command during cylindrical interpolation cannot be is-

sued, either. The program error (P481) will occur.

The workpiece coordinate system cannot be changed during normal line control.

The program error (P29) will occur. The program parameter input (G10L2) cannot

be commanded either. The program error (P29) will occur.

The local coordinate system cannot be changed during normal line control. The

program error (P29) will occur.

CAN'T RESEARCH" will occur.

ment of the normal line control axis.

mand.

check are drawn.

479

IB-1501278-B

Page 63

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

15 Program Support Functions

Function name Notes

Polar coordinate interpolation

This cannot be commanded during normal line control. The program error (P486) will occur. The normal line control command during polar coordinate interpolation cannot be issued either. The program error (P481) will occur.

Exponential interpolation If the normal line control axis is the same as the rotary axis of exponential interpo-

lation, a program error (P612) will occur. If they are different, an error will not occur, but normal line control is not applied.

Plane selection This cannot be commanded during normal line control. The program error (P903)

will occur.

System variable The block end coordinate (#5001 - ) for the normal line control axis during normal

line control cannot obtain a correct axis position.

Precautions

(1)During normal line control, the program coordinates are updated following the normal line control axis movement.

Thus, program the normal line control on the program coordinate system.

(2)The normal line control axis will stop at the turning start position for the single block, cutting block start interlock

and block start interlock.

(3)The C axis movement command is ignored during normal line control.

(4)During C axis normal line control (during the G41.1 and G42.1 modal), the C axis workpiece offset rewrite com-

mand (G92C_;) cannot be issued. The program error (P901) will occur if commanded.

(5)If mirror image is applied to either the 1-axis or 2-axis, the normal line control direction will be reversed.

(6)The rotary axis must be designated as the normal line control axis (parameter (#1522 C_axis)). Designate so that

the axis is not duplicated with the axis on the plane where normal line control is to be carried out. If an illegal axis is designated, the program error (P902) will occur when the program (G40.1, G41.1, G42.1) is commanded. The program error (P902) will also occur if the parameter "#1522 C_axis" is "0" when commanding a program.

(7)This function may not be usable, depending on the model.

(8)The movement of the normal line control axis is counted as one axis of number of simultaneous contouring control

axes. If the number of simultaneous contouring control axes exceeds the specification range by movement of the normal line control axis, the program error (P10) will occur.

IB-1501278-B

480

Page 64

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

15 Program Support Functions

15.8 Manual Arbitrary Reverse Run Prohibition ; G127

G127

Function and purpose

The manual arbitrary reverse run function controls the feedrate, which is under automatic operation in memory or MDI mode, in proportion to the manual feedrate by the jog or the rotation speed by the manual handle, and manually carries out the reverse run. After the automatic operation has been stopped in a block, the reverse run can be carried out back through the blocks (up to 20 blocks) that were executed before the block. If necessary, it is possible to correct the program buffer and execute the fixed program after carrying out the reverse run up to the return position.

This function (G127) is available to prevent the program from backing to blocks before the commanded block when carrying out the manual arbitrary reverse run. The detailed setting and operation vary depending on the machine specifications. Refer to the Instruction Manual issued by the MTB. "Forward run" means to execute blocks in the same order as for the automatic operation. "Reverse run" means to process the executed blocks backward. Whether the reverse run is prohibited for each part system depends on the MTB specifications (system variable #3004). Refer to "List of System Variables" for details.

Command format

G127 ; All part system reverse run prohibit command

This command disables the program from running reverse to blocks before G127. In part systems that do not have this command executed, the program cannot run reverse before the timing with G127 commanded in any part system even if a block is in process. No commands in the machining program can be backed in the reverse run mode. For some G codes, the operation differs from the above. Refer to "Relationship with Other Functions".

The reverse run is disabled before the G127 block in the 2nd part system. The reverse run is canceled in the middle of a block in part systems other than the 2nd part system.

481

IB-1501278-B

Page 65

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

15 Program Support Functions

Relationship with Other Functions

The following shows the relationship between the manual arbitrary reverse run command and G code.

Symbol in

"Reverse

run" col-

umn

○*1 Block with reverse run enabled ○*2 Block with restricted-reverse run enabled Refer to the Remarks for restrictions. ∆ Block with reverse run ignored. This block is ignored in both the forward and reverse run modes.

×*3 Block with reverse run prohibited. This is intended only for the command blocks. ×*4 Block with reverse run prohibited. The reverse run is also prohibited for all blocks after the mode

has been switched by this block.

×*5 Prohibits the reverse run in all part systems.

Operation

G Code Function name Re-

Remarks

verse

run

G00 Positioning ○*1 G01 Linear interpolation ○*1 - G02 Circular interpolation CW and spiral/conical

○*1 -

interpolation CW (type2)

G03 Circular interpolation CCW and spiral/coni-

○*1 -

cal interpolation CCW (type2) G02.3 Exponential interpolation CW ×*3 G03.3 Exponential interpolation CCW ×*3 G02.4 3-dimensional circular interpolation × *3 G03.4 3-dimensional circular interpolation × *3 G04 Dwell ○*1 Dwell skip is invalid. G05 High-speed high-accuracy control II/III /

× *4 -

High-speed machining mode G05.1 High-speed high-accuracy control I / Spline × *4 G06.2 NURBS interpolation × *4 G07 Hypothetical axis interpolation × *3 G07.1

Cylindrical interpolation ×*4 G107

G08 High-accuracy Control ×*4 G09 Exact stop check No. of axes ○*1 - G10 Program data input (Parameter / Compen-

sation input / Coordinate rotation by param-

∆ The reverse run is enabled, but data is not

recovered.

eter data) G10.6 Tool retract command ×*3 G11 Program parameter input / cancel ∆ The reverse run is enabled, but data is not

recovered. G12 Circular cutting CW × *3 G13 Circular cutting CCW × *3 G12.1

Polar coordinate interpolation ON ×*4 -

G112 G13.1

Polar coordinate interpolation cancel ×*4 -

G113 G15 Polar coordinate command OFF ×*4 G16 Polar coordinate command ON ×*4 -

IB-1501278-B

482

Page 66

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

15 Program Support Functions

G Code Function name Re-

Remarks

verse

run

G17 X-Y plane selection ○*2 Data is recovered using the modal informa-

tion storage block.

G18 Z-X plane selection ○*2 Data is recovered using the modal informa-

tion storage block.

G19 Y-Z plane selection ○*2 Data is recovered using the modal informa-

tion storage block.

G20 Inch command ○*1 Switched with the movement command just

after commanded.

G21 Metric command ○*1 Switched with the movement command just

after commanded. G22 Stroke check before travel ON ×*3 G23 Stroke check before travel OFF ×*3 G27 Reference position check ×*3 G28 Automatic reference position return ×*3 G29 Start position return ×*3 G30 2nd, 3rd and 4th reference position return ×*3 G30.1 Tool change position return 1 ×*3 G30.2 Tool change position return 2 ×*3 G30.3 Tool change position return 3 ×*3 G30.4 Tool change position return 4 ×*3 G30.5 Tool change position return 5 ×*3 G30.6 Tool change position return 6 ×*3 G31 Skip/Multi-step skip function 2 ×*3 G31.1 Multi-step skip function 1-1 ×*3 G31.2 Multi-step skip function 1-2 ×*3 G31.3 Multi-step skip function 1-3 ×*3 G33 Thread cutting ○*2 The reverse run is enabled, but the synchro-

nous feed is invalid. Actual cutting mode

available. G34 Special fixed cycle (bolt hole circle) ×*4 G35 Special fixed cycle (write at angle) ×*4 G36 Special fixed cycle (arc) ×*4 G37 Automatic tool length measurement ×*3 G37.1 Special fixed cycle (grid) ×*4 G38 Tool radius compensation vector designa-

×*3 -

tion G39 Tool radius compensation corner arc ×*3 G40 Tool radius compensation cancel/3-dimen-

tional tool radius compensation cancel G41 Tool radius compensation left / 3-dimention-

al tool radius compensation left G42 Tool radius compensation right / 3-dimen-

tional tool radius compensation right G40.1

Normal line control cancel ×*4 -

○*2 Data is recovered using the modal informa-

tion storage block.

○*2 Data is recovered using the modal informa-

tion storage block.

○*2 Data is recovered using the modal informa-

tion storage block.

G150 G41.1

Normal line control left ON ×*4 G151

G42.1

Normal line control right ON ×*4 G152

G43 Tool length compensation (+) ○*2 Data is recovered using the modal informa-

tion storage block.

483

IB-1501278-B

Page 67

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

15 Program Support Functions

G Code Function name Re-

Remarks

verse

run

G44 Tool length compensation (-) ○*2 Data is recovered using the modal informa-

tion storage block.

G43.1 Tool length compensation along the tool

×*3 -

axis G43.4 Tool center point control type1 ON ×*4 G43.5 Tool center point control type2 ON ×*4 G45 Tool position offset (extension) ○*2 Data is recovered using the modal informa-

tion storage block.

G46 Tool position offset (reduction) ○*2 Data is recovered using the modal informa-

tion storage block.

G47 Tool position offset (double) ○*2 Data is recovered using the modal informa-

tion storage block.

G48 Tool position offset (decreased by half) ○*2 Data is recovered using the modal informa-

tion storage block.

G49 Tool length compensation cancel / Tool cen-

ter point control cancel

○*1/ ×*3

If tool length compensation cancel is desig-

nated, reverse running is enabled. G50.2 Scaling cancel ×*4 G51.2 Scaling ON ×*4 G50.1 Mirror image by G code cancel ×*3 G51.1 Mirror image by G code ON ×*3 G52 Local coordinate system setting ○*2 Data is recovered using the modal informa-

tion storage block. G53 Machine coordinate system selection ○*2 Data is recovered using the modal informa-

tion storage block. G54 Workpiece coordinate system 1 selection ○*2 Data is recovered using the modal informa-

tion storage block. G55 Workpiece coordinate system 2 selection ○*2 Data is recovered using the modal informa-

tion storage block. G56 Workpiece coordinate system 3 selection ○*2 Data is recovered using the modal informa-

tion storage block. G57 Workpiece coordinate system 4 selection ○*2 Data is recovered using the modal informa-

tion storage block. G58 Workpiece coordinate system 5 selection ○*2 Data is recovered using the modal informa-

tion storage block. G59 Workpiece coordinate system 6 selection ○*2 Data is recovered using the modal informa-

tion storage block. G54.1 Workpiece coordinate system selection 48 /

96 sets extended

○*2 Data is recovered using the modal informa-

tion storage block. G60 Unidirectional positioning ×*3 G61 Exact stop check mode ○*1 - G61.1 High-accuracy control ON ×*4 G61.2 High-accuracy spline ×*4 G62 Automatic corner override ○*1 - G63 Tapping mode ○*1 - G63.1 Synchronous tapping mode (Forward tap-

×*4 -

ping)

G63.2 Synchronous tapping mode (Reverse tap-

×*4 -

ping) G64 Cutting mode ○*1 - G65 User macro call ○*1 - G66 User macro modal call A ○*1 - G66.1 User macro modal call B ○*1

IB-1501278-B

484

Page 68

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

15 Program Support Functions

G Code Function name Re-

Remarks

verse

run

G67 User macro modal call cancel ○*1 - G68 Coordinate rotation by program mode ON /

×*4 3-dimensional coordinate conversion mode ON

G68.2 Inclined surface machining command × *3 G68.3 Inclined surface machining command

× *3 (Based on tool axis direction)

G69 Coordinate rotation by program mode can-

×*4 cel / 3-dimensional coordinate conversion mode cancel / Inclined surface machining command cancel

G70 User fixed cycle ×*3 G71 User fixed cycle ×*3 G72 User fixed cycle ×*3 G73 Fixed cycle (step) ○*1 Data is created for each movement block in

the fixed cycle.

G74 Fixed cycle (reverse tap) ○*2 The reverse run is enabled, but the synchro-

nous feed is invalid. Actual cutting mode available.

G75 Fixed cycle (circular cutting cycle) ○*1 Data is created for each movement block in

the fixed cycle.

G76 Fixed cycle (Fine boring) ○*1 Data is created for each movement block in

the fixed cycle. G77 User fixed cycle ×*3 G78 User fixed cycle ×*3 G79 User fixed cycle ×*3 G80 Fixed cycle for drilling cancel ○*1 - G81 Fixed cycle (drill/spot drill) ○*1 Data is created for each movement block in

the fixed cycle. G82 Fixed cycle (drill/counter boring) ○*1 Data is created for each movement block in

the fixed cycle. G83 Fixed cycle (deep drilling) ○*1 Data is created for each movement block in

the fixed cycle. G84 Fixed cycle (tapping) ○*2 The reverse run is enabled, but the synchro-

nous feed is invalid. Actual cutting mode

available. G85 Fixed cycle (boring) ○*1 Data is created for each movement block in

the fixed cycle. G86 Fixed cycle (boring) ○*1 Data is created for each movement block in

the fixed cycle. G87 Fixed cycle (back boring) ○*1 Data is created for each movement block in

the fixed cycle. G88 Fixed cycle (boring) ○*1 Data is created for each movement block in

the fixed cycle. G89 Fixed cycle (boring) ○*1 Data is created for each movement block in

the fixed cycle. G90 Absolute value command ○*2 Switched with the movement command just

after commanded. G91 Incremental value command ○*2 Switched with the movement command just

after commanded. G92 Coordinate system setting ○*1 - G92.1 Workpiece coordinate system pre-setting ○*1 - G94 Asynchronous feed (feed per minute ) ○*1 -

485

IB-1501278-B

Page 69

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

15 Program Support Functions

G Code Function name Re-

Remarks

verse

run

G95 Synchronous feed (feed per revolution) ○*1 - G96 Constant surface speed control ON ○*2 Switched with the movement command just

after commanded.

G97 Constant surface speed control OFF ○*2 Switched with the movement command just

after commanded. (G94) Asynchronous feed (feed per minute ) ○*1 - (G95) Synchronous feed (feed per revolution) ○*1 - G98 Fixed cycle Initial level return ○*1 - G99 Fixed cycle R point level return ○(*1 - G115 Start point designation synchronization

○*1 -

Type 1

G116 Start point designation synchronization

○*1 -

Type 2 G118.2 Parameter switching (Spindle) ×*3 G119.2 Inertia Estimation (Spindle) ×*3 G100 to

User macro (G code call) Max. 10 ○*1 - G225

M98 Subprogram call ○*1 -

IB-1501278-B

486

Page 70

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

15 Program Support Functions

15.9 Data Input by Program

15.9.1 Parameter Input by Program ; G10 L70/L100, G11

Function and purpose

The parameters set from the setting and display unit can be changed in the machining programs. G10 L70 ... For commanding data with decimal point, and character string data. The data's command range conforms to the parameter setting range described in Setup Manual.

G10 L100 ... For setting/changing the tool shape for 3D solid program check.

Command format

G10 L70 ;...Data setting start command

P__ S__ A__ H□__ ; .......... Bit parameter

P__ S__ A__ D__ ; ............... Numerical value parameter

P__ S__ A__ <character string> ; ...... Character string parameter

P Parameter No. S Part system No. A Axis No. HData DData character string Data

G11 ; ... Data setting end command

(Note 1) The sequence of addresses in a block must be as shown above.

When an address is commanded two or more times, the last command will be valid.

(Note 2)The part system No. is set in the following manner. "1" for the 1st part system, "2" for 2nd part system, and

so forth. If the address S is omitted, the part system of the executing program will be applied. As for the parameters common to part systems, the command of part system No. will be ignored.

(Note 3)The axis No. is set in the following manner. "1" for 1st axis, "2" for 2nd axis, and so forth.

If the address A is omitted, the 1st axis will be applied. As for the parameters common to axes, the command of axis No. will be ignored.

(Note 4)Address H is commanded with the combination of setting data (0 or 1) and the bit designation □ (0 to 7).

(Note 5)Only the decimal number can be commanded with the address D.

The value that is smaller than the input setting increment (#1003 iunit) will be round off to the nearest increment.

(Note 6)The character string must be put in angled brackets "<" and ">".

If these brackets are not provided, the program error (P33) will occur. Up to 63 characters can be set.

(Note 7)Command G10 L70, G11 in independent blocks. A program error (P33, P421) will occur if not commanded

in independent blocks.

(Note 8)The following data cannot be changed with the G10 L70 command:

Tool compensation data, workpiece coordinate data, PLC switch, and PLC axis parameter.

(Note 9)The settings of the parameters with (PR) in the parameter list will be enabled after the power is turned OFF

and ON. Refer to the parameter list in your manual.

487

IB-1501278-B

Page 71

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

15 Program Support Functions

G10 L100 ;...Data setting start command

P__ T__ K__ D__ H__ I__ J__ C__ ; ... Data setting mode cancel

G11 ; ... Data setting end command

P Line No. of the tool set area 1 to 80 (Required to command) (Note 1) T Tool No. 0 to 99999999 (Required to command) K Command the tool type using a numerical value.

0: Default tool (3: Drill is set) 1: Ball end mill 2: Flat end mill 3: Drill 4: Bull nose end mill 5: Chamfer 6: Tap

7: Face mill D Tool diameter/radius (Decimal point input available) (Note 2)(Note 3) H Tool length (Decimal point input available) (Note 3) I Tool shape data 1 (Decimal point input available) J Tool shape data 2 (Decimal point input available) C Command the tool color using a numerical value.

0: Default color (2: Red is set)

1: Grey 2: Red 3: Yellow 4: Blue

5: Green 6: Light blue 7: Purple 8: Pink

(Note 1) Line No. corresponds with a line No. in the tool shape set area (tool shape set screen).

(Note 2) The setting of "#8117 OFS Diam DESIGN" determines tool diameter or tool radius.

(Note 3) The available integer range can be changed by the parameter "#11050 T-ofs digit type".

(Note 4) For details of the data, refer to the explanation of Instruction Manual "Program Check (3D)".

(Note 5) Omitted addresses cannot be set or changed.

(Note 6) When address T is set to 0, the designated line is deleted.

(Note 7) In the following cases, Program Errors (P421) occurs and the parameter in the block is not changed.

- When a block contains an address whose data are out of range

- When there is an illegal address

- When P or T is omitted

(Note 8) Command G10L100, G11 in independent blocks. The program error Program Errors (P421) will occur if not

commanded in independent blocks.

(Note 9) The parameter "#1078 Decimal point type 2" is enabled.

(Note 10) The parameter "#8044 Unit*10" is disabled.

(Note 11) The display or operation at graphic check varies depending on the model or display unit.

IB-1501278-B

488

Page 72

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

15 Program Support Functions

Program example

(1)When G10 L70 command

G10 L70; P6401 H71; Sets "1" to "#6401 bit7". P8204 S1; A2 D1.234; Sets "1.234" to "#8204 of the 1st part system 2nd axis". P8621 <X> ; Sets "X" to "#8621". G11 ;

(2)When G10 L100 command

G10 L100; P1 T1 K3 D5. H20. I0 J0 C2 ; Set the data of Line 1 P2 T10 D10. ; Set "10." for the tool diameter/radius of Line 2 P8 T0; Clear the data of Line 8 G11 ;

489

IB-1501278-B

Page 73

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

15 Program Support Functions

15.9.2 Compensation Data Input by Program ; G10 L2/L10/L11, G11

Function and purpose

The tool compensation and workpiece offset can be set or changed by the program using the G10 command. During the absolute value (G90) mode, the commanded offset amount serves as the new offset, whereas during the incremental value (G91) mode, the currently set offset plus the commanded offset serves as the new offset.

Command format

Workpiece coordinate system offset input (L2)

G90 (G91) G10 L2 P_ X_ Y_ Z_ ;

P 0 : External workpiece

1 : G54 2 : G55 3 : G56 4 : G57 5 : G58 6 : G59

X, Y, Z Offset amount of each axis

(Note)The compensation amount in the G91 will be an incremental amount and will be cumulated each time the pro-

gram is executed. Command G90 or G91 before the G10 as a cautionary means to prevent this type of error.

Extended workpiece coordinate system offset input (L20)

G10 L20 P_ X_ Y_ Z_ ;

P "n" number of G54.n (1 to 300) X, Y, Z Offset amount of each axis

Offset input to the currently selected workpiece coordinate system (When the L command is omitted)

G10 P_ X_ Y_ Z_ ;

P (1) During G54 to G59 modal 0 : External workpiece offset (EXT)

1 to 6: Workpiece offset input (G54 to G59) Other than 0 to 6: Program error (P35) (2) During G54.n modal 1 to 300: Extended workpiece coordinate system offset amount setting (G54.n) Other than 1 to 300: Program error (P35)

X, Y, Z Offset amount of each axis

IB-1501278-B

490

Page 74

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

15 Program Support Functions

Tool compensation input (L10/L11/L12/L13)

Type I

G10 L10 P_ R_ ; ... For tool compensation memory

P Compensation No. R Compensation amount

Type II

G10 L10 P_ R_ ; ... For tool compensation memory Tool length compensation shape compensation

G10 L11 P_ R_ ; ... For tool compensation memory Tool length compensation wear compensation

G10 L12 P_ R_ ; ... For tool compensation memory Tool radius shape compensation

G10 L13 P__ R__ ; ... For tool compensation memory Tool radius wear compensation

(Note) Type I is selected when parameter "#1037 cmdtyp" is set to "1", and type II is selected when set to "2".

Compensation input cancel

G11;

Common to workpiece coordinate system offset, extended workpiece coordinate system offset, and tool compensation.

491

IB-1501278-B

Page 75

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

15 Program Support Functions

Detailed description

; G10 L10 P10 R-12.345 ; G10 L10 P05 R9.8765 ; G10 L10 P30 R2.468 ;

(1) Even if this command is displayed on the screen, the offset No. and variable details will not be updated until ac-

tually executed. (2) G10 is an unmodal command and is only valid in the commanded block. (3) The G10 command does not contain movement, but must not be used with G commands other than G54 to G59,

G90 or G91. (4) Do not command G10 in the same block as the fixed cycle and sub-program call command. This will cause mal-

functioning and program errors. (5) The workpiece offset input command (L2 or L20) should not be issued in the same block as the tool compensa-

tion input command (L10). (6) If an illegal L No. or compensation No. is commanded, program errors (P172 and P170) will occur respectively.

If the offset amount exceeds the maximum command value, the program error (P35) will occur. (7) Decimal point inputs can be used for the offset amount. (8) The offset amounts for the external workpiece coordinate system and the workpiece coordinate system are com-

manded as distances from the basic machine coordinate system zero point. (9) The workpiece coordinate system updated by inputting the workpiece coordinate system will follow the previous

modal (G54 to G59) or the modal (G54 to G59) in the same block. (10) L2/L20 can be omitted when the workpiece offset is input. (11) When the P command is omitted for workpiece offset input, it will be handled as the currently selected work-

piece compensation input. (12) If the G command that cannot be combined with G10 is issued in the same block, a program error (P45) will

occur.

Program example

(1) Input the compensation amount.

H10=-12.345 H05=9.8765 H30=2.468

IB-1501278-B

492

Page 76

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

15 Program Support Functions

(2) Updating compensation amount

(a) (b1) (b2) (b3) (b4)

1000 1000 1000 1000

c1 d1

c3 d3

c2 d2

c4 d4

(Example 1) Assume that H10 = -1000 is already set.

N1 G01 G90 G43 Z-100000 H10 F100 ; (Z=-101000) N2 G28 Z0 ; N3 G91 G10 L10 P10 R-500 ; (The mode is the G91 mode, so -500 is added.) N4 G01 G90 G43 Z-100000 H10 ; (Z=-101500)

(Example 2) Assume that H10 = -1000 is already set.

Main program

N1 G00 X100000 ; a N2 #1=-1000 ; N3 M98 P1111 L4 ; b1, b2, b3, b4

Subprogram O1111

N1 G01 G91 G43 Z0 H10 F100 ; c1, c2, c3, c4 G01 X1000; d1, d2, d3, d4 #1=#1-1000 ; G90 G10 L10 P10 R#1 ; M99 ;

(Note) Final offset amount will be H10= -5000.

(Example 3) The program for Example 2 can also be written as follows.

Main program

N1 G00 X100000 ; N2 M98 P1111 L4 ;

Subprogram O1111

N1 G01 G91 G43 Z0 H10 F100 ; N2 G01 X1000 ; N3 G10 L10 P10 R-1000 ; N4 M99 ;

493

IB-1501278-B

Page 77

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

15 Program Support Functions

(3) When updating the workpiece coordinate system offset amount

- X - 20. - 10.

- 10.

- 20.

- Y

- X

N100

N101

N102

(W1)

Assume that the previous workpiece coordinate system offset amount is as follows.

X=-10.000 Y=-10.000

N100 G00 G90 G54 X0 Y0 ; N101 G90 G10 L2 P1 X-15.000 Y-15.000 ; N102 X0 Y0 ; M02 ;

Basic machine coordinate system zero point

G54 coordinate before change

(Note 1)Changes of workpiece current position display at N101, the G54 workpiece position display data will

change before and after the workpiece coordinate system is changed with G10.

X = 0

Y = 0

When workpiece coordinate system offset amount is set in G54 to G59

G90 G10 L2 P1 X-10.000 Y-10.000 ; G90 G10 L2 P2 X-20.000 Y-20.000 ; G90 G10 L2 P3 X-30.000 Y-30.000 ; G90 G10 L2 P4 X-40.000 Y-40.000 ; G90 G10 L2 P5 X-50.000 Y-50.000 ; G90 G10 L2 P6 X-60.000 Y-60.000 ;

G54 coordinate after change

→ X = +5.000

Y = +5.000

IB-1501278-B

494

Page 78

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

15 Program Support Functions

(4) When using one workpiece coordinate system as multiple workpiece coordinate systems

-X -10.

- 10.

- 20.

-Y

- 50.

- 30.

- 60.

- 40.

G54'' ''

G54'' '

G54''

G54'

G54

- 50. - 40. - 30. - 20.

Main program :

#1=-50. #2=10. ; M98 P200 L5 ; M02 ; %

Subprogram

O200

N1 G90 G54 G10 L2 P1 X#1 Y#1 ; N2 G00 X0 Y0 ; N3 X-5. F100 ; N4 X0 Y-5. ; N5 Y0 ; N6 #1=#1+#2 ; N7 M99 ; %

Basic machine coordinate system zero point

Precautions

(1) Even if this command is displayed on the screen, the offset No. and variable details will not be updated until ac-

tually executed. N1 G90 G10 L10 P10 R-100 ; N2 G43 Z-10000 H10 ; N3 G00 X-10000 Y-10000 ;

N4 G90 G10 L10 P10 R-200 ; ........ The H10 offset amount is updated when the N4 block is executed.

495

IB-1501278-B

Page 79

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

15 Program Support Functions

15.9.3 Tool Shape Input by Program ; G10 L100, G11

Function and purpose

This function sets tool shape data of the tool management screen by the machining program. Using this function saves having to execute the many steps required to input the tool shape from the screen when executing 3D checks.

Command format

Tool shape setting from program

G10 L100 ;...Data setting start command P_ T_ K_ D_ H_ I_ J_ C_ ; ...Data setting command

P Data No. Designate the data number of the tool management screen. (cannot be omitted)

The maximum data number varies depending on the number of tool management data sets.

T Tool number Designate the tool number. (cannot be omitted)

0 to 99999999 If "0" is designated, all tool shape data of the data number designated with address P is set to "0". In this case, data other than tool shape data remains unchanged.

K Type Designate the tool type using a numerical value.

[Mill tool] 1: Ball end mill 2: Flat end mill 3: Drill 4: Radius end mill 5: Chamfer 6: Tapping 7: Face mill [Turning tool] 51: Turning 52: Slotting 53: Thread cutting 54: Turning drill

55: Turning tapping D Shape data 1 Designate shape data of the tool. (Decimal point input available) H Shape data 2 I Shape data 3 For details on the setting of each tool type, refer to "Correspondence between J Shape data 4 C Tool color Designate the tool color.

Shape data setting details vary depending on the tool type.

Tool Types and Shape Data" shown below.

1: Gray 2: Red 3: Yellow 4: Blue

5: Green 6: Light blue 7: Purple 8: Pink

G11 ; ... Data setting end command

IB-1501278-B

496

Page 80

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

15 Program Support Functions

[Correspondence between tool types and shape data]

[Mill tool]

Shape data Item by tool type

Ball end mill Flat end mill Drill Radius end

Chamfering Tapping Face mill

mill

1 Tool length 2 Tool radius (*1) 3--Tool nose

Corner R Tip angle Pitch Cutter length

angle

4 - - - - Tip radius Root diame-

Shank radius

ter 5------6-------

[Turning tool]

Shape data Item by tool type

Turning Slotting Thread Cutting Turning drill Turning tapping

1 Tool length A 2 Tool length B Tool length B (*1) 3 Tool nose R Tool nose R - Tool nose angle Pitch 4 Tool nose angle Tool nose width - - Root diameter 5 Cut angle Maximum groove

---

depth

6 Tool width Tool width Tool width - -

(*1) When "#8968 Tool shape radius valid" is set to "0", enter the diameter value. When it is set to "1", enter the

radius value.

(Note 1) Omitted addresses are not set.

(Note 2) If address "P" or "T" is omitted, a program error (P422) will occur.

(Note 3) For M80 Series, tool shape data will be rewritten during graphic checks.

(Note 4) For M800W Series or M800S Series graphic checks, this change is reflected only on the graphic check

drawing. The tool shape data is not rewritten.

497

IB-1501278-B

Page 81

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

15 Program Support Functions

Detailed description

G10 L100; P1 T201 ...; P3 T203 ...;

G11;

O200

(a)

(b)

(c)

T201; (Replaced with tool A.)

T202; (Replaced with tool B.)

T203; (Replaced with tool C.)

Machining program Tool shape data

Tool A

Tool B

Tool C

3D check screen

Tool management screen

(Change the shape of tool A.)

(Newly register the shape of tool C.)

Tool shape setting from program

For 3D checks, tool drawing is switched when the tool change command is issued. Create a machining program to execute the tool shape setting command before issuing the tool change command.

(a) Draw the tool after the tool shape has been changed by the machining program.

(b) Draw the tool with the tool shape registered on the tool management screen.

Program example

(1) Tool shape setting from program

G10 L100; P1 T1 K3 D5. H20. I0 J0 C2 ; Set data of data No. 1. P2 T10 D10. ; Set "10." for the tool radius of data No. 2. P8 T0; Set "0" for the tool shape data of data No. 8. G11;

Precautions

(1) If the G10 or G11 command is not issued in an independent block, a program error (P422) will occur.

IB-1501278-B

(2) When a block contains an address whose data are out of range, a program error (P35) will occur. (3) When a block contains an invalid address, a program error (P32) will occur. (4) The parameter "#1078 Decimal pnt type 2" is valid for the position command.

Other command addresses conform to the minimum input unit ("#1015 cunit"). (Based on the MTB specifica-

tions.) (5) The parameter "#8044 UNIT*10" is invalid. (6) The parameter input in mm/inch units has the command unit changed with G20 or G21.

498

Page 82

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

15 Program Support Functions

15.9.4 R-Navi Data Input by Program ; G10 L110, G11

Function and purpose

The R-Navi setup parameters can be configured from a machining program. Command setting values with absolute

values.

The input unit conforms to the input setting unit of the 1st part system and the initial inch.

In either case, the input unit depends on the MTB specifications (parameters "#1003 iunit" and "#1041 I_inch").

The parameter "#8044 UNIT*10" is invalid.

Command format

Workpiece registration and setting

G10 L110 ;...Start setting workpiece data

Q_ <_> F_ C_ R_ X_ Y_ Z_ I_ J_ K_; ...Data setting

G11 ; ... End data setting

- Command G10 and G11 in independent blocks. A program error (P423) will occur if not commanded in independent blocks.

- Address Q cannot be omitted. If omitted, a program error (P423) will occur.

- For the omitted addresses, data remains unchanged.

Q Workpiece registration No.

(1 to 10)

< > Workpiece name

Designate the name using up to 20 one-byte alphanumeric characters, including symbols. (If "0" is entered, the setting value is cleared.)

F Workpiece shape

0: Rectangular parallelepiped 1: Circular cylinder

C Basic coordinate system of workpiece

0 to 5: G54 to G59 6 to 305: G54.1P1 to G54.1P300

R Marked point No.

When the workpiece shape is set to rectangular parallelepiped, designate the marked point to set the basic coordinate system zero point.(0 to 8)

X, Y, Z, Workpiece size

When the shape is set to circular cylinder, designate the diameter with X and the height with Y. (0.000 to 99999.999)

I, J, K Workpiece shift

Set the shift amount from the marked point to the basic coordinate system zero point. (-99999.999 to 99999.999)

- Symbols "\", "/", ",", "*", "?", """, "<", ">", "|", and " " (space) cannot be used as one-byte symbols. If an available symbol is set, a program error (P35) will occur.

- For details on each of input data, refer to the instruction manual.

499

IB-1501278-B

Page 83

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

15 Program Support Functions

Machining surface registration and setting

G10 L111 ; Start setting machining surface data

P0 Q_ D_ <_> X_ Y_ Z_ A_; ... Machining surface setting (Refer to (1).) P1 M_ B_ C_ E_ F_ H_ I_; ... Designate coordinate axis direction (1st axis). (Refer to (2).) P2 M_ B_ C_ E_ F_ H_ I_; ... Designate coordinate axis direction (2nd axis). (Refer to (2).)

G11 ; ... End data setting

G68.2 P10 Q_ D_; Select the registered machining surface

- Command G10 and G11 in independent blocks. A program error (P423) will occur if not commanded in independent blocks.

- Addresses P, Q, and D cannot be omitted. If omitted, a program error (P423) will occur.

- For the omitted addresses, data remains unchanged.

- For the machining surface designated with P0, set the coordinate axis direction with P1 and P2. Be sure to first command P0. If P1 or P2 is commanded before P0, a program error (P423) will occur.

- The machining surface cannot be registered for an undefined workpiece. If the registration command is issued, a program error (P423) will occur.

(1) Command address to register the machining surface

P Machining surface registration

(0)

Q Workpiece registration No.

(1 to 10)

D Machining surface registration No.

(2 to 17)

< > Designate the name of the machining surface using up to 15 one-byte alphanu-

meric characters, including symbols. (If "0" is entered, the setting value is cleared.)

X, Y, Z Designate the coordinate system zero point (feature coordinate system zero point)

of the machining surface with the offset from the basic coordinate zero point. In this case, designate the coordinate axis direction of the basic coordinate system. (-99999.999 to 99999.999)

A From three orthogonal axes (X, Y, and Z axes), select two coordinate axes to des-

ignate the coordinate axis direction along the machining surface. 0: Z/X axis 1: Y/Z axis 2: X/Y axis

- Symbols "\", "/", ",", "*", "?", """, "<", ">", "|", and " " (space) cannot be used as one-byte symbols. If an available symbol is set, a program error (P35) will occur.

- For details on each of input data, refer to the instruction manual.

IB-1501278-B

500

Page 84

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

15 Program Support Functions

(2) Command address to designate the coordinate axis direction

P Coordinate axis direction axis designation

1: 1st axis 2: 2nd axis

M Coordinate axis direction designation method

Designate the method to set the coordinate axis direction along the machining surface. 0: [Method 1] On-axis point (+) 1: [Method 2] Latitude/Longitude 2: [Method 3] Latitude / Projection angle 3: [Method 4] Start point / End point 4: [Method 5] Indexing angle (Z axis direction only)

B, C, E, F, H, I Coordinate axis direction setting (Note 1)

(-99999.999 to 99999.999)

(Note 1) The setting details vary depending on the coordinate axis direction designation method (M address).

[M address: 0 (On-axis point (+))] B, C, E: Coordinate value on X, Y, or Z axis F to I: Vacuous [M address: 1 (Latitude/Longitude)] B: Longitude (θ1) C : Latitude (θ2) E to I: Vacuous [M address: 2 (Latitude / Projection angle)] B: Longitude (θ1) C : Projection angle (θ2) E to I: Vacuous [M address: 3 (Start point / End point)] B: Start point coordinate value (X) C : Start point coordinate value (Y) E : Start point coordinate value (Z) F: End point coordinate value (X) H: End point coordinate value (Y) I: End point coordinate value (Z) [M address: 4 (Indexing angle)] B: 1st rotation angle (θ1) C : 2nd rotation angle (θ2) E to I: Vacuous

- Method 5 (indexing angle) in the coordinate axis direction designation method is only available in the Z axis direction. If a command is issued to an axis other than the Z axis designated by the coordinate axis selection command (P0Ax), "P423 R-Navi input error" will occur. For P0 A0 (Z/X axis), P2 M4 setting causes an error. (Method 5 is not able to be selected on the 2nd axis.) For P0 A1 (Y/Z axis), P1 M4 setting causes an error. (Method 5 is not able to be selected on the 1st axis.) For P0 A2 (X/Y axis), P1 M4 or P2 M4 setting causes an error. (Method 5 is not able to be selected.)

- For details on each of input data, refer to the instruction manual.

501

IB-1501278-B

Page 85

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

15 Program Support Functions

Operation example

WORK1

WORK2

BASE-SURFACE

SURFACE1-2

O200

(Setting of workpiece) G10 L110; Q1 <WORK1> F0 C0 R1 X50.0 Y30.0 Z20.0 I0.0 J0.0 K0.0 ; Q2 <WORK2> F0 C0 R5 X50.0 Y30.0 Z20.0 I-10.0 J-5.0 K-40.0 ; ... G11;

(Setting the machining surface) G10 L111; (Workpiece : 1, surface : 2) P0 Q1 D2 <SURFACE1_2> X50.0 Y-30.0 Z-20.0 A0; P1 M0 B1.0 C0.0 E1.732 F0.0 H0.0 I0.0; P2 M1 B90.0 C0.0 E0.0 F0.0 H0.0 I0.0; (Workpiece : 1, surface : 17) P0 Q1 D17 <SURFACE1_17> X20.0 Y20.0 Z10.0 A0; P1 M1 B0.0 C30.0 E0.0 F0.0 H0.0 I0.0; P2 M0 B0.0 C30.0 E0.0 F0.0 H0.0 I0.0; ... (Workpiece : 2, surface : 2) P0 Q2 D2 <SURFACE2_2> X20.0 Y20.0 Z10.0 A0; P1 M0 B1.0 C0.0 E1.732 F0.0 H0.0 I0.0; P2 M1 B90.0 C0.0 E0.0 F0.0 H0.0 I0.0; ... G11; ... (Selecting “Workpiece : 1, surface : 2”) G68.2 P10 Q1 D2;

Machining program

Setup parameters

Setup screen

This function enables the R-Navi setup parameters to be configured from a machining program. After the parameters have been configured from the program, you can check the values or select the machining surface from the setup screen.

IB-1501278-B

502

Page 86

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

15 Program Support Functions

15.10 Inputting The Tool Life Management Data ; G10,G11

15.10.1 Inputting The Tool Life Management Data by G10 L3 Command ; G10 L3,G11

Function and purpose

Using the G10 command (unmodal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted. There are three tool life management methods: I, II, and III. Which method is valid depends on the MTB specifications. Only group No. 1 can be used to register, change and add for the tool life management III.

Command format

Start of life management data registration

G10 L3;

P_ L_ Q_ ; (First group)

T_ H_ D_;

P_ L_ Q_ ; (Next group )

T_ H_ D_;

P Group No. LLife Q Control method T Tool No. The spare tools are selected in the order of the tool Nos. registered here. H Length compensation No. D Radius compensation No.

Start of life management data change or addition

G10 L3 P1;

P_ L_ Q_ ; (First group)

T_ H_ D_;

P_ L_ Q_ ; (Next group )

T_ H_ D_;

P Group No. LLife Q Control method T Tool No. H Length compensation No. D Radius compensation No.

503

IB-1501278-B

Page 87

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

15 Program Support Functions

Start of life management data deletion

G10 L3 P2;

P_ ; (First group)

P_ ; (Second group)

P Group No.

End of life management data registration, change, addition or deletion

G11 ;

Detailed description

Command range

Item Command range

Group No. (Pn) 1 to 99999999 (Only group No. 1 can be used for the tool life management

III)

Life (Ln) 0 to 65000 times (No. of times control method)0 to 4000 minutes (time con-

trol method)

Control method (Qn) 1 to 3

1: Number of mounts control 2: Time control

3: Number of cutting times control Tool No. (Tn) 1 to 99999999 Length compensation No. (Hn) 0 to 999 (*) Radius compensation No. (Dn) 0 to 999 (*)

(*) The setting range of the tool compensation No. differs according to the specification of the "number of tool offset

sets". If a value exceeding each command range is issued, a program error (P35) will occur.

IB-1501278-B

504

Page 88

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

15 Program Support Functions

Operation example

Program example Operation

Data registration G10 L3;

P10 L10 Q1 ; T10 H10 D10 ; G11 ; M02 ;

Group change, addition

Group deletion G10 L3 P2;

G10 L3 P1; P10 L10 Q1 ; T10 H10 D10 ; G11 ; M02 ;

P10 ; G11 ; M02 ;

1. After deleting all group data, the registration starts.

2. Group No. 10 is registered.

3. Tool No. 10 is registered in group No. 10.

4. The registration ends.

5. The program ends.

1. Changing and addition of the group and tool starts.

2. The change and addition operation takes place in the following manner. (1) When group No. 10 has not been registered.- Group No. 10 is additionally registered.

- Tool No. 10 is registered in group No. 10. (2) When group No. 10 has been registered, but tool No. 10 has not been registered.

- Tool No. 10 is additionally registered in group No. 10. (3) When group No. 10 and tool No. 10 have been both registered.- The tool No. 10 data is changed.

3. The group and tool change and addition ends.

4. The program ends.

1. The group deletion starts.

2. The group No. 10 data is deleted.

3. The group deletion ends.

4. The program ends.

505

IB-1501278-B

Page 89

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

15 Program Support Functions

15.10.2 Inputting The Tool Life Management Data by G10 L30 Command ; G10 L30,G11

Function and purpose

Using the G10 command (unmodal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted. Only group No. 1 can be used to register, change and add for the tool life management III. To specify additional compensation amount or direct compensation amount by control method, the length compensation and diameter compensation can be registered/changed with the tool compensation amount format.

Command format

Start of life management data registration

G10 L30;

P_ L_ Q_ ; (First group)

T_ H_ R_ ;

P_ L_ Q_ ; (Next group )

T_ H_ R_ ;

P Group No. LLife Q Control method T Tool No. The spare tools are selected in the order of the tool Nos. registered here. H Length compensation No. or length compensation amount R Radius compensation No. or radius compensation amount

L_, Q_, H_, and R_ cannot be omitted. If omitted, a program error (P33) occurs.

Start of life management data change or addition

G10 L30 P1;

P_ L_ Q_ ; (First group)

T_ H_ R_ ;

P_ L_ Q_ ; (Next group )

T_ H_ R_ ;

P Group No. LLife Q Length compensation data format, radius compensation data format, control method T Tool No. H Length compensation No. or length compensation amount D Radius compensation No. or radius compensation amount

L_, Q_, H_, and R_ cannot be omitted. If omitted, a program error (P33) occurs.

IB-1501278-B

506

Page 90

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

15 Program Support Functions

Start of life management data deletion

G10 L30 P2;

P_ ; (First group)

P_ ; (Second group)

P Group No.

End of life management data registration, change, addition or deletion

G11 ;

Detailed description

Command range

Item Command range

Group No. (Pn) 1 to 99999999 (Only group No. 1 can be used for the tool life management III) Tool No. (Tn) 1 to 99999999 Control method (Qabc) abc:Three integer digits

a. Tool length compensation data format 0: Compensation No. 1: Incremental value compensation amount 2: Absolute value compensation amount b. Tool radius compensation data format 0: Compensation No. 1: Incremental value compensation amount 2: Absolute value compensation amount c. Tool management method 0: Usage time 1: Number of mounts 2: Number of usages

Life (Ln) 0 to 4000 minutes (usage time)

0 to 65000 times (number of mounts) 0 to 65000 times (number of usages)

Length compensation (No./amount)

Radius compensation (No./amount)

(Hn) 0 to 999 (compensation No.) (*1)

±999.999 (incremental value compensation amount) (*2) ±999.999 (absolute value compensation amount) (*2)

(Rn) 0 to 999 (compensation No.) (*1)

±999.999 (incremental value compensation amount) (*2) ±999.999 (absolute value compensation amount) (*2)

(*1) The setting range of the tool compensation No. differs according to the specification of the "number of tool offset

sets".

(*2) Refer to (16) in "12.9.3 Precautions for Inputting the Tool Life Management Data" for the data range of compen-

sation amount.

507

IB-1501278-B

Page 91

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

15 Program Support Functions

Operation example

Program example Operation

Data registration G10 L30;

P10 L10 Q001 ; T10 H10 R10 ; G11 ; M02 ;

Group change, addition G10 L30 P1;

P10 L10 Q122 ; T10 H0.5 R0.25 ; G11 ; M02 ;

Group deletion G10 L30 P2;

P10 ; G11 ; M02 ;

1. After deleting all group data, the registration starts.

2. Group No. 10 is registered. Tool management method is number of mounts Compensation No. method is applied to tool length compensation and tool radius compensation.

3. Tool No. 10 is registered in group No. 10.

4. The registration ends.

5. The program ends.

1. Changing and addition of the group and tool starts.

2. The change and addition operation takes place in the following manner. (1) When group No. 10 has not been registered:

(a) Group No. 10 is registered additionally.

About the change and addition tool Tool management method is number of usages, Tool length compensation is the incremental value compensation amount method, and Tool radius compensation is the absolute value compensation amount method.

(b) For group No. 10, the incremental value compensation

amount "0.5" is registered for the length compensation, and the absolute value compensation amount "0.25" is registered for the radius compensation.

(2) When group No. 10 has been registered, but tool No. 10 has not been registered.

- Tool No. 10 is additionally registered in group No. 10. (3) When group No. 10 and tool No. 10 have been both registered.

- The tool No. 10 data is changed.

3. The group and tool change and addition ends.

4. The program ends.

1. The group deletion starts.

2. The group No. 10 data is deleted.

3. The group deletion ends.

4. The program ends.

IB-1501278-B

508

Page 92

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

15 Program Support Functions

15.10.3 Precautions for Inputting The Tool Life Management Data

Relationship with other functions

(1)During the following operations, the tool usage data will not be counted.

- Machine lock

- Auxiliary axis function lock

- Dry run

- Single block

- Skip

Precautions

(1) The tool life data is registered, changed, added to or deleted by executing the program in the memory or MDI

mode.

(2) The group No. and tool No. cannot be commanded in duplicate. The program error (P179) will occur.

(3) When two or more addresses are commanded in one block, the latter address will be valid.

(4) If the life data (L_) is omitted in the G10L3 command, the life data for that group will be "0".

(5) If the control method (Q_) is omitted in the G10L3 command, the control method for that group will follow the

base specification parameter "#1106 Tcount". Note that when carrying out the No. of cutting times control method, command the method from the program.

(6) If the control method (Q_) is not designated with 3-digit by G10 L30 command, the omitted high-order are equiv-

alent to "0". Therefore, "Q1" is equivalent to "Q001", and "Q12" is equivalent to "Q012".

(7) If the length compensation No. (H_) is omitted in the G10L3 command, the length compensation No. for that

group will be "0".

(8) If the radius compensation No. (D_) is omitted in the G10L3 command, the radius compensation No. for that

group will be "0".

(9) Programming with a sequence No. is not possible between G10 L3 or G10 L30 and G11. The program error

(P33) will occur.

(10) If the usage data count valid signal (YC8A) is ON, G10 L3 or G10 L30 cannot be commanded. The program

error (P177) will occur.

(11) The registered data is held even if the power is turned OFF.

(12) When G10 L3 or G10 L30 is commanded, the commanded group and tool will be registered after all of the reg-

istered data is erased.

(13) The change and addition conditions in the G10L3P1 or G10 L30 P1 command are as follows.

(a) Change conditions

Both the commanded group No. and tool No. are registered.

-> Change the commanded tool No. data.

(b) Additional conditions

Neither the commanded group No. nor tool No. is registered.

-> Additionally register the commanded group No. and tool No. data. The commanded group No. is registered, but the commanded tool No. is not registered.

-> Additionally register the commanded tool No. data to the commanded group No.

(14) The setting range of the tool compensation No. depends on the MTB specifications.

(15) Only group No. 1 can be used to register, change and add for the tool life management III.

509

IB-1501278-B

Page 93

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

15 Program Support Functions

15.10.4 Tool Life Management Set Allocation to Part Systems

250

200

400

334

333

500

Function and purpose

The number of tool life management sets can be set per part system. This function is divided into following methods and which one is used depends on the MTB specifications (parameters "#1439 Tlife-SysAssign", "#12055 Tol-lifenum"). Arbitrary allocation: Arbitrarily allocates the number of tool life management sets to each part system. Fixed allocation: Automatically and evenly allocates the number of tool life management sets to each part system. The arbitrary allocation enables the efficient allocation because when a certain part system needs only a small number of tool life management sets, the rest can be allocated to another part system. If an auxiliary-axis part system does not need the tool life management sets at all, the number of tool life management sets can be set to "0" for the auxiliary-axis part system. Subsequent description is an example in the case where the number of tool life management sets in the system is 999 sets.

(1) Arbitrary allocation (with #1439=1)

The number of sets allocated to each part system depends on the MTB specifications (parameter "#12055 Tollifenum"). The following example shows the number of tool offset sets allocated when the lathe system is a 4-part system.

(a) When the number of tool life management sets is increased for the 1st part system ($1) of 4-part system

(b) When the number of tool life management sets is set to "0 sets" for the 3rd part system ($3) of 3-part system

to use that part system as an auxiliary-axis part system

IB-1501278-B

510

Page 94

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

15 Program Support Functions

(2) Automatic and even allocation (with #1439=0)

1-part system 2-part system 3-part system

(Lathe system only)

4-part system (Lathe system only)

250

999

(*1)

500

334

(*2)

333

(*1)The maximum number of tool life management sets per part system is 999.

(*2) If there is any remainder, the remainder is allocated to the 1st part system.

Precautions

(1) The maximum number of tool life management sets for 1-part system is 999.

(2) For 1-part system, up to the number of tool life management sets in the system is available regardless of the

parameter setting.

(3) When the value of the parameter "#12055 Tol-lifenum" is equal to or lower than the number of tool life manage-

ment sets in the system, the remainder is not allocated to any part system even if the specification allows arbitrary allocation.

(4) When the value of the parameter "#12055 Tol-lifenum" is equal to or lower than the number of tool life manage-

ment sets in the system, system alarm (Y05) is generated even if the specification allows arbitrary allocation.

(5) Even if the specification allows arbitrary allocation, fixed allocation is applied if the parameter is "#12055 Tol-

lifenum"= "0" for all part systems.

(6) When entering data into the tool life management file, if the number of tool life management data exceeds that

of current tool life management sets, the excess tool life management data cannot be entered.

511

IB-1501278-B

Page 95

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

15 Program Support Functions

IB-1501278-B

512

Page 96

513

IB-1501278-B

Multi-part System Control

Page 97

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

16 Multi-part System Control

16Multi-part System Control

$1 $2

16.1 Timing Synchronization

CAUTION

When programming a multi-part system, carefully observe the movements caused by other part systems' programs.

16.1.1 Timing Synchronization Operation (! code) !n (!m ...) L

Function and purpose

The multi-axis, multi-part system complex control CNC system can simultaneously run multiple machining programs independently. The synchronization-between-part systems function is used in cases when, at some particular point during operation, the operations of 1st and 2nd part systems are to be synchronized or in cases when the operation of only one part system is required. When timing synchronization is executed in the 1st part system ($1) and the 2nd part system ($2), operations will be as follows.

Command format

Simultaneous and independent operation

Timing synchronization operation

Simultaneous and independent operation

Timing synchronization operation

2nd part system operation only 1st part system waiting

Timing synchronization operation

Simultaneous and independent operation

!n (!m ...) L_ ; ... timing synchronization operation

!n, !m, ... Timing synchronization operation (!) and part system No. (n:1 - number of part system

that can be used) Follows the settings of the parameter "#19419 Timing sync system" if part system number is omitted.

IB-1501278-B

Timing Synchronization Operation No. 0 to 9999

514

Page 98

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

16 Multi-part System Control

Detailed description

!nL1 ;

!iL1;

Pi1

Pn1

Pi2

Pn2

Pi1

Pi2

Pn1

Pn2

waiting...

Simultaneously start

Timing synchronization

(1) Timing synchronization between part systems during automatic operation

If !n L__ is commanded from a part system (i), operation of the part system i program will wait until !i L_ is commanded from the part system n program. When !i L_ is commanded, the programs for the two part systems will start simultaneously.

Timing synchronization between 2 part systems

(2) The timing synchronization operation is normally issued in a single block. However, if a movement command or

M, S or T command is issued in the same block, whether to synchronize after the movement command or M, S or T command or to execute the movement command or M, S or T command after synchronization will depend on the MTB specifications (#1093 Wnvfin). #1093 Wmvfin 0 : Wait before executing movement command. 1 : Wait after executing movement command.

(3) If there is no movement command in the same block as the timing synchronization operation, when the next block

movement starts, synchronization may not be secured between the part systems. To synchronize the part systems when movement starts after waiting, issue the movement command in the same block as the timing synchronization operation.

(4)The L command is the timing synchronization identification No. The same Nos. are waited but when they are omit-

ted, the Nos. are handled as L0.

(5) "SYN" will appear in the operation status section during timing synchronization operation. The timing synchroni-

zation operation signal will be output to the PLC I/F.

(6) In a timing synchronization operation, other part system to be waited for is specified but the own part system can

be specified with the other part system.

(7) The timing synchronization operation of a specific part system can be ignored depending on the MTB specifica-

tions. Operation will be determined by the combination of the timing synchronization operation ignore signal and parameter "#1279 ext15/bit0". For setting combination, refer to "Time synchronization when timing synchronization ignore is set". For the specifications of the machine you are using, see the instructions issued by the MTB.

515

IB-1501278-B

Page 99

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

16 Multi-part System Control

Precautions

(1) When the M code can be used, both the M code and ! code can be used.

(2) While the timing synchronization operation M code is valid, if one part system is standing by with an M code, an

alarm will occur if there is a ! code timing synchronization operation command in the other part system.

(3) While the timing synchronization operation M code is valid, if one part system is standing by with a ! code, an

alarm will occur if there is an M code timing synchronization operation command in the other part system.

(4) When macro interruption is carried out in a part system waiting, the part system can stop while waiting even if

the conditions for time synchronization are met. In this case, you will be able to continue the program, ignoring the timing synchronization with timing synchronization operation ignore signal. For details, contact the MTB.

IB-1501278-B

516

Page 100

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

16 Multi-part System Control

16.1.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115

Function and purpose

The part system can wait for the other part system to reach the start point before starting itself. The start point can be set in the middle of a block.

Command format

!n L__ G115 X__ Y__ Z__ ;

!n Timing synchronization operation (!) and part system No. (n:1 - number of part sys-

L Timing Synchronization Operation No. 0 to 9999

G115 G command X Y Z Start point

tem that can be used) Part systems follow the settings of the parameter "#19419 Timing sync system" if the number is omitted.

(It will be regarded as "L0" when omitted.)

(Command by axis and workpiece coordinate value)

517

IB-1501278-B

MITSUBISHI M80, M800 Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Introduction

Precautions for Safety

Disposal

Trademarks

Contents

Program Support Functions

15.1 Corner Chamfering I /Corner Rounding I

15.1.1 Corner Chamfering I ; G01 X_ Y_ ,C

15.1.2 Corner Rounding I ; G01 X_ Y_ ,R_

15.1.3 Corner Chamfering Expansion/Corner Rounding Expansion

15.1.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding

15.2 Corner Chamfering II /Corner Rounding II

15.2.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_

15.2.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_

15.2.3 Corner Chamfering Expansion/Corner Rounding Expansion

15.2.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding

15.3 Linear Angle Command ; G01 X_/Y_ A_/,A_

15.4 Geometric ; G01 A_

15.5 Geometric IB

15.5.1 Geometric IB (Automatic calculation of two-arc contact) ; G02/G03 P_Q_ /R_

15.5.2 Geometric IB (Automatic calculation of linear - arc intersection) ; G01 A_ , G02/G03 P_Q_H_

15.5.3 Geometric IB (Automatic calculation of linear - arc intersection) ; G01 A_ , G02/G03 R_H_

15.6 G Command Mirror Image ; G50.1,G51.1

15.7 Normal Line Control ; G40.1/G41.1/G42.1 (G150/G151/G152)

15.8 Manual Arbitrary Reverse Run Prohibition ; G127

15.9 Data Input by Program

15.9.1 Parameter Input by Program ; G10 L70/L100, G11

15.9.2 Compensation Data Input by Program ; G10 L2/L10/L11, G11

15.9.3 Tool Shape Input by Program ; G10 L100, G11

15.9.4 R-Navi Data Input by Program ; G10 L110, G11

15.10 Inputting The Tool Life Management Data ; G10,G11

15.10.1 Inputting The Tool Life Management Data by G10 L3 Command ; G10 L3,G11

15.10.2 Inputting The Tool Life Management Data by G10 L30 Command ; G10 L30,G11

15.10.3 Precautions for Inputting The Tool Life Management Data

15.10.4 Tool Life Management Set Allocation to Part Systems

Multi-part System Control

16.1 Timing Synchronization

16.1.1 Timing Synchronization Operation (! code) !n (!m ...) L

16.1.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115