Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 738)

Program Interrupt
Chapter 29
29-8
You can alter the number of blocks that the control re-executes in reverse
when returning to the start position of the interrupt. The number of return
blocks is normally 4; however, it can be altered by these codes:
M-code: Number of
Blocks Retraced:
M900 zero
M901 one
M902 two
M903 three
M904 four
These M-codes can be programmed in any block in the main program
before the interrupt program is executed. They can also be programmed
within an interrupt though the M-code will not go into effect until
execution is returned to the main program. If not programmed, the default
is 4 blocks. The default is automatically reset at the end of program
commands (M02 or M30).
The number of retrace blocks 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 takes 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 generates a linear move to the end point of the last remembered
move for retrace. Then the moves are retraced, returning the tool to the
start point of the interrupt. 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.
29.4
The Interrupt Program