Splitting Problem

[Anonymous]

Hi, I am fairly new with fusion so forgive me if the solution is obvious. I have done searching but could not find an answer.

I am trying to turn this white bushing, which is a single object, into two objects (bodies?), split by the two surfaces that you see here. The surface profiles are mirrors of eachother. The split body command will not allow me to select both of the surfaces. As an alternative to split body, I was able to add thickness to the surfaces to remove material from the bushing but this did not allow me to adjust the gap between the pieces without removing excess material. The other alternative is to duplicate the objects, remove one half of each and put them back together again (for printing purposes). Does anyone have suggestions?

Thanks,

Mike

[HughesTooling]

You don't need to use surfaces for the split you can use just lines.

When you select the line as the splitting tool it will extend to split the part.

If you really wont to use a surface use symmetric for the extrude rather than mirroring after the extrude.

Mark

[Anonymous]

The problem is that I need to split a single body with two different
profiles. The center is hollow where those two planes meet so I am
splitting each side. The problem would be the same, if I extend one of the
profiles, it would be the same all the way through, functionally it would
work but I want to learn how to do it the other way as well.
Thanks

[TrippyLighting]

Mark has shown ou severl screenshots. Perhaps its time for you to sho us what exactly you are working on so we can stop the guessing 😉

[HughesTooling · Accepted solution]

OK I see the 2 halves are different, go to the patch workspace and select Stitch and select the 2 bodies that you want to use as the splitting tool.

 

Then you'll need to select the new body from the browser as the splitting tool. As long as the zig zag part is smaller than the hole this will work.

Mark

[Anonymous]

Hi, that still didn't work for me. I got Error: Split2 Compute Failed, no intersection between target and split tool. I also tried lofting together multiple profiles and the program had the same error. In the example below, I extruded the two profiles, split the faces in the center, patched the two squares then stitched the whole thing together.

Regarding the application of this design, it is not that exciting. I am redoing my basement in an old building and there are random low voltage cables that need to pass through drywall, I wanted to make bushings that can be sized parametrically for different diameters of cables. I am going to print them out of flame retardant ABS. There are many other ways to make them interlock and I am probably going to change this design anyway for something that clicks together. When this problem came up though, I was determined to sort it out in case it came up again in the future.

Thanks,

Mike

[HughesTooling]

Well it's got to the point where you'll have to export and upload I think. The only other idea is move the 2 surfaces apart so there's a definite gap then build surfaces between.

Mark

[HughesTooling]

One thing I found was the height of the zig zag need to be less than the diameter of the hole.

Mark

[HughesTooling]

Just playing around I built a set of surfaces like this.

These allow splitting the bush even if the zig zag is bigger than the hole, but I don't think the bushes you end up with would work too well as you'd have trouble getting them on the cable.

Mark

[Anonymous]

Hi, the problem is solved, I screwed up earlier. The splitting tool in my last post worked fine. I had shifted something earlier and the tool did not extend through the solid part of my model. I went back, moved the shape and retried it. It worked fine. Thanks to Mark, his suggestions led to the solution.

Just to recap,I did the following...

-  drew one splitting profile on the center plane

-  mirrored the pattern on the same plane

-  went into the patch workspace and extruded each profile in opposing directions

-  split the middle faces horizontally on each side (this created two small squares rather than a weird figure eight type shape)

-  patched the resulting two squares

-  stitched everything together

I printed one out and it worked fine although it would benefit frome either adhesive or angled teeth as opposed to ribbing in order to hold it into the sheetrock.

Thanks,

Mike

[Anonymous]

I have a similar issue to the OP here, except that my file let me split the body once, and then never again. I have tried redrawing the lines, moving the line, moving the body, etc. I still get the same error about there being no intersection. I really regret switching to using Fusion 360 over Inventor. It's a much less refined product and I've had all kinds of problems with it already. Unfortunately it's what I have to use now. So, if someone could help me out that would be awesome. The link to the file is here (I'm guess this is how I share them):

https://a360.co/2J4fB01

You will see the successful split on one side, and the remaining body to be split on the other.

[TrippyLighting]

Generally speaking, given the very low number of post you have, you probably should have asked questions much earlier and perhaps before changing over.

The problems you are describing here may not have anything to do with the difference between Inventor and Fuiosn 360. The geometry you are trying to split has a high number of faces and "dirty" geometry easily visible. See blue highlighted lines, which should not be present in clean solid geometry.

If you create clean geometry you'll have no problem splitting it.

This is likely a geometry kernel error message and the geometric kernel between Inventor and Fusion 360 are exactly the same. Both us ASM, which is an early fork of the ACIS kernel.

[Anonymous]

Yeah, you're probably right. I should have probably cooled down a little more before writing. I was getting frustrated. This is probably more to do with me not having worked with meshes a lot before. I'm usually doing solid bodies that I created myself. So how can I fix the geometry? I did have to reduce the mesh density earlier because I couldn't convert it to a solid as it was. Did that maybe mess up the geometry?

[TrippyLighting]

Given the rectilinear shapes of the object I'd probably only use the mesh as a reference for taking dimensions and then re-create a solid model from scratch.

[Anonymous]

Is it worth it if I'm only going to end up using this to print? I'm just trying to slice it up so the pieces can fit on my printer (since the part alone is 60 cm).

[TrippyLighting]

I cannot answer that, but if you already have a mesh, why aren't you using Autodesk Meshmixer to help you with that ?

[Anonymous]

I'm not aware of a way to make cuts with registers like I showed here. I can do a cut on a plane, but not with a register. The registers are important because the pieces will be welded together I want them to have some fit while the adhesive sets. It would be nice if the feature just worked like it was supposed to.

[Anonymous]

It seems that the faces of the body are getting automatically merged during the split process without me desiring it. This is what is causing the bad geometry to be a problem. If I split at any of the three points first, they always work, but never twice in a row. It's kind of ridiculous that the program is having such problems with this. There is clearly body there to intersect, and the sketched body clearly intersects. Redrawing objects is a poor substitute for an actual solution. Is there anyone that can give me an actual solution? Here is the actual file again:

https://a360.co/2GZ2ok3

EDIT: I figured out how to solve my problem. Egg on my face for not thinking of it, because it's so simple. Also, not used to working with the confines of the software's limitations. Figures. Anyway, the solution was the join the three "blades" that were slicing the body into one continuous line, like so: