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Configuration to Chose a Shape in a Sketch

neobobkrauseneobobkrause Member Posts: 74 EDU
I have a shape that includes a surface with a pattern of holes. Sometimes I want the holes to be round, but other times I want them to be hex shaped, and so on. Prior to OnShape configurations showing up on our doorsteps, I've managed this set of variations using a sketch that included all the various hole patterns I might be interested in, but set all but the "current" pattern as Construction lines. Something like this...


In all that clutter, you'll notice that the only non-Construction element in the sketch is the hexagonal shape. Changing the hexagon to a Construction, then converting the circle, diamond, or smaller hexagon to be non-Construction will result in the shape having cutouts of those shapes.



My question is how/whether OnShape's new Configuration capabilities can be used to cleanly select the cutout shape of this object. 

- Bob

Comments

  • mahirmahir Member, Developers Posts: 794 ✭✭✭✭
    edited February 12
    @neobobkrause, construction lines are just that - for construction. Someone correct me if I'm wrong, but they don't contribute to the creation of usable contours. You can't currently use configs to switch between construction/solid sketch lines, and I doubt you ever will. You can definitely configure different contour selections, but they need to actually be selectable. To do this, you either need different sketches for the different outlines, or you need to make all the construction lines into solid lines. I'd use the first option. It adds lines to the feature tree, but it makes selecting contours much simpler.
  • mahirmahir Member, Developers Posts: 794 ✭✭✭✭
    edited February 13
    Here's an example. The config option called "Base Shape" selects between either the square or pentagon contour from the same sketch. As mentioned above, this can more easily be done with separate sketches.

    https://cad.onshape.com/documents/57acdfaae4b005c413ed9b6f/w/3fd585a46d3af1b3ba413c53/e/b02ec721136c6121c1a02cc1
  • owen_sparksowen_sparks Member, Developers Posts: 1,542 PRO
    Personally (and it's just a preference) I'd have either:-

    Simple method
    (i)  An initial sketch with just hole location vertices.
    (ii) Individual sketches for each hole type, and select these using configs.

    Nicer Method
    Make a simple featurescript with a "Hole Shape" drop down list, and then configure that input.

    This has the option that you can then use "created by" with an edge filter to add a chamfer to the hole.

    Cheers,

    Owen S.
    Production Engineer
    HWM-Water Ltd
  • andy_morrisandy_morris Moderator, Onshape Employees Posts: 79
    The way I would suggest achieving this result is to configure the selections used for the extrude feature.

    All you need to do is to add the selection list for the extrude to the configuration input, which will then display the selection count in the table. When you double click on this cell in the table you can change the selections to a different sketch, or you can add or remove regions from the selection list.



    See this simple example of configured selections:
    https://cad.onshape.com/documents/7e5e83e6885dae5776260b9a/w/2339a1a63af248955ab9d648/e/0d31f7998ae62e42f60df3ff

    Andy
    Andy Morris / User Experience Designer / Onshape, Inc.
  • owen_sparksowen_sparks Member, Developers Posts: 1,542 PRO
    Nice :-) :-) :+1:

    OwS
    Production Engineer
    HWM-Water Ltd
  • neobobkrauseneobobkrause Member Posts: 74 EDU
    The way I would suggest achieving this result is to configure the selections used for the extrude feature.

    Yeah, that’ll work. Thanks.
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