Milling Circular Pockets - Pocket2 - Siemens SINUMERIK 840D Programming Manual

Milling Cycles
3

3.8 Milling circular pockets - POCKET2

3.8 Milling circular pockets - POCKET2
Programming
POCKET2 (RTP, RFP, SDIS, DP, DPR, PRAD, CPA, CPO, FFD, FFP1, MID, CDIR,
FAL, VARI, MIDF, FFP2, SSF)
Parameters
RTP
real
RFP
real
SDIS
real
DP
real
DPR
real
PRAD
real
CPA
real
CPO
real
FFD
real
FFP1
real
MID
real
CDIR
int
FAL
real
VARI
int
MIDF
real
FFP2
real
SSF
real
The cycle requires a milling cutter with an "end tooth
cutting over center" (DIN 844).
The pocket milling cycle POCKET4 can be performed
with any tool.
3-136
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (enter without sign)
Pocket depth (absolute)
Pocket depth relative to the reference plane (enter without sign)
Pocket radius (enter without sign)
Pocket center point, abscissa (absolute)
Pocket center point, ordinate (absolute)
Feedrate for depth infeed
Feedrate for surface machining
Maximum infeed depth for infeed (enter without sign)
Milling direction for machining the pocket
Value: 2 (for G2)
3 (for G3)
Final machining allowance on pocket edge (enter without sign)
Type of machining
Value: 0=Complete machining
1=Roughing
2=Finishing
Maximum infeed depth for finishing
Feedrate for finishing
Speed for finishing
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
08.97
3
 Siemens AG 2000 All rights reserved.