12 Miscellaneous and Auxiliary Functions
12 Miscellaneous and Auxiliary Functions
12.1 Miscellaneous Functions (Codes M)
With a numerical value of max. 3 digits specified behind address M, the NC will transfer the code to the PLC.
When a movement command and a miscellaneous function (M) are programmed in a given block, function M will be issued during or after the motion command. The machine tool builder will define the way of execution.
Codes M’s include standard functions, that can be used for special selected functions only. They:
M00, M01, M02, M30, M96, M97, M98, M99: program control codes
M03, M04, M05, M19: Spindle rotation codes
M06: tool change code
M07, M08, M09: coolant management codes
M11, ..., M18:
When indexing is triggered by M, the M codes of spindle indexing are selected on the basis of a parameter.
The control system enables several M codes of different groups to be written in a given block. In this case, however, codes M’s have a fixed sequence of execution. The groups and the sequence of
execution: |
|
group 1 | M06 (tool exchange) |
group 2 | M11, ..., M18 (spindle gear range change) |
group 3 | M03, M04, M05, M19 (spindle management) |
group 4 | M07, M08, M09 (coolant management) |
group 5 | Mnnn (any other function M) |
group 6 | codes M of spindle indexing |
group 7 | M00, M01, M02, M30, M96, M97, M98, M99 (program control codes) |
The number of M functions that can be programmed in a given block is 5. Only one M of each group can be programmed in a block. Conflicting programming will produce error message 3032
CONFLICTING M CODES.
The exact functioning of each M code is defined by the builder of the particular
The program control M codes are:
M00= programmed stop
The stop condition will be generated at the end of the block, in which M00 has been specified. All modal functions remain unchanged. It can be restarted by START.
M01= conditional stop
Its effect is identical with that of code M00. It will be executed when the CONDITIONAL STOP key is activated. Unless the appropriate key is set up, it is ineffective.
M02, M30= end of program
It means the end of the main program. All operations are stopped, and the control is "reset". The machine will be reset by the PLC program. Unless the parameter PRTCNTM differ from it, each of executed M02 or M03 command increase the counters of workpiece.
71
