How can the extents of a split be controlled?

robert_scott_jr_

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

robert_scott_jr_

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

MichaelPascoe

@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_

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_williams

@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.

robert_scott_jr_

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

MichaelPascoe

@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

romeograham

[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_

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_williams

@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.

EvanReese

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.

MichaelPascoe

Sure

romeograham

Here's an IR for this: https://forum.onshape.com/discussion/15215/split-body-with-sketch/p1?new=1

MichaelPascoe

@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_sauder

MichaelPascoe that is view only would you be able to give us one we could play with? I think I would find this useful. 

MichaelPascoe

Try it now, I made it public.

wayne_sauder

 That works, Thanks.

robert_scott_jr_

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

MichaelPascoe

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.