HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 174)

8 Programming: Cycles 158
ú Set-up clearance Q200 (incremental value): Distance
between tool lower edge 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 helical drilling in mm/min
ú Infeed per helix Q334 (incremental): depth of the tool
plunge with each helix (=360°).
Note that if the infeed distance is too large, the tool or
the workpiece may be damaged.
To prevent the infeed within safe limits, enter the max.
plunge angle of the tool in the tool table, column ANGLE
(see section 5.2 ”Tool Data”). The TNC then calculates
automatically the max. infeed permitted and changes
your entered value accordingly.
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 Nominal diameter Q335 (absolute): Bore-hole
diameter. If you have entered the nominal diameter to
be the same as the tool diameter, the TNC will bore
directly to the entered depth without any helical
interpolation.
8.3 Dr
illing Cy
cles
Example NC block:
N12 G208 Q200=2 Q201=-80 Q206=150
Q334=1.5 Q203=+0 Q204=50 Q335=25*
Kkap8.pm6 29.06.2006, 08:06 158