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What's an easier way to sketch concentric closed shapes?

skybrianskybrian Member Posts: 25
Making concentric circles is easy, but what if you have a more complicated shape, like an irregular polygon? I'm currently sketching concentric shapes by hand, but it's getting old. Any tricks?

This is to make a sort of box, where the walls stay the same width but move in and out as you go up, like a candlestick. I'm currently extruding or lofting each wall section separately. Maybe there's some other way to do that?

Comments

  • eric_pestyeric_pesty Member Posts: 423 PRO
    edited March 7
    A good way to do this is to pattern a variable referencing itself. For example something like in this example: i created configurations to grow either linearly or exponentially for each step.

    https://cad.onshape.com/documents/b1ec68dff06d55ff179d8bc7/w/dc0ae0007b32017045650876/e/3f39a038645434881e565b7e

    I used a move face to create the change but you could also use a transform feature to apply x and y scales

    You could get creative and use sine function or some other formula to make it more varied.

    If you can't easily describe it with an equation, you could just pattern the shape and manually apply different scale features to each section, that would be faster than manually sketching the shape over and over!

    EDIT: more details on how this works: https://www.onshape.com/en/resource-center/tech-tips/tech-tip-how-to-use-variables-in-patterns-to-vary-features
  • S1monS1mon Member Posts: 985 PRO
    The sketch offset tool seems like the most obvious answer. It can easily select a bunch of entities at once. It’s also possible to extrude a surface and then offset that. In Solidworks I would sometimes find this approach to be more robust. 

    What sort of shapes are you dealing with? What issues are you having?  
  • steve_shubinsteve_shubin Member Posts: 841 ✭✭✭✭
    edited March 7
    @skybrian

    When people post questions, sometimes it’s all about trying to interpret, what it is, that they’re trying to accomplish.

    Something that stood out in your post was the shape of a candlestick

    MAYBE, drawing the shape at the bottom of your box first, and then drawing a profile to sweep around this base shape, well maybe that might accomplish what you’re looking for

    Take note that there are two different Part Studios in this document. Look for the two tabs at the lower left

    https://cad.onshape.com/documents/fa5f80e8d9466a1a9180b16a/w/2579123d01b71b1064a8589a/e/5333d91e327c42d8b7e1b8acWe 






  • steve_shubinsteve_shubin Member Posts: 841 ✭✭✭✭
    edited March 7
    @skybrian

    I added another part studio

    See the document in my post directly above

    In Part Studio 2, which is the one I just added, I swept a SURFACE and then THICKENED it to come up with a consistent wall thickness

    Here is a section view that shows the wall thickness being the same throughout



  • skybrianskybrian Member Posts: 25
    Thanks everyone! For what I'm doing, learning to use the Sweep tool seems promising. (Somehow I hadn't thought of using it to sweep along a closed curve.)
  • S1monS1mon Member Posts: 985 PRO
    Keep in mind if you sweep, you can sweep more than one curve and create multiple surfaces or parts at the same time too.
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