Artifacts with fillets on inside corners

[GeirS]

Hi

I am quite new to FreeCAD. I am having problems with Part Design -> Fillet creating strange artifacts on inside corners. I have tested this both on Linux (FreeCAD 0.18) and Windows (64-bit, FreeCAD 0.17 and 0.18).

I have attached a small modell which demonstrates the problem (a rectangle sketch is swept along a Z-shaped sketch, then the fillet is added).
Outside corners work fine and produces the desired results, but on the inside corners I get a strange twisting shape in half of each corner.

I am obviously doing something wrong. Any hints on how I can get around this problem?

[openBrain]

Confirmed here.
Weird thing in your design is that you use SubstractivePipe. But I did the same with AdditivePipe instead and get the same result.
Here are my findings :

• Get the same shape by Pad => Fillet works OK
• Use Part -> Refine to get a refined copy of the shape => Fillet works OK
• Set the Refine property of AdditivePipe to True => The shape isn't refined and fillet fails

I guess problem comes from fact that top face of your shape is split by the Pipe process. The really bad thing is that setting "Refine" to "True" does nothing (as it would probably solve the issue)...

[meme2704]

Hi
I think this is normal: sketch001 runs around the corner of the sketch path, visible by the rounded corner of the outside corner, so inside there is the same rounded but invisible which prevents the filet from succeeding
this also happens using sweep of "PartWb
but if I make radiuss at the angles of sketch001 using PartWb the corner is well rectangle, but not using PartdesignWb or the corner is always broken

[GeirS]

Thanks for the replies. The current behaviour kind of makes sense if one imagines a physical rectangle sweeping along a profile bent with sharp angles.
Anyways, I found a work around by adding the fillets to the sweep rectangle (creating a rounded rectangle).

I am slowly learning my way around FreeCAD. "Luckily" the delivery of my 3D printer has been delayed for a month, thus I have more time to learn (trying to find a positive angle here...).

[Roy_043]

I have read meme2704's answer, but still think it strange that the solid resulting from the sweep operation has these limitations.

[chrisb]

There are shapes that should be, but aren't refinable. Loft sometimes creates such faces. Here the situation is different, the shape is refinable, as Part->Refine shows.
So the issue is that refine isn't working here.

I think DeepSOIC has worked on the refine

ping

Is it worth a tracker issue?

[DeepSOIC]

Is it worth a tracker issue?

Absolutely.

Refinement with OpenSCAD tool works for me. So, Refine property does nothing in this case.

Also appears to be a bug: it shouldn't be easily possible to start a body with subtractive feature. Yet I tried it, and it just works as if it's additive.

[chrisb]

Also appears to be a bug: it shouldn't be easily possible to start a body with subtractive feature. Yet I tried it, and it just works as if it's additive.

I have mentioned it here before and I think there is even a tracker issue. Today tracker is slow here that I refrained from searching. But I will at least try to add the issue.

[chrisb]

issue #3927. I classified it as severe bug, although there is a workaround. But going from a body to OpenSCAD and back with a BaseFeature is a real hassle.

[voskos]

I can confirm the bug still exists, however I am unable to recompute the fillet in my version, I have to reduce the radius a bit.
Also, I can confirm the refine boolean is unhandled in src/Mod/PartDesign/App/FeatureFillet.cpp
also in Chamfer

The fillet code cannot handle inside corners?