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Forming Tools for Sheet Metal

daveaseemandaveaseeman Member, Developers Posts: 2 PRO
edited March 2017 in Using Onshape
Hi all,

Has anyone figured out a way to create sheet metal features with complex/curved surfaces other than basic bends and flanges? Thinks like louvers or other formed features?

The approach to modeling is very different than in Solidworks, which is what I'm used to. But I tried here to do it in what I thought might be the Onshape way, but with no luck. The first tab shows the approach with flanges in the center of a part, while the second tab shows how I tried to create a formed feature in a similar manner.

Thanks in advance!



  • emagdalenaC2CemagdalenaC2C Member, Developers Posts: 414 ✭✭✭✭
    Here you can see the formed feature that you try to create.
    1. Create a sheet metal model
    2. Finish the sheet metal model. So, the forming tools will not shown in the flat model
    3. Create the forming tool base part
    4. Subtract the forming tool base part to the sheet metal part. You can use "Keep tools" in the boolean feature.
    5. Shell the forming tool base part. Set the "Shell thickness" equal to the sheet metal thickness, and remove any face that you want
    6. Join the two parts with a Boolean feature
    7. Create the fillets. You should create one fillet with radius R and the other with radius R-thickness or R+thickness
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  • bryan_lagrangebryan_lagrange Member Posts: 203 ✭✭✭
    This is what I came up with:


    Since I only need a line for a .dxf I made a cut very small in width (.0005"). This contour is small enough that when the .dxf was called into Sigma Nest it saw one single line. 

    I completed the sheet metal part then added the louver feature. Since I only need the depiction of the louver in the model and only the cut line in the flat this method worked out best for me.

    Hope this helps.

    Bryan Lagrange
    Twitter: @BryanLAGdesign

  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 1,543
    edited March 2017
    Look in the FeatureScript examples (+ menu top right to add features to your toolbar) - I added an embossed foot feature. This does require the sheet metal model to be "finished" first. 
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • BLeeVNBLeeVN Member Posts: 5 PRO
    Has anyone taken the time to expand on @NeilCooke Embossing FS to use Multiple Points to generate a Polygon instead of the Sketch Circle?
  • mahirmahir Member, Developers Posts: 803 ✭✭✭✭
    edited July 10
    Several examples are laying around. Here's a feturescript I made for round embosses/feet. It will work with sheet metal, but only after finishing the part. So emboss features won't show up in the flat pattern.

  • lanalana Onshape Employees Posts: 322
    Please notice that sketches in flat can be used to mark placement of formed features. These sketches can be included in direct DXF/DWG export of flat pattern or inserted into drawings.
  • michael_bassmichael_bass Member Posts: 1 PRO
    Thanks for sharing that @mahir !
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