212
M CODES
96-8000
June 1999
M CODE D ETAILED D ESCRIPTION
M00 Stop Program
The M00 code is used to stop a program. It also stops the spindle and turns off the coolant and stops interpre-
tation lookahead processing. The program pointer will advance to the next block and stop. A cycle start will
continue program operation from the next block. If the Through the Spindle Coolant option is ON, M00 will shut
it off.
M01 Optional Program Stop
The M01 code is identical to M00 except that it only stops if OPTIONAL STOP is turned on from the front
panel. A cycle start will continue program operation from the next block. If the Through the Spindle Coolant
option is ON, M01 will shut it off.
M02 Program End
The M02 code will stop program operation the same as M00 but does not advance the program pointer to the
next block.
M03 Spindle Forward
The M03 code will start the spindle moving is a clockwise direction at whatever speed was previously set. The
block will delay until the spindle reaches about 90% of commanded speed.
When Parameter 278 bit 10, "CNCR SPINDLE", is set to 1, the machine will not wait for the spindle to come
up to speed immediately after an M03 command. Instead, it will check and/or wait for the spindle to come up
to speed immediately before the next interpolated motion is initiated.
M04 Spindle Reverse
The M04 code will start the spindle moving is a counterclockwise direction at whatever speed was previously
set. The block will delay until the spindle reaches about 90% of commanded speed.
When Parameter 278 bit 10, "CNCR SPINDLE", is set to 1, the machine will not wait for the spindle to come
up to speed immediately after an M04 command. Instead, it will check and/or wait for the spindle to come up
to speed immediately before the next interpolated motion is initiated.
M05 Spindle Stop
The M05 code is used to stop the spindle. The block is delayed until the spindle slows below 10 RPM.
M06 Tool Change
The M06 code is used to initiate a tool change. The previously selected tool (Tn) is put into the spindle. If the
spindle was running, it will be stopped. No previous axis commands are required before the tool change unless
there is a problem with tool/part/fixture clearance. The Z-axis will automatically move up to the machine zero
position and the selected tool will be put into the spindle. The Z-axis is left at machine zero. The spindle will
not be started again after the tool change but the Snnnn speed and gear will be unchanged. The Tnn must be
in the same block or in a previous block. The coolant pump will be turned off during a tool change.
To Next Page
Loading...
Need help?
General
