Technical Manual TNC 360 - heidenhain - DR. JOHANNES ...

7.1 Program halt on M functions
Normally, when an M function is produced, the program run in the operating modes "Program
run/full sequence" and "Program run/single block" is interrupted until the PLC acknowledges that the
M function has been performed.
For some applications this can be disadvantageous (e.g. laser cutting machines). In such applications
the program should be executed continuously and not wait for the acknowledgment of the M
function. This function can be selected by machine parameter MP7440, Bit 2. If this function is
selected then PLC positioning, datum correction, spindle orientation or limit switch range change are
all not permitted during the output of the M function.
This function must not be used for milling machines and boring machines.
7.2 Program halt on M06
According to ISO 6983, the M function M06 means a tool change. Machine parameter MP7440, Bit
0 can be used to select whether on transferring M06 to the PLC the program should halt. If the
control is set so that a program halt occurs on M06 then the program must be restarted after the
tool change. This can also be carried out directly by the PLC.
7.3 M function M89
The M function M89 can be used for the modal cycle call. The possibilities for calling a cycle are:
– With the NC block "CYCL CALL".
– With the miscellaneous function M99. M99 is only effective for a single block and must
be reprogrammed for each execution.
– With the miscellaneous function M89 (depending on the machine parameter).
M89 as a cycle call is modally effective, i.e. for every following positioning block
there will be a call of the last programmed machining cycle. M89 is canceled by M99 or
a CYCL CALL block.
If M89 is not defined as a modal Cycle call by machine parameters, then M89 will be transferred
to the PLC as a normal M function at the beginning of the block.
MP7440 Output of M functions
Input range: 0 to 7
Bit 0 Program halt on M06 + 0 = Program halt on M06
+ 1 = No program halt on M06
Bit 1 modal cycle call M89 + 0 = Normal code transfer of
M89 at beginning of block
+ 2 = modal cycle call M89 at end of block
Bit 2 Program halt on + 0 = Program halt until
M functions acknowledgment of M function
+ 4 = No program halt
do not wait for acknowledgment
4-140 TNC 360 7 M Functions 8/95