Artifacts with fillets on inside corners

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GeirS
Posts: 2
Joined: Thu Apr 04, 2019 12:39 pm

Artifacts with fillets on inside corners

Postby GeirS » Thu Apr 04, 2019 12:58 pm

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?
Attachments
FilletInsideCornerError.FCStd
(110.96 KiB) Downloaded 16 times
openBrain
Posts: 4509
Joined: Fri Nov 09, 2018 5:38 pm

Re: Artifacts with fillets on inside corners

Postby openBrain » Thu Apr 04, 2019 2:48 pm

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)...
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meme2704
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Location: Vosges

Re: Artifacts with fillets on inside corners

Postby meme2704 » Thu Apr 04, 2019 4:41 pm

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
Attachments
filetinside1.PNG
filetinside1.PNG (16.53 KiB) Viewed 403 times
filetinside.PNG
filetinside.PNG (18.94 KiB) Viewed 403 times
GeirS
Posts: 2
Joined: Thu Apr 04, 2019 12:39 pm

Re: Artifacts with fillets on inside corners

Postby GeirS » Fri Apr 05, 2019 7:37 am

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...).
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Roy_043
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Re: Artifacts with fillets on inside corners

Postby Roy_043 » Fri Apr 05, 2019 1:45 pm

I have read meme2704's answer, but still think it strange that the solid resulting from the sweep operation has these limitations.
chrisb
Posts: 27167
Joined: Tue Mar 17, 2015 9:14 am

Re: Artifacts with fillets on inside corners

Postby chrisb » Fri Apr 05, 2019 2:33 pm

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
DeepSOIC wrote: ping
Is it worth a tracker issue?
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DeepSOIC
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Re: Artifacts with fillets on inside corners

Postby DeepSOIC » Fri Apr 05, 2019 2:43 pm

chrisb wrote:
Fri Apr 05, 2019 2:33 pm
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
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Joined: Tue Mar 17, 2015 9:14 am

Re: Artifacts with fillets on inside corners

Postby chrisb » Fri Apr 05, 2019 6:10 pm

DeepSOIC wrote:
Fri Apr 05, 2019 2:43 pm
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
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Re: Artifacts with fillets on inside corners

Postby chrisb » Fri Apr 05, 2019 6:22 pm

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.