Siemens SINUMERIK 840D Programming Manual page 164

Milling Cycles
3
3.12 Path milling - CYCLE72
Function
With the cycle CYCLE72 it is possible to mill along
any contour defined in a subroutine. The cycle
operates with or without cutter radius compensation.
The contour does not need to be closed; internal or
external machining is defined by the position of the
cutter radius compensation (center, on left or right of
contour).
The contour must be programmed in the
direction to be milled and consist of at least 2
contour blocks (start and end point), since the
contour subroutine is called directly within the cycle.
Cycle functions:
• Selection of roughing (single-pass parallel to the
contour considering a finishing allowance if
necessary at several depths until reaching the final
machining allowance) and finishing (single-pass of
final contour, if necessary at several depths)
• Flexible approach and retraction to/from the contour
either tangentially or radially (quadrant or semi-
circle)
• Programmable depth infeed
• Intermediate motions either with rapid traverse or
at feedrate
The requirement for executing a cycle is an NC
Software Version 4.3. or higher that includes the
function "Soft approach and return".
Sequence of operations
Position reached prior to cycle start:
The starting position can be any position from which
the start of the contour at the retraction plane level
can be reached without collision.
3-164
Y
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
12.98
Contour starting point
 Siemens AG 2000 All rights reserved.
3
X