Siemens SINUMERIK 828D Operating Manual page 576

Programming technology functions (cycles)
9.7 Additional cycles and functions in ShopTurn
Parameters in the "Input complete" mode
Parameter Description
Input Complete
T Tool name
D Cutting edge number
F Feedrate
S / V Spindle speed or
constant cutting rate
Machining
Chipbreaking
•
Swarf removal
•
Z0 Reference point Z (abs)
Drilling depth Referred to
Shank
•
The drill is inserted until the drill shank reaches the value programmed for Z1. The
angle entered in the tool list is taken into account.
Tip
•
The drill is inserted until the drill tip reaches the value programmed for Z1.
Z1 Final drilling depth (abs) or final drilling depth in relation to Z0 (inc)
D Maximum depth infeed
FD1 Percentage for the feedrate for the first infeed
DF
Percentage for each additional infeed or
•
Amount for each additional infeed
•
DF = 100: Infeed increment remains constant
DF < 100: Infeed increment is reduced in direction of final drilling depth.
Example: DF = 80
Last infeed was 4 mm;
4 x 80% = 3.2; next infeed increment is 3.2 mm
3.2 x 80% = 2.56; next infeed increment is 2.56 mm, etc.
V1 Minimum depth infeed
Parameter V1 is available only if DF<100% has been programmed.
A minimum infeed is programmed using parameter V1.
V2 Retraction distance after each machining step – (only for "chipbreaking" operation)
Clearance dis- - (only for "swarf removal" operation)
tance
Manual
•
Automatic
•
V3 Clearance distance – (for "manual" clearance distance only)
DT
Dwell time in seconds
•
Dwell time in revolutions
•
576
Operating Manual, 01/2015, 6FC5398-8CP40-5BA2
Unit
mm/min
mm/rev
rpm
m/min
%
%
mm
s
rev
Turning