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How can the extents of a split be controlled?

robert_scott_jr_robert_scott_jr_ Member Posts: 68 ✭✭
In https://cad.onshape.com/documents/27251cb24bd81873539f9f4d/w/e196876967b5f1a69be951cd/e/0796b77c26485e4e07d436cb
I am trying to split the rectangular parts at their corners at a 45 degree angles. The first split uses a plane. After suppressing that feature, I used a surface for the split. In both cases the split extended beyond the corners into the vertical sides of the parts. I suspected the plane to have that result since the plane is infinite. I did not expect that to happen when using the surface since the surface is fixed to the diagonal created in the sketch using the corners of the part vertices. How can the split be restricted to the corner only? - Scotty

Best Answer

  • robert_scott_jr_robert_scott_jr_ Member Posts: 68 ✭✭
    Accepted Answer
    That is nice and appreciated. Thanks, Michael, for your work in making tasks easier to achieve in Onshape. Thanks also for the notifications of the updates. - Scotty

Answers

  • MichaelPascoeMichaelPascoe Member Posts: 250 PRO
    edited December 2020
    @robert_scott_jr_

    Instead of splitting with a plane, split using a surface as the tool.
    • Sketch a continuous set of lines
    • Extrude the lines as a single surface
    • Split the part using that surface



  • robert_scott_jr_robert_scott_jr_ Member Posts: 68 ✭✭
    Yes, thank You. That worked for me but I doubt I would have discovered that method on my own. Isn't there a method that is more intuitive? - Scotty
  • bruce_williamsbruce_williams Member, Developers Posts: 635 PRO
    @robert_scott_jr_

    Hi Scotty - hats off to @MichaelPascoe for a cool trick method.  In answer to your original question: You are correct a plane will always go infinite. With trim with surface choose 'Trim to face boundaries' to keep the trim confined to the size of your trim surface.




    www.accuratepattern.com
  • robert_scott_jr_robert_scott_jr_ Member Posts: 68 ✭✭
    Thanks for responding. I tried your suggestion before my original post. The split feature goes red when the Trim to face boundaries option is applied. I again tried it recently in Part Studio 2. Thinking perhaps it was a fault in the sketch I used to create the face to split with. Using Michael's sketch, I selected only diagonal section to create the splitting face. A new split using the boundaries option failed. I tried a new sketch using the sketch of the diagonal section but extending the line to ensure the face split the boxes at the corner. That didn't make a difference. I fail to grasp my error(s). - Scotty
  • MichaelPascoeMichaelPascoe Member Posts: 250 PRO
    edited December 2020
    @robert_scott_jr_
    I'm working on a more automated feature that will do these steps. It will be simple at first, but I will let you know when it is finished
  • romeograhamromeograham Member Posts: 547 PRO
    edited December 2020
    [edit to add some images and specific examples]

    @robert_scott_jr_ you can't split a body with a sketch element. You need a body (surface, plane, Mate Connector, etc). 

    If you are selecting sketch elements (lines, arcs, etc) then you can Split faces, but not bodies.

    However, the other thing to note is that you cannot split a body in only one location as you are trying to do. The result of the split would be that you still have 1 body, that has a location with two faces that are coincident to each other... (which doesn't work in CAD systems). I think that @bruce_williams tip will not work with your original setup, since the result of a split would still be a single body (and therefore it fails).

    Here are some examples.

    Splitting the body with the surface like this will NOT work, because the result of a split MUST be 2 separate bodies:


    Even using the "Trim to face boundaries" fails here because there's no multi-body solution:

    If you deselect that option, you can see that the splitting plane is extended through the body, and the Split works:


    If you have a body that allows a multi-body result after a split, you can see that both options work, and using the "Trim to face boundaries" gives the desired result:



    You need to do a split operation that results in 2 (or more) separate bodies. (They can still have coincident faces though). That's what @MichaelPascoe suggested with his tip.

    Hope this helps!

  • robert_scott_jr_robert_scott_jr_ Member Posts: 68 ✭✭
    However, the other thing to note is that you cannot split a body in only one location as you are trying to do. The result of the split would be that you still have 1 body, that has a location with two faces that are coincident to each other... (which doesn't work in CAD systems).

    romeograham :  Ah, that's it. Thank You.

    MichaelPascoe: I look forward to it.



  • bruce_williamsbruce_williams Member, Developers Posts: 635 PRO
    @romeograham
    nice explanation!  I discovered my method did not work on first split after posting; I am sorry for not correcting that.  Thanks for covering the topic correctly.
    www.accuratepattern.com
  • Evan_ReeseEvan_Reese Member Posts: 783 PRO
    Can we all bandwagon onto an improvement request to split bodies with sketches though? It could just extrude a surface, split, and delete the surface in the background. The current workflow has more steps than needed I think.
    Evan Reese / Principal and Industrial Designer with Ovyl
    Website: ovyl.io
    Instagram: @evan.reese.designs
  • MichaelPascoeMichaelPascoe Member Posts: 250 PRO
    Sure
  • MichaelPascoeMichaelPascoe Member Posts: 250 PRO
    edited February 16

    @robert_scott_jr_
    Here is the Split Joint feature I've been working on. It will be buggy, I need to re-write quite a bit of code to make it more robust. Consider this a beta test.

    Split Joints (BETA)


  • wayne_sauderwayne_sauder Member Posts: 90 PRO
    MichaelPascoe that is view only would you be able to give us one we could play with? I think I would find this useful. 
  • MichaelPascoeMichaelPascoe Member Posts: 250 PRO
    Try it now, I made it public.
  • wayne_sauderwayne_sauder Member Posts: 90 PRO
     That works, Thanks.
  • robert_scott_jr_robert_scott_jr_ Member Posts: 68 ✭✭
    Accepted Answer
    That is nice and appreciated. Thanks, Michael, for your work in making tasks easier to achieve in Onshape. Thanks also for the notifications of the updates. - Scotty
  • MichaelPascoeMichaelPascoe Member Posts: 250 PRO
    edited February 17
    Sure thing. As a follower of Christ, I can see how we "people" were designed to get satisfaction from helping other people out. Christ did this all the time, but the problems were more serious problems. I hope to represent him well.

    Onshape has done a fantastic job with this software. I really appreciate their work.
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