HEIDENHAIN TNC 407 (280 580) ISO Programming - Manual (Page 170)

5 - 3 7 TNC 426/TNC 425/TNC 415 B/TNC 407
5 Programming Tool Movements
5.6 M Functions for Contouring Behavior
Y
X
S
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.
If the contour steps are very small, however, the
tool would damage the contour. In such cases the
TNC interrupts program run and generates 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
M97 is effective only in the blocks in which it is
programmed.
A corner machined with M97 will not be completely finished. It may have to be reworked with a smaller tool.
Program structure
N5 G99 L ... R+20 ................................................. Large tool radius
N20 G01 X ... Y ... M97 ........................................... Move to contour point 13
N30 G91 Y–0.5 ....................................................... Machine small contour step 13-14
N40 X+100 .............................................................. Move to contour point 15
N50 Y+0.5 M97 ...................................................... Machine small contour step 15-16
N60 G90 X ... Y ... .................................................. Move to contour point 17
The outside corners are programmed in blocks N20 and N50. These are
the blocks in which you program M97.
.
.
.
.
.
.
.
.
.
Fig. 5.44: Standard contouring behavior without M97 when the control
would not generate an error message
Fig. 5.45: Contouring behavior with M97