Cycle Parameters - HEIDENHAIN TNC 620 User Manual

11

Cycle parameters

Tolerance value T: Permissible contour deviation
in mm (or inches with inch programming). Input
range 0.0000 to 10.0000
>0: With an input value > 0 the TNC uses the
maximum permissible deviation
0
programming you press the NO ENT key, the
TNC uses a value configured by the machine tool
builder
HSC MODE, Finishing=0, Roughing=1: Activate
filter:
Tolerance for rotary axes TA: Permissible
positioning error of rotary axes in degrees when
M128 is active (FUNCTION TCPM). 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 precisely move the
rotary axis to the given nominal position. The tool
orientation (position of the rotary axis with respect
to the workpiece surface) will be adjusted. The
position at Tool Center Point (TCP) is automatically
corrected. With a ball-nose cutter for example,
measured in the center and programmed to the
midpoint path, this has no negative effects on the
contour. Input range 0.0000 to 10.0000
>0: With an input value > 0 the TNC uses the
maximum permissible deviation
0
programming you press the NO ENT key, the
TNC uses a value configured by the machine tool
builder
316
you entered: If 0 is entered or if during
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
you entered: If 0 is entered or if during
Cycles: Special Functions | TOLERANCE (Cycle 32, DIN/ISO: G62)
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
NC blocks
95 CYCL DEF 32.0 TOLERANCE
96 CYCL DEF 32.1 T0.05
97 CYCL DEF 32.2 HSC-MODE:1 TA5