HEIDENHAIN iTNC 530 (340 49x-06) Cycle programming - Manual (Page 310)

310 Cycles: Special Functions
12.5 T
O
LERANCE (Cy
c
le 32, DIN/ISO: G62)
Cycle parameters
U Tolerance value T : Permissible contour deviation in
mm (or inches with inch programming). Input range
0 to 99999.9999
U HSC MODE, Finishing=0, Roughing=1 : Activate filter:
„ Input value 0:
Milling with increased contour accuracy. The
TNC uses internally defined finishing filter settings
„ Input value 1:
Milling at an increased feed rate. The TNC uses
internally defined roughing filter settings
U Tolerance for rotary axes TA : Permissible position
error of rotary axes in degrees when M128 is active
(TCPM FUNCTION). 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. Input range 0 to
179.9999
Example: NC blocks
95 CYCL DEF 32.0 TOLERANCE
96 CYCL DEF 32.1 T0.05
97 CYCL 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).