Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 366)

Coordinate Control
Chapter 13
13-14
Use the Scaling feature to reduce or enlarge a programmed shape. Enable
this feature by programming a G14.1 block as shown below:
G14.1 X__Y__Z__P__;
Where : Is :
X, Y, Z the axis or axes to be scaled and the center of scaling for those axes
P the scaling magnification factor for the specified axes.
The axes programmed in the G14.1 block determine which axes will be
scaled. The corresponding axis word values specify the center of scaling
for each axis. This position is the axis position around which the scaling
operation is performed.
The scaling magnification factor (P) is the amount of scaling to apply to
the programmed axes. Each scaled axis may have a different scale factor
by programming them in separate G14.1 blocks. The scaling range is from
0.00001 to 999.99999. A scale factor less than one will reduce a
programmed move while a scale factor greater than one will enlarge a
programmed move.
If no P word is programmed or if P0 is programmed in the G14.1 block,
the default magnification factor is used. If the programmed P word value
is out of range, an error message will be displayed on the CRT.
When absolute mode (G90) is active, scaling moves are referenced from
the programmed center of scaling.
Example 13.5
Scaling with Absolute Mode Active
Program
N01 G14.1 X6 Y6 P0.5;
N02 G90 X2 Y2 F100;
N03 X10;
N04 Y10;
N05 X2;
N06 Y2;
N07 M30;
13.5
Scaling