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

Drilling Cycles and Drilling Patterns
2
2.1 Drilling cycles
2.1.2 Drilling, centering – CYCLE81
Programming
CYCLE81 (RTP, RFP, SDIS, DP, DPR)
RTP
real
RFP
real
SDIS
real
DP
real
DPR
real
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 clearance with G0
• Traverse to final drilling depth with the feedrate
(G1) programmed in the calling program
• Retraction to retraction plane with G0
2-52
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)
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
Z
 Siemens AG 2000 All rights reserved.
03.96
2
X