Re: CATIA Model Tolerancing

From: Advantage Prototype systems (
Date: Mon May 08 2000 - 23:01:15 EEST

Thanks (for all) but its the first line that shivers the timbers. 'Once in CATIA".
Tom Husting
    -----Original Message-----
    From: Bruce Okkema <>
    To: RP Mail List <>
    Date: Monday, May 08, 2000 2:39 PM
    Subject: CATIA Model Tolerancing
    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.
    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"
    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
    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 Okkema, President
    Eagle Design & Technology, Inc.
    2437 84th Avenue
    Zeeland, MI 49464
    Ph: 616-748-1022 Fx: 616-748-1032

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