topic Splitting a shell using the XZ plane fails, "No intersection between target(s) and split tool", even though they do in Fusion Design, Validate & Document Forum

Splitting a shell using the XZ plane fails, "No intersection between target(s) and split tool", even though they do

mike_gebis — Thu, 26 Oct 2023 04:15:00 GMT

A am attempting to create a jack-o-lantern shell. I'd like to split it into a front and back half; however, when I attempt to split the body by the XZ plane, I get a "No intersection between target(s) and split tool" even thought they clearly do intersect. Having read some other posts, it appears I may have some dodgy geometry somewhere, although I cannot see it.

I have attached my f3d file; the body I am attempting to split is called "Pumpykin body"

Thank you for any ideas. Thank you.

Re: Splitting a shell using the XZ plane fails, "No intersection between target(s) and split tool", even though they do

davebYYPCU — Thu, 26 Oct 2023 05:12:45 GMT

The split Plane aligns to the creases in the main body.

Using another plane does split sucessfully, when not aligned to the crease.

Might help...

Ynt: Splitting a shell using the XZ plane fails, "No intersection between target(s) and split tool", even though they do

mufuo — Thu, 26 Oct 2023 10:34:38 GMT

As Dave (@davebYYPCU) said, the plane to be created must be related to the part. You can see how it works in the video I added below.

EDT: There was a problem with the recording.

EDT2: Edited video added.

(view in My Videos)

Re: Splitting a shell using the XZ plane fails, "No intersection between target(s) and split tool", even though they do

laughingcreek — Thu, 26 Oct 2023 15:42:39 GMT

@mike_gebis not sure if your interested in a deep dive as to why this doesn't work, but here goes-

the problem traces back to the sketches. (as it frequently does).

as a general rule, you want to fully define your sketches, keep them simple, and when ever possible NOT use sketch patterns, but pattern in the modeling space instead.

also, fusion will struggle to perform commands on funky geometry, so modeling in a way that avoids funky geometry is key. (we could get into why more, but basically...math)

so with that in mind, lets loo at some things-

here are your sketches. overly complicated, not fully defined, uses sketch patterns-

you might have gotten away with that, but a few things aren't lined up right. to check that lets put a spline along the points that will form a creese-

for good measure, I put a curvature comb on it so we can see the quality of the curvature. not TOO bad looking from this angle, but if we look normal to it-

you can see that the splines (and those the crease points that it is on) aren't on a plane, but rather wave back and forth.

another rule of thumb. curvature quality never gets better as you perform operations on/with something. at best it will stay the same, frequently it will degrade somewhat.

so putting a curvature comb on the crease of the solid after lofting we see this-

not looking good. looking normal to it we see the waving back and forth again-

at this point things aren't so bad that the model won't split at the crease. but after you perform another operation on it, the shell, things get worse (here I put the curvature comb on the crease on the inside of the pumpkin, and made the pumpkin transparent so we can see things better)-

so the comb shows further degrading of the curvature quality. do you see how there are no "teeth" on the comb. that's particularly bad news. it means some of the curvature is so extreme that it's falling in between the cracks of what fusion can calculate. again...math.

so another rule of thumb. when you use loft, use as few profiles as possible (you could have use 2 here). and also use loft only if other simpler operations will work. such as sweep in this case.

attached is a model keeping all that in mind. 2 fully defined simple sketches and a sweep. this one will split in the crease. you will note that you can make adjustments to most of the dimensions by right clicking on each sketch and selecting "show dimensions" (if not already showing),double clicking on a dim and giving it a new value. (you don't have to be in sketch edit mode).

you can change the number of creases by changing the "num_of_wedges" parameter in the parameter table-

lets check thee curvature of that crease while we're at it-

Re: Splitting a shell using the XZ plane fails, "No intersection between target(s) and split tool", even though they do

davebYYPCU — Thu, 26 Oct 2023 20:32:29 GMT

Well said,

(I ran out of time to dig into it, but had the direction to look sorted)

Screams out for TSpline ( no sketches - excellent curvature)

Might help…..

Re: Splitting a shell using the XZ plane fails, "No intersection between target(s) and split tool", even though they do

mike_gebis — Thu, 26 Oct 2023 21:05:16 GMT

Wow! Thank you for your detailed answer. And your much more elegant solution, as well. I've clearly got a lot more learning to do, but this helped a ton.