Why is Fusion claiming these two bodies don't intersect

[pupeno]

I'm trying to cut the two cylinders with the bin that goes through them, to remove the bottom part and leave the bottom of the bin clean. Fusion 360 claims there's no intersection between these two bodies, but they do interest

I'm also attaching the model if you want to play with it.

I did something similar in this model https://www.printables.com/model/1121466-wera-kraftform-micro-gridfinity-holder-half-pitch and it worked.

[TimelesslyTiredYouth]

Hi @pupeno 

Let me just clarify my though process in case I've misunderstood:

You want to use the bin as a cutting tool to remove the bottom part of the two cylinders, leaving their bases aligned cleanly with the bottom of the bin. However, Fusion 360 is not recognizing the intersection between the bin and the cylinders, which is preventing the operation.

To cut the cylinders using the bin, ensure both are solid bodies and properly intersect by using the Section Analysis tool. Confirm the bin overlaps the cylinders and use Modify > Combine, selecting the cylinders as the Target Body and the bin as the Tool Body, with Cut enabled.

See if this helps...

new year regards

Ricky

[pupeno]

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@TimelesslyTiredYouth wrote:

To cut the cylinders using the bin, ensure both are solid bodies and properly intersect by using the Section Analysis tool.

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Yes, they do intersect (I think):

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@TimelesslyTiredYouth wrote:

Confirm the bin overlaps the cylinders and use Modify > Combine, selecting the cylinders as the Target Body and the bin as the Tool Body, with Cut enabled.

I tried using Combine instead of Split Body, but it's also failing:

[TimelesslyTiredYouth]

Just out of curiosity, how often do you research into any warnings you get?

Do you have any complex geometry within the design? if so can you use the repair body to fix any troublesome geometry.

When using the combine tool, use the create new component option to see if anything different occurs.

And just check for gaps or overlaps

I am now in a state where I can open your file so I'll check over it and send back what I can.

Happy New Year Regards

Ricky

[TimelesslyTiredYouth]

The second image, do you really think that's a body that is possible? such a tiny thing...

It's not allowing you to cut, not because there not intersecting, but due to the fact that it would leave very small bodies behind, and the reason I believe it's stopping the extrusion/split/boolean subtraction, is due to the fact that these small little tiny things have very complex geometry due to the cut that Fusion can't compute...

Hope it helps...

Ricky

[pupeno]

Hello Ricky,

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@TimelesslyTiredYouth wrote:

Just out of curiosity, how often do you research into any warnings you get?

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Not sure how to answer that. I'm not very good at it, generally I try to understand it, fail, and try a different way to see if that works. Sometimes I do understand it.

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@TimelesslyTiredYouth wrote:

Do you have any complex geometry within the design? if so can you use the repair body to fix any troublesome geometry.

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I'm not sure if the gridfinity base is complex or not according to what you are saying, but I'm attaching another model where I do the same, just with boxes being cut instead of cylinders and it works.

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@TimelesslyTiredYouth wrote:

When using the combine tool, use the create new component option to see if anything different occurs.

And just check for gaps or overlaps

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I tried the new component, but it didn't work. Same error (or rather, the error didn't change).

The complex part, which is the bottom of the bin, is generated by a plug in and it's the same in other designs where this worked (different dimensions, but same plug in).

[pupeno]

I don't see the tiny bodies. There should be 4 bodies left:

• The bin
• The cylinders above the bin
• The cylinders below the bin
• The cylinders intersecting the bin.

And everything but the bin and above the bin I want to delete anyway.

Searching for the small bodies, I did notice a small issue with the model, which I corrected (attached) but it didn't help.

So, is there another way to achieve having this cylinders rise up from the bottom of the bin? Should I make a separate post about it? I know I have curves intersecting curves and that is more complex than planes intersecting planes, but hopefully this is beyond Fusion's capacity?

[KristianLaholm · Accepted solution]

It's the shell feature Shell1 (in the gridfinity section of the design) that is creating some "bad" geometry.
I changed the shell typ from Sharp to Round and after that I can combine cut the cylinders from gridfinity body.

[etfrench]

Do you have a link to the Gridfinity container?

[pupeno]

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@etfrench wrote:

Do you have a link to the Gridfinity container?

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Do you mean the plug in that generates it? It's here: https://apps.autodesk.com/FUSION/en/Detail/Index?id=7197558650811789

[pupeno]

That was it, that fixed it. I'll feed it back to the plug in creator in case it makes sense to change it at the source.