Boring 4 – Cycle88 - Siemens SINUMERIK 840D Programming Manual

03.96
2
2.1.10 Boring 4 – CYCLE88
Programming
CYCLE88 (RTP, RFP, SDIS, DP, DPR, DTB, SDIR)
Parameters
RTP
real
RFP
real
SDIS
real
DP
real
DPR
real
DTB
real
SDIR int
Function
The tool drills at the programmed spindle speed and
feedrate to the programmed final drilling depth. With
Boring 4, a dwell time, a spindle stop without orientation
M5 and a programmed stop M0 are generated when the
final drilling depth is reached. Pressing the NC START
key continues the retraction movement in rapid traverse
mode until the retraction plane is reached.
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 G1 and the
feedrate programmed before the program call
• Dwell time at final drilling depth
• Spindle stop with M5 (_ZSD[5]=1) or
• spindle and program stop with M5 M0 (_ZSD[5]=0).
Press the NC START key
after program stop.
• Retraction to retraction plane with G0
 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 final drilling depth
Direction of rotation
Drilling Cycles and Drilling Patterns
2.1 Drilling cycles
Value: 3 (for M3)
Z
2
4 (for M4)
2-85
X