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Helix and sweep question(s)

peter_patonpeter_paton Member Posts: 38 ✭✭
https://cad.onshape.com/documents/82c63688c28eac035d7fbdb0/w/6d75ea128d4a8c2b38ad4032/e/fe5838fe90bf0fa72dcb6913

I am trying to work out how to continue the sweep continuously along the part length.  The revolve has divided the part into sections - is there a way to continuously run the sweep, or is there a way of connecting the sweep line segments?

Thanks in advance.
Peter 

Comments

  • eric_pestyeric_pesty Member Posts: 219 PRO
    @peter_paton
    You should be able to just select multiple segments in the sweep path...
    Otherwise you can also create a "composite curve" before hand but that should not be necessary.

    However I just noticed your two helixes end points don't match up so you need to fix this first either way
  • MichaelPascoeMichaelPascoe Member Posts: 804 PRO
    edited May 24
    There are several ways you could do this. Eric suggested one, here is another approach you could take:
    • Create a helix surface so that you can split the face of your part. In this case you will need a slight work around: you will need two helix surfaces right beside each other so the helixes can split the main face into two parts. 
    • Split the main face using the two helix surfaces.
    • Sweep another helix in the x direction so that you will have a variable helix with an outer surface normal to your part.
    • Using the custom feature Sweep normal by @mahir, Sweep your profile along the new helix edge. Use the new helix faces that are normal to your part as a sweep normal guide.
    • Delete repair the small split in the part for a clean look.
    Note: I adjusted the main profile to have a small radius at the intersection of the two faces of the main shape. This will ensure the swept profile stays tangent along the path that it follows.

    Link to example document: (Here)



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