Program-Run Interruption With M-Functions; Program-Run Interruption With M06; Modal Cycle Call M89; Reduced Feed-Rate Of Tool Axis With M103 - HEIDENHAIN TNC 415 Technical Manual

7.1 Program-run interruption with 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, DNC-operation). In
such applications the program should be executed continuously and not wait for the
acknowledgement 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 with milling machines or boring machines.

7.2 Program-run interruption with 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-run interruption 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 Modal cycle call 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 cancelled 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.

7.4 Reduced feed-rate of tool axis with M103

The entry M103 F... can be used to reduce the contour feed-rate for movements of the tool axis in
the negative direction. The feed-rate element of the tool axis is limited to a value that the TNC
computes from the last programmed feed-rate.
F = F *F
max prog %
F = Maximum feed-rate in negative direction of tool axis
max
F = Last programmed feed-rate
prog
F = Programmed factor after M103 in %
%
M103 F... is cancelled by a new entry for M103 without a factor.
The function M103 F... is enabled by MP7440, Bit 4.
01.98 TNC 407/TNC 415/TNC 425 7 M-functions 4-161