Content      ..     9      10      11      12     ..

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 11

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

Examples

D G39 without I, J, or K

X axis

(In offset mode)

N1 Y10.0 ;

N2 G39 ;

Y axis

N3 X-10.0 ;

Block N1

Offset vector

Block N2

(0.0, 10.0)

Block N3

Programmed path

Tool center path

(-10.0, 10.0)

D G39 with I, J, and K

X axis

(In offset mode)

N1 Y10.0 ;

N2 G39 I-1.0 J2.0 ;

Y axis

N3 X-10.0 Y20.0 ;

Block N2

Block N1

Offset vector

Block N3

Programmed

path

(0.0, 10.0)

(I=-1.0, J=2.0)

Tool center

path

(-10.0, 20.0)

283

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

Tool compensation values include tool geometry compensation

14.6

values and tool wear compensation (Fig. 14.6 (a)).

TOOL COMPENSA-

TION VALUES,

NUMBER OF

Reference position

COMPENSATION

ÇÇ

VALUES, AND

OFS_G

ÇÇ

ENTERING VALUES

ÇÇ

FROM THE

OFS_W

ÇÇ

OFS_G:Geometric compensation value

PROGRAM (G10)

OFS_W:Wear compensation value

Fig. 14.6 (a) Geometric compensation and wear compensation

Tool compensation values can be entered into CNC memory from the

CRT/MDI panel (see section III-11.4.1) or from a program.

A tool compensation value is selected from the CNC memory when the

corresponding code is specified after address H or D in a program.

The value is used for tool length compensation, cutter compensation, or

the tool offset.

Explanations

Table 14.6 (a) shows the valid input range of tool compensation values.

D Valid range of tool

compensation values

Table 14.6 (a) The valid input range of tool compensation value

Increment

Geometric compensation value

Wear compensation value

system

Metric input

Inch input

Metric input

Inch input

IS-B

"999.999 mm

"99.9999inch

"99.999 mm

"9.9999 inch

IS-C

"999.9999 mm

"99.99999inch

"99.9999 mm

"9.99999 inch

D Number of tool

The memory can hold 400 tool compensation value (option).

compensation values

Address D or H is used in the program. The address used depends on

and the addresses to be

which of the following functions is used: tool length compensation(see

specified

II-14.1), tool offset (see II-14.3), or cutter compensation C (see II-14.5).

The range of the number that comes after the address (D or H) : 0 to 400.

284

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Tool compensation

Tool compensation memory C can be used.

memory and the tool

The tool compensation values are as following that are entered (set) (Table

compensation value to

14.6 (b)).

be entered

Table 14.6 (b) Setting contents tool compensation memory

and tool compensation value

Tool compensation value

Tool compensation memory C

Tool geometry compensation value

set

for address D

Tool geometry compensation value

set

for address H

Tool wear compensation for value ad-

set

dress D

Tool wear compensation

set

value for address H

Format

The programming format depends on which tool compensation value is

used.

D Input of tool

compensation value by

Table 14.6 (c) Setting range of Tool compensation memory

programing

and Tool compensation value

Tool compensation value

Format

Geometry compensation value for H code

G10L10P_R_;

Geometry compensation value for D code

G10L12P_R_;

C

Wear compensation value for H code

G10L11P_R_;

Wear compensation value for D code

G10L13P_R_;

P : Number of tool compensation

R : Tool compensation value in the absolute command(G90) mode

Value to be added to the specified tool compensation value in the

incremental command(G91) mode (the sum is also a tool

compensation value.)

NOTE

To provide compatibility with the format of older CNC

programs, the system allows L1 to be specified instead of

L11.

285

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

A programmed figure can be magnified or reduced (scaling).

14.7

The dimensions specified with X_, Y_, and Z_ can each be scaled up or

SCALING

down with the same or different rates of magnification.

(G50, G51)

The magnification rate can be specified in the program.

Unless specified in the program, the magnification rate specified in the

parameter is applied.

Y

P₄

P

3

P₄’

P₃’

P₀

P₂’

P₁’

P₂

P₁

0

X

P₀:Scaling center

Fig. 14.7 (a) Scaling(P₁ P₂ P₃ P₄³P_1’P_2’P_3’P_4’)

Format

SCALING UP OR DOWN ALONG ALL AXES

AT THE SAME RATE OF MAGNIFICATION

Format

Meaning of command

G51X_Y_Z_P_ ; Scaling start

X_Y_Z _ : Absolute command for

center coordinate value

Scaling is effective.

of scaling

(Scaling mode)

P_

: Scaling magnification

G50 ;

Scaling cancel

Scaling up or down along each axes at a different

rate of magnification (mirror image)

Format

Meaning of command

G51_X_Y_Z_I_J_K_;Scaling start

X_Y_Z_ Absolute command for

center coordinate value

Scaling is effective.

of scaling

(Scaling mode)

I_J_K_ Scaling magnification for

X axis Y axis and Z axis

G50

Scaling cancel

respectively

WARNING

Specify G51 in a separate block. After the figure is enlarged

or reduced, specify G50 to cancel the scaling mode.

286

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

Explanations

D Scaling up or down

Least input increment of scaling magnification is: 0.001 or 0.00001 It is

along all axes at the

depended on parameter SCR (No. 5400#7) which value is selected. Then,

same rate of

set parameter SCLx (No.5401#0) that enables scaling for each axis. If

magnification

scaling P is not specified on the block of scaling (G51X_Y_Z_P_ ;), the

scaling magnification set to parameter (No. 5411) is applicable. If X,Y,Z

are omitted, the tool position where the G51 command was specified

serves as the scaling center.

D Scaling of each axis,

Each axis can be scaled by different magnifications. Also when a negative

programmable mirror

magnification is specified, a mirror image is applied. First of all, set a

image

parameter XSC (No. 5400#6) which validates each axis scaling (mirror

(negative magnification)

image).

Then, set parameter SCLx (No. 5401#0) to enable scaling along each axis.

Least input increment of scaling magnification of each axis (I, J, K) is

0.001 or 0.00001( set parameter SCR (No. 5400#7)).

Magnification is set to parameter 5421 within the range +0.00001 to

+9.99999 or +0.001 to +999.999

If a negative value is set, mirror image is effected.

If magnification I, J or K is not commanded, a magnification value set to

parameter (No. 5421) is effective. However, a value other than 0 must be

set to the parameter.

NOTE

Decimal point programming can not be used to specify the

rate of magnification (I, J, K).

a/b : Scaling magnification of X axis

c/d

: Scaling magnification of Y axis

0 : Scaling center

Y axis

Programmed figure

d

Scaled figure

c

0

X axis

a

b

Fig. 14.7 (b) Scaling of each axis

287

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Scaling of circular

Even if different magnifications are applie to each axis in circular

interpolation

interpolation, the tool will not trace an ellipse.

When different magnifications are applied to axes and a circular

interpolation is specified with radius R, it becomes as following figure

14.7 (c) (in the example shown below, a magnification of 2 is applied to

the X-component and a magnification of

1 is applied to the Y-

component.).

G90 G00 X0.0 Y100.0 ;

G51 X0.0 Y0.0 Z0.0 I2000 J1000;

G02 X100.0 Y0.0 R100.0 F500 ;

Above commands are equivalent to the following command:

G90 G00 X0.0 Y100.0 Z0.0 ;

G02 X200.0 Y0.0 R200.0 F500 ;

Magnification of radius R depends on I, or J whichever is larger.

Y

Scaled shape

X

(0,0)

(100.0)

(200.0)

Fig. 14.7 (c) Scaling for circular interpolation1

When different magnifications are applied to axes and a circular

interpolation is specified with I, J and K, it becomes as following figure

14.7 (d) (In the example shown below, a magnification of 2 is applied to

the X-component and a magnification of 1 is applied to the

Y-component.).

G90 G00 X0.0 Y0.0 ;

G51 X0.0 Y0.0 I2000 J1000;

G02 X100.0 Y0.0 I0.0 J-100.0 F500 ;

Above commands are equivalent to the following commands.

G90 G00 X0.0 Y100.0;

G02 X200.0 Y0.0 I0.0 J-100.0 F500 ;

In this case, the end point does not beet the radius, a linear section is

included.

Y

(200.0)

Scaled shape

(100.0)

(0,0)

(100.0)

(200.0)

X

Fig. 14.7 (d) Scaling for circular interpolation 2

288

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Tool compensation

This scaling is not applicable to cutter compensation values, tool length

offset values, and tool offset values (Fig. 14.7 (e)).

Programmed figure

Scaled figure

Cutter compensation values are not scaled.

Fig. 14.7 (e) Scaling during cutter compensation

D Invalid scaling

Scaling is not applicable to the Z-axis movement in case of the following

canned cycle.

⋅Cut-in value Q and retraction value d of peck drilling cycle (G83, G73).

⋅Fine boring cycle (G76)

⋅Shift value Q of X and Y axes in back boring cycle (G87).

In manual operation, the travel distance cannot be increased or decreased

using the scaling function.

D Commands related to

In scaling mode, G27, G28, G29, G30, or commands related to the

reference position return

coordinate system (G52 to G59, G92) must not be specified. When any

and coordinate system

of these G codes is necessary, specify it after canceling scaling mode.

WARNING

1

If a parameter setting value is employed as a scaling magnification without specifying P, the

setting value at G51 command time is employed as the scaling magnification, and a change

of this value, if any, is not effective.

2

Before specifying the G code for reference position return (G27, G28, G29, G30) or coordinate

system setting (G52 to G59, G92), cancel the scaling mode.

3

If scaling results are rounded by counting fractions of 5 and over as a unit and disregarding

the rest, the move amount may become zero. In this case, the block is!regarded as a no

movement block, and therefore, it may affect the tool movement by!cutter compensation C. See

the description of blocks that do not move the tool at II-14.5.3.

289

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

NOTE

1

The position display represents the coordinate value after scaling.

2

When a mirror image was applied to one axis of the specified plane, the following!results:

(1)Circular command Direction of rotation is reversed.

(2)Cutter compensation C .

Offset direction is reversed.

(3)Coordinate system rotation .

Rotation angle is reversed.

Examples

Example of a mirror image program

Subprogram

O9000 ;

G00 G90 X60.0 Y60.0;

G01 X100.0 F100;

G01 Y100.0;

G01 X60.0 Y60.0;

M99;

Main program

N10 G00 G90;

N20M98P9000;

N30 G51 X50.0 Y50.0 I-1000 J1000;

N40 M98 P9000;

N50 G51 X50.0 Y50.0 I-1000 J-1000;

N60 M98 P9000;

N70 G51 X50.0 Y50.0 I1000 J-1000

N80 M98 P9000;

N90 G50;

Y

100

60

50

40

X

0

40

50

60

100

Fig. 14.7 (f) Example of a mirror image program

290

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

A programmed shape can be rotated. By using this function it becomes

14.8

possible, for example, to modify a program using a rotation command

COORDINATE

when a workpiece has been placed with some angle rotated from the

SYSTEM ROTATION

programmed position on the machine.Further, when there is a pattern

comprising some identical shapes in the positions rotated from a shape,

(G68, G69)

the time required for programming and the length of the program can be

reduced by preparing a subprogram of the shape and calling it after

rotation.

Y

Angle of rotation

Center of rotation

X

0

Fig. 14.8 (a) Coordinate system rotation

Format

Format

G17

G18

G68 α_β_R_ ; Start rotation of a coordinate system.

G19

Coordinate system rotation mode

(The coordinate system is rotated.)

G69 ;

Coordinate system rotation cancel command

Meaning of command

G17 (G18 or G19)

: Select the plane in which contains the figure to be

rotated.

α_β_

Absolute command for two of the x_,y_,and Z_ axes

that correspond to the current plane selected by a

command (G17, G18, or G19). The command

specifies the coordinates of the center of rotation for

the values

specified subsequent to G68.

R_

Angular displacement with a positive value indicates

counter clockwise rotation. Bit 0 of parameter 5400

selects whether the specified angular displacement is

alwarys considered an absolute value or is considered

an absolute or incremental value depending on the

specified G code (G90 or G91).

Least input increment:

0.001 deg

Valid data range

:

-360,000 A360,000

291

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

X

Angle of rotation R (incremental value)

Center of

Angle of rotation (absolute value)

rotation

(α, β)

Z

Fig. 14.8 (b) Coordinate system rotation

NOTE

When a decimal fraction is used to specify angular

displacement (R_), the 1’s digit corresponds to degree

units.

Explanations

D G code for selecting a

The G code for selecting a plane (G17,G18,or G19) can be specified

plane: G17,G18 or G19

before the block containing the G code for coordinate system rotation

(G68). G17, G18 or G19 must not be designated in the mode of coordinate

system rotation.

D Incremental command in

The center of rotation for an incremental command programmed after

coordinate system

G68 but before an absolute command is the tool position when G68 was

rotation mode

programmed (Fig. 14.8 (c)).

D Center of rotation

When α_β_ is not programmed, the tool position when G68 was

programmed is assumed as the center of rotation.

D Angular displacement

When R_ is not specified, the value specified in parameter 5410 is

assumed as the angular displacement.

D Coordinate system

The G code used to cancel coordinate system rotation (G69) may be

rotation cancel

specified in a block in which another command is specified.

command

D Tool compensation

Cutter compensation, tool length compensation, tool offset, and other

compensation operations are executed after the coordinate system is

rotated.

292

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

Limitations

D Commands related to

In coordinate system rotation mode, G codes related to reference position

reference position return

return (G27, G28, G29, G30, etc.) and those for changing the coordinate

and the coordinate

system (G52 to G59, G92, etc.) must not be specified. If any of these G

system

codes is necessary, specify it only after canceling coordinate system

rotation mode.

The first move command after the coordinate system rotation cancel

D Incremental command

command (G69) must be specified with absolute values. If an incremental

move command is specified, correct movement will not be performed.

Explanations

Absolute/Incremental

position commands

N1 G92 X*500.0 Y*500.0 G69 G17 ;

N2 G68 X700.0 Y300.0 R60.0 ;

N3 G90 G01 X0 Y0 F200 ;

(G91X500.0Y500.0)

N4 G91 X1000.0 ;

N5 G02 Y1000.0 R1000.0 ;

N6 G03 X*1000.0 I*500.0 J*500.0 ;

N7 G01 Y*1000.0 ;

N8 G69 G90 X*500.0 Y*500.0 M02 ;

Tool path when the incremental

command is designated in the N3

block (in parenthesis)

Originally programmed tool path

Center of rotation

(700.0,300.0)

(0,0)

60_

(-500.0,-500.0)

Tool path after rotation

Fig. 14.8 (c) Absolute/incremental command during

coordinate system rotation

293

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

Examples

D Cutter compensation C

and coordinate system

It is possible to specify G68 and G69 in cutter compensation C mode.

rotation

The rotation plane must coincide with the plane of cutter compensa-

tion C.

N1 G92 X0 Y0 G69 G01 ;

N2 G42 G90 X1000 Y1000 F1000 D01 ;

N3 G68 R*30000 ;

N4 G91 X2000 ;

N5 G03 Y1000 R1000 J500 ;

N6 G01 X*2000 ;

N7 Y*1000 ;

Programmed shape before

N8 G69 G40 G90 X0 Y0 M30 ;

coordinate system rotation

Programmed shape

after coordinate

system rotation

30°

(0, 0)

Tool path

Fig. 14.8 (d) Cutter compensation C and coordinate system rotation

D Scaling and coordinate

If a coordinate system rotation command is executed in the scaling mode

system rotation

(G51 mode), the coordinate value (α,β,) of the rotation center will also be

scaled, but not the rotation angle (R). When a move command is issued,

the scaling is applied first and then the coordinates are rotated.

A coordinate system rotation command (G68) should not be issued in

cutter compensation C mode (G41, G42) on scaling mode (G51). The

coordinate system rotation command should always be specified prior to

setting the cutter compensation C mode.

1. When the system is not in cutter compensation mode C, specify the

commands in the following order :

G51 ; scaling mode start

G68 ; coordinate system rotation mode start

G69 ; coordinate system rotation mode cancel

G50 ; scaling mode cancel

294

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

2.

When the system is in cutter compensation model C, specify the

commands in the following order (Fig. 14.8 (e)) :

(cutter compensation C cancel)

G51 ; scaling mode start

G68 ; coordinate system rotation start

:

G41 ; cutter compensation C mode start

:

G92 X0 Y0 ;

G51 X300.0 Y150.0 P500 ;

G68 X200.0 Y100.0 R45.0 ;

G01 X400.0 Y100.0 ;

Y100.0 ;

X-200.0 ;

Y-100.0 ;

X200.0 ;

When scaling and coordinate

system rotation are applied

When only coordinate

Y

system rotation is applied

When only scaling

is applied

200.0

Cutting program

100.0

X

0

200.0

400.0

Fig. 14.8 (e) Scaling and coordinate system rotation

in cutter compensation C mode

295

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Repetitive commands for

It is possible to store one program as a subprogram and recall subprogram

coordinate system

by changing the angle.

rotation

Sample program for when the RIN bit (bit 0 of parameter 5400) is set

to 1.

The specified angular displancement is treated as an absolute or

incremental value depending on the specified G code (G90 or G91).

G92 X0 Y0 G69 G17;

G01 F200 H01 ;

M98 P2100 ;

M98 P072200 ;

G00 G90 X0 Y0 M30 ;

O 2200 G68 X0 Y0 G91 R45.0 ;

G90 M98 P2100 ;

M99 ;

O 2100 G90 G01 G42 X0 Y-10.0 ;

X4.142 ;

X7.071 Y-7.071 ;

G40 ;

M99 ;

Programmed path

(0, 0)

When offset is

applied

(0, -10.0)

Subprogram

Fig. 14.8 (f) Coordinate system rotation command

296

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

When a tool with a rotation axis (C-axis) is moved in the XY plane during

14.9

cutting, the normal direction control function can control the tool so that

NORMAL DIRECTION

the C-axis is always perpendicular to the tool path (Fig. 14.9 (a)).

CONTROL

(G40.1, G41.1, G42.1

OR G150, G151,

G152)

Programmed tool path

C-axis

C-axis

Tool

Tool

Normal direction (in

which the tool moves)

Fig. 14.9 (a) Sample Movement of the tool

Format

G code

Function

Explanation

If the workpiece is to the right of the

Normal direction

tool path looking toward the direc-

G41.1 or G151

control left

tion in which the tool advances,

the normal direction control left

(G41.1 or G151) function is speci-

fied.

Normal direction

After G41.1 (or G151) or G42.1 (or

G42.1 or G152

control right

G152) is specified, the normal

direction control function is en-

abled

(normal direction control

mode).

Normal direction

When G40.1 (or G150) is speci-

G40.1 or G150

control cancel

fied, the normal direction control

mode is canceled.

297

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

Cutter center path

Cutter center path

Programmed path

Center of the arc

Programmed path

Fig. 14.9 (b) Normal direction control left (G41.1)

Fig. 14.9 (c) Normal direction control right (G42.1)

Explanations

D Angle of the C axis

When viewed from the center of rotation around the C-axis, the angular

displacement about the C-axis is determined as shown in Fig. 14.9 (d).

The positive side of the X-axis is assumed to be 0 , the positive side of

the Y-axis is 90°, the negative side of the X-axis is 180°, and the negative

side of the Y-axis is 270°.

+Y

90°

+X

180°

0°

Center of rotation

270°

Fig. 14.9 (d) Angle of the C axis

D Normal direction control

When the cancel mode is switched to the normal direction control mode,

of the C axis

the C-axis becomes perpendicular to the tool path at the beginning of the

block containing G41.1 or G42.1.

In the interface between blocks in the normal direction control mode, a

command to move the tool is automatically inserted so that the C-axis

becomes perpendicular to the tool path at the beginning of each block.

The tool is first oriented so that the C-axis becomes perpendicular to the

tool path specified by the move command, then it is moved along the X-

and Y axes.

In the cutter compensation mode, the tool is oriented so that the C-axis

becomes perpendicular to the tool path created after compensation.

In single-block operation, the tool is not stopped between a command for

rotation of the tool and a command for movement along the X- and

Y-axes. A single-block stop always occurs after the tool is moved along

the X- and Y-axes.

298

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

Cutter center path

S

N1

S : Single block stop point

Programmed path

N2

S

N3

S

Fig. 14.9 (e) Point at which a Single-Block Stop Occurs

in the Normal Direction Control Mode

Before circular interpolation is started, the C-axis is rotated so that the

C-axis becomes normal to the arc at the start point. During circular

interpolation, the tool is controlled so that the C-axis is always

perpendicular to the tool path determined by circular interpolation.

The tool is controlled so that the C-

A rotation command is inserted

axis

so that the C-axis becomes nor-

is always normal to the tool path de-

mal to the arc at the start point.

termined by circular interpolation.

Tool center path

Center of the arc

Programmed path

Fig. 14.9 (f) Normal direction control of the circular interpolation

NOTE

During normal direction control, the C axis always rotates

through an angle less than 180 deg. I.e., it rotates in

whichever direction provides the shorter route.

299

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Movement for which arc

Specify the maximum distance for which machining is performed with

insertion is ignored

the same normal direction as that of the preceding block.

D Linear movement

When distance N2, shown below, is smaller than the set value,

machining for block N2 is performed using the same direction as that

for block N1.

Tool-center path

N2

N3

N1

Distance

Programmed path

D Circular movement

When the diameter of block N2, shown below, is smaller than the set

value, machining for block N2 is performed using the same normal

direction as that for block N1. The orientation of the axis to which

normal-direction control is applied, relative to the normal direction of

block N2, does not change as machining proceeds along the arc.

Tool-center path

N2

N3

Diameter

Programmed path

N1

NOTE

1

Do not specify any command to the C axis during normal

direction control. Any command specified at this time is

ignored.

2

Before processing starts, it is necessary to correlate the

workpiece coordinate of the C axis with the actual position

of the C axis on the machine using the coordinate system

setting (G92) or the like.

3

The helical cutting option is required to use this function.

Helical cutting cannot be specified in the normal direction

control mode.

4

Normal direction control cannot be performed by the G53

move command.

5

The C-axis must be a rotation axis.

301

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

A mirror image of a programmed command can be produced with respect

14.10

to a programmed axis of symmetry (Fig. 14.10).

PROGRAMMABLE

MIRROR IMAGE

Y

Axis of symmetry (X=50)

(2)

(1)

(G50.1, G51.1)

100

60

Axis of symmetry

50

(Y=50)

40

0

(3)

(4)

0

40

50

60

100

X

(1) Original image of a programmed command

(2) Image symmetrical about a line parallel to the Y-axis and crossing

the X-axis at 50

(3) Image symmetrical about point (50, 50)

(4) Image symmetrical about a line parallel to the X-axis and crossing

the Y-axis at 50

Fig. 14.10 Programmable Mirror image

Format

G51.1IP_ ; Setting a programmable image

A mirror image of a command specified in these

blocks is produced with respect to the axis of

symmetry specified by G51.1

IP

_;.

G50.1

_ ; Canceling a programmable mirror image

IP

IP_ : Point (position) and axis of symmetry for producing

a mirror image when specified with G51.1.

Axis of symmetry for producing a mirror image when

specified with G50.1. Point of symmetry is not speci-

fied.

302

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

Explanations

D Mirror image by setting

If the programmable mirror image function is specified when the

command for producing a mirror image is also selected by a CNC external

switch or CNC setting (see III-4.8), the programmable mirror image

function is executed first.

D Mirror image on a single

Applying a mirror image to one of the axes on a specified plane changes

axis in a specified plane

the following commands as follows :

Command

Explanation

Circular command

G02 and G03 are interchanged.

Cutter compensation

G41 and G42 are interchanged.

Coordinate rotation

CW and CCW (directions of rotation) are interchanged.

Limitations

D Scaling/coordinate

Processing proceeds from program mirror image to scaling and

system rotation

coordinate rotation in the stated order. The commands should be specified

in this order, and, for cancellation, in the reverse order. Do not specify

G50.1 or G51.1 during scaling or coordinate rotation mode.

D Commands related to

In programmable mirror image mode, G codes related to reference

reference position return

position return (G27, G28, G29, G30, etc.) and those for changing the

and coordinate system

coordinate system (G52 to G59, G92, etc.) must not be specified. If any

of these G codes is necessary, specify it only after canceling the

programmable mirror image mode.

303

15. CUSTOM MACRO

PROGRAMMING

B-64124EN/01

CUSTOM MACRO

15

Although subprograms are useful for repeating the same operation, the

custom macro function also allows use of variables, arithmetic and logic

operations, and conditional branches for easy development of general

programs such as pocketing and user-defined canned cycles.A machining

program can call a custom macro with a simple command, just like a

subprogram.

Machining program

Custom macro

O0001 ;

O9010 ;

:

#1=#18/2 ;

:

G01 G42 X#1 Y#1 F300 ;

:

G02 X#1 Y-#1 R#1 ;

G65 P9010 R50.0 L2 ;

:

:

:

:

:

M30 ;

M99 ;

304

B-64124EN/01

PROGRAMMING

15. CUSTOM MACRO

An ordinary machining program specifies a G code and the travel distance

15.1

directly with a numeric value; examples are G00 and X100.0.

VARIABLES

With a custom macro, numeric values can be specified directly or using

a variable number. When a variable number is used, the variable value

can be changed by a program or using operations on the MDI panel.

#1=#2+100 ;

G01 X#1 F300 ;

Explanation

D Variable representation

When specifying a variable, specify a number sign (#) followed by a

variable number. General-purpose programming languages allow a name

to be assigned to a variable, but this capability is not available for custom

macros.

Example: #1

An expression can be used to specify a variable number. In such a case,

the expression must be enclosed in brackets.

Example: #[#1+#2-12]

D Types of variables

Variables are classified into four types by variable number.

Table 15.1 Types of variables

Variable

Type of

Function

number

variable

#0

Always

This variable is always null. No value can

null

be assigned to this variable.

#1 - #33

Local

Local variables can only be used within a

variables

macro to hold data such as the results of

operations. When the power is turned off,

local variables are initialized to null. When

a macro is called, arguments are assigned

to local variables.

#100 - #199

Common

Common variables can be shared among

#500 - #999

variables

different macro programs. When the pow-

er is turned off, variables #100 to #199 are

initialized to null. Variables #500 to #999

hold data even when the power is turned

off.

#1000 -

System

System variables are used to read and

variables

write a variety of NC data items such as

the current position and tool compensation

values.

D Range of variable values

Local and common variables can have value 0 or a value in the following

ranges :

-10⁴⁷ to -10^-29

10^-29 to 10⁴⁷

If the result of calculation turns out to be invalid, an P/S alarm No. 111

is issued.

305

15. CUSTOM MACRO

PROGRAMMING

B-64124EN/01

D Omission of the decimal

When a variable value is defined in a program, the decimal point can be

point

omitted.

Example:

When #1=123; is defined, the actual value of variable #1 is 123.000.

To reference the value of a variable in a program, specify a word address

D Referencing variables

followed by the variable number. When an expression is used to specify

a variable, enclose the expression in brackets.

Example: G01X[#1+#2]F#3;

A referenced variable value is automatically rounded according to the

least input increment of the address.

Example:

When G00X#1; is executed on a 1/1000-mm CNC with 12.3456

assigned to variable

#1, the actual command is interpreted as

G00X12.346;.

To reverse the sign of a referenced variable value, prefix a minus sign (-)

to #.

Example: G00X-#1;

When an undefined variable is referenced, the variable is ignored up to an

address word.

Example:

When the value of variable #1 is 0, and the value of variable #2 is null,

execution of G00X#1Y#2; results in G00X0;.

D Undefined variable

When the value of a variable is not defined, such a variable is referred to

as a “null” variable. Variable #0 is always a null variable. It cannot be

written to, but it can be read.

(a) Quotation

When an undefined variable is quotated, the address itself is also

ignored.

[Example] When #1 is 0 and #2 is null, the result of executing G00

X#1 Y#2; will be the same as when G00 X0; is executed.

(b) Operation

< vacant > is the same as 0 except when replaced by < vacant>

When #1 = < vacant >

When #1 = 0

#2 = #1

#2 = #1

#

#

#2 = < vacant >

#2 = 0

#2 = #1*5

#2 = #1*5

#

#

#2 = 0

#2 = 0

#2 = #1+#1

#2 = #1 + #1

#

#

#2 = 0

#2 = 0

306

B-64124EN/01

PROGRAMMING

15. CUSTOM MACRO

(c) Conditional expressions

< vacant > differs from 0 only for EQ and NE.

When #1 = < vacant >

When #1 = 0

#1 EQ #0

#1 EQ #0

#

#

Established

Not established

#1 NE 0

#1 NE 0

#

#

Established

Not established

#1 GE #0

#1 GE #0

#

#

Established

Established

#1 GT 0

#1 GT 0

#

#

Not established

Not established

VARIABLE

O1234 N12345

NO.

DATA

NO.

DATA

100

123.456

108

101

0.000

109

102

110

103

111

104

112

105

113

106

114

107

115

ACTUAL POSITION (RELATIVE)

X

0.000

Y

0.000

Z

0.000

B

0.000

MEM **** *** ***

18:42:15

[ MACRO ] [ MENU ] [ OPR

] [

] [ (OPRT) ]

D When the value of a variable is blank, the variable is null.

D The mark ******** indicates an overflow (when the absolute

value of a variable is greater than 99999999) or an underflow (when

the absolute value of a variable is less than 0.0000001).

Limitations

Program numbers, sequence numbers, and optional block skip numbers

cannot be referenced using variables.

Example:

Variables cannot be used in the following ways:

O#1;

/#2G00X100.0;

N#3Y200.0;

307

15. CUSTOM MACRO

PROGRAMMING

B-64124EN/01

15.2

System variables can be used to read and write internal NC data such as

tool compensation values and current position data. Note, however, that

SYSTEM VARIABLES

some system variables can only be read. System variables are essential

for automation and general-purpose program development.

Explanations

D Interface signals

Signals can be exchanged between the programmable machine controller

(PMC) and custom macros.

Table 15.2 (a) System variables for interface signals

(When the parameter MIF (bit 0 of No. 6001) is set to 0.)

Variable

Function

number

#1000 to #1015

A 16-bit signal can be sent from the PMC to a custom macro.

#1032

Variables #1000 to #1015 are used to read a signal bit by bit.

Variable #1032 is used to read all 16 bits of a signal at one

time.

#1100 to #1115

A 16-bit signal can be sent from a custom macro to the PMC.

#1132

Variables #1100 to #1115 are used to write a signal bit by bit.

Variable #1132 is used to write all 16 bits of a signal at one

time.

#1133

Variable #1133 is used to write all 32 bits of a signal at one

time from a custom macro to the PMC. Note, that values from

-99999999 to +99999999 can be used for #1133.

(When the parameter MIF (bit 0 of No. 6001) is set to 1.)

Variable

Function

number

#1000 to #1031

A 32-bit signal can be sent from the PMC to a custom macro.

Variables #1000 to #1031 are used to read a signal bit by bit.

#1100 to #1131

A 32-bit signal can be sent from a custom macro to the PMC.

Variables #1100 to #1131 are used to write a signal bit by bit.

#1032 to #1035

Variables #1032 to #1035 are used to output all 32 bits of a

signal at one time from the PMC to a custom macro. Note,

that values from -99999999 to +99999999 can be used for

#1032 to #1035.

#1132 to #1135

Variables #1132 to #1135 are used to write all 32 bits of a sig-

nal at one time from a custom macro to the PMC. Note, that

values from -99999999 to +99999999 can be used for

#1132 to #1135.

For detailed information, refer to the connection manual (B-64113EN-1).

308

B-64124EN/01

PROGRAMMING

15. CUSTOM MACRO

D Tool compensation

Tool compensation values can be read and written using system variables.

values

Usable variable numbers depend on the number of compensation pairs,

whether a distinction is made between geometric compensation and wear

compensation, and whether a distinction is made between tool length

compensation and cutter compensation. When the number of

compensation is not greater than 200, variables #2001 to #2400 can also

be used.

Table 15.2 (b) System variables for tool compensation memory C

Tool length compensation (H)

Cutter compensation

(D)

Compensation

number

Geometric

Wear

Geomet-

Wear

compensation

compensation

ric com-

com-

pensation

pensation

1

#11001(#2201)

#10001(#2001)

#13001

#12001

:

:

:

:

:

200

#11201(#2400)

#10201(#2200)

:

:

:

:

:

400

#11400

#10400

#13400

#12400

D Macro alarms

Table 15.2 (c) System variable for macro alarms

Variable

Function

number

#3000

When a value from 0 to 200 is assigned to variable #3000,

the CNC stops with an alarm. After an expression, an alarm

message not longer than 26 characters can be described.

The CRT screen displays alarm numbers by adding 3000 to

the value in variable #3000 along with an alarm message.

Example:

#3000=1(TOOL NOT FOUND);

→ The alarm screen displays “3001 TOOL NOT FOUND.”

D Stop with a message

Execution of the program can be stopped, and then a message can be

displayed.

Variable

Function

number

#3006

When “#3006=1 (MESSAGE);” is commanded in the macro,

the program executes blocks up to the immediately previous

one and then stops.

When a message of up to 26 characters, which is enclosed

by a control-in character (“(”) and control-out character (“)”),

is programmed in the same block, the message is displayed

on the external operator message screen.

309

15. CUSTOM MACRO

PROGRAMMING

B-64124EN/01

D Time information

Time information can be read and written.

Table 15.2 (d) System variables for time information

Variable

Function

number

#3001

This variable functions as a timer that counts in 1-millisecond in-

crements at all times. When the power is turned on, the value of

this variable is reset to 0. When 2147483648 milliseconds is

reached, the value of this timer returns to 0.

#3002

This variable functions as a timer that counts in 1-hour incre-

ments when the cycle start lamp is on. This timer preserves its

value even when the power is turned off. When 9544.371767

hours is reached, the value of this timer returns to 0.

#3011

This variable can be used to read the current date (year/month/

day). Year/month/day information is converted to an apparent

decimal number. For example, September 28, 2001 is repre-

sented as 20010928.

#3012

This variable can be used to read the current time (hours/minutes/

seconds). Hours/minutes/seconds information is converted to an

apparent decimal number. For example, 34 minutes and 56 se-

conds after 3 p.m. is represented as 153456.

D Automatic operation

The control state of automatic operation can be changed.

control

Table 15.2 (e) System variable (#3003) for automatic operation control

#3003

Single block

Completion of an auxiliary

function

0

Enabled

To be awaited

1

Disabled

To be awaited

2

Enabled

Not to be awaited

3

Disabled

Not to be awaited

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

S When single block stop is disabled, single block stop operation is not

performed even if the single block switch is set to ON.

S When a wait for the completion of auxiliary functions (M, S, and T

functions) is not specified, program execution proceeds to the next

block before completion of auxiliary functions. Also, distribution

completion signal DEN is not output.

310

B-64124EN/01

PROGRAMMING

15. CUSTOM MACRO

Table 15.2 (f) 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 Example of using variable #3004 in a tapping cycle

311

15. CUSTOM MACRO

PROGRAMMING

B-64124EN/01

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-4.6)

The value obtained in binary is converted into decimal notation.

#3007

#7

#6

#5

#4

#3

#2

#1

#0

Setting

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.

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 (g) 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)

312

Content      ..     9      10      11      12     ..