Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 766)

Program Interrupt
Chapter 29
29-8
The number of retrace blocks as set with this M code is the same for all
active or inactive interrupts. If an interrupt is enabled after this M code is
programmed it will take on the number of retrace blocks as programmed
with this M code.
When the return from interrupt is executed (M99 in the interrupt) the
control will generate a linear move to the end point of the last remembered
move for retrace. Then the moves are retraced returning the tool back to
the start point of the interrupt. Note this may not be the same location in
the main program if a different tool offset has been activated.
When you intend to use a program as an interrupt program, remember:
Any modal data (G codes, feedrates, spindle speeds, coordinate system
offsets, etc.) contained in the main program are carried into the interrupt
program. Any changes made to this modal data within the interrupt will
be effective only in the interrupt program; changes are not carried back
into the main program when the interrupt is completed. This does not
include tool or tool offset data that is changed in the interrupt. Any tool
or tool offset changes will be carried back into the suspended main part
program.
The system installer can determine if an interrupt program is to be
called as a paramacro when executed, or a subprogram when executed.
If it is to be called as a paramacro, remember that this assigns a new set
of local parameters for the interrupt. If it is to be called as a
subprogram, the same set of local parameters that applied to the
interrupted program apply to the subprogram.
If an interrupt is chosen as a macro program, it may not be a macro that
requires the assignment of local variables in the calling block (can not
require an argument).
Macro type interrupts are always called as the G65 non-modal type.
G66 and G66.1 modal types may not be called. Refer to the chapter on
paramacros for details on the G65 type macros.
The interrupt program must contain an M99 block. Any axis motion
commands that are to the left of the M99 code in the block will result as
an error. Other programming commands to the left of the M99 code in
the block will be executed. Any characters to the right of the M99 code
in the block are ignored.
29.4
The Interrupt Program