Siemens SINUMERIK 840D sl Operating Manual page 495

5. Thread cutting along a spiral path in clockwise or counter-clockwise direction (depending
on whether it is left-hand/right-hand thread, for number of cutting teeth of a milling plate
(NT) ≥ 2 only one rotation, offset in the Z direction).
To reach the programmed thread length, traversing is beyond the Z1 value for different
distances depending on the thread parameters.
6. Exit motion along a circular path in the same rotational direction at programmed feedrate.
7. With a programmed number of threads per cutting edge NT > 2, the tool is fed in (offset)
by the amount NT-1 in the Z direction. Points 4 to 7 are repeated until the programmed
thread depth is reached.
8. If the plane infeed is less than the thread depth, points 3 to 7 are repeated until the thread
depth + programmed allowance is reached.
9. Retract on the thread center point and then to retraction plane in the tool axis in rapid
traverse.
Please note that when milling an internal thread the tool must not exceed the following value:
Milling cutter diameter < (nominal diameter - 2 · thread depth H1)
Approach/retraction when milling external threads
1. Positioning on retraction plane with rapid traverse.
2. Approach of starting point of the approach circle in the current plane with rapid traverse.
3. Infeed to a starting point in the tool axis calculated internally in the controller with rapid
traverse.
4. Approach motion to thread core diameter on an approach circle calculated internally in the
controller with the programmed feedrate, taking into account the finishing allowance and
maximum plane infeed.
5. Cut thread along a spiral path in clockwise or counter-clockwise direction (depending on
whether it is left-hand/right-hand thread, with NT ≥ 2 only one rotation, offset in Z direction).
To reach the programmed thread length, traversing is beyond the Z1 value for different
distances depending on the thread parameters.
6. Exit motion along a circular path in opposite rotational direction at programmed feedrate.
7. With a programmed number of threads per cutting edge NT > 2, the tool is fed in (offset)
by the amount NT-1 in the Z direction. Points 4 to 7 are repeated until the programmed
thread depth is reached.
8. If the plane infeed is less than the thread depth, points 3 to 7 are repeated until the thread
depth + programmed allowance is reached.
9. Retraction on the retraction plane in the tool axis with rapid traverse.
Turning
Operating Manual, 05/2017, A5E40868721
Programming technology functions (cycles)
10.4 Milling
495