HEIDENHAIN iTNC 530 (340 49x-04) ISO programming - Manual (Page 478)

478 8 Programming: Cycles
8.1
0
Special Cy
cles
Influences of the geometry definition in the CAM system
The most important factor of influence in offline NC program creation
is the chord error S defined in the CAM system. The maximum point
spacing of NC programs generated in a postprocessor (PP) is defined
through the chord error. If the chord error is less than or equal to the
tolerance value T defined in Cycle G62, then the TNC can smooth the
contour points unless any special machine settings limit the
programmed feed rate.
You will achieve optimal smoothing if in Cycle G62 you choose a
tolerance value between 110% and 200% of the CAM chord error.
Programming
X
Z
T
S
CAM TNC PP
Before programming, note the following
Cycle G62 is DEF active which means that it becomes
effective as soon as it is defined in the part program.
The TNC resets Cycle G62 if you
„ Redefine it and confirm the dialog question for the
tolerance value
with NO ENT.
„ Select a new program with the PGM MGT key.
After you have reset Cycle G62, the TNC reactivates the
tolerance that was predefined by machine parameter.
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 it as inches.
If you transfer a program with Cycle G62 that contains only
the cycle parameter Tolerance value T, the TNC inserts
the two remaining parameters with the value 0 if required.
As the tolerance value increases, the diameter of circular
movements usually decreases. If the HSC filter is active
on your machine (ask your machine manufacturer, if
necessary), the circle can also become larger.
If Cycle 62 is active, the TNC shows the parameters
defined for Cycle 32 on the CYC tab of the additional status
display.