Siemens SINUMERIK 840D Programming Manual page 182

3
Milling Cycles
3.12 Path milling – CYCLE72
The cycle creates the following motion sequence
when roughing (VARI=XX1):
The depth infeeds are divided evenly using the
highest possible value according to the preset
parameter.
• Travel to starting point for initial cut with G0/G1
(and _FF3). This point is calculated internally in
the control and depends on
- the contour starting point (first point in
subroutine),
- the direction of the contour at the starting point,
- the approach mode and corresponding
parameters and
- the tool radius.
The cutter radius path compensation is activated
in this block.
• Depth infeed to first or next machining depth plus
programmed safety distance DISCL with G0/G1.
The first processing depth is given by
- the overall depth,
- the final machining allowance and
- the maximum possible depth infeed.
• Approach the contour perpendicular to the feed
depth and approach in the plane then at the
feedrate programmed for surface machining, or
programmed under _FAD for 3D machining
corresponding to the programming for soft
approach.
• Milling along the contour with G40/G41/G42.
• Soft retraction from the contour with G1 and still
with the feedrate for surface machining by lift
DISCL.
• Retraction with G0 /G1 (and feedrate for
intermediate travel _FF3) depending on program.
• Return to depth infeed point with G0/G1 (and
_FF3).
• This operating sequence is repeated on the next
machining plane, until reaching the final
machining allowance in depth.
When roughing is over, the tool lies on the contour
starting point (calculated within the control unit) at
the retraction plane level.
3-182
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
12.98
© Siemens AG, 2002. All rights reserved