Content      ..     6      7      8      9     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. OPERATOR'S MANUAL - page 8

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Variable

Category

Variable name

Description

number

<1>

#4114

[#_BUFN]

Modal information

<2>

#4314

[#_ACTN]

(sequence number N)

<3>

#4514

[#_INTN]

<1>

#4115

[#_BUFO]

Modal information

<2>

#4315

[#_ACTO]

(program number O)

<3>

#4515

[#_INTO]

<1>

#4119

[#_BUFS]

<2>

#4319

[#_ACTS]

Modal information (S code)

<3>

#4519

[#_INTS]

<1>

#4120

[#_BUFT]

<2>

#4320

[#_ACTT]

Modal information (T code)

<3>

#4520

[#_INTT]

NOTE

Previous block and running block

Since the CNC reads the block that is ahead of the block currently being

executed by the machining program, the block being retrieved by the CNC is

normally different from that currently being executed. The previous block

indicates the block that is ahead of the block being retrieved by the CNC, that is,

the block that is ahead of the program block in which #4001 to #4130 are

specified.

[Example] O1234 ;

N10 G00 X200. Y200. ;

N20 G01 X1000. Y1000. F10. ;

:

:

N50 G00 X500. Y500. ;

N60 #1 = #4001 ;

Assume that the CNC is currently executing N20. If the CNC retrieved and processed the blocks up to N60 as

shown above, the running block is N20 and the previous block is N50. Therefore, group 1 modal information in the

running block is G01 and group 1 modal information in the previous block is G00.

When N60 #1 = #4201, #1 = 1.

When N60 #1 = #4001, #1 = 0.

-

Position information #5001-#5065 (Attribute: R)

The end position of the previous block, the specified current position (for the machine coordinate system

and workpiece coordinate system), and the skip signal position can be obtained by reading the values of

system variables #5001 to #5065.

Tool position/tool

Reading

Variable

Coordinate

Variable name

Position information

length/cutter

operation during

number

system

compensation

movement

#5001

[#_ABSIO[1]]

1st axis block end point position

Workpiece

:

:

:

coordinate

Not included

Enabled

#5005

[#_ABSIO[5]]

5th axis block end point position

system

#5021

[#_ABSMT[1]]

1st axis current position

Machine

:

:

:

coordinate

Included

Disabled

#5025

[#_ABSMT[5]]

5th axis current position

system

- 186 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Tool position/tool

Reading

Variable

Coordinate

Variable name

Position information

length/cutter

operation during

number

system

compensation

movement

#5041

[#_ABSOT[1]]

1st axis current position

Workpiece

:

:

:

coordinate

Included

Disabled

#5045

[#_ABSOT[5]]

5th axis current position

system

#5061

[#_ABSKP[1]]

1st axis skip position

Workpiece

:

:

:

coordinate

Included

Enabled

#5065

[#_ABSKP[5]]

5th axis skip position

system

NOTE

1 When variables exceeding the number of control axes are specified, the alarm

PS0115, “VARIABLE NO. OUT OF RANGE” occurs.

2 The block end point position (ABSIO) of the skip (G31) is the position where the

skip signal is turned on. If the skip signal is not turned on, the position is the

end position of the block.

3 "Read operation during movement is disabled" means that the accurate reading

of values during movement is not guaranteed.

-

Tool length compensation value #5081#5085 (Attribute: R)

M

Tool length compensation in the block currently being executed can be obtained for each axis by reading

system variables #5081 to #5085.

Variable

Read operation

Variable name

Position information

number

during movement

#5081

[#_TOFS[1]]

1st axis tool length compensation value

:

:

:

Disabled

#5085

[#_TOFS[5]]

5th axis tool length compensation value

NOTE

When variables exceeding the number of control axes are specified, the alarm

PS0115, “VARIABLE NO. OUT OF RANGE” occurs.

-

Tool offset

#5081#5085, #5121-#5125 (Attribute: R)

T

Tool offset in the block currently being executed can be obtained for each axis by reading system

variables #5081 to #5085 or #5121 to #5125.

(X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic

three axes, Y-axis: Y-axis of basic three axes)

<1> Without tool geometry/wear compensation memory (bit 6 (NGW) of parameter No.8136 = 1)

Variable

Read operation

Variable name

Position information

number

during movement

#5081

[#_TOFSWX]

X-axis tool offset value

#5082

[#_TOFSWZ]

Z-axis tool offset value

#5083

[#_TOFSWY]

Y-axis tool offset value

Disabled

#5084

[#_TOFS[4]]

4th axis tool offset value

#5085

[#_TOFS[5]]

5th axis tool offset value

- 187 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

<2> With tool geometry/wear compensation memory (bit 6 (NGW) of parameter No.8136 = 0)

Variable

Read operation

Variable name

Position information

number

during movement

#5081

[#_TOFSWX]

X-axis tool offset value (wear)

#5082

[#_TOFSWZ]

Z-axis tool offset value (wear)

#5083

[#_TOFSWY]

Y-axis tool offset value (wear)

#5084

[#_TOFS[4]]

4th axis tool offset value (wear)

#5085

[#_TOFS[5]]

5th axis tool offset value (wear)

Disabled

#5121

[#_TOFSGX]

X-axis tool offset value (geometry)

#5122

[#_TOFSGZ]

Z-axis tool offset value (geometry)

#5123

[#_TOFSGY]

Y-axis tool offset value (geometry)

#5124

[#_TOFSG[4]]

4th axis tool offset value (geometry)

#5125

[#_TOFSG[5]]

5th axis tool offset value (geometry)

When the tool geometry/wear compensation memory is present (bit 6 (NGW) of parameter No. 8136 is 0),

the system variables depend on the settings of bit 2 (LWT) of parameter No. 5002 and bit 4 (LGT) of

parameter No. 5002, as shown below.

Variable

LWT=0

LWT=1

LWT=0

LWT=1

number

LGT=0

LGT=0

LGT=1

LGT=1

#5081

#5082

#5083

Wear compensation

0

Wear compensation

Wear compensation

#5084

#5085

#5121

#5122

Wear compensation +

#5123

Geometry compensation

Geometry compensation

Geometry compensation

Geometry compensation

#5124

#5125

NOTE

1 The set value is read as the tool offset regardless of bit 1 (ORC) of parameter

No.5004 and bit 0 (OWD) of parameter No.5040.

2 To read the tool offset (geometry) using #5121 to #5125, set bit 2 (VHD) of

parameter No.6004 to 0.

-

Servo position deviation #5101-#5105 (Attribute: R)

The servo position deviation for each axis can be obtained by reading system variables #5101 to #5105.

Variable

Read operation during

Variable name

Position information

number

movement

#5101

[#_SVERR[1]]

1st axis servo position deviation

:

:

:

Disabled

#5105

[#_SVERR[5]]

5th axis servo position deviation

NOTE

When variables exceeding the number of control axes are specified, the alarm

PS0115, “VARIABLE NO. OUT OF RANGE” occurs.

-

Manual handle interruption #5121-#5125 (Attribute: R)

The manual handle interruption for each axis can be obtained by reading system variables #5121 to

#5125.

- 188 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Variable

Read operation

Variable name

Position information

number

during movement

#5121

[#_MIRTP[1]]

1st axis manual handle interruption

:

:

:

Disabled

#5125

[#_MIRTP[5]]

5th axis manual handle interruption

NOTE

When variables exceeding the number of control axes are specified, the alarm

PS0115, “VARIABLE NO. OUT OF RANGE” occurs.

T

NOTE

#5121 to #5125 are enabled only when bit 2 (VHD) of parameter No.6004 is set

to 1.

-

Distance to go #5181-#5185 (Attribute: R)

The distance to go value for each axis can be obtained by reading system variables #5181 to #5185.

Variable

Read operation during

Variable name

Position information

number

movement

#5181

[#_DIST[1]]

1st axis distance to go value

:

:

:

Disabled

#5185

[#_DIST[5]]

5th axis distance to go value

NOTE

When variables exceeding the number of control axes are specified, the alarm

PS0115, “VARIABLE NO. OUT OF RANGE” occurs.

-

Workpiece origin offset value #5201-#5325 (Attribute: R/W)

The workpiece origin offset value can be obtained by reading system variables #5201 to #5325. The

offset value can also be changed by assigning values to the system variables.

Variable

Workpiece coordinate

Variable name

Controlled axis

number

system

#5201

[#_WZCMN[1]]

1st axis external workpiece origin offset value

External workpiece origin

:

:

:

offset value (applied to all

#5205

[#_WZCMN[5]]

5th axis external workpiece origin offset value

coordinate systems)

#5221

[#_WZG54[1]]

1st axis workpiece origin offset value

:

:

:

G54

#5225

[#_WZG54[5]]

5th axis workpiece origin offset value

#5241

[#_WZG55[1]]

1st axis workpiece origin offset value

:

:

:

G55

#5245

[#_WZG55[5]]

5th axis workpiece origin offset value

#5261

[#_WZG56[1]]

1st axis workpiece origin offset value

:

:

:

G56

#5265

[#_WZG56[5]]

5th axis workpiece origin offset value

#5281

[#_WZG57[1]]

1st axis workpiece origin offset value

:

:

:

G57

#5285

[#_WZG57[5]]

5th axis workpiece origin offset value

- 189 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Variable

Workpiece coordinate

Variable name

Controlled axis

number

system

#5301

[#_WZG58[1]]

1st axis workpiece origin offset value

:

:

:

G58

#5305

[#_WZG58[5]]

5th axis workpiece origin offset value

#5321

[#_WZG59[1]]

1st axis workpiece origin offset value

:

:

:

G59

#5325

[#_WZG59[5]]

5th axis workpiece origin offset value

M

The following variables can also be used when bit 5 (D15) of parameter No. 6004 is set to 0:

Axis

Function

Variable number

1st axis

External workpiece origin offset value

#2500

G54 workpiece origin offset value

#2501

G55 workpiece origin offset value

#2502

G56 workpiece origin offset value

#2503

G57 workpiece origin offset value

#2504

G58 workpiece origin offset value

#2505

G59 workpiece origin offset value

#2506

2nd axis

External workpiece origin offset value

#2600

G54 workpiece origin offset value

#2601

G55 workpiece origin offset value

#2602

G56 workpiece origin offset value

#2603

G57 workpiece origin offset value

#2604

G58 workpiece origin offset value

#2605

G59 workpiece origin offset value

#2606

3rd axis

External workpiece origin offset value

#2700

G54 workpiece origin offset value

#2701

G55 workpiece origin offset value

#2702

G56 workpiece origin offset value

#2703

G57 workpiece origin offset value

#2704

G58 workpiece origin offset value

#2705

G59 workpiece origin offset value

#2706

4th axis

External workpiece origin offset value

#2800

G54 workpiece origin offset value

#2801

G55 workpiece origin offset value

#2802

G56 workpiece origin offset value

#2803

G57 workpiece origin offset value

#2804

G58 workpiece origin offset value

#2805

G59 workpiece origin offset value

#2806

T

The following variables can be used to maintain compatibility with conventional models.

Axis

Function

Variable number

1st axis

External workpiece origin offset value

#2550

G54 workpiece origin offset value

#2551

G55 workpiece origin offset value

#2552

G56 workpiece origin offset value

#2553

G57 workpiece origin offset value

#2554

G58 workpiece origin offset value

#2555

G59 workpiece origin offset value

#2556

- 190 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Axis

Function

Variable number

2nd axis

External workpiece origin offset value

#2650

G54 workpiece origin offset value

#2651

G55 workpiece origin offset value

#2652

G56 workpiece origin offset value

#2653

G57 workpiece origin offset value

#2654

G58 workpiece origin offset value

#2655

G59 workpiece origin offset value

#2656

3rd axis

External workpiece origin offset value

#2750

G54 workpiece origin offset value

#2751

G55 workpiece origin offset value

#2752

G56 workpiece origin offset value

#2753

G57 workpiece origin offset value

#2754

G58 workpiece origin offset value

#2755

G59 workpiece origin offset value

#2756

4th axis

External workpiece origin offset value

#2850

G54 workpiece origin offset value

#2851

G55 workpiece origin offset value

#2852

G56 workpiece origin offset value

#2853

G57 workpiece origin offset value

#2854

G58 workpiece origin offset value

#2855

G59 workpiece origin offset value

#2856

NOTE

1 When variables exceeding the number of control axes are specified, the alarm

PS0115, “VARIABLE NO. OUT OF RANGE” occurs.

2 For the workpiece origin offset values for up to the number (5) of control axes,

variables #5201 to #5325 can also be used.

M

NOTE

To use variables #2500 to #2806 and #5201 to #5325, enable the workpiece

coordinate system (bit 0 (NWZ) of parameter No. 8136 is 0).

T

NOTE

To use variables #2550 to #2856 and #5201 to #5325, enable the workpiece

coordinate system (bit 0 (NWZ) of parameter No. 8136 is 0).

-

Workpiece origin offset value of the additional workpiece coordinate system

#7001-#7945, #14001-#14945 (Attribute: R/W)

M

The workpiece origin offset value of the additional workpiece coordinate system can be obtained by

reading system variables #7001 to #7945, #14001 to #14945. The offset value can also be changed by

assigning values to the system variables.

Variable

Additional workpiece

Variable name

Controlled axis

number

system number

#7001

[#_WZP1[1]]

1st axis workpiece origin offset value

1

:

:

:

(G54.1 P1)

#7005

[#_WZP1[5]]

5th axis workpiece origin offset value

- 191 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Variable

Additional workpiece

Variable name

Controlled axis

number

system number

#7021

[#_WZP2[1]]

1st axis workpiece origin offset value

2

:

:

:

(G54.1 P2)

#7025

[#_WZP2[5]]

5th axis workpiece origin offset value

:

:

:

:

#7941

[#_WZP48[1]]

1st axis workpiece origin offset value

48

:

:

:

(G54.1 P48)

#7945

[#_WZP48[5]]

5th axis workpiece origin offset value

System variable number = 7000 + (Coordinate system number -1) × 20 + Axis number

Coordinate number: 1 to 48

Axis number:

1 to 5

Variable

Additional workpiece

Variable name

Controlled axis

number

system number

#14001

[#_WZP1[1]]

1st axis workpiece origin offset value

1

:

:

:

(G54.1 P1)

#14005

[#_WZP1[5]]

5th axis workpiece origin offset value

#14021

[#_WZP2[1]]

1st axis workpiece origin offset value

2

:

:

:

(G54.1 P2)

#14025

[#_WZP2[5]]

5th axis workpiece origin offset value

:

:

:

:

#14941

[#_WZP48[1]]

1st axis workpiece origin offset value

48

:

:

:

(G54.1 P48)

#14945

[#_WZP48[5]]

5th axis workpiece origin offset value

System variable number = 14000 + (Coordinate system number -1) × 20 + Axis number

Coordinate number: 1 to 48

Axis number:

1 to 5

NOTE

1 When variables exceeding the number of control axes are specified, the alarm

PS0115, “VARIABLE NO. OUT OF RANGE” occurs.

2 To use variables #7001 to #7945 and #14001 to #14945 (G54.1 P1 to G54.1

P48), enable the addition of workpiece coordinate system pairs (48 pairs) (bit 2

(NWN) of parameter No. 8136 is 0).

-

Switching between P-CODE variables and system variables (#10000 or later)

#8570 (Attribute: R/W)

This system variable allows read/write operations of P-CODE variables (#10000 to #89999) for the macro

executor function. For details on P-CODE variables, refer to the Macro Compiler / Macro Executor

Programming Manual (B-64303EN-2).

System variable #8570 can be used to make variables #10000 or later correspond to either P-CODE

variables or system variables.

#8570 setting

Specified variable

Corresponding variable

#10000

System variables (#10000)

#8570 = 0

:

:

#89999

System variables (#89999)

- 192 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

#8570 setting

Specified variable

Corresponding variable

#10000

P-CODE variables (#10000)

#8570 = 1

:

:

#89999

P-CODE variables (#89999)

Example

#8570 = 0 ;

#10001 = 123 ; → Writing to system variable #10001 (tool compensation)

#8570 = 1 ;

#10001 = 456 ; → Writing to P-CODE variable #10001 (tool compensation)

NOTE

1 Variable #8570 can be used only when the macro executor function is enabled.

2 System variables (#10000 or later) always correspond to system variables

specified by their variable names even when #8570 is 1.

3 When an attempt is made to access a variable that cannot be used with

P-CODE variables (#10000 or later), an alarm PS0115 occurs.

14.3 ARITHMETIC AND LOGIC OPERATION

Various operations can be performed on variables. Program an arithmetic and logic operation in the same

way as for a general arithmetic expression.

#i=<expression>

<Expression>

The expression to the right of the arithmetic and logic operation contains constants and/or variables

combined by a function or operator. Variables #j and #k below can be replaced with a constant. If a

constant used in an expression has no decimal point, it is assumed to end with a decimal point.

Table 14.3 (a) Arithmetic and logic operation

Type of operation

Operation

Description

<1> Definition or

#i=#j

Definition or replacement of a variable

replacement

<2> Addition-type

#i=#j+#k

Addition

operations

#i=#j-#k

Subtraction

#i=#j OR #k

Logical OR (bit by bit of 32 bits)

#i=#j XOR #k

Exclusive OR (bit by bit of 32 bits)

<3> Multiplication-type

#i=#j*#k

Multiplication

operations

#i=#j/#k

Division

#i=#j AND #k

Logical AND (bit by bit of 32 bits)

#i=#j MOD #k

Remainder (A remainder is obtained after #j and #k are

rounded to their nearest whole numbers. When #j is a

negative value, #i is assumed to be a negative value.)

- 193 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Type of operation

Operation

Description

<4> Functions

#i=SIN[#j]

Sine (in degrees)

#i=COS[#j]

Cosine (in degrees)

#i=TAN[#j]

Tangent (in degrees)

#i=ASIN[#j]

Arc sine

#i=ACOS[#j]

Arc cosine

#i=ATAN[#j]

Arc tangent (one argument), ATN can also be used.

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

Arc tangent (two arguments), ATN can also be used.

#i=ATAN[#j,#k]

Arc tangent (two arguments), ATN can also be used.

#i=SQRT[#j]

Square root, SQR can also be used.

#i=ABS[#j]

Absolute value

#i=BIN[#j]

Conversion from BCD to binary

#i=BCD[#j]

Conversion from binary to BCD

#i=ROUND[#j]

Rounding off, RND can also be used.

#i=FIX[#j]

Rounding down to an integer

#i=FUP[#j]

Rounding up to an integer

#i=LN[#j]

Natural logarithm

#i=EXP[#j]

Exponent using base e (2.718...)

#i=POW[#j,#k]

Power (#j to the #kth power)

#i=ADP[#j]

Addition of a decimal point

Explanation

-

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.

-

ARCSIN #i = ASIN[#j];

•

The solution ranges are as indicated below:

When the bit 0 (NAT) of parameter No.6004 is set to 0: 270° to 90°

When the bit 0 (NAT) of parameter No.6004 is set to 1: -90° to 90°

•

When #j is beyond the range of -1 to 1, an alarm PS0119 is issued.

•

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

-

ARCCOS #i = ACOS[#j];

•

The solution ranges from 180° to 0°.

•

When #j is beyond the range of -1 to 1, an alarm PS0119 is issued.

•

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

-

ARCTAN #i = ATAN[#j]/[#k]; (two arguments)

•

ATAN[#j,#k] is equivalent to ATAN[#j]/[#k].

•

When point (#k,#j) on plane X-Y is given, this function returns the value of the arc tangent for the

angle made by the point.

•

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

•

The solution ranges are as follows:

When the bit 0 (NAT) of parameter No.6004 is set to 0: 0° to 360°

Example:

When #1 = ATAN[-1]/[-1]; is specified, #1 is 225.0.

When the bit 0 (NAT) of parameter No.6004 is set to 1: -180° to 180°

Example:

When #1 = ATAN[-1]/[-1]; is specified, #1 is -135.0.

- 194 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

-

Rounding up and down to an integer (FUP and FIX)

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

-

Abbreviations of arithmetic and logic operation commands

When a function is specified in a program, the first two characters of the function name can be used to

specify the function.

Example:

ROUND → RO

FIX → FI

NOTE

1 POW cannot be abbreviated.

2 When an operation command is entered in an abbreviated form, the abbreviated

form is displayed as is.

For example, when "RO" is entered, "RO" is displayed as is without being

converted to "ROUND".

-

Priority of operations

<1> Functions

<2> Operations such as multiplication and division (*, /, AND)

<3> Operations such as addition and subtraction (+, -, OR, XOR)

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

<1>

<2>

<1>, <2> and <3> indicate the order of

<3>

operations.

-

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, an alarm

PS0118 occurs.

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

<1>

<2>

<3>

<4>

<5>

<1> to <5> indicate the order of operations.

- 196 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

When bit 0 (F0C) of parameter No. 6008 is set to 1

Errors may occur when operations are performed.

Table 14.3 (b) Errors involved in operations

Operation

Average error

Maximum error

Type of error

a = b*c

1.55×10^-10

4.66×10^-10

Relative error

a = b / c

4.66×10^-10

1.88×10^-9

ε

a

a = b

1.24×10^-9

3.73×10^-9

a = b + c

2.33×10^-10

5.32×10^-10

ε

ε

MIN

b

,

c

a = b - c

a = SIN [ b ]

5.0×10^-9

1.0×10^-8

Absolute error

a = COS [ b ]

degrees

ε

a = ATAN [ b ] / [ c ]

1.8×10^-6

3.6×10^-6

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 Note that, in the case of natural logarithm #i=LN[#j]; and exponential function

#i=EXP[#j];, the relative error may become 10^-8 or greater.

6 The operation result of exponential function

#i=EXP[#j]; overflows when

#j

exceeds about 110.

•

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.)

•

Also be aware of errors that can result from conditional expressions using EQ, NE, GE, GT, LE, and

LT.

Example:

IF[#1 EQ #2] is effected by errors in both #1 and #2, possibly resulting in an incorrect decision.

Therefore, instead find the difference between the two variables with IF[ABS[#1-#2]LT0.001].

Then, assume that the values of the two variables are equal when the difference does not exceed an

allowable limit (0.001 in this case).

•

Also, be careful when rounding down a value.

Example:

When #2=#1*1000; is calculated where #1=0.002;, the resulting value of variable #2 is not exactly 2 but

1.99999997.

Here, when #3=FIX[#2]; is specified, the resulting value of variable #3 is not 2.0 but 1.0.

In this case, round down the value after correcting the error so that the result is greater than the expected

number, or round it off as follows:

#3=FIX[#2+0.001]

#3=ROUND[#2]

- 198 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

14.4 READING PARAMETERS

Overview

By using the PRM function, it is possible to read parameters.

Format

Remarks

#i = PRM[ #j, #k ] ;

In the case of parameters other than axis type parameters

#i = PRM[ #j, #k ] / [ #l ] ;

In the case of axis type parameters

Explanation

-

Reading a parameter

#i=PRM[#j,#k]

#i=PRM[#j,#k]/[#l]

• For #j, enter a parameter number. If the number of a parameter that cannot be read, alarm PS0119,

"ARGUMENT VALUE OUT OF RANGE", is issued.

• To read a bit type parameter, specify, for #k, the bit number of the bit type parameter in the range of

0 to 7. If a bit number is specified, data with the specified bit is read. If none is specified, data with

all bits is read. For parameters other than bit type parameters, the bit number is ignored.

• For #l, set the axis number of an axis type parameter in the range of 1 to 5. If an axis type parameter

is to be read but #l is not specified, alarm PS0119 is issued. For parameters other than axis type

parameters, #1 may be omitted together with '/'.

Example

1.

Reading the value of the third axis of bit 0 (MIR) of bit axis type parameter No. 0012

If parameter No. 0012 (third axis) = 10000001

#2=12 ;

Parameter number setting

#3=0 ;

Bit number setting

#4=3 ;

Axis number setting

If reading data with all bits

#1=PRM[#2]/[#4] ;

#1=10000001

If reading data with a specified bit

#1=PRM[#2, #3]/[#4] ;

#1=1

2.

Reading the value of the fourth axis of axis type parameter No. 1322

#2=1322 ;

Parameter number setting

#4=4 ;

Axis number setting

#1=PRM[#2]/[#4] ;

3.

Reading bit 2 (SBP) of bit type parameter No. 3404

If parameter No. 3404 = 10010000

#2=3404 ;

Parameter number setting

#3=2 ;

Bit number setting

If reading data with all bits

#1=PRM[#2] ;

#1=10010000

If reading data with a specified bit

#1=PRM[#2,#3] ;

#1=0

- 200 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

14.5 MACRO STATEMENTS AND NC STATEMENTS

The following blocks are referred to as macro statements:

• Blocks containing an arithmetic or logic operation (=)

• Blocks containing a control statement (such as GOTO, DO, END)

• Blocks containing a macro call command (such as macro calls by G65, G66, G67, or other G codes,

or by M codes)

Any block other than a macro statement is referred to as an NC statement.

Explanation

-

Differences from NC statements

• Even when single block mode is on, the machine does not stop. Note, however, that the machine

stops in the single block mode when bit 5 of parameter SBM No. 6000 is 1.

M

• Macro blocks are not regarded as blocks that involve no movement in the cutter compensation mode.

-

NC statements that have the same property as macro statements

• An NC statement has the same property as a macro statement when the NC statement is a

subprogram call command (subprogram call by an M98, M code or subprogram call by a T code)

and is also a block that does not include any command address other than O, N, P, and L.

• An NC statement has the same property as a macro statement when the NC statement is an M99

command and is also a block that does not include any command address other than O, N, P, and L.

14.6 BRANCH AND REPETITION

In a program, the flow of control can be changed using the GOTO statement and IF statement. Three

types of branch and repetition operations are used:

Branch and

GOTO

(unconditional branch)

repetition

IF

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

WHILE

(repetition while ...)

14.6.1 Unconditional Branch (GOTO Statement)

A branch to sequence number n occurs. When a sequence number outside of the range 1 to 99999 is

specified, an alarm PS1128 occurs. A sequence number can also be specified using an expression.

GOTOn ; n: Sequence number (1 to 99999)

Example:

GOTO 1;

GOTO #10;

WARNING

Do not specify multiple blocks with the same sequence number in a single

program. It is very dangerous to specify such blocks because the destination of

a branch from the GOTO statement is undefined.

- 201 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

NOTE

1 A backward branch takes more time as compared with a forward branch.

2 In the block with sequence number n, which is the branch destination of the

GOTO n command, sequence number n must be located at the beginning of the

block. Otherwise, the branch cannot be executed.

14.6.2 GOTO Statement Using Stored Sequence Numbers

When the GOTO statement is executed in a custom macro control command, a sequence number search is

made for sequence numbers stored at previous execution of the corresponding blocks at a high speed.

Sequence numbers stored at previous execution indicate the sequence numbers for a subprogram call and

the sequence numbers that are unique in the same program of the sequence numbers at previous execution,

and the CNC records these sequence numbers.

The storage type differs depending on the values of the following parameters.

(1) When bit 1 (MGO) of parameter No. 6000 is set to 1

•

Fixed type:

Up to 20 sequence numbers stored at execution of the corresponding blocks

from the start of operation

(2) When bit 4 (HGO) of parameter No. 6000 is set to 1

•

Variable type: Up to 30 sequence numbers stored at execution of the corresponding blocks

before execution of the GOTO statement

•

History type: Up to 10 sequence numbers stored by a sequence number search previously

made using the GOTO statement

The stored sequence numbers are canceled in the following cases:

•

Immediately after power-on

•

After a reset

•

Operation after program registration or editing (including background editing and MDI program

editing)

WARNING

Do not specify multiple blocks with the same sequence number in a single

program.

It is very dangerous to specify the sequence number of the branch destination

before and after the GOTO statement and execute the GOTO statement

because the branch destination changes according to the values of the

parameters as shown below:

When bit 1 (MGO) or 4 (HGO) of parameter No.

When both bits 1 (MGO) and 4 (HGO) of

6000 is set to 1

parameter No. 6000 are set to 0

:

:

A branch to

N10;

N10;

N10 before

:

:

A branch to

the GOTO

GOTO10;

GOTO10;

N10 after the

statement

:

:

GOTO

occurs.

N10;

N10;

statement

occurs.

When bit 1 (MGO) or 4 (HGO) of parameter No. 6000 is set to 1 and the GOTO

statement is executed, the sequence number of the branch destination may not

be contained in the sequence numbers stored at previous execution of the

corresponding blocks. In this case, a branch to the sequence number in a block

following the GOTO statement occurs (the destination is the same as when both

bits are set to 0).

- 202 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

NOTE

When an external program is read and executed by DNC operation, the

executed sequence numbers are not stored.

When a program registered in memory is executed by a subprogram call, the

sequence numbers are stored.

CAUTION

According to the restrictions on the GOTO statement, no branch to a sequence

number within a DO-END loop cannot be made. If a program in which a branch

to a sequence number within a loop occurs is executed, operation may differ

depending on whether the GOTO statement using stored sequence numbers is

used.

14.6.3 Conditional Branch (IF Statement)

Specify a <conditional expression> after IF.

IF[<conditional expression>]GOTOn

If the specified <conditional expression> is satisfied (true), a branch to sequence 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 [#1 GT 10] GOTO 2 ;

If the condition

is not satisfied

Processing

If the condition is satisfied

N2 G00 G91 X10.0

;

:

IF[<conditional expression>]THEN

If the specified <conditional expression> is satisfied (true), a macro statement specified after THEN 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 ;

If the values of #1 and #2 are the same and those of #3 and #4 are also the same, 0 is assigned to #5.

IF[[#1 EQ #2] AND [#3 EQ #4]] THEN #5 = 0 ;

If the values of #1 and #2 are the same or those of #3 and #4 are the same, 0 is assigned to #5.

IF[[#1 EQ #2] OR [#3 EQ #4]] THEN #5 = 0 ;

Explanation

-

<Conditional expression>

<Conditional expressions> are divided into <simple conditional expressions> and <complex conditional

expressions>. In a <simple conditional expression>, a relational operator described in Table 14.5 (a) is

specified between two variables or between a variable and constant to be compared. An <expression>

can be used instead of a variable. With a <complex conditional expression>, an AND (logical AND),

OR (logical OR), or XOR (exclusive OR) operation is performed for the results (true or false) of multiple

<simple conditional expressions>.

- 203 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

-

Relational operators

Relational 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 equal sign (=) and

inequality sign (>, <) cannot be used as a relational operator.

Table 14.6 (a) Relational operators

Operator

Meaning

EQ

Equal to(=)

NE

Not equal to(≠)

GT

Greater than(>)

GE

Greater than or equal to(≥)

LT

Less than(<)

LE

Less than or equal to(≤)

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

14.6.4 Repetition (WHILE Statement)

Specify a conditional expression after WHILE. While the specified condition is satisfied, the program

from DO to END is executed. If the specified condition is not satisfied, program execution proceeds to

the block after END.

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

If the

If the

Processing

condition

condition

is not

is satisfied

satisfied

END m

;

:

Explanation

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, an alarm PS0126 occurs.

-

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), an alarm PS0124

occurs.

- 204 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

1. The identification numbers (1 to

3. DO loops can be nested to a

3) can be used as many times

maximum depth of three levels.

as required.

WHILE [ … ] DO 1 ;

WHILE [ … ] DO 1 ;

:

Processing

WHILE [ … ] DO 2 ;

:

END 1 ;

WHILE [ … ] DO 3 ;

:

WHILE [ … ] DO 1 ;

Processing

Processing

END 3 ;

:

END 1 ;

END 2 ;

:

:

2. DO ranges cannot

END 1 ;

overlap.

4. Control can be transferred

WHILE [ … ] DO 1 ;

to 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 ;

Limitation

-

Infinite loops

When DO m is specified without specifying the WHILE statement, an infinite loop ranging from DO to

END is produced.

-

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. Therefore, in the case of processing in the reverse direction, use the WHILE

statement for repetition to reduce processing time.

-

Undefined variable

In a conditional expression that uses EQ or NE, a <null> and zero have different effects. In other types

of conditional expressions, a <null> is regarded as zero.

- 205 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

Sample program

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

O0001;

#1=0;

#2=1;

WHILE[#2 LE 10] DO 1;

#1=#1+#2;

#2=#2+1;

END 1;

M30;

14.7 MACRO CALL

A macro program can be called using the following methods. The calling methods can roughly be divided

into two types: macro calls and subprogram calls.

A macro program can also be called during MDI operation in the same way.

Macro call

Simple call (G65)

Modal call (G66, G67)

Macro call using a G code

Macro call using an M code

Subprogram call

Subprogram call using an M code

Subprogram call using a T code

Subprogram call using a specific code

Limitation

-

Call nesting

Macro calls can be nested to a depth of up to five levels and subprogram calls can be nested to a depth of

up to ten levels; calls can be nested to a depth of up to 15 levels in total.

-

Differences between macro calls and subprogram calls

Macro call (G65, G66, Ggg, or Mmm) differs from subprogram call (M98, Mmm, or Ttt) as described

below.

• With a macro call, an argument (data passed to a macro) can be specified. A subprogram call does

not have this capability.

• If a macro call block contains another NC command (such as G01 X100.0 G65 Pp), an alarm

PS0127 occurs.

• If a subprogram call block contains another NC command (such as G01 X100.0 M98 Pp), the

subprogram is called after the command is executed.

• In any macro call block, the machine does not stop in the single block mode.

If a subprogram call block contains another NC command (such as G01 X100.0 M98 Pp), the

machine stops in the single block mode.

• With a macro call, the level of local variables changes. With a subprogram call, the level of local

variables does not change.

(See "Local variable levels" in Limitation of Subsection 14.6.1.)

- 206 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

14.7.1 Simple Call (G65)

When G65 is specified, the custom macro specified at address P is called. Data (argument) can be

passed to the custom macro program.

G65 P p L l

<argument-

P : Number of the program to call

specification> ;

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 G91 X#3 ;

M30 ;

N9 M99 ;

Explanation

-

Call

• After G65, specify at address P the program number of the custom macro to call.

• When a number of repetitions is required, specify a number from 1 to 999999999 after address L.

When L is omitted, 1 is assumed.

• By using argument specification, values are assigned to corresponding local variables.

-

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

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

• Addresses that need not be specified can be omitted. Local variables corresponding to an omitted

address are set to null.

• Addresses do not need to be specified alphabetically. They conform to word address format.

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

Argument specification I is always used for I, J, and K by setting bit 7 (IJK) of parameter No. 6008

to 1

Example

- When bit 7 (IJK) of parameter No. 6008 is 0, I_ J_ K_ means that I = #4, J = #5,

and K = #6 while K_ J_ I_ means K = #6, J = #8, and I= #10 because argument

specification II is used.

- When bit 7 (IJK) of parameter No. 6008 is 1, K_ J_ I_ means that I = #4, J = #5,

and K = #6, which is the same as with I_ J_ K_, because argument specification

I is used.

- 207 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/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

IK3

#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

• Subscripts of I, J, and K for indicating the order of argument specification are not written in the

actual program.

NOTE

When bit 7 (IJK) of parameter No. 6008 is 1, argument specification II cannot be

used.

Limitation

-

Format

G65 must be specified before any argument.

-

Mixture of argument specifications I and II

The CNC internally identifies argument specification I and argument 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.

-

Position of the decimal point

The units used for argument data passed without a decimal point correspond to the least input increment

of each address.

- 208 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

CAUTION

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.

M

When a value is specified with no decimal point, the number of decimal places is determined as follows.

Address

For a non-axis address

For an axis address

D, E, H, M, S, or T

0

Q or R

α ^{(NOTE 2)}

A, C, I, J, K, X, Y, or Z

α ^{(NOTE 2)}

β ^{(NOTE 3)}

B, U, V^{(NOTE 1)}, or W

0

β ^{(NOTE 3)}

Second auxiliary function

γ ^{(NOTE 4)}

Address

Metric input

Inch input

F (G93 mode)

3

F (G94 mode)

0

2

F (G95 mode)

2 ^{(NOTE 5)}

4 ^{(NOTE 5)}

NOTE

1 When V is used in a call using a specific address, the number of decimal places

is determined according to the setting for the reference axis.

2 α is determined according to the increment system for the reference axis (axis

specified with parameter No. 1031) as listed in the table in NOTE 4.

3 β is determined according to the increment system for the corresponding axis

address as listed in the following table.

Increment system

Linear axis (metric input)

Linear axis (inch input)

Rotation axis

IS-A

2

3

2

IS-B

3

4

3

IS-C

4

5

4

When bit 7 (IPR) of parameter No. 1004 is set to 1, the above values from which

1 is subtracted are used. When the increment system for an axis is IS-A,

however, the setting of bit 7 (IPR) of parameter No. 1004 is not effective.

When calculator-type decimal notation for each axis is used (bit 0 (ADX) of

parameter No. 3455 is set to 1), the number of decimal places is 0. When bit 7

(EAP) of parameter No. 3452 is set to 1, however, calculator-type decimal

notation is not effective and the number of decimal places is determined as listed

in the above table.

4

γ is determined according to the increment system for the reference axis (axis

specified with parameter No. 1031) as listed in the following table.

(When bit 7

(BDX) of parameter No. 3450 is set to 1, γ is also determined in the same way.)

AUP

AUP(3450#0) = 1

Increment system for

(No.3450#0)

AUX (No.3405#0) = 0

AUX (No.3405#0) = 1

the reference axis

= 0

Metric

Inch

Metric

Inch

IS-A

2

2

3

IS-B

0

3

3

4

IS-C

4

4

5

- 209 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

NOTE

5 When bit 1 (FR3) of parameter No. 1405 is 1, the values in the table need to be

incremented by 1.

6 When calculator-type decimal notation is used (bit 0 (DPI) of parameter No. 3401

is set to 1), the number of decimal places is 0.

T

When a value is specified with no decimal point, the number of decimal places is determined as follows.

Address

For a non-axis address

For an axis address

H, M, Q, S, or T

0

R

α ^{(NOTE 1)}

D

0/α ^{(NOTE 6)}

A, B, C, I, J, K, U, V, W, X, Y, or Z

α ^{(NOTE 1)}

β ^{(NOTE 2)}

Second auxiliary function

γ ^{(NOTE 3)}

Address

Metric input

Inch input

E, F (G98 mode)

0 ^{(NOTE 4)}

2 ^{(NOTE 4)}

E, F (G99 mode)

4

6

NOTE

1 α is determined according to the increment system for the reference axis (axis

specified with parameter No. 1031) as listed in the table in NOTE 2.

2 β is determined according to the increment system for the corresponding axis

address as listed in the following table.

Increment system

Linear axis (metric input)

Linear axis (inch input)

Rotation axis

IS-A

2

3

2

IS-B

3

4

3

IS-C

4

5

4

When bit 7 (IPR) of parameter No. 1004 is set to 1, the above values from which

1 is subtracted are used. When the increment system for an axis is IS-A,

however, the setting of bit 7 (IPR) of parameter No. 1004 is not effective.

When calculator-type decimal notation for each axis is used (bit 0 (ADX) of

parameter No. 3455 is set to 1), the number of decimal places is 0. When bit 7

(EAP) of parameter No. 3452 is set to 1, however, calculator-type decimal

notation is not effective and the number of decimal places is determined as listed

in the above table.

3 γ is determined according to the increment system for the reference axis (axis

specified with parameter No. 1031) as listed in the following table.

(When bit 7

(BDX) of parameter No. 3450 is set to 1, γ is also determined in the same way.)

AUP(3450#0) = 1

Increment system for

AUP (No.3450#0)

AUX (No.3405#0) = 0

AUX (No.3405#0) = 1

the reference axis

= 0

Metric

Inch

Metric

Inch

IS-A

2

2

3

IS-B

0

3

3

4

IS-C

4

4

5

- 210 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

NOTE

4 When bit 2 (FM3) of parameter No. 1404 is 1, the values in the table need to be

incremented by 3.

5 When calculator-type decimal notation is used (bit 0 (DPI) of parameter No. 3401

is set to 1), the number of decimal places is 0.

6 When bit 2 (DPD) of parameter No. 6019 is set to 0, the number of decimal places

is 0.

When bit 2 (DPD) of parameter No. 6019 is set to 1, the number of decimal places

is α.

-

Call nesting

Macro calls can be nested to a depth of up to five levels including simple calls (G65) and modal calls

(G66). Subprogram calls can be nested to a depth of up to 15 levels including macro calls.

A macro program can also be called during MDI operation in the same way.

-

Local variable levels

• Local variables from level 0 to 5 are provided for nesting.

• The level of the main program is 0.

• Each time a macro is called (with G65, G66, Ggg, or Mmm), the local variable level is incremented

by one. The values of the local variables at the previous level are saved in the CNC.

• 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

Macro

Macro

Macro

Macro

(level 0)

(level 1)

(level 2)

(level 3)

(level 4)

(level 5)

O0001 ;

O0002 ;

O0003 ;

O0004 ;

O0005 ;

O0006

:

:

:

:

:

:

#1=1 ;

:

:

:

:

:

G65 P2 A2 ;

G65 P3 A 3;

G65 P4 A4 ;

G65 P5 A5 ;

G65 P6 A6 ;

:

:

:

:

:

:

:

:

:

:

:

:

:

M30 ;

M99 ;

M99 ;

M99 ;

M99 ;

M99 ;

Local variables

(Level 1)

(Level 2)

(Level 3)

(Level 4)

(Level 5)

(level 0)

1

2

3

4

5

6

#1

#1

#1

#1

#1

#1

:

:

:

:

:

:

:

:

:

:

:

:

:

:

:

:

:

:

#33

#33

#33

#33

#33

#33

Common variables

and written to by macros at different levels

#100-, #500-

Variables that can be read from

Sample program (bolt hole circle)

M

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

programming.

To drill in the clockwise direction, specify a negative value for B.

- 211 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

H=2

H=3

H=1

H=4

B

B

A

Center (X,Y)

Radius I

-

Calling format

G65 P9100 Xx Yy Zz Rr Ff Ii Aa Bb Hh ;

X

:

X coordinate of the center of the circle

(absolute or incremental programming)

(#24)

Y

:

Y coordinate of the center of the circle

(absolute or incremental programming)

(#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)

-

Program calling a macro program

O0002 ;

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 ;

-

Macro program (called program)

O9100 ;

#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 ;

- 212 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Meaning of variables:

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

Sample program (Drill cycle)

T

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

-

Calling format

Zz

G65 P9100

Kk Ff ;

Ww

Z

:

Hole depth (absolute programming)

W

:

Hole depth (incremental programming)

K

:

Cutting amount per cycle

F

:

Cutting feedrate

-

Program calling a macro program

O0002 ;

G50 X100.0 Z200.0 ;

G00 X0 Z102.0 S1000 M03 ;

G65 P9100 Z50.0 K20.0 F0.3 ;

G00 X100.0 Z200.0 M05 ;

M30 ;

-

Macro program (called program)

O9100;

#1=0 ;

Clear the data for the depth of the current hole.

#2=0 ;

Clear the data for the depth of the preceding hole.

IF [#23 NE #0] GOTO 1 ;

If incremental programming, specifies the jump to N1.

IF [#26 EQ #0] GOTO 8 ;

If neither Z nor W is specified, an error occurs.

#23=#5002-#26 ;

Calculates the depth of a hole.

N1

#1=#1+#6 ;

Calculates the depth of the current hole.

IF [#1 LE #23] GOTO 2 ;

Determines whether the hole to be cut is too deep?

#1=#23 ;

Clamps at the depth of the current hole.

N2 G00 W-#2 ;

Moves the tool to the depth of the preceding hole at the cutting feedrate.

G01 W- [#1-#2] F#9 ;

Drills the hole.

G00 W#1 ;

Moves the tool to the drilling start point.

- 213 -

14.CUSTOM MACRO

PROGRAMMING

B-64304EN/02

IF [#1 GE #23] GOTO 9 ;

Checks whether drilling is completed.

#2=#1 ;

Stores the depth of the current hole.

GOTO 1 ;

N9 M99 ;

N8

#3000=1 (NOT Z OR W COMMAND) ;

Issues an alarm.

14.7.2 Modal Call: Call After the Move Command (G66)

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 is issued to cancel a modal call.

G66 P p L l <argument-specification> ; P : Number of the program to call

l

: 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 ;

Explanation

-

Call

• After G66, specify at address P a program number subject to a modal call.

• When a number of repetitions is required, a number from 1 to 999999999 can be specified at address

L.

• As with a simple call (G65), data passed to a macro program is specified in arguments.

• In the G66 mode, a macro can be called.

-

Cancellation

When a G67 code is specified, modal macro calls are no longer performed in subsequent blocks.

-

Call nesting

Macro calls can be nested to a depth of up to five levels including simple calls (G65) and modal calls

(G66). Subprogram calls can be nested to a depth of up to 15 levels including macro calls.

-

Modal call nesting

For a single modal call (when G66 is specified only once), each time the move command is executed, the

specified macro is called. When nested modal macro calls are specified, the macro at the next higher

level is called each time the move command for a macro call is executed.

Macros are called in reverse order in which they are specified. Each time G67 is issued, the macros are

canceled one by one in reverse order in which they are specified.

[Example]

G66 P9100 ;

O9100 ;

O9200 ;

X10.0 ;

(1-1)

Z50.0 ;

(2-1)

X60.0 ;

(3-1)

G66 P9200 ;

M99 ;

Y70.0 ;

(3-2)

X15.0 ;

(1-2)

M99;

G67 ;

Cancels P9200.

G67 ;

Cancels P9100.

X-25.0 ;

(1-3)

- 214 -

B-64304EN/02

PROGRAMMING

14.CUSTOM MACRO

Execution order of the above program (blocks not containing the move command omitted)

(1-1)

(1-2)

(1-3)

(2-1)

(3-1)

(3-2)

(2-1)

(2-1)

* No modal call is performed after (1-3) because the mode is not the macro call mode.

Limitation

• G66 and G67 blocks are specified in pairs in the same program. If a G67 code is specified not in

the G66 mode, an alarm PS1100 occurs. Bit 0 (G67) of parameter No. 6000 can be set to 1 to

specify that the alarm does not occur in this case.

• In a G66 block, no macros can be called. Local variables (arguments) are set, however.

• G66 needs to be specified before any arguments.

• No macros can be called in a block which contains a code such as a auxiliary function that does not

involve movement along an axis.

• Local variables (arguments) can only be set in G66 blocks. Note that local variables are not set

each time a modal call is performed.

NOTE

If M99 is specified in a block in which a call is performed, it is executed after the

call is performed.

Sample program

M

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: Positioning along the X-axis

Operation 1

Point I

and Y-axis

Operation 2: Rapid traverse to point R

Operation 2

Operation 4

Operation 3: Cutting feed to point Z

R

Point R

Operation 4: Rapid traverse to point R or I

Z=0

Operation 3

Point Z

Z

-

Calling format

G66 P9110 Zz Rr Ff Ll

;

Z

: Coordinates of position Z (absolute programming only)

(#26)

R

: Coordinates of position R (absolute programming only)

(#18)

F

: Cutting feedrate

(#9)

L

: Repetition count

-

Program that calls a macro program

O0001 ;

G28 G91 X0 Y0 Z0 ;

G92 X0 Y0 Z50.0 ;

G00 G90 X100.0 Y50.0 ;

- 215 -

Content      ..     6      7      8      9     ..