Why does my combine action not work?

[dejskraber]

Hi, 

I hope someone here can help - I spend hours on this issue and I just don't get it.

In the attached file, there are two combine actions that are failing (named combine 13 and combine 14 in the timeline ). I want to cut the body Electronics comp with the one named electronics assembly as a cutting tool. Fusion is telling me that the two bodies do not intersect, but it can easily be seen by looking at them, that they do.

Why does it not work?

[TheCADWhisperer]

@dejskraber 

If this were my design - I would start over from the first sketch (pot revolve).  It can be simplified and fully defined.

Are you interested in learning how?

[jhackney1972]

The Combine is failing because the material was removed in a previous Combine operation.  The material is that was removed can be seen by turning the visibility off on the Electronics Component.  The video will explain.

[dejskraber]

Yes, I'd love to learn how, thank you.

[dejskraber]

Hi John,

Thank you for your answer.

So what you are saying is that combine12 already has done what I am trying with combine 13.

The thing is, that in combine 12, I am using the body "...assembly" to cut "...compartment". In combine I want to use them the other way around to cut the material that was added with extrude 22.

To me it seems very clear that there is an overlap between the two while the time marker is right before the extrude. For example, there's an overlap here (though it is easier to see in fusion if you flip one of the bodies on and off)

[jhackney1972 · Accepted solution]

Yes, you are correct, the previous Combine removed material your current Combine is looking for.  In my opinion, you can accomplish what you want by simply suppressing the original Combine and fixing the current Combine to do what you want.  Model attached.

[TheCADWhisperer]

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@dejskraber wrote:
Yes, I'd love to learn how, thank you.

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pot revolve sketch is far more complicated than needed with more geometry and dimensions (duplicated) than needed.

and not fully defined and a dimension that cannot be measured (in the real world).

Blue lines and white dots should keep you awake at night.

electronics comp upper sketch - again, more complicated than needed, and not fully defined.

Blue lines and white dots should keep you awake at night.

And your resulting wall thickness IS NOT 2mm (I saw same mis-application of a dimension in the first sketch).

Because your Sweep is not perpendicular to the path the wall thickness will not be 2mm.

Same issue in previous sketch...

Interference between Lid and Electronics comp.

Extraneous geometry out the lower front side.

Unnecessary Remove features. (Remove once and THEN pattern features.)

Not aesthetically pleasing geometry...

Now, let me demonstrate how I might start. 

Check back in a few minutes...

[TheCADWhisperer]

Notice how much more simple my first sketch is...

And 2nd sketch...

[dejskraber]

Thanks a lot for your help. That was really an eyeopener. I have drawn plenty of individual simple items for 3d printing, but this is more or less my first advanced multipart item. All my bad habits and my laziness really come back to bite me in ways I have not tried before.

I also still find things that should be obvious but simply passed me unnoticed. I never put any thought to some lines being blue and others black before you mentioned it. Same with the dots. Now I can't believe how I could miss it.

One of the things I've found to be particularly hard is the overall strategy of making something complicated in Fusion in such a way that the whole thing doesn't end up as a complete mess that can't be easily edited and doesn't scale. It's hard to find videos or guides on that topic. Most Fusion youtubers have a narrow focus on a very particular trick like "how to make a helical gear" and such in each of their videos, whereas the subject of the fundamental approaches to using the software the way it is meant to rather than hacking my way through it goes more or less untouched.

[TheCADWhisperer]

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@dejskraber wrote:
...fundamental approaches to using the software the way it is meant to rather than hacking my way through it goes more or less untouched.

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@dejskraber 

Any file that I attach here is rarely my first attempt.

My first attempt(s) are generally just to get an understanding of the geometry - then once I think I have a handle on the geometry I start over in a new file and clean everything up.  I see a lot of users who are resistant to starting over ("I already have x hours in this thing, I'm not starting over.") And then they spend days fighting a losing battle trying to put lipstick on a pig when starting over would have cleaned everything up in a couple of hours.

I already found a couple of things that I would have to question you about to glean your true Design Intent before I could continue.