Fillet won't go near any acceptable radius

[djon_3V3]

Hi there,

So i have been trying for days to fillet a first and single letter of a logo i need to finish even more now than beginning of the week.

I made closed spline curve from scratch, extruded and tries to have fillet of 0.3mm to 0.5mm (3mm extrusion) but that won't work. I attached the object to the post, and here is the picture of the best fillet i can do with it. It is 0.029mm radius. Just enough to get some shininess on edges.

Anything greater than this fails miserably.

Or not... if i scale the part by 10, thus have an extrusion of 30 mm, i can fillet at 1.1mm. One would expect it to max at 0.29, but logic fails here too.

I do believe this is a bug, mainly due to the fact that radius ratio changes with the scale.

Thanks for any help, have a nice day.

ridiculously limited fillet

[TrippyLighting]

No bug here. The regular fillet in Fusion 360 is called a "rolling ball" fillet. That rolling ball needs to be able to traverse between the two surfaces while never leaving the surfaces. It cannot do that when it gets too large because som of your radii on your design are just too small and fillet geometry would self intersect.

[djon_3V3]

Hi there.

I understand this reason, but i doubt it is the case here.

The simple reason is that if i scale the body, i can put in a bigger fillet than the scale ought to enable.

To reiterate:

- normal scale, i can not go over 0.029mm radius

- scale 10 times: not only can i have a 0.29mm radius, i can now have a 1.1mm radius.

Also, just download the model and look at its fillet. There is no way it is limited due to this reason. 

If you have a logical or physical explanation to this, i'd love to hear it. Otherwise, i'd keep on calling it a bug.

Have a nice day.

[djon_3V3]

One other thing...

See the picture below. I did a boolean of the letter to a cube. The has a huge spike down, spikier(?) than anything in the original form. I can have a 1.5mm fillet (on a 3mm extrude) without any problem, even if the spike is largely crumbling on itself. 

Yet, the bottom of the imprint will not accept over 0.029 fillet. And yes, the fillet is there in the picture. 

[jeff_strater]

there is certainly something strange here.  I decided to use a "divide and conquer" approach to try to find where the problem geometry is.  By dividing the body at two more or less random places, I found that I could fillet each section to 0.5mm with no problem.  The dividing planes I chose are in areas of low curvature, so I can't see that splitting the edges at those points would be meaningful at all.  Will have to dig deeper...

[jeff_strater]

even just a single split worked OK

[djon_3V3]

Hoooooo, extremely interesting find.. 

Not only it is a good thing to debug, but it might also help me deliver to my customer. Double gain, no pain. 🙂

Testing this.

Thanks a huge bunch.

[djon_3V3]

Hi there,

Ok, i think i have it. I can reproduce and see where the problem lies. (and control it)

Please check the pictures and included demo file.

In the sketch, there are two shapes. The one at right is the copy of the one at left. I just modified the selected point to have a little depression on the right of the point. That is enough to have the fillet to fail. However if you split that depression in two, it works again.

This little concave part is enough to severely limit the radius we can fillet. I can fillet the one at left until it becomes a somewhat flat dome. The one at right would only go down to 2.5 or something.

two copies of the same shape, one point modified on one of themthe modified won't filletuntil i split the concave part

[jeff_strater]

Thanks, @djon_3V3 - I'm not 100% sure that is the same problem, but it may well be.  I sent the original model off to the modeling kernel team, and they believe it is a core fillet bug, and are looking at it for a fix.  Thanks for reporting it!

the Fusion bug is FUS-88325

[djon_3V3]

Hi @jeff_strater .

Thanks for the follow-up.

I applied the same techniques to my letters, which was either cutting the spline, or making it non-concave. Both worked. Might not be the problem but whatever side-effect i am creating... ...solves it. 🙂

Please mind sending a message here when the fix comes live. 

Have a nice day.

[TrippyLighting]

@djon_3V3 very interesting find indeed!

[djon_3V3]

Hi @jeff_strater !

Do you have any news for FUS-88325?

This is blocking me from releasing to my customer, some parts can not be patched by the tricks you found.

At least a rough date estimate would help.

Thanks a lot, have a nice day.

[TrippyLighting]

I can tell you from experience that if this really is a really a bug in the geometric modeling kernel then this  is likely many months out at least.

Fusion 360 shares the geometric modeling kernel with Autodesk Inventor, which complicates the situation.

[jeff_strater]

sorry, no update to report, or even a target date.  Unfortunately, core geometry modeler bugs like this can take some time to analyze.

[djon_3V3]

(sigh) ok, thanks for the honest response.

/me fires up freecad. (in despair)