HEIDENHAIN TNC 640 (34059x-04) ISO programming - Manual (Page 342)

Programming: Miscellaneous functions
10.4 Miscellaneous functions for path behavior
10
342
TNC 640 | User's Manual for DIN/ISO Programming | 3/2014
Retraction from the contour in the tool-axis direction:
M140
Standard behavior
In the program run 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.
N250 G01 X+0 Y+38.5 F125 M140 MB50 *
N251 G01 X+0 Y+38.5 F125 M140 MB MAX *
M140 is also effective if the tilted-working-plane
function is active. On machines with tilting heads,
the TNC then moves the tool in the tilted coordinate
system.
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.
Danger of collision!
When dynamic collision monitoring (DCM) is active,
the TNC might move the tool only until it detects a
collision and, from there, complete the NC program
without any error message. This can result in tool
paths different from those programmed!