Siemens SINUMERIK 840D, Operating Manual

Page: 310 / 610

Programming technological functions (cycles)
8.2 Milling
Milling
310
Operating Manual, 03/2010, 6FC5398-7CP20-1BA0
Procedure
1. The part program or ShopMill program to be processed has been
created and you are in the editor.
2. Press the "Milling" softkey.
3. Press the "Groove" and "Circumferential groove" softkeys.
The "Circumferential Groove" 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
F Feedrate mm/min
Parameter Description Unit
FZ
(only for G code)
Depth infeed rate mm/min
in/tooth
Machining 
∇ (roughing)
 ∇∇∇ (finishing)
 ∇ + ∇∇∇ (roughing and finishing) - (only for ShopMill)

∇∇∇ edge (edge finishing) - (only for G code)

Chamfering
FZ Depth infeed rate - (only for ∇ and ∇∇∇) mm/min
Circular pattern 
Full circle
The circumferential grooves are positioned around a full circle. The groove spacing
is uniform and is calculated by the controller.

Pitch circle
The circumferential grooves are positioned around a pitch circle. The groove
spacing can be determined on the basis of angle α2.
X0
Y0
Z0 The positions refer to the center point:
Reference point X
Reference point Y
Reference point Z
mm
mm
mm
N Number of grooves
R Radius of circumferential groove mm
α0 Starting angle Degrees
α1 Opening angle of the groove Degrees
α2 Advance angle - (for pitch circle only) Degrees