Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape, CAD, maker project and design.

First time visiting? Here are some places to start:

  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Mirror / Add a "sheet metal" cardboard box

TransistorTransistor Member Posts: 3
 
I'm trying out Onshape with a cardboard box design using the sheet-metal features. I have started with a line on the Right plane, converted to sheet metal and added flanges and cut-outs. Making the right half of the box seemed like a good idea as it makes it easy to work on the inside faces.

The half-box is pretty much finished but I'm stuck with mirroring it. If I select Add and Merge with all I just get the (faulty) mirroring of the lid flap.

I'd appreciate if someone could have a look at the model and guide me through the fix. Many thanks.

Comments

  • mbartlett21mbartlett21 Member Posts: 1,141 EDU
    @Transistor
    If you model the cutout in the lid flap after mirroring, it should work better
    MB (I make FeatureScripts: view FS)
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,092
    edited November 13
    @Transistor

    Alter the sketch to also cut into the bend



    Do the extrude up to the far vertex of the bend:


    After that the mirror will work:
    https://cad.onshape.com/documents/5f3f26fc4cb5b9a7cba29404/w/157f3967ee1a3b5b828c7745/e/0d2e6fffed7a1da4f377f2c0
    Jake Rosenfeld - Modeling Team
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,092
    @Transistor

    I just noticed that even after following that procedure I pointed out, the sheet metal will not unfold.  Not sure why this is, but the best short term solution would be to follow @mbartlett21 's advice and do the mirror first, and the cut into the bend after.
    Jake Rosenfeld - Modeling Team
  • TransistorTransistor Member Posts: 3
    That seemed to work, thanks. Have you any idea why?
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,092
    @Transistor

    We've had a lot of customer reports of problems where mirror add doesn't work if the model has to mirror over a cut into a bend.  The first issue I fixed for you (with the extension of the cut downwards into the bend) has to do with leftover material being present in the underlying sheet body that represents the sheet metal model internally.  Getting rid of that material by extending the cut makes it possible to mirror.  I suspect it then fails to unfold because the up-to-vertex is the wrong depth to cut, and that the right depth is the virtual sharp of either the inner or outer side of the bend (depending on how the model has been set up), which also messes up the underlying sheet body.

    Technical mumbo-jumbo aside, the simpler answer to your question is that our system doesn't respond well to this case, you didn't do anything wrong, and we will have to fix the system for cases like this at some point :)
    Jake Rosenfeld - Modeling Team
  • TransistorTransistor Member Posts: 3
    Thank you everyone.
  • mbartlett21mbartlett21 Member Posts: 1,141 EDU
    @Jake_Rosenfeld
    Would it still have a bend attribute across that edge
    MB (I make FeatureScripts: view FS)
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,092
    @mbartlett21

    The bend attribute is needed to turn the edge of the underlying sheet body into the bend itself in both the 3d and the flat.  Without the bend attribute, the system will most likely throw a SHEET_METAL_REBUILD_ERROR (a.k.a. "Sheet metal model cannot be built.")  With mismanaged bend attributes or dangling faces, it seems like the system is responding by doing as much as it can, but failing to finish the job.
    Jake Rosenfeld - Modeling Team
  • mbartlett21mbartlett21 Member Posts: 1,141 EDU
  • lanalana Onshape Employees Posts: 398
    @mbartlett21
    you don't need to process each definition body individually in the loop, just use qUnion(smParts) everywhere, including in the opPattern
  • mbartlett21mbartlett21 Member Posts: 1,141 EDU
    @lana
    Done!
    MB (I make FeatureScripts: view FS)
Sign In or Register to comment.