Siemens SINUMERIK 840D, Operating Manual

Page: 281 / 610

Programming technological functions (cycles)
8.1 Drilling
Milling
Operating Manual, 03/2010, 6FC5398-7CP20-1BA0
281
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
F1 Drilling feedrate mm/min
mm/rev
Z0 (only for G
code)
Reference point Z mm
Z1 Thread length (inc) or end point of the thread (abs)
D Maximum depth infeed

D ≥ Z1: Infeed to the final drilling depth

D < Z1: Several infeeds with stock removal
DF 
Percentage for each additional infeed
DF=100: Amount of infeed remains constant
DF<100: Amount of infeed is reduced in direction of final drilling depth Z1
Example: last infeed 4 mm; DF 80%
next infeed = 4 x 80% = 3.2 mm
next but one infeed = 3.2 x 80% = 2.56 mm etc.
 Amount for each additional infeed
%
mm
V1 Minimum infeed - (only for DF, percentage for each additional infeed)
Parameter V1 is only provided if DF< 100 has been programmed.
If the amount of infeed becomes very small, a minimum infeed can be programmed in
parameter "V1".

V1 < amount of infeed: The tool is inserted by the infeed amount
 V1 > amount of infeed: The tool is inserted by the infeed value programmed under
V1.
mm
Predrilling Predrilling with reduced feedrate

Yes
 No
The reduced drilling feedrate is obtained as follows:
Drilling feedrate F1 < 0.15 mm/rev: Predrilling feedrate = 30% of F1
Drilling feedrate F1 ≥ 0.15 mm/U: Predrilling feedrate = 0.1 mm/rev
AZ (only for G
code)
Predrilling depth with reduced drilling feedrate (inc) - ("yes", only for pre-drilling)