convert simple imported sheet metal model into Onshape doc

bryan_lagrange

Currently Onshape does not have the ability to automaically convert an imported sheet metal model into and Onshape model that can be flatten (crossing fingers that this becomes a feature soon ) Here is a work around that I did on a simple sheet metal bracket. Granted this is a simple model and more steps will be needed to do a more complex model. I aslo did not use any convert to surfaces which would probably be another way to do this.

Step one import model:


Step 2 delete existing radius (use delete face command) of imported model so you have sharp edges to work with.



Step 3 select the sheet metal command. Select thicken and pick the face with the most geometry to convert. 



Step 4 use the flange command and use the imported model to extend the flanges to the extent of the imported model.



Step 5 repeat the process until all entites have been added to the new sheet metal part.



Here is the link to the public document.

https://cad.onshape.com/documents/c972f05d4ea87d8277c66137/w/a95780126d293c7d78aac831/e/99f3dcf247ec9ed433c58039

Hope this helps for those who work with imported sheet metal models. Can't wait until this will be a command that Onshape will do automatically.

Bryan Lagrange

brucebartlett

Yes that's what I'd do.  It would be great if Onshape could have an auto convert feature which picks up the thickness and radi and also preserves the part ID so an existing part is not lost from an assembly after converting. 

MBartlett21

@brucebartlett
@bryan_lagrange

You can select the bends in the faces to convert when you convert to sheet metal.
Also select them in the bends selection box, then they will work like normal bends

EDIT: I see, it doesn't work

You don't have to add your flanges like that though. They can be done in the Sheet Metal Model

emagdalenaC2i

First, you can create a Selection to select all the fillets in the part.
Second, as @mbartlett21 said, you can create all the faces in the sheet metal feature:


https://cad.onshape.com/documents/7c05d9bd06c06824fd6ade5a/w/8b8cf0708ba99ecea8a8448d/e/8aea9e6044d09fbc7f522437

bryan_lagrange

Thank you @emagdalenaC2C that saved me a couple steps.

Jake_Rosenfeld

Hi All!

Thanks for pointing this out, this thread has been very helpful for us.  The "tangent propagation" option on "Thicken" along with the "edges and cylinders to bend" was designed specifically for cases like this (as @mbartlett21 points out), but it appears that it's not working an intended.  Do you all find that often imported models have troubles like this?  If so, would you say that you have to use workarounds like this every time, a majority of the time, some of the time, or occasionally?

brucebartlett

Jake_Rosenfeld said:

Hi All!

Thanks for pointing this out, this thread has been very helpful for us.  The "tangent propagation" option on "Thicken" along with the "edges and cylinders to bend" was designed specifically for cases like this (as @mbartlett21 points out), but it appears that it's not working an intended.  Do you all find that often imported models have troubles like this?  If so, would you say that you have to use workarounds like this every time, a majority of the time, some of the time, or occasionally?

Delete rad's is my standard workflow for imported sheet metal geometry, not ideal.  My biggest pain point, however, is losing the part from the assembly after converting to sheet metal, I wish there was a way for the new part to delete the old and take the old parts ID.  

bryan_lagrange

Second what @brucebartlett said.

MBartlett21

brucebartlett said:

Jake_Rosenfeld said:

I wish there was a way for the new part to delete the old and take the old parts ID.  

Make an improvement request. I'll vote