Siemens SINUMERIK 840D sl Turning Operating Manual page 503

Parameter Description
Insertion Various insertion modes can be selected – (only for plane-by-plane machining method
and for ∇, ∇∇∇ and ∇∇∇ edge):
● Predrilled (only for G code)
● Vertical: Insert vertically at center of pocket
The tool executes the calculated depth infeed vertically at the center of the pocket.
Feedrate: Infeed rate as programmed under FZ
● Helical: Insert along helical path
The cutter center point traverses along the helical path determined by the radius and
depth per revolution. If the depth for one infeed has been reached, a full circle motion
is executed to eliminate the inclined insertion path.
Feedrate: Machining feedrate
Note: The vertical insertion into pocket center method can be used only if the tool can
cut across center or if the workpiece has been predrilled.
Clamp/release spindle (only for end face C/peripheral surface C, if inserted vertically)
The function must be set up by the machine manufacturer.
(only for Shop‐
Turn)
FZ Depth infeed rate – (for vertical insertion only)
(only for G code)
FZ Depth infeed rate – (for vertical insertion only)
(only for Shop‐
Turn)
EP Maximum pitch of helix - (for helical insertion only)
The helix pitch may be lower due to the geometrical situation.
ER Radius of helix - (only for helical insertion)
The radius must not be larger than the milling cutter radius, otherwise material will remain.
Also make sure the circular pocket is not violated.
Solid machining
● Complete machining
The circular pocket must be milled from a solid workpiece (e.g. casting).
● Post machining
(only for G code)
A small pocket or hole has already been machined in the workpiece, which needs to
be enlarged. Parameters AZ, and ∅1 must be programmed.
FS Chamfer width for chamfering - (for chamfering only)
ZFS Insertion depth of tool tip (abs or inc) - (for chamfering only)
AZ Depth of premachining - (for remachining only)
(only for G code)
∅1 Diameter of premachining - (for remachining only)
(only for G code)
* Unit of feedrate as programmed before the cycle call
Turning
Operating Manual, 06/2019, A5E44903486B AB
Programming technology functions (cycles)
10.4 Milling
Unit
*
mm/min
mm/tooth
mm/rev
mm
mm
mm
mm
mm
503