HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 193)

177 HEIDENHAIN TNC 410, TNC 426, TNC 430
CIRCULAR POCKET FINISHING (Cycle G214)
1 The TNC automatically 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 pocket.
2 From the pocket center, the tool moves in the working plane to
the starting point for machining. The TNC takes the workpiece
blank diameter and tool radius into account for calculating the
starting point. If you enter a workpiece blank diameter of 0, the
TNC plunge-cuts into the pocket center.
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 pocket (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 pocket 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 pocket
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
ú Feed rate for milling Q207: Traversing speed of the
tool in mm/min while milling.
8.4 Cy
cles f
or Milling P
o
c
k
ets,
St
uds and Slots
X
Y
X
Z
Q200
Q201
Q206
Q202
Q203
Q204
Example NC block:
N42 G214 Q200=2 Q201=-20 Q206=150
Q202=5 Q207=500 Q203=+0 Q204=50
Q216=+50 Q217=+50 Q222=79 Q223=80*
Kkap8.pm6 29.06.2006, 08:06 177