Siemens SINUMERIK 840D Programming Manual page 174

3
Milling Cycles
3.11 Face milling – CYCLE71
Function
With cycle CYCLE71, you can face mill any
rectangular surface. The cycle differentiates
between roughing (machining the surface in several
steps until reaching the final machining allowance)
and finishing (end milling the surface in one step).
Maximum infeed can be defined in width and depth.
The cycle operates without cutter radius
compensation. The depth infeed is programmed in
the open.
Sequence of operations
Position reached prior to cycle start:
This can be any position from which the starting
position on the infeed point at the retraction plane
level can be reached without collision.
The cycle implements the following motion
sequence:
• G0 is applied to approach the infeed point on the
current position plane. The reference plane, shifted
forward by the safety distance, is then also
approached with G0 from this position. Then, also
with G0, infeed to machining plane. G0 is possible,
since infeed occurs in the open.
There are several roughing strategies (paraxial in
one direction or back and forth).
• Motion sequence when roughing (VARI=X1):
Roughing is possible on several planes according to
the programmed values _DP, _MID and _FALD.
Machining will be performed in the downward
direction, i.e. by removing stock on one plane at a
time, and then executing the next depth infeed in
open space (parameter_FDP).
The traversing paths for stock removal on the plane
are determined by the settings in parameters
_LENG, _WID, _MIDA, _FDP, _FDP1 and the cutter
radius of the active tool.
3-174
Y
_LENG
Y
_LENG
Possible machining strategies for face milling
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
Y
_LENG
X X
Y
_LENG
X X
© Siemens AG, 2002. All rights reserved