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What's the best way to design complex parts to join together successfully (for example a puzzle)

I struggle often to create parts that slot in together and was wondering how this community solves for it.

If you design something like a puzzle then if you fabricate or print it all of the puzzle pieces won't fit together because they're exact size. Instead the parts that extend into other parts need be slightly smaller (.2mm?) and/or the parts that enclose other parts need to be slightly bigger.

I've played with duplicating parts and moving them .2mm in all directions and using the boolean tool to carve out space but it's time consuming and requires a lot of manual placement. If there was a way to shave off .2mm instead of shrinking then that would likely work but I'm not aware of an automated way to do that.

How would you all approach the problem? Example image attached

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Best Answers

  • alnisalnis Member, Developers Posts: 364 EDU
    Accepted Answer
    I put together an example using @Theo_R's method for a stained glass window:
    https://cad.onshape.com/documents/a601795284ff75dd34f65a27/w/e20702e4e573c43288fe5dd7/e/d4945405c477c239898b4bd4

    I used an imported DXF made in Inkscape to define the shape. If you're doing something artistic or making a puzzle, it's probably easier to use a 2D art program or 2D generator (such as a jigsaw puzzle generator) by importing it into a sketch rather than doing it all manually in Onshape. Note that I did some trimming using a "delete face" operation to clean up the frame.

    The key to adding the clearance is that the boolean feature at the end (to cut away the frame) has an offset specified as well as "offset all faces" checked. Hope this helps!

    Final product:


    Close up showing clearances:


    Shape designed in Inkscape:


    Onshape Intern | Get in touch: [email protected] | My personal site: https://alnis.dev

Answers

  • charles_fairchild772charles_fairchild772 Member Posts: 4
    I forgot to post the link. This is only an example though - I run into this in a variety of ways so I'm very curious for general approaches to this problem:
    https://cad.onshape.com/documents/1b97fd976c3a1da6298679e5/w/4a4dba2f5474d72ac3af53ad/e/a8c3371e3307b87fdf2e66d2

    I will say most of my work is in this almost 2d form factor though. This stained glass 3d print is a great example of something I want to achieve but would struggle to design in a way where it would all fit together correctly:
    https://pinshape.com/items/6741-3d-printed-hummingbird
  • JollsJolls Member Posts: 66 PRO
    Could you have your master sketch be the whole puzzle, then setup sub-sketches where you select loops and offset them using a variable to set the offset? Still a bit of labor, but less, and configurable later. Also allows for multiple variables if you need different offsets in something like the stain-glass humming bird example.
  • alnisalnis Member, Developers Posts: 364 EDU
    Accepted Answer
    I put together an example using @Theo_R's method for a stained glass window:
    https://cad.onshape.com/documents/a601795284ff75dd34f65a27/w/e20702e4e573c43288fe5dd7/e/d4945405c477c239898b4bd4

    I used an imported DXF made in Inkscape to define the shape. If you're doing something artistic or making a puzzle, it's probably easier to use a 2D art program or 2D generator (such as a jigsaw puzzle generator) by importing it into a sketch rather than doing it all manually in Onshape. Note that I did some trimming using a "delete face" operation to clean up the frame.

    The key to adding the clearance is that the boolean feature at the end (to cut away the frame) has an offset specified as well as "offset all faces" checked. Hope this helps!

    Final product:


    Close up showing clearances:


    Shape designed in Inkscape:


    Onshape Intern | Get in touch: [email protected] | My personal site: https://alnis.dev
  • JollsJolls Member Posts: 66 PRO
    Theo_R said:
    One solution would be extrude surface, then thicken.

    Assuming we are talking stained glass / puzzle pieces... and referring to your link.
    At some point you need to have a flat volume of "glass" (your sketch 1 with an extrude)
    Draw splines or line work sketch for cut lines (your sketch 2)
    Surface extrude the cut lines (sketch 2) - this would be vertically, aka perpendicular to the "glass"
    Thicken the surface (either one side of the line, or both for centered) - instead of New, select Remove to eliminate material from the "glass"
    Done.
    Alternatively, if you want the "lead" in the stained glass, experiment with intersect in Thicken or a Boolean feature (keep tools) etc. This would give you separate parts required.

    I like the thicken surface solution because you wind up with a thickness centered on the original line sketch.
    LMK

    Great method suggestion! I prefer that over my sketch idea.
  • charles_fairchild772charles_fairchild772 Member Posts: 4
    edited August 2020
    Oh man great idea! this will absolutely do what I was looking for! I want to give both people credit for the answer but I don't think I can. So I'm going to give it to alnis_smidchens for the work put in and then upvote Theo_R

    Just kidding it let me select both! So I selected both and upvoted you both!

    Thank you all so much! This will save me so much time
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