Content      ..     10      11      12      13     ..

FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL - page 12

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

In a program, the flow of control can be changed using the GOTO

15.5

statement and IF statement. Three types of branch and repetition

BRANCH AND

operations are used:

REPETITION

Branch and repetition

GOTO statement (unconditional branch)

IF statement (conditional branch: if ..., then...)

WHILE statement (repetition while ...)

A branch to sequence number n occurs. When a sequence number outside

15.5.1

of the range 1 to 99999 is specified, P/S alarm No. 128 occurs. A sequence

Unconditional Branch

number can also be specified using an expression.

(GOTO Statement)

GOTO n ; n: Sequence number (1 to 99999)

Example:

GOTO1;

GOTO#10;

311

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

15.5.2

Specify a conditional expression after IF. IF [<conditional expression>]

GOTO n If the specified conditional expression is satisfied, a branch to

Conditional Branch

sequence number n occurs. If the specified condition is not satisfied, the

(IF Statement)

next block is executed.

If the value of variable #1 is greater than 10, a branch to sequence number

N2 occurs.

If the condition

IF [#1 GT 10] GOTO 2 ;

is not satisfied

Processing

If the condition is satisfied

N2 G00 G91 X10.0 ;

:

IF[<conditional

If the specified conditional expression is satisfied, a predetermined macro

expression>]THEN

statement is executed. Only a single macro statement is executed.

If the values of #1 and #2 are the same, 0 is assigned to #3.

IF [#1 EQ #2] THEN #3=0;

Explanations

A conditional expression must include an operator inserted between two

D Conditional expression

variables or between a variable and constant, and must be enclosed in

brackets ([, ]). An expression can be used instead of a variable.

D Operators

Operators each consist of two letters and are used to compare two values

to determine whether they are equal or one value is smaller or greater than

the other value. Note that the inequality sign cannot be used.

Table 15.5.2 Operators

Operator

Meaning

EQ

Equal to(=)

NE

Not equal to(0)

GT

Greater than(>)

GE

Greater than or equal to(y)

LT

Less than(<)

LE

Less than or equal to(x)

Sample program

The sample program below finds the total of numbers 1 to 10.

O9500;

#1=0;Initial value of the variable to hold the sum

#2=1;Initial value of the variable as an addend

N1 IF[#2 GT 10] GOTO 2; . Branch to N2 when the addend is greater than

10

#1=#1+#2; Calculation to find the sum

#2=#2+1; Next addend

GOTO 1; Branch to N1

N2 M30;End of program

312

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

15.5.3

Specify a conditional expression after WHILE. While the specified

condition is satisfied, the program from DO to END is executed. If the

Repetition

specified condition is not satisfied, program execution proceeds to the

(While Statement)

block after END.

WHILE [conditional expression] DO m ; (m=1,2,3)

If the condition

If the condition

Processing

is not satisfied

is satisfied

END m ;

:

Explanations

While the specified condition is satisfied, the program from DO to END

after WHILE is executed. If the specified condition is not satisfied,

program execution proceeds to the block after END. The same format as

for the IF statement applies. A number after DO and a number after END

are identification numbers for specifying the range of execution. The

numbers 1, 2, and 3 can be used. When a number other than 1, 2, and 3

is used, P/S alarm No. 126 occurs.

313

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

D Nesting

The identification numbers (1 to 3) in a DO-END loop can be used as

many times as desired. Note, however, when a program includes crossing

repetition loops (overlapped DO ranges), P/S alarm No. 124 occurs.

3. DO loops can be nested to a

1. The identification numbers

maximum depth of three levels.

(1 to 3) can be used as many

times as required.

WHILE [ … ] DO 1 ;

WHILE [ … ] DO 1 ;

:

WHILE [ … ] DO 2 ;

Processing

:

WHILE [ … ] DO 3 ;

END 1 ;

:

Processing

WHILE [ … ] DO 1 ;

END 3 ;

Processing

:

END 2 ;

END 1 ;

:

END 1 ;

2. DO ranges cannot overlap.

4. Control can be transferred to the

WHILE [ … ] DO 1 ;

outside of a loop.

Processing

WHILE [ … ] DO 1 ;

WHILE [ … ] DO 2 ;

IF [ … ] GOTO n ;

:

END 1 ;

END 1 ;

Processing

Nn

END 2 ;

5. Branches cannot be made to a

location within a loop.

IF [ … ] GOTO n ;

:

WHILE [ … ] DO 1 ;

Nn … ;

END 1 ;

Limitations

D Infinite loops

When DO m is specified without specifying the WHILE statement, an

infinite loop ranging from DO to END is produced.

D Processing time

When a branch to the sequence number specified in a GOTO statement

occurs, the sequence number is searched for. For this reason, processing

in the reverse direction takes a longer time than processing in the forward

direction. Using the WHILE statement for repetition reduces processing

time.

D Undefined variable

In a conditional expression that uses EQ or NE, a null value and zero have

different effects. In other types of conditional expressions, a null value

is regarded as zero.

314

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

A macro program can be called using the following methods:

15.6

MACRO CALL

Macro call

Simple call ((G65)

modal call (G66, G67)

Macro call with G code

Macro call with M code

Subprogram call with M code

Subprogram call with T code

Restrictions

D Differences between

Macro call (G65) differs from subprogram call (M98) as described below.

macro calls and

D With G65, an argument (data passed to a macro) can be specified. M98

subprogram calls

does not have this capability.

D When an M98 block contains another NC command (for example,

G01 X100.0 M98Pp), the subprogram is called after the command is

executed. On the other hand, G65 unconditionally calls a macro.

D When an M98 block contains another NC command (for example,

G01 X100.0 M98Pp), the machine stops in the single block mode. On

the other hand, G65 does not stops the machine.

D With G65, the level of local variables changes. With M98, the level

of local variables does not change.

316

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

15.6.1

When G65 is specified, the custom macro specified at address P is called.

Data (argument) can be passed to the custom macro program.

Simple Call (G65)

G65 P_ L_ <argument-specification> ;

P_: Number of the program to call

L_

: Repetition count (1 by default)

Argument : Data passed to the macro

O0001 ;

O9010 ;

:

#3=#1+#2 ;

G65 P9010 L2 A1.0 B2.0 ;

IF [#3 GT 360] GOTO 9 ;

:

G00 X#3 ;

M30 ;

N9 M99 ;

Explanations

D Call

D After G65, specify at address P the program number of the custom

macro to call.

D When a number of repetitions is required, specify a number from 1 to

9999 after address L. When L is omitted, 1 is assumed.

D By using argument specification, values are assigned to corresponding

local variables.

D Argument specification

Two types of argument specification are available. Argument

specification I uses letters other than G, L, O, N, and P once each.

Argument specification II uses A, B, and C once each and also uses I, J,

and K up to ten times. The type of argument specification is determined

automatically according to the letters used.

Argument specification I

Address

Variable

Address

Variable

Address

Variable

number

number

number

A

#1

I

#4

T

#20

B

#2

J

#5

U

#21

C

#3

K

#6

V

#22

D

#7

M

#13

W

#23

E

#8

Q

#17

X

#24

F

#9

R

#18

Y

#25

H

#11

S

#19

Z

#26

D Addresses G, L, N, O, and P cannot be used in arguments.

D Addresses that need not be specified can be omitted. Local variables

corresponding to an omitted address are set to null.

D Addresses do not need to be specified alphabetically. They conform

to word address format.

I, J, and K need to be specified alphabetically, however.

Example

B_A_D_ … J_K_ Correct

B_A_D_ … J_I_ Incorrect

317

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

Argument specification II

Argument specification II uses A, B, and C once each and uses I, J, and

K up to ten times. Argument specification II is used to pass values such

as three-dimensional coordinates as arguments.

Variable

Variable

Variable

Address

Address

Address

number

number

number

A

#1

K₃

#12

J₇

#23

B

#2

I₄

#13

K₇

#24

C

#3

J₄

#14

I₈

#25

I₁

#4

K₄

#15

J₈

#26

J₁

#5

I₅

#16

K₈

#27

K₁

#6

J₅

#17

I₉

#28

I₂

#7

K₅

#18

J₉

#29

J₂

#8

I₆

#19

K₉

#30

K₂

#9

J₆

#20

I₁₀

#31

I₃

#10

K₆

#21

J₁₀

#32

J₃

#11

I₇

#22

K₁₀

#33

D Subscripts of I, J, and K for indicating the order of argument

specification are not written in the actual program.

Restrictions

D Format

G65 must be specified before any argument.

D Mixture of argument

The CNC internally identifies argument specification I and argument

specifications I and II

specification II. If a mixture of argument specification I and argument

specification II is specified, the type of argument specification specified

later takes precedence.

Example

G65

A1.0 B2.0

I-3.0

I4.0

D5.0

P1000;

<Variables>

#1:1.0

#2:2.0

#3:

#4:-3.0

#5:

#6:

#7:

5.0

When both the I4.0 and D5.0 arguments are commanded for

variable #7 in this example, the latter, D5.0, is valid.

D Position of the decimal

The units used for argument data passed without a decimal point

point

correspond to the least input increment of each address. The value of an

argument passed without a decimal point may vary according to the

system configuration of the machine. It is good practice to use decimal

points in macro call arguments to maintain program compatibility.

D Call nesting

Calls can be nested to a depth of four levels including simple calls (G65)

and modal calls (G66). This does not include subprogram calls (M98).

318

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

D Local variable levels

D Local variables from level 0 to 4 are provided for nesting.

D The level of the main program is 0.

D Each time a macro is called (with G65 or G66), the local variable level

is incremented by one. The values of the local variables at the previous

level are saved in the CNC.

D When M99 is executed in a macro program, control returns to the

calling program. At that time, the local variable level is decremented

by one; the values of the local variables saved when the macro was

called are restored.

Main program

Macro

(level 0)

Macro (level 1) Macro (level 2) Macro (level 3)

(level 4)

O0001 ;

O0002 ;

O0003 ;

O0004 ;

O0005 ;

:

:

:

:

:

#1=1 ;

:

:

:

:

G65 P2 A2 ;

G65 P3 A3 ;

G65 P4 A4 ;

G65 P5 A5 ;

:

:

:

:

:

:

:

:

:

:

:

M30 ;

M99 ;

M99 ;

M99 ;

M99 ;

Local variables

(level 0)

(Level 1)

(Level 2)

(Level 3)

(Level 4)

#1

1

#1

2

#1

3

#1

4

#1

5

:

:

:

:

:

:

:

:

:

:

#33

#33

#33

#33

#33

Common variables

#100-, #500-

Variables that can be read from and written to by

macros at different levels

Sample program

Move the tool beforehand along the X- and Z-axes to the position where

(Drill cycle)

a drilling cycle starts. Specify Z or W for the depth of a hole, K for the

depth of a cut, and F for the cutting feedrate to drill the hole.

Z

W

K

Cutting

Rapid traverse

319

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

15.6.2

Once G66 is issued to specify a modal call a macro is called after a block

specifying movement along axes is executed. This continues until G67

Modal Call (G66)

is issued to cancel a modal call.

G66 P p L ȏ <argument-specification> ;

P : Number of the program to call

ȏ : Repetition count (1 by default)

Argument : Data passed to the macro

O0001 ;

O9100 ;

:

:

G66 P9100 L2 A1.0 B2.0 ;

G00 Z-#1 ;

G00 G90 X100.0 ;

G01 Z-#2 F0.3 ;

X125.0 ;

:

X150.0 ;

:

G67 ;

:

:

:

M30 ;

M99 ;

Explanations

D Call

D After G66, specify at address P a program number subject to a modal

call.

D When a number of repetitions is required, a number from 1 to 9999 can

be specified at address L.

D As with a simple call (G65), data passed to a macro program is

specified in arguments.

D Cancellation

When a G67 code is specified, modal macro calls are no longer performed

in subsequent blocks.

D Call nesting

Calls can be nested to a depth of four levels including simple calls (G65)

and modal calls (G66). This does not include subprogram calls (M98).

D Modal call nesting

Modal calls can be nested by specifying another G66 code during a modal

call.

Restrictions

D In a G66 block, no macros can be called.

D G66 needs to be specified before any arguments.

D No macros can be called in a block which contains a code such as a

miscellaneous function that does not involve movement along an axis.

D Local variables (arguments) can only be set in G66 blocks. Note that

local variables are not set each time a modal call is performed.

321

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

Sample program

This program makes a groove at a specified position.

U

D Calling format

G66 P9110 Uu Ff ;

U: Groove depth (incremental specification)

F : Cutting feed of grooving

D Program that calls a

O0003 ;

macro program

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 ;

M30;

D Macro program

O9110 ;

(program called)

G01 U-#21 F#9 ;

Cuts the workpiece.

G00 U#21 ;

Retracts the tool.

M99 ;

322

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

15.6.3

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

Macro Call Using

(G65).

G Code

O0001 ;

O9010 ;

:

:

G81 X10.0 Z-10.0 ;

:

:

:

M30 ;

N9 M99 ;

Parameter No. 6050 = 81

Explanations

By setting a G code number from 1 to 9999 used to call a custom macro

program (9010 to 9019) in the corresponding parameter (Nos. 6050 to

6059), the macro program can be called in the same way as with G65.

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.

D Correspondence

between parameter

Program number

Parameter number

numbers and program

O9010

6050

numbers

O9011

6051

O9012

6052

O9013

6053

O9014

6054

O9015

6055

O9016

6056

O9017

6057

O9018

6058

O9019

6059

D Repetition

As with a simple call, a number of repetitions from 1 to 9999 can be

specified at address L.

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

D Argument specification

Argument specification I and argument specification II. The type of

argument specification is determined automatically according to the

addresses used.

Restrictions

D Nesting of calls using G

In a program called with a G code, no macros can be called using a G code.

codes

A G code in such a program is treated as an ordinary G code. In a program

called as a subprogram with an M or T code, no macros can be called using

a G code. A G code in such a program is also treated as an ordinary G code.

323

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

15.6.4

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

Macro Call Using

(G65).

an M Code

O0001 ;

O9020 ;

:

:

M50 A1.0 B2.0 ;

:

:

:

M30 ;

M99 ;

Parameter 6080 = 50

Explanations

By setting an M code number from 1 to 99999999 used to call a 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.

D Correspondence

between parameter

Program number

Parameter number

numbers and program

O9020

6080

numbers

O9021

6081

O9022

6082

O9023

6083

O9024

6084

O9025

6085

O9026

6086

O9027

6087

O9028

6088

O9029

6089

D Repetition

As with a simple call, a number of repetitions from 1 to 9999 can be

specified at address L.

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

D Argument specification

Argument specification I and argument specification II. The type of

argument specification is determined automatically according to the

addresses used.

Restrictions

- An M code used to call a macro program must be specified at the start

of a block.

- In a macro called with a G code or in a program called as a subprogram

with an M or T code, no macros can be called using an M code. An

M code in such a macro or program is treated as an ordinary M code.

324

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

15.6.5

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

Subprogram Call

a subprogram call (M98).

Using an M Code

O0001 ;

O9001 ;

:

:

M03 ;

:

:

:

M30 ;

M99 ;

Parameter 6071 = 03

Explanations

By setting an M code number from 1 to 99999999 used to call a

subprogram in a parameter (Nos. 6071 to 6076), the corresponding

custom macro program (O9001 to O9006) can be called in the same way

as with M98.

D Correspondence

between parameter

Program number

Parameter number

numbers and program

O9001

6071

numbers

O9002

6072

O9003

6073

O9004

6074

O9005

6075

O9006

6076

O9007

6077

O9008

6078

O9009

6079

D Repetition

As with a simple call, a number of repetitions from 1 to 9999 can be

specified at address L.

D Argument specification

Argument specification is not allowed.

D M code

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

ordinary M code.

Limitations

In a macro called with a G code or in a program called with an M or T code,

no subprograms can be called using an M code. An M code in such a

macro or program is treated as an ordinary M code.

325

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

15.6.6

By enabling subprograms (macro program) to be called with a T code in

a parameter, a macro program can be called each time the T code is

Subprogram Calls

specified in the machining program.

Using a T Code

O0001 ;

O9000 ;

:

:

T0203 ;

:

:

:

M30 ;

M99 ;

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

Explanations

D Call

By setting bit 5 (TCS) of parameter No. 6001 to 1, the macro program

O9000 can be called when a T code is specified in the machining program.

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

variable #149.

Limitations

In a macro called with a G code or in a program called with an M or T code,

no subprograms can be called using a T code. A T code in such a macro

or program is treated as an ordinary T code.

326

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

15.6.7

By using the subprogram call function that uses M codes, the cumulative

usage time of each tool is measured.

Sample Program

Conditions

D The cumulative usage time of each of tool numbers 1 to 5 is measured.

The time is not measured for tools whose number is 6 or more.

D 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

D 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

D Parameter setting

Set 3 in parameter No. 6071, and set 05 in parameter No. 6072.

D Variable value setting

Set 0 in variables #501 to #505.

D Program that calls a

O0001;

macro program

T0100 M06;

M03;

:

M05;

Changes #501.

T0200 M06;

M03;

:

M05;

Changes #502.

T0300 M06;

M03;

:

M05;

Changes #503.

T0400 M06;

M03;

:

M05;

Changes #504.

T0500 M06;

M03;

:

M05;

Changes #505.

M30;

327

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

For smooth machining, the CNC prereads the CNC statement to be

15.7

performed next. This operation is referred to as buffering. In tool nose

PROCESSING

radius compensation mode (G41, G42), the NC prereads NC statements

MACRO

two or three blocks ahead to find intersections. Macro statements for

STATEMENTS

arithmetic expressions and conditional branches are processed as soon as

they are read into the buffer. Blocks containing M00, M01, M02, or M30,

blocks containing M codes for which buffering is suppressed by setting

parameter(Nos. 3411 to 3420), and blocks containing G31 are not

preread.

Explanations

D When the next block is

not buffered

> N1 G31 X100.0 ;

N1

(M codes that are not

NC statement

N2 #100=1

buffered, G31, etc.)

execution

:

N2

Macro statement execution

> :Block being executed

Buffer

D Buffering the next block

in other than tool nose

> N1 X100.0 ;

N1

N4

radius compensation

NC statement

N2 #1=100 ;

execution

mode (G41, G42)

N3 #2=200 ;

(normally prereading one

N4 Z100.0 ;

N2

N3

block)

:

Macro statement

execution

N4

Buffer

> : Block being executed

V : 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.

329

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

D Buffering the next block

in tool nose radius

> N1 G01 G41 G91 Z100.0 F100 T0101 ;

compensation mode

N2 #1=100 ;

(G41, G42)

> : Block being executed

N3 X100.0 ;

V : Blocks read into the buffer

N4 #2=200 ;

N5 Z50.0 ;

:

N1

N3

NC statement

execution

N2

N4

Macro statement

execution

N3

N5

Buffer

When N1 is being executed, the NC statements in the next two blocks (up

to N5) are read into the buffer. The macro statements (N2, N4) between

N1 and N5 are processed during execution of N1.

D When the next block

involves no movement in

> N1 G01 G41 X100.0 G100 T0101 ;

tool nose radius

N2 #1=100 ;

compensation C (G41,

> : Block being executed

N3 Z50.0 ;

G42) mode

V : Blocks read into the buffer

N4 #2=200 ;

N5 M08 ;

N6 #3=300 ;

N7 X200.0 ;

:

N1

N3

NC statement

execution

N2

N4

N6

Macro statement

execution

N3

N5

N7

Buffer

When the NC1 block is being executed, the NC statements in the next two

blocks (up to N5) are read into the buffer. Since N5 is a block that involves

no movement, an intersection cannot be calculated. In this case, the NC

statements in the next three blocks (up to N7) are read. The macro

statements (N2, N4, and N6) between N1 and N7 are processed during

execution of N1.

330

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

Example )

BPRINT [ C** X#100 [3] Z#101 [3] M#10 [0] ]

Variable value

#100=0.40596

#101=-1638.4

#10=12.34

LF

12 (0000000C)

M

-1638400(FFE70000)

Z

406(00000196)

X

Space

C

D 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.

One code is output for each of the specified number of digits, starting

with the highest digit. For each digit, a code is output according to

the settings (ISO). The decimal point is also output using a code set

in the settings (ISO).

Each variable must be a numeric value consisting of up to eight digits.

When high-order digits are zeros, these zeros are not output if PRT

(bit1 of parameter 6001) is 1. If PRT (bit 1 of parameter 6001) 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 PRT (bit 1 of parameter 6001) is 0, a

space code is output to indicate a positive number instead of +; if

PRT(bit 1 of parameter 6001) is 1, no code is output.

334

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

Example )

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

Variable value

#2=128.47398

#5=-91.2

#30=123.456

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

sp

L F

T

sp

23

Z -

sp

sp sp

91.200

X

sp sp sp

128.474

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

LF

T23

Z-91.200

X128.474

D Close command PCLOS

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.

D Required setting

Specify the channel use for parameter 020. According to the specification

of this parameter, set data items

(such as the baud rate) for the

reader/punch interface.

I/O channel 0 : Parameters 101, 102 and 103

I/O channel 1 : Parameters 111, 112 and 113

I/O channel 2 : Parameters 121, 122 and 123

Never specify output to the Fanuc Cassette or floppy disks.)

When specifying a DPRNT command to output data, specify whether

leading zeros are output as spaces (by setting PRT (bit 1 of parameter

6001) to 1 or 0). To indicate the end of a line of data in ISO code, specify

whether to use only an LF (NCR, of bit 3 of parameter 0103 is 0) or an

LF and CR (NCR is 1).

335

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

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. Therefore, when a reset

operation is performed by a code such as M30 at the end

of a program that performs data output, specify a close

command at the end of the program so that processing such

as M30 is not performed until all data is output.

4

Abbreviated macro words enclosed in brackets [ ] remains

unchanged. However, note that when the characters in

brackets are divided and input several times, the second

and subsequent abbreviations are converted and input.

5

O can be specified in brackets [ ]. Note that when the

characters in brackets [ ] are divided and input several

times, O is omitted in the second and subsequent inputs.

336

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

When a program is being executed, another program can be called by

15.11

inputting an interrupt signal (UINT) from the machine. This function is

INTERRUPTION TYPE

referred to as an interruption type custom macro function. Program an

CUSTOM MACRO

interrupt command in the following format:

Format

M96 Pffff ; Enables custom macro interrupt

M97 ;

Disables custom macro interrupt

Explanations

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

O xxxx;

(UINT)

Interrupt

signal

(UINT)*

M99 (Pffff);

Nffff;

M97 ;

Interrupt

signal

(UINT)*

Fig. 15.11 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.

337

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

CAUTION

When the interrupt signal (UINT, marked by * in Fig. 15.11)

is input after M97 is specified, it is ignored. And the interrupt

signal must not be input during execution of the interrupt

program.

15.11.1

Specification Method

Explanations

D Interrupt conditions

A custom macro interrupt is available only during program execution. It

is enabled under the following conditions

- When memory operation or MDI operation is selected

- When STL (start lamp) is on

- When a custom macro interrupt is not currently being processed

D 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 NC is

reset. After M97 is specified or the NC 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.

338

Content      ..     10      11      12      13     ..