4 MACHINING PROGRAM
4-48
2. Coolant stop command
This command turns off all coolant and air.
It is not necessary to program the coolant stop command if they are not turned on in the
preparation motion for machining.
3. Home return
Perform home return on each axis. Select the order of home return for safety.
Depending on the machining method, the mill spindle may need to move to a safe position.
In that case, set the coordinate values by G53. Home return commands are not necessary for
the axes which have already returned home such as B axis.
4. Program end
M-codes of program end are shown in the figure below.
Select an appropriate command by the machining method. M30 is used for program end in this
manual.
M00: Program stop
Program execution will be stopped, At this time, the milling spindle and the
turning spindle rotations will also be stopped.
M02: End of program
NC is reset and all the machine motions: spindle rotation, coolant, air. etc. will
be stopped.
M30: Reset and rewind
This function code stops the machine similarly to M02, and calls the head of the
program.
M99: Subprogram return command
This command returns the operation from subprogram to the main program
where the subprogram was called.
Note: M30 contains the reset of NC.
G00G90G53Zz (Z-axis Positioning)
G53Xz (X-axis Positioning)
G53Yy (Y-axis Positioning)
M108
G90G53Bb (B-axis Positioning)
(for home return in order of ZXY)
G28G91Z0 (Z-axis home )
G28X0 (X-axis home )
G28Y0 (Y-axis home )
M108
G28B0 (B-axis home)
Used to bring the axes home return.
Used to position the axes to an arbitrary
position. If zero they are the same with
home.
M09: All coolants OFF
This M code turns off all machining-related fluids such as coolants and air.
Serial No. 294060
Copyright (c) 2013 YAMAZAKI MAZAK CORPORATION. All rights reserved.
To Next Page
Loading...
Need help?
General
