Siemens SINUMERIK 840D Programming Manual page 184

3
Milling Cycles
3.12 Path milling – CYCLE72
Description of parameters
See Subsection 2.1.2. (Drilling, Centering –
CYCLE81) for a description of parameters _RTP,
_RFP, _SDIS
See Section 3.9 for a description of parameters _MID,
_FAL, _FALD, _FFP1, _FFD and Section 3.11 for
parameter _DP.
See Section 3.2 for cycle setting data _ZSD[1].
_KNAME (name)
The contour to be milled is completely programmed in a
subroutine. With parameter _KNAME you can define
the name of the contour subroutine.
In SW 5.2 and higher, the milling contour can also
be a section of the calling routine or from any other
program. The section is identified by start or end
labels or by block numbers. In this case, the
program name and labels/block number are
identified by an ":".
Examples:
_KNAME="CONTOUR_1"
_KNAME="START:END"
_KNAME=
"/_N_SPF_DIR/_N_CONTOUR_1_SPF:N130:N210"
If the section is defined by block numbers, it must be
noted that these block numbers for the section in
_KNAME must be adjusted if the program is modified
and subsequently renumbered.
3-184
Z
The milling contour is the complete program
"Contour_1".
The milling contour is defined as the section
starting from the block labeled START to the
block labeled END in the calling routine.
The milling contour is defined in blocks N130
to N210 in program CONTOUR_1. The
program name must be entered complete
with path and extension, see description of
call in References: /PGA/ Programming
Guide Advanced.
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
Reference plane _RFP
Finishing allowance depth _FALD
Final machining allowance _DP
X
© Siemens AG, 2002. All rights reserved