Mirror / Add a "sheet metal" cardboard box

Transistor

 
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.

MBartlett21

@Transistor
If you model the cutout in the lid flap after mirroring, it should work better

Jake_Rosenfeld

@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

@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.

Transistor

That seemed to work, thanks. Have you any idea why?

Jake_Rosenfeld

@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

Transistor

Thank you everyone.

MBartlett21

@Jake_Rosenfeld
Would it still have a bend attribute across that edge

Jake_Rosenfeld

@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.

MBartlett21

Here is a feature to show the internal body
https://cad.onshape.com/documents/93e675ec2db4cf1b9aa0a09f/w/ccc7ed2a2a6abc1cf74f706c/e/bb627a8c4054d2284265620d

lana

@mbartlett21
you don't need to process each definition body individually in the loop, just use qUnion(smParts) everywhere, including in the opPattern

MBartlett21

@lana
Done!