Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 299)

Introduction to Programming
Chapter 10
10-31
(5) Overrides Enabled (M48)
When your execute M48, the feedrate override, rapid feedrate override,
and the spindle speed override functions become effective. These are
enabled on power up without requiring this M code to be executed. An
M48 cancels an M49 and your system installer can choose which is active
upon power-up.
(6) Overrides Disabled (M49)
Use the override cancel M--code (M49) to ignore any override set by the
operator on the MTB panel. When you ignore the override setting, the axis
feedrate, rapid feedrate, and the spindle speed override values are all set to
100 percent. An M49 cancels an M48 and your system installer can
choose which is active upon power-up. This override setting is ignored if
you are using programmed motion.
(7) Constant surface speed mode enable (M58)
M58 cancels M59 mode, and it allows the control to recognize
programmed G96 constant surface speed mode and S-words to be
specified. The spindle resumes the speed it was revolving at prior to the
designation of M59.
CAUTION: Restoring the constant surface speed mode might
cause the spindle speed to increase or decrease rapidly,
depending on the cutting tool position.
(8) Constant surface speed mode disabled (M59)
M59 cancels M58 and G96, making the constant surface speed mode
ineffective. The spindle continues to revolve at the speed it was at the
moment the M59 executed.
Z or the spindle speed can be directly designated using an S code.
(9) Subprogram call (M98)
When you execute M98, a subprogram is called and executed. This word
can be used in any program including an MDI program. For details on
programming an M98, see page 10-11.