Programming technology functions (cycles)
8.7 Additional cycles and functions in ShopTurn
Turning
492 Operating Manual, 03/2013, 6FC5398-8CP40-3BA1
Procedure
1. The ShopTurn program to be edited has been created and you are in
the editor.
2. Press the "Drilling" and "Drill centric" softkeys.
The "Drilling centered" input window opens.
Parameters Description Unit
T Tool name
D Cutting edge number
F Feedrate mm/min
mm/rev
S / V Spindle speed or
constant cutting rate
rpm
m/min
Machining
• Chipbreaking
• Stock removal
Z0 Reference point Z
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 X (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.
%
mm
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)
To Next Page
Loading...
