Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 371)

Coordinate Control
Chapter 13
13-19
Important: If an axis is configured as a rotary axis, the scaling
magnification display screen will display dashes instead of numbers for
that axis. Rotary axes cannot be scaled.
The left column lists the current center of scaling for each axis. When
scaling is cancelled, the current center of scaling for each axis is set to
zero. The format of this value is determined by the word format of the
selected axis.
The middle column lists the currently active scaling magnification value
for each axis. When scaling is cancelled, the current scaling magnification
value for each axis is set to 1.00000.
The right column lists the current scaling magnification default value for
each axis. This value is used if P is not programmed or if P0 is
programmed in the G14.1 block. The range of the default value is 0.00001
to 999.99999 with a word format of 3.5. The default values are stored in
RAM or flash memory when the control is powered down. When the
control is powered up, these values are restored.
3. Use the up or down cursor keys to move the block cursor to the
default value to be changed. The selected default value will be
shown in reverse video.
4. To replace stored default scaling magnification value, key-in the new
default value and press the {REPLCE VALUE} softkey.
While scaling is enabled, these restrictions apply:
Scaling affects only programmed axis motion. All manual axis motions
and PAL axis mover motions are performed at full scale
Scaling does not affect M, F, S, T, and B word functions. The F word
will be scaled if the control is in inverse time mode (G93). Scaling
while in inverse time mode will be applied as follows:
Programmed F word
Scaled F word (when in G93 mode) = ----------------------
Largest Scale Factor
Scaling is disabled during G27, G28, and G30 automatic home
operations. For a G29 automatic return from home operation, scaling is
re-enabled after the intermediate point is reached
When changing work coordinates (G54-G59.3), the center of scaling is
transferred from the old work coordinate system to the new work
coordinate system. The offset distance from the tool position in the old
work coordinate system to the tool position in the new work coordinate
system is not scaled
13.5.3
Scaling Restrictions