Having been asked a few times recently how to change CATIA's model
tolerance,
I thought it may be useful information to share with the list.
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It is fairly easy to change the model tolerance in CATIA.
Once in CATIA --
chose STANDARD | MODEL.
Go to the page 2 of 2 where it reads GEOMETRIC STANDARDS
and change only the bottom value labeled "MODEL DIMENSION"
(One will see the Warning: "MODIFYING THESE VALUES MAY LEAD TO UNPREDICTABLE
RESULTS"
I smile and say as far as RP is concerned "NOT MODIFYING THESE VALUES MAY
LEAD TO
UNPREDICTABLE RESULTS" But do only change the MODEL DIMENSION value and let
the others
remain at their calculated value or you will get unpredictable results.)
The default value for MODEL DIMENSION is 10000 for MM or 393.7008
for inches.
note that changing the MODEL DIMENSION value adjusts all the other
values. The most applicable
value is IDENTICAL CURVES. The default value will be .1000000 for
MM or .0039370 for inch.
The effect of this means there could be a gap of up to .003936"
between curves, but they would be
considered closed within CATIA; if the data is exported to other
Software Packages will be seen as
a gap unless it is smaller than their acceptable gap.
I suggest changing the MODEL DIMENSION value to 800 for MM or 30 for
inch. You will note the
IDENTICAL CURVES value will be significantly reduced and this is the
size that determines how much
of a gap will be accepted as closed. These smaller values will
usually yield good translations into
Pro/E and SolidWorks.
Note that changing the MODEL DIMENSION value will NOT effect or tighten any
geometry created prior to the
value change, but it is likely that much of the existing geometry will
comply, depending on construction
methods.
To find those faces that don't comply, one can toggle between dynamic
shading and wireframe modes,
watching for elements that "disappear" when shaded. Those faces will have
gaps between the boundary
curves greater than the value currently set in IDENTICAL CURVES.
To repair these, re-create the boundary curves with the new tolerance
settings.
The best test to validate your CATIA data is to create a volume under the
tighter tolerance settings.
If you will be translating your data out, make sure the model is saved with
the tighter tolerance settings.
Beyond this there are other methods, but only fairly experienced CATIA users
might understand.
We have realized very good success by following the above procedure.
We always do our CATIA design work with these tight tolerances unless we
have to export data which
must comply with a company's internal CATIA standards such as
Daimler-Chrysler or Boeing.
Best Regards,
Bruce
_________________________________________________________________________
Bruce Okkema, President
Eagle Design & Technology, Inc.
2437 84th Avenue
Zeeland, MI 49464
Ph: 616-748-1022 Fx: 616-748-1032
email: bruceo@eagledesign.com
web: eagledesign.com
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