8 Programming: Cycles
172
STUD FINISHING (Cycle 213)
1 The TNC moves the tool in the tool axis to set-up clearance, or —
if programmed — to the 2nd set-up clearance, and subsequently
to the center of the stud.
2 From the stud center, the tool moves in the working plane to the
starting point for machining. The starting point lies to the right of
the stud by a distance approx. 3.5 times the tool radius.
3 If the tool is at the 2nd set-up clearance, it moves in rapid traverse
FMAX to set-up clearance, and from there advances to the first
plunging depth at the feed rate for plunging.
4 The tool then moves tangentially to the contour of the finished
part and, using climb milling, machines one revolution.
5 After this, the tool departs the contour tangentially and returns to
the starting point in the working plane.
6 This process (3 to 5) is repeated until the programmed depth is
reached.
7 At the end of the cycle, the TNC retracts the tool in FMAX to set-
up clearance, or — if programmed — to the 2nd set-up clearance,
and finally to the center of the stud (end position = starting
position).
Before programming, note the following:
The algebraic sign for the depth parameter determines
the working direction.
If you want to clear and finish the stud with the same
tool, use a center-cut end mill (ISO 1641) and enter a low
feed rate for plunging.
ú Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
ú Depth Q201 (incremental value): Distance between
workpiece surface and bottom of stud
ú
Feed rate for plunging Q206: Traversing speed of the
tool in mm/min when moving to depth. If you are
plunge-cutting into the material, enter a low value; if
you have already cleared the stud, enter a higher feed
rate.
ú
Plunging depth Q202 (incremental value):
Infeed per cut Enter a value greater than 0.
ú
Feed rate for milling Q207: Traversing speed of the
tool in mm/min while milling.
ú
Workpiece surface coordinate Q203 (absolute value):
Coordinate of the workpiece surface
X
Y
X
Z
Q200
Q201
Q206
Q203
Q204
Q202
8.3 Cycle for Milling Pockets, Studs and Slots
Example NC blocks:
35 CYCL DEF 213 STUD FINISHING
Q200=2 ;SET-UP CLEARANCE
Q201=-20 ;DEPTH
Q206=150 ;FEED RATE FOR PLUNGING
Q202=5 ;PLUNGING DEPTH
Q207=500 ;FEED RATE FOR MILLING
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2. SET-UP CLEARANCE
Q216=+50 ;CENTER IN 1ST AXIS
Q217=+50 ;CENTER IN 2ND AXIS
Q218=80 ;1ST SIDE LENGTH
Q219=60 ;2ND SIDE LENGTH
Q220=5 ;CORNER RADIUS
Q221=0 ;ALLOWANCE
kkap8.pm6 30.06.2006, 07:03172
www.EngineeringBooksPdf.com
To Next Page
Loading...
Need help?
General
