Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 308)

Introduction to Programming
Chapter 10
10-34
End of Program, Tape Rewind (M30)
If executing a program from control memory the M30 code acts the same
as an M02, program execution is stopped and the control enters the cycle
stop state. The program is reset to the first block and a <CYCLE START>
will begin part program execution over again (see M99 for auto cycle
start).
If executing a program from an external device (such as a tape reader),
when M30 is executed, program execution is stopped and the tape is
automatically rewound to the beginning of the program just executed.
After the tape is rewound the control is enters the cycle stop state. A
<CYCLE START> will begin part program execution over again (see M99
for auto cycle start).
With some machines, the M30 code may also result in a spindle and
coolant supply stop. For details, refer to the instruction manual prepared by
the system installer.
Overrides Enabled (M48)
When M48 is executed, the feedrate override, rapid feedrate override, and
the spindle speed override functions become effective. Normally these
will be enabled on power up without requiring this M--code to be executed.
An M48 cancels an M49 and the system installer can choose which will be
active upon power-up.
Overrides Disabled (M49)
Use the override cancel M--code (M49) to ignore any override set by the
operator on the MTB panel. When the override setting is ignored, the axis
feedrate, rapid feedrate, and the spindle speed override values are all set to
100 percent. An M49 cancels an M48 and the system installer can choose
which will be active upon power-up. This override setting is ignored if
you are using programmed motion.
Subprogram call (M98)
When M98 is executed, a subprogram is called and executed. This word
may be used in any program including an MDI program. For details on
programming an M98, refer to section 10.3.1.