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Welds in Drawings?

ptc-5262290
1-Newbie

Welds in Drawings?

Hey all,

I've modeled welds into my assembly using the Weld Application, and I would like the associated symbols to appear in the drawing I've created for it, however I don't want the weld surface features to appear in the drawing. Currently I'm getting the opposite, with weld's surface features in the drawing with no weld symbols. I've tried to play around with the layer tree to fix this problem, but I've been striking out with it. Any suggestions?

Thanks!


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4 REPLIES 4

UPDATE: The weld symbols are in, however still can't get rid of the weld surfaces. Any help is very appreciated!

Can you just hide (possibly suppress) the feature or does that hide (suppress) the weld spec also?

Creo 2.0:

  1. Go into your layer tree and create a new layer.
  2. Change your selection filter (bottom right of screen) from smart to "quilts".
  3. Pick your welds and it should throw just the weld features and not the annotations onto that layer.
  4. Hide the layer.

You can also right-click cycle through the selections but the first selection may be the weld along with the annotation...just keep cycling through until it highlights just the surface. But the easiest is to change the selection filter to quilts.

Another alternative would be to change the weld feature representation to "light". But that probably defeats what you are trying to do.

I've found it useful to set the def_layer for weld features so that it places all weld annotations and features into a layer. If my memory serves me well, it doesn't separate the annotation from the quilt. Might be worth looking into.

Oh, and don't forget to set HLR for quilts in the properties of your views so they will actually be hidden:

View Properties --> View Display --> Hidden Line Removal For Quilts: Yes.

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