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ptc-42454671-Visitor
1-Visitor
January 29, 2013
Question

Foreshortened Radii and Linear Dimensions

  • January 29, 2013
  • 2 replies
  • 12074 views

I am running Creo Parametric 2.0 M030. How do I convert / make a shown model annotation on my drawing into a foreshortened dimension. I have two radii and a linear dimension that I would like to do this to. Using the Z-radius dimension is not an option (however the result of using this is the result I am looking for) and I am also not interested in some "workaround" that involves drawing a bunch of lines and other garbage on my drawing with a sketch. These dimensions need to be shown model annotations, no added dimensions are acceptable. See attached model and drawing. Sorry if I seem angry...Creo Parametric will do this to you.


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    2 replies

    J
    James621-Visitor
    1-Visitor
    January 29, 2013

    Well, the following picture shows you the way how you should go on with this.

    bug on overwritten drawing dim.JPG

    But it's buggered as you can see, and I have no idea how to get dim tol limits into model parameters. With dimension tolerance limit params you would be able to use those instead of the dimension parameter.

    I guess with the bug there, your only option now is to write the stuff you want in the Z-rad dims manually behind the @O... The linear dim should work this way without a problem.

    T
    TomD.inPDX17-Peridot
    17-Peridot
    January 30, 2013

    Jakub is almost there. Yes, this is still a bug in M030 but you can get around it easily.

    On the original dimension d6, remove the "prefix [R]" and add the R before the @D => R@D

    Now you can create drafting Z-Radius dimension and overwrite the drafting value with R&d6@O

    Someone really messed up the whole dimension formatting code somewhere along the Creo conversion. PTC development needs to go back to the original code and do a careful compare. Band-Aids are just not stopping the bleeding.

    T
    TomD.inPDX17-Peridot
    17-Peridot
    January 30, 2013

    foreshortening_dims.JPG

    The z-radius are re-associated to the original model dimension.

    The linear dimension had the extension line erased which created the double arrow. After that, you can move the double arrow with the handle.

    Files attached (Creo 2.0 M030)

    P
    ptc-42454671-VisitorAuthor
    1-Visitor
    January 30, 2013

    Is there a way to put the "Z" zig zag like the Z-Radius dim into the linear dim?

    T
    TomD.inPDX17-Peridot
    17-Peridot
    January 30, 2013

    Although very appropriate on broken views, it has never been implemented as far as I know.

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