HEIDENHAIN TNC 426B (280 472) ISO programming User Manual
Page 190
8 Programming: Cycles
174
STUD FINISHING (Cycle G213)
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
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 rapid traverse
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
8.4 Cy
cles f
or Milling P
o
c
k
ets,
St
uds and Slots
Example NC block:
N35 G213 Q200=2 Q201=-20 Q206=150
Q202=5 Q207=500 Q203=+0 Q204=50
Q216=+50 Q217=+50 Q218=80 Q219=60
Q220=5 Q221=0*
Kkap8.pm6
29.06.2006, 08:06
174