HEIDENHAIN TNC 320 (340 551-01) - Manual (Page 170)

170 7 Programming: Miscellaneous Functions
7.
4 Miscellaneous F
u
nctions f
o
r Cont
our
ing Beha
vior
Input
If you enter M140 in a positioning block, the TNC continues the dialog
and asks for the desired path of tool departure from the contour. Enter
the requested path that the tool should follow when departing the
contour, or press the MAX soft key to move to the limit of the traverse
range.
In addition, you can program the feed rate at which the tool traverses
the entered path. If you do not enter a feed rate, the TNC moves the
tool along the entered path at rapid traverse.
Effect
M140 is effective only in the block in which it is programmed.
M140 becomes effective at the start of the block.
Example NC blocks
Block 250: Retract the tool 50 mm from the contour.
Block 251: Move the tool to the limit of the traverse range.
Suppressing touch probe monitoring: M141
Standard behavior
When the stylus is deflected, the TNC outputs an error message as
soon as you attempt to move a machine axis.
Behavior with M141
The TNC moves the machine axes even if the touch probe is
deflected. This function is required if you wish to write your own
measuring cycle in connection with measuring cycle 3 in order to
retract the stylus by means of a positioning block after it has been
deflected.
Effect
M141 is effective only in the block in which it is programmed.
M141 becomes effective at the start of the block.
250 L X+0 Y+38.5 F125 M140 MB 50 F750
251 L X+0 Y+38.5 F125 M140 MB MAX
With M140 MB MAX you can only retract in positive direction.
If you use M141, make sure that you retract the touch
probe in the correct direction.
M141 functions only for movements with straight-line
blocks.