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Unable to process sheet-metal parts in Release Management Candidate due to flat-pattern properties

chandra_harshachandra_harsha Member Posts: 15 ✭✭

I have many sheet-metal components in a release candidate. But two of those, I did "Finish Sheet metal" to create embossing features in 3D. All drawings have been created through separate document, and release is being managed from there. However, these two sheet-metal parts are not letting me submit release candidate showing error as below. Did anyone face something similar issue? 

I used feature script from this document https://cad.onshape.com/documents/a752e0db24eb071ebb6f5aa0/w/47c6a6888718e30c80f1f652/e/8016367b036eb25754b58de7 to create emboss features. It automatically finishes sheet metal operation.



  • shawn_crockershawn_crocker Member, OS Professional Posts: 800 PRO
    I have seen this before but a ways back and not in the same way you are experiencing it(I don't remember what cause mine).  Something seem off though that you are seeing the flat patterns in the release.  I'm thinking you may be using flat patterns in the drawing that are not from the same version as the sheet metal part itself(looks like all workspaces from the image though).  How are you making the drawings in a different doc when in the image the parts indicate they are in the same workspace as the drawings?   Normally, the flat pattern is not shown in the release and only the actual part is shown.  The flat pattern normally just piggy backs on the actual sheet metal parts release state.
  • Ethan_BushEthan_Bush Member Posts: 4 PRO
    I am seeing the same behavior, somewhat intermittently. After many refreshes, this document is down to showing the symptom on only one of three sheet metal parts / flats. It is also visible in the sheet browser, where inserting the flat view does not show a part number.

  • eric_pestyeric_pesty Member Posts: 1,488 PRO
    I'd submit a ticket as they will be able to tell what's going on better than us guessing!
  • Ethan_BushEthan_Bush Member Posts: 4 PRO
    Onshape support resolved the issue for me! Apparently the flat pattern can "lose track of its 3D representation."
    The Extrude and Boolean operations in Part Studio Beta Controller Sheet Metal likely caused the "internal ID" of Part Controller Chassis Sheet to change.
    This change in "internal ID" broke the link between the Flat pattern and its 3D representation.

    Since I shared my document, they replaced the (post- Finish Sheet Metal Model) Boolean join with an Extrude>Add and now everything works as expected. Presumably a similar thing can happen when applying a feature script that finishes the sheet metal model.
  • chandra_harshachandra_harsha Member Posts: 15 ✭✭
    Hi @shawn_crocker . Sorry for my delayed response. About making drawings in a different document, it gives me more command to control how I can propagate changes from 3D to drawings. Keeping both in same doc works for small projects or assemblies with very few parts. When you release a drawing, automatically the part/assembly (its version) associated with it will be released along with it, which is what you are seeing in the image.

    @Ethan_Bush & @eric_pesty , Onshape support pointed to me in my case the custom feature I am using is causing the issue (which you can find in photos below). Nevertheless, looking at the reason they provided to you, I suppose "Finish Sheet Metal"  command can sometimes cause issues, which I rarely use. If the custom feature I used can't be used, I have to find another solution to create emboss or similar features on sheet-metal. I am really hoping Onshape introduces these features as soon as possible.

    (Onshape response to my problem)

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