Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 281)

Introduction to Programming
Chapter 10
10-13
M99 code acts as a return command in both sub- and main programs;
however, there are specific differences:
Using M99 in a Main Program
If you use M99
in a:
M99:
Main program executes all commands in the block, regardless if information
is programmed in the block to the right of the M99 command
clears all modal codes similar to an M02 or M30 (simulates
start-up conditions)
resets the current main program to the first block
automatically performs a cycle start on the program after it is
reset and program execution starts over.
Subprogram tells the control the end of a subprogram
will not merge any commands within a file that is used as a
subprogram and follows a M99 code in the main program into
the calling program.
Using M99 in a Subprogram
Program the M99 code anywhere in a program block, provided no axis
words are programmed to the left of M99. Any information (other than
axis words) programmed to the left of M99 is executed as part of the
subprogram, while information (including axis words) programmed in the
block to the right of the M99 command is ignored.
If you program: Then:
M99X10; X10 is ignored in this subprogram block
X10M99; X10 generates an error in this subprogram
M03M99; M03 is executed as normal in this subprogram
10.3.2
Main and Subprogram
Return (M99)