can't split body

[calexpavel]

I'm trying to split a body into multiple parts using surfaces but i get the error: "Error: Split9
Compute Failed. No intersection between target and split body"

https://a360.co/2LbfiPR

[jeff_strater]

@calexpavel, I don't seem to have access to that project on A360.  I get this:

You can always export the design to a Fusion Archive (f3d) and attach it here.

[calexpavel]

Sorry, i didn't check authorise download. Try this one please: https://a360.co/2C4C88Q

[TheCADWhisperer]

Can you File>Export and then Attach the *.f3d file directly here?

[jeff_strater]

Thanks, @calexpavel, I can export the model now, and can reproduce the problem.  We'll look into it...

[jeff_strater · Accepted solution]

OK, it took me a while (thinking slowly this morning), but I understand now what is going on.  That error is misleading.  It is not that there is no intersection between the body and the splitting tool, but that the splitting tool does not cut the body into two pieces.  This is a limitation/the nature of the beast for Split Body.  In order for Split Body to succeed, each Split has to divide the entire body.  In your model, if you try to split the body using this splitting tool:

The operation will fail, because there will not be two bodies that result.  Ideally, Split Body should allow the selection of multiple tools, so that you could split this thing all in one go.  You could do stuff like, define sketch regions that you want to cut that cut the body all in one go.

then extrude a surface:

and use that as the splitting tool:

which will trim out one section:

You can also, I think, use Boundary Fill to do this.  I need to think about that some more, and I'll try to create a video later today to explain that approach

[davebYYPCU]

It’s easier than that, 

Split body works with sketch articles,

(no need to extrude your cutter, fine for demo purposes)

selecting the lower three lines will get it done.

Might help....

[calexpavel]

Thank you very much! Hopefuly in the future we will be able to select multiple cutting objects. 

[jeff_strater]

Agreed.  Just for our internal purposes, the issue for this is FUS-28349.

[bannister_lee]

I also got that error today for a surface sweep that I was using as a tool to cut a solid body.   I discovered that for sweep's profile, a projected line is fine to use, but for the path, the projected line is not allowed.   Once I replaced that projected line with a curved spline, Fusion was happy.

[tonynicholls2]

I too, had the same problem. My solution was to create a plane (offset) where I wanted to split the bodies, draw a shape to encompass the bodies on the plane, extrude the shape as a cut, then select and delete the unwanted parts. Then use the Create, Mirror command on the same plane.