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ptc-62953941-Visitor
1-Visitor
September 10, 2014
Question

Removing hidden welds in drawing sections?

  • September 10, 2014
  • 23 replies
  • 15559 views

(Creo Parametric 2)
I am having trouble with hiding/removing a hidden weld in a section in drawing view.

With a normal projected view, I would simply select "Yes" for "Hidden line removal for quilts" in the drawing view properties.

However when I have a section view, this option is greyed out, leaving welds which should be hidden visible.

 

How do I go about hiding these, either as a general setting for the view or as a manual deleting process?

 

Many thanks


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23 replies

dschenken1-Visitor
1-Visitor
September 10, 2014

The option has to be chosen when you create the section. I think it cannot be redefined after, but it is easy enough to create a new, coincident section and replace the existing one. Once replaced, delete the original section and then rename the new one to the original name.

    ptc-62953941-VisitorAuthor
    1-Visitor
    September 11, 2014

    Which option is it that has to be chosen when it is created?

    I already tried simply selecting "Yes" for "hidden line removal for quilts", before creating the section, however it reverted to "No" when it greyed out..

    Cheers

    dschenken1-Visitor
    1-Visitor
    September 11, 2014

    When you create the section in the model, there is the option to include quilts.

    This is not the same as creating a section view in the drawing.

    TomD.inPDX17-Peridot
    17-Peridot
    September 10, 2014

    Welcome to the forum, Simon.

    Welds being quilts is problematic no matter how you deal with them.

    I don't use the intelligent layers and I rarely need to show model quilts in any view... except for the weld that may be required in only one view (spot or seem welds).

    However, I do create a layer in the model called HIDE_WELDS to specifically turn these layers of in specific views. By managing layers by view, or drawing, there are fewer issues with model layer states. I suppose you could reverse this and use SHOW_WELDS but that means your model will have to hide them by default. I never liked things popping into drawings that are suppose to be hidden. All too often I check a drawing that has been ECO'd only to find a completely unrelated view change visibility of features.

    flopes-31-Visitor
    1-Visitor
    November 28, 2014

    Hi,

    try right click on the view, and select "erase cosmetic"

    picture.png

      ecosta-21-Visitor
      1-Visitor
      January 6, 2015

      Fernando Lopes,

      Thanks, it's so useful for me. I was searching for this command.

        gfraulini17-Peridot
        17-Peridot
        July 22, 2016

        Hi all,

        I use WF 5 and in the case you have a section with weld feature, the only manner to to hide them is to create a layer with the welding feature inside and then hide the layer referred with that particular view.

        Bye

        gfraulini17-Peridot
        17-Peridot
        July 22, 2016

        Sorry, in the photo I've searched for "welding feature". It works but if you hide the feature I can't visualize the welding note.

        You have to search for "Fillet weld".

        Bye

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