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Profile keeps offsetting

Question asked by Hanni Abukhater on Feb 25, 2013
Latest reply on Mar 1, 2013 by Hanni Abukhater

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Hello,

I'm working with Solidworks 2013. I've created a profile and properly uploaded it to the directory as a library feature. I've used weldments before and have never had this problem. As you can see with the attached picture, when I select the line to create the member I encounter an issue with the member offsetting from the line. What's even weirder is that when I repeat the function, the member will offset to a different random distance/direction every time. Anybody have any ideas?

EDIT: I have also drawn the cross section sketch on the front plane, centered on the axis.

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Justin Burton Feb 26, 2013 4:49 AM
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Is there any chance that you could upload your profile and the part in the above picture?
It would make it much easier to see what is wrong. I suspect it is the profile but I cannot be sure from just the picture.

Thanks,
Justin
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Paul Cullen Feb 26, 2013 3:52 PM
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Hi Hanni

Is your weldment profile sketch fully defined, also is it centered at the origin or is it away from the origin.

When you insert a weldment profile solidworks will use the origin of your weldment profile sketch as the default point to align your weldment profile sketch with the line in your 3d / 2d sketch. You can then select locate profile when inserting your profile to select a different reference point if you want to.

Paul
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Hanni Abukhater Feb 27, 2013 1:10 AM
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Yes, the profile is sketched at the center and is fully defined. How do I upload the file? I only see a video and picture upload option. And even if the sketch was off center that wouldn't make much sense because if I repeat the function, the profile is displace in a different direction every time. That's what has me so baffled. It just doesn't add up. I though there might have been an issue with with the sketch I was using the profile on because I used mirrors so I redrew the wireframe without using mirror but ended up with the same result.
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- Justin Burton @ Hanni Abukhater on Feb 27, 2013 4:41 AM
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  Hi,
  
  If you click on "Use advanced editor" when you reply you should see an "Attach files" option at the bottom of the reply panel.
  
  As this seems an odd one, it would be good to get the profile and weldment part, then hopefully we can sort it.
  
  Justin
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  - Hanni Abukhater @ Justin Burton on Feb 27, 2013 5:20 PM
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    Alright, here's the wireframe and the cross section.
    Attachments
    1 x 1.SLDLFP.zip53.2 KB
    Wireframe 2.SLDPRT.zip62.6 KB
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    - Justin Burton @ Hanni Abukhater on Feb 28, 2013 4:47 AM
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      Hi, thanks for the files.
      
      If I use the files as you sent them I get the exact same issue.
      I would have thought that the sketch would be ok, as SW should use the origin as the default profile pierce point. This seems not to be the case for your example...
      
      The issue is that the sketch you created for the profile does not relate to the sketch origin. (you have related the sketch to the planes instead)
      Therefore when you place the weldment the sketch moves away from the profile origin as it is not in any way related.
      
      To fix the issue I would suggest drawing a centre point rectangle or add some construction geometry so that the sketch is positioned in relation to the origin.
      You can check if you have the correct references in the profile sketch. Once the sketch has been saved as a SLDLFP you will be able to see a references folder in the feature manager. Check that there is only Front plane and Sketch Point1 (origin) in the folder. if you select the items in the folder it will highlight where they are in the sketch.
      
      Also I noticed that you used two lines on each edge of the square, I assume this is so that you can poistion the profile in different orientations? If you draw a standard rectangle and add sketch points to the midpoints you should find this quicker and easier to create.
      
      See image below
      
      Thanks,
      Justin
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      - Hanni Abukhater @ Justin Burton on Mar 1, 2013 10:04 AM
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        You were 100% right. I just needed to make some relations to the orgin and it worked like a charm. Thanks a lot you guys, great support!
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