HEIDENHAIN TNC 620 (340 56x-01) - Manual (Page 368)

368
8.8 Special Cy
cles
 Tolerance value T: Permissible contour deviation in
mm (or inches with inch programming)
 HSC MODE, Finishing=0, Roughing=1: Activate filter:
„ Input value 0:
Milling with increased contour accuracy. The
TNC uses the filter settings that your machine tool
builder has defined for finishing operations.
„ Input value 1:
Milling at an increased feed rate. The TNC uses
the filter settings that your machine tool builder has
defined for roughing operations. The TNC works
with optimal smoothing of the contour points,
which results in a reduction of the machining time
 Tolerance for rotary axes TA: Permissible position
error of rotary axes in degrees when M128 is active.
The TNC always reduces the feed rate in such a way
that—if more than one axis is traversed—the slowest
axis moves at its maximum feed rate. Rotary axes are
usually much slower than linear axes. You can
significantly reduce the machining time for programs
for more than one axis by entering a large tolerance
value (e.g. 10°), since the TNC does not always have
to move the rotary axis to the given nominal position.
The contour will not be damaged by entering a rotary
axis tolerance value. Only the position of the rotary
axis with respect to the workpiece surface will
change.
Example: NC blocks
95 CYCL DEF 32.0 TOLERANCE
96 CYCL DEF 32.1 T0.05
97 CYC DEF 32.2 HSC MODE:1 TA5
The HSC MODE and TA parameters are only available if on
your machine you have software option 2 active (HSC
machining).