Unable to split body: "No intersection between target(s) and split tool."

[R.Courtney]

Any idea what I am doing wrong here?  There is clearly a little sliver of the body around the inside of the splitting tool, yet Fusion 360 tells me there is nothing there.

Thanks!!

Roger

[wilkhui]

Hi Roger - welcome to the forum!

Can you export your design as .f3d and attach it here?

Cheers,

Indy

[GrAndAG]

@wilkhui

I also several times was in the same situation with the same misleading error message. Unfortunately, I did not keep that designs except one.

[R.Courtney]

The attached file contains the body that I am trying to slice, as well as the sketch I am trying to use to perform the slice.  I am trying to remove the sloped inner edge of the body.  To do this, I used a sketch to project the inner top edge of the slope to the XY plane. Fusion 360, however, doesn't seem to like something about that.  I have tried extruding the projected line, but I get the same results.

Thanks for taking a look!

Roger

[wilkhui]

@GrAndAG, @R.Courtney - thanks for these, I'll try to get to these today or tomorrow, is that ok?

In the meantime if anyone else wants to jump in and help then please feel free!

Ciao for now,

Indy

[GrAndAG]

In my particular case no help is needed. I managed to workaround it. I just provided an example where the issue can be caught.

[mroek]

@R.Courtney

The body you're trying to split/cut, has some very funky geometry along the edge between the top surface and the sloping section. How was this created in the first place? Since you're in direct modelling mode, there's no history to tell. Perhaps this was some imported mesh?

Anyway, you can get around your issue if you just create a small offset to the projected sketch, and then split with that. Attached is one example, where I first deleted the two small faces near the opening, then projected the curve and extended it with two tangent arcs, did an offset of 0.01 in (just an arbitrarily small number), extruded to a surface and then used that to split the body and removed the leftover bodies.

I enabled design history first, so you can drag the history marker to see each step. It could have been simplified more, though, but I left it like this for illustration.

[PhilProcarioJr]

@R.Courtney

I have seen a lot of cases like this fail with slice. It seems the slice operation doesn't like to cut along an edge in a surface at times. Either way here is one solution to your problem...there are many.

[mroek]

@PhilProcarioJr

Nice solution, but by mending the projected line like you did (breaking the links and then coincident joining the ends), you avoid the issue, but the resulting edge of the sliced result ends up being segmented, for some reason. Looks like the segments are tangential though, so I gather the geometry is valid. By cutting off a tiny bit more, like I did, the same edge is continuous (except for where the two segments meet in a point). Your result is of course closer to what he wanted, because I removed more of the original shape.

[PhilProcarioJr · Accepted solution]

@mroek

I normally would have fixed the problems in his geometry but he didn't ask for that, so I just did what he asked.

Fixing the projected geometry is a must if you don't want trouble down the road...plus I like repeatable results, not something different every time I try it.

The easy solution for the bad geometry is to go to the patch mode delete the inside faces then patch them with one surface and stitch them together.

Then project the sketch geometry and do the extruded cut and you end up with nice clean geometry.

[mroek]

@PhilProcarioJr

Aha! That's a much better solution, of course! I didn't really think of that method, but it works a treat and gives a very nice result.

Edit: The patch can only be created if still in DM mode, though. In parametric mode it indicates that the patch will be created, but after pressing OK it fails to compute.

[PhilProcarioJr]

@mroek

I think the major issue that really needs to be looked into is why didn't the projected geometry connect at each end, that's also what I really wanted to show @R.Courtney is when you use projected geometry you have to make sure it doesn't have any errors. I never use slice for stuff like this I have seen it fail too many times so it's not a reliable method for this problem. If using this method with a timeline it makes things very fragile and easy to break...so I don't do it. Keep in mind I am not saying that the dev team shouldn't make it work but if they do it needs to be more reliable.

"Edit: The patch can only be created if still in DM mode, though. In parametric mode it indicates that the patch will be created, but after pressing OK it fails to compute."

Yet another reason I love my DM environment...but everyone fights it...oh well.

Here is how I would have fixed the geometry and performed the task @R.Courtney asked for.

[R.Courtney]

The slice shown is a horizontal slice of a much larger front-runner model of a race car. I am slicing it up into approximately 9x17x3 sections to machine foam molds which will be glued together to create the full-size mold for vacuum bag forming of the carbon fiber body part. Machining slopes as is leaves a slope to z=0 which results in a thin breakable edge. So, I decided to take a 1/2 slice, remove the slope, and join it to the slice below. This eliminates that thin, breakable edge.

The body was brought into F360 as a step file. I have a LOT of these to slice and rejoin. I validated the model and didn't get any issues. How can I repair the model to simplify the slicing and dicing?

Thank you all for your help!
Roger

[R.Courtney]

That should be "front-end"

[PhilProcarioJr]

@R.Courtney

In the case you describe I would create a surface to cut the entire front-end to remove the thin slices then slice it up after that. It would be much faster and a lot less work.

I would need the model to show you how though.

[R.Courtney]

Thanks everyone for your replies and help.  I was able to get this finished by unstitching and restitching the body's faces under patch.  Now I am doing the same thing with another body, and the unstitch/restitch methodology isn't working.  But then, my Fusion 360 updated itself since then.....so I am sure it isn't me  😉

[rawlogic39AAA]

I was able to resolve this by scaling the model up by factor 100, doing the split, then scaling it back down by 0.01.

[RScott9399]

I just hit the exact same issue. Not sure what to do. I tried the scaling trick and it didnt work for me. I still got the same error. 

Anyone willing to lend a hand?