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GrahameWard1-Visitor
1-Visitor
May 3, 2013
Solved

Sheet metal part won't regenerate

  • May 3, 2013
  • 5 replies
  • 2827 views

I have two sheet metal parts that are mirror images of each other and refer back to an External Copy Geometry. The one on the right works, the one on the left does not. I have used the exact same process on either part. If it works on one side it should work on the other side. Can anyone try it themselves and see what I am doing wrong (or is it just one of those inexplicable ProE thing)?


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    Best answer by gwalker

    The thickness of the failing first wall is larger than the outside radius. Change the value of "wall" parameter to .635 or remove the feature relation "d72 = wall".

    5 replies

    gwalker2-ExplorerAnswer
    2-Explorer
    May 3, 2013

    The thickness of the failing first wall is larger than the outside radius. Change the value of "wall" parameter to .635 or remove the feature relation "d72 = wall".

      TomD.inPDX17-Peridot
      17-Peridot
      May 3, 2013

      Interesting problem. In Creo 2 I also had problems getting this to be recognized.

      I removed the fillet in the Copy feature. I then offset the remaining 2 faces; and then used Join to get the bend radius back.

      I created a new surface with a fillet/bend. That too did not want to offset unless the radius was well beyond the defined bend radius. Seems a bit much for this to fail, but it does. Once the feature is created, I was able to change the sketch radius and it regenerated fine. There is a bug in there somewhere.

      For now, I recommend not copying the radius and drive it with a join command.

      TomD.inPDX17-Peridot
      17-Peridot
      May 3, 2013

      I take it back. The problem is simpler. Your default thickness in the new part became 2.0 where it is .635 in the first part. Now that the 1st wall is created, you cannot change it (why not?) I deleted the offset feature and changed the material thickness in File>Prepare>Model Properties>Thickness. After that, the offset worked fine.

      So yes, it did have a problem with the thickness and the small fillet radius with the new thicker material. That is the difference between left and right.

      I did try changing the thickness in the Model Properties with the failed feature but it wouldn't take when I resumed the failed feature. The only thing the system would allow is to delete the failed feature so I could lock in a different thickness.

      Now, the fact that you cannot change the thickness of -your- sheetmetal part with a 1st wall in it is a mystery. Even if I reverse the offset where the feature regenerates at a 2.0 thickness, I could not change the thickness where I can in a new file.

      Anyway, delete the offset and redefine the thickness and re-create the offset and all will be well. If you did intend to change the thickness to 2.0, you can use the method in my 1st post.

      GrahameWard1-VisitorAuthor
      1-Visitor
      May 3, 2013

      Apologies to all..... they were both supposed to be 0.635. On the left part I had the sheet metal thickness set by relation to equal 2.00, so that's why it couldn't be changed except through the relation. Duh.

      Never mind, it's the weekend.........

      TomD.inPDX17-Peridot
      17-Peridot
      May 3, 2013

      Thanks for clarifying that. Have a good weekend!

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