HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 165)

149 HEIDENHAIN TNC 410, TNC 426, TNC 430
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.
The TNC 426, TNC 430 with NC software 280 474-xx
also provides:
ú Dwell time at depth Q211: time in seconds that the
tool remains at the hole bottom
REAMING (Cycle G201)
1 The TNC positions the tool in the tool axis at rapid traverse to the
input set-up clearance above the workpiece surface.
2 The tool reams to the entered depth at the programmed feed
rate F.
3 If programmed, the tool remains at the hole bottom for the
entered dwell time.
4 The tool then retracts to set-up clearance at the feed rate F, and
from there — if programmed — to the 2nd set-up clearance in
rapid traverse.
Before programming, note the following:
Program a positioning block for the starting point (hole
center) in the working plane with RADIUS
COMPENSATION G40.
The algebraic sign for the depth parameter determines
the working direction.
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 hole
ú Feed rate for plunging Q206: Traversing speed of the
tool during reaming in mm/min
ú Dwell time at depth Q211: Time in seconds that the
tool remains at the hole bottom
ú Retraction feed rate Q208: Traversing speed of the
tool in mm/min when retracting from the hole. If you
enter Q208 = 0, the tool retracts at the reaming feed
rate.
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.
X
Z
Q200
Q201
Q206
Q211
Q203
Q204
Q208
8.3 Dr
illing Cy
cles
Example NC block:
N80 G201 Q200=2 Q201=-20 Q206=150
Q211=0.25 Q208=500 Q203=+0
Q204=50*
Kkap8.pm6 29.06.2006, 08:06 149