Drilling, Centering - Cycle81 - Siemens SINUMERIK 840D Programming Manual

2
Drilling Cycles and Drilling Patterns
2.1 Drilling cycles
2.1.2 Drilling, centering – CYCLE81
Programming
CYCLE81 (RTP, RFP, SDIS, DP, DPR)
real
RTP
real
RFP
real
SDIS
real
DP
real
DPR
Function
The tool drills at the programmed spindle speed and
feedrate to the programmed final drilling depth.
Sequence of operations
Position reached prior to cycle start:
The drilling position is the position in the two axes of
the selected plane.
The cycle implements the following motion
sequence:
Approach of the reference plane brought forward by
the safety distance with G0
• Traverse to final drilling depth with the feedrate
(G1) programmed in the calling program
• Retraction to retraction plane with G0.
2-64
Retraction plane (absolute)
Reference plane (absolute)
Safety distance (enter without sign)
Final drilling depth (absolute)
Final drilling depth relative to reference plane (enter without sign)
Z
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
2
03.96
X
© Siemens AG, 2002. All rights reserved