Sweep new feature - Twist issue

[Anonymous]

Thank you for adding the Twist command but, unfortunately, it works partially.

The same geometry exported from F360 as STEP

[Anonymous]

very happy with the add. now i don't have to open solidworks

[Anonymous]

FB what are you trying to achieve ? it will do what you want

[Anonymous]

Hi ironwarlock

I can't fillet the edges properly

Did you try to do that?

Thanks in advance

[Anonymous]

did not try.

[Anonymous]

It's 99,9% a bug!

[TrippyLighting]

Well, take for example the geometry you created in Solid Thinking Evolve without the fillet an look at the NURBS mesh.

Then create that same geometry in Fusion 360, export it as a STEP file and import it into Evolve and look at the NURBS mesh. I'd be interested to hear what you see.

Some other EE's do this frequently and while It might not apply to this geometry (again, I'd be interested in what you see) it looks like the Geometric Kernel used in some AD products (Inventor, Fusion 360) the ASM or Autodesk Shape Manager might just be getting a little long in the teeth.

Evolve uses the Parasolid kernel and the other software I cannot identify by the screenshot also possibly uses the Parasolid kernel.

I can only say that in a desperate moment I exported an object with a number of lofts from Fusion 360 where it failed to apply fillets half way through the fillet and used a trial version of evolve, which had no problems to fillet the object.

[lucasproko · Accepted solution]

@Anonymous,

Thanks for posting this issue. I just did a little investigation into the ability to fillet edges after a twisted sweep, and here's what I found.

If you use a straight line or an arc as your path, you should be able to fillet any edges just fine. However, if you try and fillet just the side edges of a twisted sweep where the path is a spline, the fillet is too complicated and Fusion cannot solve it. See the below images for a quick walkthrough of what I mean:

These are the paths I used

These are the results from the sweeps

These are the results from filleting the side edges. Note the one with a spline errors out

However, I did find that if you select all 12 edges in this spline path case, you are able to fillet the entire body. This isn't ideal, but it allows for certain work-arounds like filleting all the edges and then splitting the body where you'd like. See the below images for another demonstration:

The result from filleting all the edges

Creating an offset plane from both ends

Splitting the body

I don't want to launch too deep into the root causes for this limitation, but I just checked the behavior in Inventor, and Inventor cannot perform the same fillet either. This means that the limitation is not in the sweep functionality, but instead in the fillet code in our ASM solver (ASM is the solver that creates the geometry for both Inventor and Fusion). I know this isn't perfect, but hopefully you'll be able to use lines and arcs as your paths for your twisted sweeps, and if that doesn't work, I'm sure you can get creative with extending your paths and then trimming the unwanted portions of the sweeps.

Let me know if you have any other questions!

[Anonymous]

Hi, 

I just imported the F360 geometry (as STEP) within the other software. As you can see the surface I have extracted has a good CV's layout, Order4 and several Spans.

In any case the surface generated in F360 is more than good.

Yes, I confirm you that both software that I used for the test are based on Parasolid

[Anonymous]

Hi lucasproko

Many thanks!

I'll keep in mind your suggestions.

[TrippyLighting]

That does look like proper geometry! Thanks for the feedback!

[Anonymous]

Hi Lucas

Anyway, I  got the same problem by using the Taper function and, to be honest, the geometry does not seem intricate 🙂

You should be fix this issue ASAP, IMHO
FYI, I have been able to apply the fillets using Rhino too

[cekuhnen]

@lucasproko

This is an impression also have because when comparing modeling results between Fusion SW onShape

you notice that where Fusion struggles also Inventor struggles.

If both apps use the same ASM then I would be concern about this since some of the tools in Fusion need

an improvement where it seems it has to be done to the Kernel.

I am not sure if for Fusion it could be forked or and why not improve the ASM so both apps Fusion and Inventor

can participate from it.

For example Inventor and Fusion are the only two apps that require blend 3d curves to do a proper blend surface

or offering very limited G2 fillet functionality.

It seems to me to be a structural foundation issue that now shows the limitation hold Fusion back.

[TrippyLighting]

Yep! Let's attack the root cause!