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Converting sheet metal parts from other CAD system

kent_hendersonkent_henderson Member Posts: 69 PRO
in General
Take a look at this sheet metal step assembly I've imported from another CAD program. What you'll see is exactly how the import came into Onshape except I've hidden all but one part in the design studio for clarity, and I group constrained the parts in the assembly. I'm impressed with the imports integrity. My question is this..... What's the best way to covert the imported SM part called Valve Cover Body into something I can flatten and modify in Onshape.  

https://cad.onshape.com/documents/aed3d3850b326223877df48a/w/1baac759470f104a92af513a/e/28b944c1bea014f160e1dccf

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    NeilCookeNeilCooke Moderator, Onshape Employees Posts: 5,379
    edited January 2019
    Measure the thickness and inside bend radius first, then create a Sheet Metal Model feature and use the Thicken option. Pick one face first and flip the thickness if it is wrong, then check the "Tangent Propagation" checkbox (you will have to set corner relief style to "simple").

    EDIT: Just tried that and it didn't work - let me get back to you   :#

    EDIT: There's something in the bend geometry that Onshape doesn't like (we'll take a look at it in more detail). The process detailed above works fine on geometry exported then imported back into Onshape. Another way this can be done, but it takes a little more effort, is to use Delete Face on all internal and external bends. Then use the technique above - you cannot use "tangent propagation" anymore, so you will have to select each face, then select the sharp corners to add bends. 

    https://cad.onshape.com/documents/2a21c718f8a54f17d8b2fe8d/w/125b1cb6b0d5201caaf7a0ba/e/3275417cb2835cad20b69722
    Senior Director, Technical Services, EMEAI
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    brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,137 PRO
    edited January 2019
    Neil, I've never had success converting imported sheet metal parts without deleting the corners first but it would be great if this was possible.  I'll follow along here and see what the outcome is. @NeilCooke
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
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    MBartlett21MBartlett21 Member, OS Professional, Developers Posts: 2,034 EDU
    edited January 2019
    @kent_henderson
    @brucebartlett
    @NeilCooke

    Please try the recognize feature on my FeatureScript here:
    https://cad.onshape.com/documents/a39db7615a2a945ffb7076c3

    It will allow you to set a custom thickness, and if you do, it will also allow you to set bend allowance or deduction.
    mb - draftsman - also FS author: View FeatureScripts
    IR for AS/NZS 1100
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    kent_hendersonkent_henderson Member Posts: 69 PRO
    This featurescript looks super promising. It does recognize and thicken correctly. But I end up with a bunch of little pieces where each bend is a sliver of sheet metal. I'm I attacking this incorrectly?
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    MBartlett21MBartlett21 Member, OS Professional, Developers Posts: 2,034 EDU
    Can you try changing the rips to tangents?

    mb - draftsman - also FS author: View FeatureScripts
    IR for AS/NZS 1100
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    NeilCookeNeilCooke Moderator, Onshape Employees Posts: 5,379
    The FeatureScript won't work in this case due to the issues I raised above. Delete Face is the way to go with this model.
    Senior Director, Technical Services, EMEAI
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    kent_hendersonkent_henderson Member Posts: 69 PRO
    Deleting the inside and outside face of each bend seems to be the ticket.
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    kent_hendersonkent_henderson Member Posts: 69 PRO
    Regarding MBarlett21's question. Tangent was not an option on the sheet metal context window. All the pieces came in as ripped. When I tried to change to bend it showed red. Tangent wan't an option.
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    MBartlett21MBartlett21 Member, OS Professional, Developers Posts: 2,034 EDU
    Oh, ok. :(
    Would you like mine to delete the curved faces automatically?
    mb - draftsman - also FS author: View FeatureScripts
    IR for AS/NZS 1100
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