Hurco winmax, Programming Manual, Page: 102 / 254

3 - 4 Basic NC M Codes
704-0115-307
WinMax Lathe NC Programming
M00 - Program Stop
M00 causes part program execution to stop and the spindle to turn off. Press the START
CYCLE button to resume program execution and restart the look-ahead program.
Execute after tool change or motion (system M codes).
M01 - Optional Stop
M01 performs the same functions as M00, but can be toggled on or off through the Opt
Stop key on the control.
• When the Opt Stop key is Off, the program ignores M01.
• When the Opt Stop key is On, the program stops on M01 so you can inspect
the part. Press the START CYCLE button to resume running the program.
Execute after tool change or motion.
M02 - End of Program (no rewind)
M02 stops program execution and leaves the part program pointer on the block that
follows the M02 command. M02 is required at the end of all programs. It commands the
spindle to turn off. Execute at the end of the block after all motion occurs.
M03 - Spindle Clockwise
M03 turns the spindle on in the clockwise direction. M03 will execute after Tool, Spindle,
and E (Work Offset) codes execute, but before motion programmed in the block occurs.
An S code specifying the spindle speed must be programmed before the spindle will turn
on. The advanced RPM Look Ahead feature that reduces part cycle time by ramping the
spindle up to speed before the feed move begins improves the cycle time because the
control does not dwell while the spindle ramps up to the programmed speed. When this
feature is active, it is possible to create a part program containing an M03 and spindle
speed command that does not turn on the spindle.
Execute after T and S codes, but before motion.
M04 - Spindle Counterclockwise
M04 is the same as M03 except it commands the spindle to rotate in the counterclockwise
direction. Execute after T and S codes, but before motion.