Siemens SINUMERIK 840D Programming Manual page 80

2
Drilling Cycles and Drilling Patterns
2.1 Drilling cycles
MPIT and PIT (as thread size and as value)
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.
Right or left threads are specified by the sign of the
pitch parameter:
• Positive value
• Negative value
If the two pitch parameters have contradictory
values, the cycle generates alarm 61001 "Incorrect
pitch" and cycle machining is aborted.
POSS (spindle position)
Before tapping starts in the cycle, oriented spindle stop
is performed with command SPOS and the spindle is
brought into position control.
You program the spindle position for this spindle stop
under POSS.
SST (speed)
Parameter SST contains the spindle speed for the
tapping block with G331.
SST1 (retraction speed)
Under SST1 you program the speed for the retraction
out of the thread hole in the hole with G332.
If this parameter is assigned the value zero, the
retraction movement is performed with the speed
programmed under SST.
_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
2-80
→
right (like M3)
→
left (like M4).
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
2
03.96
09.01
© Siemens AG, 2002. All rights reserved