Path Milling - Cycle72 - Siemens SINUMERIK 840D Programming Manual

3
12.97
12.98
3.12 Path milling – CYCLE72
The cycle CYCLE72 is available with SW 4 (not for
FM-NC).
Programming
CYCLE72 (_KNAME, _RTP, _RFP, _SDIS, _DP, _MID, _FAL, _FALD, _FFP1, _FFD, _VARI, _RL,
_AS1, _LP1, _FF3, _AS2, _LP2)
Parameters
The following input parameters are always required:
string
_KNAME
real
_RTP
real
_RFP
real
_SDIS
real
_DP
real
_MID
real
_FAL
real
_FALD
real
_FFP1
real
_FFD
int
_VARI
int
_RL
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
Name of the contour subroutine
Retraction plane (absolute)
Reference plane (absolute)
Safety distance (to be added to the reference plane, enter without sign)
Depth (absolute)
Maximum infeed depth (incremental, enter without sign)
Final machining allowance at the edge contour (enter without sign)
Final machining allowance at the base (incremental, enter without sign)
Feedrate for surface machining
Feedrate for depth infeed (enter without sign)
Type of machining: (enter without sign)
UNITS DIGIT:
Value: 1...Roughing
2...Finishing
TENS DIGIT:
Value: 0...Intermediate paths with G0
1...Intermediate paths with G1
HUNDREDS DIGIT:
Value: 0...Return at end of contour to _RTP
1...Return at end of contour to _RFP + _SDIS
2...Return at end of contour to _SDIS
3...No return to end of contour
Contouring is centric, on right or left (with G40, G41 or G42, enter
without sign)
Value: 40...G40 (approach and return, straight line only)
41...G41
42...G42
3.12 Path milling – CYCLE72
3
Milling Cycles
3-179