Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 412)

Spindles
Chapter 17
17-14
To function as a virtual C axis, the lathe spindle must have a precision
encoder that provides position data to the control. There can be only one
encoder marker per revolution of the spindle. When the virtual C axis
feature is activated, the control switches spindle operation from an
open-loop spindle to a closed-loop virtual C positioning axis.
CAUTION: It is the responsibility of the operator (or the
control’s PAL program) to change spindle gears as required to
attain one revolution of the encoder per revolution of the
spindle prior to execution of the G16.1.
While the virtual C axis feature is active, programmed spindle commands
(M03, M04, M05, or M19) do not affect the operation of the lathe spindle.
It is up to the control’s PAL program to interpret these part program
commands and take appropriate action, such as directing them to a “live
tool” spindle.
Typically a live tool powered by an external drive and mounted on the X
and Z axes is used to machine contours on the workpiece during virtual C
operation. Operation of the live tool is controlled through PAL.
The control uses the $VIRTC PAL flag to indicate to PAL that the virtual C
axis feature is active. Refer to the documentation prepared by your system
installer for details.
Virtual C Programming Restrictions
When the virtual C axis feature is enabled, these programming restrictions
apply:
The control must be in feedrate per minute mode (G94), not feedrate per
revolution mode, before beginning virtual C programming
Work coordinate system offsets (G52, G54--G59, and G92) for the park
and feed axes (Z and X) are temporarily cancelled when in G16.1 mode.
Offsets for other axes are not affected
Tool offsets and cutter compensation/TTRC offsets are allowed during
Virtual C programming
Cutter compensation ignores the tool orientation and treats the
programmed tool as a mill tool (orientation 0)
Activation of offsets through PAL is disabled
Jog on the fly is disabled
Integrand circle/arc programming is not permitted during G02/G03
blocks. Only direct radius (R) programming is allowed