Siemens SINUMERIK 808D Programming And Operating Manual page 143

"Drilling a left-hand thread without any compensating chuck" cycle (G74):
Explanations
The cycle creates the following sequence of motions:
● Approach of reference plane shifted by the amount of the safety clearance with G0.
● Oriented spindle stop and transfer of spindle in the Axis mode.
● Tapping to the final drilling depth.
● Execution of dwell time at thread depth.
● Retraction to the reference plane and reversion of direction of rotation brought forward by the safety clearance.
● Retraction to the retraction plane with G0.
During tapping, rapid traverse override and spindle override are accepted at 100%.
The speed of rotation can be affected during the retraction with GUD _ZSFI[2]. Example: _ZSFI[2]=120; the retraction takes
place at 120% of the speed during tapping.
Restrictions
None.
Changeover of the axes
Before changing over the drilling axis, one must first deselect the fixed cycle. An alarm is output if the drilling axis in the
"Drilling without compensating chuck" mode is changed over.
Tapping
The drilling cycle is executed only if an axis motion, e.g. is programmed with X, Y, Z or R.
R
Always program R only in one block with an axis motion, otherwise the programmed values are not stored modally.
Deselection
The G functions of Group 01 (G00 to G03) and G74 should not be used together in one block, as otherwise G74 is
deselected.
Programming and Operating Manual (ISO Turning/Milling)
143
01/2017