GSK GSK928TE, Руководство пользователя

Страница: 118 / 187

GSK928TE
Ⅱ
Turning CNC System User Manual
113
3.2 M function —Miscellaneous Function
The M functions are used for the start/stop of machine and the run order of part program. M
commands consist of address characters and the following 2-digit integer. All M functions of
GSK928TE
Ⅱ
CNC System are as follows:
Command Function Format Remarks
M00 Pause to wait the restart M00 Press the run button to restart
M02 End program M02
M20
End program, and return to the first
block to execute the machining cycle
M20
M30
End of program, spindle stop and
cooling OFF
M30
M03 Spindle rotation(CW) M03
M04 Spindle rotation(CCW) M04
M05 Spindle stop M05
M08 Cooling ON M08
M09 Cooling OFF M09
M10 Workpiece clamped M10
M11 Workpiece released M11
M41 Spindle gear shifting to 1st gear M41
M42 Spindle gear shifting to 2nd gear M42
M43 Spindle gear shifting to 3rd gear M43
M78 Tailstock going forward M78
M79 Tailstock retreating backward M79
M97 Program skip M97 P Define the skipping block number by P
M98 Subprogram call M98 P L
Define the skipping block number by P and
the skipping times defined by L
M99 Subprogram return M99
M21 The No.1 user output is valid M21
M22 The No.1 user output is invalid M22
M23 The No.2 user output is valid M23
M24 The No.2 user output is invalid M24
With D parameter, the output signal keeps a
long time defined by D and the signal will be
cancelled if the time ends
M91
Wait for the invalid signal when No.
1 user input is valid
M91 P Define the skipping block number by P
M92
Wait for the valid signal when No.1
user input is invalid
M92 P Define the skipping block number by P
M93
Wait for the invalid signal when No.
2 user input is invalid
M93 P Define the skipping block number by P
M94
Wait for the valid signal when No.2
user input is invalid
M94 P Define the skipping block number by P
Note 1:
There is only one M command in each block and the leading zero can be omitted.
Note 2:
When M and G are in the same block, the execution is as follows:
·
M03, M04, M08 before G commands are executed
·M00, M02, M05, M09, M20, M30 are behind G commands
·M21, M22, M23, M24, M25, M92, M93, M94, M97, M98, M99
They are only in the separate block without other G or M.
Note 3:
P of M91, M92, M93, M94 can be omitted.
3.2.1 M00 — Pause
Command format
：
M00
Pause programs by M00, which is convenient for user to execute others and run again by
pressing the run button.
There is difference function between M00 and the feed hold key. The pause before some block
is defined by M00 according to the requirement and the feed hold key is used for the random
pause.