I have a body that cannot be joined with other bodies, but why?

[Anonymous]

I have a design with three bodies, and one is being stubborn. I can join 2 of them together, and despite the fact that the third one intersect, Fusion 360 says it cannot be joined. Any ideas how to fix it?

Here's the video showing how the problem happens: https://autode.sk/3sXHfAy And I'm attaching the file shown in the video.

I'm running into many of these problems, so I'd be interested in not only learning what the solution is, but how to find them.

[KristianLaholm]

I have had similar problems joining bodies with faces created using Loft.

This is my solution:

• Create an Offset Surface Body (in your case after the Shell)
• Create the Extrudes but use fixed distance and Join to the first body.
• Split Solid body using the Surface body
• Remove unwanted bodies.

Note: One sketch (Right wall rails) was not fully defined, was missing a coincident constrain.

[Anonymous]

I'm trying to understand your solution, but I'm a bit lost at the first step:

> Create an Offset Surface Body (in your case after the Shell)

What is this offset surface body?

[davebYYPCU]

At first I thought it was the Combine Cut, 

But with all my bag if tricks, was not able to combine anything to the Lofted body.

One for @jeff_strater 

I changed the sketch for the chamfer, and surface offset the outside of the lofted body -0.2mm to trim the shelf, and that didn't work either.

Stumped....

[KristianLaholm]

Have a look in my file, timeline position after Shell feature.

Look in the browser under bodies and you will find an orange surface body (move back timeline marker after the orange feature in timeline)

Offset Surface creates a zero thickness "skin" of the body.

In this case I used the surface body with Split Body cutting of everything outside the "skin"

[KristianLaholm]

Here is a Screencast of the steps I used to fix your problem.
https://knowledge.autodesk.com/community/screencast/8a3d9b38-e3c9-4491-9bd7-fd0b22698cca

[davebYYPCU]

I tried zero and from outside -0.2 mm and neither worked for me.

[Anonymous]

Ohh... now I get what you mean by skin of the body. Neat hack. I haven't done much work with surfaces so it's not in my mental toolset yet. Thank you.

[Anonymous]

As I was applying, extruding and joining the shelf to the box worked and then it stopped working.

[KristianLaholm]

"it stopped working" ?

If you have been working on the same file in Fusion for some time I have found it good practice saving the file and restart Fusion.

I can reproduce the workflow shown in my screen cast with no errors?

[Anonymous]

It seems the problem occurs when the shelf intersects both the lofted part and the extruded part.

[KristianLaholm · Accepted solution]

Please make a Screencast of the problem.

The strange thing is that I can do the workflow over and over on my side with no problem.

[Anonymous]

In the simplified version of the file that I shared it's still working. In my actual file, it worked, but I want the shelf to have a lip in the front (in the file I shared it's a separate sketch), so I re-did that more complex shelf and it stopped worked, I reverted to the simpler shelf and it's still not working.

[Anonymous]

Here it is. If you go to the last action in the timeline, it's the extruding of the shelf. It's extruding as a new body. Change it to join, and you'll see the error:

[KristianLaholm]

I don't have the knowledge to find a solution with the design you have.
I suspect the problem is that the inside face has some strange curvature from being an offset of a loft face.

Without the inside face (no shell) the extrude works.

If this was my project I would rethink the design of the container to avoid the need of Loft, or redesign the inside face not using Shell.

[davebYYPCU]

Thank you, I was down a wombat hole trying to make the Combine Tool happen, trimming the shelf with the surface.  

I see that you don’t need Combine at all, even though it “should” work.

[TrippyLighting]

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@KristianLaholm wrote:

I have had similar problems joining bodies with faces created using Loft.

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Check your curvature, or curvature map. THat will very often hold the answer!

The outslide looks ok, the inside leaves to be desired.

@Anonymous This is too complex of a surface to be lofted in one go.

Edit: @KristianLaholm I must have scrolled past your last post too quickly. My bad!

The outside is also NOt ok:

  

[jeff_strater]

The problem with Combine here is that there is no clear interference between the two bodies.  If you run the Interference command, it will report no overlaps, even with "Include coincident faces" is on.  This can work if the geometry is simple (e.g. planes), but as is pointed out here, the geometry here is not simple.