HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 170)

8 Programming: Cycles 154
ú Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
ú Depth of counterbore Q249 (incremental value):
Distance between underside of workpiece and the
top of the hole. A positive sign means the hole will be
bored in the positive spindle axis direction.
ú Material thickness Q250 (incremental value): Thickness
of the workpiece
ú Off-center distance Q251 (incremental value): Off-
center distance for the boring bar; value from tool data
sheet
ú Tool edge height Q252 (incremental value): Distance
between the underside of the boring bar and the main
cutting tooth; value from tool data sheet
ú Feed rate for pre-positioning Q253: Traversing speed
of the tool when moving in and out of the workpiece,
in mm/min
ú Feed rate for counterboring Q254: Traversing speed of
the tool during counterboring in mm/min
ú Dwell time Q255: Dwell time in seconds at the top of
the bore hole
ú Workpiece surface coordinate Q203 (absolute value):
Coordinate of the workpiece surface
ú 2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision
between tool and workpiece (clamping devices) can
occur.
ú Disengaging direction (0/1/2/3/4) Q214: Determine the
direction in which the TNC displaces the tool by the
off-center distance (after spindle orientation).
1: Displace tool in the negative main axis direction
2: Displace tool in the negative secondary axis direction
3: Displace tool in the positive main axis direction
4: Displace tool in the positive secondary axis direction
Danger of collision!
Check the position of the tool tip when you program a
spindle orientation to 0° (for example, in the Positioning
with Manual Data Input mode of operation). Align the
tool tip so that it is parallel to a coordinate axis. Select a
disengaging direction in which the tool can plunge into
the hole without danger of collision.
The TNC 426, TNC 430 with NC software 280 474-xx
also provides:
ú Angle for spindle orientation Q336 (absolute): angle at
which the TNC positions the tool before retracting it.
8.3 Dr
illing Cy
cles
X
Z
Q250
Q203
Q204
Q249
Q200
Q200
X
Z
Q255
Q254
Q214
Q252
Q253
Q251
Example NC block:
N11 G204 Q200=2 Q249=+5 Q250=20
Q251=3.5 Q252=15 Q253=750 Q254=200
Q255=0 Q203=+0 Q204=50 Q214=1*
Kkap8.pm6 29.06.2006, 08:06 154