MITSUBISHI CNC 700/70 Programming Manual

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

Introduction

This manual is a guide for using the MITSUBISHI CNC 700/70 Series. Programming for M2/M0 format is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study the "Precautions for Safety" on the following page to ensure safe use of this NC unit.

Details described in this manual

CAUTION

For items described in "Restrictions" or "Usable State", the instruction manual issued by the machine tool builder takes precedence over this manual.

An effort has been made to note as many special handling methods in this user's manual. Items not described in this manual must be interpreted as "not possible".

This manual has been writt e n o n t h e a ss u m p t i o n t h a t a l l o p t i on f u n c t i on s a r e added. Refer to the specifications issued by the machine tool builder before starting use.

Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.

Some screens and functions may differ depending on the NC system or its version, and some functions may not be possible. Please confirm the specifications before use.

General precautions

(1) Refer to the following documents for details on handling

MITSUBISHI CNC 700/70 Series Instruction Manual ................................. IB-1500042

Precautions for Safety

Always read the specifications issued by the machine maker, 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

WARNING

CAUTION

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

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

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

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

Not applicable in this manual.

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.

An effort has been made to describe special handling of this machine, but items that are not described must be interpreted as "not possible".

This manual is written on the assumption that all option functions are added. Refer to the specifications issued by the machine tool builder before starting use.

Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.

Some screens and functions may differ depending on the NC system or its version, and some functions may not be possible. Please confirm the specifications before use.

DANGER

WARNING

CAUTION

(Continued on next page)

2. Items related to operation

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

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

Turn the mirror image ON and OFF at the mirror image center. Refer to the Instruction Manual issued by each machine tool builder for details on each

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

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

3. Items related to programming

CAUTION

The commands with "no value after G" will be handled as "G00". “EOB", "%", and “EOR” are symbols used for explanation. The actual codes for ISO are "CR,

LF" ("LF") and "%". The programs created on the Edit screen are stored in the NC memory in a "CR, LF" format, however, the 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 a program of the multi-part system, carefully observe the movements

caused by other part systems' programs.

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

1.1 Coordinate Words and Control Axis........................................................................................1

1.2 Coordinate Systems and Coordinate Zero Point Symbols......................................................2

2. Least Command Increments........................................................................................................3

2.1 Input Setting Units...................................................................................................................3

2.2 Input Command Increment Tenfold.........................................................................................5

2.3 Indexing Increment..................................................................................................................6

3. Data Formats.................................................................................................................................7

3.1 Tape Codes.............................................................................................................................7

3.2 Program Formats ..................................................................................................................10

3.3 Tape Memory Format............................................................................................................13

3.4 Optional Block Skip...............................................................................................................13

3.4.1 Optional Block Skip ; /.....................................................................................................13

3.4.2 Optional Block Skip Addition ; /n .......................................................................................14

3.5 Program/Sequence/Block Numbers ; L(O), N.......................................................................16

3.6 Parity H/V..............................................................................................................................17

3.7 G Code Lists .........................................................................................................................18

3.8 Precautions Before Starting Machining.................................................................................21

4. Buffer Register............................................................................................................................22

4.1 Input Buffer............................................................................................................................22

4.2 Pre-read Buffers....................................................................................................................23

5. Position Commands ...................................................................................................................24

5.1 Position Command Methods ; G90, G91 ..............................................................................24

5.2 Inch/Metric Command Change; G20, G21............................................................................26

5.3 Decimal Point Input...............................................................................................................28

6. Interpolation Functions..............................................................................................................33

6.1 Positioning (Rapid Traverse); G00........................................................................................33

6.2 Linear Interpolation; G01.......................................................................................................40

6.3 Plane Selection; G17, G18, G19...........................................................................................42

6.4 Circular Interpolation; G02, G03...........................................................................................44

6.5 R-specified Circular Interpolation; G02, G03........................................................................49

6.6 Helical Interpolation ; G17 to G19, G02, G03.......................................................................52

6.7 Thread Cutting ......................................................................................................................56

6.7.1 Constant Lead Thread Cutting; G33...............................................................................56

6.7.2 Inch Thread Cutting; G33................................................................................................60

6.8 Unidirectional Positioning; G60.............................................................................................61

6.9 Cylindrical Interpolation; G07.1.............................................................................................63

6.10 Polar Coordinate Interpolation; G12.1, G13.1.....................................................................71

6.11 Exponential Function Interpolation; G02.3, G03.3..............................................................78

6.12 Polar Coordinate Command; G16/G15...............................................................................84

6.13 Spiral/Conical Interpolation; G02.0/G03.1(Type1), G02/G03(Type2).................................90

6.14 3-dimensional Circular Interpolation; G02.4, G03.4............................................................95

6.15 NURBS Interpolation.........................................................................................................100

6.16 Hypothetical Axis Interpolation; G07.................................................................................105

7. Feed Functions .........................................................................................................................107

7.1 Rapid Traverse Rate...........................................................................................................107

7.2 Cutting Feedrate .................................................................................................................107

7.3 F1-digit Feed.......................................................................................................................108

7.4 Per-minute/Per-revolution Feed (Asynchronous/Synchronous Feed); G94, G95...............110

7.5 Inverse Time Feed; G93.....................................................................................................112

7.6 Feedrate Designation and Effects on Control Axes............................................................116

7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration.........................................120

7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration........................122

7.9 Exact Stop Check; G09.......................................................................................................131

7.10 Exact Stop Check Mode; G61...........................................................................................134

7.11 Deceleration Check...........................................................................................................134

7.11.1 G1 -> G0 Deceleration Check.....................................................................................136

7.11.2 G1 -> G1 Deceleration Check.....................................................................................137

7.12 Automatic Corner Override ...............................................................................................138

7.13 Tapping Mode; G63 ..........................................................................................................143

7.14 Cutting Mode; G64............................................................................................................143

8. Dwell...........................................................................................................................................144

8.1 Per-second Dwell ; G04......................................................................................................144

9. Miscellaneous Functions .........................................................................................................146

9.1 Miscellaneous Functions (M8-digits BCD)..........................................................................146

9.2 Secondary Miscellaneous Functions (B8-digits, A8 or C8-digits).......................................148

9.3 Index Table Indexing...........................................................................................................149

10. Spindle Functions...................................................................................................................151

10.1 Spindle Functions (S6-digits Analog)................................................................................151

10.2 Spindle Functions (S8-digits) ............................................................................................151

10.3 Constant Surface Speed Control; G96, G97.....................................................................152

10.3.1 Constant Surface Speed Control................................................................................152

10.4 Spindle Clamp Speed Setting; G92..................................................................................153

10.5 Spindle/C Axis Control ......................................................................................................154

10.6 Multiple Spindle Control ....................................................................................................157

10.6.1 Multiple Spindle Control II...........................................................................................158

11. Tool Functions (T command).................................................................................................160

11.1 Tool Functions (T8-digit BCD)...........................................................................................160

12. Tool Compensation Functions ..............................................................................................161

12.1 Tool Compensation...........................................................................................................161

12.2 Tool Length Compensation/Cancel; G43/G44..................................................................165

12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44..................................168

12.4 Tool Radius Compensation; G38, G39/G40/G41,G42......................................................175

12.4.1 Tool Radius Compensation Operation........................................................................176

12.4.2 Other Commands and Operations During Tool Radius Compensation......................185

12.4.3 G41/G42 Commands and I, J, K Designation.............................................................194

12.4.4 Interrupts During Tool Radius Compensation.............................................................200

12.4.5 General Precautions for Tool Radius Compensation..................................................202

12.4.6 Changing of Compensation No. During Compensation Mode....................................203

12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation...............................205

12.4.8 Interference Check .....................................................................................................207

12.4.9 Diameter Designation of Compensation Amount........................................................214

12.4.10 Workpiece Coordinate Changing During Radius Compensation..............................216

12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42.......................................218

12.6 Tool Position Offset; G45 to G48......................................................................................229

12.7 Programmed Compensation Input; G10, G11.1................................................................236

12.8 Compensation Data Input to Variable by Program; G11...................................................241

12.9 Inputting the Tool Life Management Data; G10, G11.......................................................242

12.9.1 Inputting the Tool Life Management Data by G10 L3 Command................................242

12.9.2 Inputting the Tool Life Management Data by G10 L30 Command..............................244

12.9.3 Precautions for Inputting the Tool Life Management Data..........................................247

13. Program Support Functions ..................................................................................................248

13.1 Fixed Cycles......................................................................................................................248

13.1.1 Standard Fixed Cycles; G80 to G89, G73, G74, G75, G76........................................248

13.1.2 Drilling Cycle with High-Speed Retract.......................................................................276

13.1.3 Initial Point and R Point Level Return; G98, G99........................................................279

13.1.4 Setting of Workpiece Coordinates in Fixed Cycle Mode.............................................281

13.2 Special Fixed Cycle; G34, G35, G36, G37 .......................................................................282

13.3 Subprogram Control; G22, G22........................................................................................287

13.3.1 Calling Subprogram with G22 and G22 Commands...................................................287

13.3.2 Figure Rotation; G22 I_ J_ K_....................................................................................291

13.4 Variable Commands..........................................................................................................294

13.5 User Macro Specifications ................................................................................................299

13.5.1 User Macro Commands; G65, G66, G66.1, G67, G68(G23)......................................299

13.5.2 Macro Call Command .................................................................................................300

13.5.3 ASCII Code Macro......................................................................................................309

13.5.4 Variables.....................................................................................................................313

13.5.5 Types of Variables ......................................................................................................315

13.5.6 Arithmetic Commands.................................................................................................353

13.5.7 Control Commands.....................................................................................................358

13.5.8 External Output Commands........................................................................................361

13.5.9 Precautions.................................................................................................................363

13.5.10 Actual Examples of Using User Macros....................................................................365

13.6 G Command Mirror Image; G50.1, G51.1 / G62...............................................................369

13.7 Corner Chamfering/Corner Rounding I.............................................................................372

13.7.1 Corner Chamfering " ,C_ "..........................................................................................372

13.7.2 Corner Rounding " ,R_ ".............................................................................................374

13.8 Linear Angle Command ....................................................................................................375

13.9 Geometric Command........................................................................................................376

13.10 Circle Cutting; G12, G13.................................................................................................380

13.11 Parameter Input by Program; G10, G11.1......................................................................382

13.12 Macro Interrupt; ION, IOF...............................................................................................383

13.13 Tool Change Position Return; G30.1 to G30.6...............................................................391

13.14 Normal Line Control ; G40.1/G41.1/G42.1......................................................................394

13.15 High-accuracy Control ; G61.1, G08...............................................................................405

13.16 High-speed Machining Mode; G05, G05.1......................................................................419

13.16.1 High-speed Machining Mode I,II; G05 P1, G05 P2...................................................419

13.17 High-speed High-accuracy Control; G05, G05.1.............................................................422

13.17.1 High-speed High-accuracy Control I, II.....................................................................422

13.17.2 SSS Control ..............................................................................................................428

13.18 Spline; G05.1 ..................................................................................................................433

13.19 High-accuracy Spline Interpolation ; G61.2.....................................................................440

13.20 Scaling; G50/G51............................................................................................................442

13.21 Coordinate Rotation by Program; G68.1/G69.1..............................................................447

13.22 Coordinate Rotation Input by Parameter; G10................................................................455

13.23 3-dimensional Coordinate Conversion; G68.1/69.1........................................................458

13.24 Tool Center Point Control; G43.4/G43.5.........................................................................475

13.25 Timing-synchronization between Part Systems..............................................................497

13.26 End Point Error Check Cancellation; G69.......................................................................500

13.27 Coordinate Read Function; G14.....................................................................................502

14. Coordinates System Setting Functions................................................................................505

14.1 Coordinate Words and Control Axes.................................................................................505

14.2 Basic Machine, Workpiece and Local Coordinate Systems..............................................506

14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Positions.............................................. 507

14.4 Basic Machine Coordinate System Selection; G53...........................................................508

14.5 Coordinate System Setting; G92.......................................................................................509

14.6 Automatic Coordinate System Setting..............................................................................510

14.7 Reference (Zero) Position Return; G28, G29....................................................................511

14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30.................................................515

14.9 Reference Position Check; G27........................................................................................518

14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1).......................519

14.11 Local Coordinate System Setting; G52...........................................................................531

14.12 Workpiece Coordinate System Preset; G92.1................................................................535

14.13 Coordinate System for Rotary Axis.................................................................................540

15. Measurement Support Functions..........................................................................................543

15.1 Automatic Tool Length Measurement; G37.1...................................................................543

15.2 Skip Function; G31............................................................................................................547

15.3 Multi-step Skip Function; G31.n, G04...............................................................................552

15.4 Multi-step Skip Function 2; G31........................................................................................554

15.5 Speed Change Skip; G31.................................................................................................556

15.6 Programmable Current Limitation .....................................................................................559

15.7 Stroke Check Before Travel; G22.1/G23.1.......................................................................560

Appendix 1. Program Error .......................................................................................................562

Appendix 2. Order of G Function Command Priority..............................................................582

INDEX.............................................................................................................................................X-1

1. Control Axes

1.1 Coordinate Words and Control Axis

Function and purpose

In the standard specifications, there are 3 control axes, but, by adding an additional axis, up to 4 axes can be controlled. The designation of the processing direction responds to those axes and uses a coordinate word made up of alphabet characters that have been decided beforehand.

X-Y table

Program coordinates

Workpiece

1.1 Coordinate Words and Control Axis

X-Y table

Direction o table movement

Bed

Direction o table movement

X-Y and revolving table

rogram coordinates

Direction o movement

table

Workpiece

rection of table

revolution

1. Control Axes

Machi

1.2 Coordinate Systems and Coordinate Zero Point Symbols

Function and purpose

Workpiece coordinate system 3 (G56)

-X

: Reference position

: Machine coordinate zero point

: Workpiece coordinate zero points (G54 - G 59)

Basic machine coordinate system

Workpiece coordinate system 2 (G55)

Workpiece coordinate system 1 (G54)

zero point

st reference

position

Local coordinate

system (G52)

-Y

Workpiece coordinate system 6 (G59)

Workpiece coordinate system 5 (G58)

Workpiece coordinate system 4 (G57)

2. Least Command Increments

2.1 Input Setting Units

Function and purpose

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

With the parameters, the command units are decided for each axis, and the input setting units are decided commonly for all axes.

#1003 iunit = B

Input setting unit

Command unit

(Note 1) Inch/metric changeover is performed in either of 2 ways: conversion from the parameter

screen (#1041 I_inch: valid only when the power is turned ON) and conversion using the G command (G20 or G21).

However, when a G command is used for the conversion, the conversion applies only to

the input command increments and not to the input setting units.

Consequently, the tool offset amounts and other compensation amounts as well as the

variable data should be preset to correspond to inches or millimeters.

(Note 2) The millimeter and inch systems cannot be used together. (Note 3) During circular interpolation on an axis where the input command increments are

different, the center command (I, J, K) and the radius command (R) can be designated by the input setting units. (Use a decimal point to avoid confusion.)

= C = D = E #1015 cunit = 0 Follow #1003 iunit = 1 = 10 = 100 = 1000 = 10000

Parameters

2.1 Input Setting Units

Linear axis

Millimeter Inch

0.001 0.0001 0.001

0.0001 0.00001 0.0001

0.00001 0.000001 0.00001

0.000001 0.0000001 0.000001

0.0001 0.00001 0.0001

0.001 0.0001 0.001

0.01 0.001 0.01

0.1 0.01 0.1

1.0 0.1 1.0

Rotation axis

(°)

2. Least Command Increments

Detailed description

(1) Units of various data

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

2.1 Input Setting Units

Data

Speed data Example: rapid

Position data Example: SoftLimit+

Interpolation unit data

Unit

system

metre Inch

(2) Program command

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

Setting value

1µm (B) 0.1µm (C) 10nm (D) 1nm (E)

20000 (mm/min) 20000 20000 20000 20000Milli-

Setting range 1 to 999999 1 to 999999 1 to 999999 1 to 999999

2000 (inch/min) 2000 2000 2000 2000

Setting range 1 to 999999 1 to 999999 1 to 999999 1 to 999999

123.123 (mm) 123.123 123.1230 123.12300 123.123000MilliSetting range ±99999.999 ±99999.9999 ±99999.99999 ±99999.999999

12.1234 (inch) 12.1234 12.12340 12.123400 12.1234000 Setting range ±9999.9999 ±9999.99999 ±9999.999999 ±9999.9999999

1 (µm) 2 20 200 2000Milli-

Setting range ±9999 ±9999 ±9999 ±9999

0.001 (inch) 2 20 200 2000

Setting range ±9999 ±9999 ±9999 ±9999

Input setting unit

2. Least Command Increments

2.2 Input Command Increment Tenfold

Function and purpose

The program's command increment can be multiplied by an arbitrary scale with the parameter designation. This function is valid when a decimal point is not used for the command increment. The scale is set with the parameters.

Detailed description

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

with a CNC unit for which the command increment is set to 1µm and this function's parameter value is set to "10", machining similar to before this function is possible.

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

with a CNC unit for which the command increment is set to 0.1µm and this function's

parameter value is set to "10", machining similar to before this function is possible. (3) This function cannot be used for the dwell function G04_X_(P_);. (4) This function cannot be used for the compensation amount of the tool compensation input. (5) This function can be used when decimal point type I is valid, but cannot be used when decimal

point type II is valid.

Program example

(Machining program:

programmed with 1=10µm)

(CNC unit is 1=1µm system)

X Y X Y N1 G90 G00 X0 Y0; 0 0 0 0 N2 G91 X-10000 Y-15000; -100.000 -150.000 -10.000 -15.000 N3 G01 X-10000 Y-5000 F500; -200.000 -200.000 -20.000 -20.000 N4 G03 X-10000 Y-10000 J-10000; -300.000 -300.000 -30.000 -30.000 N5 X10000 Y-10000 R5000; -200.000 -400.000 -20.000 -40.000 N6 G01 X20.000 Y.20.000 -180.000 -380.000 0.000 -20.000

2.2 Input Command Increment Tenfold

"UNIT*10" parameter

10 1

-100 -200 -300

UNIT*10 ON

-100

-200

-300

-400

-10 -20 -30

UNIT*10 OFF

-10

-20

-30

-40

2. Least Command Increments

2.3 Indexing Increment

Function and purpose

This function limits the command value for the rotary axis. This can be used for indexing the rotary table, etc. It is possible to cause a program error with a program command other than an indexing increment (parameter setting value).

Detailed description

When the indexing increment (parameter) for limiting the command value is set, the rotary axis can be positioned with that indexing increment. If a program other than the indexing increment setting value is commanded, a program error (P20) will occur. The indexing position will not be checked when the parameter is set to 0.

(Example) When the indexing increment setting value is 2 degrees, only command with the

2-degree increment are possible.

G90 G01 C102. 000 ; … Moves to the 102 degree angle. G90 G01 C101. 000 : … Program error G90 G01 C102 ; … Moves to the 102 degree angle. (Decimal point type II)

The following axis specification parameter is used.

# Item Contents

2106 Index unit Indexing

Precautions

• When the indexing increment is set, degree increment positioning takes place.

• The indexing position is checked with the rotary axis, and is not checked with other axes.

• When the indexing increment is set to 2 degrees, the rotary axis is set to the B axis, and the B

axis is moved with JOG to the 1.234 position, an indexing error will occur if "G90B5." or "G91B5." is commanded.

increment

2.3 Indexing Increment

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

Setting range

(unit)

0 to 360 (° )

3. Data Formats

3.1 Tape Codes

Function and purpose

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

(Note 1) If a code not given in the tape code table in Fig. 1 is assigned during operation, program (Note 2) For the sake of convenience, a semicolon " ; " has been used in the CNC display to

3.1 Tape Codes

error (P32) will result. indicate the end of a block (EOB/IF) which separates one block from another. Do not use

the semicolon key, however, in actual programming but use the keys in the following table instead.

CAUTION

“EOB", "%", and “EOR” are symbols used for explanation. The actual codes for

ISO are "CR, LF" ("LF") and "%". The programs created on the Edit screen are stored in the NC memory in a "CR, LF" format, however, the 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)".

Detailed description

EOB/EOR keys and displays

Key used

End of block LF or NL ; End of record % %

(1) Significant data section (label skip function)

All data up to the first EOB ( ; ), after the power has been turned on or after operation has been

reset, are ignored during automatic operation based on tape, memory loading operation or

during a search operation. In other words, the significant data section of a tape extends from

the character or number code after the initial EOB ( ; ) code after resetting to the point where

the reset command is issued.

Code used

ISO Screen display

3. Data Formats

•••••••

•

•••

•

•••••••••

•

•••••••

•

•••••••••••••••••

•

•••••••••••••••

•••••••••

•

(2) Control out, control in

All data between control out "(" and control in ")" or ";" , from "0" to ";" (when label L) are

ignored, although these data appear on the setting and display unit. Consequently, the

command tape name, No. and other such data not directly related to control can be inserted in

this section.

This information (except (B) in the tape codes) will also be loaded, however, during tape

loading. The system is set to the "control in" mode when the power is witched on.

Example of ISO code

•

3.1 Tape Codes

•

•• ••

• • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • •

•••

• •

• • •• •

Operator information print-out example

L C S L

00X-85000Y-64000 (CUTTE

F R

• ••

•• •• •

••

•••

•

Information in this section is ignored and nothing is executed.

RE T URN)

• •

•• •

•• • ••

•••

•

••••

• • • •

••

•••••

•

The difference of the label and variable code is the following tables.

Code Control in/out range Label (L) Label (O)

ISO/EIA Form "(" to ")" Ignore the data. Ignore the data.

From "O" to "; (EOB)" Ignore the data. The value after "O" will be

handled as label No.

(Note) Always set "O" at the head of the block. A program error (P32) will occur if there is "O"

besides the head of the block.

(3) EOR (%) code

Generally, the end-or-record code is punched at both ends of the tape. It has the following

functions:

(a) Rewind stop when rewinding tape (with tape handler)

(b) Rewind start during tape search (with tape handler)

(4) Tape preparation for tape operation (with tape handler)

10cm

(EOR)

If a tape handler is not used, there is no need for the 2-meter dummy at both ends of the tape

and for the head EOR (%) code.

• • • • • • • •

;;;;

Initial block

• • • • • • • • • • • • • • • •

(EOB)

Last block

(EOB)(EOB)

10cm %

(EOR)(EOB)

3. Data Formats

( (

)

) (

)

ISO code (R-840)

Feed holes

8 7 6 5 4 3 2 1

Channel No.

3.1 Tape Codes

•

••

•

••

•

• •

•• •

•• •• •

• •• ••

•• •• •

• •• • •

• •• ••

•• •• •••

• •

•• •

• •

•• •• •

• •• • •

• •• ••

•• •• •••

•• ••

• ••

• ••• •

•

•• ••• ••

•• ••• • •

•

• •• • •

• •

•

••

Code A are stored on tape but an error results (except when they are used in the comment

section) during operation.

The B codes are non-working codes and are always ignored. Parity V check is not executed.

•

•• •

•• • •

•• ••

•• •••

•

••

•

••

•

• •

•

••

•

•••

•

•• ••

•• • •

•• ••

•• •

•• •••

•• • •

•• •

•

••• •

•

•• •

••• • •

•

••

•

•••

••• ••

••• •

••• ••

••• •••

•

••• •••

•

••• •••

•

••

4 5 6 7 8 9

•

••

D E F G H I

•

J K L M N O P Q

•

••

T U V W X

•

Z +

. , / % LF(Line Feed) or NL

Control Out Control In

•

: #

••

* = [ ] SP(Space CR(Carriage Return) BS(Back Space HT(Horizontal Tab

•

& !

•

$ ' (Apostrophe)

; < > ?

•

DEL(Delete NULL DEL(Delete

• Under the ISO code, IF or NL is EOB and % is EOR.

• Under the ISO code, CR is meaningless, and EOB will not occur.

Table of tape codes

3. Data Formats

Alp

)

3.2 Program Formats

Function and purpose

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

Detailed descripti on

(1) Word and address

A word is a collection of characters arranged in a specific sequence. This entity is used as the

unit for processing data and for causing the machine to execute specific operations. Each

word used for this controller consists of an alphabet letter and a number of several digits

(sometimes with a "-" sign placed at the head of the number.).

3.2 Program Formats

Word

Numerals

habet (address

Word configuration

The alphabet letter at the head of the word is the address. It defines the meaning of the

numerical information which follows it.

For details of the types of words and the number of significant digits of words used for this

controller, refer to the "format details".

(2) Blocks

A block is a collection of words. It includes the information which is required for the machine to

execute specific operations. One block unit constitutes a complete command. The end of each

block is marked with an EOB (end-of-block) code.

(Example 1)

G0X - 1000 ; G1X - 2000F500 ;

(Example 2)

(G0X - 1000 ; ) G1X - 2000F500 ;

(3) Programs

A program is a collection of several blocks.

2 blocks

Since the semicolon in the parentheses will not result in an EOB, it is 1 block.

3. Data Formats

Program No. L(O)8 Sequence No. N6 Preparatory function G3/G21

Movement axis

Arc and cutter radius

Dwell

Feed function (Feed per minute)

Feed function (Feed per revolution)

Tool compensation Miscellaneous function (M) Spindle function (S) Tool function (T) 2nd miscellaneous function A8/B8/C8 Subprogram

Fixed cycle

0.001(°) mm/

0.001 inch

0.0001(°) mm/

0.0001 inch

0.00001(°) mm/

0.00001 inch

0.000001(°) mm/

0.000001 inch

0.001(°) mm/

0.001 inch

0.0001(°) mm/

0.0001 inch

0.00001(°) mm/

0.00001 inch

0.000001(°) mm/

0.000001 inch

0.001(rev)/(s)

0.001(°) mm/

0.001 inch

0.0001 (°) mm/

0.0001 inch

0.00001 (°) mm/

0.00001 inch

0.000001 (°) mm/

0.000001 inch

0.0001(°) mm/

0.0001 inch

0.00001 (°) mm/

0.00001 inch

0.000001 (°) mm/

0.000001 inch

0.0000001 (°) mm/

0.0000001 inch

0.001(°) mm/

0.001 inch

0.0001(°) mm/

0.0001 inch

0.00001(°) mm/

0.00001 inch

0.000001(°) mm/

0.000001 inch

Metric command Inch command

X+53 Y+53 Z+53 α+53 X+44 Y+44 Z+44 α+44 X+53 Y+53 Z+53 α+53 X+53 Y+53 Z+53 α+53 X+54 Y+54 Z+54 α+54 X+45 Y+45 Z+45 α+45 X+54 Y+54 Z+54 α+54 X+54 Y+54 Z+54 α+54 X+55 Y+55 Z+55 α+55 X+46 Y+46 Z+46 α+46 X+55 Y+55 Z+55 α+55 X+55 Y+55 Z+55 α+55 X+56 Y+56 Z+56 α+56 X+47 Y+47 Z+47 α+47 X+56 Y+56 Z+56 α+56 X+56 Y+56 Z+56 α+56

I+53 J+53 K+53 I+44 J+44 K+44 I+53 J+53 K+53 I+54 J+54 K+54 I+45 J+45 K+45 I+54 J+54 K+54 I+55 J+55 K+55 I+46 J+46 K+46 I+55 J+55 K+55 I+56 J+56 K+56 I+47 J+47 K+47 I+56 J+56 K+56

X53/P8

F63 F54 F63 F54 (Note 6) F64 F55 F64 F55 (Note 6) F65 F56 F65 F56 (Note 6) F66 F57 F66 F57 (Note 6) F33 F34 F33 F34 (Note 6) F34 F35 F34 F35 (Note 6) F35 F36 F35 F36 (Note 6) F36 F37 F36 F37 (Note 6)

H3 D3

M8 S8

P8 H5 L4

R+53 Q53 P8 L4 R+44 Q44 P8 L4 R+53 Q53 P8 L4 R+53 Q53 P8 L4 R+54 Q54 P8 L4 R+45 Q45 P8 L4 R+54 Q54 P8 L4 R+54 Q54 P8 L4 R+55 Q55 P8 L4 R+46 Q46 P8 L4 R+55 Q55 P8 L4 R+55 Q55 P8 L4 R+56 Q56 P8 L4 R+47 Q47 P8 L4 R+56 Q56 P8 L4 R+56 Q56 P8 L4

3.2 Program Formats

Rotary axis

(Metric command)

← ← ← ← ← ← ← ← ←

← ← ←

← ← ← ← ← ← ← ← ← ← ← ← ← ← ← ← ← ←

Rotary axis

(Inch command)

I+53 J+53 K+53 I+54 J+54 K+54 I+55 J+55 K+55 I+56 J+56 K+56

(Note 5)

(Note 5) (Note 5) (Note 5)

(Note 1) α indicates the additional axis address, such as A, B or C. (Note 2) The number of digits check for a word is carried out with the maximum number of digits of that address. (Note 3) Numerals can be used without the leading zeros.

3. Data Formats

3.2 Program Formats

(Note 4) The description of the brief summary is explained below:

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

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

G00 X45.123 ;

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

(Note 5) If an arc is commanded using a rotary axis and linear axis while inch commands are being used, the

degrees will be converted into 0.1 inches for interpolation.

(Note 6) While inch commands are being used, the rotary axis speed will be in increments of 10 degrees.

Example: With the F1. (per-minute-feed) command, this will become the 10 degrees/minute command.

(Note 7) The decimal places below the decimal point are ignored when a command, such as an S command,

with an invalid decimal point has been assigned with a decimal point.

(Note 8) This format is the same for the value input from the memory, MDI or setting and display unit. (Note 9) Command the program No. in an independent block. Command the program No. in the head block of

the program.

(Note 10) The addresses of the program No. and subprogram call No. differ according to the parameter. The system must be formatted when this parameter is changed.

Setting of

“#11009 M2 labelO”

0 L L 1 O A

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

Address of the

program No.

Address to call the

subprogram

3. Data Formats

3.3 Tape Memory Format

Function and purpose

(1) Storage tape and significant sections

The others are about from the current tape position to the EOB. Accordingly, under normal conditions, operate the tape memory after resetting. The significant codes listed in "Table of tape codes" in "3.1 Tape Codes" in the above significant section are actually stored into the memory. All other codes are ignored and are not stored. The data between control out "(" and control in ")" are stored into the memory.

3.4 Optional Block Skip

3.4.1 Optional Block Skip ; /

Function and purpose

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

Detailed description

3.3 Tape Memory Format

(1) Provided that the optional block skip switch is ON, blocks starting with the "/" code are ignored.

They are executed if the switch is OFF. Parity check is valid regardless of whether the optional block skip switch is ON or OFF. When, for instance, all blocks are to be executed for one workpiece but specific block are not to be executed for another workpiece, the same command tape can be used to machine different parts by inserting the "/" code at the head of those specific blocks.

Precautions for using optional block skip

(1) Put the "/" code for optional block skip at the beginning of a block. If it is placed inside the block,

it is assumed as a user macro, a division instruction.

Example : N20 G1 X25./Y25. ;....NG (User macro, a division instruction; a program error

results.)

/N20 G1 X25. Y25. ;.....OK

(2) Parity checks (H and V) are conducted regardless of the optional block skip switch position. (3) The optional block skip is processed immediately before the pre-read buffer.

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

buffer. (4) This function is valid even during a sequence number search. (5) All blocks with the "/" code are also input and output during tape storing and tape output,

regardless of the position of the optional block skip switch.

3. Data Formats

3.4.2 Optional Block Skip Addition ; /n

Function and purpose

Whether the block with "/n (n:1 to 9)" (slash) is executed during automatic operation and searching is selected. By using the machining program with "/n" code, different parts can be machined by the same program.

Detailed description

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

Example of program

(1) When the 2 parts like the figure below are machined, the following program is used. When the

optional block skip 5 signal is ON, the part 1 is created. When the optional block skip 5 signal is

OFF, the part 2 is created.

N1 G54;

N2 G90G81X50. Z-20. R3. F100;

/5 N3 X30.;

N4 X10.;

N5 G80;

M02;

Part 1 the optional block skip 5 signal ON

3.4 Optional Block Skip

Part 2 the optional block skip 5 signal OFF

N4 N2 N2 N3

3. Data Formats

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

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

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

(3) When the parameter "#1226 aux10/bit1" is "1", when two or more "/n" are commanded inside

the same block, the commands following "/n" in the block are ignored if either of the optional block skip signal corresponding to the command is ON.

N01 G91 G28 X0.Y0.Z0.; N02 G01 F1000; N03 X1. /1 Y1. /2 Z1.; N04 M30;

3.4 Optional Block Skip

(a) Optional block skip 1 signal ON

(Optional block skip 2, 3 signals OFF)

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

(Optional block skip 1, 3 signals OFF)

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

(Optional block skip 1, 2 signals OFF)

N01 -> N02 -> N03 -> N04 -> N11 -> N12

(a) When the optional block skip 1 signal is

ON and the optional block skip 2 signal is OFF, "Y1. Z1." is ignored

(b) When the optional block skip 1 signal is

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

3. Data Formats

3.5 Program/Sequence/Block Numbers ; L(O), N

Function and purpose

These numbers are used for monitoring the execution of the machining programs and for calling both machining programs and specific stages in machining programs. (1) Program numbers are classified by workpiece correspondence or by subprogram units, and

they are designated by the address "L" (or "0") followed by a number with up to 8 digits. (2) Sequence numbers are attached where appropriate to command blocks which configure

machining programs, and they are designated by the address "N" followed by a number with

up to 6 digits. (3) Block numbers are automatically provided internally. They are preset to zero every time a

program number or sequence number is read, and they are counted up one at a time unless

program numbers or sequence numbers are commanded in blocks which are subsequently

read. Consequently, all the blocks of the machining programs given in the table below can be

determined without further consideration by combinations of program numbers, sequence

numbers and block numbers.

Machining program

L12345678 (DEMO, PROG) ; 12345678 0 0 G92 X0 Y0 ; 12345678 0 1 G90 G51 X-150. P0.75 ; 12345678 0 2 N100 G00 X-50. Y-25. ; 12345678 100 0 N110 G01 X250. F300 ; 12345678 110 0 Y-225. ; 12345678 110 1 X-50. ; 12345678 110 2 Y-25.; 12345678 110 3 N120 G51 Y-125. P0.5 ; 12345678 120 0 N130 G00 X-100. Y-75. ; 12345678 130 0 N140 G01 X-200. ; 12345678 140 0 Y-175. ; 12345678 140 1 X-100. ; 12345678 140 2 Y-75. ; 12345678 140 3 N150 G00 G50 X0 Y0 ; 12345678 150 0 N160 M02 ; 12345678 160 0 %

Program No. Sequence No. Block No.

Monitor display

3. Data Formats

•

• • •

• • • • • • • • • • • • •

•

• •

•

• • •

• •

•

• • •

•

• •

•

• • • • • • • • •

•

• •

• • •

3.6 Parity H/V

Function and purpose

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

(1) Parity H

3.6 Parity H/V

Parity H checks the number of holes configuring a character and it is done during tape

operation, tape input and sequence number search.

A parity H error is caused in the following cases.

(a) ISO code

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

(b) EIA code

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

Parity H error example

• • • •

•

• • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • •

• • • • • • • • • • • • • • •

•

• • • • • • • • •

• • •

(2) Parity V

• • • • •

• • • • • • • • • • • • • • • • •

• • • • • • • • • • • • • •

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

A parity V check is done during tape operation, tape input and sequence number search when

the I/O PARA #9n15 (n is the unit No.1 to 5) parity V check function is set to "1". It is not done

during memory operation.

A parity V error occurs in the following case: when the number of codes from the first

significant code to the EOB (;) in the significant data section in the vertical direction of the tape

is an odd number, that is, when the number of characters in one block is odd.

When a parity V error is detected, the tape stops at the code following the EOB (;).

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

(Note 2) Any space codes which may appear within the section from the initial EOB code to

• •

• • • • • • • • • •

•

• • • •

• • •

• • • • • • •

This character causes a parity H error.

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

the address code or "/" code are counted for parity V check.

3. Data Formats

3.7 G Code Lists

Function and purpose

G code Group Function

Δ 00 01 Positioning 6.1 Δ 01 01 Linear interpolation 6.2

02 01

03 01

02.1 01 Spiral/Conical interpolation CW (type1) 6.13

03.1 01 Spiral/Conical interpolation CCW (type1) 6.13

02.3 01 Exponential function interpolation positive rotation 6.11

03.3 01 Exponential function interpolation negative rotation 6.11

02.4 01 3-dimensional circular interpolation 6.14

03.4 01 3-dimensional circular interpolation 6.14

04 00 Dwell 8.1

05 00

05.1 00

06.2 01 NURBS interpolation 6.15

07 00

07.1 107

08 00 High-accuracy control 13.15 09 00 Exact stop check 7.9

10 00

11.1 00 Program data input cancel 11 00 Program compensation data input to variable 12.8

12 00 Circular cut CW (clockwise) 13.10 13 00 Circular cut CCW (counterclockwise) 13.10

12.1 21 Polar coordinate interpolation ON 6.10

* 13.1 21 Polar coordinate interpolation cancel 6.10

14 00 Coordinate data read 13.27

* 15 18 Polar coordinate command OFF 6.12

16 18 Polar coordinate command ON 6.12

Δ 17 02 Plane selection X-Y 6.3 Δ 18 02 Plane selection Z-X 6.3 Δ 19 02 Plane selection Y-Z 6.3 Δ 20 06 Inch command 5.2 Δ 21 06 Metric command 5.2

3.7 G Code Lists

Section

Circular interpolation CW (clockwise) R-specified circular interpolation CW Helical interpolation CW Spiral/Conical interpolation CW (type2) Circular interpolation CCW (counterclockwise) R-specified circular interpolation CCW Helical interpolation CCW Spiral/Conical interpolation CCW (type2)

High-speed machining mode High-speed high-accuracy control II High-speed high-accuracy control I Spline

Hypothetical axis interpolation

21 Cylindrical interpolation 6.9

Program data input (parameter /compensation data/parameter coordinate rotation data)

6.4

6.5

6.6

6.13

6.4

6.5

6.6

6.13

13.16

13.17

13.18

6.16

12.7

13.11

13.22

12.7

13.11

3. Data Formats

3.7 G Code Lists

G code Group Function

22 00 Subprogram call / figure rotation ON 13.3 23 00 Subprogram return / figure rotation cancel 13.3

22.1 04 Stroke check before travel ON 15.7

23.1 04 Stroke check before travel cancel 15.7 24 25 26 27 00 Reference position check 14.9 28 00 Reference position return 14.7 29 00 Start position return 14.7 30 00 2nd to 4th reference position return 14.8

30.1 00 Tool change position return 1 13.13

30.2 00 Tool change position return 2 13.13

30.3 00 Tool change position return 3

30.4 00 Tool change position return 4 13.13

30.5 00 Tool change position return 5 13.13

30.6 00 Tool change position return 6 13.13 31 00 Skip

Multi-step skip function 2

31.1 00 Multi-step skip function 1-1 15.3

31.2 00 Multi-step skip function 1-2 15.3

31.3 00 Multi-step skip function 1-3 15.3 32 33 01 Thread cutting 6.7 34 00 Special fixed cycle (bolt hole circle) 13.2 35 00 Special fixed cycle (line at angle) 13.2 36 00 Special fixed cycle (arc) 13.2 37 00 Special fixed cycle (grid) 13.2

37.1 00 Automatic tool length measurement 15.1 38 00 Tool radius compensation vector designation 12.4 39 00 Tool radius compensation corner arc 12.4

* 40 07

41 07

42 07

* 40.1 15 Normal line control cancel 13.14

41.1 15 Normal line control left ON 13.14

42.1 15 Normal line control right ON 13.14 43 08 Tool length compensation 12.2

* 44 08

43.1 08 Tool length compensation along the tool axis 12.3

43.4 08 Tool center point control type 1 13.24

43.5 08 Tool center point control type 2 13.24 45 00 Tool position offset (extension) 12.6 46 00 Tool position offset (reduction) 12.6 47 00 Tool position offset (doubled) 12.6 48 00 Tool position offset (halved) 12.6 49

Tool radius compensation cancel 3-dimentional tool radius compensation cancel Tool radius compensation left 3-dimentional tool radius compensation left Tool radius compensation right 3-dimentional tool radius compensation right

Tool length compensation cancel Tool center point control cancel

Section

13.13

15.2

15.4

12.4

12.5

12.4

12.5

12.4

12.5

12.2

13.24

3. Data Formats

3.7 G Code Lists

G code Group Function

* 50 11 Scaling cancel 13.20

51 11 Scaling ON 13.20

* 50.1 19 G command mirror image cancel 13.6

51.1 19 G command mirror image ON 13.6 52 00 Local coordinate system setting 14.11 53 00 Basic machine coordinate system selection 14.4

* 54 12 Workpiece coordinate system 1 selection 14.10

55 12 Workpiece coordinate system 2 selection 14.10 56 12 Workpiece coordinate system 3 selection 14.10 57 12 Workpiece coordinate system 4 selection 58 12 Workpiece coordinate system 5 selection 59 12 Workpiece coordinate system 6 selection

54.1 12 Workpiece coordinate system selection 48 / 96 sets extended 60 00 Unidirectional positioning 61 13 Exact stop check mode

61.1 13 High-accuracy control 1 ON

61.2 13 High-accuracy spline interpolation 13.19 62 19 G command mirror image 63 13 Tapping mode

63.1 13 Synchronous tapping mode (normal tapping)

63.2 13 Synchronous tapping mode (reverse tapping)

* 64 13 Cutting mode 7.14

65 00 User macro call 13.5.1 66 14 User macro modal call A 13.5.1

66.1 14 User macro modal call B 13.5.1

* 67 14 User macro modal call cancel 13.5.1

68 00 Subprogram return 13.5.1 69 00 End point error check cancellation 13.26

68.1 16

* 69.1 16

70 09 User fixed cycle 71 09 User fixed cycle 72 09 User fixed cycle 73 09 Fixed cycle (step) 13.1.1 74 09 Fixed cycle (reverse tap) 13.1.1 75 09 Fixed cycle (circle cutting cycle) 13.1.1 76 09 Fixed cycle (fine boring) 13.1.1 77 09 User fixed cycle 78 09 User fixed cycle 79 09 User fixed cycle

* 80 09 Fixed cycle cancel 13.1.1

81 09 Fixed cycle (drill/spot drill) 13.1.1 82 09 Fixed cycle (drill/counter boring) 13.1.1 83 09 Fixed cycle (deep drilling) 13.1.1 84 09 Fixed cycle (tapping) 13.1.1 85 09 Fixed cycle (boring) 13.1.1 86 09 Fixed cycle (boring) 13.1.1 87 09 Fixed cycle (back boring) 13.1.1 88 09 Fixed cycle (boring) 13.1.1 89 09 Fixed cycle (boring) 13.1.1

Programmable coordinate rotation mode ON/3-dimensional coordinate conversion mode ON Programmable coordinate rotation mode OFF/3-dimensional coordinate conversion mode OFF

Section

14.10

6.8

7.10

13.15

13.6

7.13

13.21

13.23

13.21

13.23

3. Data Formats

3.8 Precautions Before Starting Machining

G code Group Function

Δ 90 03 Absolute value command 5.1 Δ 91 03 Incremental command value 5.1

92 00 Coordinate system setting / Spindle clamp speed setting 14.5

92.1 00 Workpiece coordinate system pre-setting 14.12 93 05 Inverse time feed 7.5

Δ 94 05 Per-minute feed (asynchronous feed) 7.4 Δ 95 05 Per-revolution feed (synchronous feed) 7.4 Δ 96 17 Constant surface speed control ON 10.3 Δ 97 17 Constant surface speed control OFF 10.3

* 98 10 Fixed cycle Initial level return 13.1.2

99 10 Fixed cycle R point level return 13.1.2

100 to

255

(Note 1) Codes marked with * are codes that must be or are selected in the initial state. The codes marked with Δ are codes that should be or are selected in the initial state by

(Note 2) If two or more G codes from the same code are commanded, the latter G code will be (Note 3) This G code list is a list of conventional G codes. Depending on the machine, movements

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

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

the parameters. valid. that differ from the conventional G commands may be included when called by the G

code macro. Refer to the Instruction Manual issued by the tool builder.

(1) "Reset 1"

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

(2) "Reset 2" and "Reset & rewind"

The modal is initialized when the signal is input.

(3) Resetting when emergency stop is canceled

Follows "Reset 1".

(4) When modal is automatically reset at the start of individual functions such as

reference position return. Follows "Reset & rewind".

Section

CAUTION

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

3.8 Precautions Before Starting Machining

Precautions before starting machinin

CAUTION

When creating the machining program, select the appropriate machining conditions so that the

machine, NC performance, capacity and limits are not exceeded. The examples do not allow for the machining conditions.

Before starting actual machining, always carry out dry operation to confirm the machining

program, tool compensation amount and workpiece offset amount, etc.

4. Buffer Register

Analysi

4. Buffer Register

4.1 Input Buffer

Tape

Function and purpose

When the pre-read buffer is empty during a tape operation or RS232C operation, the contents of the input buffer are immediately transferred to the pre-read buffers and, provided that the data stored in the input buffer do not exceed 250 x 4 characters, the following data (Max. 250 characters) are read and loaded into the input buffer. This buffer is designed to eliminate the operational delay originating in the readout time of the tape reader and to smooth out the block joints. The pre-reading effects are lost, however, when the block execution time is shorter than the tape readout time of the following block.

(Buffer size : 250 x 5 characters)

Input buffe

4.1 Input Buffer

s processing

Max. 5 execution blocks

Pre-read buffer 5

Keyboard

Buffer 4

Memor

MDI data

Mode switching

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

Buffer 3

Buffer 2

Buffer 1

rithmetic

processing

The input buffer has a memory capacity of 250 x 5 characters (including the EOB code). (1) The contents of the input buffer register are updated in 250-character units.

(2) Only the significant codes in the significant data section are read into the input buffer. (3) When codes (including "(" and ")") are sandwiched in the control in or control out mode and the

optional block skip function is ON, the data extending from the "/" (slash) code up to the EOB code are read into the input buffer.

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

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

4. Buffer Register

4.2 Pre-read Buffers

Function and purpose

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

(1) The data of 1 block are stored in this buffer. (2) Only the significant codes in the significant data section are read into the pre-read buffer. (3) When codes are sandwiched in the control in and control out, and the optional block skip

function is ON, the data extending from the "/" (slash) code up to the EOB code are not read into the pre-read buffer.

(4) The pre-read buffer contents are cleared with resetting. (5) When the single block function is ON during continuous operation, the pre-read buffer stores

the following block data and then stops operation.

Other precautions

4.2 Pre-read Buffers

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

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

(2) If the external control signal such as optional block skip is turned ON/OFF with the M

command, the external control operation will not be effective on the program pre-read with the buffer register.

(3) According to the M command that operates the external controls, it prohibits pre-reading, and

the recalculation is as follows:

The M command that commands the external controls is distinguished at the PLC, and the

"recalculation request" for PLC -> NC interface table is turned ON.

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

5. Position Commands

5.1 Position Command Methods ; G90, G91

Function and purpose

By using the G90 and G91 commands, it is possible to execute the next coordinate commands using absolute values or incremental values. The R-designated circle radius and the center of the circle determined by I, J, K are always incremental value commands.

Command format

G9D X__ Y__ Z__ α__;

G90 :Absolute command G91 :Incremental command α :Additional axis

Detailed description

(1) Regardless of the current position, in the absolute

value mode, it is possible to move to the position of the workpiece coordinate system that was designated in the program.

N 1 G90 G00 X0 Y0 ;

5.1 Position Command Methods ; G90, G91

200.

Tool

100.

In the incremental value mode, the current position is the start point (0), and the movement is made only the value determined by the program, and is expressed as an incremental value.

100.

200.

300.

N 2 G90 G01 X200. Y50. F100; N 2 G91 G01 X200. Y50. F100;

Using the command from the 0 point in the workpiece coordinate system, it becomes the same coordinate command value in either the absolute value mode or the incremental value mode.

(2) For the next block, the last G90/G91 command that

was given becomes the modal.

(G90)

N 3 X100. Y100.;

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

200.

100. N3

Y = 100mm position.

(G91)

100.

200.

N 3 X-100. Y50.;

300.

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

5. Position Commands

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

addresses as either absolute values or incremental values.

N 4 G90 X300. G91 Y100.;

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

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

commands or incremental value commands with the #1073 I_Absm parameter.

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

that block.

5.1 Position Command Methods ; G90, G91

200.

100.

200. 100.

300.

5. Position Commands

5.2 Inch/Metric Command Change; G20, G21

Function and purpose

These G commands are used to change between the inch and millimeter (metric) systems.

Command format

G20/G21;

G20 : Inch command G21 : Metric command

Detailed description

The G20 and G21 commands merely select the command units. They do not select the Input units. G20 and G21 selection is meaningful only for linear axes and it is meaningless for rotation axes.

Output unit, command unit and setting unit

The counter or parameter setting and display unit is determined by parameter "#1041 I_inch". For the movement/speed command, the followings will be resulted: The movement/speed command will be displayed as metric units when "#1041 I_inch" is ON during the G21 command mode. The internal unit metric data of the movement/speed command will be converted into an inch unit and displayed when "#1041 I_inch" is OFF during the G20 command mode. The command unit for when the power is turned ON and reset is decided by combining the parameters "#1041 I_inch", "#1151 rstint" and "#1210 RstGmd/bit5".

NC axis

Item

Movement/ speed command

Counter display Metric Metric Inch Inch Speed display Metric Metric Inch Inch User parameter

setting/display Workpiece/

tool offset setting/display

Handle feed command

PLC axis

Item

Movement/ speed command

Counter display Metric Inch User parameter

setting/display

Initial inch OFF

(metric internal unit)

#1041 I_inch=0

G21 G20 G21 G20

Metric Inch Metric Inch

Metric Metric Inch Inch

#1042 pcinch=0

(metric)

Metric Inch

Initial inch ON

(inch internal unit)

#1041 I_inch=1

#1042 pcinch=1

(inch)

5. Position Commands

Precautions

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

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

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

G20/G21 command modal.

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

G code. Command in a separate block. G05 (High-speed machining mode) G7.1 (Cylindrical Interpolation) G12.1 (Polar coordinate interpolation)

5.2 Inch/Metric Command Change; G20, G21

5. Position Commands

5.3 Decimal Point Input

Function and purpose

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

Detailed description

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

in machining programs. (Note, only after G51)

(2) In decimal point input type 1 and type 2, the values of the data commands without the decimal

points are shown in the table below.

Command Command unit Type 1 Type 2

X1 ;

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

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

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

command unit cunit = 10)

Input unit

[mm]

Input unit

[inch]

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

subprograms.

(6) While the smallest decimal point command is validated, the smallest unit for a command

without a decimal point designation is the smallest command input unit set in the specifications (1µm, 10µm, etc.) or mm can be selected. This selection can be made with parameter "#1078 Decpt2".

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

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

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

decimal point type II mode.

5.3 Decimal Point Input

cunit = 10000 1000 (µm, 10-4 inch, 10-3 °) 1 (mm, inch, °) cunit = 1000 100 1 cunit = 100 10 1 cunit = 10 1 1

Movement

command (linear)

-99999.999 to

99999.999

-9999.9999 to

9999.9999

Movement

command (rotary)

-99999.999 to

99999.999

Feedrate Dwell

0. 001 to

10000000.000

0. 0001 to

1000000.0000

0 to 99999.999

5. Position Commands

Example of program

(1) Example of program for decimal point valid address

Program example

G0X123.45 (decimal points are all mm points)

G0X12345

#111 = 123, #112 = 5.55 X#111 Y#112 #113 = #111+#112 (addition) #114 = #111-#112 (subtraction)

#115 = #111∗#112 (multiplication) #116 = #111/#112 #117 = #112/#111 (division)

Decimal point input I/II and decimal point command valid/invalid

If a command does not use a decimal point at an address where a decimal point command is valid in the table on the following page, it is handled differently between decimal point input I and II modes as explained below. A command using a decimal point is handled the same way in either the decimal point input I or II mode.

(1) Decimal point input I

The least significant digit place of command data corresponds to the command unit. (Example) Command "X1" in the 1μm system is equivalent to command "X0.001".

(2) Decimal point input II

The least significant digit place of command data corresponds to the decimal point.

(Example) Command "X1" in the 1μm system is equivalent to command "X1.". (Note) When a four rules operator is contained, the data will be handled as that with a decimal

Specification

point.

division

5.3 Decimal Point Input

Decimal point command 1

When 1 = 1μm When 1 = 10μm

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

X12.345mm (last digit is 1μm unit) X123.000mm, Y5.550mm

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

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

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

#116 = 22.162 #117 = 0.045

X123.450mm X12345.000mm

X123.000mm, Y5.550mm

#116 = 22.162 #117 = 0.045

Decimal point

command 2

1 = 1mm

X123.000mm, Y5.550mm

#116 = 22.162 #117 = 0.045

(Example) When the min. input command unit is 1μm :

G0 x 123 + 0 ; ... X axis 123mm command. It will not be 123μm.

5. Position Commands

5.3 Decimal Point Input

Addresses used and validity/invalidity of decimal point commands are shown below.

Address

Decimal point

command

Application

A Valid Coordinate position data Invalid Revolving table Invalid Miscellaneous function code Valid Angle data Invalid Data settings, axis numbers (G10) Invalid Subprogram call : program No. (label O)

B Valid Coordinate position data

Invalid Revolving table Invalid Miscellaneous function code

C Valid Coordinate position data

Invalid Revolving table Invalid Miscellaneous function code

Valid Corner chamfering amount ,c

D Invalid Compensation numbers (tool position, tool radius) Valid Automatic tool length measurement: deceleration

distance d Invalid Data setting: byte type data Invalid Subprogram storing device number ,D

E Valid Inch thread: number of ridges,

precision thread: lead

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

F Valid Feedrate, automatic tool length measurement speed Valid Thread lead Valid Number of Z axis pitch in synchronous tap

G Valid Preparatory function code

H Invalid Tool length compensation number

Invalid Sequence number in subprogram (label L, O) Invalid Subprogram return destination sequence No. (label L, O) Invalid Program parameter input: bit type data Invalid Basic spindle selection

I Valid Arc center coordinates

Invalid Center of figure rotation (incremental) Valid Tool radius compensation vector components Valid Hole pitch in the special fixed cycle Valid Circle radius of cut circle (increase amount) Valid G0/G1 imposition width, drilling cycle G0 imposition width ,I Valid Stroke check before travel: lower limit coordinates

Remarks

5. Position Commands

5.3 Decimal Point Input

Address

Decimal point

command

Application

J Valid Arc center coordinates

Invalid Center of figure rotation (incremental) Valid Tool radius compensation vector components Valid Special fixed cycle's hole pitch or angle Valid G0/G1 imposition width, drilling cycle G1 imposition width Valid Stroke check before travel: lower limit coordinates

K Valid Arc center coordinates

Invalid Center of figure rotation (incremental) Valid Tool radius compensation vector components Invalid Number of holes of the special fixed cycle Invalid Number of drilling cycle repetitions Valid Stroke check before travel: lower limit coordinates

L Invalid Subprogram call program No. (label L)

Invalid Program tool compensation input/workpiece offset input:

type selection

Invalid Program parameter input: data setting selection L70 Invalid Program parameter input: 2-word type data 4 bytes Invalid Tool life data

M Invalid Miscellaneous function codes N Invalid Sequence numbers

Invalid Program parameter input: data numbers

O Invalid Program numbers (label O)

P Invalid/Valid Dwell time Parameter Invalid Subprogram call : number of repetition (label L, O) Invalid/Valid Dwell at tap cycle hole base Parameter Invalid Number of holes of the special fixed cycle (label L) Invalid Amount of helical pitch Invalid Offset number (G10) Invalid Constant surface speed control axis number Invalid Program parameter input: broad classification number Invalid Multi-step skip function 2 signal command Invalid 2nd, 3rd, 4th reference position return number Valid Scaling magnification Invalid High-speed mode type Invalid Type of the coordinate to be read Invalid Transmission source compensation No. of program

compensation data input to variable Invalid Extended workpiece coordinate system No. Invalid Tool life data group No.

Remarks

L2, L20, L12, L10, L13,

L11

5. Position Commands

5.3 Decimal Point Input

Address

Decimal point

command

Application

Q Valid Cut amount of deep hole drill cycle Valid Shift amount of back boring Valid Shift amount of fine boring Invalid Minimum spindle clamp speed Valid Starting shift angle for screw cutting Invalid Transmission destination variable No. of program

compensation data input to variable

Invalid Tool life data management method

R Valid R-point in the fixed cycle Valid R-specified arc radius Valid Corner R arc radius ,R Valid Offset amount (G10) Invalid Synchronous tap/asynchronous tap changeover Valid Automatic tool length measurement: deceleration

distance r

Valid Rotation angle

S Invalid Spindle function codes Invalid Maximum spindle clamp speed Invalid Constant surface speed control: surface speed Invalid Program parameter input: word type data 2

T Invalid Tool function codes

U Valid Coordinate position data

V Valid Coordinate position data

W Valid Coordinate position data

X Valid Coordinate position data Valid Dwell time

Y Valid Coordinate position data

Z Valid Coordinate position data

(Note 1) All decimal points are valid for the user macro arguments.

Remarks

bytes

6. Interpolation Functions

6.1 Positioning (Rapid Traverse); G00

Function and purpose

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

Command format

G00 X__ Y__ Z__ α__ ; (α represents additional axis)

X, Y, Z, α : Represent coordinates, and could be either absolute values or

Detailed description

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

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

(2) In the G00 mode, the tool is always accelerated at the start point of the block and decelerated

at the end point. Having no more command pulse in the current block and the following error status of the acceleration/deceleration paths are confirmed before advancing to the next block.

The in-position width is set with the parameters. (3) Any G command (G72 to G89) in the 09 group is cancelled (G80) by the G00 command. (4) The tool path can be selected from linear or non-linear.

The positioning time is the same for the linear and non-linear paths.

(a) Linear path......... : This is the same as linear interpolation (G01), and the speed is limited

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

incremental values, depending on the setting of G90/G91.

by the rapid traverse rate of each axis. axis.

6.1 Positioning (Rapid Traverse)

CAUTION

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

6. Interpolation Functions

Example of program

6.1 Positioning (Rapid Traverse)

Tool

+300

End point (-120,+200,+300)

+150

Start point

(+150,-100,+150)

+150

-100

-120 +200

Unit : mm

G91 G00 X-270000 Y300000 Z150000 ; (For input setting unit: 0.001mm)

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

shortest path connecting the start and end points. The positioning speed is automatically calculated so that the shortest distribution time is obtained in order that the commanded speeds for each axis do not exceed the rapid traverse rate.

When for instance, the Y axis and Z axis rapid traverse rates are both 9600mm/min, the tool will

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

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

End point

ctual Y axis rate : 6400mm/min

200

Start point

300

ctual X axis rate : 9600mm/min

(Unit : mm)

6. Interpolation Functions

6.1 Positioning (Rapid Traverse)

(Note 2) When parameter "#1086 G0Intp" is set to 1, the tool will move along the path from the start point to

the end point at the rapid traverse rate of each axis.

When, for instance, the Y axis and Z axis rapid traverse rates are both 9600mm/min, the tool will

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

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

End point

300

ctual X axis rate : 9600mm/min

Start point (Unit : mm)

ctual Y axis rate : 9600mm/min

200

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

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

6. Interpolation Functions

6.1 Positioning (Rapid Traverse)

(Note 4) Rapid traverse (G00) deceleration check

There are two methods for the deceleration check at rapid traverse; commanded deceleration

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

■ When "inpos" = "1"

Upon completion of the rapid traverse (G00), the next block will be executed after confirming that

the remaining distances for each axis are below the fixed amounts. (Refer to following drawing.)

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

setting value for the servo parameter "#2224 SV 024".

The purpose of checking the rapid feedrate is to minimize the time it takes for positioning. The

bigger the setting value for the servo parameter "#2224 SV024", the longer the reduced time is, but the remaining distance of the previous block at the starting time of the next block also becomes larger, and this could become an obstacle in the actual processing work. The check for the remaining distance is done at set intervals. Accordingly, it may not be possible to get the actual amount of time reduction for positioning with the setting value SV 024.

■ When "inpos" = "0"

Upon completion of the rapid traverse (G00), the next block will be executed after the deceleration

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

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

. L R is the

Pre vi o us bl oc k

Ts : Acceleration/deceleration

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

Next block

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

Previous block Next block

2 × Ts

cceleration/deceleration

Ts :

time constant Td : Deceleration check time Td = 2 × Ts + (0 ~ 14ms)

6. Interpolation Functions

6.1 Positioning (Rapid Traverse)

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

Pre vi o us bl oc k Next b l ock

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

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

Ts : Acceleration/deceleration

time constant Td : Deceleration check time Td = 2 × Ts + (0 ~ 14ms)

6. Interpolation Functions

Programmable in-position width command for positioning

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

G00 X__ Y__ Z__ , I__ ;

Operation during in-position check

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

Differences between in-position check with this command and in-position check with parameter

6.1 Positioning (Rapid Traverse)

In-position width Positioning coordinate value of each axis

In-position check with ",I" address command In-position check with parameter

After starting deceleration of the command system, the position error amount and commanded in-position width are compared.

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

Block being executed

Servo

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

Command

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

Block being executed

Servo

Command

In-position width (Servo system position error amount)

Start of in-position check with parameter

Ts : Acceleration/deceleration time constant Td : Deceleration check time

Td = Ts + (0 to 14ms)

6. Interpolation Functions

In-position width setting

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

In-position check using the "G0inps" value

6.1 Positioning (Rapid Traverse)

Command to motor

Outline of motor movement

G0 in-position

SV024

A stop is judged here.

In-position check using the "G1inps" value

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

(Note 1) When the in-position width (programmable in-position check width) is set in the machining program,

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

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

in-position check is carried out with the SV024 value.

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

Command to motor

Outline of motor movement

G1 in-position

SV024

A stop is judged here.

6. Interpolation Functions

6.2 Linear Interpolation; G01

Function and purpose

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

Command format

G01 X__ Y__ Z__ α__ F__ ,I__ ; (α represents additional axis)

X, Y, Z, α :Represents the coordinate value. An absolute position or

F :Feedrate (mm/min or °/min) I :In-position width. A program error occurs if a decimal point

Detailed description

(1) Once this command is issued, the mode is maintained until another G function (G00, G02, G03,

G33) in the 01 group which changes the G01 mode is issued. Therefore, if the next command is also G01 and if the feedrate is the same, all that is required to be done is to specify the coordinate words. If no F command is given in the first G01 command block, program error (P62) results.

(2) The feedrate for a rotary axis is commanded by

300

°/min)

(3) The G functions (G70 - G89) in the 09 group are cancelled (G80) by the G01 command.

6.2 Linear Interpolation

incremental position is indicated based on the state of G90/G91 at that time.

command is issued. This is valid only in the commanded block. A block that does not contain this address will follow the parameter "#1193 inpos" settings.

°/min (decimal point position unit). (F300 =

6. Interpolation Functions

Example of program

(Example 1) Cutting in the sequence of P

→ P1 is for tool positioning

6.2 Linear Interpolation

→ P2 → P3 → P4 → P1 at 300 mm/min feedrate

Unit: mm Input setting unit: 0.001mm

G90 G00 X20000 Y20000 ; G01 X20000 Y30000 F300 X30000 ; X-20000 Y-30000 ; X-30000 ;

→ P1 → P2 → P3 → P4 → P1

Programmable in-position width command for linear interpolation

This command commands the in-position width for the linear interpolation command from the machining program. The commanded in-position width is valid in the linear interpolation command only when carrying out deceleration check.

• When the error detect switch is ON.

• When G09 (exact stop check) is commanded in the same block.

• When G61 (exact stop check mode) is selected.

G01 X__ Y__ Z__ F__ , I__ ;

(Note 1)

Refer to section "6.1 Positioning (rapid traverse); G00" for details on the in-position

check operation.

In-position width Feedrate Linear interpolation coordinate value of each axis

6. Interpolation Functions

6.3 Plane Selection; G17, G18, G19

Function and purpose

The plane to which the movement of the tool during the circle interpolation (including helical cutting) and tool radius compensation command belongs is selected. By registering the basic three axes and the corresponding parallel axis as parameters, a plane can be selected by two axes that are not the parallel axis. If the rotary axis is registered as a parallel axis, a plane that contains the rotary axis can be selected.

The plane selection is as follows:

• Plane that executes circular interpolation (including helical cutting)

• Plane that executes tool radius compensation

• Plane that executes fixed cycle positioning.

Command format

G17 ; G18 ; G19 ;

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

Parameter entry

Table 1 Example of plane selection parameter entry

#1026 to 1028

base_I,J,K

(ZX plane selection) (YZ plane selection) (XY plane selection)

#1029 to 1039

aux_I,J,K

6.3 Plane Selection

I X U

J Y

K Z V

As shown in the above example, the basic axis and its parallel axis can be registered. The basic axis can be an axis other than X, Y and Z. Axes that are not registered are irrelevant to the plane selection.

6. Interpolation Functions

Plane selection system

In Table 1, I is the horizontal axis for the G17 plane or the vertical axis for the G18 plane J is the vertical axis for the G17 plane or the horizontal axis for the G19 plane K is the horizontal axis for the G18 plane or the vertical axis for the G19 plane

In other words,

G17 ..... IJ plane

G18 ..... KI plane

G19 ..... JK plane

(1) The axis address commanded in the same block as the plane selection (G17, G18, G19)

determines which basic axis or parallel axis is used for the plane selection. For the parameter registration example in Table 1.

G17X__Y__ ; XY plane G18X__V__ ; VX plane G18U__V__ ; VU plane G19Y__Z__ ; YZ plane G19Y__V__ ; YV plane

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

not commanded.

G17X__Y__ ; XY plane

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

commanded, it will be viewed as though the basic three axes address has been omitted. For the parameter registration example in Table 1.

G17 ; XY plane G17U__ ; UY plane G18U__ ; ZU plane G18V__ ; VX plane G19Y__ ; YZ plane G19V__ ; YV plane

(4) The axis command that does not exist in the plane determined by the plane selection G code

(G17, G18, G19) is irrelevant to the plane selection. For the parameter registration example in Table 1.

G17U__Z__ ;

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

plane. If the basic axis and parallel axis are commanded in duplicate in the same block as the plane selection G code (G17, G18, G19), the plane will be determined in the priority order of basic axis and parallel axis. For the parameter registration example in Table 1.

G17U__Y__W__-;

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

(Note 1)

The plane set with parameter "#1025 I_plane" will be selected when the power is turned

ON or reset.

Y__Z__ ; XY plane (plane does not change)

6.3 Plane Selection

6. Interpolation Functions

6.4 Circular Interpolation; G02, G03

Function and purpose

These commands serve to move the tool along an arc.

Command format

G02 (G03) X__ Y__ I__ J__ K__ F__;

G02 : Clockwise (CW) G03 : Counterclockwise (CCW) X, Y : End point I, J : Arc center F : Feedrate

For the arc command, the arc end point coordinates are assigned with addresses X, Y (or Z, or parallel axis X, Y, Z), and the arc center coordinate value is assigned with addresses I, J (or K).

Either an absolute value or incremental value can be used for the arc end point coordinate value command, but the arc center coordinate value must always be commanded with an incremental value from the start point. The arc center coordinate value is commanded with an input setting unit. Caution is required for the arc command of an axis for which the input command value differs. Command with a decimal point to avoid confusion.

6.4 Circular Interpolation

6. Interpolation Functions

Detailed description

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

changes its mode is issued. The arc rotation direction is distinguished by G02 and G03. G02 Clockwise (CW) G03 Counterclockwise (CCW)

6.4 Circular Interpolation

G02

G17(X-Y)plane

G03

G02

G18(Z-X)plane

G03

G02

G19(Y-Z)plane

G03

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

command.

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

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

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

(d) Arc center coordinates....... : Given by addresses I, J, K (incremental commands)

(e) Feed rate............................: Given by address F

6. Interpolation Functions

Example of program

(Example 1)

6.4 Circular Interpolation

Feedrate F = 500mm/min

X axis

Y axis

Circle cente J = 50mm

Start point/end point

G02 J50000 F500 ; Circle command

(Example 2)

Y axis

X axis

Feedrate F = 500mm/min

rc cente

J = 50mm

Start point

End point X50 Y50mm

G91 G02 X50000 Y50000 J50000 F500 ; 3/4 command

6. Interpolation Functions

Plane selection

The planes in which the arc exists are the following three planes (refer to the detailed drawings), and are selected with the following method.

XY plane G17; Command with a (plane selection G code) ZX plane G18; Command with a (plane selection G code) YZ plane G19; Command with a (plane selection G code)

Change into linear interpolation command

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

(Example) The parameter "#11029 Arc to G1 no Cent (Change command from arc to linear when no arc center designation)" = "1"

6.4 Circular Interpolation

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

；

… (a)

… (b)

(a) The circular interpolation (G02) is executed because there is a center command. (b) The linear interpolation (G01) is executed because there is no center and radius command.

6. Interpolation Functions

Precautions for circular interpolation

(1) The terms "clockwise" (G02) and "counterclockwise" (G03) used for arc operations are

defined as a case where in a right-hand coordinate system, the negative direction is viewed from the position direction of the coordinate axis which is at right angles to the plane in question.

(2) When all the end point coordinates are omitted or when the end point is the same position as

the start point, a 360° arc (full circle) is commanded when the center is commanded using I, J and K.

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

(a) Program error (P70) results at the arc start point when error ΔR is greater than parameter

"#1084 RadErr".

(G91) G02X9.899I 5. ;

larm stop

6.4 Circular Interpolation

#1084 RadErr parameter value 0.100 Start point radius = 5.000

End point radius = 4.899 Error

ΔR = 0.101

Start point

Start point radius

Cente

End point radius

End point

ΔR

(b) Spiral interpolation in the direction of the commanded end point results when error ΔR is

less than the parameter value.

(G91) G02X9.9I 5. ;

Start point

Start point radius

Center

End point radius

End point

Spiral interpolation

#1084 RadErr parameter value 0.100 Start point radius = 5.000

End point radius = 4.900

ΔR = 0.100

Error

ΔR

The parameter setting range is from 0.001mm to 1.000mm.

6. Interpolation Functions

6.5 R-specified Circular Interpolation; G02, G03

Function and purpose

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

Command format

G02 (G03) X__ Y__ R__ F__ ;

X : X axis end point coordinate Y : Y axis end point coordinate R : Arc radius F : Feedrate

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

Detailed description

The arc center is on the bisector line which is perpendicular to the line connecting the start and end points of the arc. The point, where the arc with the specified radius whose start point is the center intersects the perpendicular bisector line, serves as the center coordinates of the arc command. If the R sign of the commanded program is plus, the arc is smaller than a semisphere; if it is minus, the arc is larger than a semisphere.

6.5 R-specified Circular Interpolation

rc path when

R sign is minus

Start point

02 Center point

Center point

rc path when

R sign is plus

Cente 01

End point

point

The following condition must be met with an R-specified arc interpolation command: L/(2xr) ≤ 1 An error will occur when L/2 - r > (parameter : #1084 RadErr)

Where L is the line from the start point to end point. When the R specification and I, J, K specification are contained in the same block, the R specification has priority in processing. When the R specification and I, J, K specification are contained in the same block, the R specification has priority in processing. The plane selection is the same as for the I, J, K-specified arc command.

6. Interpolation Functions

Example of program

(Example 1)

(Example 2)

(Example 3)

(Example 4)

G02 Xx

G03 Zz

G02 Xx

Yy1 Rr1 Ff1 ; XY plane R-specified arc

Xx1 Rr1 Ff1 ; ZX plane R-specified arc

Yy1 Ii1 Jj1 Rr1 Ff1 ; XY plane R-specified arc

G17 G02 Ii

6.5 R-specified Circular Interpolation

(When the R specification and I, J, (K) specification are contained in the same block, the R specification has priority in processing.)

Jj1 Rr1 Ff1 ; XY plane This is an R-specified arc, but as

this is a circle command, it is already completed.

6. Interpolation Functions

Circular center coordinate compensation

When "the error margin between the segment connecting the start and end points" and "the commanded radius × 2" is less than the setting value because the required semicircle is not obtained by calculation error in R specification circular interpolation, "the midpoint of segment connecting the start and end points" is compensated as the circular center. Set the setting value to the parameter "#11028 Tolerance Arc Cent (Tolerable correction value of arc center error)".

(Ex.) "#11028 Tolerance Arc Cent" = "0.000 (mm)"

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

×minimum setting increment

6.5 R-specified Circular Interpolation

G90 X0 Y0 ; N1 G02 X10. R5.000;

N1, N3

N2 G0 X0; N3 G02 X10. R5.001; N4 G0 X0; N5 G02 X10. R5.002; N6 G0 X0; M02 ;

… (a)

… (b)

(a) Compensate the center coordinate: Same as N1 path (b) Do not compensate the center coordinate: Inside path a little than N1

Calculation error margin compensation allowance value: 0.002 mm Segment connecting the start and end paints: 10.000 N3: Radius × 2 = 10.002 "Error 0.002 -> Compensate" N5: Radius × 2 = 10.004 "Error 0.004 -> Do not compensate" Therefore, this example is shown in the above figure.

6. Interpolation Functions

6.6 Helical Interpolation ; G17 to G19, G02, G03

Function and purpose

While circular interpolating with G02/G03 within the plane selected with the plane selection G code (G17, G18, G19), the 3rd axis can be linearly interpolated. Normally, the helical interpolation speed is designated with the tangent speed F' including the 3rd axis interpolation element as shown in the lower drawing of Fig. 1. However, when designating the arc plane element speed, the tangent speed F on the arc plane is commanded as shown in the upper drawing of Fig. 1. The NC automatically calculates the helical interpolation tangent speed F' so that the tangent speed on the arc plane is F.

6.6 Helical Interpolation

Start point

End point

F’

Start point

Fig. 1 Designation of helical interpolation speed

Command format

G17 G02 (G03) Xx1 Yy1 Zz1 Ii1 Jj1 Pp1 Ff1 ; Helical interpolation command (Specify arc center) G17 G02 (G03) Xx

Yy2 Zz2 Rr2 Ff2 ; Helical interpolation command (Specify radius (R))

G17(G18, G19) : Plane selection (G17: XY plane, G18: ZX plane, G19: YZ plane) G02(G03) : Arc rotation direction Xx

Yy1 Xx2 Yy2 : Arc end point coordinate

Zz2 : Linear axis end point coordinate

Jj1 : Arc center coordinate

: Pitch No.

Ff2 : Feedrate

: Arc radius

The arc center coordinate and arc radius are commanded with an input setting input. Caution is required for the helical interpolation command of an axis for which the input command value differs. Command with a decimal point to avoid confusion. Absolute or incremental values can be assigned for the arc end point coordinates and the end point coordinates of the linear axis, but incremental values must be assigned for the arc center coordinates.

6. Interpolation Functions

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

#1235 set07/bit0 Meaning

1 Arc plane element speed designation is selected. 0 Normal speed designation is selected.

Z axis

Normal speed designation

Y axis

P1time

Second time First time

6.6 Helical Interpolation

End point

Start point

X axis

(1) This command should be issued with a linear axis (multiple axes can be commanded) that

does not contain a circular axis in the circular interpolation command combined. (2) For feedrate F, command the X, Y Z axis composite element directions speed. (3) Pitch l is obtained with the following expression.

(2π • P1 + θ) / 2π

= θE - θs = tan

-1

- tan-1

(0 ≤ θ < 2π)

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

xe, ye are the end point coordinates from the arc center (4) If pitch No. is 0, address P can be omitted.

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

The pitch No. designation (P command) cannot be made with the R-specified arc. (5) Plane selection

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

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

where circular interpolation is executed is commanded with the plane selection G code (G17,

G18, G19), and the 2 circular interpolation axes and linear interpolation axis (axis that

intersects with circular plane) 3 axis addresses are commanded.

XY plane circular, Z axis linear

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

ZX plane circular, Y axis linear

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

YZ plane circular, X axis linear

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

6. Interpolation Functions

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

UY plane circular, Z axis linear

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

program example can be used. Refer to the section "6.3 plane selection" for the arc planes

selected with these command methods.

Example of program

(Example 1)

6.6 Helical Interpolation

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

Z axis

Y axis

X axis

G17 ; XY plane G03 Xx1 Yy1 Zz1 Ii1 Jj1 P0 Ff1 ; XY plane arc, Z axis linear

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

axis

Y axis

X axis

(Example 2)

G17 ; XY plane G02 Xx1 Yy1 Zz1 Rr1 Ff1 ; XY plane arc, Z axis linear

(Example 3)

Z axis

Y axis

U axis

G17 G03 Uu

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

6. Interpolation Functions

(Example 4)

6.6 Helical Interpolation

U axisXaxis

Z axis

G18 G03 Xx

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

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

and the additional axis will perform linear interpolation.

(Example 5)

G18 G02 Xx

;

Uu1 Yy1 Zz1 Ii1 Jj1 Kk1

ZX plane arc, U axis, Y axis linear (The J command is ignored)

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

Arc plane element speed designation

If arc plane element speed designation is selected, the F command will be handled as modal data in the same manner as the normal F command. This will also apply to the following G01, G02 and G03 commands. For example, the program will be as follows.

(Example)

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

element is F100 G01 X20. ; Linear interpolation at F100 G02 X10. Y-10. Z4. J10. ; Helical interpolation at speed at which arc plane

element is F100 G01 Y-40. F120 ; Linear interpolation at F120 G02 X-10. Y-10. Z-4. I10. ; Helical interpolation at speed at which arc plane

element is F120 G01 X-20. ; Linear interpolation at F120

When the arc plane element speed designation is selected, only the helical interpolation speed command is converted to the speed commanded with the arc plane element. The other linear and arc commands operate as normal speed commands.

(1) The actual feedrate display (Fc) indicates the tangent element of the helical interpolation. (2) The modal value speed display (FA) indicates the command speed. (3) The speed data acquired with API functions follows the Fc and FA display. (4) This function is valid only when feed per minute (asynchronous feed: G94) is selected. If feed

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

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

6. Interpolation Functions

6.7 Thread Cutting

6.7.1 Constant Lead Thread Cutting; G33

Function and purpose

The G33 command exercises feed control over the tool which is synchronized with the spindle rotation and so this makes it possible to conduct constant-lead straight thread-cutting and tapered thread-cutting. Multiple thread screws, etc., can also be machined by designating the thread cutting angle.

Command format

G33 Z__(X__ Y__ α__) F__ Q__ ; (Normal lead thread cutting commands)

Z (X Y α) : Thread end point F : Lead of long axis (axis which moves most) direction Q : Thread cutting start shift angle, (0.000 to 360.000°)

G33 Z__(X__ Y__ α__) E__ Q__ ; (Precision lead thread cutting commands)

Z (X Y α) : Thread end point E : Lead of long axis (axis which moves most) direction Q : Thread cutting start shift angle, (0.000 to 360.000°)

Detailed description

(1) The E command is also used for the number of ridges in inch thread cutting, and whether the

ridge number or precision lead is to be designated can be selected by parameter setting. (Precision lead is designated by setting the parameter "#1229 set 01/bit 1" to 1.)

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

6.7 Thread Cutting

When a<45°, the lead is LZ. When a>45°, the lead is LX. When a=45°, the lead can be in either LX or LZ.

Tapered thread section

6. Interpolation Functions

Thread cutting metric input

6.7 Thread Cutting

Input unit

system

Command

address

Minimum

command

unit

Command

range

Input unit

system

Command

address

Minimum

command

unit

Command

range

Input unit

system

Command

address

Minimum

command

unit

Command

range

Input unit

system

Command

address

Minimum

command

unit

Command

range

B (0.001mm) C (0.0001mm)

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

1(=1.000)

(1.=1.000)

0.001~

999.999

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

1(=1.00000)

(1.=1.00000)

0.00001~

999.99999

1(=1.00000)

(1.=1.00000)

0.00001~

999.99999

D (0.00001mm) E (0.000001mm)

1(=1.0000000)

(1.=1.0000000)

0.0000001~

999.9999999

1(=1.00)

(1.=1.00)

0.03~999.99

1(=1.0000)

(1.=1.0000)

0.0255~

999.9999

1(=1.0000)

(1.=1.0000)

0.0001~

999.9999

1(=1.000000)

(1.=1.000000)

0.000001~

999.999999

1(=1.000000)

(1.=1.000000)

0.000001~

999.999999

1(=1.00000000)

(1.=1.00000000)

0.00000001~

999.99999999

1(=1.000)

(1.=1.000)

0.026~

999.999

1(=1.00000)

(1.=1.00000)

0.02541~

999.99999

Thread cutting inch input

B (0.0001inch) C (0.00001inch)

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

1(=1.0000)

(1.=1.0000)

0.0001~99.9999

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

1(=1.000000)

(1.=1.000000)

0.000001~

99.999999

1(=1.000000)

(1.=1.000000)

0.000001~

39.370078

D (0.000001inch) E (0.0000001inch)

1(=1.00000000)

(1.=1.00000000)

0.00000001~

39.37007874

1(=1.0000)

(1.=1.0000)

0.0101~

9999.9999

1(=1.000000)

(1.=1.000000)

0.010001~

9999.999999

1(=1.00000)

(1.=1.00000)

0.00001~

99.99999

1(=1.0000000)

(1.=1.0000000)

0.0000001~

99.9999999

1(=1.0000000)

(1.=1.0000000)

0.0000001~

39.3700787

1(=1.000000000)

(1.=1.000000000)

0.000000001~

39.370078740

1(=1.00000)

(1.=1.00000)

0.01001~

9999.99999

1(=1.0000000)

(1.=1.0000000)

0.0100001~

9999.9999999

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

feed exceeds the maximum cutting feed rate.

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

commands or scrolled thread cutting commands.

(4) The thread cutting command waits for the “single rotation sync“ signal of the rotary encoder

and starts movement. Make sure to carry out timing-synchronization between part systems before issuing a thread cutting command with multiple part systems. For example, with the 1-spindle specifications with two part systems, if one part system issues a thread cutting command during ongoing thread cutting by another part system, the movement will start without waiting for the rotary encoder “single rotation sync” signal causing an illegal operation.

(5) The spindle speed should be kept constant throughout from the rough cutting until the

finishing.

6. Interpolation Functions

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

will lose their shape. For this reason, feed hold does not function during thread cutting. Note that this is valid from the time the thread cutting command is executed to the time the axis moves. If the feed hold switch is pressed during thread cutting, block stop will result at the end point of the block following the block in which thread cutting is completed (no longer G33 mode).

(7) The converted cutting feedrate is compared with the cutting feed clamp rate when thread

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

(8) In order to protect the lead during thread cutting, a cutting feed rate which has been converted

may sometimes exceed the cutting feed clamp rate.

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

because of servo system delay and other such factors. Therefore, it is necessary to command a thread length which is determined by adding the illegal lead lengths to the required thread length.

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

1 ≤ R ≤ Where R ≤ Permissible speed of encoder (r/min)

(11) When the thread lead is extremely large to the maximum cutting feedrate enough to satisfy

"R<1" in the formula of (10) above, the program error (P93) may occur.

(12) Though dry run is valid for thread cutting, the feed rate based on dry run is not synchronized

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

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

command (G94).

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

thread cutting.

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

temporarily canceled and the thread cutting is executed.

(16) When the mode is switched to another automatic mode while G33 is executed, the following

block which does not contain a thread cutting command is first executed and then the automatic operation stops.

(17) When the mode is switched to the manual mode while G33 is executed, the following block

which does not contain a thread cutting command is first executed and then the automatic operation stops. In the case of a single block, the following block which does not contain a thread cutting command (when G33 mode is cancelled) is first executed and then the automatic operation stops. Note that automatic operation will stop immediately if the mode is switched before the

G33-commanded axis starts moving. (18) The handle interruption for automatic operation is valid while thread cutting. (19) The thread cutting start shift angle is not a modal. If there is no Q command with G33, this will

be handled as "Q0". (20) If a value more than 360.000 is commanded with G33 Q, the program error (P35) will occur. (21) G33 cuts one row with one cycle. To cut two rows, change the Q value, and issue the same

command.

Maximum feedrate

Thread lead

R : Spindle speed (r/min) Thread lead : mm or inches Maximum feedrate : mm/min or inch/mm (This is subject to the restrictions imposed

by the machine specifications).

6.7 Thread Cutting

6. Interpolation Functions

Example of program

6.7 Thread Cutting

10 50

N110 G90 G0 X-200. Y-200. S50 M3 ; N111 Z110. ;

The spindle center is positioned to the workpiece center, and the spindle rotates in the forward direction.

N112 G33 Z40. F6.0 ; The first thread cutting is executed.

Thread lead = 6.0mm

N113 M19 ; Spindle orientation is executed with the M19

command. N114 G0X-210. ; The tool is evaded in the X axis direction. N115 Z110. M0 ; The tool rises to the top of the workpiece, and the

program stops with M00.

Adjust the tool if required. N116 X-200. ;

Preparation for second thread cutting is done.

M3 ;

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

necessary. N11 G33 Z40. ; The second thread cutting is executed.

6. Interpolation Functions

6.7.2 Inch Thread Cutting; G33

Function and purpose

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

Command format

G33 Z__ E__ Q__ ;

Z : Thread cutting direction axis address (X, Y, Z, α) and thread length E : Number of ridges per inch in direction of long axis (axis which moves

Q : Thread cutting start shift angle, 0 to 360°.

Detailed description

(1) The number of ridges in the long axis direction is assigned as the number of ridges per inch.

(2) The E code is also used to assign the precision lead length, and whether the ridge number of

precision lead length is to be designated can be selected by parameter setting. (The number of ridges is designated by setting the parameter "#1229 set01/bit1" to 0.)

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

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

6.7 Thread Cutting

most) (decimal point command can also be assigned)

6. Interpolation Functions

Example of program

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

When programmed with δ

= 10mm using metric input

= 10mm,

6.8 Unidirectional Positioning

50.0mm

N210 G90 G0X-200. Y-200. S50M3; N211 Z110.; N212 G91 G33 Z-70.E3.0; (First thread cutting) N213 M19; N214 G90 G0X-210.; N215 Z110.M0;

M3; N217 G04 X2.0; N218 G91 G33 Z-70.; (Second thread cutting)

6.8 Unidirectional Positioning; G60

Function and purpose

The G60 command can position the tool at a high degree of precision without backlash error by locating the final tool position from a single determined direction.

N216 X-200.;

6. Interpolation Functions

Command format

G60 X__ Y__ Z__ α__ ;

α : Optional axis

Detailed description

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

parameter.

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

position by an amount equivalent to the creep distance, it move to the final position in accordance with the rapid traverse setting where its positioning is completed.

6.8 Unidirectional Positioning

G60a

Start point

Stop once

Positioning position

[Final advance direction]

End point

[G60creep distance]

G60-a

Start point

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

assigned for Z axis cancel and machine lock. (Display only)

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

intermediate position due to the mirror image function but the operation within the creep distance during its final advance will not be affected by mirror image.

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

function is valid.

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

emergency stop, interlock, feed hold and rapid traverse override zero. The tool moves over the creep distance at the rapid traverse setting. Rapid traverse override is

valid. (7) Uni-directional positioning is not performed for the drilling axis during drilling fixed cycles. (8) Uni-directional positioning is not performed for shift amount movements during the fine boring

or back boring fixed cycle. (9) Normal positioning is performed for axes whose creep distance has not been set by

parameter. (10) Uni-directional positioning is always a non-interpolation type of positioning. (11) When the same position (movement amount of zero) has been commanded, the tool moves

back and forth over the creep distance and is positioned at its original position from the final

advance direction. (12) Program error (P61) results when the G60 command is assigned with an NC system which

has not been provided with this particular specification.

6. Interpolation Functions

6.9 Cylindrical Interpolation; G07.1

Function and purpose

This function develops a shape with a cylindrical side (shape in cylindrical coordinate system) into a plane. When the developed shape is programmed as the plane coordinates, that is converted into the linear axis and rotation axis movement in the cylindrical coordinates and the contour is controlled during machining.

6.9 Cylindrical Interpolation ; G07.1

As programming can be carried out with a shape with which the side on the cylinder is developed, this is effective for machining cylindrical cams, etc. When programmed with the rotation axis and its orthogonal axis, slits, etc., can be machined on the cylinder side.

Develop-

ment

0°

2πr

360°

6. Interpolation Functions

Command format

G07.1 C__ ; (Cylindrical interpolation mode start/cancel)

C : Cylinder radius value

(Note) The above format applies when the name of the rotation axis is "C". If the name is not "C",

command the name of the rotation axis being used instead of "C".

(1) The coordinates commanded in the interval from the start to cancellation of the cylindrical

interpolation mode will be the cylindrical coordinate system.

G07.1 C Cylinder radius value; : : : G07.1 C0 ; Cylindrical interpolation mode cancel

6.9 Cylindrical Interpolation ; G07.1

• Radius value ≠ 0: Cylindrical interpolation mode start

• Radius value = 0: Cylindrical interpolation mode cancel

Cylindrical interpolation mode start (Cylindrical interpolation will start) (The coordinate commands in this interval will be the

cylindrical coordinate system)

(Cylindrical interpolation will be canceled)

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

6. Interpolation Functions

Detailed description

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

issued in the same block as another G code. (2) Program the rotation axis with an angle degree. (3) Linear interpolation or circular interpolation can be commanded during the cylindrical

interpolation mode. Note that the plane selection command must be issued just before the

G07.1 block. (4) The coordinates can be commanded with either an absolute command or incremental

command. (5) Tool radius compensation can be applied on the program command. Cylindrical interpolation will

be executed on the path after tool radius compensation. (6) Command the segment feed in the cylinder development with F. The F unit is mm/min or

inch/min. (7) Cylindrical interpolation accuracy

In the cylindrical interpolation mode, the movement amount of the rotation axis commanded

with an angle is converted on the circle periphery, and after operating the linear and circular

interpolation between the other axes, the amount is converted into an angle again. Thus, the actual movement amount may differ from the commanded value such as when the

cylinder radius is small. Note that the error generated at this time is not cumulated.

6.9 Cylindrical Interpolation ; G07.1

(8) F command during cylindrical interpolation As for the F command in the cylindrical interpolation mode, whether the previous F command

is used or not depends on that the mode just before G07.1 is the feed per minute command

(G94/G98) or feed per rotation command (G95/G99).

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

If there is no F command in the cylindrical interpolation, the previous F command feedrate

will be used.

The feedrate after the cylindrical interpolation mode is canceled will remain the F

command feedrate issued when the cylindrical interpolation mode was started or the final F command feedrate set during cylindrical interpolation.

(b) When G95 is commanded just before G07.1

The previous F command feedrate cannot be used during cylindrical interpolation, thus a

new F command must be issued.

The feedrate after the cylindrical interpolation mode is canceled will return to that applied

before the cylindrical interpolation mode was started.

When there is no F command in G07.1

Previous mode No F command After G07.1 is canceled

G94 (G98) Previous F is used G95 (G99) Program error (P62) F just before G07.1 is used

When F is commanded in G07.1

Previous mode No F command After G07.1 is canceled

G94 (G98) Commanded F is used G95 (G99) Commanded F is used *1 F just before G07.1 is used

*1) Moves with the feed per minute command during G07.1.

←

6. Interpolation Functions

6.9 Cylindrical Interpolation ; G07.1

(9) Plane selection

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

The correspondence of the rotation axis to an axis' parallel axis is set with the parameters

(#1029, #1030, #1031).

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

The plane selection command is set immediately before or after the G07.1 command. If not set

and a movement command is issued, a program error (P485) will occur.

(Example)

G19 Z0. C0. ; G07.1 C100. ; : G07.1 C0 ;

Basic coordinate system

X, Y, Z

Cylindrical coordinate system

C, Y, Z (Rotation axis is X axis' parallel axis)

#1029

G17

G18

G19

(Note)

Cylindrical coordinate system

X, C, Z (Rotation axis is Y axis' parallel axis)

#1030

Cylindrical coordinate system

X, Y , C (Rotation axis is Z axis' parallel axis)

#1031

G17

G18

G19

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

selected with G07.1 and G19.

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

plane.

Basic coordinate system

X, Y, Z

G17

G18

G19

Cylindrical coordinate system

G19

6. Interpolation Functions

(10) Related parameters

# Item Details

1516 mill_ax Milling axis

8111 Milling Radius Select the diameter and radius of the linear axis for milling

1267 (PR)

1270 (PR)

Relation with other functions

(1) The following G code commands can be used during the cylindrical interpolation

mode.

G code Details

G00 G01 G02 G03 G04 G09 G40-42 G61 G64 G65 G66 G66.1 G67 G80-89 G90/91 G94 G98 G99

ext03 (bit0)

ext06 (bit7)

6.9 Cylindrical Interpolation ; G07.1

Set the name of the rotation axis for milling interpolation

name

G code type The type of G code is changed.

Handle C axis coordinate during cylindrical interpolation

(pole coordinate interpolation, cylindrical interpolation). Only one of the rotation axes can be set.

interpolation (pole coordinate interpolation, cylindrical interpolation).

0: Radius command for all axes 1: Each axis setting (follows #1019 dia diameter

designation axis)

0: Conventional format 1: Mitsubishi special format

Specify whether the rotary axis coordinate before the cylindrical interpolation start command is issued is kept during the cylindrical interpolation or not.

0: Do not keep 1: keep

Positioning Linear interpolation Circular interpolation (CW) Circular interpolation (CWW) Dwell Exact stop check Tool nose R compensation Exact stop check mode Cutting mode Macro call (simple call) Macro modal call A (modal call) Macro modal call B (block call per macro) Macro modal call cancel (modal call cancel) Hole drilling fixed cycle Absolute/incremental value command Asynchronous feed Hole drilling cycle initial return Hole drilling cycle R point return

Setting

range

A to Z

0 / 1

A program error (P481) may occur if a G code other than those listed above is commanded

during cylindrical interpolation.

(2) Circular interpolation

(a) Circular interpolation between the rotation axis and linear axis is possible during the

cylindrical interpolation mode.

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

be designated.)

6. Interpolation Functions

(3) Tool radius compensation

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

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

When using tool radius compensation, start up and cancel the compensation within the

cylindrical interpolation mode.

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

compensation.

compensation is canceled, the position of the axis in the G07.1 command block is interpreted as the position applied after the tool radius compensation is canceled and the following operations are performed.

(4) Tool length compensation

(a) A program error (P481) will occur if the tool length compensation is carried out in the

cylindrical interpolation mode. : : G43H12 ; ... Tool length compensation before cylindrical interpolation → Valid G0 X100. Z0 ; G19 Z C ; G07.1 C100. ; : G43H11 ; ... Tool length compensation in cylindrical interpolation mode → Program error : G07.1 C0 ;

6.9 Cylindrical Interpolation ; G07.1

(b) Complete the tool compensation movement (movement of tool length and wear

compensation amount) before executing the cylindrical interpolation. If the tool compensation movement is not completed when the cylindrical interpolation start command has been issued, the followings will be resulted:

● Machine coordinate is not changed even if G07.1 is executed.

●The workpiece coordinate is changed to that of the post tool length compensation when

G07.1 is executed. (Even if canceling the cylindrical interpolation, this workpiece coordinate will not be canceled.)

(5) Cutting asynchronous feed

(a) The asynchronous mode is forcibly set when the cylindrical interpolation mode is started.

(b) When the cylindrical interpolation mode is canceled, the synchronization mode will return

to the state before the cylindrical interpolation mode was started.

control mode (G96).

(6) Miscellaneous functions

(a) The miscellaneous function (M) and 2nd miscellaneous function can be issued even in the

cylindrical interpolation mode.

(b) The S command in the cylindrical interpolation mode issues the rotary tool's rotation

speed instead of the spindle rotation speed.

6. Interpolation Functions

Restrictions and precautions

(1) The cylindrical interpolation mode is canceled when the power is turned ON or reset. (2) A program error (P484) will occur if any axis commanded for cylindrical interpolation has not

completed reference position return. (3) Tool radius compensation must be canceled before the cylindrical interpolation mode can be

canceled. (4) When the cylindrical interpolation mode is canceled, the mode will change to the cutting mode,

and the plane will return to that selected before cylindrical interpolation. (5) The program of the block during the cylindrical interpolation cannot be restarted (program

restart). (6) A program error (P486) will occur if the cylindrical interpolation command is issued during the

mirror image. (7) When the cylindrical interpolation mode is started or canceled, the deceleration check is

performed. (8) A program error (P481) will occur if the cylindrical interpolation or the pole coordinate

interpolation is commanded during the cylindrical interpolation mode.

6.9 Cylindrical Interpolation ; G07.1

6. Interpolation Functions

Example of program

6.9 Cylindrical Interpolation ; G07.1

N01 G28XZC; N02 G97S100M23; N03 G00X50.Z0.; N04 G94G01X40.F100.;

N05 G19C0Z0; N06 G07.1C20.;

N07 G41; N08 G01Z-10.C80.F150; N09 Z-25.C90.; N10 Z-80.C225; N11 G03Z-75.C270.R55.; N12 G01Z-25; N13 G02Z-20.C280.R80.; N14 G01C360. N15 G40;

N16 G07.1C0;

N17 G01X50.; N18 G0X100.Z100.; N19 M25; N20 M30;

Command of plane selection for cylindrical interpolation and command of two interpolation axes

Cylindrical interpolation start

Cylindrical interpolation cancel

<Parameter> #1029 aux_I #1030 aux_J C #1031 aux_K

-20-40-60-80

(Unit: mm)

N09

N10

N08

N09

100 150

N10

N11

N12

N13

N14

200

250

300 350°

N14

N15

6. Interpolation Functions

6.10 Polar Coordinate Interpolation; G12.1, G13.1

Function and purpose

This function converts the commands programmed with the orthogonal coordinate axis into linear axis movement (tool movement) and rotation axis movement (workpiece rotation), and controls the contour. The plane that uses the linear axis as the plane's 1st orthogonal axis, and the intersecting hypothetical axis as the plane's 2nd axis (hereafter "pole coordinate interpolation plane") is selected. Pole coordinate interpolation is carried out on this plane. The workpiece coordinate system zero point is used as the coordinate system zero point during pole coordinate interpolation.

Linear axis

X axis

C axis

Z axis

Rotation axis (hypothetical axis)

Polar coordinate interpolation plane (G17 plane)

This is effective for cutting a notch section on a linear section of the workpiece diameter, and for cutting cam shafts, etc.

Command format

G12.1 ; Pole coordinate interpolation mode start

G13.1 ; Pole coordinate interpolation mode cancel

(1) The coordinates commanded in the interval from the start to cancellation of the pole

coordinate interpolation mode will be the pole coordinate interpolation. G12.1 ; Pole coordinate interpolation mode start : (Pole coordinate interpolation will start) : (The coordinate commands in this interval will be the pole coordinate : interpolation) G13.1 ; Pole coordinate interpolation mode cancel (Pole coordinate interpolation is canceled)

6. Interpolation Functions

Detailed description

(1) Command G12.1 and G13.1 in an independent block. A program error (P33) will occur if this

command is issued in the same block as another G code. (2) Linear interpolation or circular interpolation can be commanded during the pole coordinate

interpolation mode. (3) The coordinates can be commanded with either an absolute command or incremental

command. (4) Tool radius compensation can be applied on the program command. Pole coordinate

interpolation will be executed on the path after tool radius compensation. (5) Command the segment feed in the pole coordinate interpolation plane (orthogonal coordinate

system) with F. The F unit is mm/min or inch/min. (6) When the G12.1 command is issued, the deceleration check is executed. (7) Plane selection

The linear axis and rotation axis used for pole coordinate interpolation must be set beforehand

with the parameters.

6.10 Polar Coordinate Interpolation; G12.1, G13.1

(a) Determine the deemed plane for carrying out pole coordinate interpolation with the

parameter (#1533) for the linear axis used for pole coordinate interpolation.

#1533 setting value Deemed plane

X G17 (XY plane) Y G19 (YZ plane) Z G18 (ZX plane)

Blank (no setting) G17 (XY plane)

(b) A program error (P485) will occur if the plane selection command (G16 to G19) is issued

during the pole coordinate interpolation mode.

(Note) Depending on the model or version, parameter (#1533) may not be provided. In this case,

the operation will be the same as if the parameter (#1533) is blank (no setting).

6. Interpolation Functions

(8) F command during pole coordinate interpolation

As for the F command in the pole coordinate interpolation mode, whether the previous F

command is used or not depends on that the mode just before G12.1 is the feed per minute

command (G94/G98) or feed per rotation command (G95/G99).

(a) When G94(G98) is commanded just before G12.1

If there is no F command in the pole coordinate interpolation, the previous F command feedrate will be used. The feedrate after the pole coordinate interpolation mode is canceled will remain the F command feedrate issued when the pole coordinate interpolation mode was started or the final F command feedrate set during pole coordinate interpolation. The previous F command feedrate cannot be used during pole coordinate interpolation.

(b) When G95(G99) is commanded just before G12.1

The previous F command feedrate cannot be used during pole coordinate interpolation. A new F command must be issued. The feedrate after the pole coordinate interpolation mode is canceled will return to that applied before the pole coordinate interpolation mode was started.

When there is no F command in G12.1

When F is commanded in G12.1

6.10 Polar Coordinate Interpolation; G12.1, G13.1

Previous mode No F command After G13.1 is canceled

G94(G98) Previous F is used

←

G95(G99) Program error (P62) F just before G12.1 is used

Previous mode No F command After G07.1 is canceled

G94(G98) Commanded F is used

←

G95(G99) Commanded F is used *1 F just before G12.1 is used

*1) Moves with the feed per minute command during G12.1.

(9) Related parameters

# Item Details

1516 mill_ax Milling axis

name

1517 mill_c Milling

interpolation hypothetical axis name

8111 Milling Radius Select the diameter and radius of the linear axis for

1533 mill_Pax Polar

coordinate linear axis name

Set the name of the rotation axis for milling interpolation (pole coordinate interpolation, cylindrical interpolation). Only one of the rotation axes can be set.

Select the hypothetical axis command name for milling interpolation (pole coordinate interpolation, cylindrical interpolation).

0: Y axis command 1: Command rotation axis name

milling interpolation.

0: Radius command for all axes 1: Each axis setting (follows #1019 dia diameter

designation axis)

Set the linear axis for polar coordinate interpolation. Axis

Setting

range

A to Z

0 / 1

name

6. Interpolation Functions

Relation with other functions

(1) The following G code commands can be used during the pole coordinate interpolation mode.

G code Details

G00 G01 G02 G03 G04 G09 G40-42 G61 G64 G65 G66 G66.1 G67 G80-89 G90/91 G94 G98 G99

6.10 Polar Coordinate Interpolation; G12.1, G13.1

Positioning Linear interpolation Circular interpolation (CW) Circular interpolation (CWW) Dwell Exact stop check Tool radius compensation Exact stop check mode Cutting mode Macro call (simple call) Macro modal call A (modal call) Macro modal call B (block call per macro) Macro modal call cancel (modal call cancel) Hole drilling fixed cycle Absolute/incremental value command Asynchronous feed Hole drilling cycle initial return Hole drilling cycle R point return

A program error (P481) may occur if a G code other than those listed above is commanded

during pole coordinate interpolation.

(2) Program commands during pole coordinate interpolation

(a) The program commands in the pole coordinate interpolation mode are commanded with

the orthogonal coordinate value of the linear axis and rotation axis (hypothetical axis) on the pole coordinate interpolation plane.

The axis address of the rotation axis (C) is commanded as the axis address for the plane's

2nd axis (hypothetical axis) command.

The command unit is not degree, and instead is the same unit (mm or inch) as the

command issued with the axis address for the plane's 1st axis (linear axis).

(b) The hypothetical axis coordinate value will be set to "0" when G12.1 is commanded. In

other words, the position where G12.1 is commanded will be interpreted as angle = 0, and the pole coordinate interpolation will start.

(3) Circular interpolation on pole coordinate plane The arc radius address for carrying out circular interpolation during the pole coordinate

interpolation mode is determined with the linear axis parameter (#1533).

#1533 setting value Center designation command

X I, J (pole coordinate plane is interpreted as XY plane) Y J, K (pole coordinate plane is interpreted as YZ plane) Z K, I (pole coordinate plane is interpreted as ZX plane)

Blank (no setting) I, J (pole coordinate plane is interpreted as XY plane)

The arc radius can also be designated with the R command. (Note) Depending on the model or version, parameter (#1533) may not be provided. In this case,

the operation will be the same as if the parameter (#1533) is blank (no setting).

6. Interpolation Functions

(4) Tool radius compensation The tool radius can be compensated during the pole coordinate interpolation mode.

(a) Command the plane selection in the same manner as pole coordinate interpolation.

When using tool radius compensation, it must be started up and canceled within the pole

coordinate interpolation mode.

(b) A program error (P485) will occur if polar coordinate interpolation is executed during tool

radius compensation.

tool radius compensation is canceled, the position of the axis in the G12.1 and G13.1 commands block is interpreted as the position applied after the tool radius compensation is canceled and the following operations are performed.

(5) Tool length compensation

(a) A program error (P481) will occur if the tool length compensation is carried out in the polar

coordinate interpolation mode. : : G43 H12 ; G0 X100. Z0 ; G12.1 ; : G43 H11 ;

: G13.1 ;

6.10 Polar Coordinate Interpolation; G12.1, G13.1

...Tool length compensation before polar coordinate interpolation → Valid

...Tool length compensation in polar coordinate interpolation mode → Program error

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

compensation amount) before executing the polar coordinate interpolation. If the tool compensation operation is not completed when the polar coordinate interpolation start command has been issued, the followings will be resulted:

●Machine coordinate is not changed even if G12.1 is executed..

●The workpiece coordinate is changed to that of the post tool length compensation when

G12.1 is executed. (Even if canceling the polar coordinate interpolation, this workpiece coordinate will not be canceled.)

(6) Cutting asynchronous feed

(a) The asynchronous mode is forcibly set when the pole coordinate interpolation mode is

started.

(b) When the pole coordinate interpolation mode is canceled, the synchronization mode will

return to the state before the pole coordinate interpolation mode was started.

control mode (G96).

(7) Miscellaneous functions

(a) The miscellaneous function (M) and 2nd miscellaneous function can be issued even in the

pole coordinate interpolation mode.

(b) The S command in the pole coordinate interpolation mode issues the rotary tool's rotation

speed instead of the spindle rotation speed.

6. Interpolation Functions

(8) Hole drilling axis in the hole drilling fixed cycle command during the pole coordinate

interpolation Hole drilling axis in the hole drilling fixed cycle command during the pole coordinate

interpolation is determined with the linear axis parameter (#1533).

(9) Shift amount in the G76 (fine boring) or G87 (back boring) command during the pole

coordinate interpolation

Shift amount in the G76 (fine boring) or G87 (back boring) command during the pole

coordinate interpolation is determined with the linear axis parameter (#1533).

Restrictions and precautions

(1) The program cannot be restarted (resumed) for a block in pole coordinate interpolation.

6.10 Polar Coordinate Interpolation; G12.1, G13.1

#1533 setting value Hole drilling axis

X Z (pole coordinate plane is interpreted as XY plane) Y X (pole coordinate plane is interpreted as YZ plane) Z Y (pole coordinate plane is interpreted as ZX plane)

Blank (no setting) Z (pole coordinate plane is interpreted as XY plane)

#1533 setting value Center designation command

X I, J (pole coordinate plane is interpreted as XY plane) Y J, K (pole coordinate plane is interpreted as YZ plane) Z K, I (pole coordinate plane is interpreted as ZX plane)

Blank (no setting) I, J (pole coordinate plane is interpreted as XY plane)

(2) Before commanding pole coordinate interpolation, set the workpiece coordinate system so

that the center of the rotation axis is at the coordinate system zero point. Do not change the coordinate system during the pole coordinate interpolation mode. (G50, G52, G53, relative coordinate reset, G54 to G59, etc.)

(3) The feedrate during pole coordinate interpolation will be the interpolation speed on the pole

coordinate interpolation plane (orthogonal coordinate system). (The relative speed with the tool will be converted with pole coordinate conversion.) When passing near the center of the rotation axis on the pole coordinate interpolation plane (orthogonal coordinate system), the rotation axis side feedrate after pole coordinate interpolation will be very high.

(4) The axis movement command outside of the plane during pole coordinate interpolation will

move unrelated to the pole coordinate interpolation.

(5) The current position displays during pole coordinate interpolation will all indicate the actual

coordinate value. However, the "remaining movement amount" will be the movement amount

on the pole coordinate input plane. (6) The pole coordinate interpolation mode will be canceled when the power is turned ON or reset. (7) A program error (P484) will occur if any axis commanded for pole coordinate interpolation has

not completed zero point return. (8) Tool radius compensation must be canceled before the pole coordinate interpolation mode

can be canceled. (9) When the pole coordinate interpolation mode is canceled, the mode will change to the cutting

mode, and the plane will return to that selected before pole coordinate interpolation. (10) A program error (P486) will occur if the pole coordinate interpolation command is issued

during the mirror image.

6. Interpolation Functions

(11) A program error (P486) will occur if the cylindrical interpolation or the pole coordinate

interpolation is commanded during the pole coordinate interpolation mode. (12) During pole coordinate interpolation, if X axis moveable range is controlled in the plus side, X

axis has to be moved to the plus area that includes "0" and above before issuing the polar

coordinate interpolation command. If X axis moveable range is controlled in the minus side, X

axis has to be moved to the area that does not include "0" before issuing the polar coordinate

interpolation command.

Example of program

6.10 Polar Coordinate Interpolation; G12.1, G13.1

Hypothetical C axis

N07

Hypothetical C axis

N06

N05

C axis

N09 N08

C axis

Tool

N04 N03

N10

Path after tool radius compensation Program path

N01 N02

N11

X axis

Z axis

: N01 G17 G90 G0 X40.0 C0 Z0; N02 G12.1; N03 G1 G42 X20.0 F2000; N04 C10.0; N05 G3 X10.0 C20.0 R10.0; N06 G1 X-20.0; N07 C-10.0; N08 G3 X-10.0 C-20.0 I10.0 J0; N09 G1 X20.0; N10 C0; N11 G40 X40.0; N12 G13.1;

Setting of start position Polar coordinate interpolation mode: Start Actual machining start

Shape program (Command the position with the orthogonal

coordinate on X-C hypothetical axis plane.)

Polar coordinate interpolation mode: Cancel : : M30 ;

6. Interpolation Functions

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

Function and purpose

Exponential function interpolation changes the rotation axis into an exponential function shape in respect to the linear axis movement. At this time, the other axes carry out linear interpolation between the linear axis. This allows a machining of a taper groove with constant torsion angle (helix angle) (uniform helix machining of taper shape). This function can be used for slotting or grinding a tool for use in an end mill, etc.

• Uniform helix machining of taper shape

Z axis

A axis

(Rotation axis)

(G01)

Torsion angle: J1=J2=J3

(G00)

(G02.3/G03.3)

(G01)

X axis

(Lin ea r axis)

• Relation of linear axis and rotation axis

"Relation of linear axi s and rotation axis"

X axis (Linear axis)

X=B (e {B, C ... constant}

-1)

A axis (Rotation axis)

6. Interpolation Functions

Command format

G02.3/G03.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ;

G02.3 : Forward rotation interpolation (modal) G03.3 : Negative rotation interpolation (modal) X Y Z I J R F Q K : Command will be ignored.

(Note 1) Designate the end point of the linear axis designated with parameter "#1514 expLinax" and

the axis that carries out linear interpolation between that axis.

If the end point on of the rotation axis designated with parameter "#1515 expRotax" is

designated, linear interpolation without exponential function interpolation will take place.

(Note 2) The command unit is as follows.

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

: X axis end point (Note 1) : Y axis end point (Note 1) : Z axis end point (Note 1) : Angle i1 (Note 2) : Angle j1 (Note 2) : Constant value r1 (Note 3) : Initial feedrate (Note 4) : Feedrate at end point (Note 5)

Setting unit #1003 = B #1003 = C #1003 = D #1003 = E (Unit = °) 0.001 0.0001 0.00001 0.000001

The command range is -89 to +89°. A program error (P33) will occur if there is no address I or J command. A program error (P35) will occur if the address I or J command value is 0.

(Note 3) The command unit is as follows.

Setting unit #1003 = B #1003 = C #1003 = D #1003 = E Unit Metric system 0.001 0.0001 0.00001 0.000001 mm Inch system 0.0001 0.00001 0.000001 0.0000001 inch

The command range is a positive value that does not include 0. A program error (P33) will occur if there is no address R command. A program error (P35) will occur if the address R command value is 0.

(Note 4) The command unit and command range is the same as the normal F code. (Command

as a per minute feed.) Command the composite feedrate that includes the rotation axis. The normal F modal value will not change by the address F command. A program error (P33) will occur if there is no address F command. A program error (P35) will occur if the address F command value is 0.

6. Interpolation Functions

(Note 5) The command unit is as follows.

Setting unit #1003 = B #1003 = C #1003 = D #1003 = E Unit Metric system 0.001 0.0001 0.00001 0.000001 mm Inch system 0.0001 0.00001 0.000001 0.0000001 inch

The command unit and command range is the same as the normal F code. Command the composite feedrate that includes the rotation axis. The normal F modal value will not change by the address Q command. The axis will interpolate between the initial speed (F) and end speed (Q) in the CNC

according to the linear axis. If there is no address Q command, interpolation will take place with the same value as

the initial feedrate (address F command). (The start point and end point feedrates will be

the same.) A program error (P35) will occur if the address Q command value is 0.

• Example of uniform helix machining of taper shape

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

Z axis Z axis

Linear axis ... X axis, rotation axis ... A axis, linear axis (X axis) start point ... x0

axis

X axis

x1 x0

Relational expression of exponential function

The exponential function relational expression of the linear axis (X) and rotation axis (A) in the G02.3/G03.3 command is defined in the following manner.

X (θ) = r1 ∗ (e A (θ) = (-1)

- 1) / tan (i1) (linear axis (X) movement (1))

∗ 360 ∗ θ / (2π) (rotation axis (A) movement)

D = tan (j1) / tan (i1)

ω = 0 during forward rotation (G02.3), and ω = 1 during reverse rotation (G03.3) θ is the rotation angle (radian) from the rotation axis' start point The rotation axis' rotation angle (θ) is as follows according to expression (1). θ = D ∗ 1n { (X ∗ tan (i1) / r1) + 1 }

6. Interpolation Functions

Machining example

• Example of uniform helix machining of taper shape

Z axis

z1 z2 z0

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

axis

X axis

x0 x2

r1 r2

Z (θ) = r1 ∗ (e X (θ) = r1 ∗ (e A (θ) = (-1)

-1) ∗ tan (p1) / tan (i1) + z0 ... (1)

-1) / tan (i1) ... (2)

∗ 360 ∗ θ / (2π)

D = tan (j1) / tan (i1) Z (θ) Absolute value from zero point of Z axis (axis that linearly interpolates between interval

with linear axis (X axis)) X (θ) Absolute value from X axis (linear axis) start point A (θ) Absolute value from A axis (rotation axis) start point r1 Exponential function interpolation constant value (address R command) r2 Workpiece left edge radius x2 X axis (linear axis) position at workpiece left edge x1 X axis (linear axis) end point (address X command) x0 X axis (linear axis) start point (Set as "x0 ≤ x1" so that workpiece does not interfere with

tool) z1 End point of Z axis (axis that linearly interpolates between interval with linear axis (X

axis)) (address Z command) z0 Start point of Z axis (axis that linearly interpolates between interval with linear axis (X

axis)) i1 Taper gradient angle (address I command) p1 Slot base gradient angle j1 Torsion angle (helix angle) (address J command)

ω Torsion direction (0: Forward rotation, 1: reverse direction) θ Workpiece rotation angle (radian)

f1 Initial feedrate (address F command) q1 Feedrate at end point (address Q command) k1 Insignificant data (address K command)

According to expressions (1) and (2): Z (θ) = X (θ) ∗ tan (p1) + z0 ... (3) According to expression (3), the slot base gradient angle (p1) is determined from the X axis and Z axis end point positions (x1, z1). The Z axis movement amount is determined by the slot base gradient angle (p1) and X axis position. In the above diagram, the exponential function interpolation's constant value (r1) is determined with the following expression using the workpiece left edge radius (r2), X axis start point (x0), X axis position at workpiece left edge (x2) and taper gradient angle (i1). r1 = r2 - { (x2 - x0) ∗ tan (i1) } ... (4)

6. Interpolation Functions

The taper gradient angle (i1) and torsion angle (j1) are each issued with the command address I and J. Note that if the shape is a reverse taper shape, the taper gradient angle (i1) is issued as a negative value. The torsion direction (ω) is changed with the G code. (Forward rotation when G02.3 is commanded, negative rotation when G03.3 is commanded) The above settings allow uniform helix machining of a taper shape (or reverse taper shape).

Command and operation

Start point

Command

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

G2.3(Equivalent to G3.3 if j1<0)

X movement direction > 0 X movement direction < 0

i1>0 i1<0 i1>0 i1<0

End

point

End

point

Start point

End

point

End

point

Start point

Operation

N10 G28XYZC; N20 G91G0 X100. Z100.; N30 G2.3 X100. Z100.

I50. J80. R105. F500.;

Machining

N40 M30;

program example

i1>0 i1<0 i1>0 i1<0

Start point

Command

N10 G28XYZC; N20 G91G0 X100. Z200.; N30 G2.3 X100. Z-100.

I-50. J80. R105. F500.;

N40 M30;

N10 G28XYZC; N20 G91G0 X-100. Z100.; N30 G2.3 X-100. Z100.

I50. J80. R105. F500.;

N40 M30;

N10 G28XYZC; N20 G91G0 X-100. Z200.; N30 G2.3 X-100. Z-100.

I-50. J80. R105. F500.;

N40 M30;

G3.3(Equivalent to G2.3 if j1<0)

X movement direction > 0 X movement direction < 0

End

point

End

point

Start point

End

point

End

Start point

Start

point

Operation

N10 G28XYZC; N20 G91G0 X100. Z100.; N30 G3.3 X100. Z100.

I50. J80. R105. F500.;

Machining

N40 M30;

program example

N10 G28XYZC; N20 G91G0 X100. Z200.; N30 G3.3 X100. Z-100.

I-50. J80. R105. F500.;

N40 M30;

N10 G28XYZC; N20 G91G0 X-100. Z100.; N30 G3.3 X-100. Z100.

I50. J80. R105. F500.;

N40 M30;

N10 G28XYZC; N20 G91G0 X-100. Z200.; N30 G3.3 X-100. Z-100.

I-50. J80. R105. F500.;

N40 M30;

6. Interpolation Functions

Precautions for programming

(1) When G02.3/G03.3 is commanded, interpolation takes place with the exponential function

relational expression using the start position of the linear axis and rotation axis as 0.

(2) Linear interpolation will take place in the following cases, even if in the G02.3/G03.3 mode. The feedrate for linear interpolation will be the F command in that block. (Note that the normal

F modal is not updated.)

• The linear axis designated with the parameter (#1514 expLinax) is not commanded, or the movement amount for that axis is 0.

• The rotation axis designated with the parameter (#1515 expRotax) is commanded.

(3) A program error will occur if the following commands are issued in G02.3 or G03.3 mode. A

program error will also occur if G02.3 or G03.3 command is issued in the following modes.:

• Tool length compensation (A program error will occur only when the compensation starts at the same time as the movement by exponential function interpolation. The tool length compensation will operate normally if it has started before the G02.3/G03.3 mode starts.

• Tool radius compensation

• High-speed high-accuracy control

• High-speed machining

• Scaling

• Tool length compensation along tool axis

• Figure rotation

• Coordinate rotation by program

• Coordinate rotation by parameter

• 3-dimentional coordinate conversion

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

(4) A program error (P481) will occur if commands are issued during the pole coordinate

interpolation, cylindrical interpolation or milling interpolation modes. (5) Program error (P612) will occur if commands are issued during the scaling or mirror image. (6) Program error (P34) will occur if commands are issued during the high-speed high-accuracy

control II. (7) G02.3/G03.3 will function with asynchronous feed even during the synchronous feed mode. (8) If the parameter "#1515 expRota" setting is the same axis name as the initial C axis, the axis

selected with the C axis selection signal will interpolate as the rotation axis.

6. Interpolation Functions

6.12 Polar Coordinate Command; G16/G15

Function and purpose

With this function, the end point coordinate value is commanded with the polar coordinate of the radius and angle.

Command format

G16 ; Polar coordinate command mode ON

G15 ; Polar coordinate command mode OFF

Detailed description

(1) The polar coordinate command is applied in the interval from turning ON to OFF of the polar

coordinate command mode.

G1x ; G16 ;

Plane selection for polar coordinate command (G17/G18/G19) Polar coordinate command mode ON

G9x G01 Xx1 Yy1 F2000 ;: Polar coordinate command

G9x : Center selection for polar coordinate command (G90/G91)

G90

G91 x1 : 1st axis for the plane y1 : 2nd axis for the plane

6.12 Polar Coordinate Command; G16/G15

• • •The workpiece coordinate system zero point is the

polar coordinate center.

• • •The present position is the polar coordinate center.

• • •The radius commanded

• • •The angle commanded

Commanded position

Plus

Minus

Present position

G15 ;

For G90/G17(X-Y plane)

Polar coordinate command mode OFF

(2) The plane selection during the polar coordinate command mode is carried out with G17, G18

and G19.

(3) The polar coordinate command is a modal. The polar coordinate command mode when the

power is turned ON is OFF (G15). Whether to initialize the modal at reset or not can be selected with the parameter (#1210 RstGmd/bit 11) setting.

(4) During polar coordinate command mode, command the radius with the 1st axis for the

selected plane, and the angle with the 2nd axis. For example, when the X-Y plane is selected, command the radius with the address "X", and the angle with the address "Y".

(5) For the angle, the counterclockwise direction of the selected plane is positive and the

clockwise direction is negative.

(6) The radius and angle can be commanded with both the absolute value and incremental value

(G90, G91).

6. Interpolation Functions

(7) When the radius is commanded with the absolute value, command the distance from the zero

point in the workpiece coordinate system (note that the local coordinate system is applied when the local coordinate system is set).

(8) When the radius is commanded with the incremental value command, considering the end

point of the previous block as the polar coordinate center, command the incremental value from that end point. The angle is commanded with the incremental value of the angle from the previous block.

(9) When the radius is commanded with the negative value, the same operation as the command

that the radius command value is changed to the absolute value and 180° is added to the angle command value.

Command position

(1) When the zero point in the workpiece coordinate system is applied to the polar

coordinate center

The zero point in the workpiece coordinate system is applied to the polar coordinate center by

commanding the radius with the absolute value. Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coordinate system (G52) is used.

6.12 Polar Coordinate Command; G16/G15

Command position

Radius

Angle

When the angle is the absolute value command

Command position when the zero point in the workpiece coordinate system is applied to the polar coordinate center

(2) When the present position is applied to the polar coordinate center

The present position is applied to the polar coordinate center by commanding the radius with

the incremental value.

Command position

Radius

Present position

When the angle is the incremental value command

Radius

Angle

Command position

Angle

Command position

Present position

Angle

Present position

When the angle is the absolute value command

Command position when the present position is applied to the polar coordinate center

When the angle is the incremental value command

Present position

6. Interpolation Functions

Ang

(3) When the radius command is omitted

When the radius command is omitted, the zero point in the workpiece coordinate system is

applied to the polar coordinate center, and the distance between the polar coordinate center and current position is regarded as the radius. Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coordinate system (G52) is used.

6.12 Polar Coordinate Command; G16/G15

Command position

Angle

When the angle is the absolute value command

Command position when the radius command is omitted

(4) When the angle command is omitted

When the angle command is omitted, the angle of the present position in the workpiece

coordinate system is applied to the angle command. The zero point in the workpiece coordinate system is applied to the polar coordinate center by commanding the radius with the absolute value. Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coordinate system (G52) is used. If the radius is commanded with the incremental value, the present position is applied to the polar coordinate center.

Present position

Radius

When the angle is the incremental value command

Command position

Angle

Radius

Command position

Present position

Angle

Present position

Radius

When the radius is the absolute value command

Command position when the angle command is omitted

When the radius is the incremental value command

Present position

Radius

6. Interpolation Functions

6.12 Polar Coordinate Command; G16/G15

Axis command not interpreted as polar coordinate command

The axis command with the following command is not interpreted as the polar coordinate command during the polar coordinate command mode. The movement command that has no axes commands for the 1st axis and 2nd axis in the selected plane mode is also not interpreted as polar coordinate command during the polar coordinate command mode.

Function G code Dwell G04 Program parameter input/compensation input Local coordinate system setting G52 Machine coordinate system setting G92 Machine coordinate system selection G53 Coordinate rotation by program G68.1 Scaling G51 G command mirror image G51.1 Reference position check G27 Reference position return G28 Start position return G29 2nd to 4th reference position return G30 Tool change position return 1 G30.1 Tool change position return 2 G30.2 Tool change position return 3 G30.3 Tool change position return 4 G30.4 Tool change position return 5 G30.5 Tool change position return 6 G30.6 Automatic tool length measurement G37 Skip G31 Multi-step skip function 1-1 G31.1 Multi-step skip function 1-2 G31.2 Multi-step skip function 1-3 G31.2 Linear angle command G01 Aa1

G10

6. Interpolation Functions

•

Example of program

When the zero point in the workpiece coordinate system is the polar coordinate zero point

6.12 Polar Coordinate Command; G16/G15

120°

270°

(1) When the radius and angle are the absolute value command

N1 G17 G90 G16 ; Polar coordinate command, X-Y plane selection

N2 G85 X200. Y30. Z-20. F200. ; Radius 200mm, angle 30° N3 Y120. ; Radius 200mm, angle 120° N4 Y270. ; Radius 200mm, angle 270°

N5 G15 G80 ; Polar coordinate command cancel

(2) When the radius is the absolute value command and the angle is the incremental value

command

N1 G17 G90 G16 ;

N2 G85 X200. Y30. Z-20. F200. ; Radius 200mm, angle 30° N3 G91 Y90. ; Radius 200mm, angle + 90°

N4 Y150. ; Radius 200mm, angle +150° N5 G15 G80 ; Polar coordinate command cancel

The polar coordinate zero point is the

zero point in the workpiece coordinate system.

• The plane is the X-Y plane.

30°

200mm

The polar coordinate zero point is the zero point in the workpiece coordinate system.

Polar coordinate command, X-Y plane selection The polar coordinate zero point is the zero point in the workpiece coordinate system.

MITSUBISHI CNC 700/70 Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Introduction

Precautions for Safety

Contents

1. Control Axes

1.1 Coordinate Words and Control Axis

1.2 Coordinate Systems and Coordinate Zero Point Symbols

2. Least Command Increments

2.1 Input Setting Units

2.2 Input Command Increment Tenfold

2.3 Indexing Increment

3. Data Formats

3.1 Tape Codes

3.2 Program Formats

3.3 Tape Memory Format

3.4 Optional Block Skip

3.4.1 Optional Block Skip ; /

3.4.2 Optional Block Skip Addition ; /n

3.5 Program/Sequence/Block Numbers ; L(O), N

3.6 Parity H/V

3.7 G Code Lists

3.8 Precautions Before Starting Machining

4. Buffer Register

4.1 Input Buffer

4.2 Pre-read Buffers

5. Position Commands

5.1 Position Command Methods ; G90, G91

5.2 Inch/Metric Command Change; G20, G21

5.3 Decimal Point Input

6. Interpolation Functions

6.1 Positioning (Rapid Traverse); G00

6.2 Linear Interpolation; G01

6.3 Plane Selection; G17, G18, G19

6.4 Circular Interpolation; G02, G03

6.5 R-specified Circular Interpolation; G02, G03

6.6 Helical Interpolation ; G17 to G19, G02, G03

6.7 Thread Cutting

6.7.1 Constant Lead Thread Cutting; G33

6.7.2 Inch Thread Cutting; G33

6.8 Unidirectional Positioning; G60

6.9 Cylindrical Interpolation; G07.1

6.10 Polar Coordinate Interpolation; G12.1, G13.1

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

6.12 Polar Coordinate Command; G16/G15