What is the best process to complete this design?

steve_cline · August 2021

I am trying to make an assembly of this stove box:

Image: https://us.v-cdn.net/5022071/uploads/editor/m4/yy8soj5u8h5w.jpg

It is constructed with sheet metal and rebar. The inside of the box is hollow which allows smoke from a fire below to be forced into the opening you see in the cylinder and out the back opening of the rectangular box.

I have some OnShape experience but not with anything hollow like this so I welcome any advice on next steps. This document is my design so far. I am wondering what is the best method to make a rectangular cut in the face of the cylinder and the best approach to adding the rebar shown here in the photo.

alnis · August 2021

Since you already have the skeleton of the design, you can use the sheet metal model tool to convert the faces to flattened sheet metal parts:
https://cad.onshape.com/documents/d681eacb63c592a67ca6b525/w/1c6de8cf5cabc563584d7c40/e/6368e1bb19ecb2f249cb1b63

Then, if you click the sheet metal tab, you'll get flattened parts with the right dimensions:

Image: https://us.v-cdn.net/5022071/uploads/editor/ll/lxjpxu3dmtgb.png

You can add the rebar with Neil Cooke's beam feature using the custom profile option, with a circle for your rebar's size in another part studio:
https://cad.onshape.com/documents/e15c2c668d138f01242d0c80/v/9c3d422daa69798c999d2076/e/2d5660fc1012df9598f00251

Hope this helps!

steve_cline · August 2021

Thanks @alnis for the response. I had not thought of using the sheet metal tab. Nice feature!

I see that you added a hole to the cylinder. Can you explain how you made it? I need to move it to the other side of the cylinder and resize it.

alnis · August 2021

If you take a look at Sketch 4, you'll see two lines that go across the face I want to split.
Then, in Split 1, I split that face, making two new ones that can be selected individually.
Finally, in the sheet metal model, I only pick the face I want to convert.

Please let me know if you have any other questions! Also, feel free to make a copy of the document so that you can investigate the details of it!

steve_cline · August 2021

Looks like the split only gives me the option to split the entire face of the cylinder. Is it possible to make a partial split so that the opening is only the top half of the cylinder face?

alnis · August 2021

Yep! One way to do it is by creating a surface to use for the split (see Sketch 7, Extrude 4, and the updated Split 1 feature):
https://cad.onshape.com/documents/d681eacb63c592a67ca6b525/w/1c6de8cf5cabc563584d7c40/e/6368e1bb19ecb2f249cb1b63

(it's a good idea to fully define your sketches, so don't leave them blue like I did!)

steve_cline · September 2021

I think I have done most everything correctly but if you look back at my original document, you can see that the split did not seem to remove the entire section from the cylinder and it also performed a split on both sides (i.e. there are two openings, not one). Any idea what I did wrong there?

alnis · September 2021

Looks like Sketch 2 is in the split tools. If you have a sketch in the split tools it will automatically treat it as a through all symmetric surface extrude (so going both ways, which isn't what you want)

What is the best process to complete this design?

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