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Is it possible to extrude/loft-cut using a solid shape as a tool?

christian_pettychristian_petty Member Posts: 65 PRO
I'm trying to create a mockup of a thermo-molded tray that will cradle a complex 3D shape. I was hoping I could position the part in its final place, then extrude the tray from the mold direction using the solid part as a tool. I think extrude are only for sketches/faces, and boolean isn't sufficient since the complex shape would result in several undercuts.
Thanks!

Christian Petty - Mechanical Design Engineer, Radian R&D
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Comments

  • S1monS1mon Member Posts: 2,358 PRO
    Short answer, no. 

    Longer answer, you'll probably want to use the isocline tool to split the surfaces of the part using whatever draft angle is recommended for your thermoforming, and then use ruled surfaces at that same draft angle from those splits to create the surfaces which avoid the undercuts. There will be some surfacing work to either make an enclosed solid "tool" or a surface tool to split your tray base part. Boolean has a nice option to offset the tool body which can be helpful for tolerance reasons with something like a thermoformed tray.
  • stvnvl_8501stvnvl_8501 Member Posts: 113 PRO
    Can you share an example of this?  Have quite some experience with thermoforming molds and can't really imagine what you are trying to do..
    Seems like you should be able to succed by extruding a projected contour and splitting the resulting solid with the (extendend) part surface contacting the mold. 
  • Evan_ReeseEvan_Reese Member Posts: 2,064 PRO
    @S1mon
    That's exactly how I'd approach it too.
    Evan Reese / Principal and Industrial Designer with Ovyl
    Website: ovyl.io
  • christian_pettychristian_petty Member Posts: 65 PRO
    edited August 2023
    Thank you for the help everyone.

    Essentially I'd like a tray to cradle this part as closely as possible in this orientation. Looks like I have to crate a surface to make it happen, but conceptually it seems it would make sense to be able to extrude the part as a tool from a block.
    Christian Petty - Mechanical Design Engineer, Radian R&D
  • S1monS1mon Member Posts: 2,358 PRO
    There are CAD systems which have a “solid sweep” but at least in the Solidworks implementation the surfaces it produces are pretty bad if the sweep path is a curve. In this case it shouldn’t be too hard to construct what you need. 
  • Evan_ReeseEvan_Reese Member Posts: 2,064 PRO
    There is a Project Body feature that essentially casts the shadow of a body, which can then be extruded, which might be part of a solution. I say "part" because it's going to struggle to terminate on the original body, and wouldn't account for the draft you need in a form so you might end up having to do it manually anyway. Here's an example though.


    Evan Reese / Principal and Industrial Designer with Ovyl
    Website: ovyl.io
  • glen_dewsburyglen_dewsbury Member Posts: 575 ✭✭✭
    Did I miss something in the question? Not sure what the transform is for.
    A quick Boolean subtract seams to give a cradle shape.
    https://cad.onshape.com/documents/ae39d9785e9d8914ab10960a/w/459cc02062d9e0ceed4ed0be/e/3446e2e18785c2780f69ac71  
  • Evan_ReeseEvan_Reese Member Posts: 2,064 PRO
    @glen_dewsbury
    I believe the goal is to find a way to press the object into a tray at any orientation without creating undercuts, like this example. I think a manual workflow like this is could be the way to go for a general case, but if you can get away with modeling some of it separately (or splitting and recombining it) you could project  each body and extrude up to it to get a start, like this example.


    Evan Reese / Principal and Industrial Designer with Ovyl
    Website: ovyl.io
  • christian_pettychristian_petty Member Posts: 65 PRO
    @Evan_Reese yes! Project body is a solid start. The examples are appreciated. I think that with boolean will work nicely.
    Christian Petty - Mechanical Design Engineer, Radian R&D
  • stvnvl_8501stvnvl_8501 Member Posts: 113 PRO
    hi sorry for the late reply.
    was out a few days.
    @christian_petty Is this solved then?
    @Evan_Reese s solution to me is quite elegant and closely resembles what I would propose.

  • glen_dewsburyglen_dewsbury Member Posts: 575 ✭✭✭
    Thanks for the explanation. Makes sense now.
    So essentially a tool path like I used in SW would be one answer. 
  • christian_pettychristian_petty Member Posts: 65 PRO
    @stvnvl_8501 yes good to go. Might consider a feature request for this still. Thank you
    Christian Petty - Mechanical Design Engineer, Radian R&D
  • stvnvl_8501stvnvl_8501 Member Posts: 113 PRO
    @christian_petty
    I get it now, there used to be a similar command in creo as well, if I remember correctly. 
    you could "sweep" or "extrude" a solid body  (or essentially its contour relative to the sweeping curve/ axis respectively) 
    would be nice indeed. 
  • christian_pettychristian_petty Member Posts: 65 PRO
    @stvnvl_8501 agreed. I'll put a request in
    Christian Petty - Mechanical Design Engineer, Radian R&D
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