Content      ..     12      13      14      15     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 14

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

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. 14.10 (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

370

B-63534EN/02

PROGRAMMING

14. COMPENSATION FUNCTION

2.

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

commands in the following order (Fig.14.10(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. 14.10 (e) Scaling and coordinate system rotation

in cutter compensation C mode

371

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

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. 14.10 (f) Coordinate system rotation command

372

B-63534EN/02

PROGRAMMING

14. COMPENSATION FUNCTION

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

14.11

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. 14.11 (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. 14.11 (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.

373

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

Cutter center path

Cutter center path

Programmed path

Center of the arc

Programmed path

Fig. 14.11 (b) Normal direction control left (G41.1)

Fig. 14.11 (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. 14.11 (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. 14.11 (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.

374

B-63534EN/02

PROGRAMMING

14. COMPENSATION FUNCTION

Cutter center path

S

N1

S : Single block stop point

Programmed path

N2

S

N3

S

Fig. 14.11 (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. 14.11 (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.

375

B-63534EN/02

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.

377

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

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

14.12

to a programmed axis of symmetry (Fig. 14.12 (a)).

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. 14.12 (a) 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.

378

B-63534EN/02

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-4.9), 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.

379

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

14.13

The grinding wheel compensation function creates a compensation vector

by extending the line between the specified compensation center and the

GRINDING WHEEL

specified end point, on the specified compensation plane.

WEAR

COMPENSATION

Compensation vector

Programmed path

Compensation

center

Tool center path

Format

D Selecting the

G41 Pn (n=1, 2, 3);

compensation center

G41 P1; Select the first compensation center

G41 P2; Select the second compensation center

G41 P3; Select the third compensation center

D Start-up

D_; D code other than D0

D Canceling

D0;

compensation mode

G40;

D Holding the

compensation vector

Explanations

D Setting and selecting the

Three compensation centers can be specified by specifying their center

compensation center

coordinates with parameters No. 5081 to 5086. The G41Pn (n = 1, 2, or

3) command is used to specify which compensation center is to be used.

G41 P1 ;

Select the first compensation center.

G41 P2 ;

Select the second compensation center.

G41 P3 ;

Select the third compensation center.

When selecting the compensation center, specify P1, P2, or P3 at the same

time with G41. If G41 has been specified without a P command or with

a P command other than P1, P2, and P3, P/S alarm 5069 is issued.

When specifying the compensation center with parameters, use the

workpiece coordinates.

D Start-up

To enter compensation mode, specify the compensation center, then

specify a D code other than D0. A compensation vector is created and the

tool is accordingly moved, even if the block in which the D code has been

specified does not contain a move command.

380

B-63534EN/02

PROGRAMMING

14. COMPENSATION FUNCTION

A compensation vector is created by extending the line between the

D Compensation vector

compensation center and the specified end point. The length of the

compensation vector equals to the offset value corresponding to the offset

number specified with the D code.

When the offset value is positive, the compensation vector is added to the

specified end point. When the offset value is negative, the compensation

vector is subtracted from the specified end point.

+

Z

Compensation

vector (+)

Compensation

center

Programmed path

Tool center

path

Y+

Offset value (+)

Compensation

vector (-)

+

Z

Compensation

Programmed path

center

Tool center path

Y+

Offset value (-)

D Canceling compensation

Specifying D0 cancels compensation mode, thus disabling the creation of

mode

a compensation vector.

D Holding the

Specifying G40 selects a mode for holding the current compensation

compensation vector

vector. In this mode, the specified end point is shifted by the same vector

length until a different compensation mode is specified.

Specifying D0 in compensation vector hold mode clears the

compensation vector and cancels compensation mode.

381

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

D Circular and helical

Grinding wheel wear compensation can also be applied to circular

interpolation

interpolation and helical interpolation. If the radius at the start point

differs from that at the end point, the figure does not become an arc; it

becomes a helix.

Compensation vector

Arc center

Tool center path

Programmed path

Compensation center

The compensated values are still subject to arc radius error limit

(parameter No. 3410) check.

D Circular interpolation in

Specifying an arc command in G40 mode causes the arc center to be

G40 mode

shifted by the vector length, thus causing the figure to become an arc, not

a helix.

Programmed

arc center

Held vector

Tool center path

Programmed path

D Exponential interpolation

Grinding wheel wear compensation can also be applied to exponential

interpolation.

Exponential interpolation is performed for the

compensated positions.

D Compensation plane and

A compensation vector is created only on the plane (compensation plane)

plane selection using

corresponding to the axes specified with parameters No. 5071 and 5072

G17/G18/G19

(compensation axes).

In compensation mode (including compensation vector hold mode), a

compensation vector is always created on the compensation plane

specified with parameters (No. 5071 and 5072), regardless of the plane

selected with the G17, G18, or G19 command. For example,

compensation can be performed using the YZ plane as the compensation

plane while circular interpolation is performed on the XY plane (G17).

If a move command has been specified for either compensation axis, in

compensation mode, the compensation vector component of the other

axis may be changed during compensation vector creation, thus causing

the tool to also move along that axis.

382

B-63534EN/02

PROGRAMMING

14. COMPENSATION FUNCTION

(Example 1)

When the compensation axes are the Y- and Z-axes and

linear interpolation is performed for the X- and Y-axes

Programmed path: a → b, compensated path: a’ → b’

+

a’

Vay

+

a’

Vay

Y

Y

V_b

a

a

Va

Vaz

Compensation

b’

center

b’

V_by

V_by

b

b

V_bz

X+

Z+

Paths on the XY plane

Paths on the YZ plane

(Example 2)

When the compensation axes are the Y- and Z-axes and

circular interpolation is performed for the X- and Y-axes

Programmed path: a → b, compensated path: a’ → b’

+

a’

+

Vay

a’

Y

Y

V_b

a

Va

a

Vaz

Compensation

b’

center

b’

V_by

b

b

Arc center

V_bz

Z+

X+

Paths on the YZ plane

Paths on the XY plane

D Compensation cancel

Compensation cancel mode is selected immediately after power-on or

mode

reset.

D Changing the coordinate

Before attempting to change the coordinate system, cancel compensation

system

mode.

D Reference position

Before attempting to return to the reference point (G28 or G30), cancel

return (G28, G30)

compensation mode.

Limitations

D Changing the

The compensation axes can be changed only in compensation cancel

compensation axes

mode.

D Relationship with other

Cutter compensation and three-dimensional tool compensation cannot be

offset functions

used when grinding wheel wear compensation is enabled on the system.

The tool length offset and tool position offset functions can be used with

grinding wheel wear compensation.

D Relationship with the

The coordinates of the compensation center are not subject to

coordinate change

programmable mirror image, scaling, or coordinate rotation.

function

383

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

14.14

The rotary table dynamic fixture offset function saves the operator the

trouble of re-setting the workpiece coordinate system when the rotary

ROTARY TABLE

table rotates before cutting is started. With this function the operator

DYNAMIC FIXTURE

simply sets the position of a workpiece placed at a certain position on the

OFFSET

rotary table as a reference fixture offset. If the rotary table rotates, the

system automatically obtains a current fixture offset from the angular

displacement of the rotary table and creates a suitable workpiece

coordinate system. After the reference fixture offset is set, the workpiece

coordinate system is prepared dynamically, wherever the rotary table is

located.

The zero point of the workpiece coordinate system is obtained by adding

the fixture offset to the offset from the workpiece reference point.

Y

Y

Y

X

X

F₀

F

θ

θ₀

X

Rotation axis

center

C

Z

W

W

: Workpiece origin offset value

θ₀

: Reference angle

F₀

: Reference fixture offset value

Machine coordinate

θ

: Rotation axis angle

system origin

F

: Fixture offset value

Fig.14.14 (a) Fixture offset

Format

D Fixture offset command

G54.2 Pn ;

n : Reference fixture offset value number (1 to 8)

D Fixture offset cancel

command

G54.2 P0 ;

384

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

Y

F

X

W

C

W: Workpiece origin offset value

F: Fixture offset corresponding to the

reference angle

Set the data on the fixture offset screen (See III-11.4). Eight groups

of data items can be specified.

(3) Setting a parameter for enabling or disabling the fixture offset of each

axis (bit 0 (FAX) of parameter 7575)

For the axis for which the fixture offset is enabled, set the parameter

to 1. This need not be specified for a rotation axis.

(4) Setting the type of fixture offset (bit 1 (FTP) of parameter 6004)

Specify whether to cause a movement according to the increment or

decrement of the fixture offset vector when the vector changes (when

G54.2 is specified or when a rotation axis movement occurs in the

G54.2 mode).

When 0 is set, the movement is made. (The current position on the

workpiece coordinate system does not change. The position on the

machine coordinate system changes.)

When 1 is set, the movement is not made. (The current position on

the workpiece coordinate system changes. The position on the

machine coordinate system does not change.)

D Inputting and outputting

The setting of a program and external data can be input and output as

the fixture offset

described below :

(1) Setting the reference fixture offset by G10

G10 L21 Pn IP ;

n : Number of fixture offset

IP : Reference fixture offset or reference angle of each axis

This command sets the reference fixture offset or reference angle in

a program.

When the command is executed in the G90 mode, the specified value

is set directly.

When the command is executed in the G91 mode, the specified value

plus a value set before the execution is set.

386

B-63534EN/02

PROGRAMMING

14. COMPENSATION FUNCTION

NOTE

The programmable data input function (G10) is required.

(2) Reading and writing the data by a system variable of a custom macro

System variable number = 5500 + 20:n + m

The following system variable number can be used to read and write

the reference fixture offset or reference angle. No data can be written

in the system variable area (5500 to 5508) with n = 0, however.

n : Fixture offset number (1 to 8)

When n is 0, the current offset is indicated.

m : Axis number (1 to number of controlled axes)

System variable 5500 can be used to read the selected offset number.

NOTE

The custom macro function is required.

(3) Reading and writing the data by the PMC window or open CNC

The window function can be used to read and write the custom macro

system variable with the same number as for (2).

NOTE

The NC window function and custom macro function are

required.

(4) Outputting the data to an external device

By selecting <PUNCH> on the fixture offset screen, the data can be

output to a Floppy Cassette, memory card or other external device via

RS-232C.

The data is output in the G10 form without a program number.

NOTE

The reader/punch interface function and programmable

data input function (G10) are required.

(5) Input from an external device

Register the data output in step (4) into the CNC memory as a

program and execute the program to input the data.

NOTE

The reader/punch interface function and programmable

data input function (G10) are required.

387

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

D Calculating the Fixture

Offset

(1) Relationship between the rotation axis and linear axes

First group : 5(B-axis), 1(X-axis) , 3(Z-axis)

Second group

: 4(A-axis) , 3(Z-axis) , 2(Y-axis)

Third group

: 0, 0, 0

(2) Reference angle and reference fixture offset

X : F_0X

Y : F_0Y

Z : F_0Z

A : φ₀

B : θ₀

The calculation method is shown below when data is set as above:

O

: Rotary table center

W : Workpiece origin offset value

F₀

: Fixture offset value when A = φ₀ and B = θ₀

FA

: Fixture offset value when A = 0 and B = 0

F₁

: Fixture offset value when A = 0 and B = θ

F

: Fixture offset value when A = φ and B = θ

F₁

F

Z

O

X

FA

F₀

Y

A

FA =

(F_AX, F_AY, F_AY)

F₁ =

(F_1X, F_1Y, F_1Z)

F

=

(F_X, F_Y, F_Z)

Then, the following expression is used for fixture offset calculation.

F_AX +

* sin(* q₀)

0

0

F_0X

ȱcos(*q0)

0

ȳ

ȱ1

ȳȱ

ȳ

cos(f₀)

* sin(f₀)

F_0Y

F_AY +

0

1

0

0

ȧ

ȧ

ȧ

ȧ

F_AZ +

0

* cos(* q₀)

0

sin(f₀)

cos(f₀)

F_0Z

Ȳsin(*q0)

ȴȲ

ȴȲ

ȴ

F_1X +

F_0X

0

* sin(q)

ȱ

ȳ

ȱcos(q)

ȳ

F_1Y +

0

1

0

F_0Y

ȧ

ȧ

ȧ

F_1Z +

0

cos(q)

F_0Z

Ȳsin(q)

ȴȲ

ȴ

F_X +

0

0

ȱ

1

ȳȱ^F1X

ȳ

F_Y +

0

cos(* f)

* sin(* f₀)

F_1Y

ȧ

ȧ

ȧ

F_Z +

0

sin(* f)

cos(* f₀)

F_1Z

Ȳ

ȴȲ

ȴ

388

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

Example

Parameter

Parameter 7580=4 (C-axis)

Parameter 7581=1 (X-axis)

Parameter 7582=2 (Y-axis)

Parameter 7583 to 7588=0

Parameter 7575#0(X)=1 (The offset is valid for the X-axis.)

7575#0(Y)=1 (The offset is valid for the Y-axis.)

7570#0=0 (When bit 0 of parameter 7570 is set to 1, the values in

square brackets ([ ]) are calculated.)

Data of fixture offset 1 (n = 1)

C= 180.0 (reference angle)

X= -10.0

Y= 0.0

When these parameters and data are set, the machine operates as shown

below :

Table 14.14 Example of fixture offset

Coordinates

Position on the

Position on the

workpiece coordinate

machine coordinate

Fixture offset

system (ABSOLUTE)

system (MACHINE)

Program

X

Y

C

X

Y

C

X

Y

C

N1 G90 G00 X0 Y0 C90. ;

0.0

0.0

90.0

0.0

0.0

90.0

0.0

0.0

0.0

N2 G54.2 P1 ;

0.0

0.0

90.0

0.0

10.0

90.0

0.0

10.0

0.0

[0.0

-10.0

90.0]

[0.0

0.0

90.0]

[0.0

10.0

0.0]

N3 G01 X10. Y2. F100. ;

10.0

2.0

90.0

10.0

12.0

90.0

0.0

10.0

0.0

N4 G02 X2. Y10. R10. ;

2.0

10.0

90.0

2.0

20.0

90.0

0.0

10.0

0.0

N5 G01 X0 Y0 ;

0.0

0.0

90.0

0.0

10.0

90.0

0.0

10.0

0.0

:

The values enclosed in brackets ([ ]) apply when bit 0 (FTP) of parameter

No. 7570 is set to 1.

390

B-63534EN/02

PROGRAMMING

14. COMPENSATION FUNCTION

Y

C

C=90_

N4

C=180k

N5

N3

N2

[N3]

X

Zero POINT of the machine

coordinate system

Fig.14.14 (b) Example of fixture offset

When G54.2 P1 is specified in the N2 block, the fixture offset vector (0,

10.0) is calculated. The vector is handled in the same way as the offset

from the workpiece reference point. The current position on the

workpiece coordinate system is (0, -10.0).

If bit 0 (FTP) of parameter 7570 is set to 0, the tool is moved according

to the vector. The resultant position on the workpiece coordinate system

is (0, 0), the position before the command is specified.

391

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

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 ;

392

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

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

15.1

directly with a numeric value; examples are G100 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 - #149 (#199)

Common

Common variables can be shared among

#500 - #531 (#999)

variables

different macro programs. When the pow-

er is turned off, variables #100 to #149 are

initialized to null. Variables #500 to #531

hold data even when the power is turned

off. As an option, common variables #150

to #199 and #532 to #999 are also avail-

able. However, when these values are us-

ing.

#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.

NOTE

Common variables #150 to #199 and #532 to #999 are

optional.

393

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

D Range of variable values

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

ranges :

-10⁴⁷ to -10^-29

0

10^-29 to 10⁴⁷

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

is issued.

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 Common custom macro

For two-path control, macro variables are provided for each path. Some

variables for tow paths

common variables, however, can be used for both paths, by setting

(two-path control)

parameters No. 6036 and 6037 accordingly.

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.

When #1 = < vacant >

When #1 = 0

G90 X100 Y #1

G90 X100 Y #1

#

#

G90 X100

G90 X100 Y0

394

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

(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

(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

D Custom macro variables

With the two-path control, macro variables are provided for each path.

common to tool posts

Specifying parameter Nos. 6036 and 6037 allows some of the common

(two-path control)

variables to be used for all paths.

D Displaying variable

Values

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.

395

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

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

Variable

Function

number

#1000-#1015

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

#1032

ro. 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-#1115

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

#1132

PMC. 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.

For detailed information, refer to the connection manual

(B-63523EN-1).

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

also be used.

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

Compensation number

System variable

1

#10001 (#2001)

:

:

200

#10200 (#2200)

:

:

999

#10999

Table 15.2 (c) System variables for tool compensation memory B

Compensation

Geometry compensation

Wear compensation

number

1

#11001 (#2201)

#10001 (#2001)

:

:

:

200

#11200 (#2400)

#10200 (#2200)

:

:

:

#11999

#10999

999

397

15. CUSTOM MACRO

PROGRAMMING

B-63534EN/02

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

Cutter compensation

Tool length compensation (H)

(D)

Compensation

number

Geomet-

Wear

Geometric

Wear

ric com-

com-

compensation

compensation

pensation

pensation

1

#11001(#2201)

#10001(#2001)

#13001

#12001

:

:

:

:

:

200

#11201(#2400)

#10201(#2200)

:

:

:

:

:

999

#11999

#10999

#13999

#12999

D Macro alarms

Table 15.2 (e) 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.

398

PROGRAMMING

15. CUSTOM MACRO

B-63534EN/02

D Time information

Time information can be read and written.

Table 15.2 (f) System variables for time information

Variable

Function

number

#3001

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

increments at all times. When the power is turned on, the val-

ue of this variable is reset to 0. When 2147483648 millisec-

onds 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/min-

utes/seconds). Hours/minutes/seconds information is con-

verted to an apparent decimal number. For example, 34 min-

utes and 56 seconds after 3 p.m. is represented as 153456.

D Automatic operation

The control state of automatic operation can be changed.

control

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

Completion of an auxiliary

#3003

Single block

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.

399

Content      ..     12      13      14      15     ..