HEIDENHAIN TNC 640, User Manual, Page: 490 / 948

Miscellaneous Functions | Miscellaneous functions for path behavior
11
490
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
Feed rate for circular arcs: M109/M110/M111
Standard behavior
The control applies the programmed feed rate to the path of the
tool center.
Behavior at circular arcs with M109
For inside and outside machining of circular arcs, the control keeps
the feed rate at the cutting edge constant.
NOTICE
Caution: Danger to the tool and workpiece!
If the
M109
function is active, the control might dramatically
increase the feed rate when machining very small outside
corners. During the execution, there is a risk of tool breakage or
workpiece damage.
Do not use
M109
for machining very small outside corners
Behavior at circular arcs with M110
With circular arcs, the control only keeps the feed rate constant for
inside machining operations. The feed rate will not be adjusted for
outside machining of circular arcs.
If you program
M109
or
M110
with a number > 200
before calling a machining cycle, the adjusted feed
rate will also be effective for circular arcs within these
machining cycles. The initial state is restored after
finishing or canceling a machining cycle.
Effect
M109
and
M110
become effective at the start of the block.
M109
and
M110
can be canceled with
M111
.