Mitsubishi Electric C6/C64/C64T Programming Manual

CNC

C6/C64/C64T

PROGRAMMING MANUAL

(MACHINING CENTER/TRANSFER MACHINE TYPE)

BNP-B2260B(ENG)

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 company.

Introduction

This manual is a guide for using the MELDAS C6/C64/C64T.

Programming is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study the "Precautions for Safety" on the following page to ensure safe use of the this NC unit.

Details described in this manual

CAUTION

For items described in "Restrictions" or "Usable State", the instruction manual issued by the machine manufacturer 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 written on the assumption that all option functions are added.

Refer to the specifications issued by the machine manufacturer before starting use.

Refer to the Instruction Manual issued by each machine manufacturer 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

MELDAS C6/C64/C64T Instruction Manual ........ BNP-B2259

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

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

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

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

Note that even items ranked as "

CAUTION

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

DANGER

Not applicable in this manual.

WARNING

Not applicable in this manual.

CAUTION

1. Items related to product and manual

For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by the machine manufacturer 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 manufacturer before starting use.

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

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

2. Items related to operation

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

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

(Continued on next page)

CAUTION

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

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

3. Items related to programming

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

" ; " "EOB" and " %" "EOR" are explanatory notations. The actual codes are "Line feed" and "%" for ISO, and "End of block" and "End of Record" for EIA.

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 manufacturer.

When programming the multi-part system, take special care to the movements of the programs for other part systems.

Contents

Page

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

1.1 Coordinate word and control axis ...................................................................................... 1

1.2 Coordinate systems and coordinate zero point symbols................................................... 2

2. Input Command Units ............................................................................................................... 3

2.1 Input command units.......................................................................................................... 3

2.2 Input setting units ............................................................................................................... 3

3. Data Formats.............................................................................................................................. 4

3.1 Tape codes ........................................................................................................................ 4

3.2 Program formats ................................................................................................................ 7

3.3 Program address check function ....................................................................................... 9

3.4 Tape memory format.......................................................................................................... 9

3.5 Optional block skip ; / ....................................................................................................... 10

3.6 Program/sequence/block numbers ; O, N ....................................................................... 11

3.7 Parity H/V ......................................................................................................................... 12

3.8 G code lists....................................................................................................................... 13

3.9 Precautions before starting machining ............................................................................ 16

4. Buffer Register......................................................................................................................... 17

4.1 Pre-read buffers ............................................................................................................... 17

5. Position Commands................................................................................................................ 18

5.1 Position command methods ; G90, G91.......................................................................... 18

5.2 Inch/metric command change; G20, G21........................................................................ 20

5.3 Decimal point input........................................................................................................... 21

6. Interpolation Functions .......................................................................................................... 25

6.1 Positioning (Rapid traverse); G00.................................................................................... 25

6.2 Linear interpolation; G01.................................................................................................. 31

6.3 Plane selection; G17, G18, G19 ...................................................................................... 33

6.4 Circular interpolation; G02, G03 ...................................................................................... 35

6.5 R-specified circular interpolation; G02, G03.................................................................... 39

6.6 Helical interpolation ; G17 to G19, G02, G03 .................................................................. 41

6.7 Thread cutting .................................................................................................................. 45

6.7.1 Constant lead thread cutting ; G33 .......................................................................... 45

6.7.2 Inch thread cutting; G33........................................................................................... 48

6.8 Uni-directional positioning; G60 ....................................................................................... 49

7. Feed Functions ........................................................................................................................ 51

7.1 Rapid traverse rate........................................................................................................... 51

7.2 Cutting feed rate............................................................................................................... 51

7.3 F1-digit feed ..................................................................................................................... 52

7.4 Synchronous feed; G94, G95 .......................................................................................... 54

7.5 Feedrate designation and effects on control axes........................................................... 56

7.6 Automatic acceleration/deceleration................................................................................ 59

7.7 Speed clamp .................................................................................................................... 59

7.8 Exact stop check; G09 ..................................................................................................... 60

7.9 Exact stop check mode ; G61.......................................................................................... 63

7.10 Automatic corner override ; G62.................................................................................... 64

7.11 Tapping mode ; G63 ...................................................................................................... 69

7.12 Cutting mode ; G64 ........................................................................................................ 69

8. Dwell.......................................................................................................................................... 70

8.1 Per-second dwell ; G04.................................................................................................... 70

9. Miscellaneous Functions........................................................................................................ 72

9.1 Miscellaneous functions (M8-digits BCD)........................................................................ 72

9.2 Secondary miscellaneous functions (B8-digits, A8 or C8-digits)..................................... 74

I

10. Spindle Functions ................................................................................................................. 75

10.1 Spindle functions (S2-digits BCD) ..... During standard PLC specifications ................. 75

10.2 Spindle functions (S6-digits Analog).............................................................................. 75

10.3 Spindle functions (S8-digits) .......................................................................................... 76

10.4 Multiple spindle control I ................................................................................................ 77

10.4.1 Multiple spindle control........................................................................................... 77

10.4.2 Spindle selection command ................................................................................... 78

10.5 Constant surface speed control; G96, G97 ................................................................... 80

10.5.1 Constant surface speed control ............................................................................. 80

10.6 Spindle clamp speed setting; G92 ................................................................................. 81

10.7 Spindle synchronization control I; G114.1 ..................................................................... 82

10.8 Spindle synchronization control II .................................................................................. 90

11. Tool Functions....................................................................................................................... 97

11.1 Tool functions (T8-digit BCD)......................................................................................... 97

12. Tool Offset Functions ........................................................................................................... 98

12.1 Tool offset....................................................................................................................... 98

12.2 Tool length offset/cancel; G43, G44/G49 .................................................................... 102

12.3 Tool radius compensation............................................................................................ 105

12.3.1 Tool radius compensation operation.................................................................... 106

12.3.2 Other operations during tool radius compensation.............................................. 116

12.3.3 G41/G42 commands and I, J, K designation....................................................... 124

12.3.4 Interrupts during tool radius compensation.......................................................... 130

12.3.5 General precautions for tool radius compensation .............................................. 132

12.3.6 Changing of offset No. during compensation mode ............................................ 133

12.3.7 Start of tool radius compensation and Z axis cut in operation............................. 135

12.3.8 Interference check................................................................................................ 137

12.4 Programmed offset input; G10, G11............................................................................ 144

13. Program Support Functions .............................................................................................. 149

13.1 Canned cycles.............................................................................................................. 149

13.1.1 Standard canned cycles; G80 to G89, G73, G74, G76 ....................................... 149

13.1.2 Initial point and R point level return; G98, G99.................................................... 166

13.1.3 Setting of workpiece coordinates in canned cycle mode..................................... 167

13.2 Special canned cycle; G34, G35, G36, G37.1 ............................................................ 168

13.3 Subprogram control; M98, M99 ................................................................................... 172

13.3.1 Calling subprogram with M98 and M99 commands ............................................ 172

13.4 Variable commands ..................................................................................................... 177

13.5 User macro specifications............................................................................................ 180

13.5.1 User macro commands ; G65, G66, G66.1, G67 ................................................ 180

13.5.2 Macro call instruction ........................................................................................... 181

13.5.3 Variables .............................................................................................................. 188

13.5.4 Types of variables ................................................................................................ 190

13.5.5 Arithmetic commands........................................................................................... 219

13.5.6 Control commands ............................................................................................... 224

13.5.7 External output commands .................................................................................. 227

13.5.8 Precautions .......................................................................................................... 229

13.5.9 Actual examples of using user macros ................................................................ 231

13.6 G command mirror image; G50.1, G51.1 .................................................................... 235

13.7 Corner chamfering, corner rounding............................................................................ 238

13.7.1 Corner chamfering " ,C_ " .................................................................................... 238

13.7.2 Corner rounding " ,R_ " ........................................................................................ 240

13.8 Circle cutting; G12, G13............................................................................................... 241

13.9 Program parameter input; G10, G11 ........................................................................... 243

13.10 Macro interrupt ; M96, M97........................................................................................ 244

13.11 Tool change position return ; G30.1 to G30.6 ........................................................... 253

13.12 High-accuracy control; G61.1 .................................................................................... 256

13.13 Synchronizing operation between part systems........................................................ 266

13.14 Start Point Designation Synchronizing (Type 1); G115............................................. 271

II

13.15 Start Point Designation Synchronizing (Type 2); G116............................................. 273

13.16 Miscellaneous function output during axis movement; G117.................................... 276

14. Coordinates System Setting Functions............................................................................ 278

14.1 Coordinate words and control axes ............................................................................. 278

14.2 Basic machine, work and local coordinate systems .................................................... 279

14.3 Machine zero point and 2nd, 3rd, 4th reference points (Zero point) ........................... 280

14.4 Basic machine coordinate system selection ; G53...................................................... 281

14.5 Coordinate system setting ;G92 .................................................................................. 282

14.6 Automatic coordinate system setting ........................................................................... 283

14.7 Reference (zero) point return; G28, G29..................................................................... 284

14.8 2nd, 3rd and 4th reference (zero) point return; G30.................................................... 288

14.9 Reference point check; G27 ........................................................................................ 291

14.10 Workpiece coordinate system setting and offset ; G54 to G59 (G54.1) ................... 292

14.11 Local coordinate system setting; G52 ....................................................................... 300

15. Measurement Support Functions...................................................................................... 304

15.1 Automatic tool length measurement; G37 ................................................................... 304

15.2 Skip function; G31........................................................................................................ 308

15.3 Multi-step skip function1; G31.n, G04.......................................................................... 313

15.4 Multi-step skip function 2; G31 .................................................................................... 315

Appendix 1. Program Parameter Input N No. Correspondence Table.............................. 318

Appendix 2. Program Error.................................................................................................... 323

Appendix 3. Order of G Function Command ....................................................................... 334

III

1. Control Axes

1.1 Coordinate word and control axis

1. Control Axes

1.1 Coordinate word and control axis

Function and purpose

In the standard specifications, there are 3 control axes, but, by adding an additional axis, up to 14 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

+Z

+Z

+Y

+X

Program coordinates

Workpiece

X-Y table

+Y

Direction of table movement

Bed

+X


X-Y and revolving table

+X


+Y

Workpiece

+C

Direction of table revolution

+Z

+Y

+C

+X

Program coordinates

1

1. Control Axes

1.2 Coordinate systems and coordinate zero point symbols

1.2 Coordinate systems and coordinate zero point symbols


: Reference point

: Machine coordinate zero point

-X

Work coordinate system 3 (G56)


: Work coordinate zero points (G54 - G59)

Basic machine coordinate system

Machine zero point y

1 x

1 y

3

Work coordinate system 2 (G55) x

3

Work coordinate system 5 (G58) y

5 y

2

1st reference point


2 x

Work coordinate system 4

(G57)

Local coordinate system

(G52) y x

5

-Y

2

2. Input Command Units

2.1 Input command units

2. Input Command Units

2.1 Input command units


These are the units used for the movement amounts in the program. They are expressed in millimeters, inches or degrees (

°

).

2.2 Input setting units


These are the units of setting data which are used, as with the compensation amounts, in common for all axes.

The input command units can be selected from the following types for each axis with the parameters. The input setting units can be selected from the following types common to axes. (For further details on settings, refer to the Instruction Manual.)

Input command unit

Min. movement unit

Input setting unit

Linear axis

Input unit parameters

#1015 cunit = 10

= 1

Diameter command

Radius command

Diameter Radius command command

0.001

0.0001

0.001

0.0001

0.0001

0.00001

0.0001

0.00001

#1003 iunit = B 0.0005 0.001 0.00005 0.0001

= 0.000005

#1003 iunit = B 0.001 0.001 0.0001 0.0001

axis (

°

)

0.001

0.0001

0.001

0.001

(Note 1)

Inch/metric conversion is performed in either of 2 ways: conversion from the parameter screen ("#1041 I_inch: valid only when the power is switched 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 units and not to the input setting units.

Consequently, the tool offset amounts and other compensation amounts as well as the variable data should be preset 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 units 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.)

3

3. Data Formats

3.1 Tape codes

3. Data Formats

3.1 Tape codes


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 error (P32) will result.

(Note 2)

For the sake of convenience, a semicolon " ; " has been used in the CNC display to 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 explanatory notations. The actual codes are "Line feed" and

"%" for ISO, and "End of block" and "End of Record" for EIA.

Detailed description

EOB/EOR keys and displays

Code used

Key used

End of block

End of record

LF or NL

%

;

%

(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.

4

3. Data Formats

3.1 Tape codes

(2) Control out, control in

When the ISO code is used, all data between control out "(" and control in ")" or ";" are ignored, although these data appear on the setting and display unit. Consequently, the command tape name, number 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

L C

F R

G0 0 X - 8 5 0 0 0 Y - 6 4 0 0 0 ( CU T T E R

•

•• ••

• ••

••

• •

• •

••

•

S

P

RE T URN )

L

F

• • • • • • • • • • • •

•• •

••••

• •

• •

•••

• •

•

•

•

•

•

••

••

• •

•

•

•••••

•

•

•••

•• ••••

•

••

•

•

•

•

•••

•••••

• •

Operator information print-out example

Information in this section is ignored and nothing is executed.

(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)

(c) Completion of loading during tape loading into memory

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

2m

% 10cm ;

• • • • • • • •

;

• • • • • •

;

• • • • • • • • • •

; 10cm %

(EOR) (EOB)

(EOB)

Initial block

(EOB) (EOB)

Last block

(EOR)

2m

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.

5

3. Data Formats

3.1 Tape codes

ISO code (R-840)

Feed holes

8 7 6 5 4 3 2 1

Channel No.

• ••

••

•

•

•

•

•

1

2

3

4

••

•

• •

• ••

•

•••

7

5

6

•

•

••

•••

• •

• •

• •

• •

•• •

•• •

• •

•• ••

• ••

• •

• • •

• • •

• •

• •

• •••

• •

•

• •

•

•

• •••

• •••

••

•

•••••

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

•

••

•

•

••

•

•

•

•

••

•

••

•

• •

•

•

•

• •

•

••

• •

• •

••

•

••

••

•

•

•

•••

”

!

;

:

,

/

-

.

I

8

9

0

A

B

C

D

E

F

G

H

J

K

L

M

N

O

P

Q

R

S

T

U

V

W

X

Y

Z

+

%

LF(Line Feed) or NL

( (Control Out)

) (Control In)

#

*

=

[

]

SP(Space)

CR(Carriage Return)

BS(Back Space)

HT(Horizontal Tab)

&

$

’ (Apostrophe)

<

>

?

@

DEL(Delete)

NULL

DEL(Delete)

A

B

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

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

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.

Table of tape codes

6

3. Data Formats

3.2 Program formats



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".


(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.).

Word

*

Numerals

Alphabet (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 ;

2 blocks

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

(3) Programs

A program is a collection of several blocks.

(Note 1)

When there is no number following the alphabetic character in the actual program, the numeric value following the alphabetic character is handled as a 0.

(Example)

G28XYZ;

→

G28X0Y0Z0;

7

3. Data Formats


Item

Program number

Sequence number

Preparatory function

Movement axis

Input setting unit

Input setting unit

Additional axis

Input setting unit

Input setting unit

Input setting unit

Dwell

Input setting unit

0.01(°), mm

0.001(°), mm/

0.0001 inch

0.01(°), mm

0.001(°), mm/

0.0001 inch

0.01(rev), mm X53 P8

Metric command

X+52 Y+52 Z+52

X+53 Y+53 Z+53

I+52 J+52 K+52

I+53 J+53 K+53

α

α

+52

+53

O8

N5

G2/G21

Inch command

X+44 Y+44 Z+44

I+44 J+44 K+44

α

+44

0.001(rev), mm/

0.0001 inch

X53 P8 X53 P8

Feed

Input setting unit function

Input setting unit

0.01(°), mm

0.001(°), mm/

0.0001 inch

F53

F53 F44

Input setting unit

Input setting unit

0.01(°), mm R+52 Q52 P8 L4

Fixed cycle

0.001(°), mm/

0.0001 inch

R+53 Q53 P8 L4 R+44 Q+44 P8 L4

Tool offset

Miscellaneous function

Spindle function

Tool function

H3/D3

M8

S6/S8

T8

2nd miscellaneous function A8/B8/C8

Subprogram P8H5L4

Variable number #5

(Note 1)

α

represents one of the additional axes U, V, W, A, B, or C.

(Note 2)

The No. of digits check for a word is carried out with the maximum number of digits of that address.

(Note 3)

The basic format is the same for any of the numerals input from the memory, MDI or setting display unit.

(Note 4)

Numerals can be used without the leading zeros.

(Note 5)

The program number is commanded with single block. It's necessary to command the program number in the head block of each program.

(Note 6)

The meanings of the details are as follows :

Example 1

: 08 :8-digit program number

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.

8

3. Data Formats

3.3 Program address check function

3.3 Program address check function


The program can be checked in word units when operating machining programs.


This function enables simple checking of program addresses in word units. If the alphabetic characters are continuous, the program error (P32) will occur. Availability of this function is selected by the parameter "#1227 aux11/bit4".

Note that an error will not occur for the following:

•

Reserved words

•

Comment statements

Example of program

(1) Example of program for address check

(Example 1)

When there are no numbers following an alphabetic character.

G28 X ;

→

An error will occur. Change to "G28 X0;", etc.

(Example 2)

When a character string is illegal.

TEST ;

→

An error will occur. Change to "(TEST);", etc.

3.4 Tape memory format


(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.

9

3. Data Formats

3.5 Optional block skip

3.5 Optional block skip ; /


This function selectively ignores specific blocks in a machining program which starts with the "/"

(slash) code.


(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.

10

3. Data Formats

3.6 Program/sequence/block numbers ; O, N

3.6 Program/sequence/block numbers ; O, N


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 "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 5 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

O12345678 (DEMO, PROG) ;

G92 X0 Y0 ;

G90 G51 X-150. P0.75 ;

N100 G00 X-50. Y-25. ;

N110 G01 X250. F300 ;

Y-225. ;

X-50. ;

Monitor display

Program No. Sequence No.

12345678

12345678

0

0

12345678

12345678

12345678

12345678

12345678

0

100

110

110

110

Block No.

0

1

2

0

0

1

2

N120 G51 Y-125. P0.5 ;

N130 G00 X-100. Y-75. ;

N140 G01 X-200. ;

Y-175. ;

X-100. ;

Y-75. ;

N150 G00 G50 X0 Y0 ;

N160 M02 ;

%

12345678

12345678

12345678

12345678

12345678

12345678

120

130

140

140

140

140

0

0

0

1

2

3

12345678

12345678

150

160

0

0

11

3. Data Formats

3.7 Parity H/V

3.7 Parity H/V


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.

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.

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

Parity H error example

• • • • • • • • • • • • • • • • • • •

• • • • • • • • • • • • • • • • • • •

•

•

• •

• •

•

•

•

• • •

•

•

•

• • •

•

• •

•

• •

•

• • • •

•

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

• • •

•

• • • •

•

• •

This character causes a parity H error.

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

(Note 2)

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

12

3. Data Formats

3.8 G code lists



G code

∆

00

* 01

02

03

Group

01 Positioning

01

01

01

Function

Linear interpolation

Circular interpolation CW (clockwise)

Circular interpolation CCW (counterclockwise)

06

07

08

09 00 Exact stop check

11

12

00

00

Program parameter input cancel

Circular cut CW (clockwise)

* 17

∆

18

∆

19

∆

20

13 00

14

15

16

02

02

02

Circular cut CCW (counterclockwise)

Plane selection X-Y

Plane selection Z-X

Plane selection Y-Z

06 Inch

29

30

30.1

30.2

30.3

30.4

30.5

30.6

* 21 06

22

23

24

25

26

27 00

28 00

00

00

00

00

00

00

00

00

31

31.1

31.2

31.3

00

00

00

00

32

Metric command

Reference point check

Reference point return

Start point return

2nd to 4th reference point return

Tool position return 1






Skip function / Multi-step skip function

Multi-step skip function 1-1



13

3. Data Formats

61

61.1

62

77

78

79

* 80

73

74

75

76

81

* 64

65

66

66.1

* 67

70

71

72

G code

41

42

43

44

* 49

* 50.1

51.1

52

34

35

36

37

37.1

38

39

* 40

53

* 54

55

56

57

58

59

54.1

Group

08

19

19

00

07

07

08

08

00

00

00

07

00

00

00

00

12

12

12

12

00

12

12

12

13

13

13

13

00

14

14

14

09

09

09

09

09


Function

Special fixed cycle (bolt hole circle)

Special fixed cycle (line at angle)

Special fixed cycle (arc)

Automatic tool length measurement

Special fixed cycle (grid)

Tool radius compensation vector designation

Tool radius compensation corner arc

Tool radius compensation cancel

Tool radius compensation left

Tool radius compensation right

Tool length offset (+)

Tool length offset (-)

Tool length offset cancel

G command mirror image cancel

G command mirror image ON

Local coordinate system setting

Machine coordinate system selection

Workpiece coordinate system 1 selection






Workpiece coordinate system selection 48 sets expanded

Exact stop check mode

High-accuracy control mode

Automatic corner override

Cutting mode

User macro call

User macro modal call A

User macro modal call B

User macro modal call cancel

User fixed cycle

User fixed cycle

User fixed cycle

Fixed cycle (step)

Fixed cycle (reverse tap)

User fixed cycle

Fixed cycle (fine boring)

User fixed cycle

User fixed cycle

User fixed cycle

Fixed cycle cancel

Fixed cycle (drill/spot drill)

14

3. Data Formats


86

87

88

89

∆

90

G code

82

83

84

85

Group

09

09

09

09

09

09

09

09

03

Function

Fixed cycle (drill/counter boring)

Fixed cycle (deep drilling)

Fixed cycle (tapping)

Fixed cycle (boring)


Fixed cycle (back boring)



Absolute value command

* 91

92

03

00

Incremental command value

Machine coordinate system setting

93

* 94

∆

95

∆

96

05

05

17

Asynchronous feed (per-minute feed)

Synchronous feed (per-revolution feed)

Constant surface speed control ON

* 97

* 98

99

113

114.1

17

10

10

00

00

Constant surface speed control OFF

Fixed cycle Initial level return

Fixed cycle R point level return

Spindle synchronous control OFF

100 ~ 255

00

Spindle synchronous control ON

•

Start point designation synchronization (type1)

•

Start point designation synchronization (type2)

•

User macro (G code call) Max. 10

(Note 1)

A (

∗

) symbol indicates the G code to be selected in each group when the power is turned

ON or when a reset is executed to initialize the modal.

(Note 2)

A (

∆

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

(Note 3)

A (

•

) symbol indicates a function dedicated for multi-part system.

(Note 4)

If two or more G codes from the same group are commanded, the last G code will be valid.

(Note 5)

This G code list is a list of conventional G codes. Depending on the machine, movements that differ from the conventional G commands may be included when called by the G code macro. Refer to the Instruction Manual issued by the machine manufacturer.

15

3. Data Formats


(Note 6)

Whether the modal is initialized differs for each reset input.

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

(2) "Reset 2 "and "Reset and Rewind"

The modal is initialized when the signal is input.

(3) Reset at emergency stop release

Conforms to "Reset 1".

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

Conforms to "Reset and Rewind".

CAUTION

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

3.9 Precautions before starting machining

Precautions before starting machining

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.

Carry out dry operation before actually machining, and confirm the machining program, tool offset and workpiece offset amount.

16

4. Buffer Register

4.1 Pre-read buffers

4. Buffer Register

Keyboard

Memory

MDI data

Analysis processing

Mode switching

Max. 5 execution blocks

Pre-read buffer 5 buffer 4 buffer 3 buffer 2 buffer 1

Arithmetic processing

Note

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

4.1 Pre-read buffers


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.

Precautions

(1) Depending on whether the program is executed continuously or by single blocks, the timing of the valid/invalid for the external control signals for the 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.)

17

5. Position Commands

5.1 Position command methods


5.1 Position command methods ; G90, G91


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

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

Command format

G90(G91) Xx1 Yy1 Zz1

αα

1

G90 :Absolute value command

α

:Additional


(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 ;

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.

N 2 G90 G01 X200. Y50. F100;

Y

200.

100. N1

W

Tool

100.

N2

200.

X

300.

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.

Y

200.

(G90)

N 3 X100. Y100.;

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

Y = 100mm position.

100.

N3

(G91)

N 3 X–100. Y50.;

W

100.

200.

X

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.

18


5.1 Position command methods

(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.

Y

200.

N 4 G90 X300. G91 Y100.;

N4

The X axis is treated in the absolute value mode, and with G90 is moved to the workpiece coordinate

100.

system 300.mm position. The Y axis is moved +100.mm with G91. As a result,

W

100. 200.

300.

Y moves to the 200.mm position. In terms of the next block, G91 remains as the modal and

X 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.

19


5.2 Inch/metric command change

5.2 Inch/metric command change; G20, G21


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

Command format

G20/G21;

G20

G21

: Inch command

: Metric command


G20 and G21 selection is meaningful only for linear axes and it is meaningless for rotary axes.

The input unit for G20 and G21 will not change just by changing the command unit.

In other words, if the machining program command unit changes to an inch unit at G20 when the initial inch is OFF, the setting unit of the tool offset amount will remain metric. Thus, take note to the setting value.

(Example 1)

Relationship between input command units and G20/G21 commands

(with decimal point input type 1)

Axis

Input command unit type (cunit)

Command Metric output (#1016 iout=0) Inch output (#1016 iout=1) example

G21 G20 G21 G20

X100; 0.254

mm 0.0039 inch 0.0100 inch

Y100; 0.254

mm 0.0039 inch 0.0100 inch

Z100; 0.254

mm 0.0039 inch 0.0100 inch

X100; 0.0254

Y100; 0.0254

Z100; 0.0254

(Note 1)

When changing between G20 and G21 with program commands, it is necessary in advance, to convert the parameters, variables, and the offsets for the tool diameter, tool position, tool length, to the units in the input settings of the input setting unit system (for each axis) that have inch or metric commands, and make the settings using the parameter tape.

(Example 2)

Input setting unit #1015 cunit=10, #1041 I_inch=0

Position command unit ..... 0.001mm

Compensation amount setting unit

..... When the compensation amount is 0.05mm for

0.001mm

In the above example, when changing from G21 to G20, the compensation amount must be set to 0.002 (0.05

÷

25.4

.

.

0.002).

(Note 2)

Since the data before the change will be executed at the command unit after the change, command the F speed command for the change so that it is the correct speed command for the command unit system applied after the change.

20


5.3 Decimal point input



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. A parameter "#1078 Decpt2" selects whether type 1 (minimum input command unit) or type 2 (zero point) is to apply for the least significant digit of data without a decimal point.

Command format

.

: Metric command

.

: Inch command


(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 system

cunit = 10

Type 1

1 (µm, 10

–4

inch, 10

–3

°

)

Type 2

1 (mm, inch,

°

)

cunit = 1 0.1 1

(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) See below for the number of significant digits in decimal point commands. (Input command unit cunit = 10)

Movement command (linear)

Integer

Decimal part

Movement command (rotary)

Integer

Decimal part

Feed rate

Integer

Decimal part

Dwell

Integer

Decimal part

MM

(millimeter)

0. to

99999.

.000 to

.999

0. to

99999.

.000 to.999

0. to

60000.

.00 to .99

0. to

99999.

.000 to

.999

INCH

(inch)

0. to 9999.

.0000 to

.9999

99999.

(359.)

.0 to .999 0. to 2362.

.000 to

.999

.0 to .99

.000 to

.999

(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.

21




(1) Example of program for decimal point valid address

Specification division

Program example

G0X123.45

(decimal points are all mm points)

Decimal point command 1

When 1 = 1

µ

m When 1 = 10

µ

m

Decimal point command 2

1 = 1mm

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

G0X12345

X12.345mm

(last digit is 1

µ m unit)

X123.000mm,

Y5,5550mm

X123.450mm X12345.000mm

X123.000mm,

Y5.550mm

X123.000mm,

Y5.550mm

#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)

#113 = 128.550

#114 = 117.450

#115 = 682.650

#116 = 22.162

#117 = 0.045

#113 = 128.550

#114 = 117.450

#115 = 682.650

#116 = 22.162

#117 = 0.045

#113 = 128.550

#114 = 117.450

#115 = 682.650

#116 = 22.162

#117 = 0.045

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 1

µ m 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 1

µ m system is equivalent to command "X1.".

(Note)

When a four rules operator is contained, the data will be handled as that with a decimal point.

(Example)

When the min. input command unit is 1

µ m :

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

µ m.

22


Address


Addresses used and valid/invalid decimal point commands

Decimal point command

Application Remarks

A

B

C

D

E

G

H

I

J

K

L

Valid

Invalid

Invalid

Valid

Invalid

Valid

Invalid

Valid

Invalid

Valid

Invalid

Invalid

Valid

Valid

Invalid

Invalid

Invalid

Invalid

Invalid

Valid

Valid

Valid

Valid

Valid

Valid

Valid

Valid

Valid

Invalid

Invalid

Invalid

Invalid

Invalid

Coordinate position data

Revolving table, miscellaneous function code

Data settings, axis numbers (G10)





Corner chamfering amount

Offset numbers (tool position, tool radius)

Automatic tool length measurement, deceleration range d

,c

Data settings byte type data

Synchronous spindle No. at spindle synchronization

Inch thread, number of ridges

Precision thread lead

Preparatory function code

Tool length offset number

Sequence numbers in subprograms

Program parameter input, bit type data

Linear-arc intersection selection (Geometric)

Basic spindle No. at spindle synchronization

Arc center coordinates

Tool radius compensation vector components

Hole pitch in the special fixed cycle

Circle radius of cut circle (increase amount)



Special fixed cycle's hole pitch or angle



Number of holes of the special fixed cycle

Number of fixed cycle and subprogram repetitions

Program tool compensation input type selection

Program parameter input selection

Program parameter input, 2-word type data

M Invalid Miscellaneous function codes

(Note 1)

All decimal points are valid for the user macro arguments.

L2, L12, L10,

L13, L11

L50

4 bytes

23



Address

Decimal point command

Application Remarks

Q

R

S

T

U

V

W

X

Y

Invalid

Invalid

Invalid

Invalid

Invalid

Invalid

Invalid

Invalid

Invalid

Invalid

Invalid

Valid

Valid

Valid

Invalid

Valid

Valid

Valid

Valid

Valid

Valid

Valid

Invalid

Invalid

Invalid

Invalid

Invalid

Valid

Valid

Valid

Valid

Valid

Program parameter input, data numbers

Subprogram program call No.

Dwell time at hole bottom of tap cycle

Number of holes of the special fixed cycle

Amount of helical pitch

Offset number (G10)

Constant surface speed control axis number

Program parameter input, broad classification number

Skip signal command for multi-step skip

Subprogram return destination sequence No.

2nd, 3rd, 4th reference point return number

Cut amount of deep hole drill cycle

Shift amount of back boring

Shift amount of fine boring

Minimum spindle clamp speed

Starting shift angle for screw cutting

R-point in the fixed cycle

R-specified arc radius

Corner rounding arc radius

Offset amount (G10)

Automatic tool length measurement, deceleration range r

,R

Parameter

Synchronous spindle phase shift amount

Spindle function codes

Maximum spindle clamp speed

Constant surface speed control, surface speed

Program parameter input, word type data

Tool function codes


2 bytes





Z Valid Coordinate position data

(Note 1)

All decimal points are valid for the user macro arguments.

24

6. Interpolation Functions


6.1 Positioning (Rapid traverse)


6.1 Positioning (Rapid traverse); G00


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 Xx Yy Zz

αα

,Ii ; (

α

represents additional axis)

x, y, z,

α

: Represent coordinates, and could be either absolute values or incremental values, depending on the setting of G90/G91. i : In-position width. A decimal point command will result in a program error. This is valid only in the commanded block. A block that does not contain this address will follow the parameter "#1193 inpos" settings.

The range is 1 to 999999 (

µ m).

(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. Refer to (Note4) of "Example of program".

(3) If multiple axes are controlled, the next block will be executed after confirming that the position error amounts of all the moving axes become within the specified in-position width for each part system.

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

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

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

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

(6) Refer to "Operation during in-position check" for the programmable in-position check positioning command.

CAUTION

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

25



Z


Tool

+300

Start point

(+150,-100,+150)

End point

(-120,+200,+300)

-100

+150

-120

+150

+200

Unit : mm

X

Y

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

(Note 1)

When parameter "#1086 G0Intp" is set to "0", the path along which the tool is positioned is the shortest path connecting the start and end points. The positioning speed is automatically calculated so that the shortest distribution time is obtained in order that the commanded speeds for each axis do not exceed the rapid traverse rate.

When for instance, the 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 fx

Actual X axis rate : 9600mm/min

Actual Y axis rate : 6400mm/min

Y fy

X

Start point

(Unit : mm)

26



(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

Actual Y axis rate : 9600mm/min

Y fy

X

300 fx

Actual X axis rate : 9600mm/min

Start point

(Unit : mm)

(Note 3)

The rapid traverse rate for each axis with the G00 command differs according to the individual machine and so reference should be made to the machine specifications manual.

(Note 4)

Rapid traverse (G00) deceleration check

There are two methods for the deceleration check at rapid traverse; commanded deceleration method and in-position check method. Select a method with the parameter

"#1193 inpos".

■

When “inpos” = “1”

Upon completion of the rapid traverse (G00), the next block will be executed after confirming that the remaining distances for each axis are below the fixed amounts.

(Refer to the following drawing.)

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

L

R

. L

R

is the setting value for the servo parameter "#2224 SV024".

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

27



■

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.

(a) Linear acceleration/linear deceleration Td = Ts +

α

Previous block Next block

Ts

Td

Ts : Acceleration/deceleration time constant

Td : Deceleration check time

Td = Ts + ( 0 ~ 14ms)

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

α


2 × Ts

Td Ts



Td = 2

×

Ts + ( 0 ~ 14ms)

(c) Exponential acceleration/exponential deceleration Td = 2 × Ts +

α


Ts

Td



Td = 2

×

Ts + ( 0 ~ 14ms)

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.

28



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 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

In-position check with ",I" address command

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

Block being executed

Servo

Command

In-position width

(Error amount of command end point and machine position)

In-position check with parameter

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

Command

In-position width

(Servo system position

error amount)

Ts

Td

Ts

Td

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



Td = Ts + (0 to 14ms)

Start of in-position check with parameter

29


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

Command to motor

Outline of motor movement

G0 in-position sv024

A stop is judged here.

In-position check using the

“G1inps” value

Command to motor

Outline of motor movement

G1 in-position sv024

A stop is judged here.

When the SV024 value is larger, the in-position check is completed when the motor position becomes within the specified with SV024.

The in-position check method depends on the method set in the deceleration check parameter.

(Note 1)

When the in-position width check is carried out, the in-position width command in the program takes place the in-position width set with the parameters such as SV024,

G0inps, or G1inps.

(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.

30


6.2 Linear interpolation

6.2 Linear interpolation; G01


This command is accompanied by coordinate words and a feedrate command.

It makes the tool move (interpolate) linearly from its 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 Xx Yy Zz

αα

Ff ,Ii ; (

α

represents additional axis)

x, y, z,

α

:Coordinate values and may be an absolute position or incremental position depending on the G90/G91 state. f :Feedrate (mm/min or

°

/min) i :In-position width. A decimal point command will result in a program error. This is valid only in the commanded block. A block that does not contain this address will follow the parameter "#1193 inpos" settings.

The range is 1 to 999999 (

µ m).


(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

°

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

300

°

/min)

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

31


6.2 Linear interpolation


(Example 1)

Cutting in the sequence of P

1

→

P

0

→

P

1

is for tool positioning

P

2

→

P

3

→

P

4

→

P

1

at 300 mm/min feedrate

30

Y

P

2

P

3

X

P

1

20 20

P

4

Unit: mm

Input setting unit: 0.001mm

P

0

G90 G00 X20000 Y20000 ; P

0

→

P

1

G01 X20000 Y30000 F300 P

1

X-30000 ;

P

2

Y-30000 P

P

4

→

P

→

P

3

→

P

→

P

2

3

4

1

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__ ;

In-position width

Feedrate

Linear interpolation coordinate value of each axis

(Note 1)

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

32


6.3 Plane selection

6.3 Plane selection; G17, G18, G19


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

•

Plane that executes fixed cycle positioning.

Command format

G17 ;

G18 ;

G19 ;

(ZX plane selection)

(YZ plane selection)

(XY plane selection)

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

Parameter entry

#1026 to 1028 base_I,J,K

#1029 to 1039 aux_I,J,K

I X U

J Y

K Z V

Table 1 Example of plane selection parameter entry

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

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

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

33


Plane selection system

6.3 Plane selection

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

Y__Z__ ; XY plane (plane does not change)

(3) I f 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.


G17 ; XY plane

G17U__ ;

G18U__ ;

G18V__ ;

G19Y__ ;

G19V__ ;

UY plane

ZU plane

VX plane

YZ plane

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.


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.


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.

34


6.4 Circular interpolation; G02, G03


These commands serve to move the tool along an arc.

Command format

G02 (G03) Xx Yy Ii Jj Kk Ff;

G02

G03

Xx, Yy

Ii, Jj

: Clockwise (CW)

: Counterclockwise (CCW)

: End point

: Arc center

6.4 Circular interpolation

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.

35




(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)

Z

G2

G2

G3

G3

G3

G2

Y

Y

G03

X

X

G03

Z

G03

G02 G02 G02

X

Z

Y

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

G19(Y-Z)plane

(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)?

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

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

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

36



(Example 1)

Y axis

+Y


Feedrate

F = 500mm/min

Circle center

J = 50mm

X axis

(Example 2)

G02 J50000 F500 ;

Y axis

+Y

Start point/end point

+X

Circle command

Feedrate

F = 500mm/min

Arc center

J = 50mm

End point

X50 Y50mm

X axis

+X

Start point

G91 G02 X50000 Y50000 J50000 F500 ; 3/4 command

37


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


YZ plane


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

∆

R is greater than parameter

"#1084 RadErr".

(G91) G02X9.899I 5. ;

#1084 RadErr parameter value 0.100

Start point radius = 5.000

End point radius = 4.899

Error

∆

R = 0.101

Alarm stop

Start point

Start point radius

Center

End point

End point radius

∆

R

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

∆

R is less than the parameter value.

(G91) G02X9.9I 5. ;

Spiral interpolation

#1084 RadErr parameter value 0.100

Start point radius = 5.000

End point radius = 4.900

Error

∆

R = 0.100

Start point

Start point radius

Center

End point

End point radius

∆

R

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

38


6.5 R-specified circular interpolation

6.5 R-specified circular interpolation; G02, G03


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) Xx Yy Rr Ff ;

x y r

: X-axis end point coordinate

: Y-axis end point coordinate

: Arc radius

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.


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.

Arc path when

R sign is minus

02

Center point

Center point

End point

Arc path when

R sign is plus

L

Center point

01

Start point r

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.

39



6.5 R-specified circular interpolation

(Example 1)

(Example 2)

G02 Xx

1

Yy

1

Rr

1

Ff

1

;

(Example 3)

G03 Zz

1

Xx

1

Rr

1

Ff

1

;

XY plane R-specified arc

ZX plane R-specified arc

(Example 4)

G02 Xx

1

Yy

1

Ii

1

Jj

1

Rr

1

Ff

1

; XY plane R-specified arc

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

G17 G02 Ii

1

Jj

1

Rr

1

Ff

1

; XY plane This is an R-specified arc, but as this is a circle command, it is already completed.

40


6.6 Helical interpolation

6.6 Helical interpolation ; G17 to G19, G02, G03


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.

Command format

G17 G02 (G03) Xx

1

Yy

1

Zz

1

Ii

1

Jj

1

Pp

1

Ff

1

;

G17 G02 (G03) Xx

2

Yy

2

Zz

2

Rr

2

Ff

2

;

Xx

1

Yy

1

Xx

2

Yy

2

: Arc end point coordinate

Zz

1

Zz

2

: Linear axis end point coordinate

Ii

1

Jj

Pp

1

1

: Arc center coordinate

: Pitch No.

Ff

1

Ff

2

Feedrate

Rr

2

: Arc radius

The arc center coordinate value and arc radius value 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.

41


Z axis


Y axis

P

1 time

l

Z

1

Second time

First time


θ

θ e

Y

End point

θ s

X

Start point

X axis

(1) For this command, command a linear axis (multiple axes can be commanded) that does not contain a circular axis in the circular interpolation command.

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

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

l

=

Z1

(2

π

• P1 +

θ

) / 2

π

θ

=

θ

E

− θ s = tan

–1 ye xe

– tan

–1 ys xs

(0

≤ θ

< 2

π

)

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 99.

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

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


YZ plane circular, X axis linear


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

UY plane circular, Z axis linear

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

In addition to the basic command methods above, the command methods following the program example can be used. Refer to the section "6.4 plane selection" for the arc planes selected with these command methods.

42




(Example 1)

Z axis

Y axis z

1

X axis

G17 ; XY plane

G03 Xx

1

Yy

1

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

(Example 2)

(Note)

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

Z axis

G17 ;

G02 Xx1 Yy1 Zz1 Rr1 Ff1 ;

Y axis z

1 r

1

X axis

XY plane

XY plane arc, Z axis linear

(Example 3)

Z axis

Y axis z

1

U axis

(Example 4)

G17 G03 Uu

1

Yy

1

Zz

1

Ii

1

Jj

1

P2 Ff

1

; UY plane arc, Z axis linear

U axis X axis u

1 x

1

Z axis z

1

G18 G03 Xx

1

Uu

1

Zz

1

Ii1 Kk

1

Ff

1

; 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.

43



(Example 5)

G18 G02 Xx

1

Uu

1

Yy

1

Zz

1

Ii

1

Jj

1

Kk

1

Ff

1

;

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.

44


6.7 Thread cutting


6.7.1 Constant lead thread cutting ; G33


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

Command format

G32 Zz Ff

1

Qq ; (Normal lead thread cutting commands)

Zz

Ff

Qq

: Thread cutting direction axis address (X, Y, Z, a) and thread length

: Lead of long axis (axis which moves most) direction.

: Thread cutting start shift angle, (0 to 360°)

G33 Zz Ee

1

Qq ; (Precision lead thread cutting commands)

Zz

Ee

Qq

: Thread cutting direction axis address (X, Y, Z,

α

) and thread length

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

: Thread cutting start shift angle, (0 to 360

°

)


(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.

Z

LZ a

Tapered thread section

LX

X

When a<45

°

lead is LZ

When a>45

°

lead is LX

When a=45

°

lead can be in either LX or LZ

Thread cutting Metric input

Input unit system

Command address

F (mm/rev)

Minimum command unit

Command range

1 (= 1.000),

(1.=1.000)

0.001 to

999.999

B (0.001mm)

E (mm/rev)

1 (= 1.00000),

(1.=1.00000)

0.00001 to

999.99999

E (threads/ inch)

1 (= 1.00),

(1.=1.00)

0.03 to 999.99

F (mm/rev)

1 (= 1.0000),

(1.=1.0000)

0.00001 to

99.9999

C (0.0001mm)

E (mm/rev)

1(=1.00000),

(1.=1.00000)

0.000001 to

99.99999

E (threads/ inch)

1 (= 1.000),

(1.=1.000)

0.1 to

2559999.999

45



Thread cutting Inch input


Command address

F (inch/rev)


Command range

1(=1.0000),

(1.=1.0000)

0.0001 to

99.9999

B (0.0001inch)

E (inch/rev)

1(=1.000000),

(1.=1.000000)

0.000001 to

39370078

E (threads/

inch)

1 (= 1.0000),

(1.=1.0000)

0.0255 to

9999.9999

F (inch/rev)

1(=1.00000),

(1.=1.00000)

0.00001 to

3937009

C (0.00001inch)

E (inch/rev)

1(=1.000000),

(1.=1.000000)

0.000001 to

3937009

E (threads/ inch)

1(=1.0000),

(1.=1.0000)

0.25401 to

999.9999

(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 thread cutting will start by the one rotation synchronous signal from the encoder installed on the spindle.

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

(5) If the feed hold function is employed during thread cutting to stop the feed, the thread ridges will lose their shape. For this reason, feed hold does not function during thread cutting.

If the feed hold switch is pressed during thread cutting, block stop will result at the end point of the block following the block in which thread cutting is completed (no longer G33 mode).

(6) The converted cutting 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.

(7) In order to protect the lead during thread cutting, a cutting feed rate which has been converted may sometimes exceed the cutting feed clamp rate.

(8) An illegal lead is normally produced at the start of the thread and at the end of the cutting because of servo system delay and other such factors.

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

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

1

≤

R

≤

Maximum feedrate

Thread lead

Where R

≤

Permissible speed of encoder (r/min)

R

Thread lead

: Spindle speed (r/min)

: mm or inches

Maximum feedrate : mm/min or inch/mm (This is subject to the restrictions imposed by the machine specifications).

(10) The thread cutting start angle is designated with an integer or 0 to 360.

46




10

50

10

Z

X

Y

X

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

N111 Z110. ;

N112 G33 Z40. F6.0 ;

N113 M19 ;

N114 G0X-210. ;

N115 Z110. M0 ;

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

The first thread cutting is executed. Thread lead =

6.0mm

Spindle orientation is executed with the M19 command.

The tool is evaded in the X axis direction.

The tool rises to the top of the workpiece, and the program stops with M00.

Adjust the tool if required.

Preparation for second thread cutting is done. N116 X-200. ;

M3 ;

N117 G04 X5.0 ;

N11 G33 Z40. ;

Command dwell to stabilize the spindle rotation if necessary.

The second thread cutting is executed.

47



6.7.2 Inch thread cutting; G33


If the number of ridges per inch in the long axis direction is assigned in the G33 command, the feed of the tool 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 Zz Ee Qq ;

Zz

Ee

: Thread cutting direction axis address (X, Y, Z,

Qq


α

) and thread length

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

: Thread cutting start shift angle, 0 to 360

°

.

(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.

48



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

When programmed with

δ

1

= 10mm,

δ

2

= 10mm using metric input

Z


δ

1

50.0mm

δ

2

X

Y

X

N210 G90 G0X-200. Y-200. S50M3;

N211 Z110.;

N212 G91 G33 Z-70.E3.0;

N213 M19;

(First thread cutting)

N214 G90 G0X-210.;

N215 Z110.M0;

N216 X-200.;

M3;

N217 G04 X2.0;

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

6.8 Uni-directional positioning; G60


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

49


Command format

G60 Xx Yy Zz

α

α

;

α

: Additional axis


6.8 Uni-directional positioning

(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.

G60a

Positioning position

[Final advance direction]

-

Start point

End point Start point

+

Stop once

G60-a

[G60creep distance]

(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.

50

7. Feed Functions

7.1 Rapid traverse rate


7.1 Rapid traverse rate


The rapid traverse rate can be set independently for each axis. The available speed ranges are from 1 mm/min to 1,000,000 mm/min for input setting units of 1µm. The upper limit is subject to the restrictions imposed by the machine specifications.

Refer to the specifications manual of the machine for the rapid traverse rate settings.

The feedrate is valid for the G00, G27, G28, G29, G30 and G60 commands.

Two paths are available for positioning: the interpolation type where the area from the start point to the end point is linearly interpolated or the non-interpolation type where movement proceeds at the maximum speed of each axis. The type is selected with parameter "#1086 G0Intp". The positioning time is the same for each type.

7.2 Cutting feed rate


The cutting feedrate is assigned with address F and 8 digits (F8-digit direct designation).

The F8 digits are assigned with a decimal point for a 5-digit integer and a 3-digit fraction. The cutting feedrate is valid for the G01, G02, G03 and G33 commands.

(Examples)

Feedrate Remarks

G1 X100. Y100. F200 ;

G1 X100. Y100. F123.4 ;

G1 X100. Y100. F56.789 ;

200.0mm/min

123.4mm/min

56.789mm/min

F200. or F200.000 gives the same rate.

Speed range that can be commanded (when input setting unit is 1

µ m or 10

µ m)

Command mode F command range Feed rate command range Remarks

mm/min inch/min

°

/min

0.001 to 1000000.000

0.001 to 1000000.000 mm/min

0.0001 to 39370.0787

0.0001 to 39370.0787 inch/min

0.001 to 1000000.000

0.01 to 1000000 °/min

(Note 1)

A program error (P62) results when there is no F command in the first cutting command

(G01, G02, G03) after the power has been switched on.

51


7.3 F1-digit feed



By setting the F1-digit feed parameter, the feedrate which has been set to correspond to the 1-digit number following the F address serves as the command value.

When F0 is assigned, the rapid traverse rate is established and the speed is the same as for G00.

(G modal does not change.)

When F1 to F5 is assigned, the feedrate set to correspond to the command serves as the command value.

The command greater than F6 is considered to be the normal cutting feedrate.

The F1-digit command is valid only in a G01, G02 or G03 modal.

The F1-digit command can also be used for fixed cycle.


Set the corresponding speed of F1 to F5 with the base specification parameters "#1185 spd_F1" to

"#1189 spd_F5" respectively.

Operation alarm "104" will occur when the feedrate is 0.

(1) Operation method

(a) Make the F1-digit command valid. (Set the base specification parameter "#1079 F1digt" to 1.)

(b) Set F1 to F5. (Base specification parameter "1185 spd_F1" to "#1189 spd_F5")

(2) Special notes

(a) Use of both the F1-digit command and normal cutting feedrate command is possible when the

F1-digit is valid.

(Example 1)

F0

F1 to F5

F6 or more

Rapid traverse rate

F1-digit

Normal cutting feedrate command

(b) F1 to F5 are invalid in the G00 mode and the rapid traverse rate is established instead.

(c) If F0 is used in the G02 or G03 mode, a program error (P121) will result. commands are established instead of the F1-digit command.

(e) When the commands are used with the millimeter or degree units, the feedrate set to correspond to F1 to F5 serves as the assigned speed mm (

°

)/min.

(f) When the commands are used with inch units, one-tenth of the feedrate set correspond to F1 to F5 serves at the assigned speed inch/min.

(g) During a F1-digit command, the F1-digit number and F1-digit command signal are output as the PLC signals.

52



(3) F1-digit and G commands

(a) 01 group G command in same block as F1-digit commands

G0F0

F0G0

G0F1

F1G0

G1F0

F0G1

G1F1

F1G1

Executed feedrate

Rapid traverse rate

Rapid traverse rate

Rapid traverse rate

F1 contents

Modal display rate

0

1

0

1

G modal

G0

G0

G1

G1

(b) F1-digit and unmodal commands may be assigned in the same block. In this case, the unmodal command is executed and at the same time the F1-digit modal command is updated.

53


7.4 Synchronous feed

7.4 Synchronous feed; G94, G95


Using the G95 command, it is possible to assign the feed amount per rotation with an F code.

When this command is used, the rotary encoder must be attached to the spindle.

When the G94 command is issued the per-minute feed rate will return to the designated per-minute feed (asynchronous feed) mode.

Command format

G94;

G95;

G94

G95

: Per-minute feed (mm/min) (asynchronous feed) (F1 = 1mm/min)

: Per-revolution feed (mm/rev) (synchronous feed) (F1 = 0.01mm/rev)

The G95 command is a modal command and so it is valid until the G94 command (per-minute feed) is next assigned.

(1) The F code command range is as follows.

The movement amount per spindle revolution with synchronous feed (per-revolution feed) is assigned by the F code and the command range is as shown in the table below.

Metric input


Command mode

Command address


Command range

Inch input

B (0.001mm)

Feed per minute

F (mm/min)

1 (= 1.00),

(1. = 1.00)

0.01 to 1000000.00

Feed per rotation

E (mm/rev)

1 (= 0.01),

(1. = 1.00)

0.001 to 999.999

C (0.0001mm)

Feed per minute

F (mm/min)

1 (= 1.000),

(1. = 1.000)

Feed per rotation

E (mm/rev)

1 (= 0.01),

(1. = 1.00)

0.001 to 100000.000 0.0001 to 99.9999


Command mode

Command address


B (0.0001inch)

Feed per minute

F (inch/min)

Feed per rotation

E (inch/rev)

C (0.00001inch)

Feed per minute

F (inch/min)

Feed per rotation

E (inch/rev)

1 (= 1.000),

(1. = 1.000)

1 (= 0.001),

(1. = 1.000)

1 (= 1.0000),

(1. = 1.0000)

1 (= 0.001),

(1. = 1.000)

Command range

0.001 to 100000.0000

0.0001 to 999.9999

0.0001 to

10000.00000

0.00001 to 99.99999

(2) The effective speed (actual movement speed of machine) under per-revolution feed conditions is given in the following formula (Formula 1).

FC = F

×

N

×

OVR ..... (Formula 1)

Where FC = Effective rate (mm/min, inch/min)

F = Commanded feedrate (mm/rev, inch/rev)

N =

OVR =

Spindle speed (r/min)

Cutting feed override

When a multiple number of axes have been commanded at the same time, the effective rate

FC in formula 1 applies in the vector direction of the command.

54


7.4 Synchronous feed

(Note 1)

The effective rate (mm/min or inch/min), which is produced by converting the commanded speed, the spindle speed and the cutting feed override into the per-minute speed, appears as the FC on the monitor 1. Screen of the setting and display unit.

(Note 2)

When the above effective rate exceeds the cutting feed clamp rate, it is clamped at that clamp rate.

(Note 3)

If the spindle speed is zero when synchronous feed is executed, operation alarm

"105" results.

(Note 4)

During machine lock high-speed processing, the rate will be 60,000mm/min (or

2,362 inch/min, 60,000 °/min) regardless of the commanded speed and spindle speed. When high-speed processing is not undertaken, the rate will be the same as for non-machine lock conditions.

(Note 5)

Under dry run conditions, asynchronous speed applies and movement results at the externally set rate (mm/min, inch/min, °/min).

(Note 6)

The fixed cycle G84 (tapping cycle) and G74 (reverse tapping cycle) are executed to the feed mode that is already designated.

(Note 7)

Whether asynchronous feed (G94) or synchronous feed (G95) is to be established when the power is switched on or when M02 or M30 is executed is set with parameter "#1074 I_Sync".

55


7.5 Feedrate designation and effects on control axes



It has already been mentioned that a machine has a number of control axes. These control axes can be divided into linear axes which control linear movement and rotary axes which control rotary movement. The feedrate is designed to assign the displacement speed of these axes, and the effect exerted on the tool movement speed which poses problems during cutting differs according to when control is exercised over the linear axes or when it is exercised over the rotary axes.

The displacement amount for each axis is assigned separately for each axis by a value corresponding to the respective axis. The feedrate is not assigned for each axis but assigned as a single value. Therefore, when two or more axes are to be controlled simultaneously, it is necessary to understand how this will work for each of the axes involved.

The assignment of the feedrate is described with the following related items.

When controlling linear axes

Even when only one machine axis is to be controlled or there are two or more axes to be controlled simultaneously, the feed rate which is assigned by the F code functions as a linear speed in the tool advance direction.

(Example)

When the feedrate is designated as "f" and linear axes (X and Y) are to be controlled.

Y y

P

2

(Tool end point) x

Feedrate for X axis = f x

x

2

+ y

2 y

Feedrate for Y axis = f x

x

2

+ y

2

Speed in this direction is "f"

P (Tool start point) x X

When only linear axes are to be controlled, it is sufficient to designate the cutting feed in the program. The feedrate for each axis is such that the designated rate is broken down into the components corresponding to the movement amounts.

(Note)

When the circular interpolation function is used and the tool is moved along the circumference of an arc by the linear control axis, the rate in the tool advance direction, or in other words the tangential direction, will be the feedrate designated in the program.

Y

P

2 y

Linear speed is "f" x i

P

1

X

56



(Example)

When the feedrate is designated as "f" and the linear axes (X and Y) are to be controlled using the circular interpolation function.

In this case, the feed rate of the X and Z axes will change along with the tool movement. However, the combined speed will always be maintained at the constant value "f".

When controlling rotary axes

When rotary axes are to be controlled, the designated feedrate functions as the rotary speed of the rotary axes or, in other words, as an angular speed.

Consequently, the cutting feed in the tool advance direction, or in other words the linear speed, varies according to the distance between the center of rotation and the tool. This distance must be borne in mind when designating the feedrate in the program.

(Example)

When the feedrate is designated as "f" and rotary axis (CA) is to be controlled ("f" units =

°

/min)

P

2

(tool end point)

Angular speed is "f" c

Linear speed is :

π

•r•f

180

P

1

(tool start point)

Rotation center r

In this case, in order to make the cutting feed (linear feed) in the tool advance direction "fc" : fc = f

×

π •

r

180

Therefore, the feedrate to be designated in the program must be : f = fc

×

180

π •

r

When linear and rotary axes are to be controlled at the same time

The controller proceeds in exactly the same way whether linear or rotary axes are to be controlled.

When a rotary axis is to be controlled, the numerical value assigned by the coordinate word (A, B,

C) is the angle and the numerical values assigned by the feedrate (F) are all handled as linear speeds. In other words, 1

°

of the rotary axis is treated as being equivalent to 1mm of the linear axis.

Consequently, when both linear and rotary axes are to be controlled simultaneously, the components for each axis of the numerical values assigned by F will be the same as previously described "When controlling linear axes". However, although in this case both the size and direction of the speed components based on linear axis control do not vary, the direction of the speed components based on rotary axis control will change along with the tool movement (their size will not change). This means, as a result, that the combined tool advance direction feedrate will vary along with the tool movement.

57



(Example)

When the feed rate is designated as "f" and Linear (X) and rotary © axes are to be controlled simultaneously.

In the X-axis incremental command value is "x" and the C-axis incremental command values is "c": fc

P

2 ft fx

Size and direction are fixed for fx.

Size is fixed for fc but direction varies.

Both size and direction vary for ft. fc

θ r ft

P

1 c fx

θ x

Rotation center

X-axis feedrate (linear speed) "fx" and C-axis feedrate (angular speed) "

ω

" are expressed as: fx = f

× x

x

2

+ c

2

........................................................................................ (1)

ω

= f

× c

x

2

+ c

2

......................................................................................... (2)

Linear speed "fc" based on C-axis control is expressed as: fc =

ω ×

π ×

r

180

.................................................................................................. (3)

If the speed in the tool advance direction at start point P1 is "ft" and the component speeds in the

X-axis and Y-axis directions are "ftx" and "fty", respectively, then these can be expressed as: ftx =

− rsin (

π

180

θ

)

×

π

180

ω

+ fx .............................................................. (4) fty =

− rcos (

π

θ

)

×

π

ω

..................................................................... (5)

180 180

Where r is the distance between center of rotation and tool (in mm units), and

θ

is the angle between the P1 point and the X axis at the center of rotation (in units

°

).

The combined speed "ft" according to (1), (2), (3), (4) and (5) is: ft =

ftx

2

+ fty

2

= f

×

x

2

– x

•

c

•

rsin (

π

180

θ

)

x

2

+ c

2

π

90

+ (

π •

r

•

c

180

)

2

................... (6)

Consequently, feedrate "f" designated by the program must be as follows: f = ft

×

x

2

+ c

2

x

2

– x

•

c

•

rsin (

π

180

θ

)

π

90

+ (

π •

r

•

c

180

)

2

.................... (7)

"ft" in formula (6) is the speed at the P1 point and the value of

θ

changes as the C axis rotates, which means that the value of "ft" will also change.

Consequently, in order to keep the cutting feed "ft" as constant as possible the angle of rotation which is designated in one block must be reduced to as low as possible and the extent of the change in the

θ

value must be minimized.

58


7.6 Automatic acceleration/deceleration

7.6 Automatic acceleration/deceleration


The rapid traverse and manual feed acceleration/deceleration pattern is linear acceleration and linear deceleration.

Time constant T

R

can be set independently for each axis using parameters in 1ms steps from 1 to

500ms.

The cutting feed (not manual feed) acceleration/deceleration pattern is exponential acceleration/ deceleration. Time constant Tc can be set independently for each axis using parameters in 1ms steps across a range from 1 to 500ms. (Normally, the same time constant is set for all axes.) f

With continuous

commands f

With continuous commands t t

T

R

T

R

T d

T

C

T

C

Rapid traverse acceleration/deceleration

Pattern

(T

R

= Rapid traverse time constant)

(T d

= Deceleration check time)

Cutting feed acceleration/deceleration pattern

(T c

= Cutting feed time constant)

With rapid traverse and manual feed, the following block is executed after the command pulse of the present block has become "0" and the tracking error of the acceleration/deceleration circuit has become "0". However, with cutting feed, the following block is executed as soon as the command pulse of the present block becomes "0" although an external signal (error detect) can detect that the tracking error of the acceleration/deceleration circuit has reached "0" and the following block can be executed. When the in-position check has been made valid (selected by parameter "#1193 inpos") during the deceleration check, it is first confirmed that the tracking error of the acceleration/deceleration circuit has reached "0", then it is checked that the position deviation is less than the parameter setting value "#2204 SV024", and finally the following block is executed. It depends on the machine as to whether the error detect function can be activated by a switch or M function and so reference should be made to the instructions issued by the machine maker.

7.7 Speed clamp


This function exercises control over the actual cutting feedrate in which override has been applied to the cutting feedrate command so that the speed clamp value which has been preset independently for each axis is not exceeded.

(Note)

Speed clamping is not applied to synchronous feed and thread cutting.

59


7.8 Exact stop check

7.8 Exact stop check; G09


In order to prevent roundness during corner cutting and machine shock when the tool feedrate changes suddenly, there are times when it is desirable to start the commands in the following block once the in-position state after the machine has decelerated and stopped or the elapsing of the deceleration check time has been checked. The exact stop check function is designed to accomplish this purpose.

Either the deceleration check time or in-position state is selected with parameter "#1193 inpos".

In-position check is valid when "#1193 inpos" is set to 1.

The in-position width is set with parameter "#2224 sv024" on the servo parameter screen by the machine manufacturer.

Command format

G09 ;

The exact stop check command G09 has an effect only with the cutting command (G01 - G03) in its particular block.


N001 G09 G01 X100.000 F150 ; The following block is started once the deceleration check time or in-position state has been checked after the machine has decelerated and stopped.

N002 Y100.000 ;

Tool

With G09 f (Commanded speed)

N001

X axis

N001

Without G09

N002

Time

Y axis

N002

Solid line indicates speed pattern with G09 command.

Broken line indicates speed pattern without G09 command.

Fig. 1 Exact stop check result

60



(1) With continuous cutting feed

Previous block


Next block

Ts

Fig. 2 Continuous cutting feed command

(2) With cutting feed in-position check

Previous block

Next block

Lc (in-position width)

Ts Ts

Fig. 3 Block joint with cutting feed in-position check

In Figs. 2 and 3:

Ts = Cutting feed acceleration/deceleration time constant

Lc = In-position width

As shown in Fig. 3, the in-position width "Lc" can be set into the servo parameter "#2224

SV024" as the remaining distance (shaded area in Fig. 3) of the previous block when the next block is started.

The in-position width is designed to reduce the roundness at the workpiece corners to below the constant value.

Lc

Previous block

Next block

To eliminate corner roundness, set the servo parameter "#2224 SV024" to zero and perform an in-position check or assign the dwell command (G04) between blocks.

61


(3) With deceleration check

(a) With linear acceleration/deceleration


Previous block

Next block

Ts

Td



Td = Ts + ( 0 ~ 14ms)

(b) With exponential acceleration/deceleration


Ts



Td = 2

×

Ts + ( 0 ~ 14ms)

Td

(c) With exponential acceleration/linear deceleration


2 x Ts

Td Ts



Td = 2

×

Ts + ( 0 ~ 14ms)

The time required for the deceleration check during cutting feed is the longest among the cutting feed deceleration check times of each axis determined by the cutting feed acceleration/deceleration time constants and by the cutting feed acceleration/ deceleration mode of the axes commanded simultaneously.

(Note 1)

To execute exact stop check in a fixed cycle cutting block, insert command G09 into the fixed cycle subprogram.

62


7.9 Exact stop check mode

7.9 Exact stop check mode ; G61


Whereas the G09 exact stop check command checks the in-position status only for the block in which the command has been assigned, the G61 command functions as a modal. This means that deceleration will apply at the end points of each block to all the cutting commands (G01 to G03) subsequent to G61 and that the in-position status will be checked. G61 is released by high-accuracy control mode (G61.1), automatic corner override (G62), tapping mode (G63), or cutting mode (G64).

Command format

G61 ;

In-position check is executed in the G61 block, and thereafter, the in-position check is executed at the end of the cutting command block is executed until the check mode is canceled.

63


7.10 Automatic corner override

7.10 Automatic corner override ; G62


With tool radius compensation, this function reduces the load during inside cutting of automatic corner R, or during inside corner cutting, by automatically applying override to the feed rate.

Automatic corner override is valid until the tool radius compensation cancel (G40), exact stop check mode (G61), high-accuracy control mode (G61.1), tapping mode (G63), or cutting mode

(G64) command is issued.

Command format

G62 ;

Machining inside corners

When cutting an inside corner as in Fig. 1, the machining allowance amount increases and a greater load is applied to the tool. To remedy this, override is applied automatically within the corner set range, the feedrate is reduced, the increase in the load is reduced and cutting is performed effectively.

However, this function is valid only when finished shapes are programmed. workpiece

θ

Programmed path

(finished shape)

Machining allowance

S

(3)

(1)

(2)

Workpiece surface shape

Tool center path

Machining allowance

Ci

Deceleratio range

Tool

θ

: Max. angle at inside corner

Ci : Deceleration range (IN)

Fig.1

64



(1) Operation

(a) When automatic corner override is not to be applied :

When the tool moves in the order of (1)

→

(2)

→

(3) in Fig. 1, the machining allowance at

(3) increases by an amount equivalent to the area of shaded section S and so the tool load increases.

(b) When automatic corner override is to be applied :

When the inside corner angle

θ

in Fig. 1 is less than the angle set in the parameter, the override set into the parameter is automatically applied in the deceleration range Ci.

The following parameters are set into the machining parameters :

# Parameter

#8007 OVERRIDE 0 to 100%

0 to 180

°

#8009 DSC. ZONE 0 to 99999.999mm or 0 to 3937.000 inches

Refer to the Operation Manual for details on the setting method.

Automatic corner R

Corner R center

Workpiece

Corner

R section

Ci

Machining allowance

(1) The override set in the parameter is automatically applied at the deceleration range Ci and corner R section for inside offset with automatic corner R. (There is no angle check.)

65


Application example


(1) Line line corner

θ

Ci

Tool

Program

Tool center

The override set in the parameter is applied at Ci.

(2) Line arc (outside) corner

Program

Tool center

θ

Tool

Ci


(3) Arc (inside offset)

−

line corner

Program

θ

Ci

Tool center

Tool

Tool


(

Note)

The deceleration range Ci where the override is applied is the length of the arc with an arc command.

(4) Arc (inside offset)

−

arc (outside offset) corner

N1

θ

N2

Ci

Program

Tool center


66


Relation with other functions


Function

Cutting feed override

Override at corner

Automatic corner override is applied after cutting feed override has been applied.

Override cancel

Speed clamp

Dry run

Synchronous feed

Automatic corner override is not canceled by override cancel.

Valid after automatic corner override

Automatic corner override is invalid.

Automatic corner override is applied to the synchronous feedrate.

Automatic corner override is invalid. Thread cutting

G31 skip Program error results with G31 command during tool radius compensation.

Machine lock Valid

Machine lock high speed Automatic corner override is invalid.

G00 Invalid

G01 Valid

G02, G03 Valid

67


Precautions


(1) Automatic corner override is valid only in the G01, G02, and G03 modes; it is not effective in the G00 mode. When switching from the G00 mode to the G01 (or G02 or G03) mode at a corner (or vice versa), automatic corner override will not be applied at that corner in the G00 block.

(2) Even if the automatic corner override mode is entered, the automatic corner override will not be applied until the tool diameter compensation mode is entered.

(3) Automatic corner override will not be applied on a corner where the tool radius compensation is started or canceled.

Start-up block

Program

Tool center

Cancel block

Automatic corner override will not be applied

(4) Automatic corner override will not be applied on a corner where the tool radius compensation

I, J vector command is issued.

Program

Tool center

Block containing

I, J vector command

Automatic corner override will not be applied

(G41X_Y_I_J_;)

(5) Automatic corner override will not be applied when intersection calculation cannot be executed.

Intersection calculation cannot be executed in the following case.

(a) When the movement command block does not continue for four or more times.

(6) The deceleration range with an arc command is the length of the arc.

(7) The inside corner angle, as set by parameter, is the angle on the programmed path.

(8) Automatic corner override will not be applied when the maximum angle in the parameter is set to 0 or 180.

(9) Automatic corner override will not be applied when the override in the parameter is set to 0 or

100.

68


7.11 Tapping mode

7.11 Tapping mode ; G63


The G63 command allows the control mode best suited for tapping to be entered, as indicated below :

(1) Cutting override is fixed at 100%.

(2) Deceleration commands at joints between blocks are invalid.

(3) Feed hold is invalid.

(4) Single block is invalid.

(5) In-tapping mode signal is output.

G63 is released by the exact stop check mode (G61), high-accuracy control mode (G61.1), automatic corner override (G62),or cutting mode (G64) command.

Command format

G63 ;

7.12 Cutting mode ; G64


The G64 command allows the cutting mode in which smooth cutting surfaces are obtained to be established. Unlike the exact stop check mode (G61), the next block is executed continuously with the machine not decelerating and stopping between cutting feed blocks in this mode.

G64 is released by the exact stop check mode (G61), high-accuracy control mode (G61.1), automatic corner override (G62), or tapping mode (G63) command.

This cutting mode is established in the initialized status.

Command format

G64 ;

69

8. Dwell

8.1 Per-second dwell

8. Dwell

The G04 command can delay the start of the next block. The dwell remaining time can be canceled by adding the multi-step skip function.

8.1 Per-second dwell ; G04


The machine movement is temporarily stopped by the program command to make the waiting time state. Therefore, the start of the next block can be delayed. The waiting time state can be canceled by inputting the skip signal.

Command format

G04 X__ ; or G04 P__ ;

X, P : Dwell time

The input command unit for the dwell time depends on the parameter.


(1) When designating the dwell time with X, the decimal point command is valid.

(2) The dwell time command range is as follows.

0.001 ~ 99999.999 (s)

(3) The dwell time setting unit applied when there is no decimal point can be made 1s by setting 1 in the parameter "#1078 Decpt2". This is effect only for X and P for which the decimal command is valid.

(4) When a cutting command is in the previous block, the dwell command starts calculating the dwell time after the machine has decelerated and stopped. When it is commanded in the same block as an M, S, T or B command, the calculation starts simultaneously.

(5) The dwell is valid during the interlock.

(6) The dwell is valid even for the machine lock.

(7) The dwell can be canceled by setting the parameter "#1173 dwlskp" beforehand. If the set skip signal is input during the dwell time, the remaining time is discarded, and the following block will be executed.

Previous block cutting command

Next block

Dwell command

Dwell time

70

8. Dwell


8.1 Per-second dwell

Command

G04 X500 ;

G04 X5000 ;

G04 X5. ;

G04 X#100 ;

G04 P5000 ;

G04 P12.345 ;

G04 P#100 ;

Dwell time [sec]

#1078 Decpt2 = 0

0.5

#1078 Decpt2 = 1

500

5

5

1000

5

12.345

1000

5000

5

1000

5000

12.345

1000

(Note 1)

The above examples are the results under the following conditions.

•

Input setting unit 0.001mm or 0.0001inch

•

#100 = 1000 ;

(Note 2)

If the input setting unit is 0.0001inch, the X before G04 will be multiplied by 10. For example for "X5. G04 ;", the dwell time will be 50 sec.

Precautions

(1) When using this function, command X after G04 in order to make sure that the dwell is based on X.

71

9. Miscellaneous Functions

9.1 Miscellaneous functions (M8-digits BCD)




The miscellaneous (M) functions are also known as auxiliary functions, and they include such numerically controlled machine functions as spindle forward and reverse rotation, operation stop and coolant ON/OFF.

These functions are designated by an 8-digit number (0 to 99999999) following the address M with this controller, and up to 4 groups can be commanded in a single block.

(Example)

G00 Xx Mm1 Mm2 Mm3 Mm4 ;

When five or more commands are issued, only the last four will be valid.

The output signal is an 8-digit BCD code and start signal.

The eight commands of M00, M01, M02, M30, M96, M97, M98 and M99 are used as auxiliary commands for specific objectives and so they cannot be used as general auxiliary commands. This therefore leaves 92 miscellaneous functions which are usable as such commands. Reference should be made to the instructions issued by the machine manufacturer for the actual correspondence between the functions and numerical values.

When the M00, M01, M02, and M30 functions are used, the next block is not read into the pre-read buffer due to pre-read inhibiting.

An M function can be specified together with other commands in the same block, and when such a function is specified together with a movement command in the same block, there are two possible sequences in which the commands are executed. Which of these sequences actually applies depends on the machine specifications.

(1) The M function is executed after the movement command.

(2) The M function is executed at the same time as the movement command.

Processing and completion sequences are required in each case for all M commands except M96, M97, M98 and M99.

The 8 M functions used for specific purposes will now be described.

Program stop : M00

When the NC has read this function, it stops reading the next block. Whether such machine functions as the spindle rotation and coolant supply are stopped or not differs according to the machine in question.

Re-start is enabled by pressing the automatic start button on the machine operation board.

Whether resetting can be initiated by M00 depends on the machine specifications.

Optional stop : M01

If the M01 command is read when the optional stop switch on the machine operation board is ON, reading of the next block will stop and the same effect as with the M00 function will apply.

(Example)

:

N10 G00 X1000 ;

N11 M01 ;

N12 G01 X2000 Z3000 F600 ;

:

Optional stop switch status and operation

Stops at N11 when switch is ON

Next command (N12) is executed without stopping at N11 when switch is OFF

72



Program end : M02 or M30

This command is normally used in the final block for completing the machining, and so it is primarily used for tape rewinding. Whether the tape is actually rewound or not depends on the machine specifications. Depending on the machine specifications, the system is reset by the M02 or M30 command upon completion of tape rewinding and any other commands issued in the same block.

(Although the contents of the command position display counter are not cleared by this reset action, the modal commands and compensation amounts are canceled.)

The next operation stops when the rewinding operation is completed (the in-automatic operation lamp goes off). To restart the unit, the automatic start button must be pressed or similar steps must be taken.

(Note 1)

Independent signals are also output respectively for the M00, M01, M02 and M30 commands and these outputs are each reset by pressing the reset key.

(Note 2)

M02 or M30 can be assigned by manual data input (MDI). At this time, commands can be issued simultaneously with other commands.

Macro interrupt : M96, M97

M96 and M97 are M codes for user macro interrupt control.

The M code for user macro interrupt control is processed internally, and is not output externally.

To use M96 and M97 as a miscellaneous code, change the setting to another M code with the parameter (#1109 subs_M and #1110 M96_M, #1111 M97_M).

Subprogram call/completion : M98, M99

These commands are used as the return instructions from branch destination subprograms and branches to subprograms.

M98 and M99 are processed internally and so M code signals and strobe signals are not output.

Internal processing with M00/M01/M02/M30 commands

Internal processing suspends pre-reading when the M00, M01, M02 or M30 command has been read. Indexing operation other than M02/M03 and the initialization of modals by resetting differ according the machine specifications.

73


9.2 Secondary miscellaneous functions (B8-digits, A8 or C8-digits)

9.2 Secondary miscellaneous functions (B8-digits, A8 or C8-digits)


These serve to assign the indexing table positioning and other such functions. In this controller, they are assigned by an 8-digit number from 0 to 99999999 following address A, B or C. The machine maker determines which codes correspond to which positions.

When the A, B and C functions are commanded in the same block as movement commands, there are 2 sequences in which the commands are executed, as below. The machine specifications determine which sequence applies.

(1) The A, B or C function is executed after the movement command.

(2) The A, B or C function is executed simultaneously with the movement command.

Processing and completion sequences are required for all secondary miscellaneous functions.

The table below given the various address combinations. It is not possible to use an address which is the same for the axis name of an additional axis and secondary miscellaneous function.

Secondary miscellaneous function

A

B

C

Additional axis name

A B C

(Note)

When A has been assigned as the secondary miscellaneous function address, the following commands cannot be used.

(1) Linear angle commands

(2) Geometric commands

74

10. Spindle Functions

10.1 Spindle functions (S2-digits BCD)


10.1 Spindle functions (S2-digits BCD) ..... During standard PLC specifications


The spindle functions are also known simply as S functions and they assign the spindle rotation speed. In this controller, they are assigned with a 2-digit number following the S code ranging from

0 to 99, and 100 commands can be designated. In actual fact, however, it depends on the machine specifications as to how many of these 100 functions are used and which numbers correspond to which functions, and thus reference should be made to the instruction issued by the machine manufacturer. When a number exceeding 2 digits is assigned, the last 2 digits will be valid.

When S functions are commanded in the same block as movement commands, there are 2 sequences in which the commands are executed, as below. The machine specifications determine which sequence applies.

(1) The S function is executed after the movement command.

(2) The S function is executed simultaneously with the movement command.

Processing and completion sequences are required for all S commands from S00 to S99.

10.2 Spindle functions (S6-digits Analog)


When the S6-digits function is added, commands with a 6-dight number following the S code can be designated. Other commands conform to the S2-digits function.

By assigning a 6-digit number following the S code, these functions enable the appropriate gear signals, voltages corresponding tot he commanded spindle speed (r/min) and start signals to be output.

If the gear step is changed manually other than when the S command is being executed, the voltage will be obtained from the set speed at that gear step and the previously commanded speed, and then will be output.

The analog signal specifications are given below.

(1) Output voltage.............. 0 to 10V

(2) Resolution .................... 1/4096 (2

–12

)

(3) Load

Ω

(4) Output

Ω

If the parameters for up to 4 gear stages are set in advance, the gear stage corresponding to the S command will be selected and the gear signal will be output. The analog voltage is calculated in accordance with the input gear signal.

(1) Parameters corresponding to individual gears ....... Limit rotation speed, maximum rotation speed, shift rotation speed and tapping rotation speed

(2) Parameters corresponding to all gears .................. Orientation rotation speed, minimum

rotation speed

75


10.3 Spindle functions (S8-digits)

10.3 Spindle functions (S8-digits)


These functions are assigned with an 8-digit (0 to 99999999) number following the address S, and one group can be assigned in one block.

The output signal is a 32-bit binary data with sign and start signal. Processing and completion sequences are required for all S commands.

76


10.4 Multiple spindle control I


10.4.1 Multiple spindle control


Spindle rotation command for up to 7 spindles is provided.

Although the S

∗∗∗∗∗

command is normally used to designate the spindle rotation speed, the

Sn=

∗∗∗∗∗

command is also used for multiple spindle control.

S commands can be issued from the machining program of any part systems.

Number of usable spindles differ the machine model, confirm the specifications of the model used.

Command format

Sn=

∗∗∗∗∗

;

n

∗∗∗∗∗

S6-digit binary data.

Designate the spindle number with one numeric character.

Rotation speed or constant surface speed command value.


(1) Each spindle command is delimited by the details of n.

(Example)

S1 = 3500 ; 1st spindle 3500(r/min) command

S2 = 1500 : 2nd spindle 1500(r/min) command

S3 = 2000 ; 3rd spindle 2000(r/min) command

S4 = 2500 : 4th spindle 2500(r/min) command

S5 = 2000 ; 5th spindle 2000(r/min) command

S6 = 3000 : 6th spindle 3000(r/min) command

S7 = 3500 ; 7th spindle 3500(r/min) command

(2) Multiple spindles can be commanded in one block.

(3) If two or more commands are issued to the same spindle in a block, the command issued last will be valid.

(Example)

S1 = 3500 S1 = 3600 S1 = 3700 ; S1 = 3700 will be valid.

(4) The

∗∗∗∗∗

command and Sn=

∗∗∗∗∗

command can be used together.

The spindle targeted for the S

∗∗∗∗∗

command is normally the 1st spindle, however, the S

∗∗∗∗∗ command can be used for 2nd or following spindle according to the spindle selection command.

(5) The commands for each spindle can be commanded from the machining program of any part systems.

The spindles will rotate with the speed commanded last.

If the S commands are issued from two or more part systems, the command from the part system of largest No. will be valid.

(6) As for C6 T-type and L-type, C64 T-type, and C64T T-type, the multiple spindles control can not be used in a part system. A program error (P33) will occur when the Sn=

∗∗∗∗∗

command is issued. Refer to "10.4.2 Spindle selection command" for details.

77



10.4.2 Spindle selection command


This function controls which spindle’s rotation the cutting follows, in addition, designates the spindle to be selected when "S

∗∗∗∗∗∗

" command is issued.

Command format

G43.1;

G44.1;

Selected spindle (nth spindle) control mode ON

(Selected with parameter)

2nd spindle control mode ON


(1) G43.1 and G44.1 are modal G codes.

(2) The spindle control mode entered when the power is turned ON or reset depends on the parameter setting.

Designate the spindle No. to be selected in G43.1 modal with the parameter (basic specifications parameter "#1199 Sselect").

This parameter is provided for every part system to set as follows.

# Items

1199 Sselect Select initial spindle control

Details

Select the initial condition of spindle control when power is turned ON or reset.

Setting range (unit)

0: Selected spindle control mode (G43.1)

1: 2nd spindle control mode

(G44.1)

21049 SPname Designate the spindle No. selected for the G43.1 modal in each part system.

0: 1st spindle 4: 4th spindle

1: 1st spindle 5: 5th spindle

2: 2nd spindle 6: 6th spindle

3: 3rd spindle 7: 7th spindle

Reset the NC after changing "#1199 Sselect " and "#21049 SPname" parameters. It is no use to turn the power OFF once and ON again.

(3) As for C6 L-type, T-type, C64 T-type and C64T T-type, there are following restrictions;

· A program error (P34) will occur if G44.1 command is issued.

· No data can be set to "#1199 Sselect". "0" is set when the NC power is turned ON.

· Only one spindle than is selected with "#21049 SPname" can be commanded as "S

∗∗∗∗∗

" in each part system.

· A program error (P33) will occur if the "S0=

∗∗∗∗∗

" command is issued.

(4) If the S command is issued in the same as the spindle selection commands (G43.1, and

G44.1), which spindle the S command is valid for depends on the order that G43.1, G44.1, and S command are issued.

When S command precedes the G codes, it follows the G43.1 / G44.1 mode before S command is issued.

When G codes precede, it follows the G43.1 / G44.1 mode issued in the same block.

(5) G43.1 and G44.1 commands can be issued from every part system.

78


Relation with other functions


(1) The following functions change after the spindle selection command.

(a) Per rotation command (synchronous feed)

Even if F is commanded in the G95 mode, the per rotation feedrate for the selected spindle

(nth spindle) will be applied during G43.1 mode and for the 2nd spindle during G44.1 mode.

(b) S commands (S

∗∗∗∗∗

, Sn=

∗∗∗∗∗

), constant surface speed control, thread cutting

Function

S command during G97/G96 constant surface speed control

Upper limit / Lower limit of spindle rotation speed command during constant surface speed control (G92

S_ Q)

Thread cutting

G43.1 mode

Command control for the selected spindle

(nth spindle).

(Note 1)

G44.1 mode

Command control for the 2nd spindle.

(Note 1)

The spindle selected during G43.1 mode depends on the parameter "#21049

(2) The

SPname".

Sn=

∗∗∗∗∗

command can be used to command the other spindle even if it is commanded during G43.1 or G44.1 mode.

Note that the rotation speed designation will be applied for such command even if the G96 mode is ON.

(Example)

When "SPname" = 0;

G43.1;

G97 S1000;

:

S2 = 2000;

:

G96 S100;

:

S2 = 2500;

:

G44.1 S200;

:

S1 = 3000;

:

G97 S4000;

:

1st spindle

1000(r/min)

100(m/min)

(Note 2)

3000(r/min)

2nd spindle

0(r/min)

2000(r/min)

2500(r/min)

200(m/min)

4000(r/min)

(Note 2)

The constant surface speed control will be switched to the 2nd spindle by G44.1 command. Therefore, the 1st spindle retains its rotation speed as that of "G44.1

S200;" command.

The 1st spindle rotation speed will be 3000 (r/min) when "S1=3000;" command is issued.

79


10.5 Constant surface speed control

10.5 Constant surface speed control; G96, G97

10.5.1 Constant surface speed control


These commands automatically control the spindle speed in line with the changes in the radius coordinate values as cutting proceeds in the diametrical direction, and they serve to keep the cutting point speed constant during the cutting.

Command format

G96 Ss Pp; Constant surface speed ON

Ss

Pp

: Surface speed (1 to 99999999 m/min)

: Assignment of constant surface speed control axis

G97 ; Constant surface speed cancel


(1) The constant surface speed control axis is set by parameter "#1181 G96_ax".

0 : Fixed at 1st axis (P command invalid)

1 : 1st axis

2 : 2nd axis

3 : 3rd axis

(2) When the above-mentioned parameter is not zero, the constant surface speed control axis can be assigned by address P.

(Example)

With G96_ax (1)

Program

G96 S100 ;

G96 S100 P3 ;

Constant surface speed control axis

1st axis

3rd axis

(3) Example of selection program and operation

G90 G96 G01 X50. Z100. S200 ;

G97 G01 X50. Z100. F300 S500 ;

The spindle speed is controlled so that the peripheral speed is 200m/min.

The spindle speed is controlled to 500r/min.

M02 ;

The modal returns to the initial setting.

(4) Constant surface speed control can be commanded on the selected spindle (nth spindle) / the

2nd spindle.

Select which spindle (the selected spindle or 2nd one) the commands are made to by the spindle selection G codes (G43.1 and G44.1).

Select which spindle (the selected spindle or 2nd one) is valid as the initial state with the parameter (base specifications parameter "#1199 Sselect").

(5) Select whether calculating the surface speed at rapid traverse command is performed constantly or only at the block end poing.

80


10.6 Spindle clamp speed setting

10.6 Spindle clamp speed setting; G92


The maximum clamp speed of the spindle can be assigned by address S following G92 and the minimum clamp speed by address Q.

Command format

G92 Ss Qq;

Ss

Qq

: Maximum clamp speed

: Minimum clamp speed


(1) Besides this command, parameters can be used to set the rotational speed range up to 4 stages in 1 r/min units to accommodate gear selection between the spindle and spindle motor.

The lowest upper limit and highest lower limit are valid among the rotational speed ranges based on the parameters and based on G92 Ss Qq ;

(2) Set in the parameters "#1146 Sclamp" and "#1227 aux11/bit5" whether to carry out rotation speed clamp only in the constant surface speed mode or even when the constant surface speed is canceled.

(Note)

G92S command and speed clamp operation

Sclamp = 0 aux11/bit5 = 0 aux11/bit5 = 1

Command

Operation

In G96

In G97

In G96

In G97

Rotation speed clamp command

Spindle rotation speed command

Rotation speed clamp execution

No rotation speed clamp

Sclamp = 1 aux11/bit5 = 0 aux11/bit5 = 1








No rotation speed clamp

81


10.7 Spindle synchronous control I

10.7 Spindle synchronous control I; G114.1


In a machine having two or more spindles, this function controls the rotation speed and phase of one spindle (basic spindle) in synchronization with the rotation of the other spindle (synchronous spindle).

The function is used "when the rotation speed of the two spindles must be matched, for example, if a workpiece grasped by the 1st spindle is to be grasped by a 2nd spindle", or "if the spindle rotation speed has to be changed when one workpiece is grasped by both the 1st and 2nd spindles".

With the spindle synchronous control function I, designation of spindles and controls start / stop of synchronization are commanded using G codes in the machining program.

Command format

(1) Spindle synchronous control ON (G114.1)

This command designates the basic spindle and synchronous spindle, and synchronizes the two designated spindles. By commanding the synchronous spindle phase shift amount, the phases of the basic spindle and synchronous spindle can be aligned.

G114.1 H_ D_ R_ A_ ;

H_ Basic spindle selection

D_

R_

A_

Synchronous spindle selection

Spindle synchronization phase shift amount

Spindle synchronization acceleration/deceleration time constant

(2) Spindle synchronous control cancel (G113)

This command cancels the synchronous state of the two spindles rotating in synchronization with the spindle synchronous command.

G113 ;

Add- ress

Meaning of address

selection

Select the No. of the spindle to be used as the basic spindle from the two spindles.

Command range (unit)

1 to 7

1: 1st spindle

2: 2nd spindle

:

7: 7th spindle

•

Remarks

A program error (P35) will occur if a value exceeding the command range or spindle No. without specifications is commanded.

•

A program error (P33) will occur if there is no command.

•

A program error (P610) will occur if a spindle not serially connected is commanded.

82



Add- ress

D Synchronous


spindle selection

Select the No. of the spindle to be synchronized with the basic spindle from the two spindles. phase shift amount

Command the shift amount from the

Z-phase point (one rotation signal) of the synchronous spindle.

A Spindle synchronization acceleration/deceleration time constant

Command the acceleration/deceleration time constant for when the spindle synchronous command rotation speed changes.

(Command this to accelerate or decelerate at a speed slower than the time constant set in the parameters.)

Command range

(unit)

1 to 7 or –1 to –7

1: 1st spindle

2: 2nd spindle

:

7: 7th spindle or

0 to 35999

(° × 10

–3

)

0.001 to 9.999 (s) or

1 to 9999 (ms)

Remarks

•

A program error (P35) will occur if a value exceeding the command range or spindle No. without specifications is commanded.

•

A program error (P33) will occur if there is no command.

•

A program error (P33) will occur if the same spindle as that commanded for the basic spindle selection is designated.

•

The rotation direction of the synchronous spindle in respect to the basic spindle is commanded with the

D sign.

•

A program error (P610) will occur if a spindle not serially connected is commanded.

•

A program error (P35) will occur if a value exceeding the command range is commanded.

•

The commanded shift amount is effective in the clockwise direction of the basic spindle.

•

The commanded shift amount's minimum resolution is as follows:

For semi-closed

(Only gear ratio 1:1)

360/4096 (° )

For full closed

(360/4096)

∗

K (° )

K: Spindle and encoder gear ratio

•

If there is no R command, the phases will not be aligned.

•

A program error (P35) will occur if a value exceeding the command range is commanded.

•

If the commanded value is smaller than the acceleration/deceleration time constant set with the parameters, the value set in the parameters will be applied.

83



Rotation and rotation direction

(1) The rotation speed and rotation direction of the basic spindle and synchronous spindle during spindle synchronous control are the rotation speed and rotation direction commanded for the basic spindle. Note that the rotation direction of the synchronous spindle can be reversed from the basic spindle through the program.

(2) The basic spindle's rotation speed and rotation direction can be changed during spindle synchronous control.

(3) The synchronous spindle's rotation command is also valid during spindle synchronous control.

When spindle synchronous control is commanded, if neither a forward run command nor reverse run command is commanded for the synchronous spindle, the synchronization standby state will be entered without starting the synchronous spindle's rotation. If the forward run command or reverse run command is input in this state, the synchronous spindle will start rotation. The synchronous spindle's rotation direction will follow the direction commanded in the program.

If spindle stop is commanded for the synchronous spindle during spindle synchronization control (when both the forward run and reverse run commands are turned OFF), the synchronous spindle rotation will stop.

(4) The rotation speed command (S command) and constant surface speed control are invalid for the synchronous spindle during spindle synchronous control. Note that the modal is updated, so these will be validated when the spindle synchronization is canceled.

(5) The constant surface speed can be controlled by issuing a command to the basic spindle even during spindle synchronous control.

84


Rotation synchronization


(1) When rotation synchronization control (command with no R address) is commanded with the

G114.1 command, the synchronous spindle rotating at a random rotation speed will accelerate or decelerate to the rotation speed commanded beforehand for the basic spindle, and will enter the rotation synchronization state.

(2) If the basic spindle's commanded rotation speed is changed during the rotation synchronization state, acceleration/deceleration will be carried out while maintaining the synchronization state following the spindle acceleration/deceleration time constants set in the parameters, and the commanded rotation speed will be achieved.

(3) In the rotation synchronization state, the basic spindle can be controlled to the constant surface speed even when two spindles are grasping one workpiece.

(4) Operation will take place in the following manner.

M23 S2=750 ;

:

M03 S1=1000 ;

:

G114.1 H1 D-2 ;

:

S1=500 ;

:

G113 ;

... Forward rotate 2nd spindle (synchronous spindle) at 750 r/min (speed command)

... Forward rotate 1st spindle (basic spindle) at 1000 r/min

(speed command)

... Synchronize 2nd spindle (synchronous spindle) to 1st spindle (basic spindle) with reverse run

... Change 1st spindle (basic spindle) rotation speed to 500 r/min

... Cancel spindle synchronization

<Operation>

1000

750

500

Forward run

Rotation speed

0

(r/min)

Reverse run

–500

–750

–1000

2nd spindle (synchronous spindle) reverse run synchronization

1st spindle (basic spindle) forward run

2nd spindle (synchronous spindle) forward run

Basic spindle

Synchronous spindle

Spindle synchronization cancel

1st spindle (basic spindle) rotation speed change

85


Phase synchronization


(1) When phase synchronization (command with R address) is commanded with the G114.1 command, the synchronous spindle rotating at a random rotation speed will accelerate or decelerate to the rotation speed commanded beforehand for the basic spindle, and will enter the rotation synchronization state.

Then, the phase is aligned so that the rotation phase commanded with the R address is reached, and the phase synchronization state is entered.

(2) If the basic spindle's commanded rotation speed is changed during the phase synchronization state, acceleration/deceleration will be carried out while maintaining the synchronization state following the spindle acceleration/deceleration time constants set in the parameters, and the commanded rotation speed will be achieved.

(3) In the phase synchronization state, the basic spindle can be controlled to the constant surface speed even when two spindles are grasping one workpiece.

(4) Operation will take place in the following manner.

M23 S2=750 ;

:

M03 S1=1000 ;

:

G114.1 H1 D-2 Rxx ;

:

:

S1=500 ;

:

G113 ;

... Forward rotate 2nd spindle (synchronous spindle) at 750 r/min (speed command)

... Forward rotate 1st spindle (basic spindle) at 1000 r/min

(speed command)

... Synchronize 2nd spindle (synchronous spindle) to 1st spindle (basic spindle) with reverse run

Shift phase of synchronous spindle by R command value

... Change 1st spindle (basic spindle) rotation speed to 500 r/min

... Cancel spindle synchronization

<Operation>

Basic spindle

Synchronous spindle

1000

750

500

Forward run

Rotation speed

0

(r/min)

Reverse run

–500

–750

–1000

2nd spindle (synchronous spindle) reverse run synchronization

1st spindle (basic spindle) forward run

2nd spindle (synchronous spindle) forward run

Phase alignment

Spindle synchronization cancel

1st spindle (basic spindle) rotation speed change

86


Cautions on programming


(1) To enter the rotation synchronization mode while the basic spindle and synchronous spindle are chucking the same workpiece, turn the basic spindle and synchronous spindle rotation commands ON before turning the spindle synchronous control mode ON.

$1 (1st part system)

:

M6 ; 1st spindle chuck close :

$2 (2nd part system)

:

:

:

!2 ;

M5 S1=0 ;

:

M3 ;

!2 ;

M25 S2=0 ; 2nd spindle stops at S=0

:

!1 ; Waiting between part systems

2nd spindle chuck close 1st spindle stops at S=0 M15 ;

1st spindle rotation command ON

M24 ; 2nd spindle rotation command ON

:

!1 ; Waiting between part systems

:

:

S1=1500 ; Synchronous rotation at

S=1500

:

S1=0 ;

G113 ;

Both spindles stop

D-2 ;

:

:

:

Synchronization mode OFF

(2) To chuck the same workpiece with the basic spindle and synchronous spindle in the phase synchronization mode, align the phases before chucking.

$1 $2

:

M6 ; 1st spindle chuck close

:

:

: :

M3

S1=1500 ;

:

1st spindle rotation command ON

:

G114.1 H1 D-2 R0 ; Phase synchronization

:

:

:

:

:

:

M24 ; 2nd spindle rotation command ON

:

M15 ; 2nd spindle chuck close

(Note 1)

:

(Note 1)

Close the chuck after confirming that the spindle phase synchronization complete signal (X42A) has turned ON (phase alignment complete).

87



CAUTION

Do not make the synchronous spindle rotation command OFF with one workpiece chucked by the basic spindle and synchronous spindle during the spindle synchronous control mode.

Failure to observe this may cause the synchronous spindle stop, and hazardous situation.

Precautions and restrictions

(1) To carry out the spindle synchronization, it is required to command spindle rotation for both basic spindle and synchronous spindle. Note that the rotating direction of the synchronous spindle follows the rotating direction of the basic spindle and rotating direction designation by

"D" address.

(2) The spindle rotating with spindle synchronous control will stop when emergency stop is applied.

(3) The rotation speed clamp during spindle synchronization control will follow the smaller clamp value set for the basic spindle or synchronous spindle.

(4) Orientation of the basic spindle and synchronous spindle is not possible during the spindle synchronous control mode. To carry out orientation, cancel the spindle synchronous control mode first.

(5) The rotation speed command (S command) is invalid for the synchronous spindle during the spindle synchronous control mode. Note that the modal will be updated, so this will be validated when spindle synchronous control is canceled.

(6) The constant surface speed control is invalid for the synchronous spindle during the spindle synchronization control mode. Note that the modal will be updated, so this will be validated when spindle synchronization is canceled.

(7) The rotation speed command (S command) and constant surface speed control for the synchronous spindle will be validated when spindle synchronous control is canceled. Thus, the synchronous spindle may carry out different operations when this control is canceled.

(8) An attention should be made that if the phase synchronization command is executed with the phase error not obtained by the phase shift calculation request signal, the phase shift amount will not be obtained correctly.

(9) The spindle rotation speed command (S command) and the constant surface speed control for the synchronous spindle will become valid when the spindle synchronous control is canceled.

Thus, special attention should be made because the synchronous spindle may do different action than before when the spindle synchronous control is canceld.

(10) If the phase synchronization command (command with R address) is issued while the phase shift calculation request signal is ON, an operation error (1106) will occur.

(11) If the phase shift calculation request signal is ON and the basic spindle or synchronous spindle is rotation while rotation synchronization is commanded, an operation error (1106) will occur.

(12) If the phase synchronization command R0 (<Ex.> G114.2 H1 D-2 R0) is commanded while the phase offset request signal is ON, the basic spindle and synchronous spindle phases will be aligned to the phase error of the basic spindle and synchronous spindle saved in the NC memory.

(13) If a value other than the phase synchronization command R0 (<Ex.> G114.1 H1 D-2 R000) is commanded while the phase offset request signal is ON, the phase error obtained by adding the value commanded with the R address command to the phase difference of the basic spindle and synchronous spindle saved in the NC memory will be used to align the basic spindle and synchronous spindle.

88



(14) The phase offset request signal will be ignored when the phase shift calculation request signal is ON.

(15) The phase error of the basic spindle and synchronous spindle saved in the NC is valid only when the phase shift calculation signal is ON and for the combination of the basic spindle selection (H_) and synchronous spindle (D_) commanded with the rotation synchronization command (no R address).

For example, if the basic spindle and synchronous spindle phase error is saved as "G114.1

H1 D-2 ;", the saved phase error will be valid only when the phase offset request signal is ON and "G114.1 H1 D_2 R

∗∗∗

;" is commanded. If "G114.1 H2 D-1 R

∗∗∗

;" is commanded in this case, the phase shift amount will not be calculated correctly.

(16) The phase error of the basic spindle and synchronous spindle saved in the NC is retained until the spindle synchronization phase shift calculation, in other words, until the rotation synchronous control command completes with the phase shift calculation request signal is

ON.

(17) Synchronous tapping can not be used during spindle synchronous mode.

(18) When the spindle synchronous control commands are being issued with the PLC I/F method

(#1300 ext36/bit7 OFF), a program error (P610) will occur if the spindle synchronous control is commanded with G114.1/G113.

89


10.8 Spindle synchronization control II



In a machine having two or more spindles, this function controls the rotation speed and phase of one spindle (synchronous spindle) in synchronization with the rotation of the other spindle (basic spindle).

The function is used if a workpiece grasped by the basic spindle is to be grasped by a synchronous spindle, or if the spindle rotation speed has to be changed when one workpiece is grasped by both spindles.

With the spindle synchronous control II, selection of the spindles and synchronization start, etc., are all designated from the PLC.

Basic spindle and synchronous spindle selection

Select the basic spindle and synchronous spindle for synchronous control from the PLC.

Device No. Signal name Abbrev.

selection spindle selection

Explanation

Select a serially connected spindle to be controlled as the basic spindle.

(0: 1st spindle), 1: 1st spindle, 2: 2nd spindle,

… , 7: 7th spindle

(Note 1)

Spindle synchronization control will not take place if a spindle not connected in serial is selected.

(Note 2)

If "0" is designated, the 1st spindle will be controlled as the basic spindle.

Select a serially connected spindle to be controlled as the synchronous spindle.

(0: 2nd spindle), 1: 1st spindle, 2: 2nd spindle,

… , 7: 7th spindle

(Note 3)

Spindle synchronous control will not take place if a spindle not connected in serial is selected or if the same spindle as the basic spindle is selected.

(Note 4)

If "0" is designated, the 2nd spindle will be controlled as the synchronous spindle.

90


Starting spindle synchronization


The spindle synchronous control mode is entered by inputting the spindle synchronous control signal (SPSYC). The synchronous spindle will be controlled in synchronization with the rotation speed commanded for the basic spindle during the spindle synchronous control mode.

When the difference of the basic spindle and synchronous spindle rotation speeds reaches the spindle synchronization rotation speed reach level setting value (#3050 sprlv), the spindle rotation speed synchronization complete signal (FSPRV) will be output.

The synchronous spindle's rotation direction is designated with the spindle synchronization rotation direction designation as the same as the basic spindle or the reverse direction.


Y432 Spindle synchronous control

Explanation

SPSYC The spindle synchronous control mode is entered when this signal turns ON. spindle This notifies that the mode is the spindle synchronous control synchronous control. rotation This turns ON when the difference of the basic speed synchronization complete spindle and synchronous spindle rotation speeds reaches the spindle rotation speed reach level setting value during the spindle synchronous control mode.

This signal turns OFF when the spindle synchronous control mode is canceled, or when an error exceeding the spindle rotation speed reach level setting value occurs during the spindle synchronous control mode.

Y434 Spindle synchronization rotation direction designation

SPSDR Designate the basic spindle and synchronous spindle rotation directions for spindle synchronous control.

0: The synchronous spindle rotates in the same direction as the basic spindle.

1: The synchronous spindle rotates in the reverse direction of the basic spindle.

91


Spindle phase alignment


Spindle phase synchronization starts when the spindle phase synchronous control signal (SPPHS) is input during the spindle synchronization control mode. The spindle phase synchronization complete signal is output when the spindle synchronization phase reach level setting value (#3051 spplv) is reached.

The synchronous spindle's phase shift amount can also be designated from the PLC.


Explanation

phase Spindle phase synchronization starts when this synchronous control signal is turned ON during the spindle synchronous control mode.

(Note 1)

If this signal is turned ON in a mode other than the spindle synchronous control mode, it will be ignored. phase This signal is output when the spindle synchronization complete synchronization phase reach level is reached after starting spindle phase synchronization. amount setting

Designate the synchronous spindle's phase shift amount.

Unit: 360°/4096

Spindle synchronous control

(Y432)

In spindle synchronous control (X42A)

Spindle synchronization complete (X42B)

Spindle phase synchronous control (Y433)

Spindle phase synchronization complete (X42C)

(Note 2)

Spindle phase synchronization complete ON

Spindle phase synchronous control ON

Spindle synchronization complete ON

Spindle phase synchronous control OFF

Spindle synchronization control ON


(Note 2)

Turns OFF temporarily to change the rotation speed during phase synchronization.

92



Calculating the spindle synchronization phase shift amount and requesting phase offset

The spindle phase shift amount calculation function obtains and saves the phase difference of the basic spindle and synchronous spindle by turning the PLC signal ON during spindle synchronization. When calculating the spindle phase shift, the synchronous spindle can be rotated with the handle, so the relation of the phases between the spindles can also be adjusted visually.

If the spindle phase synchronization control signal is input while the phase offset request signal

(SSPHF) is ON, the phases will be aligned using the position shifted by the saved phase shift amount as a reference.

This makes aligning of the phases easier when grasping the material that the shape of one end differ from another end.


Explanation

shift If spindle synchronization is carried out while calculation request this signal is ON, the phase difference of the basic spindle and synchronous spindle will be obtained and saved. offset If spindle phase synchronization is carried out request while this signal is ON, the phases will be aligned using the position shifted by the saved phase shift amount as a basic position.

R55 Phase difference output

– data

The delay of the synchronous spindle in respect to the basic spindle is output.

Unit: 360°/4096

(Note 1)

If either the basic spindle or synchronous spindle has not passed through the Z phase, etc., and the phase cannot be calculated, –1 will be output.

(Note 2)

This data is output only while calculating the phase shift or during spindle phase synchronization.

The phase difference saved with phase shift calculation is output.

Unit: 360°/4096

(Note 3)

This data is output only during spindle synchronous control.

Phase shift calculation request (Y435)

Spindle synchronous control (Y436)



The phase difference in this interval is saved.

(The synchronous spindle can be controlled with the handle.)

Spindle synchronous control ON


Phase shift calculation request ON

Phase shift calculation request OFF

(Note 4)

The phases cannot be aligned while calculating the phase shift.

(Note 5)

The synchronous spindle cannot be rotated with the handle when the manual operation mode is set to the handle mode.

93


Chuck close signal


The synchronous spindle side carries out droop compensation while the chuck is opened, and aligns itself with the basic spindle. However, when the chuck is closed, the droop compensation is added, and the synchronization error with the base increases. Droop compensation is prevented with the chuck close signal and the position where the chuck is grasped is maintained with position compensation.


Y431 Chuck close

Explanation

SPCMPC This turns ON when the chuck of both spindles are closed. This signal is ON while the basic spindle and the synchronous spindle grasp the same workpiece. close This turns ON when the chuck close signal is confirmation received during the spindle synchronous control mode.

Chuck close

Chuck close confirmation

Chuck close

Chuck open confirmation

Chuck open

Chuck close

Basic spindle chuck

Synchronous spindle chuck

Chuck close

Chuck open

Spindle synchronous control (Y432)



Chuck close (Y431)

Error temporary cancel

(Y437)

Error canceled

(Note 1)

Use the error temporary cancel only when there is still an error between the spindle and synchronization with the chuck close signal.

Error temporary cancel function

When spindle synchronization is carried out while grasping the workpiece with the basic spindle and rotating, if the chuck is closed to grasp the workpiece with the synchronous spindle, the speed will fluctuate due to external factors and an error will occur. If spindle synchronization is continued without compensating this error, the workpiece will twist.

This torsion can be prevented by temporarily canceling this error.


Explanation

temporary The error is canceled when this signal is ON.

cancel

(Note 1)

Even if the chuck close signal (Y431) is OFF, the error will be canceled while this signal

(Y437) is ON.

(Note 2)

Turn this signal ON after the both chucks of basic spindle side and synchronous spindle side are closed to grasp the workpiece.

Turn this signal OFF if even one chuck is opened.

94


Phase error monitor


The phase error can be monitored during spindle phase synchronization.


monitor monitor (lower limit value) monitor (upper limit value)

Explanation

The phase error during spindle phase synchronous control is output as a pulse unit.

The lower limit value of the phase error during spindle phase synchronous control is output as a pulse unit.

The upper limit value of the phase error during spindle phase synchronous control is output as a pulse unit.

Multi-speed acceleration/deceleration

Up to eight steps of acceleration/deceleration time constants for spindle synchronization can be selected according to the spindle rotation speed.

Rotation speed

Sptc3

Sptc2

(1) Time required from stopped state to sptc1 setting rotation speed

spt

(2) Time required from sptc1 to sptc2 setting rotation speed

spt

∗

spdiv1

(3) Time required from sptc2 to sptc3 setting rotation speed

spt

∗

spdiv2

Sptc1

Time

(1) (2)

(3)

95


Precautions and restrictions


(1) When carrying out spindle synchronization, a rotation command must be issued to both the basic spindle and synchronous spindle. The synchronous spindle's rotation direction will follow the basic spindle rotation direction and spindle synchronization rotation direction designation regardless of whether a forward or reverse run command is issued.

(2) The spindle synchronization control mode will be entered even if the spindle synchronization control signal is turned ON while the spindle rotation speed command is ON. However, synchronous control will not actually take place. Synchronous control will start after the rotation speed is commanded to the basic spindle, and then the spindle synchronization complete signal will be output.

(3) The spindle rotating with spindle synchronization control will stop when emergency stop is applied.

(4) An operation error will occur if the spindle synchronization control signal is turned ON while the basic spindle and synchronous spindle designations are illegal.

(5) The rotation speed clamp during spindle synchronization control will follow the smaller clamp value set for the basic spindle or synchronous spindle.

(6) Orientation of the basic spindle and synchronous spindle is not possible during the spindle synchronization. To carry out orientation, turn the spindle synchronization control signal OFF first.

(7) The rotation speed command is invalid for the synchronous spindle during the spindle synchronization. Note that the modal is rewritten, thus, the commanded rotation speed will be validated after spindle synchronization is canceled.

(8) The constant surface speed control is invalid for the synchronous spindle during the spindle synchronization. However, note that the modal is rewritten and it will be valid after spindle synchronization is canceled.

(9) If the phase offset request signal is turned ON before the phase shift is calculated and then spindle phase synchronization is executed, the shift amount will not be calculated and incorrect operation results.

(10) The spindle rotation speed command (S command) and the constant surface speed control for the synchronous spindle will become valid when the spindle synchronous control is canceled.

Thus, special attention should be made because the synchronous spindle may do different action than before when the spindle synchronous control is canceled.

(11) The spindle Z-phase encoder position parameter (sppst) is invalid (ignored) when phase offset is carried out.

This parameter will be valid when the phase offset request signal is OFF.

(12) If spindle phase synchronization is started while the phase shift calculation request signal is

ON, the error "M01 OPERATION ERROR 1106" will occur.

(13) Turn the phase shift calculation request signal ON when the basic spindle and synchronous spindle are both stopped. If the phase shift calculation request signal is ON while either of the spindles is rotating, the error "M01 OPERATION ERROR 1106" will occur.

(14) The phase offset request signal is ignored when the phase shift calculation request signal

(Y435) is ON.

(15) "M01 OPERATION ERROR 1106" will occur when a spindle No. out of specifications is designated in the R registers to set the basic spindle and the synchronous spindle, or when the spindle synchronous control signal (Y432) is turned ON with R resister value illegal.

(16) The phase shift amount saved in the NC is held until the next phase shift is calculated. (This value is saved even when the power is turned OFF.)

(17) Synchronous tapping can not be used during spindle synchronous mode.

96

11. Tool Functions

11.1 Tool functions (T8-digit BCD)

11. Tool Functions

11.1 Tool functions (T8-digit BCD)


The tool functions are also known simply as T functions and they assign the tool numbers and tool offset number. They are designated with a 8-digit number following the address T, and one set can be commanded in commanded one block. The output signal is an 8-digit BCD signal and start signal.

When the T functions are commanded in the same block as movement commands, there are 2 sequences in which the commands are executed, as below. The machine specifications determine which sequence applies.

(1) The T function is executed after the movement command.

(2) The T function is executed simultaneously with the movement command.

Processing and completion sequences are required for all T commands.

97

12. Tool Offset Functions

12.1 Tool offset




The basic tool offset function includes the tool length offset and tool diameter compensation. Each offset amount is designated with the tool offset No. Each offset amount is input from the setting and display unit or the program.

Reference point

Tool length

Tool length offset

(Side view)

Tool diameter compensation

Right compensation

(Plane view)

Left compensation

98


Tool offset memory


There are two types of tool offset memories for setting and selecting the tool offset amount. (The type used is determined by the machine maker specifications.)

The offset amount or offset amount settings are preset with the setting and display unit.

Type 1 is selected when parameter "#1037 cmdtyp" is set to "1", and type 2 is selected when set to

"2".

Type of tool offset memory

Type 1

Type 2

Classification of length offset, diameter compensation

Not applied

Applied

Classification of shape offset, wear compensation

Not applied

Applied

Reference

Reference tool

Shape

Tool length offset

Wear amount

Shape

Tool diameter compensation

Wear amount

99



Type 1

One offset amount corresponds to one offset No. as shown on the right. Thus, these can be used commonly regardless of the tool length offset amount, tool diameter offset amount, shape offset amount and wear offset amount.

(D1) = a

1

, (H1) = a

1

(D2) = a

2

, (H2) = a

2

: :

(Dn) = a n

, (Hn) = a n

Offset No.

Offset amount

1 a

1

2 a

2

3 a

3

• •

• • n a n

Type 2

The shape offset amount related to the tool length, wear offset amount, shape offset related to the tool diameter and the wear offset amount can be set independently for one offset No. as shown below.

The tool length offset amount is set with H, and the tool diameter offset amount with D.

(H1) = b1 + c1, (D1) = d1 + e1

(H2) = b2 + c2, (D2) = d2 + e2

: :

(Hn) = bn + cn, (Dn) = dn + en

Offset

No.

Tool length (H)

Shape offset amount

Wear offset amount

Tool diameter(D)/

(Position offset)

Shape offset amount

Wear offset amount

1 b1 c1 d1 e1

2 b2 c2 d2 e2

3 b3 c3 d3 e3

• • • • •

• • • • • n bn cn dn en

CAUTION

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

100


Tool offset No. (H/D)


This address designates the tool offset No.

(1) H is used for the tool length offset, and D is used for the tool position offset and tool diameter offset.

(2) The tool offset No. that is designated once does not change until a new H or D is designated.

(3) The offset No. can be commanded once in each block. (If two or more Nos. are commanded, the latter one will be valid.)

(4) The No. of offset sets that can be used will differ according to the machine.

For 40 sets: Designate with the H01 to H40 (D01 to D40) numbers.

(5) If a value larger than this is set, the program error "P170" will occur.

(6) The setting value ranges are as follows for each No.

The offset amount for each offset No. is preset with the setting and display unit.

Input setting unit

Shape offset amount Wear offset amount

Metric system Inch system Metric system Inch system

#1015 cunit=100 ±99999.99mm

±9999.999 inch ±9999.99 mm ±999.999 inch

#1015 cunit=10 ±9999.999mm

±999.9999 inch ±999.999 mm ±99.9999 inch

101


12.2 Tool length offset/cancel

12.2 Tool length offset/cancel; G43, G44/G49


The end position of the movement command can be offset by the preset amount when this command is used. A continuity can be applied to the program by setting the actual deviation from the tool length value decided during programming as the offset amount using this function.

Command format

When tool length offset is +

G43 Zz Hh ; Tool length offset + start

:

G49 Zz ; Tool length offset cancel

When tool length offset is

−

G44 Zz Hh ; Tool length offset

−

start

:

G49 Zz ;


(1) Tool length offset movement amount

The movement amount is calculated with the following expressions when the G43 or G44 tool length offset command or G49 tool length offset cancel command is issued.

Z axis movement amount

G43 Zz Hn

1

G44 Zz Hh

1

G49 Zz

; z + ( l h

1

) Offset in + direction by tool offset amount

; z

−

( l h

; z

−

(+) ( l h

1

1

) Offset

) Offset amount cancel. l h

1

: Offset amount for offset No. h

1

Regardless of the absolute value command or incremental value command, the actual end point will be the point offset by the offset amount designated for the programmed movement command end point coordinate value.

The G49 (tool length offset cancel) mode is entered when the power is turned ON or when

M02 has been executed.

(Example 1)

For absolute value command

R

N1 G28 Z0 T01 M06 ;

N2 G90 G92 Z0 ;

N3 G43 Z5000 H01 ;

N4 G01 Z-50000 F500 ;

(Example 2)

For incremental value command

H01

N1 G28 Z0 T01 M06 ;

N2 G91 G92 Z0 ;

N3 G43 Z5000 H01 ;

N4 G01 Z-55000 F500 ;

Tool length offset

H01=-100.

+5.00

0

W

-50.000

102



(a) The offset amount differs according to the compensation type.

Type 1

G43 Hh

1

;

When the above is commanded, the offset amount

l

h

1

commanded with offset No. h

1

will be applied commonly regardless of the tool length offset amount, tool diameter offset amount, shape offset amount or wear offset amount.

R

l

h

1

Workpiece

Table

Type 2

G43 Hh

1

;

When the above is commanded, the offset amount

l

h

1

commanded with offset No. h

1

will be as follows.

l

h

1

: Shape offset (Note) + wear offset amount amount

R

l

h

1

Shape offset

Workpiece

Table

(b) The valid range of the offset No. will differ according to the specifications (No. of offset sets).

(c) If the commanded offset No. exceeds the specification range, the program error "P170" will occur.

(d) Tool length cancel will be applied when H0 is designated.

(e) The offset No. commanded in the same block as G43 or G44 will be valid for the following modals.

(Example 3)

G43 Zz1 Hh1 ; ........... Tool length offset is executed with h1.

:

G45 Xx1 Yy1 Hh6 ;

:

G49 Zz2 ; ................... The tool length offset is canceled.

:

G43 Zz2 ; ................... Tool length offset is executed again with h1.

(f) If G43 is commanded in the G43 modal, an offset of the difference between the offset No. data will be executed.

(Example 4)

G43 Zz1 Hh1 ; ........... Becomes the z1 + ( l h1) movement.

:

G43 Zz2 Hh2 ; ........... Becomes the z2 + ( l h2 - lh1) movement.

:

The same applies for the G44 command in the G44 modal.

103



(3) Axis valid for tool length offset

(a) When parameter "#1080 Dril_Z" is set to "1", the tool length offset is always applied on the

Z axis.

(b) When parameter "#1080 Dril_Z" is set to "0", the axis will depend on the axis address commanded in the same block as G43. The order of priority is shown below.

Zp > Yp > Xp

(Example 5)

G43 Xx1 Hh1 ; ................+ offset to X axis

:

G49 Xx2 ;

:

G44 Yy1 Hh2 ; ................

− offset to Y axis

:

G49 Yy2 ;

:

G43

αα

1 Hh3 ; ................+ offset to additional offset

:

G49

αα

1 ;

:

G43 Xx3 Yy3 Zz3 ; .........Offset is applied on Z axis

:

G49 ;

The handling of the additional axis will follow the parameters "#1029 to 1031 aux_I, J and

K" settings.

If the tool length offset is commanded for the rotary axis, set the rotary axis name for one of the parallel axes.

(c) If H (offset No.) is not designated in the same block as G43, the Z axis will be valid.

(Example 6)

G43 Hh1 ; ......................... Offset and cancel to X axis

:

49 ;

(4) Movement during other commands in tool length offset modal

(a) If reference point return is executed with G28 and manual operation, the tool length offset will be canceled when the reference point return is completed.

(Example 7)

G43 Zz1 Hh1 ;

:

G28 Zz2 ; ........................ Canceled when reference point is reached.

:

G43 Zz2 Hh2 ;

:

(Same as G49)

G49 G28 Zz2 ; ................ After the Z axis is canceled, reference point return is executed.

(b) The movement is commanded to the G53 machine coordinate system, the axis will move to the machine position when the tool offset amount is canceled. When the G54 to G49 workpiece coordinate system is returned to, the position returned to will be the coordinates shifted by the tool offset amount.

104


12.3 Tool radius compensation



This function compensates the radius of the tool. The compensation can be done in the random vector direction by the radius amount of the tool selected with the G command (G38 to G42) and the D command.

Command format

G40X___Y___ ; : Tool radius compensation cancel

G41X___Y___ ; : Tool radius compensation (left)

G42X___Y___ ; : Tool radius compensation (right)

G38I___J___ ; : Change or hold of compensation vector

G39X___Y___ ; : Corner changeover

Can be commanded only during the radius compensation mode.


The No. of compensation sets will differ according to the machine model.

(The No. of sets is the total of the tool length offset, tool position offset and tool radius compensation sets.)

The H command is ignored during the tool radius compensation, and only the D command is valid.

The compensation will be executed within the plane designated with the plane selection G code or axis address 2 axis, and axes other than those included in the designated plane and the axes parallel to the designated plane will not be affected. Refer to the section on plane selection for details on selecting the plane with the G code.

105



12.3.1 Tool radius compensation operation

Tool radius compensation cancel mode

The tool radius compensation cancel mode is established by any of the following conditions.

(1) After the power has been switched on

(2) After the reset button on the setting and display unit has been pressed

(3) After the M02 or M30 command with reset function has been executed

(4) After the tool radius compensation cancel command (G40) has been executed

The offset vectors are zero in the compensation cancel mode, and the tool nose point path coincides with the programmed path.

Programs including tool radius compensation must be terminated in the compensation cancel mode.

Tool radius compensation start (start-up)

Tool radius compensation starts when all the following conditions are met in the compensation cancel mode.

(1) A movement command is issued after the G41or G42 command has been issued.

(2) The tool radius compensation offset No. is 0 < D

≤

max. offset No.

(3) The movement command of positioning (G00) or linear interpolation (G01) is issued.

At the start of compensation, the operation is executed after at least three movement command blocks (if three movement command blocks are not available, after five movement command blocks) have been read regardless of the continuous operation or single block operation.

During compensation, 5 blocks are pre-read and the compensation is arithmetically processed.

Control mode transition diagram

Machining program

Pre-read buffer

Execution block

T____; S____; G00____; G41____; G01____; G02____;

T__; S__;

T__; S__;

G00_; G41_;

Start of pre-reading 5 blocks

G01_; G02_;

G01_; G02_;

G00_; G41_; G01_; G02_;

There are two ways of starting the compensation operation: type A and type B.

The type can be selected with bit 2 of parameter "#1229 set 01". This type is used in common with the compensation cancel type.

In the following explanatory figure, "S" denotes the single block stop point.

106



Start of movement for tool radius compensation

Start point

(1) For inner side of corner

Linear Linear

θ s

Program path r = Compensation amount

Tool center path

G42

θ

G42

Linear Circular

r s

Tool center path

Program path

Start point

Center of circular

(2) For outer side of corner (obtuse angle) [90°

≤

0<180°]

Linear Linear(Type A)

s

Tool center path r = Compensation amount

G41

Program path

θ

Linear Circular(Type A)

s r

Tool center path

G41

θ

Start point

G41

Linear Linear(Type B)

Point of intersection s r r

Tool center path

Program path

θ

Start point

Center of circular

Program path

Linear Circular(Type B)


Tool center path

G41

θ

Start point

Start point

Center of circular

Program path

107



r s

θ

(3) For outer side of corner (obtuse angle) [0<90°]

Linear Linear(Type A)

Tool center path

Linear Circular(Type A)

s r

Center of circular

Tool center path

Program path

G41

Program path

θ

G41 s

Start point

Linear Linear(Type B)

r r

Tool center path

θ

Program path s

Start point

Linear Circular(Type B)

Center of circular

Tool center path

Program path r r

θ

G41

G41

Start point

Start point

(Note 1)

Where is no axis movement command in the same block as G41 or G42, compensation is performed perpendicularly to the next block direction.

108



Operation in compensation mode

Relative to the program path (G00, G01, G02, G03), the tool center path is found from the straight line/circular arc to make compensation.

Even if the same compensation command (G41, G42) is issued in the compensation mode, the command will be ignored.

When 4 or more blocks not accompanying movement are commanded continuously in the compensation mode, overcutting or undercutting will result.

When the M00 command has been issued during tool radius compensation, pre-reading is prohibited.

(1) Machining an outer wall

Linear Linear (90

°≤θ

<180

°

) Linear Linear (0

°

<

θ

<90

°

)

θ

Program path s

Point of intersection

Tool center path

Linear Circular (90

°≤θ

180

°

) s r

Tool center path r

θ

Program path

θ r r s

Program path

Tool center path

Center of circular s

Center of circular

Linear Circular (0

°

<

θ

<90)

Tool center path r r

θ

Program path

109


Circular Linear (90

°≤θ

<180

°

)


Circular Linear (0

°

<

θ

<90

°

)

Center of circular

Program path

θ

Program path

θ r

Tool center path r r s


Circular Circular (90

°≤θ

<180

°

)

Tool center path r


Circular Circular (0

°

<

θ

<90

°

)

Center of circular

Program path

θ r r



Tool center path r


θ r

Program path

Tool center path

Center of circular

110


(2) Machining an inner wall

Linear Linear (Obtuse angle)

θ

Program path r s

Point of

Tool center path intersection


Linear Linear (Acute angle)

θ r r s

Program path

Tool center path

Linear Circular (Obtuse angle)

θ

Program path

Tool center path s

Point of intersection r

Center of circular r

Circular Linear (Obtuse angle)

θ

Program path s


Tool center path

Center of circular

Linear Circular (Acute angle)

Program path

Tool center path r

θ s


Center of circular

Circular Linear (Acute angle)

θ s


Center of circular

Program path

Tool center path

111


Circular Linear (Obtuse angle)

Point of intersection s

Tool center path

θ

Program path

Center of circular

Center of circular r


Circular Linear (Acute angle)

θ



Center of

Tool center path

Program path

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

For spiral arc ..............................A spiral arc will be interpolated from the start to end point of the arc.

For normal arc command...........If the error after compensation is within parameter "#1084

RadErr", the area from the arc start point to the end point is interpolated as a spiral arc.

Hypothetical circle

Tool center path

Program path

End point of circular r s r

R

Center of circular

(4) When the inner intersection point does not exist

In an instance such as that shown in the figure below, the intersection point of arcs A and B may cease to exist due to the offset amount. In such cases, program error (P152) appears and the tool stops at the end point of the previous block.

Tool center path

Program error stop r

Center of circular A r

Program path

A

B

Line intersecting circulars A, B

112



Tool radius compensation cancel

If either of the following conditions is met in the tool radius compensation mode, the compensation will be canceled. However, the movement command must be a command which is not a circular command.

If the compensation is canceled by a circular command, program error (P151) results.

(1) The G40 command has been executed.

(2) The D00 tool number has been executed.

The cancel mode is established once the compensation cancel command has been read, 5-block pre-reading is suspended an 1-block pre-reading is made operational.

Tool radius compensation cancel operation

End point

(1) For inner side of corner

Linear Linear

θ Program path r = Compensation amount s

Tool center path

G40

End point

Circular Linear

θ r s

G40

Tool center path

Center of circular

Program path

113



(2) For outer side of corner (obtuse angle)

Linear Linear (Type A) s

Tool center path

Circular Linear (Type A) s r = Compensation amount r

Tool center path

G40

G40

Program path

θ

θ

End point

End point

Linear Linear (Type B)

G40


Tool center path

Program path

θ

End point

G40

End point

Center of circular

Program path

Circular Linear (Type B)


Tool center path

θ

Program path

Center of circular

114



r

(3) For outer side of corner (acute angle)

Circular Linear (Type A)

Linear Linear (Type A)

Center of circular s Tool center path

θ

G40

Program path s

Tool center path r

Program path

θ

G40

End point

Linear Linear (Type B)

End point

Circular Linear (Type B)

Center of circular

Tool center path s r

Tool center path r

θ

Program path s r r

θ

Program path

G40

G40

End point

End point

115



12.3.2 Other operations during tool radius compensation

Insertion of corner arc

Inserted circular

An arc that uses the compensation amount as the radius is inserted without calculating the point of intersection at the workpiece corner when G39 (corner arc) is commanded. s


Tool center path r = Compensation amount

Program path

Inserted circular s

Program path r = Compensation

amount

Tool center path


(With G39 command)

(No G39 command)

For outer side compensation

(With G39 command)

(No G39 command)

For inner side compensation

Y

N6

N7

Tool center path

Program path

N5

N4

N1 G28X0Y0 ;

N2 G91G01G42X20.Y20.D1F100 ;

N3 G39X40. ;

N4 G39Y40. ;

N5 G39X-40. ;

N6 Y-40. ;

N7 G40X-20.Y-20. ;

N8 M02 ;

N3

N2

X

D1=5.000

N1

Changing and holding of compensation vector

The compensation vector can be changed or held during tool diameter compensation by using the

G38 command.

(1) Holding of vector: When G38 is commanded in a block having a movement command, the point of intersection will not be calculated at the program end point, and instead the vector of the previous block will be held.

G38 Xx Yy ;

This can be used for pick feed, etc.

(2) Changing of vector: A new compensation vector direction can be commanded with I, J and K, and a new offset amount with D.

(These can be commanded in the same block as the movement

command.)

G38 Ii Jj Dd ; (I, J and K will differ according to the selected plane.)

116


Tool center path r

1

N13

Program path

N12

N14


r

2 i

2

+ j

2

=

× r

j

1 r

1

N15

N16 i j

N11

N11G1Xx

11

;N12G38Yy

12

;N13G38Xx

13

;N14G38Xx

14

Yy

14

;N15G38Xx

15

IiJjDd

2

;N16G40Xx

16

Yy

16

;

Vector hold Vector change

Changing the compensation direction during tool diameter compensation

The compensation direction is determined by the tool diameter compensation commands (G41,

G42) and compensation amount sign.

G code

Compensation amount sign +

−

G41 Left-hand compensation Right-hand compensation

G42 Right-hand compensation Left-hand compensation

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

Refer to section 12.3.5 "Precautions for tool diameter compensation" for the movement when the symbol is changed.

Linear Linear

Tool center path


Program path

G41

G41 r r

G42 r

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

117



Linear

↔

Circular r r r

G41

G42 r

G41

G41 r

G42 r

Program path

Tool center path

Linear return

Tool center path

Program path

G41

G42

Arc exceeding 360

°

due to compensation

G42

Tool center path

Program path r

In the case below, it is possible that the arc may exceed 360

° a. With offset direction selection based on

G41/G42 b. I, J, K was commanded in G40.

In cases like this the tool center path will pass through a section where the arc is doubled due to the compensation and a section will be left uncut.

G42

G41

Uncut section

118



Command for eliminating offset vectors temporarily

When the following command is issued in the compensation mode, the offset vectors are temporarily eliminated and a return is then made automatically to the compensation mode.

In this case, the compensation is not canceled, and the tool goes directly from the intersection point vector to the point without vectors or, in other words, to the programmed command point.

When a return is made to the compensation mode, it goes directly to the intersection point.

(1) Reference point return command

S

S

S

N5

Intermediate point

N6

N7 N8

(G41)

N6 G28 X50. Y-40. ;

Temporarily no compensation vectors at

N7 X30. Y-60. ; intermediate point.

N8 X70. Y40. ;

(Reference point when there is no intermediate point)

(2) G33 thread cutting command

Tool nose radius compensation does not apply to the G33 block.

G33


Tool center path

(G41) r

Program path

(3) The compensation vector will be eliminated temporarily with the G53 command (basic machine coordinate system selection).

(Note 1)

The offset vectors do not change with the coordinate system setting (G92) command.

119



Blocks without movement and pre-read inhibit M command

The following blocks are known as blocks without movement. a. M03 ; .................................. M command b. S12 ; .................................. S command c. T45 ; .................................. T command d. G04 X500 ; ........................ Dwell e. G22 X200. Y150. Z100 ; .... Machining inhibit region setting f. G10 L10 P01 R50 ; ............ Offset amount setting g. G92 X600. Y400. Z500. ; ... Coordinate system setting h. (G17) Z40. ; ...................... Movement but not on offset plane

No movement j. G91 X0 ; ............................ Zero movement amount ..... Movement amount is zero

M00, M01, M02 and M30 are handled as pre-read inhibit M codes.

(1) When command is assigned at start of the compensation

Perpendicular compensation will be applied on the next movement block.

N1 X30. Y60. ;

N2

N3

N2 G41 D10 ;

N3 X20. Y-50. ;

movement

N1

N4 X50. Y-20. ;

N4

Compensation vector cannot be generated when 4 or more blocks continue without movement or when a pre-reading prohibit M code is issued.

N2, 3, 4, 5, 6

N1 X30. Y60. ;

N2 G41 D10 ;

N3 G4 X1000 ;

N4 F100 ;

Block without movement

N5 S500 ;

N6 M3 ;

N7 X20. Y-50. ;

N8 X50. Y-20. ;

N1

N7

Point of

intersection

N8

N1 G41 X30. Y60. D10 ;

N2 G4 X1000 ;

N3 F100 ;

N4 S500 ;


N5 M3 ;

N6 X20. Y-50. ;

N7 X50. Y-20. ;

N1

N2 N5

N6


N7

120



(2) When command is assigned in the compensation mode

When the blocks without movement follows up to 3 blocks in succession in the compensation mode and there is no pre-reading prohibit M code is issued, the intersection point vectors will be created as usual.

N6 G91 X100. Y200. ;

N7 N8

N7 G04 X P1000 ;


N8 X200. ;

N6

N8

Block N7 is executed

N6 here.

When 4 or more blocks without movement follow in succession or if there is a pre-read inhibit

M code, the offset vectors are created perpendicularly at the end point of the previous block.

N11

N6 X100. Y200. ;

N7 G4 X1000 ;


N10 M4 ;

N6

N6

N11

N7 N10

In this case, a cut results.

(3) When commanded together with compensation cancel

N6 X100. Y200. ;

N7 G40 M5 ;

N8 X100. Y50. ;

N7

N8

N6

121



When I, J, K are commanded in G40

(1) If the final movement command block in the four blocks before the G40 block is the G41 or

G42 mode, it will be assumed that the movement is commanded in the vector I, J or K direction from the end point of the final movement command. After interpolating between the hypothetical tool center path and point of intersection, it will be canceled. The compensation direction will not change.

(a,b)

Hypothetical tool center path

(i,j)

Tool center path

N2

G41

N1

Program path r

A r

N1 (G41) G1X_ ;

N2 G40XaYbIiJj;

In this case, the point of intersection will always be obtained, regardless of the compensation direction, even when the commanded vector is incorrect as shown below.

(a,b)

N2

Tool center path

G41

N1

Program path r r

A

When the I and j symbols in the above program example are incorrect

(i,j)


122



If the compensation vector obtained with point of intersection calculation is extremely large, a perpendicular vector will be created in the block before G40.

(a,b)

G40

Tool center path

G41

Program path

(i,j)

A r r


(2) If the arc is 360° or more due to the details of I, J and K at G40 after the arc command, an uncut section will occur. r

Uncut section

N2

Program path

Tool center path

N1 r

G42

(i,j) r

G40

N3

Corner movement

N1 (G42,G91) G01X200. ;

N2 G02 J150. ;

N3 G40 G1X150. Y-150. I-100. J100. ;

When a multiple number of offset vectors are created at the joints between movement command blocks, the tool will move in a straight line between those vectors.

This action is called corner movement.

When the vectors do not coincide, the tool moves in order to machine the corner although this movement is part and parcel of the joint block. Consequently, operation in the single block mode will execute the previous block + corner movement as a single block and the remaining joining movement + following block will be executed as a single block in the following operation.

Program path

N1

N2

θ r

Tool center path r

Center of circular

This movement and feedrate fall under block N2.

Stop point with single block

123



12.3.3 G41/G42 commands and I, J, K designation


The compensation direction can be intentionally changed by issuing the G41/G42 command and

I, J, K in the same block.

Command format

G17 (XY plane) G41/G42 X__ Y__ I__ J__ ;

G18 (ZX plane) G41/G42 X__ Z__ I__ K__ ;

G19 (YZ plane) G41/G42 Y__ Z__ J__ K__ ;

Assign an linear command (G00, G01) in a movement mode.

I, J type vectors (G17 XY plane selection)

The new I, J type vector (G17 plane) created by this command is now described. (Similar descriptions apply to vector I, K for the G18 plane and to J, K for the G19 plane.)

As shown in the figures, the vectors with a size equivalent to the offset amount are made to serve as the I, J type compensation vector perpendicularly to the direction designated by I, J without the intersection point of the programmed path being calculated. the I, J vector can be commanded even in the mode (G41/G42 mode in the block before) and even at the compensation start (G40 mode in the block before).

(1) When I, J is commanded at compensation start

Y

N100

X

N110

N120

N130

N140

D1

N150

Program path

(G40)

N100 G91 G41 X100. Y100. I150. D1 ;

N110 G04 X1000 ;

N120 G01 F1000 ;

N130 S500 ;

N140 M03 ;

N150 X150. ;

Tool center path

(2) When there are no movement commands at the compensation start.

Y

N3

(G40)

N1 G41 I150. D1 ;

N2 G91 X100. Y100. ;

N3 X150. ;

D1 N1

N2

X

124



(3) When I, J has been commanded in the G41/G42 mode (G17 plane)

Y

N100

N120

(N120)

(I,J)N110

(2)

D1

(1)

(2)

(G17 G41 G91)

N100 G41 G00X150. J50. ;

N120 G00 X

−

150. ;

X

Program path

Tool center path

Tool path after interrupt

(1) I, J type vector

(2) Intersection point calculation type vector

(Reference)

(K,I) N110

X

N100

N120

(N120)

Z

Z

N100

N120

(N120)

Y

(J,K) N110

(G18 G41 G91)

N100 G41 G00 Z150. I50. ;

N120 G00 Z

−

150. ;

(G19 G41 G91)

N100 G41 G00 Y150. K50. ;

N120 G00 Y

−

150. ;

125



(4) When I, J has been commanded in a block without movement

N3

N4

N5

N2

(I,J)

N1 G41 D1 G01 F1000 ;

N2 G91 X100. Y100. ;

N3 G41 I50. ;

N4 X150. ;

N5 G40 ;

D1

N1

Direction of offset vectors

(1) In G41 mode

Direction produced by rotating the direction commanded by I, J through 90° to the left from the forward direction of the Z axis (axis 3) as seen from the zero point

(Example 1)

With I100.

Offset vector direction

(Example 2)

With I-100.

(-100, 0 IJ direction)

(100, 0 IJ direction)


(2) In G42 mode

Direction produced by rotating the direction commanded by I, J through 90° to the right from the forward direction of the Z axis (axis 3) as seen from the zero point

(Example 1)

With I100.

(0, 100 IJ direction)

(Example 2)

With I-100.


Offset vector direction (-100, 0 IJ direction)

126


Selection of offset modal


The G41 or G42 modal can be selected at any time. y

N3

D1

N2 x

N4

N5

D2

(I,J)

N6

N1 G28 X0 Y0 ;

N2 G41 D1 F1000 ;

N3 G01 G91 X100. Y100. ;

N4 G42 X100. I100. J-100. D2 ;

N5 X100. Y-100. ;

N6 G40 ;

N7 M02 ;

%

Offset amount for offset vectors

The offset amounts are determined by the offset number (modal) in the block with the I, J designation.

< Example 1>

Y

D1

N100

A

D1

(I,J)

(G41 D1 G91)

N100 G41 X150. I50. ;

N110 X100. Y-100. ;

N110

X

Vector A is the offset amount entered in offset number modal D1 in the N200 block.

< Example 2>

Y

D1

N200

B

D2

(I,J)

(G41 D1 G91)

N200 G41 X150. I50. D2 ;

N210 X100. Y-100. ;

N210

X

Vector B is the offset amount entered in offset number modal D2 in the N200 block.

127


Precautions


(1) Issue the I, J type vector in a linear mode (G0, G1). If it is issued in an arc mode at the start of compensation, program error (P151) will result.

An IJ designation in an arc mode functions as an arc center designation in the offset mode.

(2) When the I, J type vector has been designated, it is not deleted (avoidance of interference) even if there is interference.

Consequently, overcutting may arise in such a case.

Y

X

Cut section

(I,J)

N1 G28 X0Y0 ;

N2 G42 D1 F1000 ;

N3 G91 X100. ;

N4 G42 X100. Y100. I10. ;

N5 X100. Y-100. ;

N6 G40 ;

N7 M02 ;

N2

N4

N5

N6

N3

(3) The vectors differ for the G38 I _J_ (K_) command and the G41/G42 I_J_(K_) command.

G38 G41/G42

(G41)

G38 G91 X100. I50. J50. ;

(I J)

(G41)

G41 G91 X100. I50. J50. ;

(I J)

(Offset amount)

(Offset amount)

Vector in IJ direction having an offset amount size

Vector perpendicular in IJ direction and having an offset amount size

128



(4) Refer to the following table for the offset methods based on the presence and/or absence of the G41 and G42 commands and I, J, (K) command.

G41/G42

No

I, J (K)

No

Offset method

Intersection point calculation type vector

No Yes Intersection point calculation type vector

Yes No Intersection point calculation type vector

Yes Yes

I, J, type vector

No insertion block

N3

A

N2

N4

Y

(I,J)

N1 G91 G01 G41 X200. D1 F1000 ;

N2 X-150. Y150. ;

N3 G41 X300. I50. ;

N4 X-150. Y-150. ;

N5 G40 X-200. ;

During the I, J type vector compensation, the A insertion block will not exist.

N1

X

N5

129



12.3.4 Interrupts during tool radius compensation

MDI interrupt

Tool radius compensation is valid in any automatic operation mode-whether memory or MDI operation.

An interrupt based on MDI will give the result as in the figure below after block stop during memory operation.

(1) Interrupt without movement (tool path does not change)

N1 G41D1; S (Stopping position

for single block)

N2 X20. Y50. ;

MDI interrupt

N3 G3 X40. Y-40. R70. ; S1000 M3;

N2

N3

(2) Interrupt with movement

The offset vectors are automatically re-ca lculated at the movement block after interrupt.

With linear interrupt

N1 G41D1;

N2 X20. Y50. ;

MDI interrupt

N3 G3 X40.Y-40. R70. ; X50. Y-30. ;

X30. Y50. ;

S

S

N2

N3

With circular interrupt

N1 G41 D1 ;

N2 X20. Y50. ;

MDI interrupt

N3 G3 X40. Y-40. R70.; G2 X40. Y-40. R70. ;

G1 X4. ;

S

S

N2

N3

130


Manual interrupt


(1) Interrupt with manual absolute OFF.

The tool path is shifted by an amount equivalent to the interrupt amount.

Tool path after interrupt

Interrupt

Tool path after compensation

Program path

(2) Interrupt with manual absolute ON.

In the incremental value mode, the same operation results as with manual absolute OFF.

In the absolute value mode, however, the tool returns to its original path at the end point of the block following the interrupted block, as shown in the figure.

Interrupt

Interrupt

131



12.3.5 General precautions for tool radius compensation

Precautions

(1) Designating the offset amounts

The offset amounts can be designated with the D code by designating an offset amount No.

Once designated, the D code is valid until another D code is commanded. If an H code is designated, the program error (P170) No COMP No will occur.

Besides being used to designate the offset amounts for tool radius compensation, the D codes are also used to designate the offset amounts for tool position offset.

(2) Changing the offset amounts

Offset amounts are normally changed when a different tool has been selected in the compensation cancel mode. However, when an amount is changed in the compensation mode, the vectors at the end point of the block are calculated using the offset amount designated in that block.

(3) Offset amount symbols and tool center path

If the offset amount is negative (

−

), the figure will be the same as if G41 and G42 are interchanged. Thus, the axis that was rotating around the outer side of the workpiece will rotate around the inner side, and vice versa.

An example is shown below. Normally, the offset amount is programmed as positive (+).

However, if the tool path center is programmed as shown in (a) and the offset amount is set to be negative (

−

), the movement will be as shown in (b). On the other hand, if the program is created as shown in (b) and the offset amount is set to be negative (

−

), the movement will be as shown in (a). Thus, only one program is required to execute machining of both male and female shapes. The tolerance for each shape can be randomly determined by adequately selecting the offset amount.

(Note that a circle will be divided with type A when compensation is started or canceled.)

Workpiece

Workpiece

Tool center path

Tool center path

G41 offset amount (+) or G42 offset amount (

−

)

(a)

G41 offset amount (

−

) or G42 offset amount (+)

(b)

132



12.3.6 Changing of offset No. during compensation mode


As a principle, the offset No. must not be changed during the compensation mode. If changed, the movement will be as shown below.

When offset No. (offset amount) is changed:

G41 G01 ............................. Dr1 ;

N101

N102

G0

α

Xx1 Yy1 ;

α

= 0, 1, 2, 3

G0

α

Xx2 Yy2 Dr2 ; ................................... Offset No. changed

N103 Xx3 Yy3 ;

linear

The offset amount designated with N101 will be applied.

The offset amount designated with N102 will be applied.

Tool center path r1

N101

Program path r1

N102 r2

N103 r2

Tool center path

Program path r1 r1 r1 r1 r2 r2

133



(2) Linear circular

Tool center path

Program path r1

N101 r1

N102

G02 r2

Tool center path

Program path

N101 r1 r1

N102 r2

G03 r1 r1

Center of circular

Center of circular

(3) Circular circular

Tool center path

Program path

N101 r1 r1

N102 r2

Center of circular

Tool center path

Program path

Center of circular r1 r1 r1 r1 r2

Center of circular

Center of circular

134



12.3.7 Start of tool radius compensation and Z axis cut in operation


Often when starting cutting, a method of applying a radius compensation (normally the XY plane) beforehand at a position separated for the workpiece, and then cutting in with the Z axis is often used. When using this method, create the program so that the Z axis movement is divided into the two steps of rapid traverse and cutting feed after nearing the workpiece.


When the following type of program is created:

Tool center path

N1 G91 G00 G41 X 500. Y 500. D1 ;

N2 S1000 ;

N3 M3 ;

N4 G01 Z-300. F1 ;

N6 Y 100. F2 ;

•

•

•

•

N1

N6

N4: Z axis lowers

(1 block)

Y

N1

X

N4

Z

N6

Y

With this program, at the start of the N1 compensation the program will be read to the N6 block.

The relation of N1 and N6 can be judged, and correct compensation can be executed as shown above.

If the above program's N4 block is divided into two

N1

N1 G91 G00 G41 X 500. Y 500. D1;

N2 S1000 ;

N3 M3 ;

N4 Z-250. ;

N6

N4

N5 G01 Z-50. F1 ;

N6 Y 100. F2 ;

N6

N5

Y

Cut in

Z

N1

X

X

In this case, the four blocks N2 to N5 do not have a command in the XY plane, so when the N1 compensation is started, the program cannot be read to the N6 block.

As a result, the compensation is done based only on the information in the N1 block, and the compensation vector is not created at the start of compensation. Thus, an excessive cut in occurs as shown above.

135



In this case, consider the calculation of the inner side, and before the Z axis cutting, issue a command in the same direction as the direction that the Z axis advances in after lowering, to prevent excessive cutting.

N1 G91 G00 G41 X 500. Y 400. D1 ;

N2 Y100. S1000 ;

N3 M3 ;

N4 Z-250. ;

N5 G01 Z-50. F1 ;

N6 Y 100. F2 ;

N2

N6

N2

N4

N6

N5

N6

Y N1

Y

N1

X

Z

The movement is correctly compensated as the same direction as the N6 advance direction is commanded in N2.

136



12.3.8 Interference check


(1) Outline

A tool, whose radius has been compensated with the tool radius compensation function by the usual 2-block pre-read, may sometimes cut into the workpiece. This is known as interference, and interference check is the function which prevents this from occurring.

There are three types of interference check, as indicated below, and each can be selected for use by parameter.

Function Parameter

Interference check alarm function

#8102 : OFF

#8103 : OFF

Operation

A program error results before the execution of the block in which the cut arises, and operation stops.

Interference check avoidance function

#8102 : ON

#8103 : OFF

The tool path is changed so that workpiece is not cut into.

Interference check invalid function

#8103 : ON Cutting proceeds unchanged even when it occurs.

Use this for microscopic segment programs.

(Note)

#8102 COLL. ALM OFF (interference check avoidance)

#8103 COLL. CHK OFF (interference check invalid)


(Example)

Avoidance path

Outer diameter of tool

(G41)

N1 G90 G1 X50. Y-100.;

N2 X70. Y-100.;

N3 X120. Y0;

N1 N3

Cutting with N2

N2

Cutting with N2

(1) With alarm function

The alarm occurs before N1 is executed and so, using the edit function, N1 can be changed as below and machining can be continued :

N1 G90 G1 X20. Y

−

40. ;

(2) With avoidance function

The intersection point of N1 and N3 is calculated and the interference avoidance vectors are created.

137



(3) With interference check invalid function

The tool passes while cutting the N1 and N3 line.

(2) (3)' (4)'

(1)

(2)'

(3) N3

(4)

(1)'

N1

Vectors (1) (4)' check

↓


↓


N2

Example of interference check

→

No interference

→

No interference

→

Interference

→

↓

Erase vectors (3) (2)'

Erase vectors (4) (1)'

With the above process, the vectors (1), (2), (3)' and (4)' will remain as the valid vectors, and the path that connects these vectors will be executed as the interference avoidance path.

138


Conditions viewed as interference


If there is a movement command in three of the five pre-read blocks, and if the compensation calculation vectors created at the contacts of each movement command intersect, it will be viewed as an interference.

Tool center path

Program path r

N1

N3

Vectors intersect

N2

When interference check cannot be executed

(1) When three of the movement command blocks cannot be pre-read

(When there are three or more blocks in the five pre-read blocks that do not have movement)

(2) When there is an interference following the fourth movement block

Tool center path

Program path

N6

N1

N5

N2

Interference check is not possible

N3

N4

139


Operation during interference avoidance


The movement will be as shown below when the interference avoidance check is used.

Tool center path

Program path

N1

N3

N2

Tool center path w hen interference is

Tool center path w ithout interference

Program path

N2

N3

Solid line vector : Valid

Dotted line vector : Invalid

N1

Linear movement

N1 r r

Tool center path w hen interference is

Tool center path w ithout interference check

Program path

N2 N3

Center of circular

140



N3

Avoidance vector

N2

If all of the line vectors for the interference avoidance are deleted, create a new avoidance vector as shown on the right to avoid the interference.

Tool center path

Program path

N1

Avoidance vector r2 r1

N3

N4

Tool center path 2

Avoidance vector 1

Avoidance vector 2

N2

Tool center path 1 r2 r1

N1

Program path

In the case of the figure below, the groove will be left uncut.

Interference avoidance path

Tool center path

Program path

141


Interference check alarm


The interference check alarm occurs under the following conditions.

(1) When the interference check alarm function has been selected

(a) When all the vectors at the end block of its own block have been deleted.

When, as shown in the figure, vectors 1 through 4 at the end point of the N1 block have all been deleted, program error

(P153) results prior to N1 execution.

N1

1

N2

2 3

N3

4

(2) When the interference check avoidance function has been selected

(a) When there are valid vectors at the end point of the following block even when all the vectors at the end point of its own block have been deleted.

(i) When, in the figure, the

N2 interference check is conducted, the N2 end point vectors are all deleted but the N3 end point vectors are regarded as valid.

Program error (P153) now occurs at the N1 end point.

Alarm stop

3

2

N1

N4

4

1

N3

N2

(ii) In a case such as that shown in the figure, the tool will move in the reverse direction at N2.

Program error (P153) occurs after N1 execution.

1 2 3 4

N1

N4

N2

N3

142



(b) When avoidance vectors cannot be created

(i) Even when, as in the figure, the conditions for creating the avoidance vectors are met, it may still be impossible to create these vectors or the interference vectors may interfere with N3.

Program error (P153) will occur at the N1 end point when the vector intersecting angle is more than 90

°

.

N1

N2

Alarm stop

N4

N3

Alarm stop

N1

N2

N4

N3

Angle of intersection

(c) When the program advance direction and the advance direction after compensation are reversed

In the following case, interference is still regarded as occurring even when there is actually no interference.

When grooves which are narrower than the tool radius or which have parallel or widening walls are programmed

Program path

Tool center path

Stop

143


12.4 Programmed offset input

12.4 Programmed offset input; G10, G11


The tool offset and workpiece offset can be set or changed on the tape using the G10 command.

During the absolute value (G90) mode, the commanded offset amount will become the new offset amount, and during the incremental value (G91) mode, the commanded offset amount will be added to the currently set offset amount to create the new offset amount.

Command format

(1) Workpiece offset input

G90 G10 L2 P__Xp__Yp__Zp__;

G91

P : 0 External workpiece

1 G54

2 G55

3 G56

4 G57

5 G58

6 G59

If a value other than the above is set or if the P command is omitted, the currently selected workpiece offset will be handled as the input.

(Note)

The offset amount in the G91 will be an incremental value and will be cumulated each time the program is executed. Command G90 or G91 before the G10 as a cautionary means to prevent this type of error.

(2) Tool offset input

(a) For tool offset memory I

G10 L10 P__R__ ;

P : Offset No.

R : Offset amount

(b) For tool offset memory II

G10 L10 P__R__ ;

G10 L11 P__R__ ;

G10 L12 P__R__ ;

G10 L13 P__R__ ;

Tool length compensation shape offset

Tool length compensation wear compensation

Tool radius shape offset

Tool radius wear compensation

(3) Offset input cancel

G11 ;

144




(1) Program error (P171) will occur if this command is input when the specifications are not available.

(2) G10 is an unmodal command and is valid only in the commanded block.

(3) The G10 command does not contain movement, but must not be used with G commands other than G21, G22, G54 to G59, G90 or G91.

(4) If an illegal L No. or offset No. is commanded, the program errors (P172 and P170) will occur respectively.

If the offset amount exceeds the maximum command value, the program error (P35) will occur.

(5) Decimal point inputs can be used for the offset amount.

(6) The offset amounts for the external workpiece coordinate system and the workpiece coordinate system are commanded as distances from the basic machine coordinate system zero point.

(7) The workpiece coordinate system updated by inputting the workpiece coordinate system will follow the previous modal (G54 to G59) or the modal (G54 to G59) in the same block.

(8) L2 can be omitted when the workpiece offset is input.

(9) Do not command G10 in the same block as fixed cycles and subprogram call commands.

This will cause malfunctioning and program errors.


(1) Input the offset amount.

• • • • • • ; G10L10P10R–12345 ; G10L10P05R98765 ; G10L10P30R2468 ; • • •

H10=–12345 H05=98765 H30=2468

(2) Updating of offset amount

(Example 1)

Assume that H10 = -1000 is already set.

N1 G01 G90 G43 Z – 100000 H10; (Z = –101000)

N3 G91 G10 L10 P10R – 500 ;

(The mode is the G91 mode, so –500 is added.)

N4 G01 G90 G43 Z – 100000

H10 ;

(Z = –101500)

145



(Example 2)

Assume that H10 = –1000 is already set.

Main program

N1 G00 X100000 ;

N2 #1 = –1000 ;

N3 M98 P1111 L4 ; a b

1

, b

2

, b

3

, b

4

Subprogram

O1111

N1 G01 G91 G43 Z0 H10 F100 ; c

1

, c

2

, c

3

, c

4

G01 X1000 ;

#1 = #1

−

1000 ; d

1

, d

2

, d

3

, d

4

G90 G10 L10 P10 R#1 ;

M99;

(a) (b

1

) (b

2

) (b

3

) (b

4

) c

1 d

1 c

2 d

2 c

3 d

3 c

4 d

4

(Note)

Final offset amount will be H10= –5000.

1000 1000 1000 1000

(Example 3)

The program for Example 2 can also be written as follows.

Main program

N1

N2

G00 X100000 ;

M98 P1111 L4 ;

Subprogram

O1111 N1

G01 G91 G43 Z0 H10 F100 ;

N2

N3

G01 X1000 ;

G10 L10 P10 R

−

1000 ;

146



(3) When updating the workpiece coordinate system offset amount

Assume that the previous workpiece coordinate system offset amount is as follows.

X =

−

10.000 Y =

−

10.000

N100 G00 G90 G54 X0 Y0 ;

N101 G90 G10 L2 P1 X

−

15.000 Y

−

15.000 ;

N102 X0 Y0 ;

M02 ;

-X -20. -10.

M

Basic machine coordinate system zero point

N100

-X

G54 coordinate before change

N101

(W1)

G54 coordinate after

-X change

W1

N102

-10.

-Y

-20.

-Y

-Y

(Note 1)

Changes of workpiece position display at N101

At N101, the G54 workpiece position display data will change before and after the workpiece coordinate system is changed with G10.

X = 0

→

Y = 0

X = +5.000

Y = +5.000

When workpiece coordinate system offset amount is set in G54 to G59

G90 G10 L2 P1 X

−

10.000 Y

−

10.000 ;

G90 G10 L2 P2 X

−

20.000 Y

−

20.000 ;

G90 G10 L2 P3 X

−

30.000 Y

−

30.000 ;

G90 G10 L2 P4 X

−

40.000 Y

−

40.000 ;

G90 G10 L2 P5 X

−

50.000 Y

−

50.000 ;

G90 G10 L2 P6 X

−

60.000 Y

−

60.000 ;

147



(4) When using one workpiece coordinate system as multiple workpiece coordinate systems

Main program

Subprogram

O200

#1 =

−

50. #2 = 10. ;

M98 P200 L5 ;

M02 ;

%

N1 G90 G54 G10 L2 P1 X#1 Y#1 ;

N2 G00 X0 Y0 ;

N3 X

−

5. F100 ;

N4 X0 Y

−

5. ;

N6 #1 = #1 + #2 ;

%

G54

G54’

W

G54”

G54”’

G54””

W

M

W

5th time

-10.


-20.

4th time

W

-30.

3rd time

W

-40.

2nd time

1st time

-50.

-Y

Precautions

(1) Even if this command is displayed on the screen, the offset No. and variable details will not be updated until actually executed.

N1 G90 G10 L10 P10R

−

100 ;

N2 G43 10000 H10 ;

N3 G0 X–10000 Y

−

10000 ;

N4 G90 G10 L10 P10 R

−

200 ; .. The H10 offset amount is updated when the N4 block is executed.

148

13. Program Support Functions

13.1 Canned cycles



13.1.1 Standard canned cycles; G80 to G89, G73, G74, G76


These standard canned cycles are used for predetermined sequences of machining operations such as positioning, hole drilling, boring, tapping, etc. which are specified in a block. The various sequences in the table below are provided for the standard canned cycles.

By editing the standard canned cycle subprogram, the canned cycle sequence can be changed by the user. The user can also register and edit an original canned cycle program. For the standard canned cycle subprogram, refer to the list of the canned cycle subprogram in the appendix of the operation manual. The list of canned cycle functions for this control unit is shown below.

G code

G80

Hole machining

Operation at hole bottom start

(

−

Z direction)

Dwell Spindle

Return operation

(+Z direction)

⎯ ⎯ ⎯ ⎯

Application

Cancel

⎯

Yes

⎯

⎯

Rapid feed

Rapid feed

Drill, spot drilling cycle

Drill, counter boring cycle

G83 Intermittent

⎯ ⎯

Rapid feed

Deep hole drilling cycle

G86

G88

Cutting feed

Rapid traverse

Yes

⎯

Yes

⎯

Yes

Yes

Reverse rotation

⎯

Stop

Forward rotation

Stop

⎯

⎯

Cutting feed

Cutting feed

Rapid feed

Cutting feed

Rapid feed

Cutting feed

Tapping cycle

Boring cycle

Boring cycle

Back boring cycle

Boring cycle

Boring cycle

Yes Rapid feed Stepping cycle

Forward rotation

Cutting feed

Reverse tapping cycle

—

Oriented spindle stop

Rapid feed Fine boring cycle

A canned cycle mode is canceled when the G80 or any G command in (G00, G01, G02, G03) is issued. The various data will also be cleared simultaneously to zero.

149


Command format


G8

∆

(G7

∆

) X__ Y__ Z__ R__ Q__ P__ F__ L__ S__ , S __ ,R __ ,I__ ,J__;

G8

∆

(G7

∆

)

X__ Y__ Z__

R__ Q__ P__ F__

L__

: Hole machining mode

: Hole positioning data

: Hole machining data

: Number of repetitions

S__

, S__

, R__

, I__

,J__

: Spindle rotation speed

: Spindle rotation speed at during retract

: Synchronization changeover

: Positioning axis in-position width

: Drilling axis in-position width

As shown above, the format is divided into the hole machining mode, hole positioning data, hole machining data, No. of repetitions, spindle rotation speed, synchronization changeover (or spindle rotation speed at during retract), positioning axis in-position width and drilling axis in-position width.


(1) Data outline and corresponding address

(a) Hole machining mode : Fixed cycle modes such as drilling, counter boring,

(b) Hole position data

(c) Hole machining data

(d) No. of repetitions tapping and boring

: Data used to position the X and Y axes (unmodal)

: Machining data actually used for machining (modal)

: Number of times to carry out drilling machining (unmodal)

(e) Synchronization changeover : Command for selecting synchronous/asynchronous tapping during G84/G74 tapping (modal)

(2) If M00 or M01 is commanded in the same block as the canned cycle or during the canned cycle mode, the canned cycle will be ignored. Instead, M00 and M01 will be output after positioning.

The canned cycle will be executed if X, Y, Z or R is commanded.

150



(3) There are 7 actual operations which are each described in turn below.

Operation 1

Operation 2

Initial point

Operation 3

R point

Operation 7

Operation 4

Operation 6

Operation 5

Operation 1 : This indicates the X and Y axes positioning, and executes positioning with G00.

Operation 2 : This is an operation done after positioning is completed (at the initial hole), and when G87 is commanded, the M10 command is output from the control unit to the machine. When this M command is executed and the finish signal (FIN) is received by the control unit, the next operation will start. If the single block stop switch is ON, the block will stop after positioning.

Operation 3 : The tool is positioned to the R point by rapid traverse.

Operation 4 : Hole machining is conducted by cutting feed.

Operation 5 : This operation takes place at the hole bottom position and it differs according to the canned cycle mode. Possible actions include spindle stop (M05) spindle reverse rotation (M04), spindle forward rotation (M03), dwell and tool shift.

Operation 6 : The tool is retracted to the R point.

Operation 7 : The tool is returned to the initial pint at the rapid traverse rate.

Whether the canned cycle is to be completed at operation 6 or 7 can be selected by the following G commands.

G98 ............ Initial level return

G99 ............ R point level return

These are modal commands, and for example, if G98 is commanded once, the G98 mode will be entered until G99 is designated. The initial state when the NC is ready is the G98 mode.

The hole machining data will be ignored if X, Y, Z or R is not commanded. This function is mainly used with the special canned cycled.

(4) Canned cycle addresses and meanings

Address

G

X

Y

Z

P

Q

R

F

L

I, J, K

S

, S

, R

Significance

Selection of hole machining cycle sequence (G80 to G89, G73, G74, G76)

Designation of hole drilling position (absolute value or incremental value)

Designation of hole drilling position (absolute value or incremental value)

Designation of hole bottom position (absolute value or incremental value)

Designation of dwell time at hole bottom position (decimal points will be ignored)

Designation of cut amount for each cutting pass with G73 or G83, or designation of the shift amount at G76 or G87 (incremental value)

Designation of R point position (absolute value or incremental value)

Designation of feed rate for cutting feed

Designation of number of repetitions. 0 to 9999

Designation of shift amount at G76 or G87 (incremental value)

(The shift amount is designated with the Q address depending on the parameter setting.)

Spindle rotation speed command

Spindle rotation speed designation for synchronous tap retract

Synchronous/asynchronous tap cycle selection

151



(5) Difference between absolute value command and incremental value command

For absolute value

For incremental value

-r

R point

+r

R point

-z

-z

Workpiece

Workpiece

(6) Feed rate for tapping cycle and tapping retract

The feed rates for the tapping cycle and tapping retract are as shown below.

(a) Selection of synchronous tapping cycle/asynchronous tapping cycle

Program G84×××, Rxx

, R00

Control parameter

Synchronous tapping

⎯

Synchronous/ asynchronous

Asynchronous

, Rxx

No designation

, R01

−

is irrelevant to the setting

OFF

ON

⎯

Synchronous

(b) Selection of asynchronous tapping cycle feed rate

G94/G95

Control parameter

F1-digit value

F command value Feed designation

G94

ON

G95

⎯

−

is irrelevant to the setting

Other than F0 to

F8

F0 to F8 (no decimal point)

F designation

Per-minute feed

F1-digit feed

Per-revolution feed

(c) Spindle rotation speed during retract of synchronous tapping cycle

Address


Command range

(unit)

Remarks

,S Spindle The data is held as modal speed during retract information.

If the value is smaller than the speed rotation speed, the speed rotation speed value will be valid even during retract.

If the spindle rotation speed is not 0 during retract, the tap retract override value will be invalid.

152


Positioning plane and hole drilling axis


The canned cycle has basic control elements for the positioning plane and hole drilling axis. The positioning plane is determined by the G17, G18 and G19 plane selection command, and the hole drilling axis is the axis perpendicular (X, Y, Z or parallel axis) to the above plane.

Plane selection

G17 (X

−

Y)

G18 (Z

−

X)

G19 (Y

−

Z)

Positioning plane

Xp

Zp

Yp

−

−

−

Yp

Xp

Zp

Hole drilling axis

Zp

Yp

Xp

Xp, Yp and Zp indicate the basic axes X, Y and Z or an axis parallel to the basic axis.

A random axis other than the hole drilling axis can be commanded for positioning.

The hole drilling axis is determined by the axis address of the hole drilling axis commanded in the same block as G81 to G89, G73, G74 or G76. The basic axis will be the hole drilling axis if there is no designation.

(Example 1)

When G17 (XY plane) is selected, and the axis parallel to the Z axis is set as the W axis.

G81 ... W__; The W axis is used as the hole drilling axis.

G81 ... Z __; The Z axis is used as the hole drilling axis.

G81 ... ; (No Z or W) The Z axis is used as the hole drilling axis.

(Note 1)

The hole drilling axis can be fixed to the Z axis with parameter #1080 Dril_Z.

(Note 2)

Change over the hole drilling axis in the canned cycle canceled state.

In the following explanations on the movement in each canned cycle mode, the XY plane is used for the positioning plane and the Z axis for the hole drilling axis.

Note that all command values will be incremental values, the positioning plane will be the XY plane and the hole drilling axis will be the Z axis.

153



(a) G81 (Drilling, spot drilling)

Program

G81 Xx1 Yy1 Zz1 Rr1 Ff1 ,Ii1 ,Jj1;

(1) x

1

, y

1

(2) r

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

1

(4) G98 mode G0Z

−

(z

1

G99 mode G0Z

−

z

1

+r

1

)

(3)

(4)

(4) z

1

G98 G99 mode mode

The operation stops at after the (1), (2) and (4) commands during single block operation.

Operation pattern i1 j1

(b) G82 (Drilling, counter boring)

Program

G82 Xx

1

Yy

1

Zz

1

Rf

1

Ff

1

Pp

1

,Ii

1

,Jj

1

;

P : Dwell designation

(1) x

1

, y

1

(2)

(3)

(5)

(5)

(4)

G98 G99

mode mode r

1 z

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

1

(4) G4 Pp

1

(Dwell) mode G0Z (z

1

+r

1

)

G0Z



154



(c) G83 (Deep hole drilling cycle)

Program

G83 Xx

1

Yy

1

Zz

1

Rr

1

Qq

1

Ff

1

,Ii

1

,Jj

1

;

Q : This designates the cutting amount per pass, and is always designated with an incremental value.

(1) x

1

,y

1

(2) r

1 q

1

(3) (4) q

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zq

1

Ff

1

(4) G0 Z

−

q

(5) G0 Z (q

1

1

−

m) q

1

(6) G1 Z (q

1

+ m) Ff

1

(7) G0 Z

−

2 • q

(8) G0 Z (2 • q

1

1

−

m)

(9) G1 Z (q

1

+ m) Ff

1

(10) G0 Z

−

3 • q

1

:

: mode G0Z (z

1

+r

1

)

G0Z m

(5)

(7)

(8)

(6)

(10)

(9) m

(n) (n)

(n) - 1

G98 G99

mode mode z

1


:

:

When executing a second and following cutting in the G83 as shown above, the movement will change from rapid traverse to cutting feed several mm before the position machined last. When the hole bottom is reached, the axis will return according to the G98 or G99 mode. m will differ according to the parameter "#8013 G83 n". Program so that q

1

>m.

The operation stops at after the (1), (2) and (n) commands during single block operation.

155



(d) G84 (Tapping cycle)

Program

G84 Xx

1

Yy

1

Zz

1

Rr

1

Ff

1

Pp

1

Ss

1

,Ss

2

,Rr

2

,Ii

1

,Jj

1

;

P : Dwell designation

(1) x

1

,y

1

(2)

(7)

(8)

(7) (8)

(3) (6) (6) r

1 z

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

1

(4) G4 Pp

1

(5) M4 (Spindle reverse rotation)

(6) G1 Z

−

z

1

Ff

1

Pp

1

(8) M3 (Spindle forward rotation)

(9)

G0Z

G99 mode No movement

(4) (5)

G98 G99 mode mode


• When r2 = 1, the synchronous tapping mode will be entered, and when r2 = 0, the asynchronous tapping mode will be entered.

• When G84 is executed, the override will be canceled and the override will automatically be set to 100%.

• Dry run is valid when the control parameter "G00 DRY RUN" is on and is valid for the positioning command. If the feed hold button is pressed during G84 execution, and the sequence is at (3) to (6), the movement will not stop immediately, and instead will stop after (6). During the rapid traverse in sequence (1), (2) and (9), the movement will stop immediately.

• The operation stops at after the (1), (2) and (9) commands during single block operation.

• During the G84 modal, the "Tapping" NC output signal will be output.

• During the G84 synchronous tapping modal, the M3, M4, M5 and S code will not be output.

156



This function allows spindle acceleration/deceleration pattern to be approached to the speed loop acceleration/deceleration pattern by dividing the spindle and drilling axis acceleration/deceleration pattern into up to three stages during synchronous tapping.

The acceleration/deceleration pattern can be set up to three stages for each gear.

When returning from the hole bottom, rapid return is possible depending on the spindle rotation speed during return. The spindle rotation speed during return is held as modal information.

(i) When tap rotation speed < spindle rotation speed during return

≤

synchronous tap changeover spindle rotation speed 2

Smax

S2

S(S1)

T1

T2

T1

T1

T1

S1

S'

S2

Smax T2

S : Command spindle rotation speed

S' : Spindle rotation speed during return

S1 : Tap rotation speed (spindle base specification parameters #3013 to #3016)

S2 : Synchronous tap changeover spindle rotation speed 2

(spindle base specification parameters #3037 to #3040)

Smax : Maximum rotation speed (spindle base specification parameters #3005 to

#3008)

T1 : Tap time constant (spindle base specification parameters #3017 to #3020)

T2 : Synchronous tap changeover time constant 2


157



(ii) When synchronous tap changeover spindle rotation speed 2 < spindle rotation speed during return

Smax

S2

S(S1)

T1

T1

T2

T3

T1 T1

S1

S2

S'(Smax)

T3

T2

S : Command spindle rotation speed

S' : Spindle rotation speed during return

S1 : Tap rotation speed (spindle base specification parameters #3013 to #3016)

S2 : Synchronous tap changeover spindle rotation speed 2


Smax : Maximum rotation speed (spindle base specification parameters #3005 to

#3008)

T1 : Tap time constant (spindle base specification parameters #3017 to #3020)





158



Program

G85 Xx

1

Yy

1

Zz

1

Rr

1

Ff

1

;

(1) x

1

, y

1

(2) (5) r

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

(4) G1 Z

−

z

1

1

Ff

1

(5)

G0Z

G99 mode No movement z

1

(3)

(4)

(4)

G98 G99 mode mode

The operation stops at after the (1), (2), and (4) or (5) commands during single block operation.

Program

G86 Xx

1

Yy

1

Zz

1

Rr

1

Ff

1

Pp

1

;

(1) x

1

, y

1

(7)

(2)

(3)

(7)

(6) (6) r

1 z

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

1

(4) G4 Pp

1

(5) M5 (Spindle stop)

(6)

G0Z

G0Z

1

+r

1

)


(4)(5)

G98 G99 mode mode


159



(g) G87 (Back boring)

Program

G87 Xx

1

Yy

1

Zz

1

Rr

1

Iq

1

Jq

2

Ff

1

;

(Note)

Take care to the z

1

and r

1

designations.

1

symbols are reversed).

There is no R point return.

(1) x

1

, y

1

(2)

(12)(11)

(3)

Xq

1

(Yq

2

)

(10) r

1

(8) (9)

(7)

(6) (5)

(4) z

1

Xx

1

Yy

1

(2) M19 (Spindle orient)

Xq

1

(Yq

2

) (Shift)

Zr

(5) G1

1

X

− q

1

(Y

− q

2

) Ff

1

(Shift)


Zz

1

Ff

1


Xq

1

(Yq

2

) (Shift)

G0Z

1

)

(10)

+z

1

)

(11) G0 X

− q

1

(Y

− q

2

) (Shift)


The operation stops at after the (1), (4), (6) and (11) commands during single block operation.

When this command is used, high precision drilling machining that does not scratch the machining surface can be done.

(Positioning to the hole bottom and the escape (return) after cutting is executed in the state shifted to the direction opposite of the cutter.)

The shift amount is designated as shown below with addresses I, J and K.

Tool during cutting

Tool after cutting

Cutter

Spindle orient position

For G17 : I, J

For G18 : K, I

For G19 : J, K

Shift amount

Machining hole

The shift amount is executed with linear interpolation, and the feed rate follows the F command.

Command I, J, and K with incremental values in the same block as the hole position data.

I, J and K will be handled as modals during the canned cycle.

(Note)

If the parameter "#1080 Dril_Z" which fixes the hole drilling axis to the Z axis is set, the shift amount can be designated with address Q instead of I and j. In this case, whether to shift or not and the shift direction are set with parameter

"#8207 G76/87 IGNR" and "#8208 G76/87 (

−

)". The symbol for the Q value is ignored and the value is handled as a positive value.

The Q value is a modal during the canned cycle, and will also be used as the

G83, G73 and G76 cutting amount.

160



Program

G88 Xx

1

Yy

1

Zz

1

Rr

1

Ff

1

Pp

1

;

(1) x

1

, y

1

(2)

(3)

(8)

(9)

(8)

(9) r

1 z

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

1

(4) G4 Pp

1

(5) M5 (Spindle stop)

(6) Stop when single block stop switch is ON.

(7) Automatic start switch ON

(8)

G0Z

1

+r

1

)

G0Z


(4)(5)(6)(7)

G98 G99 mode mode

The operation stops at after the (1), (2), (6) and (9) commands during single block operation.

Program

G89 Xx

1

Yy

1

Zz

1

Rr

1

Ff

1

Pp

1

;

(1) x

1

, y

1

(2)

(3)

(6)

(5)

(5) r

1 z

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

1

(4) G4 Pp

(5) G1 Z

1

−

z

1

Ff

1

(6)

G0Z


(4)

G98 G99 mode mode

The operation stops at after the (1), (2) and (5) or (6) commands during single block operation.

161



(j) G73 (Step cycle)

Program

G73 Xx

1

Yy

1

Zz

1

Qq

1

Rr

1

Ff

1

Pp

1

;

(1) x

1

, y

1

(2) q q q

(3) m

(4)

(5)

(6)

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zq

1

Ff

1

(4) G4 Pp

1

m

1

+ m) Ff

1

: mode G0Z (z

1

+r

1

)

G0Z

(n) -1

(n)

(n)

G98 G99 mode mode r

1 z

1

When executing a second and following cutting in the G73 as shown above, the movement will return several m mm with rapid traverse and then will change to cutting feed.

The return amount m will differ according to the parameter "#8012 G73 n".

The operation stops at after the (1), (2) and (n) commands during single block operation.

162



(k) G74 (Reverse tapping cycle)

Program

G74 Xx

1

Yy

1

Zz

1

Rr

1

Pp

1

Ss

1

,Ss

2

Rr

2

,Ii

1

,Jj

1

;

(1) x

1

,y

1

(2)

(3)

(4)(5)

(9)

(7) (8)

(6)

(7)(8)

(6)

G98 G99 mode mode r

1 z

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

1

(4) G4 Pp

1


(6) G1 Z – z

1

Ff

1

(7) G4 Pp

1

(8) M4 (Spindle reverse rotation)

(9)

G0Z


When r

2

= 1, the synchronous tapping mode will be entered, and when r

2

= 0, the asynchronous tapping mode will be entered.

When G74 is executed, the override will be canceled and the override will automatically be set to 100%. Dry run is valid when the control parameter "#1085 G00Drn" is set to "1" and is valid for the positioning command. If the feed hold button is pressed during G74 execution, and the sequence is at (3) to (6), the movement will not stop immediately, and instead will stop after (6). During the rapid traverse in sequence (1), (2) and (9), the movement will stop immediately.


During the G74 and G84 modal, the "Tapping" NC output signal will be output.

During the G74 synchronous tapping modal, the M3, M4, M5 and S code will not be output.

This function allows spindle acceleration/deceleration pattern to be approached to the speed loop acceleration/deceleration pattern by dividing the spindle and drilling axis acceleration/deceleration pattern into up to three stages during synchronous tap.

Refer to the item "d) G84 (Tapping cycle)" for details of multi-stages of the spindle acceleration/deceleration pattern.

163



(l) G76 (Fine boring)

Program

G76 Xx

1

Yy

1

Zz

1

Rr

1

Iq

1

Jq

2

Ff

1

; x

1

, y

1

(7)

(1)

(2)

(8)

(3)

(8)

(7)

(6) r

1

(6) z

1

(1) G0 Xx

1

Yy

1

(2) G0 Zr

1

(3) G1 Zz

1

Ff

1


(5) G1 Xq

(6)

1

(Yq

2

) Ff

−

1

(Shift)

1

+r

1

)

(7) G0 X

−

q

1

G0Z

(Y

−

q

2

) Ff

1

(Shift)


(4)(5)

G98 G99 mode mode


When this command is used, high precision drilling machining that does not scratch the machining surface can be done.

(Positioning to the hole bottom and the escape (return) after cutting is executed in the state shifted to the direction opposite of the cutter.)

Tool during cutting

Cutter

Spindle orient position

Cancel

Cancel

Shift

Shift

Tool after cutting

The shift amount is designated as shown below with addresses I, J and K.

For G17 : I, J

For G18 : K, I

For G19 : J, K

The shift amount is executed with linear interpolation, and the feed rate follows the F command.

Shift amount

Machining hole

Command I, J, and K with incremental values in the same block as the hole position data.

I, J and K will be handled as modals during the canned cycle.

(Note)

If the parameter "#1080 Dril_z" which fixes the hole drilling axis to the Z axis is set, the shift amount can be designated with address Q instead of I and J. In this case, whether to shift or not and the shift direction are set with parameter

"#8207 G76/87 IGNR" and "#8208 G76/87 (

−

)". The symbol for the Q value is ignored and the value is handled as a positive value.

The Q value is a modal during the canned cycle, and will also be used as the

G83, G87 and G73 cutting amount.

164


Precautions for using canned cycle


(1) Before the canned cycle is commanded, the spindle must be rotating in a specific direction with an M command (M3 ; or M4 ;).

Note that for the G87 (back boring) command, the spindle rotation command is included in the canned cycle so only the rotation speed command needs to be commanded beforehand.

(2) If there is a basic axis, additional axis or R data in the block during the canned cycle mode, the hole drilling operation will be executed. If there is not data, the hole will not be drilled.

Note that in the X axis data, if the data is a dwell (G04) time command, the hole will not be drilled.

(3) Command the hole machining data (Q, P, I, J, K) in a block where hole drilling is executed.

(Block containing a basic axis, additional axis or R data.)

(4) The canned cycle can be canceled by the G00 to G03 or G33 command besides the G80 command. If these are designated in the same block as the canned cycle, the following will occur.

(Where, 00 to 03 and 33 are m, and the canned cycle code is n)

Gm Gn X___Y___Z___R___Q___P___L___F___;

Execute Ignore Execute Ignore Record

Gm Gn X___Y___Z___R___Q___P___L___F___;

Ignore Execute Ignore Record

Note that for the G02 and G03 commands, R will be handled as the arc radius.

(5) If an M function is commanded in the same block as the canned cycle command, the M code and MF will be output during the initial positioning. The next operation will be moved to with

FIN (finish signal).

If there is a No. of times designated, the above control will be executed only on the first time.

(6) If another control axis (ex., rotary axis, additional axis) is commanded in the same block as the canned cycle control axis, the canned cycle will be executed after the other control axis is moved first.

(7) If the No. of repetitions L is not designated, L1 will be set. If L0 is designated in the same block as the canned cycle G code command, the hole machining data will be recorded, but the hole machining will not be executed.

(Example)

G73X___Y___Z___R___Q___P___F___L0___;

Execute Record only code having an address

(8) When the canned cycle is executed, only the modal command commanded in the canned cycle program will be valid in the canned cycle subprogram. The modal of the program that called out the canned cycle will not be affected.

(9) Other subprograms cannot be called from the canned cycle subprogram. subprogram.

(11) If the No. of repetitions L is 2 or more during the incremental value mode, the positioning will also be incremented each time.

(Example)

G91G81X10. Z

−

50.R

−

20.F100.L3 ;

Z

10.

10.

10.

X

165



13.1.2 Initial point and R point level return; G98, G99


Whether to use R point or initial level for the return level in the final sequence of the canned cycle can be selected.

Command format

G98 ;

G99 ;

G98

G99

:Initial level return

:R point level return


The relation of the G98/G99 mode and No. of repetition designation is as shown below.

No. of hole drilling

Only one execution

Program example

G81X100.

Y100.

Z

−

50.

R25.

F1000;

G98

At power ON, at cancel with M02, M30, and reset button

Initial point

R point

G99

Initial point

R point

Initial level return is executed.

R point level return is executed.

Second and following executions

G81X100.

Y100.

Z

−

50.

R25.

L5F1000;

First time

Second time

Final time

Initial level return is executed for all times.

First time

Second time

Final time


(Example 1)

G82 Zz

Xx

1

1

Rr

1

Pp

1

Yy

1

;

Ff

1

L0 ;

Record only the hold machining data

(Do not execute)

Execute hole drilling operation with

G82 mode

The No. of canned cycle repetitions is designated with L. If L1 is designated or L not designated, the canned cycle will be executed once. The setting range is 1 to 9999.

If L0 is commanded, only the hole machining data will be recorded.

G8

∆

(7

∆

) Xx

1

Yy

1

Zz

1

Rr

1

Pp

1

Qq

1

Ff

1

Ll

1

;

166



The ideology of the data differs between the absolute value mode (G90) and incremental value mode (G91) as shown below.

R point

R

Z

Z axis absolute value zero point

R point

R

Z

Absolute value mode (G90) Incremental value mode (G91)

Designate a command value with a symbol for X, Y and Z. R indicates the coordinate value from the zero point in the absolute value mode, so a symbol must always be added. However, in the incremental value the symbol will be ignored and will be viewed as the same symbol as for Z. Note that the symbols will be viewed in reverse for G87.

The hole machining data is held as shown below in the canned cycle. The hole machining data is canceled when the G80 command or G commands (G00, G01, G02, G03, G2.1, G3.1, G33) in the

01 group are reached.

(Example 2)

N001 G81 Xx

1

Yy

1

Zz

1

Rr

1

Ff

1

;

N002 G81 ;

N003 Xx

2

Yy

2

;

N004 M22 ;

N005 G04 Xx

3

;

N006 G92 Xx

4

Yy

4

;

N007 G28 (G30) Z0 ;

N008 ;

Only selection of canned cycle sequence

Change of positioning point, and execution of canned cycle

Execution of only M22

Execution of only dwell

Execution of only coordinate system setting

Execution of only reference point (zero point) return

No work

N009 G99 Zz

2

Rr

2

Ff

2

L0 ; Execution of only hole machining data recording

N010 Xx

5

Yy

5

Ll

5

; Change of positioning point, and execution of R point return canned cycle for I

5

times

N011 G98 Xx

6

Yy

6

Zz

6

Rr

6

; Change of positioning point, and execution of canned cycle

N012 Ww

1

; Execute W axis according to 01 group modal before N001, and then execute canned cycle

13.1.3 Setting of workpiece coordinates in canned cycle mode

The designated axis moves with the workpiece coordinate system set for the axis.

The Z axis is valid after the R point positioning after positioning or from Z axis movement.

(Note)

When the workpiece coordinates are changed over for address Z and R, re-program even if the values are the same.

(Example)

G54 Xx

1

Yy

1

Zz

1

;

G81 Xx

2

Yy

2

Zz

2

Rr

2

;

G55 Xx

3

Yy

3

Zz

2

Rr

2

; Re-command even if Z and R are the same as the previous value.

Xx

4

Yy

4

;

Xx

5

Yy

5

;

167


13.2 Special canned cycle

13.2 Special canned cycle; G34, G35, G36, G37.1


The special canned cycle is used with the standard canned cycle. Before using the special canned cycle, program the canned cycle sequence selection G code and hole machining data to record the hole machining data. (If there is no positioning data, the canned cycle will not be executed, and only the data will be recorded.)

Even after the special canned cycle is executed, the recorded standard canned cycled will be held until canceled.

If the special canned cycle is designated when not in the canned cycle mode, only positioning will be executed, and the hole drilling operation will not be done.

Bolt hole circle (G34)

G34 X x

1

Y y

1

I r J

θ

K n ;

X, Y :Positioning of bolt hole cycle center. This will be affected by G90/G91.

I :Radius r of the circle. The unit follows the input setting unit, and is given with a positive number.

J :Angle

(The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001

°

.)

K :No. of holes n to be drilled. 1 to 9999 can be designated, but 0 cannot be designated. When the value is positive, positioning will take place in the CCW direction, and when negative, will take place in the CW direction. If 0 is designated, the alarm P221 Special Canned Holes Zero will occur.

Drilling of n obtained by dividing the circumference by n will start at point created by the Z axis and angle

θ

. The circumference is that of the radius R centering on the coordinates designated with XX and Y. The hole drilling operation at each hole will hold the drilling data for the standard canned cycle such as G81.

The movement between hole positions will all be done in the G00 mode. G34 will not hold the data even when the command is completed.

(Example)

When input setting unit is 0.001mm

N001 G91 ;

N002 G81 Z

−

10000 R5000 L0 F200 ;

N003 G90 G34 X200000 Y100000 I100000 J20000 K6 ;

N004 G80 ; ............... (Cancel of G81)

N005 G90 G0 X500000 Y100000 ; x

1

=200mm n = 6 holes

20

°

I=100mm y

1

=100mm

(500mm, 100mm)

Position before

G34 is executed

N005 G0 command

As shown in the example, the tool position after the G34 command is completed is over the final hole. When moving to the next position, the coordinate value must be calculated to issue the command with an incremental value. Thus, use of the absolute value mode is handy.

168


Line at angle (G35)


G35 X x1 Y y1 I d J

θ

K n ;

X, Y :Designation of start point coordinates. This will be affected by G90/G91.

I :Interval d. The unit follows the input setting unit. If d is negative, the drilling will take place in the direction symmetrical to the point that is the center of the start point.

K

(The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001

°

.)

:No. of holes n to be drilled. 1 to 9999 can be designated, and the start point is included.

Using the position designated by X and Y as the start point, the Zn holes will be drilled with interval d in the direction created by X axis and angle

θ

. The hole drilling operation at each hole position will be determined by the standard canned cycle, so the hole drilling data (hole machining mode and hole machining data) must be held beforehand. The movement between hole positions will all be done in the G00 mode. G35 will not hold the data even when the command is completed.

(Example)


G91 ;

G81 Z

−

10000 R5000 L0 F100 ;

G35 X200000 Y100000 I100000 J30000 K5 ; d=100mm n = 5 holes

θ

=30

° y

1

=100mm x

1

=200mm

Position before

G35 is executed

(Note 1)

If the K command is K0 or if there is no K command, the program error (P221) will occur.

(Note 2)

If the K value is more than four digits, the last four digits will be valid.

(Note 3)

If a group 0 G command is issued in the same block as the G35 command, the command issued later is the priority.

(Example)

G35 G28 Xx

1

Yy

1

Ii

1

Jj

1

Kk

1

;

G35 is ignored G 28 is executed as Xx1 Yy1

(Note 4)

If there is a G72 to G89 command in the same block as the G35 command, the canned cycle will be ignored, and the G35 command will be executed.

169


Arc (G36)


G36 X x1 Y y1 I r J

θ

P

∆θ

K n ;

X, Y :Center coordinates of arc. This will be affected by G90/G91.

I :Radius r of arc. The unit follows the input setting unit, and is given with a positive

No.

K direction, and in the CW direction when negative. (The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001

°

.)

:No. of holes n to be drilled. 1 to 9999 can be designated.

The n holes aligned at the angle interval

∆θ

will be drilled starting at point created by the X axis and angle

θ

. The circumference is that of the radius R centering on the coordinates designated with XX and Y. As with the bolt hole circle, the hole drilling operation at each hole will depend on the standard canned cycle.

The movement between hole positions will all be done in the G00 mode. G36 will not hold the data even when the command is completed.

(Example)

point position will be the degree class. If there is no decimal point, the unit will be

0.001

°

.)


N001 G91 ;

N002 G81 Z

−

10000 R5000 F100 ;

N003 G36 X300000 Y100000 I300000 J10000 P15000 K6 ; n = 6 holes

∆

θ

=

15

°

θ

=10

°

Position before

G36 is executed y

1

=100mm x

1

=300mm

170


Grid (G37.1)


G37.1 X x1 Y y1 I Dx P nx J Dy K ny ;

X, Y :Designation of start point coordinates. This will be affected by G90/G91.

I :Interval Dx of the X axis. The unit will follow the input setting unit. If Dx is positive, the interval will be in the forward direction looking from the start point, and when negative, will be in the reverse direction looking from the start point.

P

J

:No. of holes nx in the X axis direction. The setting range is 1 to 9999.

:Interval Dy of the Y axis. The unit will follow the input setting unit. If Dy is positive, the interval will be in the forward direction looking from the start point, and when

K negative, will be in the reverse direction looking from the start point.

:No. of holes ny in the Y axis direction. The setting range is 1 to 9999.

The nx points on a grid are drilled with an interval

∆ x parallel to the X axis, starting at the position designated with X, Y. The drilling operation at each hole position will depend on the standard canned cycle, so the hole drilling data (hole machining mode and hole machining data) must be held beforehand.

The movement between hole positions will all be done in the G00 mode. G37.1 will not hold the data even when the command is completed.

(Example)


G91 ;

G81 Z

−

10000 R5000 F20 ;

G37.1 X300000 Y

−

100000 I50000 P10 J100000 K8 ;

Position before

G37 is executed y

1

=100mm ny = 8 holes

∆ y=

100mm

∆ x=50mm x

1

=300mm nx = 10 holes

(Note 1)

If the P and K commands are P0 or K0, or if there is no P or K command, the program error "P221" will occur.

If the P or K value is more than four digits, the last four digits will be valid.

(Note 2)

If an address other than G, L, N, X, Y, I, P, J, K, F, M, S or B is programmed in the same block as the G37.1 command, that address will be ignored.

(Example)

G37.1 Xx

1

Yy

1

Ii

1

Pp

1

Jj

1

Kk

1

Qq

1

;

Ignore

(Note 3)

If a group 0 G command is issued in the same block as the G37.1 command, the command issued later is the priority.

(Note 4)

If there is a G72 to G89 command in the same block as the G37.1 command, the canned cycle will be ignored, and the G37.1 command will be executed.

171


13.3 Subprogram control

13.3 Subprogram control; M98, M99

13.3.1 Calling subprogram with M98 and M99 commands


Fixed sequences or repeatedly used patterns can be stored in the memory as subprograms which can then be called from the main program when required. M98 serves to call subprograms and

M99 serves to return operation from the subprogram to the main program. Furthermore, it is possible to call other subprograms from particular subprograms and the nesting depth can include as many as 8 levels.

Main program

O0010 ;

M98 P1000 ;

M02 ;

Subprogram Subprogram Subprogram Subprogram

M98 P1200

H20 ;

M99 ;

; O1200 O2000 ;

N20 ;

M98 P2000 ;

N60 ;

M99 ;

M98 P2500 ;

M99 P60 ; M99 ;

(Level 1) (Level 2)

Nesting depth

(Level 3) (Level 4)

The table below shows the functions which can be executed by adding and combining subprogram control functions and canned cycle functions.

1. Subprogram control

2. Canned cycles

Case 1

No

No

Case 2

Yes

No

Case 3

Yes

Yes

Case 4

No

Yes

Function

1. Memory operation

2. Subprogram call

3. Subprogram variable designation

(Note 2)

4. Subprogram nesting level call (Note 3)

5. Canned cycles

6. Canned cycle subprogram editing

(Note 1)

" " denotes function which can be used and " " a function which cannot be used.

(Note 2)

Variables cannot be transferred with the M98 command but variable commands in subprograms can be used provided that the variable command specifications are available.

(Note 3)

A maximum of 8 nesting levels can be possible.

172


Command format


Subprogram call

M98 P H L ;

P

H

L

:Program number of subprogram to be called (own program if omitted)

P can only be omitted during memory operation and MDI operation.

(Numerical value with up to 8 digits)

:Sequence number in subprogram to be called (head block if omitted)

(Numerical value with up to 5 digits)

:Number of subprogram repetitions (When omitted, this is interpreted at

L1, and is not excuted when L0)

(1 to 9999 with numerical value up to 4 digits)

For instance

M98 P1 L3 ; is equivalent to the following:

M98 P1 ;

M98 P1 ;

M98 P1 ;

Return to main program from subprogram

M99 P H Q R L ;

M99 Subprogram return command

P_

H_

Sequence number of return destination (return to the block that follows the calling block if omitted)

Program number of return destination (return to the main program at calling if omitted)

Q_

R_

L_

Sequence number to start searching of return destination (the block that follows the calling block will be handled as the search start position if omitted)

Sequence number to finish searching of return destination (the block that precedes the calling block will be handled as the search finish position if omitted)

Number of times after repetition number has been changed ("-1" if omitted)

Creating and entering subprograms

Subprograms have the same format as machining programs for normal memory operation except that the subprogram completion instruction M99 (P__) is entered as an independent block at the last block.

O

∆∆∆∆∆∆∆∆

; Program number as subprogram

................................ ;

................................ ;

:

:

; Main body of subprogram

................................ ;

M99 ; Subprogram return command

% (EOR) Entry completion code

(1) The above program is entered by editing operations at the setting and display unit. For further details, refer to the section on program editing in the Control Instructions.

173



(2) Only those subprogram numbers ranging from 1 through 99999999 designated by the optional specifications can be used.

(3) No distinction between main programs and subprograms is made since they are entered in the sequence in which they were read. This means that main programs and subprograms should not be given the same numbers. (If they are, error "E11" appears during entry.)

Registration example

;

O ;

................................ ;

:

M99 ;

%

O

∆∆∆∆

;

................................ ;

:

M99 ;

%

O * * * * ;

................................ ;

:

M99 ;

%

(4) Main programs can be entered in the memory or program by MDI operation but subprograms must be entered in the memory.

(5) Besides the M98 command, subprogram nesting is subject to the following commands:

• G65 Macro call

• G66 Modal call

• G66.1 Modal call

• G code call

• Miscellaneous function call (M, S, T, etc.)

• Macro interrupt

• MDI interrupt

• Automatic tool length measurement

• Multi-step skip function

(6) Subprogram nesting is not subject to the following commands which can be called even beyond the 8th nesting level.

• Canned cycles

(7) When the subprogram is to be repeatedly used, it will be repeatedly executed for l

1

times provided that "M98 Pp

1

Ll

1

;" is programmed.

174




When there are 3 subprogram calls (known as 3 nesting levels)

Main program Sub program 1 Sub program 2 Sub program 3

M98P1;

M02;

(1)

(1)'

O1;

M98P10;

M99;

(2)

(2)'

O10;

M98P20;

M99;

(3)

(3)'

O20;

M99;

Sequence of execution : (1)

→

(2)

→

(3)

→

(3)'

→

(2)'

→

(1)'

(1) For nesting, the M98 and M99 commands should always be paired off on a 1:1 basis, (1)' for

(1), (2)' for (2), etc.

(2) Modal information can be rewritten according to the execution sequence without distinction between main programs and subprograms. This means that after calling a subprogram, attention must be paid to the modal data status when programming.

Example of program 2

The M98H__; M99P__; commands designate the sequence numbers in a program with a call instruction.

For M98H__ ;

M98H3;

N3___;

M99;

For M99P__ ;

N100___;

M98P123;

N200_;

N300___;

N400___;

O123;

M99P200;

175



Precautions

(1) Program error (P232) results when the designated program number (P) is not located.

(2) Single block stop does not occur with the M98P__; M99; block. If any address except O, N, P,

L or H is used, single block stop can be executed. (With X100. M98 P100;, operation branches to O100 after X100. Is executed.)

(3) When M99 is commanded by the main program, operation returns to the head. (This is same for MDI.)

(4) Operation can branch from BTR operation to a subprogram by M98P__ but the sequence number of the return destination cannot be designated with M99P__;, (P__ is ignored.)

(5) Bear in mind that the search operation will take time when the sequence number is designated by M99P__; .

176


13.4 Variable commands



Programming can be endowed with flexibility and general-purpose capabilities by designating variables, instead of giving direct numerical values to particular addresses in a program, and by assigning the values of those variables as required when executing a program.

Command format

#

∆∆∆

= or #

∆∆∆

= [formula]


(1) Variable

Example

(a) #m

(b) # [f] m = value consisting of 0 to 9 f = one of the following in the formula

#100

# [-#120]

Numerical value m

Variable

Formula operator formula

−

(minus) formula

[Formula] function [formula]

123

#543

#110+#119

-#120

[#119]

SIN [#110]

(Note 1)

The 4 standard operators are +,

−

,

∗

and /.

(Note 2)

Functions cannot be used unless the user macro specifications are available.

(Note 3)

Error "P241" results when a variable number is negative.

(Note 4)

Examples of incorrect variable expressions are given below.

Incorrect

#6/2

#- -5

#- [#1]

Correct

→

#[6/2] (Note that expression such as "#6/2" is regarded as

"[#6] /2")

→

#[- [-5]]

→

#[-#1]

177



(2) Type of variables

The following table gives the types of variables.

Type of variable

Common variables

No. of variable sets option

50 + 50 × number of part systems

Common variables

1

(Common to part systems)

#500 to #549

(50 sets)

Number

Common variables 2

(Provided per part system)

#100 to #149

(50 sets)

Function

Can be used in common throughout main, sub and macro programs.



#500 to #599

(100 sets)

#500 to #699

(200 sets)

#100 to #199

(100 sets)

#100 to #199

(100 sets)

Local variables

System variables

Canned cycle variables

1 to 33

1000 to

1 to 32

Can be used for local variables in macro programs.

Application is fixed by system.

Local variables in canned cycle programs.

(Note 1)

All common variables are retained even when the power is switched off.

(Note 2)

When the power is turned off or reset, the common variables can be set to <null> by setting the parameter "#1128 RstVC1", "#1129 PwrVC1".

(Note 3)

The common variables are divided into the following two types.

Common variables 1 : Used in common through all part systems

Common variables 2 : Used in common in the programs of the part system

178



Variables can be used for all addresses except O, N and / (slash).

(a) When the variable value is used directly:

X#1 ...................................Value of #1 is used as the X value.

(b) When the complement of the variable value is used:

X - #2 ................................ Value with the #2 sign changed is used as the X value.

(c) When defining variables:

#3 = #5 .............................Variable #3 uses the equivalent value of variable #5.

#1 = 1000 .........................Variable #1 uses the equivalent value 1000 (which is treated as

1000.)

(d) When defining variables:

#1 = #3 + #2 – 100 ...........The value of the arithmetic result of #3 + #2 - 100. Is used as the

#1 value.

X[#1 + #3 + 1000]............. The value of the arithmetic result of #1 + #3 + 1000. Is used as the X value.

(Note 1)

A variable cannot be defined in the same block as an address. It must be defined in a separate block.

Incorrect Correct

X#1 = #3 + 100;

→

#1 = #3 + 100;

X#1;

(Note 2)

Up to five sets of square parentheses [ ] may be used.

#543 =

−

[[[[[#120]/2+15.]

∗

3

−

#100]/#520 + #125 + #128]

∗

#130 + #132]

(Note 3)

There are no restrictions on the number of characters and number of variables for variable definition.

(Note 4)

The variable values should be within a range form 0 to

±

99999999.

If this range is exceeded, the arithmetic operations may not be conducted properly.

(Note 5)

The variable definitions are valid from the moment that the variables are actually defined.

#1 = 100 ;.............................. #1 = 100 Valid from the next command

#1 = 200 #2 = #1 + 200 ; ..... #1 = 200, #2 = 400 Valid from the next command

#3 = #1 + 300 ; ..................... #3 = 500 Valid from the next command

(Note 6)

Variable quotations are always regarded as having a decimal point at the end.

When #100 = 10, then X#100 ; is treated as X10.

179


13.5 User macro specifications


13.5.1 User macro commands ; G65, G66, G66.1, G67


By combining the user macros with variable commands, it is possible to use macro program call, arithmetic operation, data input/output with PLC, control, decision, branch and many other instructions for measurement and other such applications.

O Main program O Macro program

....... ; ....... ;

Macro call instruction

M30 ; M99 ;

Macro programs use variables, arithmetic instructions and control instructions to create subprograms which function to provide special-purpose control.

These special-purpose control functions (macro programs) are called by the macro call instructions exactly when required from the main program.

The following G codes are available for the macro call commands.

G code

G65

G66

G66.1

G67

User macro Simple call

User macro Modal call A (called after the movement command)

User macro Modal call B (called after the every block)

User macro Modal call cancel

Function


(1) When the G66 (or 66.1) command is entered, the specified user macro subprogram will be called after each block has been executed (or after the movement command in the block) with the movement commands has been executed until the G67 (cancel) command is entered.

(2) The G66 (or G66.1) and G67 commands must be paired in the same program.

180



13.5.2 Macro call instruction


Included among the macro call commands are the simple calls which apply only to the instructed block and also modal calls (types A and B) which apply to each block in the call modal.

Simple macro calls

Main program

G65Pp1L

l

1 <argument>;

To subprogram

Subprogram (O o1

)

O o1

M99

To main program

M99 is used to conclude the user macro subprogram.

Format

G65 P___ L___ <argument> ;

P___

L___

: Program No.

: No. of repetitions

When the <argument> must be transferred as a local variable to a user macro subprogram, the actual value should be designated after the address.

Regardless of the address, a sign and decimal point can be used in the argument. There are 2 ways in which arguments are designated.

181



(1) Argument designation I

Format : A__ B__ C__ • • • • X__ Y__ Z__

Detailed description

(a) Arguments can be designated using any address except G, L, N, O and P.

(b) Except for I, J and K, there is no need for designation in alphabetical order.

(c) I, J and K must be designated in alphabetical order.

I__ J__ K__ ................... Correct

J__ I__ K__ ................... Incorrect

(d) Address which do not need to be designated can be omitted.

(e) The following table shows the correspondence between the addresses which can be designated by argument designation I and the variable numbers in the user macro main body.

Address and variable number correspondence

Argument designation I address

Variable in macro

Call instructions and usable address

G65, G66

A #1

B #2

C #3

D #7

E #8

F #9

G66.1

G #10

∗

H #11

I #4

J #5

K #6

L #12

M #13

N #14

∗

∗

O #15

P #16

∗

Q #17

R #18

S #19

T #20

U #21

V #22

W #23

X #24

Y #25

Z #26

: Can be used.

: Cannot be used.

∗

: Can be used while G66.1 command is modal.

182



(2) Argument designation II

Format : A__ B__ C__ I__ J__ K__ I__ J__ K__• • • •


(a) In addition to address A, B and C, up to 10 groups of arguments with I, J, K serving as 1 group can be designated.

(b) When the same address is duplicated, designate the addresses in the specified order.

(c) Addresses which do not need to be designated can be omitted.

(d) The following table shows the correspondence between the addresses which can be designated by argument designation II and the variable numbers in the user macro main body.

Argument designation II

Variable within macro

Argument designation II

Variable within macro address address

A # J5 #17

B # K5 #18

C # I6 #19

I1 # J6 #20

J1 # K6 #21

I7 #22

I2 # J7 #23

J2 # K7 #24

I8 #25

I3 #10 J8 #26

J3 #11 K8 #27

K3 #12 I9 #28

I4 #13 J9 #29

J4 #14 K9 #30

K4 #15 I10 #31

I5 #16 J10 #32

K10 #33

(Note 1)

The numbers 1 through 10 accompanying I, J and K denote the sequence of the commanded groups and they are not required for the actual instructions.

(3) Using arguments designations I and II together

If addresses corresponding to the same variable are commanded when both types I and II are used to designate arguments, the latter address is valid.

(Example 1)

Call instruction G65 A1.1 B-2.2 D3.3 I4.4 I7.7 ;

Variable

#1 : 1.1

#2 : –2.2

#4 : 4.4

#5 :

#6 :

#7 : 3.3 7.7

In the above example, the last I7.7 argument is valid when both arguments D3.3 and

I7.7 are commanded for the #7 variable.

183



Modal call A (called after the movement command)

Main program

G65Pp1L

G67

l

1 <argument>;

To subprogram

Subprogram

O o1

M99

To main program

To subprogram

When the block with a movement command is commanded between G66 and G67, the movement command is first executed and then the designated user macro subprogram is executed. The number of times the subprogram is executed is l

1 times with each call.

The <argument> is the same as for a simple call.

Format

G66 P___ L___ <argument> ;

P___ : Program No.

L___ : No. of repetitions


(1) When the G66 command is entered, the specified user macro subprogram will be called after the movement command in the block with the movement commands has been executed until the G67 (cancel) command is entered.

(2) The G66 and G67 commands must be paired in the same program.

A program error will result when G67 is issued without the G66 command.

(Example)

Drill cycle

N1 G90 G54 G0 X0Y 0Z0;

N2 G91 G00 X-50.Y-50. Z-200.;

N3 G66 P9010 R-10. Z-30.F100;

N4 X-50.Y-50.;

N5 X-50.;

N6 G67;

To subprogram af ter axis command execution

To subprogram af ter axis command execution

To main program

O 9010

N10 G00 Z #18 M0;

N20 G09 G01 Z #26 F#9;

N30 G00 Z- [#18+ #26];

M99;

X

-150. -100. -50.

N2

N3

N4

N5

W

N1

-50.

-100.

Y

N10

N20

Argument R

N30

Argument Z

Argument F

(Note 1)

After the axis command is executed in the main program, the subprogram is executed.

(Note 2)

The subprogram is not executed in the blocks following G67.

184


Modal call B (called after the every block)


The specified user macro subprogram is called unconditionally for each command block which is assigned between G66.1 and G67 and the subprogram is executed the number of times designated with “L” address.

Format

G66.1 P___ L___ <argument> ;

P___ : Program No.

L___ : No. of repetitions


(1) In the G66.1 mode, everything except the O, N and G codes in the various command blocks which are read are handled as the argument without being executed. Any G code designated last or any N code commanded after anything except O and N will function as the argument.

(2) The same applies as when G65P__ is assigned at the head of a block for all significant blocks in the G66.1 mode.

(Example 1)

N100 G01 G90 X100. Y200. F400 R1000; in the G66.1 P1000; mode is the same as: N100 G65 P1000 G01 G90 X100. Y200. F400 R1000;

(Note 1)

The Call is performed even in the G66.1 command block in the G66.1 mode and the correspondence between the argument address and the variable number is the same as for G65 (simple call).

(3) The range of the G and N command values which can be used anew as variables in the G66.1 mode is subject to the restrictions applying to values as normal NC command values.

(4) Program number O, sequence numbers N and modal G codes are updated as modal information.

G code macro call

User macro subprogram with prescribed program numbers can be called merely by issuing the G code command.

Format

G

∗∗

<argument> ;

G

∗∗

:G code for macro call


(1) The above instruction functions in the same way as the instructions below, and parameters are set for each G code to determine the correspondence with the instructions. a.

∆∆∆∆

; b.

∆∆∆∆∆

<argument> ;

G66P <argument> ; d.

∆∆∆∆∆

<argument> ;

When the parameters corresponding to c and d above are set, issue the cancel command

(G67) either in the user macro or after the call code has been commanded so as to cancel the modal call.

185



(

2) The correspondence between the "XX" which conducts the macro call and the program number P

∆∆∆∆

of the macro to be called is set by parameter.

(3) Up to 10 G codes from G100 to G255 can be used with this instruction. (G01 to 99 can also be used with parameter "#1081 Gmac_P").

(Note 1)

G101 to G110 and G200 to G202 are user macro I codes, but if the parameters are set as the G code call codes, the G code call will be the priority, and these codes cannot be used for user macro I.

(4) These commands cannot be issued during a user macro subprogram which has been called by a G code.

Program example

G16X100. Y100. Z100. F500 ;

O9016

M99 ;

Miscellaneous command macro call (for M, S, T, B code macro call)

The user macro subprogram of the specified program number can be called merely by issuing an

M (or S, T, B) code. (Only entered codes apply for M but all S, T and B codes apply.)

Format

M

∗∗

; (or S

∗∗

;, T

∗∗

;, B

∗∗

;)

M

∗∗

M code for macro call (or S, T, B code)


(1) The above instruction functions in the same way as the instructions below, and parameters are set for each M code to determine the correspondence with the instructions. (Same for S, T and B codes)

a : M98 P

∆∆∆∆

;

b : G65 P

∆∆∆∆

M

∗∗

;

c : G66 P

∆∆∆∆

M

∗∗

;

d : G66. 1P

∆∆∆∆

M

∗∗

;

M98, M

∗∗

are not output

When the parameters corresponding to c and d above are set, issue the cancel command

(G67) either in the user macro or after the call code has been commanded so as to cancel the modal call.

(2) The correspondence between the "M

∗∗

" which conducts the macro call and the program number P

∆∆∆∆

of the macro to be called is set by parameter. Up to 10 M codes from M00 to

M95 can be entered. Note that the codes to be registered are the codes basically required for the machine, and codes excluding M0, M1, M2, M30 and M96 to M99.

(3) As with M98, it is displayed on the screen display of the setting and display unit but the M codes and MF are not output.

186



(4) Even if the miscellaneous command entered above is issued during a user macro subprogram called by the M code, macro call will not result and it will be handled as an ordinary miscellaneous command.

(5) All S, T and B codes call the subprograms in the prescribed program numbers of the corresponding S, T and B functions.

(6) A maximum of 10 M codes can be set. However when not setting all 10. Set the parameters as shown below.

[ MACRO ]

<Code> <Type> <Program No.>

M [01] 20

M [02] 21

0

0

8000

8001

M [03] 9999

M [04] 9999

0 199999999

0 199999999

M [05] 9999 0 199999999

: : :

: : :

M [10] 9999 0 199999999

Setting to call O8000 with type 0

(M98 type) during M20 command

Setting to call O8001 with type 0

(M98 type) during M21 command

Set parameters not being used as shown on left.

Differences between M98 and G65 commands

(1) The argument can be designated for G65 but not for M98.

(2) The sequence number can be designated for M98 but no for G65, G66 and G66.1.

(3) M98 executes a subprogram after all the commands except M, P, H and L in the M98 block have been executed, but G65 branches to the subprogram without any further operation.

(4) When any address except O, N, P, H or L is included in the M98 block, single block stop results. This is not the case with G65.

(5) The level of the M98 local variables is fixed but it can be varied in accordance with the nesting depth for G65. (#1, for instance, has the same significance either before or after M98 but a different significance in each case with G65.)

(6) The M98 nesting depth extends up to 8 levels in combination with G65, G66 and G66.1. The

G65 nesting depth extends up to only 4 levels in combination with G66 and G66.1.

Macro call command nesting depth

Up to 4 nesting levels are available for macro subprogram calls based on simple call or modal call.

The argument with a macro call instruction is valid only on the called macro level. Since the nesting depth for macro calls extends up to 4 levels, the argument can be used as a local variable for the program with each respective macro call.

(Note 1)

When a G65, G66, G66.1 G code macro call or miscellaneous command macro call is conducted, this is regarded as nesting level 1 and the level of the local variables is also incremented by one.

(Note 2)

The designated user macro subprogram is called every time the movement command is executed with modal call A. However, when the G66 command has been duplicated, the next user macro subprogram is called every time an axis is moved even with movement commands in the macro.

User macro subprograms are called in sequence from the subprogram commanded last.

187



(Example 1)

Main program

G66Pp

1

;

(p

1 call)

Zz1 ;

Macro p

1

After Z1 execution

G66Pp

2

;

(p

2 call)

Zz2 ;

Macro p

2

After Z2 execution

G67 ;

(p

2 cancel)

Zz3 ;

Macro p

1

After Z3 execution

G67 ;

(p

1 cancel)

Zz4 ;

Zz5 ;

13.5.3 Variables


x

1

User macro operation y

1 x

2

M99 x

1 x

1

Macro p

1 y

1 y

1

Macro p

1 x

2 x

2

M99

Macro p

1

M99

Both the variable specifications and user macro specifications are required for the variables which are used with the user macros.

The offset amounts of the local, common and system variables among the variables for this

MELDAS NC system except #33 are retained even when the unit's power is switched off.

(Common variables can also be cleared by parameter "#1129 PwrVC1".)

Use of multiple variables

When the user macro specifications applied, variable numbers can be turned into variables

(multiple use of variables) or replaced by <formula>. Only one of the four basic arithmetic rule (+, –,

×

,

÷

) operations can be conducted with <formula>.

(Example 1)

Multiple use of variables

#1 = 10 #10 = 20 #20 = 30 ;

#5 = #[#[#1]] ;

#[#[#1]] = #[#10] from #1 = 10.

#[#10] = #20 from #10 = 20.

Therefore, #5 = #20 or #5 = 30.

#1 = 20 #10 = 20 #20 = 30 #5 #[#[#1]] = #[#10] from #1 = 10.

= 1000 ;

#[#[#1]] = #5 ;

#[#10] = #20 from #10 = 20.

Therefore, #20 = #5 or #20 = 1000.

(Example 2)

Example of multiple designation of variables

#10 = 5

In which case ##10 = 100 ; #5 =

100

<Formula>##10 = 100; is handled in the same manner as # [#10] = 100.

188



(Example 3)

Replacing variable numbers with <formula>

#10 = 5 ;

#[#10 + 1] = 1000 ;

#[#10

#[#10

∗

3] = 100 ;

#[#10/2]

In which case, #6 = 1000.

In which case, #4 =

−

(fraction rounded up)

1000.

In which case, #15 = 100.

In which case, #3 =

−

100.

Undefined variables

Variables applying with the user macro specifications such as variables which have not been used even once after the power was switched on or local variables not quoted by the G65, G66 or G66.1 commands can be used as <vacant>. Also, variables can forcibly be set to <vacant>. Variable #0 is always used as the <vacant> variable and cannot be defined in the left-side member.

#1 = #0 ; ................... #1 = <vacant>

#2 = #0 + 1 ;............. #2 = 1

#3 = 1 + #0 ;............. #3 = 1

#4 = #0

∗

10 ; ............. #4 = 0

#5 = #0 + #0 ;........... #5 = 0

It should be borne in mind that <vacant> in an arithmetic expression is handled in the same way as 0.

<Vacant> + <Vacant> = 0

<Vacant> + <Constant> = Constant

<Constant> + <Vacant> = Constant

When undefined variables only are quoted, they are ignored up to the address.

When #1 = <Vacant>

G0 X#1 Y1000 ; ............... Equivalent to G0 Y1000 ;

G0 X#1 + 10 Y1000 ; ....... Equivalent to G0 X10 Y1000 ;

<Vacant> and 0 are not equivalent for EQ and NE only. (#0 means <vacant>.)

When #101 = <Vacant>

#101 EQ #0

<Vacant> = <Vacant> established

#101 NE 0

<Vacant>

≠

0 established

#101 GE #0

<Vacant>

≥

<Vacant> established

#101 GT 0

<Vacant> > 0 not established

#101 LE #0

<Vacant>

≤


#101 LT 0

<Vacant> < 0 not established

When #101 = 0

#101 EQ #0

0 = <Vacant> not established

#101 NE 0

0

≠

0 not established

#101 GE #0

0

≥


#101 GT 0

0 > 0 not established

#101 LE #0

0

≤


#101 LT 0

0 < 0 not established

(Note 1)

EQ and NE should be used only for integers. For comparison of numeric values with decimals, GE, GT, LE, and LT should be used.

189



13.5.4 Types of variables

Common variables

Common variables can be used commonly from any position. Number of the common variables sets depends on the specifications. Refer to "13.4 Variable commands" for details.

Local variables (#1 to #33)

These can be defined as an <argument> when a macro subprogram is called or used locally within main programs and subprograms. They can be duplicated regardless of the relationship existing between macros (up to 4 levels).

G65 Pp

1

Ll

1

<argument> ;

P

1

l

1

: Program number

: Number of repetitions

The <argument> is assumed to be Aa1 Bb1 Cc1 .............. Zz1.

The following table shows the correspondences between the addresses designated by

<argument> and the local variable numbers used in the user macro main bodies.

∗

∗

∗

∗

[Argument specification I]

Call command

G65

G66

G66.1

Argument address

Local variable number

Call command

G65

G66

G66.1

Argument address

Local variable number

A #1

B #2

C #3

D #7

E #8

F #9

Q #17

R #18

S #19

T #20

U #21

V #22

G #10

H #11

I #4

J #5

K #6

W #23

X #24

Y #25

Z #26

−

#27

L #12

−

M #13

−

#28

#29

N #14

−

O #15

−

P #16

−

−

#30

#31

#32

#33

" " in the above table denotes an argument address which cannot be used. However, provided that the G66.1 mode has been established, an argument address denoted by the asterisk can be added for use.

"

−

" denotes that a corresponding address is not available.

190



[Argument specification II]

Argument specification

II address


Argument specification II address


I6 #19

J6 #20

K6 #21

I7 #22

J7 #23

K7 #24

I3 #10

J3 #11

K3 #12

I4 #13

J4 #14

I8 #25

J8 #26

K8 #27

I9 #28

J9 #29

K9 #30

I10 #31

J10 #32

K4 #15

I5 #16

J5 #17

K5 #18

K10 #33

(Note 1)

Subscripts 1 to 10 for I, J, and K indicate the order of the specified command sets. They are not required to specify instructions.

(1) Local variables in subprograms can be defined by means of the <argument> designation during macro call.

Main program

G65 P9900 A60. S100. F800;

M02;

To subprogram

Subprogram (9900)

G91 G01 X [#19

∗

COS [#1] ]

Y [#19

∗

SIN [#1] ] F#9;

M99;

Refer to the local variables and control the movement, etc.

Local variables set by argument

Local variable data table

A(#1)= 60.000

F(#9)= 800

S(#19)= 100.000

191



(2) The local variables can be used freely in that subprogram.

Main program

Subprogram (1)

G65 P1 A100. B50. J10. F500;

Example of front surface milling

B

To subprogram

#30=FUP [#2/#5/2] ;

#5=#2/#30/2 ;

M98 H100 L#30 ;

X#1 ;

M99 ;

N100 G1 X#1 F#9 ;

Y#5 ;

X-#1 ;

Y#5 ;

M99 ;

The local variables can be changed in the subprogram.

J

A

Local variables set by argument

The local variables can be changed in the subprogram.

Local variable data table

A (#1) 100.000

B (#2) 50.000

F (#9) 500

J (#5) 10.000 8.333

(#30) 3

In the front surface milling example, argument J is programmed as the milling pitch 10.mm.

However, this is changed to 8.333mm to create an equal interval pitch.

The results of the No. of reciprocation data calculation is set in local variable #30.

192



(3) Local variables can be used independently on each of the macro call levels (4 levels).

Local variables are also provided independently for the main program (macro level 0).

Arguments cannot be used for the level 0 local variables.

Main (level 0)

#1=0.1 #2=0.2 #3=0.3;

G65 P1A1. B2. C3.;

M02;

O1 (macro level 1)

G65 P10A10. B20. C30.;

M99;

O10 (macro level 2)

G65 P100A100. B200.;

M99;

O100 (macro level 3)

M99;

Local variables (0)

#1 0.100

#2 0.200

#3 0.300

#32

Local variables (1)

A (#1) 1.000

B (#2) 2.000

C (#3) 3.000

D (#7)

Z(#26)

#32

Local variables (2)

A (#1) 10.000

B (#2) 20.000

C (#3) 30.000

D (#7)

Z(#26)

#32

Local variables (3)

A (#1) 100.000

B (#2) 200.000

C (#3)

Z(#26)

#32

The status of the local variables appear on the setting and display unit.

Refer to the Operation Manual for details.

193



Macro interface inputs (#1000 to #1035, #1200 to #1295) : PLC

→

NC

The status of the interface input signals can be ascertained by reading out the values of variable numbers #1000 to #1035, #1200 to #1295. A variable value which has been read out can be only one of 2 values: 1 or 0 (1: contact closed, 0: contact open). All the input signals from #1000 to

#1031 can be read at once by reading out the value of variable number #1032.

Similarly, the input signals #1200 to #1231, #1232 to #1263, and #1264 to #1295 can be read by reading the values of the variable numbers #1033 to #1035.

Variable numbers #1000 to #1035, #1200 to #1295 are for readout only, and cannot be placed in the left side member of their arithmetic formula. Input here refers to input to the control unit.

To use the macro interface function by part system, set the bit selection parameter "#6454/bit0".

Refer to (2) for the signals provided for each part system.

(1) Macro interface common to part systems (input)

System variable

No. of points

Interface input signal

System variable

No. of points


#1000

#1001

#1002

#1003

#1004

#1005

#1006

#1007

#1008

#1009

#1010

#1011

#1012

#1013

#1014

#1015

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

Register R24 bit 0

Register R24 bit 1

Register R24 bit 2

Register R24 bit 3

Register R24 bit 4

Register R24 bit 5

Register R24 bit 6

Register R24 bit 7

Register R24 bit 8

Register R24 bit 9

Register R24 bit 10

Register R24 bit 11

Register R24 bit 12

Register R24 bit 13

Register R24 bit 14

Register R24 bit 15

#1016

#1017

#1018

#1019

#1020

#1021

#1022

#1023

#1024

#1025

#1026

#1027

#1028

#1029

#1030

#1031

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

Register R25 bit 0

Register R25 bit 1

Register R25 bit 2

Register R25 bit 3

Register R25 bit 4

Register R25 bit 5

Register R25 bit 6

Register R25 bit 7

Register R25 bit 8

Register R25 bit 9

Register R25 bit 10

Register R25 bit 11

Register R25 bit 12

Register R25 bit 13

Register R25 bit 14

Register R25 bit 15

System variable

#1032

#1033

#1034

#1035

No. of points

32

32

32

32


Register R24, R25

Register R26, R27

Register R28, R29

Register R30, R31

194



System variable

#1200

#1201

#1202

#1203

#1204

#1205

#1206

#1207

#1208

#1209

#1210

#1211

#1212

#1213

#1214

#1215

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R26 bit 0

Register R26 bit 1

Register R26 bit 2

Register R26 bit 3

Register R26 bit 4

Register R26 bit 5

Register R26 bit 6

Register R26 bit 7

Register R26 bit 8

Register R26 bit 9

Register R26 bit 10

Register R26 bit 11

Register R26 bit 12

Register R26 bit 13

Register R26 bit 14

Register R26 bit 15

System variable

#1216

#1217

#1218

#1219

#1220

#1221

#1222

#1223

#1224

#1225

#1226

#1227

#1228

#1229

#1230

#1231

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R27 bit 0

Register R27 bit 1

Register R27 bit 2

Register R27 bit 3

Register R27 bit 4

Register R27 bit 5

Register R27 bit 6

Register R27 bit 7

Register R27 bit 8

Register R27 bit 9

Register R27 bit 10

Register R27 bit 11

Register R27 bit 12

Register R27 bit 13

Register R27 bit 14

Register R27 bit 15

System variable

#1232

#1233

#1234

#1235

#1236

#1237

#1238

#1239

#1240

#1241

#1242

#1243

#1244

#1245

#1246

#1247

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R28 bit 0

Register R28 bit 1

Register R28 bit 2

Register R28 bit 3

Register R28 bit 4

Register R28 bit 5

Register R28 bit 6

Register R28 bit 7

Register R28 bit 8

Register R28 bit 9

Register R28 bit 10

Register R28 bit 11

Register R28 bit 12

Register R28 bit 13

Register R28 bit 14

Register R28 bit 15

System variable

#1248

#1249

#1250

#1251

#1252

#1253

#1254

#1255

#1256

#1257

#1258

#1259

#1260

#1261

#1262

#1263

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R29 bit 0

Register R29 bit 1

Register R29 bit 2

Register R29 bit 3

Register R29 bit 4

Register R29 bit 5

Register R29 bit 6

Register R29 bit 7

Register R29 bit 8

Register R29 bit 9

Register R29 bit 10

Register R29 bit 11

Register R29 bit 12

Register R29 bit 13

Register R29 bit 14

Register R29 bit 15

195



System variable

#1264

#1265

#1266

#1267

#1268

#1269

#1270

#1271

#1272

#1273

#1274

#1275

#1276

#1277

#1278

#1279

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R30 bit 0

Register R30 bit 1

Register R30 bit 2

Register R30 bit 3

Register R30 bit 4

Register R30 bit 5

Register R30 bit 6

Register R30 bit 7

Register R30 bit 8

Register R30 bit 9

Register R30 bit 10

Register R30 bit 11

Register R30 bit 12

Register R30 bit 13

Register R30 bit 14

Register R30 bit 15

System variable

#1280

#1281

#1282

#1283

#1284

#1285

#1286

#1287

#1288

#1289

#1290

#1291

#1292

#1293

#1294

#1295

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R31 bit 0

Register R31 bit 1

Register R31 bit 2

Register R31 bit 3

Register R31 bit 4

Register R31 bit 5

Register R31 bit 6

Register R31 bit 7

Register R31 bit 8

Register R31 bit 9

Register R31 bit 10

Register R31 bit 11

Register R31 bit 12

Register R31 bit 13

Register R31 bit 14

Register R31 bit 15

196



(2) Macro interface by part system (input)

(Note)

As for the C64T system, the input/output signals used for this function are valid up to

3rd part system.

System variable

No. of Interface input signal points

$1 $2 $3 $4 $5 $6 $7

R970 R1070 R1170 R1270 R1370 R1470 R1570

#1000

#1001

#1002

#1003

#1004

#1005

#1006 bit0 bit0 bit1 bit1 bit2 bit2 bit3 bit3 bit4 bit4 bit5 bit5 bit6 bit6 bit0 bit1 bit2 bit3 bit4 bit5 bit6 bit0 bit1 bit2 bit3 bit4 bit5 bit6 bit0 bit0 bit0 bit1 bit1 bit1 bit2 bit2 bit2 bit3 bit3 bit3 bit4 bit4 bit4 bit5 bit5 bit5 bit6 bit6 bit6

#1007 bit7 bit7

#1008 bit8 bit8

#1009 bit9 bit9

#1010 1 bit10 bit10

#1011 1 bit11 bit11

#1012 1 bit12 bit12

#1013 1 bit13 bit13

#1014 1 bit14 bit14

#1015 1 bit15 bit15 bit7 bit8 bit9 bit10 bit11 bit12 bit13 bit14 bit15 bit7 bit8 bit9 bit10 bit11 bit12 bit13 bit14 bit15 bit7 bit7 bit7 bit8 bit8 bit8 bit9 bit9 bit9 bit10 bit10 bit10 bit11 bit11 bit11 bit12 bit12 bit12 bit13 bit13 bit13 bit14 bit14 bit14 bit15 bit15 bit15

System variable

No. of points

$1 $2


$3 $4 $5 $6 $7

R971 R1071 R1171 R1271 R1371 R1471 R1571

#1016 bit0 bit0 bit0 bit0 bit0 bit0 bit0

#1017

#1018

#1019

#1020 bit1 bit1 bit2 bit2 bit3 bit3 bit4 bit4 bit1 bit2 bit3 bit4 bit1 bit2 bit3 bit4 bit1 bit1 bit1 bit2 bit2 bit2 bit3 bit3 bit3 bit4 bit4 bit4

#1021 bit5 bit5

#1022 bit6 bit6

#1023 bit7 bit7

#1024 bit8 bit8

#1025 bit9 bit9 bit5 bit6 bit7 bit8 bit9 bit5 bit6 bit7 bit8 bit9 bit5 bit5 bit5 bit6 bit6 bit6 bit7 bit7 bit7 bit8 bit8 bit8 bit9 bit9 bit9

#1026 1 bit10 bit10

#1027 1 bit11 bit11

#1028 1 bit12 bit12

#1029 1 bit13 bit13

#1030 1 bit14 bit14

#1031 1 bit15 bit15 bit10 bit11 bit12 bit13 bit14 bit15 bit10 bit11 bit12 bit13 bit14 bit15 bit10 bit10 bit10 bit11 bit11 bit11 bit12 bit12 bit12 bit13 bit13 bit13 bit14 bit14 bit14 bit15 bit15 bit15

System variable

No. of points

$1

#1032 32

R970,

R971

#1033 32

R972,

R973

#1034 32

R974,

R975

#1035 32

R976,

R977

$2

R1070,

R1071

R1072,

R1073

R1074,

R1075

R1076,

R1077


$3 $4 $5

R1170,

R1171

R1172,

R1173

R1174,

R1175

R1176,

R1177

R1270,

R1271

R1272,

R1273

R1274,

R1275

R1276,

R1277

R1370,

R1371

R1372,

R1373

R1374,

R1375

R1376,

R1377

$6

R1470,

R1471

R1472,

R1473

R1474,

R1475

R1476,

R1477

$7

R1570,

R1571

R1572,

R1573

R1574,

R1575

R1576,

R1577

197



Macro interface outputs (#1100 to #1135, #1300 to #1395) : NC

→

PLC

The interface output signals can be sent by substituting values in variable numbers #1100 to #1135,

#1300 to #1395. An output signal can be only 0 or 1.

All the output signals from #1100 to #1131 can be sent at once by substituting a value in variable number #1132.

Similarly, the output signals #1300 to #1311, #1332 to #1363, and #1364 to #1395 can be sent by assigning values to the variable numbers #1133 to #1135. (2

0

~ 2

31

)

The status of the writing and output signals can be read in order to offset the #1100 to #1135,

#1300 to #1395 output signals. Output here refers to the output from the NC.

To use the macro interface function by part system, set the bit selection parameter "#6454/bit0".

Refer to (2) for the signals provided for each part system.

(1) Macro interface common to part systems (output)

System variable

#1100

#1101

#1102

#1103

#1104

#1105

#1106

#1107

#1108

#1109

#1110

#1111

#1112

#1113

#1114

#1115

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

Interface output signal

Register R124 bit 0

Register R124 bit 1

Register R124 bit 2

Register R124 bit 3

Register R124 bit 4

Register R124 bit 5

Register R124 bit 6

Register R124 bit 7

Register R124 bit 8

Register R124 bit 9

Register R124 bit 10






System variable

#1116

#1117

#1118

#1119

#1120

#1121

#1122

#1123

#1124

#1125

#1126

#1127

#1128

#1129

#1130

#1131

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R125 bit 0

Register R125 bit 1

Register R125 bit 2

Register R125 bit 3

Register R125 bit 4

Register R125 bit 5

Register R125 bit 6

Register R125 bit 7

Register R125 bit 8

Register R125 bit 9







System variable

#1132

#1133

#1134

#1135

No. of points

32

32

32

32


Register R124, R125

Register R126, R127

Register R128, R129

Register R130, R131

198



(Note 1)

(Note 2)

System variable

#1308

#1309

#1310

#1311

#1312

#1313

#1314

#1315

#1300

#1301

#1302

#1303

#1304

#1305

#1306

#1307

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

The last values of the system variables #1100 to #1135 sent are retained as 1 or 0.

(They are not cleared even with resetting.)

The following applies when any number except 1 or 0 is substituted into #1100 to

#1131.

<Vacant> is treated as 0.

Any number except 0 and <vacant> is treated as 1.

Any value less than 0.00000001 is indefinite.


Register R126 bit 0

Register R126 bit 1

Register R126 bit 2

Register R126 bit 3

Register R126 bit 4

Register R126 bit 5

Register R126 bit 6

Register R126 bit 7

Register R126 bit 8

Register R126 bit 9







System variable

#1316

#1317

#1318

#1319

#1320

#1321

#1322

#1323

#1324

#1325

#1326

#1327

#1328

#1329

#1330

#1331

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R127 bit 0

Register R127 bit 1

Register R127 bit 2

Register R127 bit 3

Register R127 bit 4

Register R127 bit 5

Register R127 bit 6

Register R127 bit 7

Register R127 bit 8

Register R127 bit 9







System variable

#1332

#1333

#1334

#1335

#1336

#1337

#1338

#1339

#1340

#1341

#1342

#1343

#1344

#1345

#1346

#1347

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R128 bit 0

Register R128 bit 1

Register R128 bit 2

Register R128 bit 3

Register R128 bit 4

Register R128 bit 5

Register R128 bit 6

Register R128 bit 7

Register R128 bit 8

Register R128 bit 9







System variable

#1348

#1349

#1350

#1351

#1352

#1353

#1354

#1355

#1356

#1357

#1358

#1359

#1360

#1361

#1362

#1363

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R129 bit 0

Register R129 bit 1

Register R129 bit 2

Register R129 bit 3

Register R129 bit 4

Register R129 bit 5

Register R129 bit 6

Register R129 bit 7

Register R129 bit 8

Register R129 bit 9







199



System variable

#1364

#1365

#1366

#1367

#1368

#1369

#1370

#1371

#1372

#1373

#1374

#1375

#1376

#1377

#1378

#1379

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R130 bit 0

Register R130 bit 1

Register R130 bit 2

Register R130 bit 3

Register R130 bit 4

Register R130 bit 5

Register R130 bit 6

Register R130 bit 7

Register R130 bit 8

Register R130 bit 9







System variable

#1380

#1381

#1382

#1383

#1384

#1385

#1386

#1387

#1388

#1389

#1390

#1391

#1392

#1393

#1394

#1395

No. of points

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1

1


Register R131 bit 0

Register R131 bit 1

Register R131 bit 2

Register R131 bit 3

Register R131 bit 4

Register R131 bit 5

Register R131 bit 6

Register R131 bit 7

Register R131 bit 8

Register R131 bit 9







200



(2) Macro interface by part system (output)

(Note)

As for the C64T system, the input/output signals used for this function are valid up to

3rd part system.

System variable

No. of points

$1 $2


$3 $4 $5 $6 $7

R270 R370 R470 R570 R670 R770 R870

#1100

#1101 bit0 bit0 bit1 bit1 bit0 bit1 bit0 bit1 bit0 bit0 bit0 bit1 bit1 bit1

#1102

#1103 bit2 bit2 bit3 bit3

#1104 bit4 bit4

#1105 bit5 bit5

#1106 bit6 bit6 bit2 bit3 bit4 bit5 bit6 bit2 bit3 bit4 bit5 bit6 bit2 bit2 bit2 bit3 bit3 bit3 bit4 bit4 bit4 bit5 bit5 bit5 bit6 bit6 bit6

#1107 bit7 bit7

#1108 bit8 bit8

#1109 bit9 bit9

#1110 1 bit10 bit10

#1111 1 bit11 bit11

#1112 1 bit12 bit12

#1113 1 bit13 bit13

#1114 1 bit14 bit14

#1115 1 bit15 bit15 bit7 bit8 bit9 bit10 bit11 bit12 bit13 bit14 bit15 bit7 bit8 bit9 bit10 bit11 bit12 bit13 bit14 bit15 bit7 bit7 bit7 bit8 bit8 bit8 bit9 bit9 bit9 bit10 bit10 bit10 bit11 bit11 bit11 bit12 bit12 bit12 bit13 bit13 bit13 bit14 bit14 bit14 bit15 bit15 bit15

System variable

No. of points

$1 $2


$3 $4 $5 $6 $7

R271 R371 R471 R571 R671 R771 R871

#1116

#1117 bit0 bit0 bit1 bit1 bit0 bit1 bit0 bit1 bit0 bit0 bit0 bit1 bit1 bit1

#1118 bit2 bit2

#1119 bit3 bit3

#1120 bit4 bit4 bit2 bit3 bit4 bit2 bit3 bit4 bit2 bit2 bit2 bit3 bit3 bit3 bit4 bit4 bit4

#1121 bit5 bit5

#1122 bit6 bit6

#1123 bit7 bit7

#1124 bit8 bit8

#1125 bit9 bit9

#1126 1 bit10 bit10

#1127 1 bit11 bit11

#1128 1 bit12 bit12

#1129 1 bit13 bit13

#1130 1 bit14 bit14

#1131 1 bit15 bit15 bit5 bit6 bit7 bit8 bit9 bit10 bit11 bit12 bit13 bit14 bit15 bit5 bit6 bit7 bit8 bit9 bit10 bit11 bit12 bit13 bit14 bit15 bit5 bit5 bit5 bit6 bit6 bit6 bit7 bit7 bit7 bit8 bit8 bit8 bit9 bit9 bit9 bit10 bit10 bit10 bit11 bit11 bit11 bit12 bit12 bit12 bit13 bit13 bit13 bit14 bit14 bit14 bit15 bit15 bit15

System variable

No. of points

#1132 32

#1133 32

#1134 32

$1

R270,

R271

R272,

R273

R274,

R275

#1135 32

R276,

R277

$2

R370,

R371

R372,

R373

R374,

R375

R376,

R377


$3 $4 $5

R470,

R471

R472,

R473

R474,

R475

R476,

R477

R570,

R571

R572,

R573

R574,

R575

R576,

R577

R670,

R671

R672,

R673

R674,

R675

R676,

R677

$6

R770,

R771

R772,

R773

R774,

R775

R776,

R777

$7

R870,

R871

R872,

R873

R874,

R875

R876,

R877

201


Input signal

#1032 (R24,R25)

#1000

#1001

#1002

#1003

Read only


#1132 (R124,R125)

Output signal

#1100

#1101

#1102

Read/write

#1103

#1028

#1029

#1030

#1031

32 bit

(R26,R27)

#1033

(R28,R29)

#1034

#1035

(R30,R31)

#1128

#1129

#1130

#1131

(R126,R127)

#1133

(R128,R129)

#1134

32 bit

#1135

(R130,R131)

202


Tool offset


Variable number range

#10001 to #10000 + n

#11001 to #11000 + n

#16001 to #16000 + n

#17001 to #17000 + n

#2001 to #2000 + n

#2201 to #2200 + n

#2401 to #2400 + n

#2601 to #2600 + n

Type 1 Type 2

(Length dimension)

(Length wear)

(Radius dimension)

(Radius wear)

Tool data can be read and values substituted using the variable numbers.

Either the numbers in the #10000 order or #2000 order can be used.

The last 3 digits of the variable numbers correspond to the tool offset number. n corresponds to the No. of tool offset sets.

If there are 400 tool offset sets and type 2 is being used, avoid variable Nos. in the #2000 order, and instead use the #10000 order.

The tool offset data are configured as data with a decimal point in the same way as for other variables. Consequently, this decimal point must be commanded when data below the decimal point is to be entered.

Programming example Common variables Tool offset data

#101=1000;

#10001=#101;

#102=#10001;

After execution

#101=1000.0

#102=1000.0

H1=1000.000

(Example 1)

Calculation and tool offset data setting

G28 Z0 T01 ;

M06 ;

#1=#5003 ;

G00 Z-500. ;

G31 Z-100. F100;

#10001=#5063-#1 ;

Zero point return

Tool change (spindle T01)

Start point memory

Rapid traverse to safety position

Skip measurement

Measured distance calculation and tool offset data setting

# 1

#5063

G00

G31

Sensor

H 1

(Note)

In this example, no consideration is given to the delay in the skip sensor signal.

#5003 is the Z-axis start point position and #5063 is the Z-axis skip coordinates, and indicated is the position at which the skip signal is input while G31 is being executed.

203


Work coordinate system offset


By using variable numbers #5201 to #532n, it is possible to read out the work coordinate system offset data or to substitute values.

(Note)

The number of axes which can be controlled differs according to the specifications.

The last digit in the variable number corresponds to the control axis number.

Axis No.

Axis name

Axis 1 Axis 2 Axis 3 Axis 4

. . Axis n

Remarks

External work offset #5201 #5202 #5203 #5204

. .

#520n

G54 #5221

. .

#522n

G55 #5241

. .

#524n

G56 #5261

. .

#526n

G57 #5281

. .

#528n

G58 #5301

. .

#530n

G59 #5321

. .

#532n

External workpiece offset specifications are required.

(Example 1)

N1 G28 X0 Y0 Z0 ;

N2 #5221=-20. #5222=-20. ;

N3 G90 G00 G54 X0 Y0 ;

N10 #5221=-90. #5222=-10. ;

N11 G90 G00 G54 X0Y0 ;

M02 ;

(Example 2)

Coordinate system before change

N100 #5221=#5221+#5201 ;

#5222=#5222+#5202 ;

#5241=#5241+#5201 ;

#5242=#5242+#5202 ;

#5201=0 #5202=0;

W1

N11

N1

-90.

-20.

N3

-10.

-20.

W1

G54 work coordinate system defined by

N10

G54 work coordinate system defined by

N2

Base machine coordinate system

External workpiece offset

W2 (G55)

G55

G54

W1 (G54)

M

Coordinate system after change

Base machine coordinate system

G55

G54

W2 (G55)

W1 (G54)

M

This is an example where the external workpiece offset values are added to the work coordinate

(G54, G55) system offset values without changing the position of the work coordinate systems.

204


Alarm (#3000)


The NC system can be forcibly set to the alarm state by using variable number #3000.

Format

#3000 = 70 (CALL#PROGRAMMER#TEL#530) :

70 : Alarm number

CALL#PROGRAMMER#TEL#530 : Alarm message

Any alarm number from 1 to 9999 can be specified.

The alarm message must be less than 31 characters long.

The "P277" user macro alarm message appears in the <alarm> column on diagnosis screen 1 while the alarm number and alarm message CALL #PROGRAMMER #TEL#530 is indicated in the

<operator message>.

Example of program (alarm when #1 = 0)

IF [#1 NE 0] GOTO 100 ;

#3000=70

(CALL#PROGRAMMER#TEL#530) ;

N100

Stops with

NC alarm

<Alarm>

P277 : Macro alarm message

<Operator message>

CALL#PROGRAMMER#TEL#530 70

(Note 1)

Alarm number 0 is not displayed and any number exceeding 9999 cannot be indicated.

(Note 2)

The characters following the first alphabet letter in the right member is treated as the alarm message. Therefore, a number cannot be designated as the first character of an alarm message. It is recommended that the alarm messages be enclosed in round parentheses.

205


Integrating (run-out) time (#3001, #3002)


The integrating (run-out) time can be read during automatic operation or automatic start or values can be substituted by using variable numbers #3001 and #3002.

Type

Integrating

(run-out) time 1

Integrating

(run-out) time 2

Variable number

Unit

3001

3002

1ms

Contents when power is switched on

Initialization of contents

Count condition

Same as when power is switched off

Value substituted for variable

At all times while power is ON

In-automatic start

The integrating run time returns to zero in about 2.44

×

10

11

ms (approximately 7.7 years).

(allowable

G65P9010 T ms;

To subprogram

O9010

#3001=0 ;

WHILE [#3001LE#20] DO1 ;

END1 :

M99 ;

Entered in local

Local variable variable #20

T#20

Allowable time portion :

DO1-END is repeated and when allowable time is reached, operations jumps to M99.

Suppression of single block stop and miscellaneous function finish signal waiting

By substituting the values below in variable number #3003, it is possible to suppress single block stop in the subsequent blocks or to advance to the next block without waiting for the miscellaneous function (M, S, T, B) finish (FIN) signal.

#3003 Single block stop

1 Suppressed

2 Not suppressed

Miscellaneous function finish signal

Awaited

3 Suppressed

Awaited

Not awaited

(Note 1)

#3003 is cleared to zero by NC reset.

206


Feed hold, feedrate override, G09 valid/invalid


By substituting the values below in variable number #3004, it is possible to make the feed hold, feedrate override and G09 functions either valid or invalid in the subsequent blocks.

Contents (value)

#3004 Bit 0

Feed hold

Bit 1

Feedrate override

Bit 2

G09 check

(Note 1)

Variable number #3004 is set to zero by NC reset.

(Note 2)

The functions are valid when the above bits are 0 and invalid when they are 1.

Message display and stop

By using variable number #3006, the execution is stopped after the previous block has been executed and, if message display data have been commanded, then the corresponding message will be indicated on the operator message area.

Format

#3006 = 1 ( TAKE FIVE ) :

TAKE FIVE Message

The message should not be longer than 31 characters and it should be enclosed within round ( ) parentheses.

Mirror image

By reading variable number #3007, it is possible to ascertain the status of mirror image at a particular point in time for each axis.

The axes correspond to the bits of #3007.

When the bits are 0, it means that the mirror image function is not valid; when they are 1, it means that it is valid.

#3007

Bit 15 14 12 11 10 9 8 7 6 5 4 3 2 1 0

nth 5 3 1

207


G command modals


Using variable numbers #4001 to #4021, it is possible to read the G modal commands which have been issued up to the block immediately before.

Similarly, it is possible to read the modals in the block being executed with variable numbers #4201 to #4221.

Variable number

Pre-read block

Execution block

Function

Interpolation mode

#4001 #4201

: G00:0, G01:1, G02:2, G03:3,

G33:33

#4002

#4003

#4202 Plane selection

#4203 Absolute/incremental

: G17:17, G18:18, G19:19

: G90:90, G91:91

#4004

#4005

#4006

#4204

#4205

No variable No.

Feed designation

#4206 Inch/metric

: G94:94, G95:95

: G20:20, G21/21

#4007 #4207 : G40:40, G41:41, G42:42

#4008 #4208 Tool length offset : G43:43, G44:44, G49:49

Canned cycle

#4009 #4209

#4010 #4210 Return level

: G80:80, G73 to 74, G76:76,

G81 to G89:81 to 89

: G98:98, G99:99

#4011 #4211

#4012

#4014

#4212

#4214

Work coordinate system

Macro modal call

#4015 #4215

: G54 to G59:54 to 59

Acceleration/deceleration

#4013 #4213

: G61 to G64:61 to 64,

G61.1:61.1

: G66:66, G66.1:66.1, G67:67

#4016 #4216

#4017 #4217 Constant surface speed control : G96:96, G97:97

#4018

#4019

#4218

#4219

No variable No.

Mirror image

#4020 #4220

: G50.1:50.1, G51.1:51.1

(Example)

G28 X0 Y0 Z0 ;

G90 G1 X100. F1000;

G91 G65 P300 X100. Y100.;

M02;

O300;

#1 = #4003;

→

Group 3G modal (pre-read) #1 = 91.0

#2 = #4203;

→

Group 3G modal (now being executed) #2 = 90.0

G#1 X#24 Y#25;

M99;

%

208


Other modals


Using variable numbers #4101 to #4120, it is possible to read the model commands assigned up to the block immediately before.

Similarly, it is possible to read the modals in the block being executed with variable numbers #4301 to #4320.

Variable number

Pre-read

Executio n

#4101 #4301

#4102 #4302

#4103 #4303

#4104 #4304

Modal information

#4105 #4305

#4106 #4306

Tool radius

#4107 #4307 compensation No. D

#4108 #4308

#4109 #4309 Feedrate F

#4110 #4310

Variable number

Pre-read

Executio n


#4111 #4311 Tool length offset No.H

#4112 #4312

#4114

#4115

#4314

#4315

Sequence number N

Program number O

#4116 #4316

#4117 #4317

#4118 #4318

#4119

#4120

#4319

#4320

Spindle function S

Tool function T

Position information

Using variable numbers #5001 to #5104, it is possible to read the servo deviation amounts, skip coordinates, work coordinates, machine coordinates and end point coordinates in the block immediately before.

Axis No.

Position information

End point coordinate of block immediately before

Machine coordinate

Work coordinate

Skip coordinate

Servo deviation amount

1

2

3

4

: n

Remarks (reading during movement)

#5001 #5021 #5041 #5061 #5101

#5002 #5022 #5042 #5062 #5102

#5003 #5023 #5043 #5063 #5103

#5004 #5024 #5044 #5064 #5104

: : : : :

#5000+n #5020+n #5040+n #5060+n #5100+n

Yes No No Yes Yes

(Note1)

The number of axes which can be controlled differs according to the specifications.

(Note2)

The last digit of the variable number corresponds to the control axis number.

209





W

M

G00

G01

Read command

[End point coordinates]

W


[Work coordinates]

Machine coordinate system

[Machine coordinates]

M

(1) The positions of the end point coordinates and skip coordinates are positions in the work coordinate system.

(2) The end point coordinates, skip coordinates and servo deviation amounts can be read even during movement. However, it must first be checked that movement has stopped before reading the machine coordinates and the work coordinates.

(3) The position where the skip signal is turned ON in the G31 block is indicated for the skip coordinates. The end point position is indicated when the skip signal has not been turned ON.

(For further details, refer to the section on tool length measurement.)

Read command

Skip coordinates

Gauge, etc.

210



(4) The tool nose position where the tool offset and other such factors are not considered is indicated as the end point position. The tool reference point position with consideration given to tool offset is indicated for the machine coordinates, work coordinates and skip coordinates.

Skip signal

G31

F (feedrate)

[Input coordinates of skip signal]

W


[Work coordinates]

M

[Machine coordinates]


For " ", check stop and then proceed to read.

For " ", reading is possible during movement.

The position of the skip signal input coordinates is the position in the work coordinate system.

The coordinates in variable numbers #5061 to #5064 memorize the moments when the skip input signal during movement was input and so they can be read at any subsequent time. For further details, reference should be made to the section on the skip function.

211



(Example 1)

Example of workpiece position measurement

An example to measure the distance from the measured reference point to the workpiece edge is shown below.

Main program

G65 P9031 X100. Y100. Z-10. F200;

Argument

<Local variable>

F(#9) 200

X(#24)100.000

Y(#25)100.000

Z(#26) -10.000

To subprogram

<Common variable>

#101 87.245

#102 87.245

#103 123.383

O9031

N1 #180=#4003;

N2 #30=#5001 #31=#5002;

N3 G91 G01 Z#26 F#9;

N4 G31 X#24 Y#25 F#9;

N5 G90 G00 X#30 Y#31;

N6 #101=#30-#5061 #102=#31-#5062;

N7 #103=SQR [#101

∗

#101+#102*#102] ;

N8 G91 G01Z-#26;

N9 IF [#180 EQ 91] GOTO 11;

N10 G90;

N11 M99;

Skip input

Y

Start point N4

#102

Z

N8

X

N3

N5

#103

#101

#101 X axis measurement amount

#102 X axis measurement amount

N1

N2

#103 Measurement linear segment N3

G90/G91 modal recording

X, Y start point recording

Z axis entry amount

amount N4

#5001 X axis measurement start point N5

X, Y measurement (Stop at skip input)

Return to X, Y start point

#5002 Y axis measurement start point N6 X, Y measurement incremental value calculation

#5061 X axis skip input point

#5062 Y axis skip input point

N7

N8

Measurement linear segment calculation

Z axis escape

N9, N10 G90/G91 modal return

(Example 2)

Reading of skip input coordinates

-X

-150 -75

-25

Y

X

N1 G91 G28 X0 Y0;

N2 G90 G00 X0 Y0;

N3 X0Y-100.;

N4 G31 X-150. Y-50. F80;

N5 #111=#5061#112=#5062;

N6 G00 Y0;

N7 G31 X0;

N8 #121=#5061#122=#5062;

N9 M02;

-50

-75

-100

-Y

Skip signal

#111 =

−

75. +

ε

#112 =

−

75. +

ε

#121 =

−

25. +

ε

#122 =

−

75. +

ε

ε

is the error caused by response delay.

(Refer to the section on the skip function for details.)

#122 is the N4 skip signal input coordinates as there is no Y command at N7.

212


Variable name setting and quotation


Any name (variable name) can be given to common variables #500 to #519. It must be composed of not more than 7 alphanumerics and it must begin with a letter. Do not use "#" in variable names.

It causes an alarm when the program is executed.

Format

SETVN n [ NAME

1

, NAME

2

, • • • • • • • ] :

n

NAME1

NAME2

: Head number of variable to be named

: #n name (variable name)

: #n + 1 name (variable name)

Variable names are separated by a comma (,).


(1) Once variable names have been set, they will not be cleared even when the power is switched off.

(2) Variables in programs can be quoted by their variable names. In cases like this, the variables should be enclosed in square parentheses.

(Example 1)

G01X [#POINT1] ;

[#NUMBER] = 25 ;

(3) The variable numbers, data and variable names appear on the screen of the setting and display unit.

(Example 2)

Program ...... SETVN500 [A234567, DIST, TOOL25] ;

[Common variables]

#500 -12345.678 A234567

#501 5670.000 DIST

#502 -156.500 TOOL25

#518 10.000 NUMBER

Common variable #(502) Data (-156.5) Name (TOOL25)

(Note)

At the head of the variable name, do not use the characters determined by the NC for use in arithmetic commands, etc. (e.g. SIN, COS).

Workpiece coordinate shift amount

The workpiece coordinate system shift amount can be read using variables #2501 and #2601.

By substituting a value in these variables, the workpiece coordinate system shift amount can be changed.

Axis

No.

Workpiece coordinate system shift amount

1 #2501

2 #2601

213



Number of workpiece machining times

The n umber of workpiece machining times

can be read using variables #3901 and #3902.

By substituting a value in these variables, the number of workpiece machining times can be changed.

Variable No.

Data setting range Type

Number of workpiece machining times

Maximum workpiece value

#3901

#3902

0 to 999999

(Note)

Always substitute a positive value for the number of workpiece machining times.

Tool life management

(1) Definition of variable numbers

(a) Designation of group No.

#60000

The tool life management data group No. to be read with #60001 to #64700 is designated by substituting a value in this variable. If a group No. is not designated, the data of the group registered first is read. This is valid until reset.

(b) Tool life management system variable No. (Read)

#60001 to #64700

# ? ? ? ? ?

+ Variable No. or data type

Data class

6: Tool life management

(c) Details of data classification

Data class

00

M System

For control

05

10

15

20

25

Group No.

Tool No.

Tool data flag

Tool status

Life data

L System

For control

Group No.

Tool No.

Remarks

Refer to following types

Refer to registration No.


Method

Status



Life time/No. of times Refer to registration No.

Usage time/No. of times


35

40

45

Tool length compensation data

Tool radius compensation data

Auxiliary data

–

–

–




The group No., L System method, and life data are common for the group.

214



M System

L System

1 to 200

1 to 16

Type

remaining registered tools

1

2

3

4

5

6

7

8

M System

Number of registered tools

Number of registered tools

L System

Life current value Life current value

Tool selected No. Tool selected No.

Number of remaining registered tools

Signal being executed

Cutting time cumulative value

(minute)

Life end signal

Life prediction signal

Number of remaining registered tools

Signal being executed

Cutting time cumulative value (minute)

Life end signal

Life prediction signal

Variable No.

60002

60003

Item

registered tools

Common to system

Life current value

Tool selected No.

For each group

(Designate group No.

#60000)

Remarks

Total number of tools registered in each group. 0 to 200

Usage time/No. of uses of tool being used.

Spindle tool usage data or usage data for tool in use (#60003).

0 to 4000 minutes

0 to 9999 times

Registration No. of tool being used.

Spindle tool registration No. (If spindle tool is not data of the designated group, ST:1 first tool, or if

ST:1 is not used, the first tool of ST:0. When all tools have reached their lives, the last tool.)

0 to 200

No. of first registered tool that has not reached its life.

0 to 200 executed

"1" when this group is used in program being executed.

"1" when spindle tool data group No. and designated group No. match.

Indicates the time that this group is used in the program being executed.

0/1

60007 cumulative value

(minute)

Life end signal signal

"1" when lives of all tools in this group have been reached.

0/1

"1" when all tools registered in designated group reach lives.

"1" when new tool is selected with next command in this group.

0/1

"1" when there is a tool for which ST is "0: Not used" in the designated group, and there are no tools for which ST is "1: Tools in use".

215



Variable No.

60500

+***

61000

+***

61500

+***

Item

Group No.

Tool No.

Tool data flag

62000

+***

62500

+***

63000

+***

63500

+***

Tool status

Life data

Usage data

Tool length compen-sation data

Each group/ registration No.

(Designate the group No.

#60000 and registration No.

*** .)

Note the group

No., method and life are common for the groups.

This group's No.

Tool No.

Usage data count method, length compensation method, radius compensation method, etc., parameters.

bit 0, 1 : Tool length compensation data format

bit 2, 3 : Tool radius compensation data format

0: Compensation No. method

1: Incremental value compensation amount method

2: Absolute value compensation amount method

bit 4, 5 : Tool life management method

0: Usage time

1: No. of mounts

2: No. of usages

Tool usage state

0: Not used tool

1: Tool being used

2: Normal life tool

3: Tool error 1

4: Tool error 2

Life time or No. of lives for each tool

1 to 99999999

1 to 99999999

0 to FF (H)

0 to 4

Usage time or No. of uses for each tool

Length compensation data set as compensation

No., absolute value compensation amount or increment value compensation amount method.

0 to 4000 minutes

0 to 9999 times

0 to 4000 minutes

0 to 9999 times

Compensation

No.:

0 to No. of tool compensation sets

Absolute value compensation amount

±

99999.999

Increment value compensation amount

±

99999.999

216



Variable No.

64000

+***

Item

Tool radius compensation data

Radius compensation data set as compensation

No., absolute value compensation amount or increment value compensation amount method.

Spare data

Compensation

No.:

0 to No. of tool compensation sets

Absolute value compensation amount

±

99999.999

Increment value compensation amount

±

99999.999

0 to 65535 64500

+***

Auxiliary data

Example of program for tool life management

#101 = #60001 ; ........... Reads the number of registered tools.

#102 = #60002 ; ........... Reads the life current value.

#103 = #60003 ; ........... Reads the tool selection No.

#60000 = 10 ; ............... Designates the group No. of the life data to be read.

#104 = #60004 ; ........... Reads the remaining number of registered tools in group 10.

#105 = #60005 ; ........... Reads the signal being executed in group 10.

#111 = #61001 ; ........... Reads the group 10, #1 tool No.

#112 = #62001 ; ........... Reads the group 10, #1 status.

#113 = #61002 ; ........... Reads the group 10, #2 status.

%

Designated program No. is valid until reset.

(2) When group No. is not designated.

#104 = #60004 ; ........... Reads the remaining number of registered tools in the group registered first.

#111 = #61001 ; ........... Reads the #1 tool No. in the group registered first.

%

(3) When non-registered group No. is designated. (Group 9999 does not exist.)

#60000 = 9999 ; ........... Designates the group No.

#104 = #60004 ; ........... #104 = –1.

(4) When registration No. not used is designated. (Group 10 has 15 tools)

#111 = #61016 ; ........... #101 = –1.

(5) When registration No. out of the specifications is designated.

#60000 = 10 ;

#111 = #61017 ; ........... Program error (P241)

217



(6) When tool life management data is registered with G10 command after group No. is designated.

#60000 = 10 ; ..............Designates the group No.

G10 L3 ; .......................Starts the life management data registration.

P10 LLn NNn ; ............10 is the group No., Ln is the life per tool,

The group 10 life data

Nn is the method.

TTn ; ............................Tn is the tool No.

:

G11 ; ...........................Registers the group 10 data with the G10 is registered.

command.

#111 = #61001 ; ..........Reads the group 10, #1 tool No.

G10 L3 ; .......................Starts the life management data registration.

P1 LLn NNn ; ..............1 is the group No., Ln is the life per tool,

Nn is the method.

TTn ; ............................Tn is the tool No.

:

The life data other than group 10 is registered.

G11 ; ............................Registers the life data with the G10

command.

(The registered data is deleted.)

#111 = 61001 ; ............Group 10 does not exist. #201 = –1.

Precautions for tool life management

(1) If the tool life management system variable is commanded without designating a group No., the data of the group registered at the head of the registered data will be read.

(2) If a non-registered group No. is designated and the tool life management system variable is commanded, "-1" will be read as the data.

(3) If an unused registration No. tool life management system variable is commanded, "-1" will be read as the data.

(4) Once commanded, the group No. is valid until NC reset.

218



13.5.5 Arithmetic commands

A variety of arithmetic operations can be performed between variables.

Command format

#i = <formula>

<Formula> is a combination of constants, variables, functions and operators.

Constants can be used instead of #j and #k below. substitution of variables

#i = #j

(3) Multiplication

Definition, substitution

#i = #j + #k

#i = #j – #k

Addition

Subtraction

#i = #j OR #k Logical sum (at every bit of 32 bits)

#i = #j XOR #k Exclusive OR (at every bit of 32 bits)

#i = #j

∗

#k

Multiplication

#i = #j / #k Division

(4) Functions

#i = #j MOD #k Remainder

#i = #j AND #k Logical product (at every bit of 32 bits)

#i = SIN [#k] Sine

#i = COS [#k] Cosine

#i = TAN [#k] Tangent (sin/cos used for tan)

#i = ATAN [#j] Arctangent (ATAN or ATN may be used)

#i = ACOS [#j] Arc-cosine

#i = SQRT [#k]

Square root (SQRT or SQR may be used)

#i = ABS [#k]

#i = BIN [#k]

Absolute value

Conversion from BCD to BIN

#i = BCD [#k] Conversion from BIN to BCD

#i = ROUND [#k] Rounding off

(ROUND or RND may be used)

#i = FIX [#k] Discard fractions less than 1

#i = FUP [#k]

#i = LN [#k]

#i = EXP [#k]

Add for fractions less than 1

Natural logarithm

Exponent with e (=2.718 .....) as bottom

(Note 1)

A value without a decimal point is basically treated as a value with a decimal point at the end (1 = 1.000).

(Note 2)

Offset amounts from #10001 and work coordinate system offset values from #5201 are handled as data with a decimal point. Consequently, data with a decimal point will be produced even when data without a decimal point have been defined in the variable numbers.

(Example)

#101 = 1000 ;

#10001 = #101 ;

#102 = #10001 ;

Common variables after execution

#101 1000.000

#102 1000.000

(Note 3)

The <formula> after a function must be enclosed in the square parentheses.

219



Sequence of arithmetic operations

(1) The sequence of the arithmetic operations (1) through (3) is, respectively, the functions followed by the multiplication arithmetic followed in turn by the addition arithmetic.

#101 = #111 + #112

∗

SIN[#113]

(1) Function

(2) Multiplication arithmetic

(3) Addition arithmetic

(2) The part to be given priority in the operation sequence should be enclosed in square parentheses. Up to 5 pairs of such parentheses including those for the functions may be used.

#101 = SQRT [ [ [ #111 = #112 ]

∗

SIN[#113] + #114]

∗

#15] ;

First pair of parentheses

Second pair of parentheses

Third pair of parentheses

Examples of arithmetic commands

(1) Main Program and argument designation

G65 P100 A10 B20.;

#101 = 100.000 #102 =

200.000 ;

(2) Definition and substitution (=)

#1 = 1000

#2 = 1000.

#3 = #101

#4 = #102

#5 = #5041

(3) Addition and subtraction (+,

−

)

#11 = #1 + 1000

#12 = #2 – 50.

#13 = #101 + #1

#14 = #5041 – 3.

#15 = #5041 + #102

(4) Logical sum (OR) #3 = 100

#4 = #3OR14

(5) Exclusive OR

(XOR)

#3 = 100

#4 = #3XOR14

#1 10.000

#2 20.000

#101 100.000

#102 200.000

#1 1000.000

#2 1000.000

#5

−

10.000 From amount

#11 2000.000

#12 950.000

#13 1100.000

#14

−

13.000

#15 190.000

#3 = 01100100

14 = 00001110

#4 = 01101110 = 110

#3 = 01100100

14 = 00001110

#4 = 01101010 = 106

220



(6) Multiplication and division (

∗

,/)

#21 = 100

∗

100

#22 = 100.

∗

100

#23 = 100

∗

100

#24 = 100.

∗

100.

#25 = 100/100

#26 = 100./100.

#27 = 100/100.

#28 = 100./100.

#29 = #5041

∗

#101

#30 = #5041/#102

(7) Remainder (MOD) #31 = #19MOD#20

(8) Logical product

(AND)

#9 = 100

#10 = #9AND15

#21 10000.000

#22 10000.000

#23 10000.000

#24 10000.000

#25 1.000

#26 1.000

#27 1.000

#28 1.000

#29

−

1000.000

#30

−

0.050

(9) Sin (SIN) #501 = SIN [60]

#502 = SIN [60.]

#503 = 1000

∗

SIN [60]

#504 = 1000

∗

SIN [60.]

#505 = 1000.

∗

SIN [60]

#506 = 1000.

∗

SIN [60.]

Note

: SIN [60] is equivalent to SIN [60.]

(10) Cosine (COS) #541 = COS [45]

#542 = COS [45.]

#543 = 1000

∗

COS [45]

#544 = 1000

∗

COS [45.]

#545 = 1000.

∗

COS [45]

#546 = 1000.

∗

COS [45.]

Note

: COS [45] is equivalent to COS [45.]

(11) Tangent (TAN) #551 = TAN [60]

#552 = TAN [60.]

#553 = 1000

∗

TAN [60]

#554 = 1000

∗

TAN [60.]

#555 = 1000.

∗

TAN [60]

#556 = 1000.

∗

TAN [60.]

Note

: TAN [60] is equivalent to TAN [60.]

(12) Arctangent

(ATAN or ATN)

#561 = ATAN [173205/100000]

#562 = ATAN [173205/100.]

#563 = ATAN

[173.205/100000]

#564 = ATAN [173.205/100.]

#565 = ATAN [1.732]

#19/#20 = 48/9 = 5 with 3 over

#9 = 01100100

15 = 00001111

#10 = 00000100 = 4

#501 0.860

#502 0.860

#503 866.025

#504 866.025

#505 866.025

#506 866.025

#541 0.707

#542 0.707

#543 707.107

#544 707.107

#545 707.107

#546 707.107

#551 1.732

#552 1.732

#553 1732.051

#554 1732.051

#555 1732.051

#556 1732.051

#561 60.000

#562 60.000

#563 60.000

#564 60.000

#565 60.000

221



(13) Arc-cosine

(ACOS)

(14) Square root

(SQR or SQRT)

(15) Absolute value

(ABS)

(16) BIN, BCD

#521 = ACOS [100./141.421]

#522 = ACOS [100./141.421]

#523 = ACOS [1000./1414.213]

#524 = ACOS [10./14.142]

#525 = ACOS [0.707]

#571 = SQRT [1000]

#572 = SQRT [1000.]

#573 = SQRT [10.

∗

10.+20.

∗

20.]

#574 = SQRT

[14

∗

#14+#15

∗

#15]

Note

: In order to increase the accuracy, proceed with the operation inside

parentheses.

#576 =

−

1000

#577 = ABS [#576]

#3 = 70.#4 =

−

50.

#580 = ABS [#4

−

#3]

#1 = 100

#11 = BIN [#1]

#12 = BCD [#1]

(17) Rounding off

(ROUND or RND)

#21 = ROUND [14/3]

#22 = ROUND [14./3]

(18) Discarding fractions below decimal point

(FIX)

#23 = ROUND [14/3.]

#24 = ROUND [14./3.]

#25 = ROUND [

−

14/3]

#26 = ROUND [

−

14./3]

#27 = ROUND [

−

14/3.]

#28 = ROUND [

−

14./3.]

#21 = FIX [14/3]

#22 = FIX [14./3]

#23 = FIX [14/3.]

#24 = FIX[14./3.]

#25 = FIX [

−

14/3]

#26 = FIX [

−

14./3]

#27 = FIX [

−

14/3.]

#28 = FIX [

−

14./3.]

(19) Adding fractions less than 1 (FUP)

#21 = FUP [14/3]

#22 = FUP [14./3]

#23 = FUP [14/3.]

#24 = FUP [14./3.]

#25 = FUP [

−

14/3]

#26 = FUP [

−

14./3]

#27 = FUP [

−

14/3.]

#28 = FUP [

−

14./3.]

(20) Natural logarithms (LN)

#101 = LN [5]

#102 = LN [0.5]

#103 = LN [

−

5]

(21) Exponents (EXP) #104 = EXP [2]

#105 = EXP [1]

#106 = EXP [

−

2]

#521 45.000

#522 45.000

#523 45.000

#524 44.999

#525 45.009

#571 31.623

#572 31.623

#573 22.361

#574 190.444

#576

−

1000.000

#577 1000.00

#580 120.000

#11 64

#12 256

#21 5

#22 5

#23 5

#24 5

#25

−

5

#26

#27

#28

−

5

−

5

−

5

#21 4.000

#22 4.000

#23 4.000

#24 4.000

#25

−

4.000

#26

#27

#28

−

4.000

−

4.000

−

4.000

#21 5.000

#22 5.000

#23 5.000

#24 5.000

#25

−

5.000

#26

#27

#28

−

5.000

−

5.000

−

5.000

#101 1.609

#102

−

0.693

Error "P282"

#104 7.389

#105 2.718

#106 0.135

222



Arithmetic accuracy

As shown in the following table, errors will be generated when performing arithmetic operations once and these errors will accumulate by repeating the operations.

Arithmetic format Average error Maximum error Type of error

a = b + c a = b

−

c a = b

∗ c 1.55 a = b/c

2.33

×

10

−

10

10

4.66

×

10

−

10

×

10

10

−

10

Min.

|

Relative error

ε

/a|

/c| a = b 1.24

×

10

−

9 a = SIN [b] a = COS [b] a = ATAN [b/c]

5.0

×

10

−

9

1.8

×

10

−

6

8

1.0

6

3.6

Absolute error

|

ε

|

°

(Note)

SIN/COS is calculated for the function TAN.

Notes on reduced accuracy

(1) Addition and subtraction

It should be noted that when absolute values are used subtractively in addition or subtraction, the relative error cannot be kept below 10

−

8

.

For instance, it is assumed that the real values produced as the arithmetic calculation result of

#10 and #20 are as follows (these values cannot be substituted directly) :

#10 = 2345678988888.888

#20 = 2345678901234.567

Performing #10

−

#20 will not produced #10

−

320 = 87654.321. There are 8 significant digits in the variables and so the values of #10 and #20 will be as follows (strictly speaking, the internal values will differ somewhat from the values below because they are binary numbers) :

#10 = 2345679000000.000

#20 = 2345678900000.000

Consequently, #10

−

#20 = 100000.000 will generate a large error.

EQ, NE, GT, LT, GE and LE are basically the same as addition and subtraction and so care should be taken with errors. For instance, to determine whether or not #10 and #20 are equal in the above example :

IF [#10EQ#20]

It is not always possible to provide proper evaluation because of the above mentioned error.

Therefore, when the error is evaluated as in the following expression :

IF [ABS [#10

−

#20] LT200000] and the difference between #10 and #20 falls within the designated range error, both values should be considered equal.

Absolute errors are guaranteed with trigonometric functions but since the relative error is not under 10

−

8

, care should be taken when dividing or multiplying after having used a trigonometric function.

223



13.5.6 Control commands

The flow of programs can be controlled by IF-GOTO- and WHILE-DO-.

Branching

Format

IF [conditional expression] GOTO n; (n = sequence number in the program)

When the condition is satisfied, control branches to "n" and when it is not satisfied, the next block is executed.

IF [conditional expression] can be omitted and, when it is, control passes to "n" unconditionally.

The following types of [conditional expressions] are available.

#i EQ #j = When #i and #j are equal

#i NE #j

≠

When #i and #j are not equal

#i GT #j > When #i is greater than #j

#i LT #j < When #i is less than #j

#i GE #j

≥

When #i is #j or more

#i LE #j

≤

When #i is #j or less

"n" of GOTO n must always be in the same program. Program error (P231) will result if it is not. A formula or variable can be used instead of #i, #j and "n".

In the block with sequence number "n" which will be executed after a GOTO n command, the sequence number must always be at the head of the block.

Otherwise, program error (P231) will result.

If "/" is at the head of the block and Nn follows, control can be branched to the sequence number.

N10 #22=#20 #23=#21;

IF [#2 EQ1] GOTO100;

#22=#20-#3;

#23=#21-#4;

N100 X#22 Y#23;

#1=#1+1;

Branching to

N100 when content of #2 is 1

N100

Branch search

With

N10

To head

(Note 1)

When the sequence number of the branch destination is searched, the search is conducted up to the end of the program (% code) from the block following IF……; and if it is not found, it is then conducted from the top of the program to the block before IF……;.

Therefore, branch searches in the opposite direction to the program flow will take longer to execute compared with branch searches in the forward direction.

(Note 2)

EQ and NE should be used only for integers. For comparison of numeric values with decimals, GE, GT, LE, and LT should be used.

224



Iteration

Format

WHILE [conditional expression] DOm ; (m = 1, 2, 3 ..... 127)

END m ;

(1) Same identifier number can be used any number of times.

While the conditional expression is established, the blocks from the following block to ENDm are repeatedly executed; when it is not established, execution moves to the block after ENDm. DOm may come before WHILE, WHILE [conditional expression] DOm and ENDm must be used as a pair.

IF WHILE [conditional expression] is omitted, these blocks will be repeatedly ad infinitum. The repeating identification numbers range from 1 through 127 (DO1, DO2, DO3, ....... DO127). Up to

27 nesting levels can be used.

(2) Any number may be used for the WHILE

−

DOm identifier number.

WHILE ~ DO1 ;

END1 ;

Possible

WHILE ~ DO1 ;

END1 ;

WHILE ~ DO3 ;

END3 ;

Possible

Possible

WHILE ~ DO1 ;

END1 ;

WHILE ~ DO2 ;

END2 ;

(3) Up to 27 nesting levels for WHILE

−

DOm. "m" is any number from 1 to 127 for the nesting depth.

DO1

WHILE ~ DO1 ;

DO2

WHILE ~ DO2 ;

:

WHILE~DO27; DO27

WHILE ~ DO1 ;

END1 ;

(4) The number of WHILE

−

DOm nesting levels cannot exceed 27.

WHILE ~ DO1 ;

WHILE ~ DO2 ;

:

WHILE ~ DO3 ;

WHILE ~ DO28;

END 27 ;

:

END 2 ;

END 1 ;

(Note)

:With nesting, "m" which has been used once cannot be used.

END 28;

END 3 ;

:

END 2 ;

END 1 ;

225



(5) WHILE

−

DOm must be designated first and

ENDm last.

Not possible

END 1 ;

WHILE ~ DO1 ;

(6) WHILE

−

DOm and ENDm must correspond on a 1:1 (pairing) basis in the same program.

Not possible

WHILE ~ DO1 ;

WHILE ~ DO1 ;

(7) Two WHILE

−

DOm's must not overlap.

Not possible

WHILE ~ DO1 ;

WHILE ~ DO2 ;

END 1 ;

END 1 ;

(8) Branching externally is possible from the WHILE

−

DOm range.

Possible

WHILE ~ DO1 ;

IF ~ GOTOn ;

END 1 ;

END 2 ;

(9) No branching is possible inside WHILE

−

DOm.

IF~GOTOn;

WHILE~DO1;

IF~GOTOn;

WHILE~DO1; END1;

Nn;

END1;

WHILE~DO1;

Nn;

END1;

Nn

(10) Subprograms can be called by M98, G65 or

G66 between WHILE

−

DOm's.

Main program

WHILE~DO1;

G65

P100;

To subprogram

END1;

M02;

Subprogram

WHILE~DO02;

END2;

M99;

(11) Calls can be initiated by G65 or G66 between

WHILE

−

DOm's and commands can be issued again from 1. Up to 27 nesting levels are possible for the main program and subprograms.

Main program Subprogram

(12) A program error will occur at M99 if WHILE and

END are not paired in the subprogram

(including macro subprogram).

Main program

M98

P100;

To subprogram

Subprogram

WHILE

~DO1;

M02;

M99;

WHILE ~ DO1 ;

G65 P100 ;

END 1 ;

To subprogram

M02 ;

WHILE ~ DO1 ;

END 1 ;

M99 ;

Don ENDn constitutes illegal usage.

(Note)

As the canned cycles G73 and G83 and the special canned cycle G34 use WHILE, these will be added multiple times.

226



13.5.7 External output commands


Besides the standard user macro commands, the following macro instructions are also available as external output commands. They are designed to output the variable values or characters via the RS-232C interface.

Command format

POPEN For preparing the processing of data outputs

PCLOS For terminating the processing of data outputs

BPRNT For character output and variable value binary output

DPRNT For character output and digit-by-digit variable numerical output

Command sequence

POPEN

Open command

DPRNT

Data output command

PCLOS

Closed command

Open command : POPEN

(1) The command is issued before the series of data output commands.

(2) The DC2 control code and % code are output from the NC system to the external output device.

(3) Once POPEN; has been issued, it will remain valid until PCLOS; is issued.

Close command : PCLOS

(1) This command is issued when all the data outputs are completed.

(2) The DC4 control code and % code are output from the NC unit to the external output device.

(3) This command is used together with the open command and it should not be issued unless the open mode has been established.

(4) Issue the close command at the end of the program even when operation has been suspended by resetting or some other operation during data output.

227


Data output command : DPRNT


DPRNT [ l1 # v1 [ d1 c1 ] l 2 # v2 [ d2 c2 ] • • • • • • • • • • • ]

l1 : Character string v1 d1 c1

: Variable number

: Significant digits above decimal point

: Significant digits below decimal point c + d

≤

8

(1) The character output and decimal output of the variable values are done with ISO codes.

(2) The commanded character string is output as is by the ISO code.

Alphanumerics (A to Z, 0 to 9) and special characters (+,

−

,

∗

, /) can be used.

(3) The required significant digits above and below the decimal point in the variable values are commanded within square parentheses. As a result, the variable values equivalent to the commanded number of digits including the decimal point are output in ISO code in decimal notation from the high-order digits. Trailing zeroes are not omitted.

(4) Leading zeroes are suppressed.

The leading zeroes can also be replaced by blank if so specified with a parameter. This can justify printed data on the last column.

(Note)

A data output command can be issued even in dual-system mode. In this case, however, note that the output channel is shared for both systems. So, take care not to execute data output in both systems simultaneously.

228



13.5.8 Precautions

Precautions

When the user macro commands are employed, it is possible to use the M, S, T and other NC control commands together with the arithmetic, decision, branching and other macro commands for preparing the machining programs. When the former commands are made into executable statements and the latter commands into macro statements, the macro statement processing should be accomplished as quickly as possible in order to minimize the machining time, because such processing is not directly related to machine control.

As a result, the parameter "#8101 macro single" can be set and the macro statements can be processed in parallel with the execution of the executable statement.

(The parameter can be set OFF during normal machining to process all the macro statements together or set ON during a program check to execute the macro statements block by block. This enables the setting to be made in accordance with the intended objective in mind.)

Example of program

G91G28X0Y0Z0 ;

G92X0Y0Z0 ;

G00X-100.Y-100. ;

• • • • • (1)

• • • • • (2)

• • • • • (3)

#101=100.

∗

COS [210.] ; • • • • • (4)

#102=100.

∗

SIN [210.] ; • • • • • (5)

G01X#101Y#102F800 ; • • • • • (6)

Macro statement

Macro statements are:

(1) Arithmetic commands (block including =)

(2) Control commands (block including GOTO, DO-END, etc.)

(3) Macro call commands (including macro calls based on G codes and cancel commands (G65,

G66, G66.1, G67))

Executable statements indicate statements other than macro statements.

Flow of processing

Program analysis (1) (2) (3) (4)(5)(6)

Block executing

Program analysis

(1)

(1)

(2)

(2) (3) (4)(5)(6)

(3) (4) (5) (6)

Block executing

(1) (2) (3) (4) (5) (6)

229



Machining program display

[In execution] N3 G00 X-100. Y-100. ;

[Next command]N6 G01 X#101 Y#102

F800 ;

[In execution]

N3 G00 X-100. Y-100. ;

[Next command]

N4 #101=100.

∗

COS [210.] ;

N4, N5 and N6 are processed in parallel with the control of the executable statement of N3, N6 is an executable statement and so it is displayed as the next command. If the N4, N5 and N6 analysis is in time during N3 control, the machine movement will be continuously controlled.

N4 is processed in parallel with the control of the NC executable statement of N3, and it is displayed as the next command. N5 and N6 is executed after N3 has finished, and so the machine control is held on standby during the N5 and N6 analysis time.

230



13.5.9 Actual examples of using user macros

The following three examples will be described.

(Example 1)

SIN curve

(Example 2)

Bolt hole circle

(Example 3)

Grid

(Example 1) SIN curve

G65 Pp1 Aa1 Bb1 Cc1 Ff1 ; a1 ; Initial value 0

° b1 ; Final value 360

° c1 ; R of %

∗

SIN

θ f1 ; Feedrate

(SIN

θ

)

Y

100.

0

-100.

Main program

G65P9910A0B360.C100.F100;

To subprogram

90.

180.

O9910 (Subprogram)

Local variable set by argument

#1=0

#2=360.000

#3=100.000

#9=100.000

WHILE [#1LE#2] DO1;

#101=#3

∗

SIN [#1] ;

G90G01X#1Y#10F#9;

#1=#1+10.;

END1;

M99;

270.

(Note 1)

X

360.

(Note 1)

Commanding with one block is possible when

G90G01X#1Y [#3

∗

SIN [#1]] F#9 ; is issued.

231



(Example 2) Bolt hole circle

After defining the hole data with canned cycle (G72 to G89), the macro command is issued as the hole position command.

-X x1

W

Main program

G81Z–100.R50.F300L0

G65P9920Aa1Bb1Rr1Xx1Yy1 ;

To subprogram a1 ; Start angle b1 ; No. of holes r1 ; Radius x1 ; X axis center position y1 ; Y axis center position a1 y1

-Y

O9920 (Subprogram)

#101=0 ;

#102=#4003 ;

#103=#5001 ;

(Note 1)

#104=#5002 ;

#111=#1 ;

WHILE [#101LT#2] DO1 ;

#120=#24+#18

∗

COS [#111] ;

#121=#25+#18

∗

SIN [#111] ;

#122=#120 #123=#121 ;

IF [#102EQ90] GOTO100 ;

#122=#120

−

#103 ;

#123=#121

−

#104 ;

(Note 1)

(Note 1)

#103=#120

#104=#121

(Note 1)

N100 X#122Y#123 ;

#101=#101+1 ;

#111=#1+360.

∗

#101/#2 ;

END1 ;

M99 ;

(Note 1)

(Note 1)

The processing time can be shortened by programming in one block.

O9920

0

→

#101

G90, G91 mode

Read in

→

#102

Read previous coordinates

X

→

#103

Y

→

#104

Start angle

→

111

#101 = No. of hole count

#102 = G90 or G91

#103 = X axis current position

#104 = Y axis current position

#111 = Start angle

#101

≤

No. of holes

N

END

Y

Radius

∗

COS [#111]

+ Center coordinates X

→

#120

Radius

∗

SIN [#111]

+ Center coordinates Y

→

#121

#120

→

#122

#121

→

#123

#120 = Hole position

X coordinates

#121 = Hole position

Y coordinates

#122 = X axis absolute value

#123 = Y axis absolute value

#102=90

N

#120-#103

→

#122

#121-#104

→

#123

#120

→

#103

#121

→

#104

N100X#122Y#123

#101+1

→

#101

360 deg.

∗

#101/

No. of holes+#1

→

#111

Y

Judgment of G90, G91 mode

#122 = X axis incremental value

123 = Y axis incremental value

X axis current position update

Y axis current position update

Drilling command

No.of holes counter up

#111 = Hole position angle

232


G28 X0 Y0 Z0;

T1 M06;

G90 G43 Z100.H01;

G54 G00 X0 Y0;

G81 Z-100.R3.F100 L0 M03;

G65 P9920 X-500. Y-500. A0 B8 R100.;

G65 P9920 X-500. Y-500. A0 B8 R200.;

G65 P9920 X-500. Y-500. A0 B8 R300.;

•

•

To subprogram

To subprogram

To subprogram

-X

200R


-500.

W

300R

100R

-500.

-Y

(Example 3) Grid

After defining the hole data with the canned cycle (G72 to G89), macro call is commanded as a hole position command.

G81 Zz1 Rr1 Ff1;

G65Pp1 Xx1 Yy1 Ii1 Jj1 Aa1 Bb1; x1 ; X axis hole position y1 ; Y axis hole position

Subprogram is on next page i1 ; X axis interval j1 ; Y axis interval a1 ; No. of holes in X direction b1 ; No. of holes in Y direction

-X i1 x1 j1

W y1

-Y

G28 X0 Y0 Z0;

T1 M06;

G90 G43 Z100.H01;

G54 G00 X0 Y0;

G81 Z-100. R3.F100 L0 M03;

G65 P9930 X0 Y0 I-100. J-75. A5B3;

G84 Z-90. R3. F250 M03;

G65 P9930 X0 I-100. J-75. A5B3;

To subprogram

To subprogram

-X

100.

100. 100.

W

-75.

-75.

-Y

-X

-100.

-Z

233



O9930 (Subprogram) O9930

#101=#24 ;

#102=#25 ;

#103=#4 ;

#104=#5 ;

(Note 1)

#106=#2 ;

WHILE [#106GT0] DO1 ;

#105=#1 ;

WHILE [#105GT0] DO2 ;

G90 X#101 Y#102 ;

#101=#101+#103 ;

#105=#105

−

1 ;

(Note 1)

END2 ;

#101=#101-#103;

#102=#102+#104;

#103=

−

#103 ;

#106=#106

−

1 ;

(Note 1)

END1 ;

M99 ;

(Note 1)

The processing time can be shortened by programming in one block.

Start point X coordinates : x

1

→

#101

Start point Y coordinates : y

1

→

#102

X axis interval

Y axis interval

: i

1

→

#103

: j

1

→

#104

No. of holes in Y direction : b

1

→

#106

#106 > 0

Y

Y direction drilling completion check

#105 > 0

X#101 Y#102

#101 + #103

→

#101

#105

−

1

→

#105

#101

−

#103

→

#101

#102 + #104

→

#102

−

#103

→

#103

#106

−

1

→

#106

#101 = X axis start point

#102 = Y direction interval

#103 = X direction interval

#106 = No. of holes in

Y direction

N

No. of holes in Y direction

END

No. of holes in X direction set

No. of holes in Y direction check

Positioning, drilling

X coordinates update

No. of holes in X direction

−

1

X coordinates revision

Y coordinates update

X axis drilling direction reversal

No. of holes in Y direction

−

1

234


13.6 G command mirror image

13.6 G command mirror image; G50.1, G51.1


When cutting a shape that is symmetrical on the left and right, programming time can be shortened by machining the one side and then using the same program to machine the other side. The mirror image function is effective for this.

For example, when using a program as shown below to machine the shape on the left side, a symmetrical shape can be machined on the right side by applying mirror image and executing the program.

Base shape (program)

Shape when machining program for left side is executed after the mirror command.

Y

X

Mirror axis

Command format

G51.1 Xx

1

Yy

1

Zz

1

; (Mirror image ON)

G50.1 Xx

2

Yy

2

Zz

2

; (Mirror image OFF)

Xx/Yy/Zz : Mirror image command axis


(1) The coordinate word for G51.1 is commanded with the mirror image command axis, and the coordinate value commands the mirror image center coordinate with an absolute value or incremental value.

(2) The coordinate word in G50.1 expresses the axis for which mirror image is to be turned OFF, and the coordinate value is ignored.

(3) If mirror image is applied on only one axis in the designated plane, the rotation direction and compensation direction will be reversed for the arc or tool diameter compensation and coordinate rotation, etc.

(4) This function is processed on the local coordinate system, so the center of the mirror image will change when the counter is preset or when the workpiece coordinates are changed.

235



(5) Reference point return during mirror image

If the reference point return command (G28, G30) is executed during the mirror image, the mirror image will be valid during the movement to the intermediate point, but will not be applied on the movement to the reference point after the intermediate point.

Intermediate point when mirror is applied

Intermediate point

Path on which mirror is applied

Programmed path

Mirror center

(6) Return from zero point during mirror image

If the return command (G29) from the zero point is commanded during the mirror image, the mirror will be applied on the intermediate point.

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

236



Precautions

C CAUTION

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

If mirror image is canceled at a point other than the mirror center, the absolute value and machine position will deviate as shown below. (In this state, execute the absolute value command

(positioning with G90 mode), or execute reference point return with G28 or G30 to continue the operation.) The mirror center is set with an absolute value, so if the mirror center is commanded again in this state, the center may be set to an unpredictable position.

Cancel the mirror at the mirror center or position with the absolute value command after canceling.

Absolute value (position commanded in program)

Machine position

When moved with the incremental command after mirror cancel

Issue mirror cancel command here

Issue mirror axis command here

Mirror center

Combination with other functions

(1) Combination with diameter compensation

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

Programmed path

When only diameter compensation is applied

Mirror center

When only mirror image is applied

When both mirror image and diameter compensation are applied

237


13.7 Corner chamfering, corner rounding


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

13.7.1 Corner chamfering " ,C_ "


The corner is chamfered in such a way that the positions produced by subtracting the lengths commanded by ",C_" from the imaginary starting and final corners which would apply if no chamfering were to be performed, are connected.

Command format

N100 G01 X_ Y_ ,C_ ;

N200 G01 X_ Y_ ;

,C_ : Length up to chamfering starting point or end point from imaginary corner

Chamfering is performed at the point where N100 and N200 intersect.


(1) G91 G01 X100., C10. ;

(2) X100. Y100. ;

Y axis

(2)

Imaginary corner intersection point

Chamfering start point

Chamfering end point

(1)

10.0

10.0

Y100.0

X axis

X100.0

X100.0

238




(1) The start point of the block following the corner chamfering serves as the imaginary corner intersection point.

(2) When the comma in ",C" is not present, it is handled as a C command.

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

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

(5) Program error "P381" results when there is an arc command in the block following the corner chamfering block.

(6) Program error "P382" results when the block following the corner chamfering block does not have a linear command.

(7) Program error "P383" results when the movement amount in the corner chamfering block is less than the chamfering amount.

(8) Program error "P384" results when the movement amount in the block following the corner chamfering block is less than the chamfering amount.

239



13.7.2 Corner rounding " ,R_ "


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

Command format

N100 G01 X_ Y_ , R_ ;

N200 G02 X_ Y_ ;

,R_ : Arc radius of corner rounding

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


(1) G91 G01 X100., R10. ;

(2) X100. Y100. ;

Y axis

Corner rounding start point

Corner rounding end point

(2)

Y100.0

Imaginary corner intersection point

(1)

R10.0

X axis

X100.0

X100.0


(1) The start point of the block following the corner R serves as the imaginary corner intersection point.

(2) When the comma in ",R" is not present, it is handled as an R command.

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

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

(5) Program error "P381" results when there is an arc command in the block following the corner rounding block.

(6) Program error "P382" results when the block following the corner rounding block does not have a linear command.

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

(8) Program error "P384" results when the movement amount in the block following the corner rounding block is less than the R value.

240


13.8 Circle cutting

13.8 Circle cutting; G12, G13


Circle cutting starts the tool from the center of the circle, and cuts the inner circumference of the circle. The tool continues cutting while drawing a circle and returns to the center position.

Command format

G12 (G13) Ii

1

Dd

1

Ff

1

;

I

D

: Radius of circle (incremental value), the symbol is ignored

: Offset No. (The offset No. and offset data are not displayed on the setting and display unit.)


(1) The symbol + for the offset amount indicates reduction, and

−

indicates enlargement.

(2) The circle cutting is executed on the plane G17, G18 or G19 currently selected.

5

Circle radius

4 i

1 d1 offset amount + d1 offset amount

−

3

1

0

7

6

2

Offset amount symbol +

Offset amount symbol

−

Y

For G12 (tool center path)

0 1 2 3 4 5 6 7 0

For G13 (tool center path)

0 7 6 5 4 3 2 1 0

X

241



(Example 1)

G12 I5000 D01 F100 ; (Input setting unit 0.01)

When offset amount is +10.00mm

13.8 Circle cutting

Y

Tool

X

10.000m

Offset

50.000m

Radius

Cautions

(1) If the offset No. "D" is not issued or if the offset No. is illegal, the program error (P170) will occur.

(2) If [Radius (I) = offset amount] is 0 or negative, the program error (P233) will occur.

(3) If G12 or G13 is commanded during diameter compensation (G41, G42), the diameter compensation will be validated on the path after compensating with the D commanded with

G12 or G13.

(4) If an address, not included in the format, is commanded in the same block as G12 and G13, a program error (P32) will occur.

242


13.9 Program parameter input

13.9 Program parameter input; G10, G11


The parameters set from the setting and display unit can be changed in the machining programs.

The data format used for the data setting is as follows.

Command format

G10 L50 ; Data setting command

P major classification number N data number H bit type data ;

P major classification number A axis number N data number

D byte type data ;

P major classification number A axis number N data number S word type data ;

P major classification number A axis number N data number L 2 word type data ;

G11 ; Data setting mode cancel (data setting completed)

There are 8 types of data formats according to the type of parameter (axis-common and axis-independent) and data type, as listed below.

With axis-common data

Axis-common bit-type parameter ....................................... P N H ;

Axis-common byte-type parameter ..................................... P N D ;

Axis-common word-type parameter .................................... P N S ;

Axis-common 2-word-type parameter................................. P N L ;

With axis-independent data

Axis-independent bit-type parameter .................................. P A N H ;

Axis-independent byte-type parameter ............................... P A N D ;

Axis-independent word-type parameter .............................. P A N S ;

Axis-independent 2-word-type parameter ........................... P A N L ;

(Note 1)

The sequence of addresses in a block must be as shown above.

(Note 2)

Whether the parameter value is replaced or added depends on the modal state of

G90/G91 when G10 is commanded.

(Note 3)

Refer to Appendix Table 1 for the P, N number correspondence table.

(Note 4)

For a bit type parameter, the data type will be H

(

is a value between 0 and 7).

(Note 5)

The axis number is set in the following manner: 1st axis is 1, 2nd axis is 2, and so forth.

When using multiple part system, the 1st axis in each part system is set as 1, the second axis is set as 2, and so forth.

(Note 6)

Command G10L50, L11 in independent blocks. A program error (P33, P421) will occur if not commanded in independent blocks.


(Example) To turn ON bit 2 of bit selection #6401

G10 L50 ;

P8 N1 H21 ;

G11 ;

243


13.10 Macro interrupt

13.10 Macro interrupt ; M96, M97


A user macro interrupt signal (UIT) is input from the machine to interrupt the program being currently executed and instead call another program and execute it. This is called the user macro interrupt function.

Use of this function allows the program to operate flexibly enough to meet varying conditions.

For setting the parameters of the function, refer to the Operation manual and the machine parameters in Appendix 1.

Command format

M96 P__ H__ ;

M97 ;

P

H

User macro interrupt enable

User macro interrupt disable

:Interrupt program number

:Interrupt sequence number

The user macro interrupt function is enabled and disabled by the M96 and M97 commands programmed to make the user macro interrupt signal (UIT) valid or invalid. That is, if an interrupt signal (UIT) is input from the machine side in a user macro interrupt enable period from when M96 is issued to when M97 is issued or the NC is reset, a user macro interrupt is caused to execute the program specified by P__ instead of the one being executed currently.

Another interrupt signal (UIT) is ignored while one user macro interrupt is being in service. It is also ignored in a user macro interrupt disable state such as after an M97 command is issued or the system is reset.

M96 and M97 are processed internally as user macro interrupt control M codes.

Interrupt enable conditions

A user macro interrupt is enabled only during execution of a program. The requirements for the user macro interrupt are as follows :

(1) An automatic operation mode memory, or MDI has been selected.

(2) The system is running in automatic mode.

(3) No other macro interrupt is being processed.

(Note 1)

A macro interrupt is disabled in manual operation mode (JOG, STEP, HANDLE, etc.)

244


Outline of operation


(1) When a user macro interrupt signal (UIT) is input after an M96Pp1 ; command is issued by the current program, interrupt program Op1 is executed. When an M99; command is issued by the interrupt program, control returns to the main program.

M99Pp

2

; is specified, the blocks from the one next to the interrupted block to the last one are searched for the block with sequence number Np2 ;. Control thus returns to the block with sequence number Np2 that is found first in the above search.

Current program

Interrupt program

User macro interrupt signal

(UIT)

M96Pp1;

Interrupt signal (UIT) not acceptable within a user macro program

Op1 ;

M99(Pp2) ;

(If Pp2 is specified)

Np2 ;

Np2 ;

M97 ;

245


Interrupt type


Interrupt types 1 and 2 can be selected by the parameter "#1113 INT_2".

[Type 1]

•

When an interrupt signal (UIT) is input, the system immediately stops moving the tool and interrupts dwell, then permits the interrupt program to run.

•

If the interrupt program contains a move or miscellaneous function (MSTB) command, the commands in the interrupted block are lost. After the interrupt program completes, the main program resumes operation from the block next to the interrupted one.

•

If the interrupted program contains no move and miscellaneous (MSTB) commands, it resumes operation, after completion of the interrupt program, from the point in the block where the interrupt was caused.

If an interrupt signal (UIT) is input during execution of a miscellaneous function (MSTB) command, the NC system waits for a completion signal (FIN). The system thus executes a move or miscellaneous function command (MSTB) in the interrupt program only after input of FIN.

[Type 2]

•

When an interrupt signal (UIT) is input, the program completes the commands in the current block, then transfers control to the interrupt program.

•

If the interrupt program contains no move and miscellaneous function (MSTB) commands, the interrupt program is executed without interrupting execution of the current block.

However, if the interrupt program has not ended even after the execution of the original block is completed, the system may stop machining temporarily.

246


[Type 1]

Main program

block(1) block(2) block(3)


If the interrupt program contains a move or miscellaneous function command, the reset block (2) is lost. block(3)

block(1) block(2)

Interrupt program

block(1)

User macro interrupt block(2) block(2)

If the interrupted program contains no move and miscellaneous commands, it resumes operation from where it left in block (2), that is, all the reset commands. block(3)

Interrupt program

User macro interrupt

[Type 2]

Main program

block(1) block(2) block(3)

Executing

block(1) block(2)

Interrupt program


block(1) block(2)

Interrupt program

User macro interrupt block(3)

If the interrupted program contains no move and miscellaneous commands, the interrupted program is kept executed in parallel to execution of the interrupt program block (3). block(3)

The move or miscellaneous command in the interrupt program is executed after completion of the current block.

247


Calling method


User macro interrupt is classified into the following two types depending on the way an interrupt program is called. These two types of interrupt are selected by parameter "#1229 set01/bit0".

Both types of interrupt are included in calculation of the nest level. The subprograms and user macros called in the interrupt program are also included in calculation of the nest level. a. Subprogram type interrupt b. Macro type interrupt

Subprogram type interrupt The user macro interrupt program is called as a subprogram.

As with calling by M98, the local variable level remains unchanged before and after an interrupt.

Macro type interrupt The user macro interrupt program is called as a user macro. As with calling by G65, the local variable level changes before and after an interrupt.

No arguments in the main program can be passed to the interrupt program.

Acceptance of user macro interrupt signal (UIT)

A user macro interrupt signal (UIT) is accepted in the following two modes: These two modes are selected by a parameter "#1112 S_TRG". a. Status trigger mode b. Edge trigger mode

Status trigger mode

Edge trigger mode

The user macro interrupt signal (UIT) is accepted as valid when it is on.

If the interrupt signal (UIT) is ON when the user macro interrupt function is enabled by M96, the interrupt program is activated.

By keeping the interrupt signal (UIT) ON, the interrupt program can be executed repeatedly.

The user macro interrupt signal (UIT) is accepted as valid at its rising edge, that is, at the instance it turns on.

This mode is useful to execute an interrupt program once.

User macro interrupt signal (UIT)

ON

OFF

(Status trigger mode)

User macro interrupt

(Edge trigger mode)

Accepting user macro interrupt signal (UIT)

248


Returning from user macro interrupt


M99 (P__) ;

An M99 command is issued in the interrupt program to return to the main program. Address P is used to specify the sequence number of the return destination in the main program. The blocks from the one next to the interrupted block to the last one in the main program are first searched for the block with sequence number Np2;. If it is not found, all the blocks before the interrupted one are then searched. Control thus returns to the block with sequence number Np2; that is found first in the above search.

(This is equivalent to M99P__ used after M98 calling.)

249


Modal information affected by user macro interrupt


If modal information is changed by the interrupt program, it is handled as follows after control returns from the interrupt program to the main program.

Returning with M99;

Returning with M99P__;

The change of modal information by the interrupt program is invalidated and the original modal information is not restored.

With interrupt type 1, however, if the interrupt program contains a move or miscellaneous function (MSTB) command, the original modal information is not restored.

The original modal information is updated by the change in the interrupt program even after returning to the main program.

This is the same as in returning with M99P__; from a program called by M98.

Main program being executed

M96Pp1 ;

Interrupt program

Op1 ;

(Modal change)


(UIT)

Modal before interrupt is restored.

M99(p2) ;

(With Pp2 specified)

Np2 ;

Modal modified by interrupt program remains effective.

Modal information affected by user macro interrupt

250


Modal information variables (#4401 to #4520)


Modal information when control passes to the user macro interrupt program can be known by reading system variables #4401 to #4520.

The unit specified with a command applies.

System variable

#4401 to #4421


G code (group 01 to group 21) Some groups are not used.

The above system variables are available only in the user macro interrupt program. If they are used in other programs, program error (P241) results.

M code for control of user macro interrupt

The user macro interrupt is controlled by M96 and M97. However, these commands may have been used for other operation. To be prepared for such case, these command functions can be assigned to other M codes.

(This invalidates program compatibility.)

User macro interrupt control with alternate M codes is possible by setting the alternate M code in parameters "#1110 M96_M" and "#1111 M97_M" and by validating the setting by selecting parameter "#1109 subs_M".

(M codes 03 to 97 except 30 are available for this purpose.)

If the parameter "#1109 subs_M" used to enable the alternate M codes is not selected, the M96 and M97 codes remain effective for user macro interrupt control.

In either case, the M codes for user macro interrupt control are processed internally and not output to the outside.

251



Parameters

Refer to the Instruction Manual for details on the setting methods.

(1) Subprogram call validity "#1229 set 01/bit 0"

1 : Subprogram type user macro interrupt

0 : Macro type user macro interrupt

(2) Status trigger mode validity "#1112 S_TRG"

1 : Status trigger mode

0 : Edge trigger mode

(3) Interrupt type 2 validity "#1113 INT_2"

1 : The executable statements in the interrupt program are executed after completion of execution of the current block. (Type 2)

0 : The executable statements in the interrupt program are executed before completion of execution of the current block. (Type 1)

(4) Validity of alternate M code for user macro interrupt control "#1109 subs_M"

1 : Valid

0 : Invalid

(5) Alternate M codes for user macro interrupt

Interrupt enable M code (equivalent to M96) "#1110 M96_M"

Interrupt disable M code (equivalent to M97) "#1111 M97_M"

M codes 03 to 97 except 30 are available.

Restrictions

(1) If the user macro interrupt program uses system variables #5001 and after (position information) to read coordinates, the coordinates pre-read in the buffer are used.

(2) If an interrupt is caused during execution of the tool diameter compensation, a sequence number (M99P__;) must be specified with a command to return from the user macro interrupt program. If no sequence number is specified, control cannot return to the main program normally.

252


13.11 Tool change position return

13.11 Tool change position return ; G30.1 to G30.6


By specifying the tool change position in a parameter "#8206 TOOL CHG. P" and also specifying a tool change position return command in a machining program, the tool can be changed at the most appropriate position.

The axes that are going to return to the tool change position and the order in which the axes begin to return can be changed by commands.

Command format

(1) The format of tool change position return commands is as follows.

G30. n;

n = 1 to 6 : Specify the axes that return to the tool change position and the order in which they return.

For the commands and return order, see next table.

G30.1

G30.2

G30.3

G30.4

G30.5

G30.6

Z axis

→

X axis

•

Y axis

Z axis

→

X axis

→

Y axis

Z axis

→

Y axis

→

X axis

X axis

→

Y axis

•

Z axis

Y axis

→

X axis

•

Z axis

X axis

•

Y axis

•

Z axis

(

→

added axis)

(

→

added axis)

(

(

(

(

→

→

→

→

added axis)

added axis)

added axis)

added axis)

(Note 1)

An arrow (

→

) indicates the order of axes that begin to return. An period (

•

) indicates that the axes begin to return simultaneously. (Example : "Z axis

→

X axis,

Y axis" indicate that the Z axis returns to the tool change position, then the X and Y axes does.)

(2) The tool change position return on/off for the added axis can be set with parameter "#1092

Tchg_A" for the added axis.

Note, however, that the added axis always return to the tool change position only after the standard axes complete returning (see the above table).

The added axis alone cannot return to the tool change position.

253


Example of operates


(1) The figure below shows an example of how the tool operates during the tool change position return command. (Only operations of X and Y axes in G30.1 to G30.3 are figured.)

Y

G30.3

Tool changing position

G30.1

G30.2

X

1) G30.1 command: The Z axis returns to the tool change position, then the X and Y axes simultaneously do the same thing. (If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X, Y and Z axes reach the tool change position.)

2) G30.2 command: The Z axis returns to the tool change position, then the X axis does the same thing. After that, the Y axis returns to the tool change position.

(If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X, Y and Z axes reach the tool change position.)

3) G30.3 command: The Z axis returns to the tool change position, then the X axis does the same thing. After that, the X axis returns to the tool change position.

(If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X and Z axes reach the tool change position.)

4) G30.4 command: The X axis returns to the tool change position, then the Y axis and Z axis simultaneously do the same thing.

(If tool change position return is on for an added axis, the added axis also return to the tool change position after the X, Y and X axes reach the tool change position.)

5) G30.5 command: The Y axis returns to the tool change position, then the X and Z axes return to the tool change position simultaneously.


6) G30.6 command: The X, Y and Z axes return to the tool change position simultaneously.


254



(2) After all necessary tool change position return is completed by a G30.n command, tool change position return complete signal TCP (X64B) is turned on. When an axis out of those having returned to the tool change position by a G30.n command leaves the tool change position, the

TCP signal is turned off.

With a G30.1 command, for example, the TCP signal is turned on when the Z axis has reached the tool change position after the X and Y axes did (after the additional axis did if additional axis tool change position return is valid). The TCP signal is then turned off when the

X or Y axis leaves the position. If tool change position return for added axes is on with parameter "#1092 Tchg_A", the TCP signal is turned on when the added axis or axes have reached the tool change position after the standard axes did. It is then turned off when one of the X, Y, Z, and added axes leaves the position.

[TCP signal output timing chart] (G30.3 command with tool change position return for added axes set on)

Work program

Arrival of Z axis to tool change position

Arrival of X, Y axes to tool change position

Arrival of added axis to tool change position

Tool change position return complete signal (TCP)

G30.3;

T02; G00X-100.

• • •

(3) When a tool change position return command is issued, tool offset data such as for tool length offset and tool radias compensation for the axis that moved is canceled.

(4) This command is executed by dividing blocks for every axis. If this command is issued during single-block operation, therefore, a block stop occurs each time one axis returns to the tool change position. To make the next axis return to the tool change position, therefore, a cycle start needs to be specified.

255


13.12 High-accuracy control

13.12 High-accuracy control; G61.1


Until now, trouble such as the following occurred when using control:

(1) Corner rounding occurred at the corners that linear and linear are connected because the following command movement started before the previous command finished. (Refer to Fig. 1)

(2) When cutting circle commands, an error occurred further inside the commanded path, and the resulting cutting path was smaller than the commanded path. (Refer to Fig. 2)

Commanded path

Commanded path

Actual path

Actual path

Fig. 1 Rounding at linear corners

Fig. 2 Radius reduction error in circle commands

This function controls the operation so the lag is eliminated in control systems and servo systems. With this function, machining accuracy can be improved, especially during high-speed machining, and machining time can be reduced.

The high-accuracy control function is configured of the following functions.

(1) Pre-interpolation acceleration/deceleration (linear acceleration/deceleration)

(2) Optimum speed control

(3) Vector accuracy interpolation

(4) Active feed forward

(5) Arc entrance/exit speed control

256



Command format

G61.1 Ff1 ;

G61.1 : High-accuracy control mode

The high-accuracy control mode is validated from the block containing the G61.1 command.

G64 G61.1

The high-accuracy control mode is canceled with one of the following G commands.

•

G61 (exact stop check)

•

G62 (automatic corner override)

•

G63 (tapping mode)

•

G64 (cutting mode)


(1) The "high-accuracy control" specifications are required to use this function.

If G61.1 is commanded when the specifications are not available, program error (P123) will occur.

(2) The feedrate command F is clamped by the rapid traverse rate or maximum cutting feedrate set with the parameters.

(3) Refer to the "Optimum speed control" mentioned later for details on the speed clamp during an arc command.

(4) The own system waits for the other system to move and reach the designated start point, and then starts.

(5) The modal holding state of the high-accuracy control mode depends on the conditions of the base specification parameter "#1151 rstint" (reset initial) and "#1148 I_G611" (initial high- accuracy).

Parameter

Default state

Reset

Block interruption

Block stop

Emergency stop

NC alarm

OT

Emergency stop cancel

OFF OFF

OFF ON

C

H

ON OFF C

H C C

*

H

*

H H

C C C

H

H

H

H

H

H

H

H

H

H

H

H

H

H

H

H

H

C

ON ON

H

*

H

*

H H H H

(Note)

The cases marked with an asterisk (*) in the above table indicate that the modal will shift to the high-accuracy control mode (G61.1) even in modes other than the high-accuracy control mode (modes G61 to G64).

*

H H H H

H (hold) : Modal hold (G61.1

→

G61.1)

C (cancel) : Modal cancel (G61.1

→

G64)

257



Pre-interpolation acceleration/deceleration

Acceleration/deceleration control is carried out for the movement commands to suppress the impact when the machine starts or stops moving. However, with conventional post-interpolation acceleration/deceleration, the corners at the block seams are rounded, and path errors occur regarding the commanded shape.

In the high-accuracy control function mode, acceleration/deceleration is carried out before interpolation to solve the above problems. This pre-interpolation acceleration/deceleration enables machining on a machining path that more closely follows the command.

The acceleration/deceleration time can be reduced because constant inclination acceleration/ deceleration is carried out.

(1) Basic patterns of acceleration/deceleration control in linear interpolation commands

Normal mode

G1tL G1tL

Time clamp clamp

(a) Because of the constant time constant acceleration/deceleration, the rising edge/falling edge becomes more gentle as the command speed becomes slower.

(b) The acceleration/deceleration time constant can be independently set for each axis.

Linear type, exponential function type, or both can be selected.

Note that if the time constant of each axis is not set to the same value, an error will occur in the path course.

#2002 clamp : G01 clamp speed

#2007 G1tL : Linear type acceleration/ deceleration time constant

#2008 G1t1 : Exponential function type acceleration/deceleration time constant

High-accuracy control mode

G1t1

G1btL/2

G1btL

G1bF

G1bF/2

Time

G1t1 clamp

G1btL/2

G1btL

Time

(a) Because of the constant inclination type linear acceleration/deceleration, the acceleration/ deceleration time is reduced as the command speed becomes slower.

(b) The acceleration/deceleration time constant becomes one value (common for each axis) in the system.

#2002 clamp : G01 clamp speed

#1206 G1bF : Target speed

#1207 G1btL : Acceleration/deceleration time to target speed

G1bF and G1btL are values for specifying the inclination of the acceleration/deceleration time; the actual cutting feed maximum speed is clamped by the "#2002 clamp" value.

258



(2) Path control in circular interpolation commands

When commanding circular interpolation with the conventional post-interpolation acceleration/ deceleration control method, the path itself that is output from the CNC to the servo runs further inside the commanded path, and the circle radius becomes smaller than that of the commanded circle. This is due to the influence of the smoothing course droop amount for CNC internal acceleration/deceleration.

With the pre-interpolation acceleration/deceleration control method, the path error is eliminated and a circular path faithful to the command results, because interpolation is carried out after the acceleration/deceleration control. Note that the tracking lag due to the position loop control in the servo system is not the target here.

The following shows a comparison of the circle radius reduction error amounts for the conventional post-interpolation acceleration/deceleration control and pre-interpolation acceleration/deceleration control in the high-accuracy control mode.

F

F

∆

R

R

R : Commanded radius (mm)

∆

R : Radius error (mm)

F : Cutting feedrate (mm/min)

The compensation amount of the circle radius reduction error (

∆

R) is theoretically calculated as shown in the following table.

Post-interpolation acceleration/deceleration control

(normal mode)

Linear acceleration/deceleration

Pre-interpolation acceleration/deceleration control

(high-accuracy control mode)

Linear acceleration/deceleration

∆

R =

1

2R

1

⎝

12

Ts

2

+ Tp

2

⎠

Exponential function acceleration/deceleration

∆

R =

1

2R

⎝

F

60

⎞

2

(

Ts

2

+ Tp

2

)

F

⎝

60

⎞

2

∆

R =

1

2R

{

Tp

2

(

1

−

Kf

2

)

}

⎝

F

60

⎞

2

(a) Because the item Ts can be ignored by using the pre-interpolation acceleration/deceleration control method, the radius reduction error amount can be reduced.

(b) Item Tp can be negated by making Kf = 1.

Ts : Acceleration/deceleration time constant in the CNC (s)

Tp : Servo system position loop time constant (s)

Kf : Feed forward coefficient

259


Optimum speed control


(1) Optimum corner deceleration

By calculating the angle of the seam between blocks, and carrying out acceleration/ deceleration control in which the corner is passed at the optimum speed, highly accurate edge machining can be realized.

When the corner is entered, that corners optimum speed (optimum corner speed) is calculated from the angle with the next block. The machine decelerates to that speed in advance, and then accelerates back to the command speed after the corner is passed.

Corner deceleration is not carried out when blocks are smoothly connected. In this case, the criteria for whether the connection is smooth or not can be designated by the machining parameter "#8020 DCC ANGLE".

When the corner angle is larger than the parameter "DCC ANGLE" for a linear

− linear connection, or for a circle, etc, and the corner is passed at a speed V, the acceleration

∆

V occurs due to the change in the direction of progress.

θ

V Speed before entering the corner

∆

V Speed change at the corner

V

Speed after the corner is passed

The corner angle V is controlled so that this

∆

V value becomes less than the pre-interpolation acceleration/ deceleration tolerable value set in the parameters ("#1206 G1bF", "#1207

G1btL").

In this case the speed pattern is as follows.

Y axis

X axis

θ

N01 G01X100.Y1.F500 ; N02 G01X100.Y-1.F500 ;

The optimum corner speed is represented by V0.

V0 is obtained from the pre-interpolation acceleration/deceleration tolerable value

(

∆

V') and the corner angle (outside angle)

θ

.

∆

V’ =

G1bF

G1btL

Combined speed pattern

Speed

Time

V0

V0 =

V0x

2

+ V0y

2

To further reduce the corner speed V0

(to further improve the edge accuracy), the V0 value can be reduced in the machining parameter "#8019

R COMPEN".

X axis speed pattern

Speed

Time

Y axis speed pattern

Speed

Time

V0x

V0y

V0’ =

V0

×

(100

−

Ks)

100

Ks: R COMPEN

(Note)

In this case, the cycle time may increase due to the increase in the time required for acceleration/ deceleration.

260



(2) Arc speed clamp

During circular interpolation, even when moving at a constant speed, acceleration is generated as the advance direction constantly changes. When the arc radius is large compared to the commanded speed, control is carried out at the commanded speed. However, when the arc radius is relatively small, the speed is clamped so that the generated acceleration does not exceed the tolerable acceleration/deceleration speed before interpolation, calculated with the parameters.

This allows arc cutting to be carried out at an optimum speed for the arc radius.

∆θ

θ

F

F

F

F

∆

V

F : Commanded speed (mm/min)

R : Commanded arc radius (mm)

∆

θ

: Angle change per interpolation unit

∆

V : Speed change per interpolation unit

The tool is fed with the arc clamp speed F so that

∆

V does not exceed the tolerable acceleration/deceleration speed before interpolation

∆

V.

F

≤

R ×

∆

V × 60 × 1000 (mm/min)

∆

V =

G1bF (mm/min)

G1btL (ms)

When the above F' expression is substituted in the expression expressing the maximum logical arc radius reduction error amount

∆

R explained in the section "a) Pre-interpolation acceleration/deceleration", the commanded radius R is eliminated, and

∆

R does not rely on R.

1

∆

R

≤

2R

{Tp

2

(1

−

Kf

2

F

) } ( )

2

60

1

≤

2R

{Tp

2

(1

−

Kf

2

∆

V’ × 1000

) } ( )

60

∆

R : Arc radius reduction error amount

Tp : Position loop gain time constant of servo system


In other words, with the arc command in the high-accuracy control mode, in logical terms regardless of the commanded speed F or commanded radius R, machining can be carried out with a radius reduction error amount within a constant value.

To further lower the arc clamp speed (to further improve the roundness), the arc clamp speed can be lowered with the machining parameter "#8019 R COMPEN". In this case, speed control is carried out to improve the maximum arc radius reduction error amount

∆

R by the set percentage.

∆

R’

≤

∆

R × (100

−

Ks)

(mm)

∆

R’ : Maximum arc radius reduction error amount

Ks : R COMPEN (%)

100

After setting the "R COMPEN", the above

∆

R' will appear on the parameter screen.

R COMPEN (0.078) 50

Accuracy coefficient setting value

∆

R’

(Note 1)

When the "R COMPEN" is set, the arc clamp speed will drop, so in a machining program with many arc commands, the machining time will take longer.

(Note 2)

The "R COMPEN" is valid only when the arc speed clamp is applied. To reduce the radius reduction error when not using the arc speed clamp, the commanded speed F must be lowered.

261


Vector accuracy interpolation


When a fine segment is commanded and the angle between the blocks is extremely small (when not using optimum corner deceleration), interpolation can be carried out more smoothly using the vector accuracy interpolation.

Vector accuracy interpolation

Commanded path

Feed forward control

With this function, the constant speed error caused by the position loop control of the servo system can be greatly reduced. However, as machine vibration is induced by the feed forward control, there are cases when the coefficient cannot be increased.

In this case, use this function together with the smooth high gain (SHG) control function and stably compensate the delay by the servo system's position loop to realize a high accuracy. As the response is smoother during acceleration/deceleration, the position loop gain can be increased.

(1) Active feed forward control

Command during acceleration/ deceleration before interpolation

Command during acceleration/ deceleration after interpolation

+

+

−

Active feed forward control

Kp

+

−

Kv

Kp : Position loop gain

Kv : Speed loop gain

M : Motor

M

Detector

Machine error compensation amount

S

262



(2) Reduction of arc radius reduction error amount using feed forward control

With the high-accuracy control, the arc radius reduction error amount can be greatly reduced by combining the pre-interpolation acceleration/deceleration control method above-mentioned and the active feed forward control/SHG control.

The logical radius reduction error amount

∆

R in the high-accuracy control mode is obtained with the following expression.

Active feed forward control SHG control + active feed forward control

∆

R

≤

1

2 R

{ T p

2

( 1

−

K f

2

F

) } ( )

6 0

2

R : Arc radius (mm)

F : Cutting feedrate (mm/min)

Tp : Position loop time constant (s)


By setting Kf to the following value, the delay elements caused by the position loop in the servo system can be eliminated, and the logical

∆

R can be set to 0.

Kf = 1 (Feed forward gain 100%) The equivalent feed forward gain to set Kf to 1 can be obtained with the following expression.

100 1

⎧

⎨

1

50

⎞

2

⎫

⎬

⎛

PGN1 for conventional control

⎟

2 × PGN1 for SHG control

⎞

2

The feed forward gain can be set independently for G00 and G01.

F

∆

R

R

Path for pre-interpolation acceleration/deceleration control method (Kf = 1)

Path for pre-interpolation acceleration/deceleration control method (Kf = 0)

Path for post-interpolation acceleration/deceleration control method

(Note)

If the machine vibrates when Kf is set to 1, Kf must be lowered or the servo system must be adjusted.

263


Arc entrance/exit speed control


There are cases when the speed fluctuates and the machine vibrates at the joint from the straight line to arc or from the arc to straight line.

This function decelerates to the deceleration speed before entering the arc and after exiting the arc to reduce the machine vibration. If this is overlapped with corner deceleration, the function with the slower deceleration speed is valid.

The validity of this control can be changed with the base specification parameter "#1149 cireft".

The deceleration speed is designated with the base specification parameter "#1209 cirdcc".

(Example 1)

When not using corner deceleration

<Program>

G61.1 ;

•

•

N1 G01 X-10. F3000 ;

N2 G02 X-5. Y-5. J-2.5 ;

N3 G01 Y-10. ;

•

•

<Operation>

N2

N3

N1

<Deceleration pattern>

Speed

Commanded speed

N1

N2

N3

Arc clamp speed

Arc deceleration speed

Time

264


(Example 2) When using corner deceleration

<Program>

G61.1 ;

•

•

N1 G01 X-10. F3000 ;

N2 G02 X5. Y-5. I2.5 ;

N3 G01 X10. ;

•

•

<Deceleration pattern>

Speed

Commanded speed

Arc clamp speed

Arc deceleration speed

Corner deceleration speed

N1


<Operation>

N1

N2

N3

N2 N3

Time

265


13.13 Synchronizing operation between part systems


CAUTION

When programming a multi-part system, carefully observe the movements caused by other part systems' programs.


The multi-axis, multi-part system complex control NC system can simultaneously run multiple machining programs independently. The synchronizing-between-part systems function is used in cases when, at some particular point during operation, the operations of part systems 1 and 2 are to be synchronized or in cases when the operation of only one part system is required.

Part system 1 machining program

Part system 2 machining program

! ......;

! ......;

No program

! ......;

%

! ......;

! ......;

! ......;

%

Simultaneous and independent operation

←

Synchronized operation

Simultaneous and independent operation

←


Part system 2 operation only; part system 1 waiting

←


Simultaneous and

independent operation

266



Command format

(1) Command for synchronizing with nth part system

!nLl; n : Part system number l : Synchronizing number 01 to 9999

$1 $2 $3

!2L1;


!1L1;

!1L2;

!3L2;


(2) Command for synchronizing among three part systems

!n!m

･･･

Ll; n, m : Part system number n = m l : Synchronizing number 01 to 9999

$1 $2 $3

!2!3L1;


!1!3L1;

!1!2L1;


267




(1) When the "!nLl" code is issued from the part system "i", the operation of that program will wait until the "!iLl" code is issued from the part system "n".

When the "!iLl" code is issued, the programs of both part systems "i" and "n" will start running simultaneously.

Part system "i" program

Pi1

Part system "n" program

Pn1

!nLl;


!iLl;

Pi2 Pn2

Part system "m" program

Pm1

Part system "i"

Part system "n"

Pn1

Simultaneous start

Pn2

Pm1

Part system "m"

(2) Synchronizing among three part systems is as follows. When the "!n!mLl" command is issued from the part system "i", the program of part system "i" operation will wait until the "!i!mLl" command is issued from the part system "n" and the "!i!nLl" command is issued from the part system "m".

When the synchronizing commands are issued, programs of part systems "i", "n" and "m" will start operating simultaneously.

Part system "i" program

Pi1

!n!mLl;


Part system "n" program

Pn1

!i!mLl;


Pi2 Pn2

Part system "m" program

Pm1

!i!nLl;

Pm2

Part system "i"

Part system "n"

Pn1

Waiting

Part system "m"

Pn2

Pm1 Pm2

Simultaneous start

268



(3) Program error (P35) occurs when an illegal system number has been issued.

(4) The synchronizing command is normally issued in a single block. However, if a movement command or M, S or T command is issued in the same block, whether to synchronize after the movement command or M, S or T command or to execute the movement command or M, S or

T command after synchronization will depend on the parameter (#1093 Wmvfin).

#1093 Wmvfin 0: Synchronize before movement command execution.

1: Synchronize after executing movement command.

(5) If there is no movement command in the same block as the synchronizing command, when the next block movement starts, synchronization may not be secured between the part systems.

To synchronize the part systems when movement starts after synchronization, issue the movement command in the same block as the synchronizing command.

(6) Synchronizing is done only while the part system to be synchronized is operating automatically.

If this is not possible, the synchronizing command will be ignored and operation will advance to the next block.

(7) The L command is the synchronizing identification number. The same numbers are synchronized but when they are omitted, the numbers are handled as L0.

(8) The synchronizing command designates the number of the other part system number to be synchronized, and can also be issued along with its own part system number.

(Example)

Part system "i" command: !i!n!mLl;

(9) When the part system No. is omitted (when only "!" is issued), part system 1 will be handled as

"!2" and part system 2 as "!1". The command using only "!" cannot be used for synchronizing with part system 3 and following.

If the command using only "!" is used for part system 3 or following, the program error (P33) will occur.

(10) "SYN" will appear in the operation status section during synchronization. The synchronizing signal will be output to the PLC I/F. ($1: X63C, $2: X6BC, $3: X73C, $4: X7BC, $5: X83C, $6:

X8BC, $7: X93C)

269



Example of synchronizing between part systems

$1 $2

P11

P21

$3

!2L2;

P31

!2L1;

P12

!1L1;

P22

!1!2L3;

P32

!1L4;

P33

!2!3L3;

P13

!3L2;

P23

!3L4;

P14

!1!3L3;

P24

The above programs are executed as follows:

$1

$2

$3

P11 P12

L1

P21 P22 P23

L2

P31

P13

L3

P24

L3

P32

L4

P14

P33

270


13.14 Start Point Designation Synchronizing (Type 1)

13.14 Start Point Designation Synchronizing (Type 1); G115


The part system can wait for the other part system to reach the start point before starting itself.

The synchronization point can be set in the middle of a block.

Command format

!nL1 G115 X_ Z_ C_ ;

X_ Z_ C_ Start point (Command axis and workpiece coordinate values for checking synchronization of other part system.)


(1) Designate the start point using the workpiece coordinates of the other part system.

(2) The start point check is executed only for the axis designated by G115.

(Example)

!L2 G115 X100.;

Once the other part system reaches X100., the own part system will start. The other axes are not checked.

(3) The other part system starts first when synchronizing is executed.

(4) The own part system waits for the other part system to move and reach the designated start point, and then starts.

Own part system !G115

Other part system


！

Designated start point



Other part system

！


271



(5) When the start point designated by G115 is not on the next block movement path of the other part system, the own system starts once the other part system has reached all of the start point axis coordinates.

例

X also has passed

Z has passed

X

: Movement : Command point

: Actual start point

Z

(6) The following operation is executed by parameters (base specification parameter #1229 set01/bit5) when the start point cannot be determined by the next block movement of the other system.

(a) When the parameter is ON

Operation waits until the start point is reached by the movement in the next and subsequent blocks.

Own part system

!G115

Waiting

Other part system

!

(b) When the parameter is OFF

The own part system starts upon completion of the next block movement.

Own part system

!G115

Other part system

!

(7) The waiting status continues when the G115 command has been duplicated between part systems.

(8) Designate the start point using the workpiece coordinates of the other part system.

(9) Program error "P33" occurs when the G115 command is issued for 3 part systems.

(10) The single block stop function does not apply for the G115 block.

(11) When the G115 command is issued continuously in 2 or more blocks, the block in which it was issued last will be valid.

(12) A program error (P32) will occur if an address other than an axis is designated in G115 command block.

272



13.15 Start Point Designation Synchronizing (Type 2); G116


Starting of the other part system can be delayed until the own part system reaches the designated start point.

The synchronization point can be set in the middle of a block.

Command format

!nL1 G116 X_ Z_ C_ ;

X_ Z_ C_ Start point (Command axis and workpiece coordinate values for checking synchronization of own part system.)


(1) Designate the start point using the workpiece coordinates of the own part system.

(2) The start point check is executed only for the axis designated by G116.

(Example)

!L1 G116 X100.;

Once the own part system reaches X100., the other part system will start. The other axes are not checked.

(3) The own part system starts first when synchronizing is performed.

(4) The other part system waits for the own part system to move and reach the designated start point, and then starts.


! G116

Own part system

Other part system

Own part system

Other part system !

!


! G116



273



(5) When the start point designated by G116 is not on the next block movement path of the own system, the other system starts once the own system has reached all of the start point axis coordinates.

例

X also has passed

Z has passed

X

Z

: Movement

: Command point : Actual start point

(6) The next operation is executed by parameters (base specification parameter #1229 set01/bit5) when the start point cannot be determined by the next block movement of the own part system.

(a) When the parameter is ON

Program error "P33" occurs before the own part system moves.

Own part system

!G116

Program error

Other part system

!

Waiting

(b) When the parameter is OFF

The other part system starts upon completion of the next block movement.


Other part system

!

(7) If the G116 command overlaps between part systems, the waiting state will continue.

Own part system

!L1 G116

Waiting

Other part system

!L1 G116

(8) Designate the start point using the workpiece coordinates of each part system.

274



(9) The two other part systems start when the G116 command is issued for 3 part systems.

Own part system !2!3 L1 G116

Other part system A

!1!3 L1

Other part system B

!1!2 L1

(10) The single block stop function does not apply for the G116 block.

(11) When the G116 command is issued continuously in 2 or more blocks, the block in which it was issued last will be valid.

(12) A program error (P32) will occur if an address other than an axis is designated in G116 command block.

275


13.16 Miscellaneous function output during axis movement

13.16 Miscellaneous function output during axis movement; G117


This function controls the timing of the miscellaneous function to be output. The miscellaneous function is output when the position designated in axis movement is reached.

Command format

G117 X_ Z_ M_ S_ T_ (2nd M)_ ;

X Z

M_ S_ T_ (2nd M)_


Start point of operation

Miscellaneous function

(1) This command is issued independently immediately before the block with the movement command that activates the miscellaneous function.

(2) Single block stop does not apply to this command.

(3) The maximum number of groups to which the miscellaneous functions in the G117 block can be issued is as follows:

M commands : 4 sets

S commands

T commands

: 2 sets

: 1 set

2nd miscellaneous function : 1 set

(4) This command can be issued in up to two consecutive blocks.

When issued in three or more consecutive blocks, the last two blocks will be valid.

(Example)

G117 Xx1 Zz1 Mm1 Mm2 Mm3 Mm4;

G117 Xx2 Zz2 Mm5 Mm6 Mm7 Mm8;

G01 X200 Z200;

Mm1

Mm2

Mm3

Mm4

(x2,z2)

End point (200,200)

Start point

(x1,z1)

Mm5

Mm6

Mm7

Mm8

(5) When the operating start point commanded by G117 is not on the movement path, the miscellaneous function will be output once the movement has reached all the coordinate values of the operating start point. In addition, only the commanded axis is checked.

(Example)

G117 X100. M

××

; M

××

is output when X100. is reached.

(Note)

The other axes are not subject to the check.

(6) The completion of the miscellaneous function in the previous group is checked at the operating start point, and the miscellaneous function of the next group is output. Thus, normal PLC interfacing is possible.

276


13.16 Miscellaneous function output during axis movement

(7) A miscellaneous function issued in the same block as the block with the movement command is output before the movement and starts the movement. During movement, operation will not stop at the operating start point. However, at the end point of the block, the completion of all the miscellaneous functions is checked first, and then the execution of the next block is started.

(8) G117 should be issued in the sequence of operating start points. Program error (P33) occurs if the sequence of the operating start point is the reverse of the movements.

When operating start points coincide, the miscellaneous functions are output in the sequence in which they were issued.

(9) When an operating start point cannot be determined by the next block movement, the next operation is performed by the parameter.

Basic specification parameter

"#1229 set01/bit5"

ON

OFF

Not during intermediate point movement

Refer to (9) for second block.

Operation

Program error P33 occurs before movement

The functions are output when the next block movement is completed.

(10) The following tables show the combinations of (8) and (9).

G17 First block

Second block

During intermediate point movement

During intermediate point movement

Refer to (8).

Not during intermediate point movement

Program error (P33) due to (8).

Refer to (9).

With output, the sequence of first block, second block is followed regardless of the sequence of the designated points.

Precautions

(1) Command G117 in order of the operation start points. If the operation start point order is the opposite of the movement, a program error (P33) will occur.

277

14. Coordinates System Setting Functions

14.1 Coordinate words and control axes


14.1 Coordinate words and control axes


There are three controlled axis for the basic specifications, but when an additional axis is added, up to 14 axes can be controlled. Pre-determined alphabetic coordinate words that correspond to the axes are used to designate each machining direction.

For XY table

+Z

+Z

+Y

+X

Program coordinates

Workpiece

XY table

+Y

Table movement direction

Bed

+X


For XY table

For XY and rotary table

+X


+Y

Workpiece

+C

+Z

Table rotation direction

+Y

+C

+X

Program coordinates

278


14.2 Basic machine, work and local coordinate systems

14.2 Basic machine, work and local coordinate systems


The basic machine coordinate system is fixed in the machine and it denotes that position which is determined inherently by the machine.

The work coordinate systems are used for programming and in these systems the reference point on the workpiece is set as the coordinate zero point. the local coordinate systems are created on the work coordinate systems and they are designed to facilitate the programs for parts machining.

R#1

Reference point

W3 (Workpiece 3 coordinate system)


W4 (Workpiece 4

M


(Basic machine coordinate system)


W1

W2

M

R#1

279


14.3 Machine zero point and 2nd, 3rd, 4th reference points (Zero point)

14.3 Machine zero point and 2nd, 3rd, 4th reference points (Zero point)


The machine zero point serves as the reference for the basic machine coordinate system. It is inherent to the machine and is determined by the reference (zero) point return.

2nd, 3rd and 4th reference (zero points) points (zero points) relate to the position of the coordinates which have been set beforehand by parameter from the zero point of the basic machine coordinate system.

2nd reference point


Machine zero point x y y

(X

1

,Y

1

)

(X

2

,Y

2

) x

Local coordinate system y

G52 coordinate system x

1st reference point

3rd reference point

4th reference point

280


14.4 Basic machine coordinate system selection

14.4 Basic machine coordinate system selection ; G53


The basic machine coordinate system is the coordinate system that expresses the position (tool change position, stroke end position, etc.) that is characteristic to the machine.

The tool is moved to the position commanded on the basic machine coordinate system with the

G53 command and the coordinate command that follows.

Command format

Basic machine coordinate system selection

(G90) G53 Xx Yy Zz

αα

;

αα

:Additional


(1) When the power is switched on, the basic machine coordinate system is automatically set as referenced to the reference (zero) point return position, which is determined by the automatic or manual reference (zero) point return.

(2) The basic machine coordinate system is not changed by the G92 command.

(3) The G53 command is valid only in the block in which it has been designated.

(4) In the incremental value command mode (G91), the G53 command provides movement with the incremental value in the coordinate system being selected.

(5) Even if G53 is commanded, the tool diameter offset amount for the commanded axis will not be canceled.

(6) The 1st reference point coordinate value indicates the distance from the basic machine coordinate system 0 point to the reference point (zero point) return position.

(7) The G53 commands will all move with rapid traverse.

(8) If the G53 command and G28 command (reference point return) are issued in the same block, the command issued last will be valid.

(500,500)

-X

M

R#1

Reference (zero) point return position (#1)


1st reference point coordinates

X = +500 Y = +500

-Y

281


14.5 Coordinate system setting

14.5 Coordinate system setting ;G92


By commanding G92, the absolute value (workpiece) coordinate system and current position display value can be preset in the command value without moving the machine.

Command format

G92 Xx

1

Yy

1

Zz

1

αα

1

;

αα

:Additional


(1) After the power is turned on, the first reference point return will be done with dog-type, and when completed, the coordinate system will be set automatically. (Automatic coordinate system setting)

R


R,M

Reference point return completed

Power ON position

Reference point return

The basic machine coordinate system and workpiece coordinate system are created at the preset position.

Power ON position

100.

Workpiece coordinate system

[Current value]

X 0.000

Y 0.000

[Workpiece]

X 300.000

Y 200.000

WG54 100. 200.

(2) By commanding G92, the absolute value (workpiece) coordinate system and current position display value can be preset in the command value without moving the machine.

200.

100.

[Tool position]

50.

R,M

[Current value]

X -200.000

Y -150.000

[Workpiece]

X 100.000

Y 50.000

Coordinate system setting

For example, if

G92X 0 Y 0; is commanded, the workpiece coordinate system will be newly created.

-100

[Tool position]

100.

WG54'100. 200.

-50.

R,M

[Current value]

X 0.000

Y 0.000

[Workpiece]

X 0.000

Y 0.000

WG54 100. 200. 300.

WG54

(Note)

If the workpiece coordinate system deviated because the axis is moved manually when the manual absolute position switch is OFF, etc., the workpiece coordinate system can be corrected with the following steps.

(1) Execute reference point return while the coordinate system is deviated.

(2) After that, command G92G53X0Y0Z0;. With this command, the workpiece coordinate value and current value will be displayed, and the workpiece coordinate system will be preset to the offset value.

282


14.6 Automatic coordinate system setting

14.6 Automatic coordinate system setting


This function creates each coordinate system according to the parameter values input beforehand from the setting and display unit when the reference point is reached with the first manual reference point return or dog-type reference point return when the NC power is turned ON.

Basic machine coordinate

Machine zero point y

1 x

1 y

3 y

2

1st reference point



3


2 y

4




4


(1) The coordinate systems created by this function are as follow:

(a) Basic machine coordinate system

(b) Work coordinate systems (G54 to G59)

(2) The parameters related to the coordinate system all provide the distance from the zero point of the basic machine coordinate system. Therefore, it is decided at which position in the basic machine coordinate system the first reference point should be set and then the zero point positions of the work coordinate systems are set.

(3) When the automatic coordinate system setting function is executed, the following functions are canceled: workpiece coordinate system shift based on G92, local coordinate system setting based on G52, workpiece coordinate system shift based on origin setting and workpiece coordinate system shift based on manual interrupt.

(4) When a parameter has been used to select the dog-type of first manual reference point return or automatic reference point return after the power has been turned ON, the dog-type reference point return will be executed for the 2nd and subsequent manual reference point returns or automatic reference point returns.

CAUTION

If the workpiece coordinate offset amount is changed during automatic operation

(including single block operation), the changes will be valid from the next block of the command several blocks later.

283


14.7 Reference (zero) point return

14.7 Reference (zero) point return; G28, G29


(1) After the commanded axes have been positioned by G0, they are returned respectively at rapid traverse to the first reference (zero) point when G28 is commanded.

(2) By commanding G29, the axes are first positioned independently at high speed to the G28 or

G30 intermediate point and then positioned by G0 at the commanded position.

2nd reference point

(0,0,0,0) Machine zero point

Reference point

(x

3

,y

3

,z

3

,

α

3

)

G30P2

G28

G28

G29

Start point

G30

(x

1

,y

1

,z

1

,

α

1

)

Intermediate point

G30P3

G30P4

(x

2

,y

2

,z

2

,

α

2

)

G29

4th reference point

3th reference point

Command format

G28 Xx

1

Yy

1

G29 Xx

αα

1

/

αα

2

2

Yy

2

Zz

1

αα

1

; Automatic reference point return

Zz

2

αα

2

; Start position return

: additional axis

284




(1) The G28 command is equivalent to the following:

G00 Xx

1

Yy

1

Zz

1

G00 Xx

3

Yy

3

Zz

3

In this case, x

3

, y

3

αα

1

;

, z

3

αα

3

;

and

α

3

are the reference point coordinates and they are set by a parameter “#2037 G53ofs” as the distance from the zero point of the basic machine coordinate system.

(2) After the power has been switched on, the axes which have not been subject to manual reference (zero) point are returned by the dog type of return just as with the manual type. In this case, the return direction is regarded as the command sign direction. If the return type is straight-type return, the return direction will not be checked. For the second and subsequence returns, the return is made at high speed to the reference (zero) point which was stored at the first time and the direction is not checked.

(3) When reference (zero) point return is completed, the zero point arrival output signal is output and also #1 appears at the axis name line on the setting and display unit screen.

(4) The G29 command is equivalent to the following:

G00 Xx

1

Yy

1

Zz

1

αα

1

;

Rapid traverse (non-interpolation type) applies

G00 Xx

2

Yy

2

Zz

2

αα

2

; independently for each axis for the positioning from the reference point to the intermediate point.

In this case, x

1

, y

1

, z

1

and

α

1

are the coordinates of the G28 or G30 intermediate point.

(5) Program error (P430) results when G29 is executed if automatic reference (zero) point return

(G28) is not performed after the power has been switched on.

(6) When the Z axis is canceled, the movement of the Z axis to the intermediate point will be ignored, and only the position display for the following positioning will be executed. (The machine itself will not move.)

(7) The intermediate point coordinates (x

1

, y

1

, z

1

,

α

1

) of the positioning point are assigned by the position command modal. (G90, G91).

(8) G29 is valid for either G28 or G30 but the commanded axes are positioned after a return has been made to the latest intermediate point.

(9) The tool offset will be canceled during reference point return unless it is already canceled, and the offset amount will be cleared.

(10) Control from the intermediate point to the reference (zero) point is ignored for reference (zero) point return in the machine lock status. The next block is executed when the commanded axis survives as far as the intermediate point.

(11) Mirror image is valid from the start point to the intermediate point during reference (zero) point return in the mirror image mode and the tool will move in the opposite direction to that of the command. However, mirror image is ignored from the intermediate point to the reference

(zero) point and the tool will move to the reference (zero) point.

285




(Example1)

G28 Xx

1

Zz

1

;

R

Reference (zero) point position (#1)

1st operation after power has been switched on

2nd and subsequent operations

G0Xx

3

Zz

3

;

(x

1

,z

1

)

Intermediate point

Return start position

G0Xx

1

Zz

1

;

1st operation after power has been switched on

2nd and subsequent operations

Rapid traverse rate

Near-point dog

Reference (zero) point position (#1)

R

286



(Example2)

G29 Xx

2

Zz

2

;

R

Present position

(G0)Xx

1

Zz

1

;

G28, G30 intermediate point (x

1

, z

1

)

G0 Xx

2

Zz

2

;

(x

2

,z

2

)

(Example 3)

G28 Xx

1

Zz

1

; (From point A to reference (zero) point)

G30 Xx

2

Zz

2

; (From point B to 2nd reference (zero) point)

G29 Xx

3

Zz

3

; (From point C to point D)

Present position

A

R

1

Reference (zero) point position

(#1)

New intermediate point

G30

(x

2

,z

2

)

G28

Old intermediate

(x

1

,z

1

) point

C

B

G29

(x

3

R

2

D

,z

3

)

2nd reference (zero) point position (#2)

287


14.8 2nd, 3rd and 4th reference (zero) point return

14.8 2nd, 3rd and 4th reference (zero) point return; G30


The tool can return to the second, third, or fourth reference (zero) point by specifying G30 P2 (P3 or P4).

2nd reference point

Reference point

Command format

G30P2

G28

G28

G29

Start point

G30

(x

1

,y

1

,z

1

,

α

1

)

Intermediate point

G30P3

G30P4

G29

4th reference point

3rd reference point

G30 P2 (P3, P4) Xx

1

Yy

1

Zz

1

aa

1

;

αα

1

288




(1) The second, third, or fourth reference (zero) point return is specified by P2, P3, or P4. A command without P or with P0, P1, P5 or a greater P number is ignored, returning the tool to the second reference (zero) point.

(2) In the second, third, or fourth reference (zero) point return mode, as in the first reference

(zero) point return mode, the tool returns to the second, third, or fourth reference (zero) pint via the intermediate point specified by G30.

(3) The second, third, and fourth reference (zero) point coordinates refer to the positions specific to the machine, and these can be checked with the setting and display unit.

(4) If G29 is specified after completion of returning to the second, third, and fourth reference

(zero) points, the intermediate position used last is used as the intermediate position for returning by G29.

-X

R#1

Intermediate point (x

1

,y

1

)

G30P3Xx

1

Yy

1

;

1st reference (zero) point

G29Xx

2

Yy

2

;

R#3

(x

2

,y

2

)

-Y

3rd reference (zero) point

(5) With reference (zero) point return on a plane during compensation, the tool moves without tool diameter compensation (zero compensation) from the intermediate point. with a subsequent

G29 command, the tool moves with tool diameter compensation until the G29 command from the intermediate point.

-X

R#3

Tool nose center path

Programmed path

G30P3Xx

1

Yy

1

;

Intermediate point


(x

1

,y

1

)

-Y

G29Xx

2

Yy

2

;

(x

2

,y

2

)

289



(6) The tool length offset amount for the axis involved is canceled after the second, third and fourth reference (zero) point returns.

(7) With second, third and fourth reference (zero) point returns in the machine lock status, control from the intermediate point to the reference (zero) point will be ignored. When the designated axis reaches as far as the intermediate point, the next block will be executed.

(8) With second, third and fourth reference (zero) point returns in the mirror image mode, mirror image will be valid from the start point to the intermediate point and the tool will move in the opposite direction to that of the command. However, mirror image is ignored from the intermediate point to the reference (zero) point and the tool moves to the reference (zero) point.

-X

R#3


X-axis mirror image

-Y

G30P3Xx

1

Yy

1

;

No mirror image

290


14.9 Reference point check

14.9 Reference point check; G27


This command first positions the tool at the position assigned by the program and then, if that positioning point is the first reference point, it outputs the reference point arrival signal to the machine in the same way as with the G28 command. Therefore, when a machining program is prepared so that the tool will depart from the first reference point and return to the first reference point, it is possible to check whether the tool has returned to the reference point after the program has been run.

Command format

G27 Xx

1

Yy

1

Zz

1

Pp

1

;

G27

Xx

1

Yy

1

Zz

1

Pp

1

: Check command

: Return control axis

: Check number

P1 : 1st reference point check

P2 : 2nd reference point check

P3 : 3rd reference point check

P4 : 4th reference point check


(1) If the P command has been omitted, the first reference point will be checked.

(2) The number of axes whose reference points can be checked simultaneously depends on the number of axes which can be controlled simultaneously.

Note that the display shows one axis at a time from the final axis.

(3) An alarm will occur if the reference point is not reached after the command is completed.

291


14.10 Workpiece coordinate system setting and offset

14.10 Workpiece coordinate system setting and offset ; G54 to G59 (G54.1)


(1) The workpiece coordinate systems are for facilitating the programming of workpiece machining in which the reference point of the workpiece to be machined is to serve as the zero point.

(2) These commands enable the tool to move to the positions in the workpiece coordinate system.

There are 6 workpiece coordinate systems which are used by the programmer for programming. (G54 to G59)

In addition to the six sets of workpiece coordinate systems between G54 and G59, there are

48 additional workpiece coordinate system sets. (The 48 sets are options.)

(3) Among the workpiece coordinate systems currently selected by these commands, any workpiece coordinate system with coordinates which have been commanded by the present position of the tool is reset. (The "present position of the tool" includes the offset amounts for tool radius, tool length and tool position offset.)

(4) An imaginary machine coordinate system with coordinates which have been commanded by the present position of the tool is set by this command.

(The "present position of the tool" includes the offset amounts for tool diameter, tool length and tool position offset.) (G54, G92)

Command format

(1) Workpiece coordinate system selection (G54 to G59)

(G90) G54 Xx

1

Yy

1

αα

1

Zz

1

αα

1

;

(2) Workpiece coordinate system setting (G54 to G59)

(G54) G92 Xx

1

Yy

1

αα

1

Zz

1

αα

1

;

(3) Workpiece coordinate system selection (expanded : P1 to P48)

G54.1 Pn ;

(4) Workpiece coordinate system setting (expanded : P1 to P48)

G54.1 Pn ;

G92 Xx Yy Zz ;

(5) Workpiece coordinate system offset amount setting (expanded : P1 to P48)

G10 L20 Pn Xx Yy Zz ;

292




(1) With any of the G54 through G59 commands, the tool diameter offset amounts for the commanded axes will not be canceled even if workpiece coordinate system selection is commanded.

(2) The G54 workpiece coordinate system is selected when the power is switched on.

(3) Commands G54 through G59 are modal commands (group 12).

(4) The coordinate system will move with G92 in a workpiece coordinate system.

(5) The offset setting in a workpiece coordinate system denotes the distance from the zero point of the basic machine coordinate system.

-X

M

R#1

(#1)

Reference point

(zero point) return position

-X(G55)(-2000,

-1000)

-X(G54)(-500,

-500)

W2

-Y(G55)

W1

-Y

(G54)


G54 reference point (zero point)

-Y

G55 reference point (zero point)

G54 X =

−

500

Y

G55 X

−

2000

Y

(6) The offset settings of workpiece coordinate systems can be changed any number of times.

(They can also be changed by G10 L2 Pp1 Xx1 Zz1.)

Handling when L or P is omitted

G10 L2 Pn Xx Yy Zz ;

G10 L2 Xx Yy Zz ;

;n=0 : Set the offset amount in the external workpiece coordinate system. n=1 to 6 : Set the offset amount in the designated workpiece coordinate system.

Others : The program error (P35) will occur.

Set the offset amount in the currently selected workpiece coordinate system.

When in G54.1 modal, the program error (P33) will occur.

G10 L20 Pn Xx Yy Zz ; n=1 to 48 : Set the offset amount in the designated workpiece coordinate system.

Others : The program error (P35) will occur.

G10 L20 Xx Yy Zz ; Set the offset amount in the currently selected workpiece coordinate system.

When in G54 to G59 modal, the program error (P33) will occur.

G10 Pn Xx Yy Zz ;

G10 Xx Yy Zz ;

L2 (workpiece offset) will be judged if there is no L value.

293



(7) A new workpiece coordinate system 1 is set by issuing the G92 command in the G54

(workpiece coordinate system 1) mode. At the same time, the other workpiece coordinate systems 2 through 6 (G55 to G59) will move in parallel and new workpiece coordinate systems

2 through 6 will be set.

(8) An imaginary machine coordinate system is formed at the position which deviates from the new workpiece reference (zero) point by an amount equivalent to the workpiece coordinate system offset amount.

-X

-X

[M]

-X(G55)

-X(G54)

W1

M

R#1

Reference (zero) point return position


Imaginary machine coordinate system coordinate point based on G92

Old work 1 (G54) coordinate system

Old work 2 (G55) coordinate system

-X(G54')

W2

New work 1 (G54) coordinate system

-X(G55')

[W1]

-Y(G55) -Y(G54)

New work 2 (G55) coordinate system

[W2]

-Y

-Y(G54')

-Y(G55')

-Y

After the power has been switched on, the imaginary machine coordinate system is matched with the basic machine coordinate system by the first automatic (G28) or manual reference (zero) point return.

(9) By setting the imaginary basic machine coordinate system, the new workpiece coordinate system will be set at a position which deviates from that imaginary basic machine coordinate system by an amount equivalent to the workpiece coordinate system offset amount.

(10) When the first automatic (G28) or manual reference (zero) point return is completed after the power has been switched on, the basic machine coordinate system and workpiece coordinate systems are set automatically in accordance with the parameter setting.

(11) If G54X-Y-; is commanded after the reference return (both automatic or manual) executed after the power is turned ON, the program error (P62) will occur. (A speed command is required as the movement will be controlled with the G01 speed.)

(12) Do not command a G code for which a P code is used in the same block as G54.1. The P code will be used in the prioritized G command.

(13) When number of workpiece offset sets additional specifications is not added, the program error (P39) will occur when the G54.1 command is executed.

294



(14) When number of workpiece offset sets additional specifications is not added, the program error (P172) will occur when the G10 L20 command is executed.

(15) The local coordinate system cannot be used during G54.1 modal. The program error (P438) will occur when the G52 command is executed during G54.1 modal.

(16)A new workpiece coordinate system P1 can be set by commanding G92 in the G54.1 P1 mode.

However, the workpiece coordinate system of the other workpiece coordinate systems G54 to

G59, G54.1 and P2 to P48 will move in parallel with it, and a new workpiece coordinate system will be set.

(17) The offset amount of the extended workpiece coordinate system is assigned to the variable number as shown in Table 1.

Table 1 Variable numbers of the extended workpiece coordinate offset system

P14

P15

P16

P17

P18

P19

P20

P21

P22

P23

P24

P 1

P 2

P 3

P 4

P 5

P 6

P 7

P 8

P 9

P10

P11

P12

P13

1st axis to 6th axis

#7001 to #7006

#7021 to #7026

#7041 to #7046

#7061 to #7066

#7081 to #7086

#7101 to #7106

#7121 to #7126

#7141 to #7146

#7161 to #7166

#7181 to #7186

#7201 to #7206

#7221 to #7226

#7241 to #7246

#7261 to #7266

#7281 to #7286

#7301 to #7306

#7321 to #7326

#7341 to #7346

#7361 to #7366

#7381 to #7386

#7401 to #7406

#7421 to #7426

#7441 to #7446

#7461 to #7466

P38

P39

P40

P41

P42

P43

P44

P45

P46

P47

P48

P25

P26

P27

P28

P29

P30

P31

P32

P33

P34

P35

P36

P37

1st axis to 6th axis

#7481 to #7486

#7501 to #7506

#7521 to #7526

#7541 to #7546

#7561 to #7566

#7581 to #7586

#7601 to #7606

#7621 to #7626

#7641 to #7646

#7661 to #7666

#7681 to #7686

#7701 to #7706

#7721 to #7726

#7741 to #7746

#7761 to #7766

#7781 to #7786

#7801 to #7806

#7821 to #7826

#7841 to #7846

#7861 to #7866

#7881 to #7886

#7901 to #7906

#7921 to #7926

#7941 to #7946

CAUTION

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

295




(Example 1)

(1) G28 X0Y0 ;

(2) G53 X

−

1000 Y

−

500 ;

(3) G53 X0Y0 ;

Present position

(1)

(2)

(3)

M

R#1


When the first reference point coordinate is zero, the basic machine coordinate system zero point and reference (zero) point return position (#1) will coincide.

(Example 2)

(1) G28X0Y0 ;

(2) G90G00G53X0Y0 ;

(3) G54X-500 Y

−

500 ;

(4) G01G91X

−

500F 100 ;

(5) Y

−

500 ;

(6) X+500 ;

(7) Y+500 ;

(8) G90G00G55X0Y0 ;

(9) G01X

−

500 F200 ;

(10) X0Y

−

500 ;

(11) G90G28X0Y0 ;

-X(G55)


(1)

Present position

(2)

-X(G54)

(9)

-1000 -500

W2

(8)

(10)

(5) (4)

(11)

(6)

(7)

(3)

W1

-

500

-

1000

M

-500

-1000

-1500

-Y

(G55)

-Y

(G54)

296



(Example 3)

When workpiece coordinate system G54 has shifted (

−

500,

−

500) in example 2 (It is assumed that 3 through 10 in example 2 have been entered in subprogram 01111.)

(1) G28 X0 Y0 ;

(2) G90 G53 X0 Y0 ; (This is not required when there is no G53 offset.)

(3) G54 X

−

500Y

−

500 ;

Amount by which workpiece coordinate system deviates

(4) G92 X0 Y0 ;

(5) M98 P1111 ;

New workpiece coordinate system is set.

(#1) Reference (zero) point return position

(1)

(2)

-X

Present position

Old G55 coordinate system

-X(G55)

-X

(G54')

New G55 coordinate system

-X(G55')

W2

-X(G54)

-Y

(4)

(G55)

(3)

W1

-Y

(G54)

-Y

(G54')

M

Old G54 coordinate system

New G54 coordinate system

-Y(G55')

-Y

(Note)

The workpiece coordinate system will shift each time steps 3 through 5 are repeated. The reference point return (G28) command should therefore be issued upon completion of the program.

297



(Example 4)

When six workpieces are placed on the same coordinate system of G54 to G59, and each is to be machined with the same machining.

(1) Setting of workpiece offset data

Workpiece1 X =

−

100.000 Y =

−

100.000 ....................................... G54

2 X =

−

100.000 Y =

−

500.000 ...................................... G55

3 X =

−

500.000 Y =

−

100.000 ...................................... G56

4 X =

−

500.000 Y =

−

500.000 ...................................... G57

5 X =

−

900.000 Y =

−

100.000 ...................................... G58

6 X =

−

900.000 Y =

−

500.000 ....................................... G59

(2) Machining program (subprogram)

O100;

N1 G90 G0 G43X-50. Y-50. Z-100. H10; Positioning

N2 G01 X-200. F50;

Y-200. ;

X- 50. ;

Face cutting

Y- 50. ;

N3 G28 X0 Y0 Z0 ;

N4 G98 G81 X-125. Y-75. Z-150. R-100. F40;

G80;

X-175. Y-125. ;

X-125. Y-175. ;

X- 75. Y-125. ;

N5 G28 X0 Y0 Z0 ;

N6 G98 G84 X-125. Y-75. Z-150. R-100. F40 ;

X-175. Y-125. ;

X-125. Y-175. ;

X- 75. Y-125. ;

G80;

M99;

Drilling

Tapping

1

2

3

4

1

2

3

4

(3) Positioning program (main)

G28 X0 Y0 Z0 ;

When power is turned ON

N1 G90 G54 M98 P100 ;

N2 G55 M98 P100 ;

N3 G57 M98 P100 ;

N4 G56 M98 P100 ;

N5 G58 M98 P100 ;

N6 G59 M98 P100 ;

N7 G28 X0 Y0 Z0 ;

N8 M02 ;

%

298



299


14.11 Local coordinate system setting

14.11 Local coordinate system setting; G52


The local coordinate systems can be set independently on the G54 through G59 workpiece coordinate systems using the G52 command so that the commanded position serves as the programmed zero point.

The G52 command can also be used instead of the G92 command to change the deviation between the zero point in the machining program and the machining workpiece zero point.

Command format

G54 (54 to G59) G52Xx

αα

1

1

Yy

1

Zz

1

αα

1

;


(1) The G52 command is valid until a new G52 command is issued, and the tool does not move.

This command comes in handy for employing another coordinate system without changing the zero point positions of the workpiece coordinate systems (G54 to G59).

(2) The local coordinate system offset will be cleared by the dog-type manual reference (zero) point return or reference (zero) point return performed after the power has been switched on.

(3) The local coordinate system is canceled by (G54 to G59) G52X0 Y0 Z0

α

0 ;.

(4) Coordinate commands in the absolute value (G90) cause the tool to move to the local coordinate system position.

Ln

(G91) G52X_Y_;

Incremental value

Ln

Absolute value

Local coordinate systems

Absolute value

Ln

Wn(n=1 to 6)

(G90)

G52X_Y_;


Reference point

R

Workpiece coordinate system offset

(DDB input, screen setting, G10L2P

_

X

_

Y

_

;)

External workpiece coordinate system offset

(DDB input, screen setting, G10 P0 X_Z_;)

M


(Note)

If the machining program is executed many times repeatedly, the workpiece coordinate system may deviate slightly per execution.

Command to execute reference point return at the program end.

300



(Example 1)

Local coordinates for absolute value mode (The local coordinate system offset is not cumulated)

(2) G00G90X1. Y1. ;

(5) G52X1. Y1. ;

(10) G00X0Y0 ;

2500

2000

1500

1000

500

(3)

(2)

(5)

(4)

(6)

[W1]L1

(8)

(9)

(7)

Local coordinate system created by (5).

(1)

R#1

W1

(10)

[W1]

New coordinate system created by (3)

Matched with local coordinate system by (9).

500 1000 1500 2000 2500 3000

Current position

X

The local coordinate system is created by (5), canceled (9) and matched with the coordinate system f (3)

(Note)

If the program is executed repeatedly, the workpiece coordinate system will deviate each time. Thus, when the program is completed, the reference point return operation must be commanded.

(Example 2)

Local coordinates for incremental value mode (The local coordinate system offset is cumulated.)

(5) G52X1. Y1. ;

(7) G52X-1.5 Y1.5 ;

(A) O100 ;

(B) G90G00X0Y0 ;

(C) G01X500 ;

(D) Y500 ;

(E) G91 ;

Y

'

Y

"

Y

2500

2000

(D)

(B)

(6)

1500

1000

[W1]L2

(C)

X

"


(D)

(B)

(4)

500

(3)

(2)

(1)

(8)

[W1]L1

(C)

X

'


500 1000 1500 2000 2500 3000

R#1

W1

Current position

Matched with local

X coordinate system by (7).

(Explanation)

The local coordinate system X'Y' is created at the XY coordinate system (500,500) position by (3).

The local coordinate system X"Y" is created at the X'Y' coordinate system (1000,1000) position by (5).

The local coordinate system is created at the X"Y" coordinate system (-1500, -1500) position by (7).

In other words, the same occurs as when the local coordinate system and XY coordinate system are matched and the local coordinate system is canceled.

301



(Example 3)

When used together with workpiece coordinate system

X 1000

Y 500

%

Y

3000

2500

2000

1500

1000

500

(D)

(B)

(C)

(5) W2

(2)

(3)

(B)

(7)

(C)

[W1] L1

(D)

W1

G55

Local coordinate system created by (3)

G54

1

R#1

500 1000 1500 2000 2500 3000

Current position

X

(Explanation)

The local coordinate system is created at the G54 coordinate system (500,500) position by (3), but the local coordinate system is not created for the G55 coordinate system.

During the movement for (7), the axis moves to the G54 local coordinate system's reference point (zero point).

The local coordinate system is canceled by G90G54G52X0Y0;.

302



(Example 4)

Combination of workpiece coordinate system G54 and multiple local coordinate systems

G54

X 500

Y 500

(parameter setting value)

(4) G52X1. Y1. ;

(6) G52X2. Y2. ;

M02 ;

(A) O300 ;

(B) G00X0Y0 ;

(C) G01X500F100 ;

(D) Y500 ;

(E) X0Y0 ;

%

3000

2500

2000

1500

1000

500

(2)

(8)

(3)

(D)

(B)

(E)

W1

(C)

R#1

(5)

[W1] L1

(7)

[W1] L2



G54

500 1000 1500 2000 2500 3000

Current position

(Explanation)

The local coordinate system is created at the G54 coordinate system (1000,1000) position by (4).

The local coordinate system is created at the G54 coordinate system (2000,2000) by (6).

The G54 coordinate system and local coordinate system are matched by (8).

303

15. Measurement Support Functions

15.1 Automatic tool length measurement


15.1 Automatic tool length measurement; G37


These functions issue the command values from the measuring start position as far as the measurement position, move the tool in the direction of the measurement position, stop the machine once the tool has arrived at the sensor, cause the NC system to calculate automatically the difference between the coordinate values at that time and the coordinate values of the commanded measurement position and provide this difference as the tool offset amount.

When offset is already being applied to a tool, it moves the tool toward the measurement position with the offset still applied, and if a further offset amount is generated as a result of the measurement and calculation, it provides further compensation of the present offset amount.

If there is one type of offset amount at this time, and the offset amount is distinguished between tool length offset amount and wear offset amount, the wear amount will be automatically compensated.

Command format

G37Z__R__D__F__ ;

Z : Measuring axis address and coordinates of measurement position ..... X, Y, z,

α

(where,

α

is the additional axis)

R : This commands the distance between the measurement position and point where the movement is to start at the measuring speed.

D : This commands the range within which the tool is to stop.

F : This commands the measuring feedrate.

When R_, D_ of F_ is omitted, the value set in the parameter is used instead.

<Parameter> ("TLM" on machining parameter screen)

• #8004 SPEED (measuring feedrate) : 0 to 60000 (mm/min)

• #8005 ZONE r (deceleration range) : 0 to 99999.999 (mm)

• #8006 ZONE d (measurement range) : 0 to 99999.999 (mm)

304



Example of execution

For new measurement

0

-100

-200

F

-300

R

D

-400

-Z

H01=0

Instrument

D

T01 ;

M06 T02 ;

G90 G00 G43 Z0 H01 ;

G37 Z-400 R200 D150 F1 ;

Coordinate value when measurement position is reached = -300

-300 - (-400) = 100

0+100 = 100 Where, H01 = 100

305




(1) Operation with G37 command

Rapid traverse rate

Speed

Distance

Measuring position

Operation 1

Stop point

Sensor output

Operation 2

Operation 3

Measurement allowable range

D(d) D(d)

F(Fp)

R(r)

Offset amount

Or no detection

Normal completion

Alarm stop (P607)

Alarm stop (P607)

(2) The sensor signal (measuring position arrival signal) is used in common with the skip signal.

(3) The feedrate will be 1mm/min if the F command and parameter measurement speed are 0.

(4) An updated offset amount is valid unless it is assigned from the following Z axis (measurement axis) command of the G37 command.

(5) Excluding the corresponding values at the PLC side, the delay and fluctuations in the sensor signal processing range from 0 to 0.2ms.

As a result, the measuring error shown below is caused.

Maximum measuring error (mm) = Measuring speed (mm/min)

•

1

60

•

0.2 (ms)

1000

(6) The machine position coordinates at that point in time are ready by sensor signal detection, and the machine will overtravel and stop at a position equivalent to the servo droop.

Maximum overtravel (mm)

= Measuring speed (mm/min)

•

1

60

•

The standard position loop gain is 33 (s

−

1

).

1

Position loop gain (s

−

1

)

306



Precautions

(1) Program error (P600) results if G37 is commanded when the automatic tool length measurement function is not provided.

(2) Program error (P604) results when no axis has been commanded in the G37 block or when two or more axes have been commanded.

(3) Program error (P605) results when the H code is commanded in the G37 block.

(4) Program error (P606) results when G43_H is not commanded prior to the G37 block.

(5) Program error (P607) results when the sensor signal was input outside the allowable measuring range or when the sensor signal was not detected even upon arrival at the end point.

(6) When a manual interrupt is applied while the tool is moving at the measuring speed, a return must be made to the position prior to the interrupt and then operation must be resumed.

(7) The data commanded in G37 or the parameter setting data must meet the following conditions:

|Measurement point

−

start point| > R command or parameter r

> D command or parameter d

(8) When the D command and parameter d in (7) above are zero, operation will be completed normally only when the commanded measurement point and sensor signal detection point coincide. Otherwise, program error (P607) will results.

(9) When the R and D commands as well as parameters r and d in (7) above are all zero, program error (P607) will result regardless of whether the sensor signal is present or not after the tool has been positioned at the commanded measurement point.

(10) The automatic tool length measurement command (G37) must be commanded together with the G43H_ command that designates the offset No.

G43H_;

G37 Z_ R_ D_ F_;

307


15.2 Skip function

15.2 Skip function; G31


When the skip signal is input externally during linear interpolation based on the G31 command, the machine feed is stopped immediately, the remaining distance is discarded and the command in the following block is executed.

Command format

G31 Xx Yy Zz

αα

Ff ; (where, a is the additional axis)

x, y, z,

α

: Axis coordinates; they are commanded as absolute or incremental values according to the G90/G91 modal when commanded.

Linear interpolation can be executed using this function. If the skip signal is input externally while this command is being executed, the machine will stop, the remaining commands will be canceled and operation will be executed from the next block.


(1) If Ff is commanded as the feedrate in the same block as G31 command, commanded speed

"f" will apply; if it not commanded, the value set in the parameter "#1174 skip_F" will serve as the feedrate. In either case, the F modal will not be updated.

(2) Normally, the machine will not automatically accelerate or decelerate with the G31 block.

However, setting the base specification parameter "#21101 add01/bit3" to "1" allows the automatic acceleration/deceleration valid.

In such case, the acceleration/deceleration will apply following to the cutting feed acceleration/deceleration pattern set with the axis specification parameter "#2003 smgst".

Since the deceleration at skip signal input follows the cutting feed acceleration/deceleration pattern mentioned above, the coasting amount from the skip signal input to stop may be larger than the normal specifications (when automatic acceleration/deceleration is invalid)

(3) The stop condition (such as feed hold, stroke end) is also valid for the G31 block.

(4) With the normal specifications, override and dry run are invalid during execution of G31 block.

However, setting the base specification parameter "#21101 add01/bit3" to "1" allows the override and dry run.

(5) The G31 command is unmodal and so it needs to be commanded each time.

(6) If the skip signal is input during G31 command start, the G31 command will be completed immediately.

When a skip signal has not been input until the G31 block completion, the G31 command will also be completed upon completion of the movement commands.

(7) When the G31 command is issued during nose R compensation, program error (P608) will result.

(8) When there is no F command in the G31 command and the parameter speed is also zero, program error (P603) will result.

(9) If only the Z axis is commanded when the machine lock is ON or the Z axis cancel switch is

ON, the skip signal will be ignored and execution will continue as far as the end of the block.

308


Execution of G31

G90 G00 X-100000 Y0 ;

G31 X-500000 F100 ;

G31 X0 F100 ;

G31 X-50000 F100 ;


-500000

G01

G31

G31

G31

G01

G01

-10000

0

Y

W

X

-100000

G01

-200000

-300000

Detailed description (Readout of skip coordinates)

The coordinate positions for which the skip signal is input are stored in the system variables #5061

(1st axis) to #506n (nth axis), so these can be used in the user macros.

G90 G00 X-100. ;

G31 X-200. F60 ;

#101 = #5061

Skip command

Skip signal input coordinate values (workpiece coordinate system) are readout to #101.

309


Detailed description (G31 coasting)


The amount of coasting from when the skip signal is input during the G31 command until the machine stops differs according to the parameter "#1174 skip_F" or F command in G31.

The time to start deceleration to a stop after responding to the skip signal is short, so the machine can be stopped precisely with a small coasting amount

δ

0

=

F

60

×

Tp +

F

60

×

( t

1

±

t

2

) =

F

60

×

( Tp + t

1

)

±

F

60

×

t

2

δ

0

: Coasting amount (mm)

δ

1

δ

2

F : G31 skip speed (mm/min.)

Tp : Position loop time constant (s) = (position loop gain)

−

1 t

1

: Response delay time (s) = (time taken from the detection to the arrival of the skip signal at the controller via PC) t

2

: Response error time (0.001 s)

When G31 is used for calculation, the value calculated from the section indicated by

δ

1 in the above equation can be compensated, however,

δ

2 results in calculation error.

F

Skip signal input

Area inside shaded section denotes coasting amount

δ

0

Time (S) t

1

± t

2

Tp

Stop pattern with skip signal input

The relationship between the coasting amount and speed when Tp is 30ms and t

1

is 5ms is shown in the following figure.

0.050

Tp = 0.03

t

1

= 0.005

0.040

Max. value

Average

Min. value

0.030

0.020

0.010

0 10 20 30 40 50 60 70

Feedrate F (mm/min)

Relationship between coasting amount and feedrate (example)

(Note)

When the base specification parameter "#21101 add01/bit3" is set to "1", the automatic acceleration/deceleration becomes valid for the deceleration at skip signal input.

Thus, the coasting amount from the skip signal input to stop may be larger than when the automatic acceleration/deceleration is invalid.

310


Detailed description (Skip coordinate readout error)


(1) Skip signal input coordinate readout

The coasting amount based on the position loop time constant Tp and cutting feed time constant Ts is not included in the skip signal input coordinate values.

Therefore, the work coordinate values applying when the skip signal is input can be read out across the error range in the following formula as the skip signal input coordinate values.

However, coasting based on response delay time t1 results in a measurement error and so compensation must be provided.

ε

: Readout error (mm)

ε

=

±

F

60

×

t

2

t

2

: Response error time 0.001 (s)

+1

0

-1

Measurement value comes within shaded section.

60

Feedrate (mm/min)

Readout error of skip signal input coordinates

Readout error of skip input coordinates

Readout error with a 60mm/min feedrate is:

ε

=

± ×

0.001 =

±

0.001 (mm)

Measurement value is within readout error range of

±

1

µ m.

(2) Readout of other coordinates

The readout coordinate values include the coasting amount. Therefore, when coordinate values are required with skip signal input, reference should be made to the section on the G31 coasting amount and compensation provided. As in the case of (1), the coasting amount based on the delay error time t2 cannot be calculated, and this generates a measuring error.

311


Examples of compensating for coasting


(1) Compensating for skip signal input coordinates

#110 = Skip feedrate ;

#111 = Response delay time t

1

;

G31 X100. F100 ;

G04 ;

#101 = #5061 ;

#102 = #110

∗

#111/60 ;

#105 = #101

−

#102

−

#103 ;

Skip command

Machine stop check

Skip signal input coordinate readout

Coasting based on response delay time

Skip signal input coordinates

(2) Compensating for work coordinates

#110 = Skip feedrate ;

#111 = Response delay time t

1

;

#112 = Position loop time constant Tp ;

G31 X100. F100 ;

G04 ;

#101 = #5061 ;

#102 = #110

∗

#111/60 ;

#103 = #110

∗

#112/60 ;

#105 = #101

−

#102

−

#103 ;

Skip command

Machine stop check

Skip signal input coordinate readout

Coasting based on response delay time

Coasting based on position loop time constant

Skip signal input coordinates

312


15.3 Multi-step skip function1

15.3 Multi-step skip function1; G31.n, G04


The setting of combinations of skip signals to be input enables skipping under various conditions.

The actual skip operation is the same as with G31.

The G commands which can specify skipping are G31.1, G31.2, G31.3, and G04, and the correspondence between the G commands and skip signals can be set by parameters.

Command format

G31.1 Xx Yy Zz

αα

Ff ;

Xx Yy Zz

αα

; Command format axis coordinate word and target coordinates

Ff ; Feedrate (mm/min)

Same with G31.2 and G31.3 ; Ff is not required with G04

As with the G31 command, this command executes linear interpolation and when the preset skip signal conditions have been met, the machine is stopped, the remaining commands are canceled, and the next block is executed.


(1) Feedrate G31.1 set with the parameter corresponds to "#1176 skip1f", G31.2 corresponds to

"#1178 skip2f", and G31.3 corresponds to "#1180 skip3f".

(2) A command is skipped if it meets the specified skip signal condition.

(3) The G31.n and G04 commands work the same as the G31 command for other than (1) and (2) above.

(4) The feedrates corresponding to the G31.1, G31.2, and G31.3 commands can be set by parameters.

(5) The skip conditions (logical sum of skip signals which have been set) corresponding to the

G31.1, G31.2, G31.3 and G04 commands can be set by parameters.

Parameter setting

1

Valid skip signal

4 3 2 1

× × ×

×

4 × × ×

5 × ×

× 6 ×

7 ×

8 × × ×

9

10

11

12

13

14

15

× ×

× ×

×

× ×

×

×

(Skip when " " signal is input.)

313


Example of operation

15.3 Multi-step skip function1

(1) The multi-step skip function enables the following control, thereby improving measurement accuracy and shortening the time required for measurement.

Parameter settings :

Skip condition Skip speed

G31.1 : 7 20.0mm/min (f1)

G31.2 : 3 5.0mm/min (f2)

G31.3 : 1 1.0mm/min (f3)

Program example :

N10G31.1 X200.0 ;

N20G31.2 X40.0 ;

N30G31.3 X1.0 ; f

Operation

(f

1

)

N10

Measurement distance

Skip speed

(f

2

) N20

(f

3

) N30 t

Input of skip signal 3



(Note 1)

If skip signal 1 is input before skip signal 2 in the above operation, N20 is skipped at that point and N30 is also ignored.

(2) If a skip signal with the condition set during G04 (dwell) is input, the remaining dwell time is canceled and the following block is executed.

314


15.4 Multi-step skip function 2

15.4 Multi-step skip function 2; G31


During linear interpolation, command operation is skipped if skip signal parameter Pp specified with a skip command (G31), which indicates external skip signals 1 to 4, is met.

If multi-step skip commands are issued simultaneously in different part systems, both part systems perform skip operation simultaneously if the input skip signals are the same, or they perform skip operation separately if the input skip signals are different. The skip operation is the same as with a normal skip command (G31 without P parameter).

X1

X1

Skip signal 1

Skip signal 1

Z

Z

X2

Skip signal 1

Skip signal 2

X2

Same skip signals input in both part systems 1 and 2

Different skip signals input in part systems 1 and 2

If the skip condition specified by the parameter "#1173 dwlskp" (indicating external skip signals 1 to

4) is met during execution of a dwell command (G04), the remaining dwell time is canceled and the following block is executed. Similarly, if the skip condition is met during revolution dwelling, the remaining revolution is canceled and the following block is executed.

Command format

G31 Xx Zz

αα

Pp Ff ;

Xx Zz

αα

Pp

Ff

: Command format axis coordinate word and target coordinates

: Skip signal parameter

: Feedrate (mm/min)

315




(1) The skip is specified by command speed f. Note that the F modal is not updated.

(2) The skip signal is specified by skip signal parameter p. p can range from 1 to 15. If p is specified outside the range, program error (P35) occurs.

Skip signal command

P

1

Valid skip signal

4 3 2 1

× × ×

×

4 × × ×

5 × ×

× 6 ×

7 ×

8 × × ×

9

10

11

× ×

×

×

×

12

13

14

15

× ×

×

×

(Skip when " " signal is input.)

(3) The specified skip signal command is a logical sum of the skip signals.

(Example)

G31 X100. P5 F100 ;

Operation is skipped if skip signal 1 or 3 is input.

316



(4) If skip signal parameter Pp is not specified, the skip condition specified by the G31 parameter works. If speed parameter Ff is not specified, the skip speed specified by the G31 parameter works.

Relations between skip and multi-step skip

Skip specifications

G31 X100 ;

Without P and F

G31 X100 P5 ;

Without F

G31 X100 F100 ;

Without P

G31 X100 P5 F100 ;

x o

Condition Speed condition Speed

Program error (P601)




Skip 1

Command value

Skip 1

Command value

Parameter

Parameter

Command value

Command value

(Note)

"Parameter" in the above table indicates that specified with a skip command (G31).

(5) If skip specification is effective and P is specified as an axis address, skip signal parameter P is given priority and axis address P is ignored.

(Example)

G31 P500. F100 ;

This is regarded as a skip signal parameter and program error (P35) results.

(6) Those items other than (1) to (5) are the same with the ordinary skip function (G31 without P).

317

Appendix 1. Program Parameter Input N No. Correspondence Table


(Note 1)

The units in the table indicate the minimum setting units for the parameter data.

(Note 2)

The setting ranges given in the table are the setting ranges on the screen. Designate parameters related to the length by doubling the input setting unit. However, the parameters with " z

" in "etc" column (ZERO-RTN PARAM 2027, 2028, 2029) must be excluded.

(Example 1)

To set 30mm in a parameter when the input setup unit is B (0.001mm) and metric system.

L60000

(Example 2)

To set 5 inch in a parameter when the input setup unit is B (0.0001 inch) and inch system.

L100000

(Note 3)

The binary type parameters must be converted into byte-type data, and commanded with a decimal data after address D.

(Example 1)

Binary data

01010101

B

= 55

H

= 85

D

....................... Command 85

(Example 2)

ASCII code

"M" = 01001101

B

= 4D

H

= 77

D

............. Command 77

(B indicates Binary, H indicates Hexadecimal, and D indicates Decimal.)

P No. 2 (Axis independent parameter)

Parameter

No.

#8201

#8202

#8204

#8205

Axis bit parameter 2

Axis bit parameter 1

Data type

Setting range

Bit Same as above

(Unit)

Soft limit (

−

)

(User stroke end lower

limit)

Soft limit (+)

(User stroke end upper

limit)

912 2-word

±

99999999

×

2 Interpolation unit

Remarks

896 bit0 : bit1 : bit2 : bit3 : bit4 : bit5 : bit6 : Axis bit7 : removal

897 Bit d0 : No. d bit

OFF or d1 : No. d bit ON

(d : 0 ~ 7)

916 2-word

±

99999999

×

2 Interpolation unit bit1 : bit2 : Soft limit invalid bit3 : bit4 : bit5 : bit6 : bit7 :

924 2-word

±

99999999

×


318


P No. 2 (Axis independent parameter)

Parameter

No.

Details N type

#2013 OT-

Setting range (Unit)

292 2-word

±

99999999

×


#2014 OT+

#2015 tlml-

#2016 tlml+

288 2-word

±

99999999

×


300 2-word

±

99999999

×


296 2-word

±

99999999

×


#2017 tap_g 58 Word 0.25 ~ 200.00 (rad/s)

#2025

#2026

#2027

G28rap

G28crp

G28sft

260

38

44

2-word 1 ~ 999999

Word 1 ~ 60000

Word 0 ~ 65535

(

(min)

(min)

μ m)

Remarks

Axis specifications parameter





Zero point return parameter



●

#2029 grspc 42 Word -32767 ~ 999 (mm)

#2028 grmask 40 Word 0 ~ 65535

(

μ m)


●


●

#2030

#2031

#2032 dir(-) noref nochk

#2037 G53ofs

#2038 #2_rfp

#2039 #3_rfp

#2040 #4_rfp

#2061 OT-1B-

#2062 OT-1B+

20

21

Bit2

Bit2

0 ~ 1

0 ~ 1



54 Bit0 0 ~ 1

272 2-word

±

99999999

×


276 2-word

±

99999999

×


280 2-word

±

99999999

×


284 2-word

±

99999999

×


324 2-word

±

99999999

×







320 2-word

±

99999999

×


Axis specifications parameter 2

Axis specifications parameter 2

319


P No. 5 (PLC constant)

Parameter

No.

#6301

~

#6348

Details N type

PLC constant 1 ~

48

Setting range

2-word 0 ~ 99999999

(Unit) Remarks

•

N No. corresponds to the constant

No. (# No.) on the PLC constant screen.

P No. 6 (PLC timer)

Parameter

No.

#6000

~

#6015

Details N type

10ms addition timer

(T0 ~ T15)

0 ~

15

Setting range

Word 0 ~ 32767

10ms addition timer

(T16 ~ T95)

16 ~

95

Word 0 ~ 32767 #6016

~

#6095

#6096

~

#6103

10ms addition timer

(T96 ~ T103)

96 ~

103

Word 0 ~ 32767

P No. 7 (PLC counter)

(Unit)

0.01 s

0.1 s

0.1 s

Parameter

No.

#6200

~

#6223

Counter (C0 ~ C23) 0 ~

23

Data type

Setting range

Word 0 ~ 32767

(Unit)

Remarks

•

Each N No. corresponds to the # No. on the

PLC timer screen.

Remarks

•

N No. corresponds to the # No. on the

PLC counter screen.

P No. 8 (Bit selection parameter)

Parameter

No.

#6401

~

#6496

Details N type

Bit selection parameter

0 ~

96

Setting range

Word 8-digit designation

(Reading abbreviation not possible)

Each bit 0 or 1 d0 : No. d bit

OFF or d1 : No. d bit ON

(d : 0 ~ 7)

(Unit) Remarks

•

N No. corresponds to the # No. on the bit selection screen.

•

N Nos. 49 to 96 are used by the machine maker and Mitsubishi.

These must not be used by the user.

320


P No. 11 (Axis common parameters (per part system))

Parameter

No.

#8004

Details N type

Automatic tool length measurement instrument speed

Setting range

844 2-word 1 ~ 60000

#8005 Automatic tool length measurement deceleration range r

836 2-word 0 ~ 99999999

×

2

#8006 Automatic tool length measurement deceleration range d

840 2-word 0 ~ 99999999

×

2

#8010 override max. angle override precorner length

Wear data input max. value

756 2-word 0 ~ 180

Degree (

°

)

Machining parameter

760 2-word 0 ~ 99999999 Interpolation unit

Machining parameter

776 2-word 0 ~ 99999 unit

(Unit)

(mm/min)

Interpolation unit

Interpolation

Interpolation unit

Remarks

Machining parameter

Machining parameter

Machining parameter

Machining parameter

#8011

#8013

#8014

#8015

#8016

#8017

#8301 X X axis chuck barrier range 1





#8306 X

#8301 Z

#8302 Z

#8303 Z

#8304 Z

Wear data input max. addition

G83 return amount

Thread cutting cycle cutoff angle

Thread cutting cycle chamfering amount

G71 cut amount

G71 cut amount change amount

X axis chuck barrier range 6

Z axis chuck barrier range 1




780 2-word 0 ~ 99999 Interpolation unit

Machining parameter

832

1011

1012

2-word 0 ~ 99999999

Byte

Byte

2

0 ~ 89

1 ~ 127

×

Interpolation unit

Machining parameter

Degree (

°

)

Machining parameter

0.1 lead Machining parameter

788 2-word 0 ~ 99999

×

2

Interpolation unit

792 2-word 0 ~ 99999

×

2

Interpolation unit

1136 2-word

±

99999999

×


1140 2-word

±

99999999

×


1144 2-word

±

99999999

×


1148 2-word

±

99999999

×


1152 2-word

±

99999999

×


1156 2-word

±

99999999

×


1160 2-word

±

99999999

×


1164 2-word

±

99999999

×


1168 2-word

±

99999999

×


1172 2-word

±

99999999

×


Machining parameter

Machining parameter

Barrier

Barrier

Barrier

Barrier

Barrier

Barrier

Barrier

Barrier

Barrier

Barrier

321


P No. 11 (Axis common parameters (per system))

Parameter

No.

#8305 Z Z axis chuck barrier range 5

Details N type

Setting range (Unit)

1176 2-word

±

99999999

×


#8306 Z Z axis chuck barrier range 6

1180 2-word

±

99999999

×


Remarks

Barrier

Barrier

322

Appendix 2. Program Error


(The message in bold characters appears on the screen.)

These alarms occur during automatic operation, and the causes of these alarms are mainly program errors which occur, for instance, when mistakes have been made in the preparation of the machining programs or when programs which conform to the specification have not been prepared.

Error No. Details

P10 EXCS AXIS NO.

The number of axis addresses commanded in the same block exceeds the specifications.

Remedy

•

Divide the alarm block command into two.

•

Check the specifications

P11

•

Revise the axis names in the program.

AXIS ADR. ERROR

The axis address commanded by the program and the axis address set by the parameter do not match.

•

Check the program.

An axis command which cannot be divided by the command unit has been issued.

The number of holes per character on the paper tape is an even number for EIA codes and an odd number for ISO codes.

•

Check the paper tape.

•

Check the tape puncher and tape reader.

The number of characters per block on the paper tape is odd.

An address not listed in the specifications has been used.

•

Make the number of characters per block on the paper tape even.

•

Set the parameter parity V selection off.

•

Check and revise the program address.

•

Check the specifications.

•

Check the program.

The command format in the program is not correct.

A G code not listed in the specifications has been used.

•

Check and correct the G code address in the program.

•

Check the program.

The setting range for the addresses has been exceeded.

P36

P37

P39

PRGRAM END ERR

"EOR" has been read during tape and memory operation.

PROG NO. ZERO

A zero has been designated for a program number or sequence number.

NO SPEC ERR

•

Enter the M02 and M30 commands at the end of the program.

•

Enter the M99 command at the end of the subprogram.

•

The program numbers are designated across a range from 1 to 99999999.

•

The sequence numbers are designated across a range from 1 to 99999.

•

Check the specifications

A command not found in the specifications was issued.

P40

•

Review the program.

PREREAD BL. ERR

When executing tool radius compensation, there was an error in the pre-read block, so the interference could not be checked.

323


Error No.

P60

Details

OVER CMP. LENG.

The commanded movement distance is too long.

(2

31

was exceeded.)

•

Remedy

Review the axis address command range.

P72

No feedrate command has been issued.

There is an error in the arc start and end points as well as in the arc center.

The arc center is not sought during

R-specified circular interpolation.

NO HELICAL SPC

A helical command has been issued though it is not included in the specifications.

•

The default movement modal command at power on is G01.

This causes the machine to move without a

G01 command if a movement command is issued in the program, and an alarm results.

Use an F command to specify the feedrate.

•

Specify F with a thread lead command.

•

Check the numerical values of the addresses that specify the start and end points as well as the arc center in the program.

•

Check the "+" and "

−

" directions of the address numerical values.

•

Check the numerical values of the addresses in the program.

•

Check the helical specifications.

•

An Axis 3 command was issued in the circular interpolation command.

•

If the command is not a helical command, the linear command axis will be moved to the next block.

•


P90

P93

NO THREAD SPEC

A thread cutting command has been issued though it is not included in the specifications.

SCREW PITCH ERR

The screw pitch has not been set correctly when the thread cutting command is issued.

P111 PLANE CHG (CR)

A plane selection command (G17, G18, G19) was issued during the coordinate rotation command (G68).

P112 PLANE CHG (CC)

• A plane selection command (G17, G18,

G19) has been issued when the tool radius compensation command (G41,

G42) or nose radius compensation command (G41, G42, G46) is issued.

• After nose R compensation was completed, there was no axis movement command after G40, and the plane selection command was issued before the compensation was canceled.

•

•

•

Issue the thread cutting command and then set the screw pitch command properly.

After the G68 command, always command

G69 (coordinate rotation cancel), and then issue the plane selection command.

Issue the plane selection command after completing the tool radius compensation and nose R compensation commands (issue the axis movement command after issuing the

G40 cancel command).

The arc command axis is not on the selected plane.

•

Issue arc command on the correctly selected plane.

324


Error No. Details

P122 NO AUTO C-OVER

An automatic corner override command

(G62) has been issued though it is not included in the specifications.

P130 2ND AUX. ADDR

The second miscellaneous function address specified in the program does not match that set by the parameter.

P131 NO G96 SPEC

(No constant surface speed)

The constant surface speed command (G96) was issued despite the fact that such a command does not exist in the specifications.

P132 SPINDLE S = 0

No spindle speed command has been input.

P133 CONTROL AXIS NO. ERR

An invalid constant surface speed control axis has been specified.

P150 NO C-CMP SPEC

•

A tool radius compensation command

(G41, G42) has been issued though there are no tool radius compensation specifications.

•

A nose R compensation command (G41,

G42 G46) has been issued though there are no nose R compensation specifications.

P151 G2, 3 CMP ERR

A compensation command (G40, G41,

G42, G43, G44, G46) has been issued in the arc mode (G02, G03).

Remedy

•


•

Delete the G62 command from the program.

•

•

•

•

•

•

Check and correct the second miscellaneous function address in the program.


Change from the constant surface speed command (G96) to the speed command

(G97).

Review the program.

Review the parameter specified for the constant surface speed control axis.


•

Issue the linear command (G01) or rapid traverse command (G00) in the compensation command block or cancel block.

(Set the modal to linear interpolation.)

•

Review the program.

In interference block processing during execution of a tool radius compensation

(G41 or G42) or nose radius compensation

(G41, G42, or G46) command, the intersection point after one block is skipped cannot be determined.

•

Review the program.

An interference error has arisen while the tool radius compensation command (G41, G42) or nose radius compensation command

(G41, G42, G46) was being executed.

P155 F-CYC ERR (CC)

A fixed cycle command has been issued in the tool radius compensation mode.

At the start of G46 nose radius compensation, the compensation direction is undefined if this shift vector is used.

•

The tool radius compensation mode is established when a fixed cycle command is executed and so the tool radius compensation cancel command (G40) should be issued.

•

Change the vector to that with which the compensation direction is defined.

•

Exchange with a tool having a different tip point number.

325


Error No. Details

During G46 nose radius compensation, the compensation direction is inverted.

P158 ILLEGAL TIP P

During G46 nose radius compensation, the tip point is illegal (other than 1 to 8).

P170 NO CORR. NO.

The compensation number (D , T

,

H

) command was not given when the tool radius compensation (G41, G42, G43,

G46) command was issued. Alternatively, the compensation number is larger than the number of sets in the specifications.

P172 P10 L-NO. ERR (G10 L-number error)

The L address command is not correct when the G10 command is issued.

P173 G10 P-NO. ERR (G10 compensation error)

When the G10 command is issued, a compensation number not within the permitted number of sets in the specifications has been commanded for the compensation number command.

Remedy

•

Change the G command to that which allows inversion of the compensation direction (G00,

G28, G30, G33, or G53).

•

Exchange with a tool having a different tip point number.

•

Turn on the G46 inversion error avoidance parameter.

•

Change the tip point number to a legal one.

•

Add the compensation number command to the compensation command block.

•

Check the number of compensation number sets and correct it to a compensation number command within the permitted number of compensation sets.

•

Check the address L-Number of the G10 command and correct the number.

•

First check the number of compensation sets and then set the address P designation to within the permitted number of sets.

•

The tool life management data cannot be registered when counting the used data. Turn the used data count valid signal OFF.

P178

Registration of tool life management data with G10 was attempted when the used data count valid signal was ON.

LIFE REGISTRATION OVER

The No. of registration groups, total No. of registered tools or the No. of registrations per group exceeded the specifications range.

Review the No. of registrations.

The maximum No. of registrations is shown below.

System

No. of groups

No. of tools

System 1

80

80

System 2

40/40

40/40

Per group 16

•

The group No. cannot be commanded in duplicate. When registering the group data, register it in group units.

•

Correct to the correct group No.

P179 Group No. Illegal

•

When registering the tool life management data with G10, the group No. was commanded in duplicate.

•

A group No. that was not registered was designated during the T

99 command.

•

An M code command, which must be commanded independently, was issued in the same block as other M code commands.

•

One or more M code commands set in the same group were found in the same block.

326


Error No. Details

P180 NO BORING CYC.

A fixed cycle command was issued though there are not fixed cycle (G72 ~ G89) specifications.

P181 NO S-CMD (TAP)

The spindle speed command has not been issued when the tapping fixed cycle command is given.

P182 SYN TAP ERROR

Connection to the main spindle unit was not established.

Remedy

•


•

Correct the program.

•

•

•

Issue the spindle speed command (S) when the tapping fixed cycle command G84, G74

(G84, G88) is given.

Check connection to the main spindle unit.

Check that the main spindle encoder exists.

The pitch or thread number command has not been issued in the tap cycle of a boring fixed cycle command.

P184 NO PTC/THD CND

The pitch or the number of threads per inch is illegal in the tap cycle of the drilling fixed cycle command

P190 NO CUTTING CYC

A lathe cutting cycle command was input although the lathe cutting cycle was undefined in the specification.

P191 TAPER LENG. ERR

In the lathe cutting cycle, the specified length of taper section is illegal.

•

Specify the pitch data and the number of

•

•

• threads by F or E command.

Check the pitch or the number of threads per inch.

Check the specification.

Delete the lathe cutting cycle command.

Chamfering in the thread cutting cycle is illegal.

P200 NO MRC CYC SPC

A compound type fixed cycle I command

(G70 to G73) was issued although this cycle was undefined in the specification.

P201 PROG. ERR (MRC)

When called with a compound type fixed cycle I command, the subprogram contained at least one of the following commands:

•

Reference point return command (G27,

G28, G30)

•

Thread cutting (G33)

•

Fixed-cycle skip-function (G31)

•

The first move block of the finish shape program in compound type fixed cycle I contains an arc command.

P202 BLOCK OVR (MRC)

The number of blocks in the shape program of the compound type fixed cycle I is over

50.

•

The radius command value in the lathe cutting cycle command must be smaller than the axis shift amount.

•

Set a chamfering amount not exceeding the cycle.

•


•

Delete the following G codes from this subprogram that is called with the compound type fixed cycle I commands (G70 to G73):

G27, G28, G30, G31, G33, fixed-cycle

G-code.

•

Remove G02 and G03 from the first move block of the finish shape program in multiple fixed cycle I.

•

The number of blocks in the shape program called by the compound type fixed cycle I commands (G70 to G73) must be decreased below 50.

327


Error No. Details

P203 CONF. ERR (MRC)

The compound type fixed cycle I (G70 to

G73) shape program could not cut the work normally because it defined an abnormal shape.

Remedy

•

Check the compound type fixed cycle I (G70 to G73) shape program.

•

Check the compound type fixed cycle (G70 to

G76) command value.

A command value of the compound type fixed cycle (G70 to G76) is illegal.

P210 NO PAT CYC SPC

A compound type fixed cycle II (G74 to

G76) command was input although it was undefined in the specification.

P220 NO SPECIAL CYC

No special fixed cycle specifications are available.

P221 NO HOLE (S-CYC)

A 0 has been specified for the number of holes in special fixed cycle mode.

P222 G36 ANGLE ERR

A G36 command specifies 0 for angle intervals.

P223 G12, G13 R ERR

The radius value specified with a G12 or G13 command is below the compensation amount.

P224 NO G12, G13 SPEC

There are no circular cutting specifications.

•

•

•

•

•

•



Review the program.

Review the program.

Review the program.


A subprogram has been called 8 or more times in succession from the subprogram.

At subprogram call time, the sequence number set at return from the subprogram or specified by GOTO, was not set.

•

Check the number of subprogram calls and correct the program so that it does not exceed

8 times.

•

Specify the sequence numbers in the call block of the subprogram.

•

When using the IC card, check the program in the IC card and the number of IC card program calls.

•

Enter the subprogram.

•

Check the program number in the IC card.

P232 NO PROGRAM NO.

The subprogram has not been set when the subprogram is called.

P241 NO VARI NUMBER

The variable number commanded is higher than the numbers in the specifications.

P242 EQL. SYM. MSSG.

The "=" sign has not been commanded when a variable is defined.

•

•

•


Check the program variable number.

Designate the "=" sign in the variable definition of the program.

•

Correct the program.

An invalid variable has been specified in the left or right side of an operation expression.

P260 NO COOD-RT SPC

The coordinate rotation command was issued when the coordinate rotation specifications were not available.

•


328


Error No. Details

P270 NO MACRO SPEC

A macro specification was commanded though there are no such command specifications.

P271 NO MACRO INT.

A macro interrupt command has been issued though it is not included in the specifications.

Remedy

•


•


An NC statement and a macro statement exist together in the same block.

•

Review the program and place the executable statement and macro statement in separate blocks.

•

Review the program and correct it so that the macro calls do not exceed the limit imposed by the specification.

The frequency of the macro call has exceeded the limit imposed by the specification.

P275 MACRO ARG. EX.

The number of macro call argument type II sets has exceeded the limit.

•

Review the program.

P277

A G67 command was issued though it was not during the G66 command modal.

MACRO ALM MESG

An alarm command has been issued in

#3000.

•

Review the program.

•

The G67 command is the call cancel command and so the G66 command must be designated first before it is issued.

•

Refer to the operator messages on the DIAG screen.

•

Refer to the instruction manual issued by the machine manufacturer.

•

Review the program and correct it so the number of " [ " or " ] " does not exceed five.

P280 EXC [ , ]

The number of parentheses [ , ] which can be commanded in a single block has exceeded five.

P281 [ , ] ILLEGAL

The number of " [" and " ] " parentheses commanded in a single block does not match.

•

Review the program and correct it so that " [ " and " ] " parentheses are paired up properly.

•

Review the program and correct the formula.

The arithmetic formula is incorrect.

P283 DIVIDE BY ZERO

The denominator of the division is zero.

In the process of the calculation the integral number has exceeded –2

31

(2

31

–1).

•

Review the program and correct it so that the denominator for division in the formula is not zero.

•

Check the arithmetic formula in the program and correct it so that the value of the integral number after calculation does not exceed

−

2

31

.

•

Check the variable data in the program.

The variable data has overflowed.

P290 IF SNT. ERR

There is an error in the IF conditional

GOTO

statement.

P291 WHILE SNT. ERR

There is an error in the WHILE conditional

DO

~END

statement.

•

•

Review the program.

Review the program.

329


Error No. Details

P292 SETVN SNT. ERR

There is an error in the SETVN

statement when the variable name setting was made.

The number of

s for DO-END

WHILE conditional DO has exceeded 27.

-END

in the

statement

Remedy

•

Review the program.

•

The number of characters in the variable name of the SETVN statement must be 7 or less.

•

Review the program and correct it so that the number of the DO-END statement does not exceed 27.

The DO’s and END’s are not paired off properly.

•

Review the program and correct it so that the

DO and END are paired off properly.

There is a WHILE or GOTO statement on the tape during tape operation.

•

During tape operation, a program which includes a WHILE or GOTO statement cannot be executed and so the memory operation mode is established instead.

•

Review the program.

P296 NO MACRO ADDR.

A required address has not been specified in the user macro.

•

Review the program.

The user macro does not use address A as a variable.

P298 PTR OP (MACRO)

User macro G200, G201, or G202 was specified during tape or MDI operation.

P300 VAR. NAME ERROR

The variable names have not been commanded properly.

P301 VAR NAME DUPLI

The name of the variable has been duplicated.

P360 NO PROG. MIRR

A mirror image (G50.1 or G51.1) command has been issued though the programmable mirror image specifications are not provided.

P380 NO CORNER R/C

A command was issued for corner rounding or corner chamfering though there are no such specifications.

P381 NO ARC R/C SPC

Corner rounding or chamfering was specified in the arc interpolation block although corner chamfering/corner rounding II is unsupported.

P382 CORNER NO MOVE

The block next to corner rounding/ chamfering is not a movement command.

•

•

•

•

•

•

•

•

Review the program.

Review the variable names in the program and correct them.

Correct the program so that the name is not duplicated.



Remove the corner rounding or chamfering command from the program.


Replace the block succeeding the corner rounding/chamfering command by movement command block.

330


Error No. Details

In the corner rounding or chamfering command, the movement distance was shorter than the value in the corresponding command.

Remedy

•

Make the corner rounding or chamfering less than the movement distance since this distance is shorter than the corner rounding or chamfering.

When the corner rounding or chamfering command was input, the movement distance in the following block was shorter than the length of the corner rounding or chamfering.

P385 G0 G33 IN CORN

A block with corner rounding/chamfering was given during G00 or G33 modal.

•

Make the corner rounding or chamfering less than the movement distance since this distance in the following block is shorter than the corner rounding or chamfering.

•

Recheck the program.

•


A geometric command was issued though there are no geometric specifications.

P391 NO GEOMETRIC 2

There are no geometric IB specification.

P392 LES AGL (GEOMT)

The angular difference between the geometric line and line is 1

°

or less.

P393 INC ERR (GEOMT)

The second geometric block was specified by an incremental value.

P394 NO G01 (GEOMT)

The second geometric block contains no linear command.

P395 NO ADRS (GEOMT)

The geometric format is invalid.

P396 PL CHG. (GEOMT)

A plane switching command was executed during geometric command processing.

P397 ARC END EPR (GEOMT)

In geometric IB, the circular arc end point does not contact or cross the next block start point.

P398 NO GEOMT IB

Although the geometric IB specifications are not included, a geometric command is given.

•

•

•

•

•

•

•

•


Correct the geometric angle.

Specify this block by an absolute value.

Specify the G01 command.

Recheck the program.

Execute the plane switching command before geometric command processing.

Recheck the geometric circular arc command and the preceding and following commands.


•


Although the programmable parameter input specifications are not provided, the command was given.

331


Error No. Details

P421 PRAM IN ERROR

•

The specified parameter number or set data is illegal.

•

An illegal G command address was input in parameter input mode.

•

A parameter input command was input during fixed-cycle modal or nose R compensation.

P430 AXIS NOT RET.

•

A command was issued to move an axis, which has not returned to the reference point, away from that reference point.

•

A command was issued to an axis removal axis.

P431 NO 2ND REF.

A command for second, third or fourth reference point return was issued though there are no such command specifications.

Remedy

•

Check the program.

•

Execute reference point return manually.

•

The command was issued to an axis for which axis removal is validated so invalidate axis removal.

•


•

Check the program.

One of the axes did not return to the start position when the origin point collate command (G27) was executed.

An M command was issued simultaneously in the G27 command block.

An M command was issued simultaneously in the G29 command block.

•

An M code command cannot be issued in a

G27 command block and so the G27 command and M code command must be placed in separate blocks.

•

An M code command cannot be issued in a

G29 command block and so the G29 command and M code command must be placed in separate blocks.

•


P450 NO CHUCK BARR.

The chuck barrier on command (G22) was specified although the chuck barrier was undefined in the specification.

P460 TAPE I/O ERROR

An error has arisen in the tape reader or, alternatively, in the printer during macro printing.

•

•

Check the power and cable for the connected device.

Check the input/output unit parameters.

A file of the machining program cannot be read.

•

During memory operation, the program saved in the memory may be corrupted. Output all of the programs and tool data, etc., once, and format the memory.

•


P600 NO AUTO TLM

An automatic tool length measurement command (G37) was executed though there are no such command specifications.

P601 NO SKIP SPEC

A skip command (G31) was issued though there are no such command specifications.

•


332


Error No. Details

Remedy

•


A multiple skipping command (G31.1,

G31.2 or G31.3) was issued though there are no such command specifications.

P603 SKIP SPEED F0

The skip speed is 0.

P604 TLM ILL. AXIS command

No axis or more than one axis was specified in the automatic tool length measurement block.

P605 T-CMD IN BLOCK

The T code is in the same block as the automatic tool length measurement block.

P606 NO T-CMD BEFOR

The T code was not yet specified in automatic tool length measurement.

P607 TLM ILL. SIGNL

Before the area specified by the D command or decelerating area parameter d, the measurement position arrival signal went ON. The signal remains OFF to the end.

P608 SKIP ERROR (CC)

A skip command was specified during tool radius compensation processing.

P610

ILLEGAL PARA.

•

G114.1 was commanded when the spindle synchronization with PLC I/F command was selected.

•

Spindle synchronization was commanded to a spindle that is not connected serially.

P701

REGARD A POINT

A decimal point was added to a decimal point invalid address.

•

Specify the skip speed.

•

Specify one axis.

•

Specify this T code before the automatic tool length measurement block.

•

Specify this T code before the block.

•

Check the program.

•

Specify a diameter cancel (G40) command, or remove the skip command.

•

Check the program.

•

Check the argument of G114.1 command.

•

Check the state of spindle connection.

• Do not add a decimal point to the decimal point invalid address.

•

Reduce the number of commands that require pre-reading or delete such commands. combining commands that required pre-reading (nose R offset, corner chamfering corner R, geometric I, geometric IB, and compound type fixed cycle commands) resulted in eight or more pre-read blocks.

333

Appendix 3. Order of G Function Command Priority


(Command in a separate block when possible)

(Note)

Upper level: When commanded in the same block indicates that both commands are executed simultaneously

G code

Commanded

G code

01

G00 ~ G03

G00~G03.1

Positioning/ interpolation

G command commanded last is valid.

Group 1 modal is updated

02

G17 ~ G19

Also possible during arc modal

03

G90, G91

05

G94, G95

06

G20, G21

07

G40 ~ G42

08

G43, G44,

G49

Arc and G41,

G42 cause error P151

Arc and G43~

G49 cause error P70

Radius is compensated, and then moves

The G49 movement in the arc modal moves with

G01

G04 is executed

G04 is executed

G40~G42 are ignored

G43~G49 are ignored

G04

Dwell

Group 1 modal is updated

G04 is executed

G09

Exact stop check

G10, G11

Program data setting

G10 is priority for axis

G10 is used for axis, so the

No movement selected plan axis will be the

I, J, K rotation basic axis. input

G17 ~ G19

Plane selection


G10, G11 are executed


G40~G42 are ignored

G43~G49 are ignored

Plane axis changeover during radius compensation causes error P112

334


G code

Commanded

01

G00 ~ G03

G code

G20, G21

Inch/metric changeover

02

G17 ~ G19

G27 ~ G30

G00~G03.1 modals are

Reference point updated compare/ return

G27~G30 are executed

G31 ~ G31.3

Skip

G33

Thread cutting


G37

G37 is executed


G00~G33 are ignored

Arc and G41,

G42 cause error P151

G40 ~ G42

Tool radius compensation

G41 and G42 in arc modal cause error

P151

Plane axis changeover during radius compensation causes error P112

03

G90, G91

05

G94, G95

06

G20, G21

07

G40 ~ G42

08

G43, G44,

G49

Possible in same block



G40~G42 are ignored

G43~G49 are ignored

Error:P608

Error:P608

G37 is executed

G37 is executed

G40~G42 are ignored

G43~G49 are ignored


335


G code

Commanded

09

G73 ~ G89

G code

Group 1 command is executed

Group 9 is canceled G00~G03.1

Positioning/ interpolation

10

G98, G99

12

G54 ~ G59

13

G61 ~ G64

14

G66 ~ G67

G66 ~ G67 are executed

G00~G03.1 modals are updated

17

G96, G97

G04

Dwell

G04 is executed

G73~G89 are ignored

G09

Exact stop check

G10, G11

Program data setting


G73~G89 are ignored

G17 ~ G19

Plane selection

G04 is executed

Group 12 is changed

G10 is executed

G54~G59 modals are updated


G10 is ignored

19

G50.1

G51.1

During the arc command, all axis names become mirror center data

Movement with mirror shape executed

G50.1 and

G51.1 are ignored


G50.1 and

G51.1 are ignored

336


G code

Commanded

09

G73 ~ G89

G code

G20, G21

Inch/metric changeover

G27 ~ G30

Reference point compare/ return

G31 ~ G31.3

Skip

Group 1 command is executed

G33

Thread cutting

Group 9 is canceled

G37


Error:P155

G40 ~ G42

Tool radius compensation

Error:P155

10

G98, G99

12

G54 ~ G59

13

G61 ~ G64

14

G66

~

G67


G27~G30 are ignored


G33 modals is updated


G37 modals is ignored

17

G96, G97

19

G50.1

G51.1


G50.1 and

G51.1 are ignored executed

G50.1 and

G51.1 are ignored

337


G code

G00~G03.1

Commanded

01

G33

G code

G43, G44, G49 error P70

Length

Arc and G43,

G44 cause compensation

G50.1

G51.1

Program mirror image

G52


G53


02

G17 ~ G19

G54 ~ G59


G61 ~ G64

Mode selection

G65 is executed

G65

Macro call


03

G90, G91

05

G94, G95

06

G20, G21

07

G40 ~ G42

08

G43, G44,

G49


G52 is executed

G52 is executed

G40~G42 are ignored

G43~G49 are ignored

G53 is executed

G53 is executed

G40~G42 are ignored

G40~G42 are ignored


G65 is executed

338


G code

G00~G03.1

Commanded

01

G33

G code


G66 ~ G67

Macro call


02

G17, G19

03

G90, G92

G73~G89 are canceled

G73 ~ G89

Canned cycle


G90, G91

Absolute value/ incremental value

G92


G94, G95

Synchronous/ asynchronous

G96, G97

Constant surface speed control

G98, G99

Initial point/ R point return

Use in same block

05

G94, G95

commanded last is valid.

06

G20, G21

07

G40 ~ G42

08

G43, G44

G49

Error:P155

Canned cycle during compensa-tio n



Error:P155

339


G code

Commanded

09

G73 ~ G89

G code

G43, G44, G49

Length compensation

G50.1

G51.1

Program mirror image

G52


G52 is executed

G73~G89 are ignored

G53


G54 ~ G59


G61 ~ G64

Mode selection

G65

Macro call

G65 is executed

G73~G89 are ignored

10

G98, G99

12

G54 ~ G59

13

G61 ~ G65

14

G66

~

G67




G50.1

G51.1 is ignored





Error

17

G96, G97

19

G50.1

G51.1

executed

G50.1

G51.1 is ignored commanded last is valid. executed

G50.1

G51.1 is ignored executed

G50.1

G51.1 is invalid

340


G code

Commanded

09

G73 ~ G89

G code

G66 ~ G67

Macro call


G73~G89 are ignored

10

G98, G99

G73 ~ G89

Canned cycle


12

G54 ~ G59



G90, G91

Absolute value/ incremental value

G92

G92 is executed


G73~G89 are ignored

G94, G95

Synchronous/ asynchronous

G96, G97

Constant surface speed control

G98, G99

Initial point/R point return


13

G61 ~ G67

14

G66 ~ G67



G73~G89 are ignored

17

G96, G97


19

G50.1

G51.1


G50.1

G51.1 is ignored

All axes become mirror center

Note that G92 is priority for axis

341

Date of revision Manual No. Revision details

December 2000 BNP-B2260

∗

First edition created.

May 2004 BNP-B2260B • The contents revised following to the software Ver.C and Ver.D.

• Mistakes, etc. were corrected.

Notice

Every effort has been made to keep up with software and hardware revisions in the contents described in this manual. However, please understand that in some unavoidable cases simultaneous revision is not possible.

Please contact your Mitsubishi Electric dealer with any questions or comments regarding the use of this product.

Duplication Prohibited

This instruction manual may not be reproduced in any form, in part or in whole, without written permission from Mitsubishi Electric Corporation.

©

2000-2004 MITSUBISHI ELECTRIC CORPORATION

ALL RIGHTS RESERVED

(0405) MEE

MITSUBISHI ELECTRIC CORPORATION

HEAD OFFICE : MITSUBISHI DENKI BLDG., 2-2-3, MARUNOUCHI, CHIYODA-KU, TOKYO 100-8310, JAPAN

MODEL

MODEL

CODE

Manual No.

MC6/C64/C64T(M/T)

008-047

BNP-B2260B （ ENG)

Specifications subject to change without notice.

Printed in Japan on recycled paper.

Mitsubishi Electric C6/C64/C64T Programming Manual

PROGRAMMING MANUAL

(MACHINING CENTER/TRANSFER MACHINE TYPE)

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 company.

This manual is a guide for using the MELDAS C6/C64/C64T.

Programming is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study the "Precautions for Safety" on the following page to ensure safe use of the this NC unit.

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

MELDAS C6/C64/C64T Instruction Manual ........ BNP-B2259

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".

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

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

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

Note that even items ranked as "

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

©

MITSUBISHI ELECTRIC CORPORATION

Related manuals

Table of contents

Mitsubishi Electric C6/C64/C64T Programming Manual

PROGRAMMING MANUAL

(MACHINING CENTER/TRANSFER MACHINE TYPE)

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 company.

This manual is a guide for using the MELDAS C6/C64/C64T.

Programming is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study the "Precautions for Safety" on the following page to ensure safe use of the this NC unit.

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

MELDAS C6/C64/C64T Instruction Manual ........ BNP-B2259

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".

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

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

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

Note that even items ranked as "

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

©

MITSUBISHI ELECTRIC CORPORATION

Related manuals

Mitsubishi Electric

C6/C64/C64T

Mitsubishi Electric

C70

Mitsubishi Electric

M600L Series

Mitsubishi Electric

C70

Mitsubishi Electric

EZ Motion E60/E68 Series

Mitsubishi Electric

EZ Motion E60/E68 Series

Mitsubishi Electric

M60/M60S MAGIC64 Series

Mitsubishi Electric

E70 Series

Mitsubishi Electric

700/70 Series

Mitsubishi Electric

E70 Series

Mitsubishi Electric

M700V/M70V Series

Mitsubishi Electric

700/70 Series

Table of contents