HEIDENHAIN TNC 360 User Manual - Manual (Page 121)

5-37 TNC 360
5 Programming Tool Movements
Fig. 5.44: Contouring behavior with M97
Fig. 5.43: Standard behavior without M97 if the block were to be
executed as programmed
5.6 M-Functions for Contouring Behavior and Coordinate Data
WZ
Y
X
S
WZ
Y
X
13
14
16
15
17
S
.
.
.
.
.
.
.
.
.
Machining small contour steps: M97
Standard behavior – without M97
The TNC inserts a transition arc at outside corners.
At very short contour steps this would cause the
tool to damage the contour. In such cases the TNC
interrupts the program run and shows the error
message TOOL RADIUS TOO LARGE.
Machining contour steps with M97
The TNC calculates the contour intersection S
(see figure) of the contour elements – as at inside
corners – and moves the tool over this point. M97
is programmed in the same block as the outside
corner point.
Duration of effect
The miscellaneous function M97 is effective only in
the blocks in which it is programmed.
A contour machined with M97 is less complete than one without. You may wish to rework the contour with a
smaller tool.
Program example
5 TOOL DEF L ... R+20 ......................................... Large tool radius
13 L X ... Y ... R.. F .. M97 ....................................... Move to contour point 13
14 L IY–0.5 .... R .. F.. .............................................. Machine the small contour step 13 - 14
15 L IX+100 ... ......................................................... Move to contour point 15
16 L IY+0.5 ... R .. F.. M97 ...................................... Machine the small contour step 15 - 16
17 L X .. Y ... ............................................................ Move to contour point 17
The outer corners are programmed in blocks 13 and 16: these are the
blocks in which you program M97.