Cannot fillet with a radius that matches the edge length?

[Moult]

A very common shape in architectural detailing is this type of window reveal / bevel / bead / cornice shape. In this scenario, I am trying to draw a 20mm quarter arc fillet.

I can draw a 20x20mm square extruded frame, and then fillet it by 19mm to produce the screenshot below. However, I cannot fillet it by 20mm (no error message, but it doesn't fillet). Is there a way I can fillet by 20mm, or is there a better / easier way to draw such a shape?

2019-05-19-163934_753x283_scrot.png (18.73 KiB) Viewed 1277 times

[vocx]

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I can draw a 20x20mm square extruded frame, and then fillet it by 19mm to produce the screenshot below. However, I cannot fillet it by 20mm (no error message, but it doesn't fillet). Is there a way I can fillet by 20mm, or is there a better / easier way to draw such a shape?
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That shape looks like a "pipe", that is, a profile that is extruded along a path. You should probably do this in PartDesign Workbench.

Create a Sketch, which is the flat section (profile) of any portion of the frame; this profile should have the appropriate curvature in the sketch itself, that is, there is no need to add a fillet; create a second sketch that defines the path of the extrusion, then use PartDesign AdditivePipe. You may have to use four sketches, and four paths, for each of the four portions of the frame (if it's a rectangular window).

[chrisb]

To answer your question: no it is not possible that a fillet consumes the whole adjacent face, but 1/1000 left is enough - or even less.

[wieszak17]

You can also make it wider, say 21mm, then fillet with 20mm and cut outer part with one additional sketch.

[Moult]

Thanks, marking as solved.

The method I liked the most was to use a sweep in the part workbench. It seemed the most natural. But thank you very much for the variety of ways to solve this!

[toralf]

Instead of drawing 4 sketches and 4 paths, you might use multiple transformations to copy one body to create the other 3

[Moult]

I am resurrecting this topic (removing the [SOLVED]) to see if people are interested in an updated fillet tool that can create fillets where the radius matches the depth of the object.

In other software, such as Blender and Revit, this type of fillet / bevel is possible, and is such an incredible timesaver than having to do a sweep.

I can investigate implementing such a feature ...

[czinehuba]

Hi All,

I'm still relative new to FreeCAD. Had been following the progress of development for the last year or so. Great work from the developers and everybody involved.
I do a bit of freelance work in Mechanical Design and try to implement FreeCAD as much as possible in my workflow.

The aforementioned issue happens both in fillet and chamfer command in part design workbench as well. It would be definitely a nicety to have. Coming from other parametric CAD, never had this issue.

Thanks

[chrisb]

Yes, that would be very nice, but it may turn out to be difficult. Fillets are coming from the depths of the OCC kernel, and even one of the OCC guys said, that this code is hardly maintainable and should be rewritten. I don't want to discourage you and your very welcome enthusiasm, but I doubt that anything can be done from the FreeCAD side.

[vocx]

... to see if people are interested in an updated fillet tool that can create fillets where the radius matches the depth of the object.
...

Obviously it would be good to fix this issue. However, as chrisb says, I believe the fillet is created by an OpenCascade (OCCT) operation, so unless you fix this internal code, how would you plan on solving it? I think FreeCAD basically detects the limit condition, which OCCT can't handle, and reports an invalid shape. There are two "solutions" currently: using a very close value to the one desired, say, 9.999 mm, instead of 10 mm; or modelling the figure in a different way, like extruding the profile.