Simple custom profile helical sweep cut fails with "Compute Failed"

[graham.wideman]

My model, which is to be a form for a wire coil, consists of a cylinder with  "custom thread" cut into it, like this:

(The cylindrical form is in two halves, to make it easier to 3D print.)

The number of turns is parametric. Seven turns works, but if I increase it to eight, Fusion throws a Compute Failed error:

Obviously, I would like to find out how to avoid this.  I thought I followed the recommended practice to do something like this, as demonstrated by Lars Christensen in "Forgot About Sweep's & Custom Threads?"  https://www.youtube.com/watch?v=WvCNGR8C2uo

Start with a triangular coil:

... and on the face of the end of the coil, make a sketch of the desired cutting profile, which is simply a rectangle with a semicircle on one side.

Then sweep that profile along the triangle edge, using a second triangle age as a guide rail:

This results in my two semi-cylinders, plus the custom-profile helix, ready for use as the cutting tool in the combine operation.

But, as shown above, if I increase the turns above eight, I get the Compute Error.  (And I actually need this to work for twenty or thirty or more turns.)

Any idea how to solve this? Have I inadvertently introduced some compute-intensive geometry?  Yet the steps are so simple it's hard to imagine that Fusion 360 can't cope with this.

The f3d project is attached, in case anyone is curious to try it.  Thanks!

[jeff_strater]

I know that Sweep sometimes fails on these kinds of periodic paths after some distance/number of turns.  It's on my list to look into.  See:  surface-sweep-function-too-restricted 

[TrippyLighting]

Here's a screencast that explains how to do a "better" sweep.

[graham.wideman]

@TrippyLightingI appreciate you taking the time to make this demo, and I tried out your alternate way to produce the profile and get it to sweep properly. However, it performs worse than my original method, in that F360 throws a compute error at only 5 turns, as opposed to the 7 that my method reached.

[graham.wideman]

Update:  I gave up on trying to apply the strategy of sweeping a custom profile sketch along the helical path from a coil, and then subtracting that from the cylinder.  I think that feature of F360 is just broken.

However, I realized that I could compose the profile I wanted from multiple "stock" coils. So I've combined a circle-profile coil with a square-profile coil to make a body to use as the cutter to combine with the cylinder. 

This appears to work well. I've tested it up to 100 turns (more than I'll need), and it succeeds.

So my specific problem is solved, but I look forward to the "custom profile" method receiving some attention so that it works better.

[TrippyLighting]

I wonder how you can call that ‘broken’ when I demonstrated how to create the required geometry step by step in a screencast?

[graham.wideman]

@TrippyLighting   So far as I could tell, your demo showed an alternate way to create the geometry for the tool, but did not go so far as to apply the tool to combine-subtract from the cylinder.  It's at the combine-subtract that the compute error occurs.   I recreated your demo following your screencast step by step, and when I extended it with the combine-subtract, I got the compute error, as before, but at fewer turns.

[TheCADWhisperer]

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@TrippyLighting wrote:

I wonder how you can call that ‘broken’ ...

---

Based on my experience I would say that Helix-based geometry has never worked well in Fusion.

[TrippyLighting]

@graham.wideman you are correct. I did not try to create combine operation as I had assumed that it would work fine.

However, it does not so there's definitely a problem here! 

@TheCADWhisperer Agreed!

[KristianLaholm]

Another alternative workflow, works up to 90 turns and then Combine fails.

• Created the Helix path using Surface Sweep with twist angle.
• Placed the Cut profile on a Plan along Path.
• Solid Sweep the Cut profile with Guide surface similar to @TrippyLighting but I used the XY plane for guide surface.
• Extrude the cylinder and did the combine with "cut tool" then split the cylinder in 2 parts (you wanted the cut out on both parts?).

Cylinder

[jeff_strater]

sorry for the slow response, @graham.wideman.  I was on vacation last week and did not really investigate this until today, so I did not realize that the failure was in the Combine, not the Sweep itself. So, I apologize for that incorrect diagnosis.  I somewhat suspect that the problem is here:

that is the first vertical split in that surface, so the evidence is pretty circumstantial, but it is interesting that this split occurs on the 8th turn.  I'll create a bug to investigate further.  Thanks for sharing the model.

[edit] created bug FUS-89570 for this issue

[graham.wideman]

Thanks for the response @jeff_strater .  I can certainly see your interest in the vertical split in the tool.  Indeed, perhaps you could enlighten us in general on what is the significance of those vertical splits that appear in the helical sweep and why they appear?

[graham.wideman]

Interesting alternative strategy, thanks.

In your second step, to clarify for other readers -- "Plan along Path" should be "Plane along Path".

So Construct > Plane along Path, choosing the helix of the previous step as the path.

[jeff_strater]

@graham.wideman - sorry for the delay.  This model is quite intriguing.  Today, when I went to look at it, even with 7 turns, on Compute All, it failed.  For a while, it would not succeed unless I went down to 4 turns.  Then, magically, it started working again, but only up to 5.  So, my theory about the surface split after turn 7, I think, was nonsense.  I think this will take some investigation by our kernel team to figure out exactly what is going on.  Very strange.

[graham.wideman]

@jeff_strater   Well, I'm glad I was able to provide such entertainment :-).  If you are able to discuss the root cause when it's found, I'm sure it will be interesting!

Graham

[jeff_strater]

not a whole lot to add here, but I did get an acknowledgement that this looks like a bug in the kernel Boolean code, but they are just investigating it.  I would not expect a fix to be available for a while, but the core message here is:  you are not doing anything wrong in your modeling.  Not very helpful, I understand...