HEIDENHAIN iTNC 530 (340 420) - Manual (Page 387)

HEIDENHAIN iTNC 530 359
8.1
0
Special Cy
cles
TOLERANCE (Cycle 32)
The TNC automatically smoothes the contour between two path
elements (whether compensated or not). The tool has constant
contact with the workpiece surface. If necessary, the TNC
automatically reduces the programmed feed rate so that the program
can be machined at the fastest possible speed without short pauses
for computing time. As a result the surface quality is improved and the
machine is protected.
A contour deviation results from the smoothing. The size of this
deviation (tolerance value) is set in a machine parameter by the
machine manufacturer. With Cycle 32, you can change the pre-set
tolerance value and select different filter settings. 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
Machine and control must be specially prepared by the
machine tool builder for use of this cycle.
The input parameters FINISHING/ROUGHING and TOLERANCE
FOR ROTARY AXES
are effective only if the HSC filter
(software option 2) is active on your machine. The TNC will
otherwise display an error message. If necessary, contact
your machine tool builder.
Before programming, note the following:
Cycle 32 is DEF active which means that it becomes
effective as soon as it is defined in the part program.
You can reset Cycle 32 by defining it again and confirming
the dialog question after the tolerance value with NO
ENT. Resetting reactivates the pre-set tolerance.
In a program with millimeters set as unit of measure, the
TNC interprets the entered tolerance value in millimeters.
In an inch program it interprets them as inches.
The input parameters for finishing/roughing and the
tolerance for rotary axes are effective only if the HSC filter
is active on your machine. If necessary, contact your
machine tool builder.