Siemens SINUMERIK 840D, Operating Manual

Page: 268 / 610

Programming technological functions (cycles)
8.1 Drilling
Milling
268
Operating Manual, 03/2010, 6FC5398-7CP20-1BA0
8.1.3 Drilling (CYCLE82)
Function
With the "Drilling" function, the tool drills with the programmed spindle speed and feedrate
down to the specified final drilling depth (shank or tip).
The tool is retracted after a programmed dwell time has elapsed.
Approach/retraction
1. The tool moves with G0 to safety clearance of the reference point.
2. The tool is inserted into the workpiece with G1 and the programmed feedrate F until it
reaches the programmed final depth Z1.
3. When a dwell time DT expires, the tool is retracted at rapid traverse G0 to the retraction
plane.
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 "Drilling Reaming" softkey.
4. Press the "Drilling" softkey.
The "Drilling" input window opens.
Parameters, G code program Parameters, ShopMill program
PL Machining plane T Tool name
RP Retraction plane mm D Cutting edge number
SC Safety clearance mm F Feedrate mm/min
mm/rev
S / V Spindle speed or constant
cutting rate
rpm
m/min
Parameter Description Unit
Machining
position (only
for G code)
 Single position
Drill hole at programmed position
 Position pattern
Position with MCALL
Z0 (only for G
code)
Reference point Z mm