HEIDENHAIN TNC 620 (73498x-01) ISO programming - Manual (Page 291)

HEIDENHAIN TNC 620 291
9.4 Miscellaneous functions f
o
r cont
our
ing beha
vior
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.