Pocket Milling With Islands - Cycle73, Cycle74, Cycle75 (Sw 5.2 And Higher) - Siemens SINUMERIK 840D Programming Manual

3
Milling Cycles
3.15 Pocket milling with islands – CYCLE73, CYCLE74, CYCLE75
Explanation of parameters
The edge contour can be programmed either in a
separate program or in the main program that calls the
routine. The contour is transferred to the cycle by
parameter _KNAME, name of program or _LSANF,
_LSEND and the program section from ... to identified
by block numbers or labels.
So there are three options for contour programming:
• Contour is defined in a separate program,
in which case only _KNAME needs to be
programmed;
e.g. CYCLE74 ("EDGE","","")
• Contour is defined in the calling program,
in which case only _LSANF and _LSEND need to
be programmed;
e.g. CYCLE74 ("","N10","N160")
• The edge contour is part of a program but not
part of the program that calls the cycle,
in which case all three parameters need to be
programmed.
e.g. CYCLE74("EDGE","MARKER_START",
"MARKER_END")
The program name is describable by its path name and
program type.
Example:
_KNAME="/N_WKS_DIR/_N_EXAMPLE3_WPD/_N_EDGE_MPF"
3-200
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
10.00
© Siemens AG, 2002. All rights reserved