Drill And Thread Milling - Siemens SINUMERIK 840D Operation/Programming Manual

3
Programming with ShopMill
3.7 Drilling

3.7.7 Drill and thread milling

Cut thread
3-242
You can use a drill and thread milling cutter to manufacture an internal
thread with a specific depth and pitch in one operation. This means
that you can use the same tool for drilling and thread milling, a change
of tool is superfluous.
The thread can be machined as a right- or left-hand thread.
Sequence:
• The tool travels at rapid traverse to the safety distance.
• If pre-drilling is required, the tool travels at a reduced drilling
feedrate to the pre-drilling depth defined in a machine data.
Please refer to the machine manufacturer's instructions.
• The tool drills to the first drilling depth D with drilling feedrate F1. If
the final drilling depth is not reached, the tool will travel back to the
workpiece surface in rapid traverse for stock removal. Then the
tool will travel at rapid traverse to a position 1mm above the drilling
depth previously achieved - allowing it to continue drillling at drill
feedrate F1 at the next infeed.
• If another feedrate FR is required for through-boring, the residual
drilling depth ZR is drilled with this feedrate.
• If required, the tool travels back to the workpiece surface for stock
removal before thread milling at rapid traverse.
• The tool travels directly to the starting position for thread milling.
• The thread milling is carried out (climb milling, conventional milling
or conventional milling + climb milling) with milling feedrate F2. The
thread milling acceleration path and deceleration path is traversed
in a semicircle with concurrent infeed in the tool axis.
Press the "Drilling", "Thread" and "Cut thread" softkeys.
Thread
>
SINUMERIK 840D/840Di/810D Operation/Programming ShopMill (BAS) – 10.04 Edition
3
10.04
 Siemens AG, 2004. All rights reserved