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What is the easy way to add weld to tricky sheet metal intersections?
pmd
Posts: 65 PRO
Is there an easy way to fill in the gaps between these two sheet metal items to show the welding? I want to boolean them together but it will not let me due to (I assume) the knife edges.
I have tried loft and fill but cannot find enough geometry to make either work and move face will not accept the blue bend radius face.
https://cad.onshape.com/documents/f7f85e0fc1de556379efb232/w/92b4c6f01299700b0a41628b/e/acc556ffedf5fbb93ac3dbb3
I have tried loft and fill but cannot find enough geometry to make either work and move face will not accept the blue bend radius face.
https://cad.onshape.com/documents/f7f85e0fc1de556379efb232/w/92b4c6f01299700b0a41628b/e/acc556ffedf5fbb93ac3dbb3
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Best Answers
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How about this one? What do you guys think?
- Move face to get intersecting geometry
- Boolean to union them together
- Move face to remove the weird corner
- Delete face to get rid of the rest of the joint
- Variable radius fillet to mimic a weld
https://cad.onshape.com/documents/ac5f5b3843056e16f00ec423/w/ccf74d1670fafb21525a424b/e/03713666a9d3481e48464fad
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Another Direct edit approach https://cad.onshape.com/documents/0a2ed088634f185b03bda809/w/14e9faad0cbb613df4cfdbb9/e/dd560c3ef239fb61d2a91786 Notice use of replace face
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@lana - amazing what delete & replace face do 'automagically' Not intuitive for me and I love learning those tricks.
Just for ideas - here is my take using built in extrude & then split with surface method.
@pmd I agree this is one of the ways extrude could be enhanced.
www.accuratepattern.com5
Answers
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@pmd
Easiest way I could fine to do it
Is this what you’re looking for ?
SEE THE POST BELOW FOR URL TO DOCUMENT
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@pmd
https://cad.onshape.com/documents/c1e70aae29271db6257b4db3/w/d6f37d98e38960c34248a035/e/bb984b22726922686a414833
I deleted the URL I had in the post up above. I went back and read your original post and I saw that you wanted everything booleaned together and that just was not so in that documentSo here is a document where everything is booleaned together
You asked for easy.
I’ll just say this was tricky0 -
Thanks @steve_shubin - The split idea helps a lot but I too hope there is an easier way0
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How about this one? What do you guys think?
- Move face to get intersecting geometry
- Boolean to union them together
- Move face to remove the weird corner
- Delete face to get rid of the rest of the joint
- Variable radius fillet to mimic a weld
https://cad.onshape.com/documents/ac5f5b3843056e16f00ec423/w/ccf74d1670fafb21525a424b/e/03713666a9d3481e48464fad
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@michael_mcclain - That does work for my example but is very dependent on angle. If you change the 30 dimension in Sketch 1 to 69 it breaks.
However it certainly solves my current problem. Interesting in my actual document (too messy to share) the corner move face with a magic value of 5mm actually makes the main vee-slot go away so I did not even need the final delete faces!
So in summary the procedure is:- Move one of the knife-edge faces by 0.1mm
- Boolean the parts
- Move the small face on the first item 'behind' the corner radius of the 2nd item by some amount (varies and will go red if try too large)
- Delete all vee-grove faces (3 to 5)
- Fillet for cosmetics
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Another Direct edit approach https://cad.onshape.com/documents/0a2ed088634f185b03bda809/w/14e9faad0cbb613df4cfdbb9/e/dd560c3ef239fb61d2a91786 Notice use of replace face
5 -
@lana - amazing what delete & replace face do 'automagically' Not intuitive for me and I love learning those tricks.
Just for ideas - here is my take using built in extrude & then split with surface method.
@pmd I agree this is one of the ways extrude could be enhanced.
www.accuratepattern.com5 -
@lana
Lana those two delete face features were very very cool. I really liked that. Thanks for showing that
@pmd
https://cad.onshape.com/documents/5d7465c58bbc768eae96d53a/w/2a22c713db0860b7058b1c4d/e/5cd4a2fdd1c813ca60a6147fSince one of the keywords in the original post was EASY — well I just thought this basic way of doing the whole project should be remembered also. Now it’s not an edit after the fact. But it does take the least amount of steps. And I would certainly classify this way of doing it as easy.
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Sometimes it's a simple solution
If you are trying to represent a weldment as a single part in an assembly (and thus create a correct BOM), then simply make a 'composite' part out of the constituent parts.
I hope this helps.Philip Thomas - Onshape1 -
@philip_thomas - I did know about composite parts but in this case I actually needed the part to look like it would after welding and painting for a quote letter0
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@steve_shubin - nice try :-) but it has to be sheet metal as that is what we make!0
