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Craig_Euro1-Visitor
1-Visitor
November 8, 2017
Question

How do you stop two extrudes merging in a single part file

  • November 8, 2017
  • 13 replies
  • 10104 views

In a single part file I want to create a fabricated hollow section framework built up of many extruded features. The problem is that each extrude is automatically merged together where they touch showing no join line. I would like all the join lines to show up in the part model and drawing file so that the welding fabricator can see where and how I would like the frames to be welded. For example, 90 degree connections or mitred corners. I basically don't want each extrude to join up automatically. I know leaving a very tiny gap at each connection will stop this happening but this can't be good practice and is time consuming process.

I don't want to have to create an assembly of all the various tube lengths so that they show up seperately.

13 replies

StephenW
StephenW23-Emerald III
23-Emerald III
November 8, 2017

What you are looking for is multi-body parts. That is NOT something that Creo does.

In Creo your process would be to build all the components as parts and use an assembly to put them all together.

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Craig_Euro1-VisitorAuthor
1-Visitor
November 8, 2017
Spoiler
Thanks for the fast response Stephen.
I knew about the option of making it an assembly but it's not realy what I wanted. This would mean that for a large frame, each length of tubing would require a part number and storing correctly on our Windchill server. I was trying to avoid this. I just want to make frame structures made from many extrusions. This is how I used to do it in Unigraphics NX. Look like I am stuck with the assembly option:Smiley Sad
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    BenLoosli23-Emerald III
    23-Emerald III
    November 8, 2017

    NX (Parasolid) allows multi-part bodies in a single file. Creo (Granite One) does not.

    We had the same issue where I used to work with welded structures when we switched from Unigraphics to Pro/Engineer. We would model the welded structure in a single UG part file made up of multiple extrudes. When we switched to Pro/E, we had to do the individual tube files and an assembly for the welded structure. We just assigned (-xx) part number suffixes to the tubes and did not use them in any other assemblies. If we needed the same size tube for another assembly, it was either remodeled or we did a save-as. Since we were building to manufacturing orders, we did not stock (or sell replacements) the tubes.

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    LndoVnBtchmrk12-Amethyst
    12-Amethyst
    November 8, 2017

    I've used multi-body "parts" for rough concepting work.  I'll make each extrude/revolve/sweep/etc. a surface feature with capped ends.  The features won't merge into each other without you telling them to (via quilt merge).

     

    I use this method just to quickly iterate a design to see what's possible.  After I settle on a direction I may use the surface model as a skeleton to create individual parts.

     

    A couple downsides to this method is that you won't be able measure any mass properties or generate BOM's from the surface model.  Works for me since I don't need those for concepting.

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      Craig_Euro1-VisitorAuthor
      1-Visitor
      November 9, 2017

      I tried the surfaces and capped ends and you are right, it will work for concept work. I will be able to use this for some of my projects. It's a shame that it does not let you add holes into the frames for fixing outside guarding to and other items.

       

      Great suggestion, thanks.

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      dschenken1-Visitor
      1-Visitor
      November 8, 2017

      You can model using gaps, which will typically be present in pre-weld fitups. Alternatively create datum curves to represent the separations. Both are more tedious than a feature that Creo doesn't have, but they are available.

       

      Keep in mind that in an actual weldment there will be no gap and it will tend to look the way that Creo defaults to.

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      Craig_Euro1-VisitorAuthor
      1-Visitor
      November 9, 2017

      I have used gaps before and also thought about curves. Like you say, they take a little longer.

      I only tended to use a very small gap that is hardly visible. I am trying to go away from this method.

       

      Thank you.

      StephenW
      StephenW23-Emerald III
      23-Emerald III
      November 9, 2017

      You are killing your productivity by trying to use Creo like NX. All the time you save in managing only one part in windchill is lost in the modeling. And if another user ever has to work on the model who doesn't understand your hybrid NX-Creo modeling, it'll be a complete redo, ie more time wasted.

       

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      dgschaefer21-Topaz II
      21-Topaz II
      November 8, 2017

      Have you looked at AFX (advanced framework extension)?  All seats include a "lite" version which includes full functionality but assemblies are limited to 20 items.  With some creativity in splitting your assy up into sub-assys, you can get around that.

       

      It's made for welded tube structures and has all the features for placing them and doing all the miter cuts.  It's a bit quirky, but if you look up the how to videos on the Learning Exchange and you should be able to pick it up pretty quickly.

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      Craig_Euro1-VisitorAuthor
      1-Visitor
      November 9, 2017

      I'm fairly new to Ceo so I hadn't tried the AFX feature. I gave it a go and managed to create some frames, corners, move pieces etc. so I now know what it's capable of. I have some extra training in the New Year planned so I will request the AFX to be added to the training material.

      It still only works in assembly mode and makes all the pieces individual parts but it looks quit good. In a part file the framework menu is not available.

       

      Thanks Doug.

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      dgschaefer21-Topaz II
      21-Topaz II
      November 9, 2017

      You're welcome.  Keep in mind that you'll need a full license (extra cost) to eliminate the 20 part per assy (or per session) limit.  Also, I'm not sure how easy it is to implement your start parts on the AFX template files or to add profiles.  

       

      However, it works pretty well and you can layout tubular frameworks pretty quickly.

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