Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:

  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Forming Tools for Sheet Metal

daveaseemandaveaseeman Member, Developers Posts: 3 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!



  • emagdalenaC2iemagdalenaC2i Member, Developers Posts: 545 ✭✭✭✭✭
    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
    Un saludo,

    Eduardo Magdalena                           C2i Change 2 improve                           ☑ ¿Por qué no organizamos una reunión online?   
                                                                 Consulting Partner de Onshape                                      Averigua a quién conocemos en común
  • bryan_lagrangebryan_lagrange Member Posts: 242 ✭✭✭
    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: 2,193
    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: 855 ✭✭✭✭
    edited July 2018
    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: 456
    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 !
  • MBartlett21MBartlett21 Member Posts: 1,554 EDU

    I have just made a forming tool FS: https://cad.onshape.com/documents/a752e0db24eb071ebb6f5aa0
    Please try it out and let me know what you think
    MB - I make FeatureScripts: view FS (My FS's have "Official" beside them)
  • lanalana Onshape Employees Posts: 456
    @mbartlett21 ; Looks great! That implementation is very close to what we have in mind, except that we'll have to do some work so that calling sheetMetalEnd will not be necessary and there will be some representation of the formed tool in flat. So if users of this feature build a library of configured forming tools, they will be able to keep using it when native forming feature becomes available.  
  • owen_sparksowen_sparks Member, Developers Posts: 2,267 PRO
    How cool is that?

    Production Engineer
    HWM-Water Ltd
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,285

    Excellent use for reference parameter! Nice feature!
    Jake Rosenfeld - Modeling Team
  • xphilipxphilip Member Posts: 6 PRO
    @mbartlett21 - We are impressed :)
  • xphilipxphilip Member Posts: 6 PRO
    @mbartlett21 - I meant to do that as my 'Onshape' ego.
    "We are impressed!" :)
  • lanalana Onshape Employees Posts: 456
    I took a liberty of adding processSubfeatureStatus() call after sheetMetalEnd. This causes a blue info message about changes not being reflected in the flat to appear when the Form SM feature is edited.
     If you agree with this change please release another version. This might save us some support questions from this feature users in the future. Thank you for helping us with sheet metal functionality development.
  • MBartlett21MBartlett21 Member Posts: 1,554 EDU


    I have released the version as V 0.1.8
    MB - I make FeatureScripts: view FS (My FS's have "Official" beside them)
Sign In or Register to comment.