HEIDENHAIN TNC 320 (340 551-01) - Manual (Page 167)

HEIDENHAIN TNC 320 167
7.
4 Miscellaneous F
u
nctions f
o
r Cont
our
ing Beha
vior
Machining open contours: M98
Standard behavior
The TNC calculates the intersections of the cutter paths at inside
corners and moves the tool in the new direction at those points.
If the contour is open at the corners, however, this will result in
incomplete machining.
Behavior with M98
With the miscellaneous function M98, the TNC temporarily suspends
radius compensation to ensure that both corners are completely
machined.
Effect
M98 is effective only in the blocks in which it is programmed.
M98 takes effect at the end of block.
Example NC blocks
Move to the contour points 10, 11 and 12 in succession:
Feed rate for circular arcs: M109/M110/M111
Standard behavior
The TNC applies the programmed feed rate to the path of the tool
center.
Behavior at circular arcs with M109
The TNC adjusts the feed rate for circular arcs at inside and outside
contours so that the feed rate at the tool cutting edge remains
constant.
Behavior at circular arcs with M110
The TNC keeps the feed rate constant for circular arcs at inside
contours only. At outside contours, the feed rate is not adjusted.
Effect
M109 and M110 become effective at the start of block.
To cancel M109 and M110, enter M111.
10 L X... Y... RL F
11 L X... IY... M98
12 L IX+ ...
X
Y
S S
X
Y
11 12
10
M110 is also effective for the inside machining of circular
arcs using contour cycles. If you define M109 or M110
before calling a machining cycle, the adjusted feed rate is
also effective for circular arcs within machining cycles. The
initial state is restored after finishing or aborting a
machining cycle.