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Efficient Egg Crate Pattern

caylan_larsoncaylan_larson Member Posts: 2
edited October 2015 in Using Onshape
I'm looking for advice in creating this egg crate pattern. I've tried using the pattern tool on a lofted object but it quickly overwhelms the service. Any ideas? My eventual goal is to have an easily to modify model that lets me measure and target a surface area.


  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    Sometimes it can help performance to nest patterns: produce (say) a 4x4 pattern, then pattern THAT at 4x4 to produce a 16x16 matrix, and so on.
    Another thing to try would be to derive a unit part into a new Part Studio and see if that performs better when patterned
  • philip_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,381
    @caylan_larson - thank you for your question. I am not sure what 'quickly overwhelms the service' means - but a good benchmark is to always comment on the relative performance of the same operations in SolidWorks,CATIA, NX, Creo on any box. Large scale patterns are incredibly resource hungry and a 100% cloud based system like Onshape is usually your best bet. For my own curiosity, i built one for you. My advice (and you can see this in the document) is to build a single cone (?) including the surrounding fillets, so that you are not repeatedly asking the system to fillet a very large number of edges (also an expensive operation). As with a lot of things in CAD (meshes (think bug screen), detailed threads, treadplate and anything with a highly repetitive pattern), we try very hard to NOT model them in any cad system simply for performance reasons. That all said, here is what I think is a good solution - of course, any number of people may be able to improve on this.


    Philip Thomas - Onshape
  • daniel_mooredaniel_moore Member Posts: 4
    edited October 2015
    Hmm!  I'm experimenting with this and trying to re-invent the wheel.

    I have a basic series of egg-shaped cones in a 3x3 grid, but rather than trying to chamfer and adjust how they all fit together, is it possible to *delete* that shape from a solid block?

    I want to delete Part 2 (in orange) from Part 1 (just a basic square blind-extruded 1").  Then I want to chamfer and fool with the resulting part.

    I've tried to tell the Revolution to 'Remove' from the extrusion (does not resolve), tried to use Boolean to delete Part 2 from Part 1 (does not resolve), not having much luck here.


  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    Boolean will work (and this applies to "Remove" instructions are built-in booleans) unless the resulting geometry breaks the rules for a valid solid.
    The rule your solid is breaking will be the one about "zero thickness geometry" which is a no-no. 
    If you search this forum for that phrase (or google the www) you will be presented with typical examples.

    The cure is simply to raise the boolean "tool" (orange solid in your graphic) slightly to eliminate the problem nodes.

    Other rules for a valid solid are so obscure I can't remember any right now! This is the usual culprit, particularly from a Boolean operation (and that applies equally to boolean addition).  If you ever have to model something where corners, rather than faces, of adjacent bodies touch: you will need first to split the body up so that those edges are on different bodies (Parts, in Onshape-speak) 
  • philip_thomasphilip_thomas Member, Moderator, Onshape Employees, Developers Posts: 1,381
    For the academics - for a boolean to succeed the resultant body/bodies must be 'manifold'.

    The definition of manifold is such that at all points in the resultant bodies, an infinitely small sphere may not encompass more than 1 region of solid. 
    In the above image, the boolean would fail because at the top of the cones is a zero thickness area and an infinitely small sphere would encompass two regions of solid.

    Another one of life's great mysteries resolved :)

    @andrew_troup is correct - raising the orange block would be the solution.

    Philip Thomas - Onshape
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,440 PRO
    @philip_thomas must have completely different set of smilies in his browser than the rest of us  B)
    But you always make one remember that a picture is worth thousand words..
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    I thought (perhaps I should say, I hoped) a chimp had run off with PT's smartphone and taken a selfie. :smile: 
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    I thought (perhaps I should say, I hoped) a chimp had run off with PT's smartphone and taken a selfie. :smile: 
  • luuk_akkermanluuk_akkerman Member Posts: 1
    edited August 2019
    Old thread I stumbled upon during my try to model egg crate / waffle foam correctly.

    Although the wavy pattern can have any shape, based on the available tooling later (assuming your modeling something for physical world), most eggcrate foams can be created to sweep a perfect sinus wave (length, amplitude etc free to choose) over another perpendicular sinus curve that matches the amplitude and wave length to get the perfect grid pattern of repeating smooth domes.

    I like to start with a block and cut (or divide) by this sinus*sinus surface.
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