HEIDENHAIN TNC 640 (34059x-05) - Manual (Page 382)

Programming: Miscellaneous functions
10.4 Miscellaneous functions for path behavior
10
382
TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 1/2015
Retraction from the contour in the tool-axis
direction: M140
Standard behavior
In the program run modes Program run single block and Program
run full sequence 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 L X+0 Y+38.5 F125 M140 MB 50 F750
251 L X+0 Y+38.5 F125 M140 MB MAX
M140 is also effective if the tilted-working-plane
function is active. On machines with swivel 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!
If you modify the position of a rotary axis with the
handwheel superimposition
M118 function and then
run M140, the TNC ignores the superimposed values
with the retraction movement.
This may cause undesired motion or collisions on
machines with rotary axes in the head.