Siemens SINUMERIK 840D Programming Manual page 78

2
Drilling Cycles and Drilling Patterns
2.1 Drilling cycles
int
_TECHNO
(SW 6.2 or
higher)
int
_VARI
(SW 6.2 or
higher)
real
_DAM
(SW 6.2 or
higher)
real
_VRT
(SW 6.2 or
higher)
Function
The tool drills at the programmed spindle speed and
feedrate to the programmed thread depth.
With cycle CYCLE84 you can perform rigid tapping
operations.
In SW 6.2 or higher, the cycle is also capable of
performing tapping operations in several stages (deep
hole drilling).
Cycle CYCLE84 can be used if the spindle to be used
for the boring operation is technically able to go into
position-controlled spindle operation.
A separate cycle CYCLE840 exists for tapping with
compensating chuck (see Subsection 2.1.6).
2-78
Technological settings
UNITS DIGIT: Exact stop behavior
Values: 0...and as programmed before cycle call
1...(G601)
2...(G602)
3...(G603)
TENS DIGIT: Feedforward control
Values: 0...and as programmed before cycle call
1...with feedforward control (FFWON)
2...without feedforward control (FFWOF)
HUNDREDS DIGIT: Acceleration
Values: 0...and as programmed before cycle call
1...soft acceleration of axes (SOFT)
2...brisk acceleration of axes (BRISK)
3...reduced acceleration of axes (DRIVE)
THOUSANDS DIGIT:
Values: 0...activate spindle mode again (with MCALL)
1...stay in position-control mode (with MCALL)
Type of machining
Values: 0...tapping in one pass
1...deep hole tapping with chip breakage
2...deep hole tapping with stock removal
Incremental drilling depth
Value range: 0 <= max. value
Variable retraction distance for chip breakage
Value range: 0 <= max. value
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
2
03.96
09.01
© Siemens AG, 2002. All rights reserved