Content .. 51 52 53 54 ..

FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 53

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 380 -

NOTE

This function is available when the G-code system
B or C is set.

CAUTION

1 Specify G51 in a separate block.
2 After the figure is enlarged or reduced, specify G50

to cancel the scaling mode.

NOTE

1 Entering electronic calculator decimal point input

mode (bit 0 (DPI) of parameter No. 3401 = 1) does
not cause the units of the magnification rates P, I, J,
and K to change.

2 Setting the least input increment equal to 10 times

the least command increment (bit 7 (IPR) of
parameter No. 1004 = 1) does not cause the units
of the magnification rates P, I, J, and K to change.

3 An attempt to specify 0 as a magnification rate

causes alarm PS0142 to occur in a G51 block.

Explanation
- Axis for which scaling is to be enabled

For the axis for which scaling is to be enabled, set bit 0 (SCL) of
parameter No. 5401 to 1.

- Minimum unit of scaling magnification

Least input increment of scaling magnification is: 0.001 or 0.00001.
It is 0.00001 (one hundred thousandth) if bit 7 (SCR) of parameter No.
5400 is 0 and 0.001 if it is 1.

- Scaling center

Even in incremental command (G91) mode, the scaling center
coordinates IP_ specified in the G51 block are assumed those of an
absolute position.
If the scaling center coordinates are omitted, the position assumed
when G51 is specified is assumed the scaling center.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 381 -

CAUTION

With the move command subsequent to the G51
block, execute an absolute (G90 mode) position
command.

If no absolute position command is executed after
the G51 block, the position assumed when G51 is
specified is assumed the scaling center; once an
absolute position command is executed, the scaling
center assumes the coordinates specified in the
G51 block, after that block.

- Scaling along each axis at the same rate of magnification

Set bit 6 (XSC) of parameter No. 5400 to 0.
If the scaling magnification P is not specified, the magnification set in
parameter No. 5411 is used.
Decimal point input is not accepted as the magnification P. If decimal
point input is made, alarm PS0007 will occur.
A negative value cannot be specified as the magnification P. If a
negative value is specified, alarm PS0006 will occur.
The allowable magnification range is from 0.00001 to 9999.99999.

- Scaling of each axis, programmable mirror image (negative magnification)

Each axis can be scaled by different  magnifications. Also when a
negative magnification is specified, a mirror image is applied.    The
axis subject to the mirror image is the one that contains the scaling
center.
Set bit 6 (XSC) of parameter No. 5400to 1 to validate each axis
scaling (mirror image).
Using I, J, and K, specify the scaling magnifications for the basic 3
axes (X to Z axes).    Use parameter No. 1022 to specify which axes to
use as the basic 3 axes.    For those of the X to Z axes for which I, J,
and K are not specified and for axes other than the basic 3 axes, the
magnification set with parameter No. 5421 is used.
A value other than 0 must be set to parameter No. 5421.
Decimal point programming can not be used to specify the rate of
magnification (I, J, K).
Magnification can be set within the range of

0.00001 to

9999.99999.

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 382 -

Y axis

X axis

a/b

: Scaling magnification of X axis

c/d

: Scaling magnification of Y axis

o : Scaling center

Programmed figure

Scaled figure

Fig. 15.2 (b) Scaling of each axis

CAUTION

Specifying the following commands at the same
time causes them to be executed in the order
indicated below:
<1> Programmable mirror image (G51.1)
<2> Scaling (G51) (including a mirror image with a

negative magnification)

<3> Mirror image due to the external switch of the

CNC or the settings of the CNC

In this case, the programmable mirror image is
effective to the scaling center and magnification as
well.

To specify G51.1 and G51 at the same time,
specify them in this order; to cancel them, specify
them in the reverse order.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 383 -

- Scaling of circular interpolation

Even if different magnifications are applied to each axis in circular
interpolation, the tool will not trace an ellipse.

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

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

(A magnification of 2 is applied to the X-component and a
magnification of 1 is applied to the Y-component.)

G02 X100.0 Y0.0 I0 J–100.0 F500;

Above commands are equivalent to the following command:

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

G02 X200.0 Y0.0 I0 J–100.0 F500;

(Because the end point is not on an arc, spiral interpolation is
assumed.)

(0,0)

(100.0)

(200.0)

Scaled shape

Fig. 15.2 (c) Scaling for circular interpolation1

Even for an R-specified arc, scaling is applied to each of I, J, and K
after the radius value (R) is converted into a vector in the center
direction of each axis.
If, therefore, the above G02 block contains the following R-specified
arc, the operation will be same as that in which I and J are specified.

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

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 384 -

- Scaling and coordinate system rotation

If both scaling and coordinate system rotation are specified at the
same time, scaling is performed first, followed by coordinate system
rotation. In this case, scaling is effective to the rotation center as
well.
To specify both of them, specify scaling first and then coordinate
system rotation. To cancel them, specify them in the reverse order.

Example
Main program
O1

G90 G00 X20.0 Y10.0 ;

M98 P1000 ;

G51 X20.0 Y10.0 I3000 J2000 ; (x 3 in the X direction and x 2

in the Y direction)

M98 P1000 ;

G17 G68 X35.0 Y20.0 R30. ;

M98 P1000 ;

G69

;

G50

;

M30

;

Subprogram
O1000

;

G01 X20.0 Y10.0 F500 ;

G01 X50.0 ;

G01 Y30.0 ;

G01 X20.0 ;

G01 Y10.0 ;

M99

;

Scaling center

Original program

Shape after
coordinate system

rotation

Scaled shape

Rotation center of
coordinate system

after scaling

Rotation center
of coordinate
system before
scaling

Fig. 15.2 (d) Scaling and coordinate system rotation

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 385 -

- Scaling and optional chamfering/corner R

Chamfering

Scaling
x 2 in the X direction

x 1 in the Y direction

Corner R

If different magnifications are applied to the individual axes, corner R results in
a spiral, not an arc, because scaling is applied to the end point and radius of
the arc.

Scaling
x 2 in the X direction

x 1 in the Y direction

Fig. 15.2 (e) Scaling and optional chamfering/corner R

Limitation
- Tool compensation

This scaling is not applicable to tool radius

⋅

tool nose radius

compensation values, tool length compensation values, and tool offset
values (Fig. 15.2 (f) ).

Cutter compensation values are not scaled.

Programmed figure

Scaled figure

Fig. 15.2 (f) Scaling during cutter compensation

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 386 -

- Invalid scaling

Scaling is not applied to the travel distance during canned cycle
shown below.

•

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.

This function is available to G code systems B and C only; it is not
available to G code system A.
During scaling, the following functions cannot be used. If any of
them is specified, alarm PS0300 will occur.

•

Finishing cycle (G70, G72)

•

Outer surface rough cutting cycle (G71, G73)

•

End rough cutting cycle (G72, G74)

•

Closed loop cutting cycle (G73, G75)

•

End cutting off cycle (G74, G76)

•

Outer/inner surface cutting off cycle (G75, G77)

•

Multiple threading cycle (G76, G78)

•

Traverse grinding cycle (for grinding machines) (G71, G72)

•

Traverse direct constant-size grinding cycle (for grinding

machines) (G72, G73)

•

Oscillation grinding cycle (for grinding machines) (G73, G74)

•

Oscillation direct constant-size grinding cycle (for grinding

machines) (G74, G75)

•

Face drilling cycle (G83, G83)

•

Face tapping cycle (G84, G84)

•

Face boring cycle (G85, G85)

•

Side drilling cycle (G87, G87)

•

Side tapping cycle (G88, G88)

•

Side boring cycle (G89, G89)

•

Outer/inner surface turning cycle (G77, G20)

•

Threading cycle (G78, G21)

•

End turning cycle (G79, G24)

(The G code in system B is given first, followed by that of system C.)

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

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 387 -

CAUTION

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, etc.) or coordinate
system setting (G52 to G59, G92, etc.), 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. See the description of cutter
compensation.

4 Refrain from scaling on a rotation axis for which the

rollover function is enabled. Otherwise, the tool
may rotate in a short-cut manner, possibly resulting
in unexpected movement.

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) Tool radius

⋅

tool nose radius compensation

................................ Offset direction is reversed.

(3) Coordinate system rotation

................................. Rotation angle is reversed.

Content .. 51 52 53 54 ..