Siemens SINUMERIK 840D, Operating Manual, Page: 365 / 610

Programming technological functions (cycles)
8.4 Turning - only for G code programs
Milling
Operating Manual, 03/2010, 6FC5398-7CP20-1BA0
365
8.4.6 Thread turning (CYCLE99)
Function
You can use the "Longitudinal thread", "Tapered thread" or "Face thread" cycle to turn
external or internal threads with a constant or variable pitch.
There may be single or multiple threads.
For metric threads (thread pitch P in mm/rev), the cycle assigns a value (calculated on the
basis of the thread pitch) to the thread depth H1 parameter. You can change this value.
The default must be activated via setting data SD 55212
$SCS_FUNCTION_MASK_TECH_SET.
Machine manufacturer
Please refer to the machine manufacturer's specifications.
The cycle requires a speed-controlled spindle with a position measuring system.
Thread re-machining
You have the option of subsequently machining threads. To do this, change into the "JOG"
operating mode and carry out a thread synchronization.
Approach/retraction
1. The tool moves to the starting point calculated internally in the cycle at rapid traverse.
2. Thread with advance:
The tool moves at rapid traverse to the first starting position displaced by the thread
advance LW.
Thread with run-in:
The tool moves at rapid traverse to the starting position displaced by the thread run-in
LW2.
3. The first cut is made with thread pitch P as far as the thread run-out LR.
4. Thread with advance:
The tool moves at rapid traverse to the return distance VR and then to the next starting
position.
Thread with run-in:
The tool moves at rapid traverse to the return distance VR and then back to the starting
position.
5. Steps 3 and 4 are repeated until the thread is finished.
6. The tool moves back to the retraction plane at rapid traverse.
Thread machining can be stopped at any time with the "Rapid lift" function. It ensures that
the tool does not damage the thread when it is raised.