HEIDENHAIN TNC 620 Programming Station, User Manual, Page: 473 / 695

Running CAM programs 12.6
12
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
473
Further adaptations
Take the following points into account with CAM programming:
For slow machining feed rates or contours with large radii,
define the chord error to be only one-third to one-fifth of the
tolerance
T
in Cycle 32. Additionally, define the maximum
permissible point spacing to be between 0.25 mm and 0.5 mm
The geometry error or model error should also be specified to
be very small (max. 1 µm).
Even at higher machining feed rates, point spacings of greater
than 2.5 mm are not recommended for curved contour areas
For straight contour elements, one NC point at the beginning of
a line and one NC point at the end suffice. Avoid the output of
intermediate positions
In programs with five axes moving simultaneously, avoid large
changes in the ratio of path lengths in linear and rotational
blocks. Otherwise large reductions in the feed rate could result
at the tool reference point (TCP)
The feed-rate limitation for compensating movements (e.g. via
M128 F...
, ) should be used only in exceptional cases. The feed-
rate limitation for compensating movements can cause large
reductions in the feed rate at the tool reference point (TCP).
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
Cycle 32 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