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gcontreras1-Visitor
1-Visitor
October 20, 2014
Solved

Schweißnaht--Weldseam

  • October 20, 2014
  • 9 replies
  • 7217 views

Hello,

i have a question with the weldseam from creo. I use Creo 2.0 and my model have been welded. I would like to know if there is a tool that can measure the length of the whole weldseam (schweißnaht), like the sum of all it. If there is a parameter or something in which it could be meassured, without needing to be meassuring one by one.

Thanks a lot.

Best regards,

Edna García

    Best answer by TomD.inPDX

    On further testing, you cannot do analysis on reference features which is strange.

    In this case, you will have to select measure analysis references for all your welds.

    Below is a video of the process to convert a measurement to a relation and annotation.

    9 replies

    KaelLizak16-Pearl
    16-Pearl
    October 20, 2014

    Hello Garcia,

    You have posted this question in the Integrity Community, rather than the Creo Community. I have moved it into the Creo Community for you.

    Regards,

    Kael

      TomD.inPDX17-Peridot
      17-Peridot
      October 20, 2014

      You can save an analysis value. To best manage the weld edge references, you can make a intent feature from the edges used in the weld and use that for the analysis (length measurement). You can then create a parameter from the analysis feature. You might consider using a "post regen" option on the parameter.

        gcontreras1-VisitorAuthor
        1-Visitor
        October 21, 2014

        thanks! What do you mean with an "intent feature" how can I do that? I´m already in parameter and selected all the edges which are welded, but I´m lost there. I can´t create the parameter.

        And sorry for the multiple questions, but how can I save the analysis value? I have seen it before, but now I can´t manage to save this value.

        Thank you very much!!

        TomD.inPDX17-Peridot
        17-Peridot
        October 21, 2014

        An intent feature is a datum reference. Under the datum drop-down, pick reference. You can select a reference type and create a sort of group of features. This will be saved in the model tree.

        The analysis in your care is a length measurement of the reference. If you select the save option, it becomes a feature.

        To use the analysis feature, create a relation; say weldlength=... here you use the parameter button in the relation dialog (the [ ] button) and select "feature" and pick the analysis result in the model tree. This will show you the analysis feature ID and you can insert it in your relation window using the button at the bottom.

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