Bug Report: Cannot Complete Extrusion to Object, the Extrusion Profile Falls Outside of the Boundary of the Selected Body

[therealsamchaney]

Please check out the attached Fusion 360 model to see the bug.

I'm tying to make a pretty simple hollow form with a shadow line, loosely following this tutorial video. This should have taken me 5 minutes, but of course Fusion has a bug that makes it impossible to do the simple thing that he does in OnShape in the video, and the error message it gives doesn't make any sense with respect to what's happening

I just made a simple shape, then I hollowed it then sliced it with a curved surface. Then I made a sketch where I projected the walls and made an offset, then I just tried to extrude To Object selecting the face at the top of the walls so I could cut a groove into it to make a shadow line. Fusion 360 gives the error "Cannot complete extrusion to object. The extrusion profile falls outside the boundary of the selected object."

It's impossible that this profile falls outside of the boundary of the selected object because the profile is literally a projection of that exact object! Either Fusion failed to exactly replicate the edge when I projected it to the sketch, or it's failing to properly extrude the profile. Either way, somehow Fusion is introducing an error where these two edges no longer match, even though they should be literally mathematically identical since one of them is just a projection of the other one. Even if I simplify the sketch and remove the offset and only project the top surface of the wall to the sketch then try to extrude that sketch To Object and select that top wall surface I get the same error. Seems like there's some fuzzy math going on under the hood where there shouldn't be.

Anyway, this is a huge blocker for me, as shadow lines like this are very useful in designing enclosures and parts that fit together, and this bug makes that impossible without some crazy workaround.

[KristianLaholm]

Is this the desired outcome?

I changed the Extent Type from "To Selected face" too "To Adjacent faces".
Somebody with more insight can better explane the difference of this 2 options.

[therealsamchaney]

Yes and no. The resulting solid is theoretically the same as the intended outcome, but I did not intend to use the central profile as you did. If you deselect the center profile and only select the 2 outer ones as I intended (the projected inner edge and the offsets), then the extrusion will still fail even if you use To Adjacent Faces. This should work. That projected edge is the inner edge of the wall, the same object we are attempting to extrude to. It does not fall outside the boundary.

Further, it doesn't make any sense that adding in the inner profile allows it to work, as that profile is outside the boundary, and yet that one works.

Clearly there is some problem with the two edges being very close but somehow not identical. I would theorize there is some rounding going on somewhere, maybe due to poorly handled floating point math.

[KristianLaholm]

I think you are right on the in sketch projected edge not being exactly the same as the edge of the body.
A small offset of the sketch line inwards will make the profile it overlap the edge and the extrude works.

Some insider or expert can give you a better answer to the root of the problem.

[TrippyLighting]

I think if you worked with arcs (instead of splines) as the guy in the video tutorial di this would not be a problem.

When Projecting curved, spline-based edges into sketches, Fusion 360 approximates the curve with a control point spline within a given tolerance. If you break the link between the projected curve you'll see that is has  a pretty dense control point distribution.

In Fusion 360 it is almost always better to work with offset surfaces than with projected edges. 

[g-andresen]

Hi,

maybe  a better way?

günther

[therealsamchaney]

"When Projecting curved, spline-based edges into sketches, Fusion 360 approximates the curve with a control point spline within a given tolerance"

Well that certainly would explain the problem, and it's also just incredibly bad. The trade off of saving a little bit on processing and/or memory they get from approximating is absolutely not worth breaking everything that requires an exact match, which is a lot in a CAD program. I can't believe they handle splines this way. Well I do believe it,  but it's still pretty incredible.

I will try using offset surfaces instead of projections, but it just shouldn't be necessary. Projection supposed to be a core part of the Fusion 360 workflow. All Fusion tutorials use projection and very few if any use offset surfaces in their stead. Projection is clearly presented as the "right way" to include other geometry in your sketch.

It's asinine to me that the developers decided to use an approximation when projecting splines, especially because it's inconsistent with projecting other types of curves like arcs as you mention. It really seems like a huge foundational problem.

[TrippyLighting]

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@therealsamchaney wrote:

"When Projecting curved, spline-based edges into sketches, Fusion 360 approximates the curve with a control point spline within a given tolerance"

Well that certainly would explain the problem, and it's also just incredibly bad. The trade off of saving a little bit on processing and/or memory they get from approximating is absolutely not worth breaking everything that requires an exact match, which is a lot in a CAD program. I can't believe they handle splines this way. Well I do believe it,  but it's still pretty incredible.

I will try using offset surfaces instead of projections, but it just shouldn't be necessary. Projection supposed to be a core part of the Fusion 360 workflow. All Fusion tutorials use projection and very few if any use offset surfaces in their stead. Projection is clearly presented as the "right way" to include other geometry in your sketch.

It's asinine to me that the developers decided to use an approximation when projecting splines, especially because it's inconsistent with projecting other types of curves like arcs as you mention. It really seems like a huge foundational problem.

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I think you are getting a little ahead of yourselves with some of your assessments!

Approximation is a necessary evil and is done in many areas in any CAD system. It might well be that there are two different tolerances at play here that don't quite agree with each other. There is likely a tolerance within which the projected curve is approximated. There might be another tolerance within which Fusion 360 decides whether two profiles match. These might be different, which might be the reason this error occurs. "Might" because this is to some part speculation and to another part deductions from feedback here on the forum and other channels.

The reason some things work in other older and perhaps more mature systems is that many thousands of development hours have been spent by very capable software engineers to make these things work transparently so unassuming users can create models.

When that fails a lot of folks nowadays feel they have what it takes to criticize "developers" again overly simplifying what actually goes on under the hood.

This can easily be circumvented by using a still sketch based, but more robust workflow as suggested by @KristianLaholm .

Using offset surfaces is IMHO a much better and more robust workflow than any sketch based approach. It also translated much better to other CAD system than a sketch based approach. 

[g-andresen]

Hi,

thin extrusion is even easier to realize.

günther

[TrippyLighting]

I think my last post can be misunderstood as dismissing buggy behavior.

Just to clarify, what @therealsamchaney tried should actually work.

If a user has subscribed to the plastic design extension, there is a relatively new Lip feature that makes creating these lip/groove pairs short work, including the necessary drafts for injection molded parts.

That tool also fails to create the needed geometry using the OP's geometry. I am wondering if the implementation is simply incomplete  - that would be nothing new - or if it inherently flawed.

Edit: The Lip tool implementation works just fine with the OP's geometry. It is simply a matter of modeling properly. 

Using a surface extruded from a spline as a split tool creates undesirable geometry. 

A ruled surface approach for splitting the geometry creates better geometry for such a split:

Model is attached.