Rockwell Automation 8520-GUM 9/Series CNC Grinder Operation and Programming Manual Documentation Set - Manual (Page 693)

Paramacros
Chapter 20
20-49
You can use a paramacro call to call any program that has a program name
of up to 5 numeric digits following the letter O (see page 10-8 for details
on program names). This program must also contain an M99 end of
subprogram or macro code somewhere in the program before an M02 or
M30 is read. This M99 code causes control to return to the main program
or restarts the paramacro if it executes more than one time.
The control first searches the main program directory for the program
called by the paramacro. If the control does not find the program in the
main program directory, it then checks the protectable program directory
for the program. If programs in the main and protectable directories have
the same name, the control uses the program in the main directory.
Important: The M99 code can be programmed anywhere in a paramacro
program block provided no axis words are programmed to the left of the
M99. Any information (other than axis words) programmed to the left of
M99 is executed as part of the paramacro. Any information (including axis
words) programmed in the block to the right of the M99 command is
ignored.
M99X10; X10 is ignored
X10M99; Error is generated
M03M99; M03 is executed
After the macro has been executed the specified number of times (as
specified by the L word), execution is returned to the block following the
paramacro call in the calling program.
ATTENTION: Any edits that are made to a subprogram, or to a
paramacro program that has already been called for automatic
execution, are ignored until the calling program is disabled and
reactivated (see page 7-7). Subprograms and paramacros are
called for automatic execution the instant that the calling
program is selected as active (see page 7-8).