Rockwell Automation 8520-GUM 9/Series CNC Grinder Operation and Programming Manual Documentation Set - Manual (Page 311)

Introduction to Programming
Chapter 10
10-33
(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.
The spindle speed can be directly programmed using an S word.
(9) Subprogram Call (M98)
When M98 is executed, a subprogram is called and executed. You can use
this word in any program including an MDI program. For details on
programming an M98, see page 10-12.
(10) End of Subprogram or Main Program Auto Start (M99)
M99 End of Subprogram or Paramacro program
When M99 is executed, subprogram execution is completed and
program execution returns to the calling program. This word is not
valid in an MDI command, though it can be contained in a subprogram
called by an MDI command. For details on programming an M99, see
page 10-12 or chapter 20.
M99 End of Main Program with Auto Start
If executing a program from memory, an M99 as the last block in a main
program causes program execution to stop at that location. The
program is reset to the first block and a <CYCLE START>
automatically starts program execution for you.
If executing a program from an external device (such as a tape reader),
when M99 is executed, program execution is stopped and the tape is
automatically rewound to the beginning of the program just executed.
Pressing <CYCLE START> automatically starts program execution.
ATTENTION: The M99 code is commonly used as the end of
program for fully automated systems that automatically load the
next part. Typically this code requires that some PAL interface
be written that make sure the part is fully loaded and ready for
grinding before block execution is allowed to restart. Failure to
do so can cause injury to operators or damage to equipment.
Other M codes are described in later sections that deal specifically with
their function.