Pocket Milling With Islands - Cycle73 - Siemens SINUMERIK 840D Programming Manual

Milling Cycles
3
3.15 Pocket milling with islands - CYCLE73, CYCLE74, CYCLE75

3.15.4 Pocket milling with islands - CYCLE73

Pocket milling with islands is an option and requires
SW 5.2 in both the NCK and MMC 103.
Programming
CYCLE73 (_VARI, _BNAME, _PNAME, _TN, _RTP,
_RFP, _SDIS, _DP, _DPR, _MID, _MIDA, _FAL, _FALD,
_FFP1, _FFD, _CDIR, _PA, _PO, _RAD, _DP1)
Parameters
_VARI
int
_BNAME
string
_PNAME
string
_TN
string
_RTP
real
_RFP
real
_SDIS
real
_DP
real
_DPR
real
_MID
real
_MIDA
real
_FAL
real
_FALD
real
3-188
Type of machining: (enter without sign)
UNITS POSITION (select machining):
Value: 1...Rough cut (remove stock) from solid material
2...Rough cut residual material
3...Finish edge
4...Finish base
5...Rough drill
TENS DIGIT (select insertion strategy):
Value: 1...Perpendicular with G1
2...Along a helix
3...Oscillate
HUNDREDS DIGIT (select liftoff mode):
Values:0...to retraction plane (_RTP)
1...by safety clearance (_SDIS) via reference plane (_RFP)
THOUSANDS DIGIT (select start point):
Values:1...Automatic
2...Manual
Name for program of drill positions
Name for pocket milling machining program
Name of stock removal tool
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (to be added to the reference plane, enter without sign)
Pocket depth (absolute)
Pocket depth (incremental)
Maximum infeed depth for infeed (enter without sign)
Maximum infeed depth in the plane (enter without sign)
Final machining allowance in the plane (enter without sign)
Final machining allowance on base (enter without sign)
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
08.99
3
 Siemens AG 2000 All rights reserved.