Siemens SINUMERIK 840D Programming Manual page 87

2
03.96
09.01
The feed is then calculated in the cycle from the lead
and the speed. After the cycle has ended, the last
programmed feed applies again.
Programming:
ENC=11, programming the lead in MPIT or PIT
• Tapping with encoder with dwell time (SW 6.2 or higher):
As an alternative, you can program a dwell time in
the parameter DTB for tapping with encoder (G33
thread) from SW 6.2. It applies after tapping and
before retraction to the retraction plane RTP, and is
required for machines with unfavorable spindle
dynamics.
Programming:
ENC=20, entering the dwell time in parameter DTB
MPIT and PIT (as thread size and as value)
The parameter for the spindle pitch only has a meaning
if tapping is performed with encoder. The cycle
calculates the feedrate from the spindle speed and the
pitch.
The value for the thread pitch can either be defined as
the thread size (for metric threads between M3 and M48
only) or as a value (distance from one thread turn to the
next as a numerical value). The parameter not required
in each case is omitted from the call or assigned the
value zero.
If the two thread pitch parameters have conflicting
values, alarm 61001 "Thread pitch wrong" is generated
by the cycle and cycle execution is aborted.
_AXN (tool axis)
By programming the drilling axis via _AXN, it is
possible to omit the switchover from plane G18 to
G17 when the deep hole tapping cycle is used on
turning machines. Meaning:
_AXN=1 1st axis of the current plane
_AXN=2 2nd axis of the current plane
_AXN=3 3rd axis of the current plane.
For example, to machine a center drilling (in Z) in
plane G18, you program:
G18
_AXN=1
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
Drilling Cycles and Drilling Patterns
2.1 Drilling cycles
2
2-87