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Adding Ribs to solid with curved tops and bottom

Eric_92Eric_92 OS Professional Posts: 19 PRO
Struggling with this:
Going through the motions of trying to add ribs to a solid with a curved profile and can't clean up the excess geometry.
Ideally I want to end up with different potions of this part that are shelled / drafted from either side depending on which space it is.

Part was shelled first from the bottom.
Ribs added via: line sketches along a top plane, extruded as surfaces, thickened (add) (basically the video tutorial):


Same thing after various faces deleted to clean up the top:


Bottom view - Note in an ideal world the middle 3 voids would still be solid and shelled from the TOP down.

Closeup of geometry I can't get rid of...

Thoughts? Different way to do this?
Tagged:

Comments

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    If you  want to shell different parts of a solid body removing some parts of a given face and not others, one way is to first split that body using surfaces, and shell the resulting bodies removing the desired face(s) applicable to each. You may have to hide some of the split subparts at times, in order to access some faces to remove....

    As for ribs overrunning: perhaps you could reposition the sketch plane partway up the body and extrude in both directions, either up to next or up to surface? (in the latter case you'd have to create terminating surfaces)
  • Eric_92Eric_92 OS Professional Posts: 19 PRO
    Ok thanks Andrew, Splitting it with surfaces helps.

    I also found that keeping it one piece - shelling it, then adding ribs via extruded sketches that use the side profile worked even better with less headaches and better / easier control over the wall thicknesses.
  • joris_kofmanjoris_kofman Member Posts: 59 ✭✭
    I created an example using multiple bodies and using some boolean operations. I hope this could inspire you to a new way of seeing the problem.

    https://cad.onshape.com/documents/f6b0b5517b624c4b9a4971bb/w/d51c235db7db46679e163f73

    It allows for multiple ribs, different thickness in body, top, ribs and adjusting of the cutting surface shapes without breaking too much of the part.

    What would really make this much more smooth was if one could select all parts that result from a feature in one go. This would allow boolean operations to be much more parametric since the number of bodies would be allowed to change dynamically (in this example when changing the number of ribs).




  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    ......

    What would really make this much more smooth was if one could select all parts that result from a feature in one go. This would allow boolean operations to be much more parametric since the number of bodies would be allowed to change dynamically (in this example when changing the number of ribs).
    I suppose there are some kludge workarounds which might be feasible if the user knew the rib number would need to be edited (perhaps more relevant when we get design tables)
    One possibility might be to include a "fin" which joined all the ribs into a single body until the boolean, perhaps like the spine of a heatsink, and then add some sort of cleanup feature to remove or patch the results of the fin, but it's a slightly klunky concept which would probably have a rather klunky implementation.
  • navnav Member Posts: 258 ✭✭✭✭
    Eric_92 said:
    Closeup of geometry I can't get rid of...

    Thoughts? Different way to do this?

      Try using the replace face command.

    Nicolas Ariza V.
    Indaer -- Aircraft Lifecycle Solutions
  • Eric_92Eric_92 OS Professional Posts: 19 PRO
    Thanks!
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