HEIDENHAIN TNC 128 (77184x-02) - Manual (Page 259)

Miscellaneous functions for path behavior 9.4
9
TNC 128 | User's Manual HEIDENHAIN Conversational Programming | 5/2014
259
Retraction from the contour in the tool-axis direction:
M140
Standard behavior
In the Program Run, Single Block and Program Run, Full Sequence
operating modes the TNC moves the tool as defined in the part
program.
Behavior with M140
With M140 MB (move back) you can enter a path in the direction of
the tool axis for departure from the contour.
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 MB 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 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.
250 X+0 F125 M140 MB 50 F750
251 X+0 F125 M140 MB MAX
With
M140 MB MAX you can only retract in the
positive direction.
Always define a TOOL CALL with a tool axis before
entering
M140, otherwise the direction of traverse is
not defined.