Content      ..     13      14      15      16     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 15

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

Table 15.2 (h) System variable (#3004) for automatic operation control

#3004

Feed hold

Feedrate Override

Exact stop

0

Enabled

Enabled

Enabled

1

Disabled

Enabled

Enabled

2

Enabled

Disabled

Enabled

3

Disabled

Disabled

Enabled

4

Enabled

Enabled

Disabled

5

Disabled

Enabled

Disabled

6

Enabled

Disabled

Disabled

7

Disabled

Disabled

Disabled

S

When the power is turned on, the value of this variable is 0.

S

When feed hold is disabled:

(1) When the feed hold button is held down, the machine stops in the

single block stop mode. However, single block stop operation is not

performed when the single block mode is disabled with variable

#3003.

(2) When the feed hold button is pressed then released, the feed hold lamp

comes on, but the machine does not stop; program execution continues

and the machine stops at the first block where feed hold is enabled.

S

When feedrate override is disabled, an override of 100% is always

applied regardless of the setting of the feedrate override switch on the

machine operator’s panel.

S

When exact stop check is disabled, no exact stop check (position

check) is made even in blocks including those which do not perform

cutting.

O0001 ;

N1 G00 G91 X#24 Y#25 ;

N2 Z#18 ;

G04 ;

N3 #3003=3 ;

N1

N8, N9,

N4 #3004=7 ;

N10

N5 G01 Z#26 F#9 ;

N2

N6 M04 ;

N7 G01

Z-[ROUND[#18]+ROUND[#26]] ;

N3, N4

G04 ;

N7

N8 #3004=0 ;

N5

N9 #3003=0 ;

N10M03 ;

M99 ;

N6

Fig. 15.2 (a) Example of using variable #3004 in a tapping cycle

400

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

D Settings

Settings can be read and written. Binary values are converted to

decimals.

#3005

#15

#14

#13

#12

#11

#10

#9

#8

Setting

FCV

#7

#6

#5

#4

#3

#2

#1

#0

Setting

SEQ

INI

ISO

TVC

#9 (FCV)

: Whether to use the FS15 tape format conversion capability

#5 (SEQ) : Whether to automatically insert sequence numbers

#2 (INI)

: Millimeter input or inch input

#1 (ISO)

: Whether to use EIA or ISO as the output code

#0 (TVC)

: Whether to make a TV check

D Mirror image

The mirror-image status for each axis set using an external switch or

setting operation can be read through the output signal (mirror-image

check signal). The mirror-image status present at that time can be

checked. (See III-4.9)

The value obtained in binary is converted into decimal notation.

#3007

#7

#6

#5

#4

#3

#2

#1

#0

Setting

8th axis

7th axis

6th axis

5th axis

4th axis

3th axis

2th axis

1th axis

0 (mirror-image function is disabled)

For each bit,

or

is indicated.

1 (mirror-image function is enabled)

Example : If #3007 is 3, the mirror-image function is enabled for the first and second axes.

S When the mirror-image function is set for a certain axis by both the

mirror-image signal and setting, the signal value and setting value are

ORed and then output.

S When mirror-image signals for axes other than the controlled axes are

turned on, they are still read into system variable #3007.

S System variable #3007 is a write-protected system variable. If an

attempt is made to write data in the variable, P/S 116 alarm “WRITE

PROTECTED VARIABLE” is issued.

401

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

D Number of machined

The number (target number) of parts required and the number (completion

parts

number) of machined parts can be read and written.

Table 15.2(i) System variables for the number of parts required and the

number of machined parts

Variable number

Function

#3901

Number of machined parts (completion number)

#3902

Number of required parts (target number)

NOTE

Do not substitute a negative value.

D Modal information

Modal information specified in blocks up to the immediately preceding

block can be read.

Table 15.2 (j) System variables for modal information

Variable number

Function

#4001

G00, G01, G02, G03, G33

(Group 01)

#4002

G17, G18, G19

(Group 02)

#4003

G90, G91

(Group 03)

#4004

(Group 04)

#4005

G94, G95

(Group 05)

#4006

G20, G21

(Group 06)

#4007

G40, G41, G42

(Group 07)

#4008

G43, G44, G49

(Group 08)

#4009

G73, G74, G76, G80-G89

(Group 09)

#4010

G98, G99

(Group 10)

#4011

G50, G51

(Group 11)

#4012

G65, G66, G67

(Group 12)

#4013

G96,G97

(Group 13)

#4014

G54-G59

(Group 14)

#4015

G61-G64

(Group 15)

#4016

G68, G69

(Group 16)

:

:

:

#4022

(Group 22)

#4102

B code

#4107

D code

#4109

F code

#4111

H code

#4113

M code

#4114

Sequence number

#4115

Program number

#4119

S code

#4120

T code

#4130

P code (number of the currently selected addition-

al workpiece coordinate system)

Example:

When #1=#4001; is executed, the resulting value in #1 is 0, 1, 2, 3, or

33.

If the specified system variable for reading modal information

corresponds to a G code group which cannot be used, a P/S alarm is

issued.

402

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

D Current position

Position information cannot be written but can be read.

Table 15.2 (k) System variables for position information

Read

Tool com-

Variable

Position

Coordinate

operation

pensation

number

information

system

during

value

movement

#5001-#5008

Block end point

Workpiece

Not

Enabled

coordinate

included

system

#5021-#5028

Current position

Machine

Included

Disabled

coordinate

system

#5041-#5048

Current position

Workpiece

coordinate

#5061-#5068

Skip signal position

system

Enabled

#5081-#5088

Tool length offset

Disabled

value

#5101-#5108

Deviated servo

position

S The first digit (from 1 to 8) represents an axis number.

S The tool length offset value currently used for execution rather than the

immediately preceding tool offset value is held in variables #5081 to

5088.

S The tool position where the skip signal is turned on in a G31 (skip

function) block is held in variables #5061 to #5068. When the skip

signal is not turned on in a G31 block, the end point of the specified

block is held in these variables.

S When read during movement is ”disabled,” this means that expected

values cannot be read due to the buffering (preread) function.

403

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

D Workpiece coordinate

Workpiece zero point offset values can be read and written.

system compensation

Table 15.2 (l) System variables for workpiece zero point offset values

values (workpiece zero

point offset values)

Variable

Function

number

#5201

First-axis external workpiece zero point offset value

:

:

#5208

Eighth-axis external workpiece zero point offset value

#5221

First-axis G54 workpiece zero point offset value

:

:

#5228

Eighth-axis G54 workpiece zero point offset value

#5241

First-axis G55 workpiece zero point offset value

:

:

#5248

Eighth-axis G55 workpiece zero point offset value

#5261

First-axis G56 workpiece zero point offset value

:

:

#5268

Eighth-axis G56 workpiece zero point offset value

#5281

First-axis G57 workpiece zero point offset value

:

:

#5288

Eighth-axis G57 workpiece zero point offset value

#5301

First-axis G58 workpiece zero point offset value

:

:

#5308

Eighth-axis G58 workpiece zero point offset value

#5321

First-axis G59 workpiece zero point offset value

:

:

#5328

Eighth-axis G59 workpiece zero point offset value

#7001

First-axis workpiece zero point offset value (G54.1 P1)

:

:

#7008

Eighth-axis workpiece zero point offset value

#7021

First-axis workpiece zero point offset value (G54.1 P2)

:

:

#7028

Eighth-axis workpiece zero point offset value

:

:

#7941

First-axis workpiece zero point offset value (G54.1 P48)

:

:

#7948

Eighth-axis workpiece zero point offset value

#14001

First-axis workpiece zero point offset value (G54.1 P1)

:

:

#14008

Eighth-axis workpiece zero point offset value

#14021

First-axis workpiece zero point offset value (G54.1 P2)

:

:

#14028

Eighth-axis workpiece zero point offset value

:

:

#19980

First-axis workpiece zero point offset value (G54.1 P300)

:

:

#19988

Eighth-axis workpiece zero point offset value

404

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

The following variables can also be used:

Axis

Function

Variable number

First axis

External workpiece zero point offset

#2500

#5201

G54 workpiece zero point offset

#2501

#5221

G55 workpiece zero point offset

#2502

#5241

G56 workpiece zero point offset

#2503

#5261

G57 workpiece zero point offset

#2504

#5281

G58 workpiece zero point offset

#2505

#5301

G59 workpiece zero point offset

#2506

#5321

Second

External workpiece zero point offset

#2600

#5202

axis

G54 workpiece zero point offset

#2601

#5222

G55 workpiece zero point offset

#2602

#5242

G56 workpiece zero point offset

#2603

#5262

G57 workpiece zero point offset

#2604

#5282

G58 workpiece zero point offset

#2605

#5302

G59 workpiece zero point offset

#2606

#5322

Third axis

External workpiece zero point offset

#2700

#5203

G54 workpiece zero point offset

#2701

#5223

G55 workpiece zero point offset

#2702

#5243

G56 workpiece zero point offset

#2703

#5263

G57 workpiece zero point offset

#2704

#5283

G58 workpiece zero point offset

#2705

#5303

G59 workpiece zero point offset

#2706

#5323

Fourth axis

External workpiece zero point offset

#2800

#5204

G54 workpiece zero point offset

#2801

#5224

G55 workpiece zero point offset

#2802

#5244

G56 workpiece zero point offset

#2803

#5264

G57 workpiece zero point offset

#2804

#5284

G58 workpiece zero point offset

#2805

#5304

G59 workpiece zero point offset

#2806

#5324

NOTE

To use variables #2500 to #2806 and #5201 to #5328,

optional variables for the workpiece coordinate systems are

necessary.

Optional variables for 48 additional workpiece coordinate

systems are #7001 to #7948 (G54.1 P1 to G54.1 P48).

Optional variables for 300 additional workpiece coordinate

systems are #14001 to #19988 (G54.1 P1 to G54.1 P300).

With these variables, #7001 to #7948 can also be used.

405

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

The operations listed in Table 15.3(a) can be performed on variables. The

15.3

expression to the right of the operator can contain constants and/or

ARITHMETIC AND

variables combined by a function or operator. Variables #j and #K in an

LOGIC OPERATION

expression can be replaced with a constant. Variables on the left can also

be replaced with an expression.

Table 15.3 (a) Arithmetic and logic operation

Function

Format

Remarks

Definition

#i=#j

Sum

#i=#j+#k;

Difference

#i=#j-#k;

Product

#i=#j*#k;

Quotient

#i=#j/#k;

Sine

#i=SIN[#j];

An angle is specified in de-

Arcsine

#i=ASIN[#j];

grees. 90 degrees and 30

Cosine

#i=COS[#j];

minutes is represented as

Arccosine

#i=ACOS[#j];

90.5 degrees.

Tangent

#i=TAN[#j];

Arctangent

#i=ATAN[#j]/[#k];

Square root

#i=SQRT[#j];

Absolute value

#i=ABS[#j];

Rounding off

#i=ROUND[#j];

Rounding down

#i=FIX[#j];

Rounding up

#i=FUP[#j];

Natural logarithm

#i=LN[#j];

Exponential function

#i=EXP[#j];

OR

#i=#j OR #k;

A logical operation is per-

XOR

#i=#j XOR #k;

formed on binary numbers

AND

#i=#j AND #k;

bit by bit.

Conversion from BCD to BIN

#i=BIN[#j];

Used for signal exchange

Conversion from BIN to BCD

#i=BCD[#j];

to and from the PMC

Explanations

D Angle units

The units of angles used with the SIN, COS, ASIN, ACOS, TAN, and

ATAN functions are degrees. For example, 90 degrees and 30 minutes is

represented as 90.5 degrees.

D ARCSIN #i = ASIN[#j];

S The solution ranges are as indicated below:

When the NAT bit (bit 0 of parameter 6004) is set to 0: 270_ to 90_

When the NAT bit (bit 0 of parameter 6004) is set to 1: -90_ to 90_

S When #j is beyond the range of -1 to 1, P/S alarm No. 111 is issued.

S A constant can be used instead of the #j variable.

D ARCCOS #i = ACOS[#j];

S The solution ranges from 180° to 0°.

S When #j is beyond the range of -1 to 1, P/S alarm No. 111 is issued.

S A constant can be used instead of the #j variable.

406

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

D Rounding up and down

With CNC, when the absolute value of the integer produced by an

to an integer

operation on a number is greater than the absolute value of the original

number, such an operation is referred to as rounding up to an integer.

Conversely, when the absolute value of the integer produced by an

operation on a number is less than the absolute value of the original

number, such an operation is referred to as rounding down to an integer.

Be particularly careful when handling negative numbers.

Example:

Suppose that #1=1.2 and #2=-1.2.

When #3=FUP[#1] is executed, 2.0 is assigned to #3.

When #3=FIX[#1] is executed, 1.0 is assigned to #3.

When #3=FUP[#2] is executed, -2.0 is assigned to #3.

When #3=FIX[#2] is executed, -1.0 is assigned to #3.

D Abbreviations of

When a function is specified in a program, the first two characters of the

arithmetic and logic

function name can be used to specify the function (See III-9.7).

operation commands

Example:

ROUND → RO

FIX → FI

D Priority of operations

Functions

Operations such as multiplication and division (*, /, AND)

Operations such as addition and subtraction (+, -, OR, XOR)

Example) #1=#2+#3*SIN[#4];

,

and

indicate the order of operations.

D Bracket nesting

Brackets are used to change the order of operations. Brackets can be used

to a depth of five levels including the brackets used to enclose a function.

When a depth of five levels is exceeded, P/S alarm No. 118 occurs.

Example) #1=SIN [ [ [#2+#3] *#4 +#5] *#6] ;

to

indicate the order of operations.

408

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

Limitations

D Brackets

Brackets ([, ]) are used to enclose an expression. Note that parentheses

are used for comments.

D Operation error

Errors may occur when operations are performed.

Table 15.3 (b) Errors involved in operations

Average

Maximum

Operation

Type of error

error

error

a = b*c

1.55×10^-10

4.66×10^-10

Relative error(*1)

a = b / c

4.66×10^-10

1.88×10^-9

e

a

Ǹ

1.24×10^-9

3.73×10^-9

a+

b

(*2)

a = b + c

2.33×10^-10

5.32×10^-10

e

e

a = b - c

Min

b

”

c

a = SIN [ b ]

5.0×10^-9

1.0×10^-8

Absolute error(*3)

a = COS [ b ]

ε

degrees

a = ATAN [ b ] / [ c ]

1.8×10^-6

3.6×10^-6

(*4)

NOTE

1

The relative error depends on the result of the operation.

2

Smaller of the two types of errors is used.

3

The absolute error is constant, regardless of the result of the

operation.

4

Function TAN performs SIN/COS.

5

If the result of the operation by the SIN, COS, or TAN

function is less than 1.0 x 10^-8 or is not 0 because of the

precision of the operation, the result of the operation can be

normalized to 0 by setting bit 1 (MFZ) of parameter No. 6004

to 1.

S The precision of variable values is about 8 decimal digits. When very

large numbers are handled in an addition or subtraction, the expected

results may not be obtained.

Example:

When an attempt is made to assign the following values to variables

#1 and #2:

#1=9876543210123.456

#2=9876543277777.777

the values of the variables become:

#1=9876543200000.000

#2=9876543300000.000

In this case, when #3=#2-#1; is calculated, #3=100000.000 results.

(The actual result of this calculation is slightly different because it is

performed in binary.)

409

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

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 ...)

15.5.1

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

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;

15.5.2

Specify a conditional expression after IF.

Conditional Branch

(IF Statement)

IF[<conditional

If the specified conditional expression is satisfied, a branch to sequence

expression>]GOTOn

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

is executed.

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

N2 occurs.

If the condi-

IF [#1 GT 10] GOTO 2 ;

tion is not sa-

tisfied

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

D Conditional expression

A conditional expression must include an operator inserted between two

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

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

412

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

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

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 condi-

If the condi-

Processing

tion is not sa-

tion is satis-

tisfied

fied

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.

413

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

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

1. The identification numbers

a maximum depth of three lev-

(1 to 3) can be used as many

els.

times as required.

WHILE [ … ] DO 1 ;

WHILE [ … ] DO 1 ;

:

WHILE [ … ] DO 2 ;

Processing

:

END 1 ;

WHILE [ … ] DO 3 ;

:

Processing

WHILE [ … ] DO 1 ;

END 3 ;

Processing

:

END 2 ;

END 1 ;

:

END 1 ;

2. DO ranges cannot overlap.

4. Control can be transferred to

WHILE [ … ] DO 1 ;

the 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 <vacant> and zero have

different effects. In other types of conditional expressions, a <vacant> is

regarded as zero.

414

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

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 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 ;

O9010 ;

:

#3=#1+#2 ;

G65 P9010 L2 A1.0 B2.0 ;

IF [#3 GT 360] GOTO 9 ;

:

G00 G91 X#3 ;

M30 ;

N9 M99 ;

Explanations

D Call

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

macro to call.

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

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

S By using argument specification, values are assigned to corresponding

local variables.

Two types of argument specification are available. Argument

D Argument specification

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

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

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

corresponding to an omitted address are set to null.

S 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

417

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

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.

Address

Variable

Address

Variable

Address

Variable

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

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

specification are not written in the actual program.

Limitations

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:

#7:4.0

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).

418

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

D Local variable levels

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

S The level of the main program is 0.

S 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.

S 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 ;

#1=2;

#1=3;

#1=4;

#1=5;

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

419

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

Sample program

A macro is created which drills H holes at intervals of B degrees after a

(bolt hole circle)

start angle of A degrees along the periphery of a circle with radius I.

The center of the circle is (X,Y). Commands can be specified in either

the absolute or incremental mode. To drill in the clockwise direction,

specify a negative value for B.

H=2

ÉÉ

H=3

H=1

ÉÉ

ÉÉÉÉÉ

ÉÉ

ÉÉÉÉÉ

H=4

B

B

A

Center (X,Y)

Radius I

D Calling format

G65 P9100 X x Y y Z z R r F f I i A a B b H h ;

X: X coordinate of the center of the circle

(absolute or incremental specification)

(#24)

Y: Y coordinate of the center of the circle

(absolute or incremental specification)

(#25)

Z: Hole depth

(#26)

R: Coordinates of an approach point

(#18)

F : Cutting feedrate

(#9)

I

: Radius of the circle

(#4)

A: Drilling start angle

(#1)

B: Incremental angle (clockwise when a negative value is specified)

(#2)

H: Number of holes

(#11)

D Program calling a macro

O0002;

program

G90 G92 X0 Y0 Z100.0;

G65 P9100 X100.0 Y50.0 R30.0 Z-50.0 F500 I100.0 A0 B45.0 H5;

M30;

420

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

D Macro program

O9100;

(called program)

#3=#4003; Stores G code of group 3.

G81 Z#26 R#18 F#9 K0; (Note) Drilling cycle.

Note: L0 can also be used.

IF[#3 EQ 90]GOTO 1;

Branches to N1 in the G90 mode.

#24=#5001+#24;

Calculates the X coordinate of

the center.

#25=#5002+#25;

Calculates the Y coordinate of

the center.

N1 WHILE[#11 GT 0]DO 1;

. . . . . . . . . . . . . . . . . . . . . . . . . . Until the number of remaining holes

reaches 0

#5=#24+#4*COS[#1];

Calculates a drilling position on

the X-axis.

#6=#25+#4*SIN[#1];

Calculates a drilling position on

the Y-axis.

G90 X#5 Y#6;

Performs drilling after moving to

the target position.

#1=#1+#2;

Updates the angle.

#11=#11-1;

Decrements the number of holes.

END 1;

G#3 G80;

Returns the G code to the original state.

M99;

Meaning of variables:

#3: Stores the G code of group 3.

#5: X coordinate of the next hole to drill

#6: Y coordinate of the next hole to drill

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 F300 ;

Y200.0 ;

:

X150.0 Y300.0 ;

:

G67 ;

:

:

:

M30 ;

M99 ;

421

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

Explanations

D Call

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

call.

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

be specified at address L.

S 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.

Limitations

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

S G66 needs to be specified before any arguments.

S 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.

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

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

Sample program

The same operation as the drilling canned cycle G81 is created using a

custom macro and the machining program makes a modal macro call. For

program simplicity, all drilling data is specified using absolute values.

Rapid traverse

The canned cycle consists of the following

basic operations:

Cutting feed

Operation 1:

Operation 1

Position I

Positioning along the X-axis and Y-axis

Operation 2:

Operation 4

Operation 2

Rapid traverse to point R

R

Position R

Operation 3:

Cutting feed to point Z

Z=0

Operation 3

Operation 4:

Rapid traverse to point R or I

Position Z

Z

422

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

D Calling format

G65 P9110 X x Y y Z z R r F f L l ;

X: X coordinate of the hole (absolute specification only)

(#24)

Y: Y coordinate of the hole (absolute specification only)

(#25)

Z : Coordinates of position Z (absolute specification only) . . .

(#26)

R : Coordinates of position R (absolute specification only) . . .

(#18)

F : Cutting feedrate

(#9)

L: Repetition count

D Program that calls a

O0001;

macro program

G28 G91 X0 Y0 Z0;

G92 X0 Y0 Z50.0;

G00 G90 X100.0 Y50.0;

G66 P9110 Z-20.0 R5.0 F500;

G90 X20.0 Y20.0;

X50.0;

Y50.0;

X70.0 Y80.0;

G67;

M30;

D Macro program

O9110;

(program called)

#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;

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

15.6.3

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 Y20.0 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 (O9010 to O9019) in the corresponding parameter (N0.6050 to

No.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.

423

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

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.

Limitations

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.

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 an

(G65).

M Code

O0001 ;

O9020 ;

:

:

M50 A1.0 B2.0 ;

:

:

:

M30 ;

M99 ;

Parameter No.6080 = 50

Explanations

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

macro program (9020 to 9029) in the corresponding parameter (No.6080

to No.6089), the macro program can be called in the same way as with

G65.

424

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

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.

Limitations

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

of a block.

S 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.

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 No.6071 = 03

Explanations

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

subprogram in a parameter (No.6071 toNo. 6079), the corresponding

custom macro program (O9001 to O9009) can be called in the same way

as with M98.

425

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

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.

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

15.6.6

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 ;

:

:

T23 ;

:

:

:

M30 ;

M99 ;

Bit 5 of parameter 6001 = 1

Explanations

D Call

By setting bit 5 of parameter TCS 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.

426

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

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

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

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

S 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

S 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

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;

427

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

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

15.7

performed next. This operation is referred to as buffering. During AI

PROCESSING

contour control mode or AI nano contour control mode, the CNC prereads

MACRO

not only the next block but also the multiple blocks. And in the cutter

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

STATEMENTS

two or three blocks ahead to find intersections even if the CNC is not in

AI contour control mode nor AI nano contour control mode. 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 parameter

(No.3411-3432), and blocks containing prevention buffering G codes

such as 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.

15.7.1

Details of NC

Statements and Macro

Statements Execution

D When the next block is

not buffered

> N1 G31 X100.0 ;

N1

(M codes that are not

NC statement

N2 #100=1

buffered, G53, G31, etc.)

execution

:

N2

Macro statement execution

> :Block being executed

Buffer

NOTE

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 are 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.

429

Content      ..     13      14      15      16     ..