Path Milling - Cycle72 - Siemens SINUMERIK 840D Programming Manual

Milling Cycles
3

3.12 Path milling - CYCLE72

3.12 Path milling - CYCLE72
The cycle CYCLE72 is available with Software
Version 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:
_KNAME
string
_RTP
real
_RFP
real
_SDIS
real
_DP
real
_MID
real
_FAL
real
_FALD
real
_FFP1
real
_FFD
real
_VARI
int
_RL
int
3-162
Name of the contour subroutine
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (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
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
12.98
3
 Siemens AG 2000 All rights reserved.