Siemens SINUMERIK 840D, Operating Manual

Page: 271 / 610

Programming technological functions (cycles)
8.1 Drilling
Milling
Operating Manual, 03/2010, 6FC5398-7CP20-1BA0
271
Approach/retraction during chipbreaking
1. The tool moves with G0 to safety clearance of the reference point.
2. The tool drills with the programmed spindle speed and feedrate F = F · FD1 [%] up to the
1st infeed depth.
3. Dwell time at drilling depth DTB.
4. The tool is retracted by retraction distance V2 for chipbreaking and drills up to the next
infeed depth with programmed feedrate F.
5. Step 4 is repeated until the final drilling depth Z1 is reached.
6. Dwell time at final drilling depth DT.
7. The tool retracts to the retraction plane at rapid traverse.
Approach/retraction during stock removal
1. The tool moves with G0 to safety clearance of the reference point.
2. The tool drills with the programmed spindle speed and feedrate F = F · FD1 [%] up to the
1st infeed depth.
3. Dwell time at drilling depth DTB.
4. The tool retracts from the workpiece for the stock removal with rapid traverse to the safety
clearance.
5. Dwell time at starting point DTS.
6. Approach of the last drilling depth with G0, reduced by the clearance distance V3.
7. Drilling is then continued to the next drilling depth.
8. Steps 4 to 7 are repeated until the programmed final drilling depth Z1 is reached.
9. The tool retracts to the retraction plane at rapid traverse.
Procedure
1. The part program or ShopMill program to be processed has been
created and you are in the editor.
2. Press the "Drilling" softkey.
3. Press the "Deep-hole drilling" softkey.
The "Deep-hole Drilling" input window opens.
Parameters, G code program Parameters, ShopMill program
PL Machining plane T Tool name
Milling direction D Cutting edge number
RP Retraction plane mm F Feedrate mm/min
mm/rev
SC Safety clearance mm S / V Spindle speed or constant cutting
rate
rpm
m/min