Please Note While Programming - HEIDENHAIN TNC 640 User Manual

Cycles: Special Functions | TOLERANCE (Cycle 32, DIN/ISO: G62)

Please note while programming:

With very small tolerance values the machine cannot cut
the contour without jerking. These jerking movements
are not caused by poor processing power in the TNC,
but by the fact that, in order to machine the contour
element transitions very exactly, the TNC might have to
drastically reduce the speed.
Cycle 32 is DEF active which means that it becomes
effective as soon as it is defined in the part program.
The TNC resets Cycle 32 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 32, the TNC reactivates the
tolerance that was predefined by machine parameter.
In a program with millimeters set as unit of measure,
the control interprets the entered tolerance value T in
millimeters. In an inch program it interprets it as inches.
If you transfer a program with Cycle 32 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, unless HSC
filters are active on your machine (set by the machine
tool builder).
If Cycle 32 is active, the TNC shows the parameters
defined for Cycle 32 on the CYC tab of the additional
status display.
NC programs for 5-axis simultaneous machining with
spherical cutters should preferably be output for the
center of the sphere. The NC data are then generally
more consistent. Additionally, in you can set a higher
rotational axis tolerance TA (e.g. between 1° and 3°)
for an even more constant feed-rate curve at the tool
reference point (TCP).
For NC programs for 5-axis simultaneous machining
with toroid cutters or radius cutters where the NC
output is for the south pole of the sphere, choose a
lower rotational axis tolerance. 0.1° is a typical value.
However, the maximum permissible contour damage is
the decisive factor for the rotational axis tolerance. This
contour damage depends on the possible tool tilting,
tool radius and contact depth of the tool.
With 5-axis gear hobbing with an end mill you can
calculate the maximum possible contour damage T
directly from the cutter contact length L and permissible
contour tolerance TA:
T ~ K x L x TA K = 0.0175 [1/°]
Example: L = 10 mm, TA = 0.1°: T = 0.0175 mm
HEIDENHAIN | User's manual for cycle programming | 10/2017
11
321