Content      ..     7      8      9      10     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. OPERATOR'S MANUAL - page 9

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

G66 P9110 Z-20.0 R5.0 F500 ;

G90 X20.0 Y20.0 ;

X50.0 ;

Y50.0 ;

X70.0 Y80.0 ;

G67 ;

M30 ;

-

Macro program (program called)

O9110 ;

#1=#4001 ;

Stores G00/G01.

#3=#4003 ;

Stores G90/G91.

#4=#4109 ;

Stores the cutting feedrate.

#5=#5003 ;

Stores the Z coordinate at the start of drilling.

G00 G90 Z#18 ;

Positioning at position R

G01 Z#26 F#9 ;

Cutting feed to position Z

IF[#4010 EQ 98]GOTO 1 ;

Return to position I

G00 Z#18 ;

Positioning at position R

GOTO 2 ;

N1 G00 Z#5 ;

Positioning at position I

N2 G#1 G#3 F#4 ;

Restores modal information.

M99 ;

Sample program

T

This program makes a groove at a specified position.

U

-

Calling format

G66 P9110 Uu Ff

;

U : Groove depth (incremental programming)

F

: Cutting feed of grooving

-

Program that calls a macro program

O0003 ;

G50 X100.0 Z200.0 ;

S1000 M03 ;

G66 P9110 U5.0 F0.5 ;

G00 X60.0 Z80.0 ;

Z50.0 ;

Z30.0 ;

G67 ;

G00 X00.0 Z200.0 M05 ;

- 216 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

M30 ;

-

Macro program (program called)

O9110 ;

G01 U-#21 F#9 ;

Cuts the workpiece.

G00 U#21 ;

Retracts the tool.

M99 ;

14.7.3 Macro Call Using a G Code

By setting a G code number used to call a macro program in a parameter, the macro program can be

called in the same way as for a simple call (G65).

O0001 ;

O9010 ;

:

:

G81 X10.0 Y20.0 Z-10.0 ;

:

:

:

M30 ;

N9 M99 ;

Parameter No.6050=81

Explanation

By setting a G code number from -9999 to 9999 used to call a custom macro program (O9010 to O9019)

in the corresponding parameter (No.6050 to No.6059), the macro program can be called in the same way

as with G65.

If a negative G code is set, a modal call (equivalent to G66) is made.

For example, when a parameter is set so that macro program O9010 can be called with G81, a

user-specific cycle created using a custom macro can be called without modifying the machining

program.

-

Correspondence between parameter numbers and program numbers

Parameter number

Program number

6050

O9010

6051

O9011

6052

O9012

6053

O9013

6054

O9014

6055

O9015

6056

O9016

6057

O9017

6058

O9018

6059

O9019

-

Repetition

As with a simple call, a number of repetitions from 1 to 99999999 can be specified at address L.

-

Argument specification

As with a simple call, two types of argument specification are available: Argument specification I and

argument specification II. The type of argument specification is determined automatically according to

the addresses used.

- 217 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Limitation

-

Nesting of calls using G codes

• To call another program in a program called using a G code, only G65, M98, or G66 can be used

normally.

• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using an M code, T code, or specific

code can be performed in a program called using a G code.

14.7.4 Macro Call Using a G Code (Specification of Multiple

Definitions)

By setting the starting G code number used to call a macro program, the number of the starting program

to be called, and the number of definitions, macro calls using multiple G codes can be defined.

Explanation

As many custom macros as the number specified in parameter No. 6040 can be called using as many G

codes as the number specified in parameter No. 6040. The numeric value set in parameter No. 6038

indicates the starting G code number and the program number set in parameter No. 6039 indicates the

starting program number. To disable this type of call, set 0 in parameter No. 6040.

If parameter No. 6038 is set to a negative G code, a modal call (equivalent to G66) is made.

The number of repetitions and argument specification are set in the same way as with a macro call using a

G code.

[Example]

Set parameter No. 6038 to 900, parameter No. 6039 to 1000, and parameter No. 6040 to 100.

G900 → O1000

G901 → O1001

G902 → O1002

:

G999 → O1099

Custom macro calls (simple calls) for 100 combinations are defined as shown above. When parameter

No. 6038 is changed to -900, custom macro calls (modal calls) for the same combinations are defined.

NOTE

1 The calls defined by this setting become all invalid in the following cases:

<1> A value outside the valid data range is set in one of the above parameters.

<2> (Setting of parameter No.6039 + Setting of parameter No.6040 - 1) > 9999

2 Simple and modal calls cannot be mixed in the specification.

3 If the G code set in parameter Nos. 6050 to 6059 to call the corresponding

macro program is within the G code range for calling programs using multiple G

codes, the macro program corresponding to the G code set in parameter Nos.

6050 to 6059 is called.

14.7.5 Macro Call Using an M Code

By setting an M code number used to call a macro program in a parameter, the macro program can be

called in the same way as with a simple call (G65).

O0001 ;

O9020 ;

:

:

M50 A1.0 B2.0 ;

:

:

:

M30 ;

M99 ;

Parameter No.6080=50

- 218 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Explanation

By setting an M code number from 3 to 99999999 used to call custom macro program O9020 to O9029 in

the corresponding parameter (Nos. 6080 to 6089), the macro program can be called in the same way as

with G65.

-

Correspondence between parameter numbers and program numbers

Parameter number

Corresponding program number

6080

O9020

6081

O9021

6082

O9022

6083

O9023

6084

O9024

6085

O9025

6086

O9026

6087

O9027

6088

O9028

6089

O9029

Example)

When parameter No. 6080 is set to 990, O9020 is called using M990.

-

Repetition

As with a simple call, a number of repetitions from 1 to 99999999 can be specified at address L.

-

Argument specification

As with a simple call, two types of argument specification are available: Argument specification I and

argument specification II. The type of argument specification is determined automatically according to

the addresses used.

Limitation

• An M code used to call a macro program must be specified at the start of a block.

• To call another program in a program called using an M code, only G65, M98, or G66 can be used

normally.

• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a G code can be performed in a

program called using an M code.

14.7.6 Macro Call Using an M Code (Specification of Multiple

Definitions)

By setting the starting M code number used to call a macro program, the number of the starting program

to be called, and the number of definitions, macro calls using multiple M codes can be defined.

Explanation

As many custom macros as the number specified in parameter No. 6049 can be called using as many M

codes as the number specified in parameter No. 6049. The numeric value set in parameter No. 6047

indicates the starting M code number and the program number set in parameter No. 6048 indicates the

starting program number. To disable this type of call, set 0 in parameter No. 6049.

The number of repetitions and argument specification are set in the same way as with a macro call using a

M code.

- 219 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

[Example]

Set parameter No. 6047 to 90000000, parameter No. 6048 to 4000, and parameter No. 6049 to 100.

M90000000 → O4000

M90000001 → O4001

M90000002 → O4002

:

M90000099 → O4099

Custom macro calls (simple calls) for 100 combinations are defined as shown above.

NOTE

1 The calls defined by this setting become all invalid in the following cases:

<1> A value outside the valid data range is set in one of the above parameters.

<2> (Setting of parameter No.6048 + Setting of parameter No.6049 - 1) > 9999

2 If the M code set in parameter Nos. 6080 to 6089 to call the corresponding

macro program is within the M code range for calling programs using multiple M

codes, the macro program corresponding to the M code set in parameter Nos.

6080 to 6089 is called.

14.7.7 Subprogram Call Using an M Code

By setting an M code number used to call a subprogram (macro program) in a parameter, the macro

program can be called in the same way as with a subprogram call (M98).

O0001 ;

O9001 ;

:

:

M03 ;

:

:

:

M30 ;

M99 ;

Parameter No.6071=03

Explanation

By setting an M code number from 3 to 99999999 used to call subprogram O9001 to O9009 in the

corresponding parameters Nos. 6071 to 6079, the subprogram can be called in the same way as with M98.

-

Correspondence between parameter numbers and program numbers

Parameter number

Program number

6071

O9001

6072

O9002

6073

O9003

6074

O9004

6075

O9005

6076

O9006

6077

O9007

6078

O9008

6079

O9009

-

Repetition

As with a simple call, a number of repetitions from 1 to 99999999 can be specified at address L.

-

Argument specification

Argument specification is not allowed.

- 220 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

-

M code

An M code in a macro program that has been called is treated as an ordinary M code.

Limitation

• To call another program in a program called using an M code, only G65, M98, or G66 can be used

normally.

• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a G code can be performed in a

program called using an M code.

14.7.8 Subprogram Call Using an M Code (Specification of Multiple

Definitions)

By setting the starting M code number used to call a subprogram, the number of the starting subprogram

to be called, and the number of definitions, subprogram calls using multiple M codes can be defined.

Explanation

As many sub programs as the number specified in parameter No. 6046 can be called using as many M

codes as the number specified in parameter No. 6046. The numeric value set in parameter No. 6044

indicates the starting M code number and the program number set in parameter No. 6045 indicates the

starting program number. To disable this type of call, set 0 in parameter No. 6046.

[Example]

Set parameter No. 6044 to 80000000, parameter No. 6045 to 3000, and parameter No. 6046 to 100.

M80000000 → O3000

M80000001 → O3001

M80000002 → O3002

:

M80000099 → O3099

Subprogram calls for 100 combinations are defined as shown above.

NOTE

1 The calls defined by this setting become all invalid in the following cases:

<1> A value outside the valid data range is set in one of the above parameters.

<2> (Setting of parameter No.6045 + Setting of parameter No.6046 - 1) > 9999

2 If the M code set in parameter Nos. 6071 to 6079 to call the corresponding

subprogram is within the M code range for calling subprograms using multiple M

codes, the subprogram corresponding to the M code set in parameter Nos. 6071

to 6079 is called.

14.7.9 Subprogram Calls Using a T Code

By enabling subprograms to be called with a T code in a parameter, a subprogram can be called each time

the T code is specified in the machining program.

O0001 ;

O9000 ;

:

:

T23 ;

:

:

:

M30 ;

M99 ;

Bit 5 (TCS) of parameter No. 6001 = 1

- 221 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Explanation

-

Call

By setting bit 5 (TCS) of parameter No. 6001 to 1, subprogram O9000 can be called each time a T code is

specified in a machining program. A T code specified in a machining program is assigned to common

variable #149.

-

Repetition

As with a simple call, a number of repetitions from 1 to 99999999 can be specified at address L.

-

Argument specification

Argument specification is not allowed.

Limitation

• To call another program in a program called using a T code, only G65, M98, or G66 can be used

normally.

• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a G code can be performed in a

program called using a T code.

14.7.10 Subprogram Call Using a Specific Address

By enabling subprograms to be called with a specific address in a parameter, a subprogram can be called

each time the specific address is specified in the machining program.

O0001 ;

O9004 ;(#146=100.)

:

:

B100. ;

:

:

:

M30 ;

M99 ;

Parameter No.6090=66(B)

Explanation

-

Call

By setting the code (ASCII code converted to decimal) corresponding to a specific address in parameter

No. 6090 or No. 6091, the custom macro program, O9004 or O9005, corresponding to each parameter can

be called when the specific address is specified in a machining program. The code value corresponding

to a specific address specified in a machining program is assigned to the common variables (#146, #147).

The table below indicates the addresses that can be set.

M

Address

Parameter setting

A

65

B

66

D

68

F

70

H

72

I

73

J

74

K

75

L

76

M

77

P

80

Q

81

- 222 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Address

Parameter setting

R

82

S

83

T

84

V

86

X

88

Y

89

Z

90

NOTE

When address L is set, the number of repetitions cannot be set.

T

Address

Parameter setting

A

65

B

66

F

70

H

72

I

73

J

74

K

75

L

76

M

77

P

80

Q

81

R

82

S

83

T

84

NOTE

When address L is set, the number of repetitions cannot be set.

-

Correspondence between parameter numbers and program numbers and

between the parameter numbers and common variables

Parameter number

Program number

Common variable

6090

O9004

#146

6091

O9005

#147

-

Repetition

As with a simple call, a number of repetitions from 1 to 99999999 can be specified at address L.

-

Argument specification

Argument specification is not allowed.

Limitation

• To call another program in a program called using a specific address, only G65, M98, or G66 can be

used normally.

• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a G code can be performed in a

program called using a specific address.

- 223 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Sample program

By using the subprogram call function that uses M codes, the cumulative usage time of each tool is

measured.

Conditions

• The cumulative usage time of each of tools T01 to T05 is measured.

No measurement is made for tools with numbers greater than T05.

• The following variables are used to store the tool numbers and measured times:

#501

Cumulative usage time of tool number 1

#502

Cumulative usage time of tool number 2

#503

Cumulative usage time of tool number 3

#504

Cumulative usage time of tool number 4

#505

Cumulative usage time of tool number 5

• Usage time starts being counted when the M03 command is specified and stops when M05 is

specified. System variable #3002 is used to measure the time during which the cycle start lamp is

on. The time during which the machine is stopped by feed hold and single block stop operation is

not counted, but the time used to change tools and pallets is included.

Operation check

-

Parameter setting

Set 3 in parameter No.6071, and set 5 in parameter No.6072.

-

Variable value setting

Set 0 in variables #501 to #505.

-

Program that calls a macro program

O0001 ;

T01 M06 ;

M03 ;

:

M05 ;

Changes #501.

T02 M06 ;

M03 ;

:

M05 ;

Changes #502.

T03 M06 ;

M03 ;

:

M05 ;

Changes #503.

T04 M06 ;

M03 ;

:

M05 ;

Changes #504.

T05 M06 ;

M03 ;

:

M05 ;

Changes #505.

M30 ;

-

Macro program (program called)

O9001(M03) ;

Macro to start counting

M01 ;

IF[#4120 EQ 0]GOTO 9 ;

No tool specified

IF[#4120 GT 5]GOTO 9 ;

Out-of-range tool number

- 224 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

#3002=0 ;

Clears the timer.

N9 M03 ;

Rotates the spindle in the

M99 ;

forward direction.

O9002(M05) ;

Macro to end counting

M01 ;

IF[#4120 EQ 0]GOTO 9 ;

No tool specified

IF[#4120 GT 5]GOTO 9 ;

Out-of-range tool number

#[500+#4120]=#3002+#[500+#4120] ;

Calculates cumulative time.

N9 M05 ;

Stops the spindle.

M99 ;

14.8 PROCESSING MACRO STATEMENTS

For smooth machining, the CNC prereads the NC statement to be performed next. This operation is

referred to as buffering. For example, many NC statements are buffered during look-ahead by AI

advanced preview control (M series) / AI contour control (M series).

In the cutter compensation mode (G41 or G42) for M series, the CNC prereads the NC statements at least

three blocks ahead to find intersections even if look-ahead by AI contour control and so forth is not

applied.

Macro statements for arithmetic expressions and conditional branches are processed as soon as they are

read into the buffer. Therefore, the timing of the macro statement execution is not always the specified

order.

At the blocks containing M00, M01, M02 or M30, blocks containing M-codes for which buffering is

suppressed by setting parameters Nos. 3411 to 3420 and No.3421 to 3432, and blocks containing

prevention buffering G codes such as G31 or G53, the CNC stops to preread the NC statement after that.

Then, the stop of the macro statement execution is guaranteed until such M codes or G codes complete its

execution.

Explanation

-

When the next block is not buffered (M codes that are not buffered, G31, etc.)

> N1 G31 X100.0 ;

N1

NC statement

N2 #100=1

:

execution

N2

Macro statement execution

> :Block being executed

Buffer

CAUTION

In case that you need to execute the macro statement after completing the block

just before the macro statement, specify M code or G code that is not buffered

just before the macro statement. Specially, in case of reading/writing the system

variables to control signals, coordinates, offset value, etc., it may different system

variable data by the timing of the NC statement execution. To avoid this

phenomenon, specify such M codes or G codes before the macro statement, if

necessary.

- 225 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

-

Buffering the next block in other than cutter compensation mode (G41, G42)

> N1 X100.0 ;

N1

N4

NC statement

execution

N2 #1=100 ;

N3 #2=200 ;

N2

N3

Macro statement

N4 Y200.0 ;

execution

Buffer

N4

> : Block being executed

: Block read into the buffer

When N1 is being executed, the next NC statement (N4) is read into the buffer.

The macro statements

(N2, N3) between N1 and N4 are processed during execution of N1.

-

In cutter compensation mode (G41, G42)

M

> N1 G01 G41 X100.0 F100 Dd ;

N2 #1=100 ;

> : Block being executed

N3 Y100.0 ;

: Blocks read into the buffer

N4 #2=200 ;

N5 Y150.0 ;

N6 #3=300 ;

N7 X200.0 ;

:

N1

N3

NC statement

execution

N2

N4

N6

Macro statement

execution

N3

N5

N7

Buffer

When N1 is being executed, the NC statements in the next three blocks (up to N7) are read into the buffer.

The macro statements (N1, N4, N6) between N1 and N7 are processed during execution of N1.

14.9 REGISTERING CUSTOM MACRO PROGRAMS

Custom macro programs are similar to subprograms. They can be registered and edited in the same way

as subprograms. The storage capacity is determined by the total length of tape used to store both custom

macros and subprograms.

- 226 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

14.10 CODES AND RESERVED WORDS USED IN CUSTOM

MACROS

In addition to the codes used in ordinary programs, the following codes are used in custom macro

programs.

Explanation

-

Codes

(1)

When the ISO code is used or when bit 4 (ISO) of parameter No. 6008 is set to 0

(The codes are represented in hexadecimal.)

Meaning

Code

0AAh

=

0BDh

#

0A3h

[

0DBh

]

0DDh

?

03Fh

@

0C0h

&

0A6h

_

05Fh

O

0CFh

(2)

When the EIA code is used or when the ISO code is used with bit 4 (ISO) of parameter No. 6008 set

to 1

Meaning

Code

Code set in parameter No. 6010

=

Code set in parameter No. 6011

#

Code set in parameter No. 6012

[

Code set in parameter No. 6013

]

Code set in parameter No. 6014

?

Code set in parameter No. 6015

@

Code set in parameter No. 6016

&

Code set in parameter No. 6017

_

Code set in parameter No. 6018

For O, the same code as for O indicating a program number is used. Set a hole pattern for each of *, =, #,

[, ], ?, @, &, and _ in the ISO or EIA code in the corresponding parameter (Nos. 6010 to 6018).

The code 00h cannot be used. The code indicating an alphabetic character can be used for the code

indicating a character listed above, but the code can be no longer used to indicate the original character.

-

Reserved words

The following reserved words are used in custom macros:

AND, OR, XOR, MOD, EQ, NE, GT, LT, GE, LE, SIN, COS, TAN, ASIN, ACOS, ATAN, ATN, SQRT,

SQR, ABS, BIN, BCD, ROUND, RND, FIX, FUP, LN, EXP, POW, ADP, IF, GOTO, WHILE, DO,

END, BPRNT, DPRNT, POPEN, PCLOS, SETVN

System variable (constant) names and registered common variable names are also used as reserved words.

- 227 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

14.11 EXTERNAL OUTPUT COMMANDS

In addition to the standard custom macro commands, the following macro commands are available.

They are referred to as external output commands.

• BPRNT

• DPRNT

• POPEN

• PCLOS

These commands are provided to output variable values and characters through the reader/puncher

interface.

Explanation

Specify these commands in the following order:

Open command: POPEN

Before specifying a sequence of data output commands, specify this command to establish a

connection to an external input/output device.

Data output command: BPRNT or DPRNT

Specify necessary data output.

Close command: PCLOS

When all data output commands have completed, specify PCLOS to release a connection to an

external input/output device.

-

Open command POPEN

The POPEN command establishes a connection to an external input/output device. It must be specified

before a sequence of data output commands. The CNC outputs a DC2 control code.

-

Data output command BPRNT

The BPRNT command outputs characters and variable values in binary.

BPRNT [ a

#b

[c] … ]

Number of significant decimal places

Variable

Character

(i)

Specified characters are converted to the codes according to the setting data (ISO) that is output at

that time.

Specifiable characters are as follows:

• Letters (A to Z)

• Numbers

• Special characters (*, /, +, -, ?, @, &, _)

NOTE

1 An asterisk (*) is output by a space code.

2 When using ?, @, &, and/or _, use the ISO code as the punch code (setting data

(ISO) = 1).

(ii) All variables are stored with a decimal point. Specify a variable followed by the number of

significant decimal places enclosed in brackets. A variable value is treated as 2-word (32-bit) data,

including the decimal digits. It is output as binary data starting from the highest byte.

(iii) When specified data has been output, an EOB code is output according to the setting code (ISO).

(iv)

<Null> variables are regarded as 0.

- 228 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Example

BPRNT [ C** X#100 [3] Y#101 [3] M#10 [0] ]

Variable value

#100=0.40956

#101=-1638.4

#10=12.34

are output as follows:

C3 A0 A0 D8 00 00 01 9A 59 FF E7 00 00 4D 00 00 00 0C 0A

↓

↓

C sp sp X0000019A YFFE70000 M0000000C

LF

( * * )

(410)

(-1638400)

(12)

( ; )

-

Data output command DPRNT

DPRNT

[ a

#b

[c

d] … ]

Number of significant decimal places

Number of significant digits in the integer part

Variable

Character

The DPRNT command outputs characters and each digit in the value of a variable according to the code

set in the settings (ISO).

(i)

For an explanation of the DPRNT command, see Items (i), (iii), and (iv) for the BPRNT command.

(ii) When outputting a variable, specify # followed by the variable number, then specify the number of

digits in the integer part and the number of decimal places enclosed in brackets.

For the value of a variable, as many codes as the specified number of digits are output according to

the settings one by one, starting with the highest digit. The decimal point is also output using the

set code.

Each variable must be a numeric value consisting of up to nine digits. When high-order digits are

zeros, these zeros are not output if bit 1 (PRT) of parameter No. 6001 is 1. If parameter PRT is 0, a

space code is output each time a zero is encountered.

When the number of decimal places is not zero, digits in the decimal part are always output. If the

number of decimal places is zero, no decimal point is output.

When bit 1 (PRT) of parameter No. 6001 is 0, a space code is output to indicate a positive number

instead of +; if parameter PRT is 1, no code is output.

- 229 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Example

DPRNT [ X#2 [53] Y#5 [53] T#30 [20] ]

Variable value

#2=128.47398

#5=-91.2

#30=123.456

are output as follows:

(1) Parameter PRT (No.6001#1) = 0

D8 A0 A0 A0 B1 B2 B8 2E B4 B7 B4 59 2D A0 A0 A0 39 B1 2E B2 30 30 D4 A0 B2 33 0A

↓

↓

↓

↓

X sp sp sp

128.474

Y- sp sp sp

91.200

T

sp

023 LF

(2) Parameter PRT (No.6001#1) = 1

D8 B1 B2 B8 2E B4 B7 B4 59 2D 39 B1 2E B2 30 30 D4 A0 B2 33 0A

↓

X128.474

Y-91.200

T023 LF

-

Close command PCLOS

The PCLOS command releases a connection to an external input/output device. Specify this command

when all data output commands have terminated. DC4 control code is output from the CNC.

-

Required setting

Specify the specification number of an input/output device to be used for the I/O device specification

number.

According to the above settings, set data items (such as the baud rate) for the reader/puncher interface.

Do not specify the FANUC Cassette or FLOPPY unit as an external output device.

When specifying a DPRNT command to output data, specify whether leading zeros are output as spaces

(by setting bit 1 (PRT) of parameter No. 6001 to 1 or 0).

To indicate the end of a line of data in ISO code, specify whether to use only an LF (bit 4 (CRO) of

parameter 6001 is 0) or an LF and CR bit 4 (CRO) of parameter 6001 is 1).

NOTE

1 It is not necessary to always specify the open command (POPEN), data output

command (BPRNT, DPRNT), and close command (PCLOS) together. Once an

open command is specified at the beginning of a program, it does not need to be

specified again except after a close command was specified.

2 Be sure to specify open commands and close commands in pairs. Specify the

close command at the end of the program. However, do not specify a close

command if no open command has been specified.

3 When a reset operation is performed while commands are being output by a

data output command, output is stopped and subsequent data is erased. If a

reset is caused by M30 or other commands at the end of a program that is

outputting data, wait until all data is output by, for example, specifying the close

command at the end of the program and then execute M30 or other commands.

- 230 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

14.12 RESTRICTIONS

-

Single block

Even while a macro program is being executed, blocks can be stopped in the single block mode.

A block containing a macro call command (G65, G66, Ggg, Mmm, or G67) does not stop even when the

single block mode is on.

Whether blocks containing arithmetic and logic operation commands and control commands are stopped

depends on the settings of bits 5 (SBM) and 7 (SBV) of parameter No. 6000 as shown in the following

table.

Bit 5 (SBM) of parameter No. 6000

0

1

Not stopped when the single block mode

Can be stopped in the single block mode.

0

is on.

(Variable #3003 cannot be used to

Bit 7 (SBV) of

Can be stopped in the single bock mode.

disable single block stop. Single block

parameter No. 6000

1

(Variable #3003 can be used to enable or

stop is always enabled.)

disable single block stop.)

M

Note that when a single block stop occurs at a macro statement in cutter compensation mode, the

statement is assumed to be a block that does not involve movement, and proper compensation cannot be

performed in some cases.

(Strictly speaking, the block is regarded as specifying a movement with a

travel distance 0.)

-

Optional block skip

A / appearing in the middle of an <expression> (enclosed in brackets [

] on the right-hand side of an

arithmetic expression) is regarded as a division operator; it is not regarded as the specifier for an optional

block skip code.

-

Operation in EDIT mode

By setting bit 0 (NE8) of parameter No.3202 and bit 4 (NE9) of parameter No.3202 to 1, deletion and

editing are disabled for custom macro programs and subprograms with program numbers 8000 to 8999

and 9000 to 9999. This prevents registered custom macro programs and subprograms from being

destroyed by accident. When the entire memory is cleared, the contents of memory such as custom

macro programs are deleted.

-

Reset

With a reset operation, local variables and common variables #100 to #199 are cleared to null values.

However, bit 6 (CCV) of parameter No. 6001 can be set to prevent variables #100 to #199 from being

cleared.

A reset operation clears any called states of custom macro programs and subprograms, and any DO states,

and returns control to the main program.

-

Display of the PROGRAM RESTART

As with M98, the M and T codes used for subprogram calls are not displayed.

-

Feed hold

When a feed hold is enabled during execution of a macro statement, the machine stops after execution of

the macro statement. The machine also stops when a reset or alarm occurs.

-

DNC operation

The control commands (such as GOTO and WHILE-DO) cannot be executed during DNC operation.

- 231 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

However, this restriction is removed when a program registered in program memory is called during DNC

operation.

-

Constant values that can be used in <expression>

+0.00000000001 to +999999999999

-999999999999 to -0.00000000001

The number of significant digits is 12 (decimal).

If this range is exceeded, an alarm PS0012 occurs.

14.13 INTERRUPTION TYPE CUSTOM MACRO

When a program is being executed, another program can be called by inputting an interrupt signal (UINT)

from the machine.

This function is referred to as an interruption type custom macro function. Program an interrupt

command in the following format:

Format

M96Pxxxx ; Enables custom macro interrupt

M97 ;

Disables custom macro interrupt

Explanation

Use of the interruption type custom macro function allows the user to call a program during execution of

an arbitrary block of another program. This allows programs to be operated to match situations which

vary from time to time.

(1) When a tool abnormality is detected, processing to handle the abnormality is started by an external

signal.

(2) A sequence of machining operations is interrupted by another machining operation without the

cancellation of the current operation.

(3) At regular intervals, information on current machining is read.

Listed above are examples like adaptive control applications of the interruption type custom macro

function.

M96 Pxxxx;

Interrupt signal

(UINT)

Oxxxx;

Interrupt signal

(UINT) **

M99 (Pyyyy);

Nyyyy;

M97;

Interrupt signal

(UINT) *

Fig 14.13 (a) Interruption type custom macro function

When M96Pxxxx is specified in a program, subsequent program operation can be interrupted by an

interrupt signal (UINT) input to execute the program specified by Pxxxx. When the interrupt signal

- 232 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

((UINT)** and (UINT)* in Fig 14.13 (a)) is input during execution of the interrupt program or after M97,

it is ignored.

14.13.1 Specification Method

Explanation

-

Interrupt conditions

A custom macro interrupt is available only during program execution. It is enabled under the following

conditions

• When memory operation, DNC operation, or MDI operation is selected

• When STL (start lamp) is on

• When a custom macro interrupt is not currently being processed

A custom macro interrupt cannot be performed during manual operation.

-

Specification

Generally, the custom macro interrupt function is used by specifying M96 to enable the interrupt signal

(UINT) and M97 to disable the signal.

Once M96 is specified, a custom macro interrupt can be initiated by the input of the interrupt signal

(UINT) until M97 is specified or the CNC is reset. After M97 is specified or the CNC is reset, no

custom macro interrupts are initiated even when the interrupt signal (UINT) is input. The interrupt

signal (UINT) is ignored until another M96 command is specified.

M96

M97

M96

1

0

Interrupt signal

(UINT)

Effective interrupt

input signal

When UINT is kept on

The interrupt signal (UINT) becomes valid after M96 is specified. Even when the signal is input in M97

mode, it is ignored. When the signal input in M97 mode is kept on until M96 is specified, a custom

macro interrupt is initiated as soon as M96 is specified (only when the status-triggered scheme is

employed); when the edge-triggered scheme is employed, the custom macro interrupt is not initiated even

when M96 is specified.

NOTE

For the status-triggered and edge-triggered schemes, see Item "Custom macro

interrupt signal (UINT)" of II-14.12.2.

- 233 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

CAUTION

For interrupt type I, operation after control is returned differs depending on

whether the interrupt program contains an NC statement.

When the program number block contains EOB (;), it is assumed to contain an

NC statement.

(Program containing an NC statement)

(Program containing no NC statement)

O0013 ;

O0013#101=#5041 ;

#101=#5041 ;

#102=#5042 ;

#102=#5042 ;

#103=#5043 ;

#103=#5043 ;

M99 ;

M99 ;

Type I (when an interrupt is performed even in the middle of a block)

(i)

When the interrupt signal (UINT) is input, any movement or dwell being performed is stopped

immediately and the interrupt program is executed.

(ii)

If there are NC statements in the interrupt program, the command in the interrupted block is lost and

the NC statement in the interrupt program is executed. When control is returned to the interrupted

program, the program is restarted from the next block after the interrupted block.

(iii)

If there are no NC statements in the interrupt program, control is returned to the interrupted program

by M99, then the program is restarted from the command in the interrupted block.

Interrupted by macro interrupt

Execution in progress

Normal program

CNC command restart;

Interrupt signal

when there are no NC statements

(UINT) input

in the interrupt program

Execution in progress

Custom macro interrupt

Fig. 14.13 (b) Custom macro interrupt and NC command (type I)

Type II (when an interrupt is performed at the end of the block)

(i)

If the block being executed is not a block that consists of several cycle operations such as a drilling

canned cycle and automatic reference position return (G28), an interrupt is performed as follows:

When an interrupt signal (UINT) is input, macro statements in the interrupt program are executed

immediately unless an NC statement is encountered in the interrupt program. NC statements are

not executed until the current block is completed.

(ii)

If the block being executed consists of several cycle operations, an interrupt is performed as follows:

When the last movement in the cycle operations is started, macro statements in the interrupt program

are executed unless an NC statement is encountered. NC statements are executed after all cycle

operations are completed.

- 235 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Execution in progress

Normal program

Interrupt signal (UINT) input

Execution in progress

Custom macro interrupt

NC statement in the interrupt

program

Fig. 14.13 (c) Custom macro interrupt and NC command (type II)

M

NOTE

During execution of a program for cycle operations, interrupt type II is performed

regardless of whether bit 2 (MIN) of parameter No. 6003 is set to 0 or 1. Cycle

operations are available for the following functions:

<1> Automatic reference position return

<2> Cutter compensation (generating multiple blocks using the specified block

such as when the tool moves around the outside of an acute angle)

<3> Canned cycle

<4> Automatic tool length measurement

<5> Normal direction control

T

NOTE

During execution of a program for cycle operations, interrupt type II is performed

regardless of whether bit 2 (MIN) of parameter No. 6003 is set to 0 or 1. Cycle

operations are available for the following functions:

<1> Automatic reference position return

<2> Tool nose radius compensation (generating multiple blocks using the

specified block such as when the tool moves around the outside of an acute

angle)

<3> Canned cycle (No interruption type custom macro can be used during

execution of a multiple repetitive canned turning cycle, however.)

<4> Automatic tool compensation

<5> Chamfering/corner R

-

Conditions for enabling and disabling the custom macro interrupt signal

The interrupt signal becomes valid after execution starts of a block that contains M96 for enabling custom

macro interrupts. The signal becomes invalid when execution starts of a block that contains M97.

While an interrupt program is being executed, the interrupt signal becomes invalid. The signal become

valid when the execution of the block that immediately follows the interrupted block in the main program

is started after control returns from the interrupt program. In type I, if the interrupt program consists of

only macro statements, the interrupt signal becomes valid when execution of the interrupted block is

started after control returns from the interrupt program.

- 236 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

-

Custom macro interrupt signal (UINT)

There are two schemes for custom macro interrupt signal (UINT) input: The status-triggered scheme

and edge-triggered scheme. When the status-triggered scheme is used, the signal is valid when it is on.

When the edge triggered scheme is used, the signal becomes valid on the rising edge when it switches

from off to on status.

One of the two schemes is selected with bit 3 (TSE) of parameter No.6003.

When the status-triggered scheme is selected by this parameter, a custom macro interrupt is generated if

the interrupt signal (UINT) is on at the time the signal becomes valid. By keeping the interrupt signal

(UINT) on, the interrupt program can be executed repeatedly.

When the edge-triggered scheme is selected, the interrupt signal (UINT) becomes valid only on its rising

edge. Therefore, the interrupt program is executed only momentarily (in cases when the program

consists of only macro statements). When the status-triggered scheme is inappropriate, or when a

custom macro interrupt is to be performed just once for the entire program (in this case, the interrupt

signal may be kept on), the edge-triggered scheme is useful.

Except for the specific applications mentioned above, use of either scheme results in the same effects.

The time from signal input until a custom macro interrupt is executed does not vary between the two

schemes.

In the example shown in Fig 14.12 (d), an interrupt is executed four times when the status-triggered

scheme is used; when the edge-triggered scheme is used, the interrupt is executed just once.

1

0

Interrupt signal (UINT)

Interrupt

Interrupt

Interrupt

execution execution execution

Interrupt

execution

Status-triggered scheme

Interrupt execution

Edge-triggered scheme

Fig. 14.13 (d) Custom macro interrupt signal

-

Return from a custom macro interrupt

To return control from a custom macro interrupt to the interrupted program, specify M99. A sequence

number in the interrupted program can also be specified using address P. If this is specified, the

program is searched from the beginning for the specified sequence number. Control is returned to the

first sequence number found.

- 237 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

NOTE

If a block containing M99 is alone or has address O, N, P, L, or M only, this block

is programmatically assumed to be the same as the previous block. Therefore,

a single-block stop does not occur for this block. In terms of programming, the

following <1> and <2> are basically the same.

(The difference is whether Gxx

is executed before M99 is recognized.)

<1>

Gxx Xxxx ;

M99 ;

<2>

Gxx Xxxx M99 ;

-

Custom macro interrupt and modal information

A custom macro interrupt is different from a normal program call. It is initiated by an interrupt signal

(UINT) during program execution. In general, any modifications of modal information made by the

interrupt program should not affect the interrupted program.

For this reason, even when modal information is modified by the interrupt program, the modal

information before the interrupt is restored when control is returned to the interrupted program by M99.

When control is returned from the interrupt program to the interrupted program by M99 Pyyyy, however,

modal information can again be controlled by the program. In this case, the new continuous information

modified by the interrupt program is passed to the interrupted program.

In this case, take the following action as required:

<1> The interrupt program provides modal information to be used after control is returned to the

interrupted program.

<2> After control is returned to the interrupted program, modal information is specified again as

necessary.

{ ΔΔΔΔ

M96 Pxxxx;

{ xxxx;

Interrupt signal (UINT)

Modify modal information

(Without P specification)

Modal information remains

unchanged before and after

M99 (Pyyyy);

the interrupt.

(With P specification)

Nyyyy;

The new modal information modified by the interrupt program is present.

Fig. 14.13 (e) Custom macro interrupt and modal information

Modal information when control is returned by M99

The modal information present before the interrupt becomes valid. The new modal information

modified by the interrupt program is made invalid.

- 238 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Modal information when control is returned by M99 Pyyyy

The new modal information modified by the interrupt program remains valid even after control is

returned.

Modal information which was valid in the interrupted block

The old modal information which was valid in the interrupted block can be read using custom macro

system variables #4401 to #4530.

M

System variable

Modal information which was valid when a custom macro interrupt was generated

#4401

G code (group 01)

:

:

#4430

G code (group 30)

#4502

B code

#4507

D code

#4508

E code

#4509

F code

#4511

H code

#4513

M code

#4514

Sequence number

#4515

Program number

#4519

S code

#4520

T code

#4530

Additional workpiece coordinate system number

T

System variable

Modal information which was valid when a custom macro interrupt was generated

#4401

G code (group 01)

:

:

#4430

G code (group 30)

#4508

E code

#4509

F code

#4513

M code

#4514

Sequence number

#4515

Program number

#4519

S code

#4520

T code

-

System variables (position information values) for the interrupt program

Position information can be read as follows.

Macro variable

Condition

Position information value

#5001 or above

Until the first NC statement appears

Coordinates of point A

After an NC statement with no move command appears

Coordinates of point A'

After an NC statement with a move command appears

Coordinates of the end point of the

move command

#5021 or above

Machine coordinates of point B'

#5041 or above

Workpiece coordinates of point B'

- 239 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Tool center path

Interrupt generated

B

B

A

A’

Offset vector

Programmed tool path

-

Custom macro interrupt and custom macro modal call

When the interrupt signal (UINT) is input and an interrupt program is called, the custom macro modal

call is canceled (G67). However, when G66 is specified in the interrupt program, the custom macro

modal call becomes valid. When control is returned from the interrupt program by M99, the modal call

is restored to the state it was in before the interrupt was generated. When control is returned by M99

Pyyyy ;, the modal call in the interrupt program remains valid.

-

Custom macro interrupt and program restart

In program restart, when the interrupt signal (UINT) is input during dry run recovery after a search, the

interrupt program is called after restart of all axes is completed.

That is, interrupt type II is assumed regardless of the parameter setting.

M

NOTE

1 Alarm PS1101 occurs in the following cases:

<1>An interrupt is generated in the programmable mirror image (G51.1) mode

and another G51.1 is specified in the interrupt program.

<2>An interrupt is generated in the coordinate system rotation (G68) mode and

another G68 is specified in the interrupt program.

<3>An interrupt is generated in the scaling (G51) mode and another G51 is

specified in the interrupt program.

2 In program restart, do not input the interrupt signal (UINT) during dry run

recovery after a search.

T

NOTE

1 No interruption type custom macro can be used during execution of a multiple

repetitive canned turning cycle.

2 In program restart, do not input the interrupt signal (UINT) during dry run

recovery after a search.

- 240 -

15.PROGRAMMABLE

B-64304EN/02

PROGRAMMING

PARAMETER INPUT (G10)

15 PROGRAMMABLE PARAMETER INPUT

(G10)

Overview

The values of parameters and pitch error compensation data can be entered in a program. This function is

used for setting pitch error compensation data when attachments are changed or the maximum cutting

feedrate or cutting time constants are changed to meet changing machining conditions.

Format

-

Parameter entry mode

G10 L52 ;

Parameter entry mode setting

N_ (Q_) R_ ;

For parameters other than the axis type or spindle type

N_ P_ (Q_) R_ ;

For axis type or spindle type parameters

:

G11 ;

Parameter entry mode cancel

N_

: Parameter number

R_

: Parameter setting value (Leading zeros can be omitted.)

(Q_) : Bit number 0 to 7 (to be set when a bit type parameter is input)

(Enabled when bit 4 (G1B) of parameter No.3454 = 1.)

P_

: Axis number 1 to maximum controlled axis number (to be specified when an axis

type parameter or spindle type parameter is specified)

NOTE

G10L52 cannot be used to enter pitch error compensation data.

-

Pitch error compensation data entry mode

G10 L50 ; Pitch error compensation data entry mode setting

N_ R_ ; Pitch error compensation data entry

:

:

G11 ;

Pitch error compensation data entry mode cancel

N_ : Compensation position number for pitch errors compensation +10,000

R_ : Pitch error compensation data

NOTE

G10L50 cannot be used to enter parameter.

Explanation

-

Setting value (R_)

Do not use a decimal point in the setting (R_) of a parameter or pitch error compensation data.

To change a bit type parameter if bit 4 (G1B) of parameter No. 3454 is 1, specify 0 or 1. If a value other

than 0 and 1 is specified, alarm PS1144, "G10 FORMAT ERROR", is issued.

As the value of R, a custom macro variable can be used.

When a parameter of real type is used, set an integer value in (R_) according to the increment system of

the parameter.

- 241 -

15. PROGRAMMABLE

PARAMETER INPUT (G10)

PROGRAMMING

B-64304EN/02

-

Bit number (Q＿)

Bit number (Q_) is effective if bit 4 (G1B) of parameter No. 3454 is 1. To set a bit type parameter, set a

number in the range of 0 to 7.

A custom macro variable can be used as the value of Q.

-

Axis number (P_)

As the axis number (P_), specify the order of a controlled axis to be displayed on the CNC display screen,

by using an axis type parameter.

For example, specify P2 for the control axis which is displayed second.

For a spindle type also, specify the order of an axis to be display on the CNC display screen.

A custom macro variable can be used as the value of P.

WARNING

1 Do not fail to perform reference position return manually after changing the pitch

error compensation data or backlash compensation data. Without this, the

machine position can deviate from the correct position.

2 The canned cycle mode must be cancelled before entering of parameters. When

not cancelled, the drilling motion may be activated.

CAUTION

Compatibility with the Series 0i-C:

This model has parameters that are not compatible with the Series 0i-C.

So, before using this function, make a check according to the Parameter Manual

(B-64310EN) of this model.

NOTE

Other NC statements cannot be specified while in parameter input mode.

Example

1.

Set bit 2 (SBP) of bit type parameter No. 3404 (when the bit 4 (G1B) of parameter No. 3454 is set to

0)

G10 L52 ;

Parameter entry mode

N3404 R00000100 ;

SBP setting

G11 ;

Cancel parameter entry mode

2.

Set bit 2 (SBP) of bit type parameter No. 3404 (when the bit 4 (G1B) of parameter No. 3454 is set to

1)

G10 L52 ;

Parameter entry mode

N3404 Q2 R1 ;

SBP setting

G11 ;

Cancel parameter entry mode

3.

Change the values for the Z-axis (3rd axis) and A-axis (4th axis) in axis type parameter No. 1322

(the coordinates of stored stroke limit 2 in the positive direction for each axis).

(When the increment systems for the

3rd and

4th axes are IS-B and millimeter machine,

respectively)

G10 L52 ;

Parameter entry mode

N1322 P3 R4500 ;

Change the value for the Z-axis to 4.500

N1322 P4 R12000 ; Change the value for the A-axis to 12.000

G11 ;

Cancel parameter entry mode

- 242 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

16 HIGH-SPEED CUTTING FUNCTIONS

Chapter 16, "HIGH-SPEED CUTTING FUNCTIONS", consists of the following sections:

16.1 ADVANCED PREVIEW CONTROL (T SERIES) / AI ADVANCED PREVIEW CONTROL

(M SERIES) / AI CONTOUR CONTROL (II) (M SERIES)

244

16.2 MACHINING CONDITION SELECTING FUNCTION

261

16.3 MACHINING QUALITY LEVEL ADJUSTMENT (M Series)

262

16.4 JERK CONTROL (M Series)

263

16.1 ADVANCED PREVIEW CONTROL (T SERIES) / AI

ADVANCED PREVIEW CONTROL (M SERIES) / AI

CONTOUR CONTROL (II) (M SERIES)

Overview

Advanced preview control (T series), AI advanced preview control (M series), and AI contour control (II)

(M series) are intended for high-speed, high-precision machining. The use of these functions suppresses

the acceleration/deceleration delay that tends to increase as the feedrate becomes faster, as well as the

delay in the servo system, reducing the machining profile error.

The following table shows the functions included in these functions.

APC

AI APC

AICC

AICC II

Model

0i-TD

0i Mate-MD

0i-MD

0i-MD

0i-MD

Basic/Option

Option

Basic

Option

Option

Look-ahead block count

1

12

20

40

200

Look-ahead linear acceleration/

○

○

○

○

deceleration before interpolation

Look-ahead bell-shaped acceleration/

－

－

☆

☆

deceleration before interpolation

Function for changing time constant of

－

－

☆

☆

bell-shaped acceleration/deceleration

Advanced feed forward

○

○

○

○

Acceleration setting for each axis

○

○

○

○

Speed control based on the feedrate

○

○

○

○

difference on each axis

Speed control with

○

○

○

○

acceleration in circular interpolation

Speed control with

－

○

○

○

the acceleration on each axis

Smooth speed control

－

－

－

○

Speed control with cutting load

－

－

－

○

Disregard of feedrate command

－

－

－

○

Jerk control

- Speed control with change of

acceleration on each Axis

－

－

－

☆

- Look-ahead smooth bell-shaped

acceleration/deceleration before Interpolation

Nano smoothing

－

－

－

☆

APC

: Advanced preview control

- 244 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

AI APC

: AI advanced preview control

AICC

: AI contour control

AICC II

: AI contour control II

-: Function not supported

○: Standard function

☆: Optional function

M

The function for changing time constant of bell-shaped acceleration/deceleration is included in

look-ahead bell-shaped acceleration/deceleration before interpolation.

The look-ahead bell-shaped acceleration/deceleration before interpolation is optional function.

Format

T

-

Advanced preview control

G08 P_ ;

P1 : Advanced preview control mode on

P0 : Advanced preview control mode off

NOTE

1 Always specify G08 in an independent block.

2 The advanced preview control mode is also cleared by the reset operation.

M

・AI advanced preview control/AI contour control (II)

G05.1 Q_ ;

Q1 : AI advanced preview control mode/AI contour control (II) mode on

Q0 : AI advanced preview control mode/AI contour control (II) mode off

NOTE

1 Always specify G05.1 in an independent block.

2 The AI advanced preview control/AI contour control (II) mode is also cleared by

the reset operation.

Explanation

-

Look-ahead acceleration/deceleration before interpolation

T

Acceleration/deceleration type of look-ahead acceleration/ deceleration before interpolation function is

look-ahead linear acceleration/deceleration before interpolation function.

M

There are two look-ahead acceleration/deceleration before interpolation functions - look-ahead linear

acceleration/deceleration before interpolation and look-ahead bell-shaped acceleration/ deceleration

before interpolation. Look-ahead bell-shaped acceleration/deceleration before interpolation offers more

smooth acceleration and deceleration.

- 245 -

Content      ..     7      8      9      10     ..