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Smart design pattern for a half lap splice joint

baumarbaumar OS Professional Posts: 76 PRO
in Community Support
I tried to create a half lap splice joint.

I tried to create a beam with the full thickness and then a half lap and eventually create a union between them. Then I did the whole process for the counter part. It looked right on the screen, but it wasn't truely right as eventually it was not right to select both surfaces of the beams. In addition that technique is really cumbersome when designing a lot of these joints.

From my point of view, the coolest approach would be to design one beam including both counterparts and then cut the half laps out of it, but I couldn't figure our how to do that.

Therefore I would like to ask if anybody has a smart and efficient technique how to design them. 

(Illustration for half lap splice joints: https://upload.wikimedia.org/wikibooks/en/thumb/3/3f/Lap_joint.png/350px-Lap_joint.png or http://timberframehq.com/wp-content/uploads/2012/06/6c-half-lap.jpg )

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  • lemon1324lemon1324 Member, Developers Posts: 223 EDU
    Manually, I'd do this by

    1. Create both beams so that they're independent parts but intersecting.
    2. Create a new part by extruding the area of the lap halfway through the beams.
    3. Subtract this from one of the beams, deleting the tool.
    4. Subtract this half-lapped beam from the other, keeping tools.
    I can throw together a GIF when I have time if that's not clear.

    If this is going to be something you need to do regularly, setting up a custom feature to do it using FeatureScript would probably be worth it, using basically the same algorithm as above.  I might take a crack at that and post it when I find time.

    Arul Suresh
    PhD, Mechanical Engineering, Stanford University
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 5,354
    I already did this a few weeks back and will post it on the website but in the meantime perhaps you can test it for me. 

    I just made it public, search "FeatureScript Lap Joint"
    Senior Director, Technical Services, EMEAI
  • lemon1324lemon1324 Member, Developers Posts: 223 EDU
    Looks good for nearly every case plausibly called a lap joint.

    The three ways I can get it to fail are
    1. Intersect parts such that size(outerPlanes) < 2 but there aren't two faces parallel to the top plane selection.  This is fine, as I can't find such a geometry I would actually call a "lap joint".
    2. Intersecting parts such that size(outerPlanes) > 3.  This is a plausible geometry (e.g. in this document) when the two boards share one or more fillet faces in a corner or T-joint. In this particular case, the faces are ordered so the T-joint works, but that depends on the order faces of the intersect get returned.
    3. Boards with non-square cross section.  This might be relevant for molding applications, but usually that'll be a miter or coped joint, not a lap.
    Only #2 is possibly an issue, but asking the user to pick a parallel face and pre-filling it with a heuristic should resolve that issue.
    Arul Suresh
    PhD, Mechanical Engineering, Stanford University
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 5,354
    @baumar press the + button TOP RIGHT to add custom feature then search public for featurescript lap joint then select the lap joint feature. It will then appear in your toolbar. No need to see the code. 
    Senior Director, Technical Services, EMEAI
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 5,354
    Thanks @lemon1324 - you found an error (#2) that manifested itself in other geometry scenarios too. Could not figure out until I discovered that I put a hard coded value in there that I must have used during testing and then forgot to remove. Anyway I will post this on onshape.com/featurescript as it seems to pretty robust now. Thanks again!

    Senior Director, Technical Services, EMEAI
  • baumarbaumar OS Professional Posts: 76 PRO
    Hi Neil, I kind of managed to load your script - it seems it was found, but it sais no features available.
    It also sais, that 22 changes had been maid and it asks to create a version in lab joint, but that did not react. So eventually it seems the feature is there, but I don't see how to use it - sorry, I'm new with feature scripts. 
    is there a description or maybe a video showing how to use it?
    Thanks

  • lemon1324lemon1324 Member, Developers Posts: 223 EDU
    Open the Lap Joint FeatureScript document, and click the "+ Custom Features" button:

    Arul Suresh
    PhD, Mechanical Engineering, Stanford University
  • baumarbaumar OS Professional Posts: 76 PRO
    Embarrasing, I managed to download the script and I can open it, but I don't know how to apply. Maybe this is due to the fact that I don't know exactly how to use intersection. Of course I read the help, but that text is very short and did not give me the idea whatfor the intersection is useful. I also made a couple of attempts with intersection from extrude - where I did not find an explication at all, but it never leaded to the result I expected. 
    Is there any reference or tutorial how to use intersection (other then https://cad.onshape.com/help/#sketch-tools-intersection.htm?Highlight=intersect)? Or would there be a video showing the how to apply the lap joint (the video above shows how to call the function, but not how to apply it. )

    I created a workspace for the situation how I understood it that far https://cad.onshape.com/documents/6780de7c80e4680b32e5be66/w/30a71d446089db976dd90e07/e/a10ad9f717590bbdf82bd03b 

    Thanks for help

    Markus
  • kevin_o_toole_1kevin_o_toole_1 Onshape Employees, Developers, HDM Posts: 565
    @baumar: The "intersection" option in extrude is likely not what you're looking for. It functions to remove everything in the merge scope that doesn't intersect your new extrusion.

    The FeatureScript Lap Joint feature does require two bodies that partially occupy the same space, and the new lap joint will be created in that overlapping space.

    I've made the adjustments to a copy of your document which gets a lap joint to work:
    https://cad.onshape.com/documents/57d30e858cd458111dae1c70/w/7bc6669f4d067bce79ff5207/e/bb3e29b3ba7f493e40ff125b

  • baumarbaumar OS Professional Posts: 76 PRO
    Hi Kevin, 
    thanks a lot for your help! With your example I could reproduce the solution. 
    There are still a couple of things I miss. Eg the parallel reference plain is not evident when I saw it, but I guess now it is the plane to orientate the lap joint. But it is not evident since selecting the Top plane gives the same result as selecting the right plane. I also didn't understand the effect of full cut.
    It's such a pity there is no time for good documentation, I know you guys are pushed by feature creep like most SW-developments but still... I'm shure there are so many cool features laying around that only very few people can find and use. I think that's a pity, but that comment is more targeting towards onshape as a company as to you.

    again thanks for your great help, that will save me a lot of time!

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