Tapping With Compensating Chuck – Cycle840 - Siemens SINUMERIK 840D Programming Manual

03.96
2
2.1.6 Tapping with compensating chuck – CYCLE840
Programming
CYCLE840 (RTP, RFP, SDIS, DP, DPR, DTB, SDR, SDAC, ENC, MPIT, PIT)
Parameters
RTP
real
RFP
real
SDIS
real
DP
real
DPR
real
DTB
real
SDR
int
SDAC
int
ENC
int
MPIT
real
PIT
real
Function
The tool drills at the programmed spindle speed and
feedrate to the programmed thread depth.
With this cycle, tapping with compensating chuck
can be performed
• without encoder and
• with encoder.
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (enter without sign)
Final drilling depth (absolute)
Final drilling depth relative to reference plane (enter without sign)
Dwell time at thread depth
Direction of rotation for retraction
Values: 0 (automatic reversal of direction of rotation)
3 or 4 (for M3 or M4)
Direction of rotation after end of cycle
Values: 3, 4 or 5 (for M3, M4 or M5)
Tapping with/without encoder
Values: 0 = with encoder
1 = without encoder
Thread pitch as thread size
Value range: 3 (for M3) ... 48 (for M48)
Thread pitch as value
Value range: 0.001 ... 2000.000 mm
Drilling Cycles and Drilling Patterns
2.1 Drilling cycles
2
2-69