How to fillet mirrored part

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drmacro
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Re: How to fillet mirrored part

Post by drmacro »

MobiusStrip wrote: Wed Jun 07, 2023 11:03 pm And I still can't get filleting to work after the part is mirrored. If I fillet it as depicted in the screen shot above and then mirror it, of course I get the indentations in the edge along the plane of reflection
Did you try setting the Refine property of the Mirror, then attempting to fillet.


And, yes, the fillet/chamfer has plenty of buggy behavior and qwerks. :(
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
MobiusStrip
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Re: How to fillet mirrored part

Post by MobiusStrip »

I don't see a "refine" property in the mirror, in Part Design's workbench's Mirror pattern or in Part workbench's mirror function. But I did use Part workbench's "create a copy / refine shape" option, and the resulting body did happily fillet. What "refine" option were you referring to?

It's a bit disappointing to have to clutter up the model with yet another copied body and not be able to do it all in Part Design.
chrisb
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Re: How to fillet mirrored part

Post by chrisb »

MobiusStrip wrote: Thu Jun 08, 2023 1:25 am I don't see a "refine" property in the mirror, in Part Design's workbench's Mirror pattern or in Part workbench's mirror function.
Look carefully!
In PartDesign at the very bottom:
SnipScreenshot-a8aae6.png
SnipScreenshot-a8aae6.png (21.33 KiB) Viewed 1159 times
In Part as mentioned the mirror is only the mirrored half, not its source. If you union both halfs, then the Union has the Refine property.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
drmacro
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Re: How to fillet mirrored part

Post by drmacro »

MobiusStrip wrote: Thu Jun 08, 2023 1:25 am I don't see a "refine" property in the mirror, in Part Design's workbench's Mirror pattern or in Part workbench's mirror function. But I did use Part workbench's "create a copy / refine shape" option, and the resulting body did happily fillet. What "refine" option were you referring to?

It's a bit disappointing to have to clutter up the model with yet another copied body and not be able to do it all in Part Design.
@chrisb has explained the appropriate mirror/fuse, Refine workflow. Sorry, I was not specific enough for an inexperienced user.

The mirror can be done in Part Design.
Attachments
Screenshot from 2023-06-08 06-26-36.png
Screenshot from 2023-06-08 06-26-36.png (103.64 KiB) Viewed 1129 times
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
MobiusStrip
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Re: How to fillet mirrored part

Post by MobiusStrip »

Thanks, guys. Actually the main issue there was that I thought "refine" was an option in the UI presented when performing the mirroring, not after the fact down in the info pane.

This works when doing the mirroring with the Part workbench, but the fillet on the resulting object is riddled with artifacts and odd geometry around the perimeter; even stranger is that the defects are not symmetrical between the halves.

When I do it all in Part Design, the model outline looks exactly like yours, but the attempt to fillet fails with "recompute failed."

Files with each of those mirroring methods attached.
Attachments
ring_mirrorWithPartWB.FCStd
(480.99 KiB) Downloaded 3 times
ring_mirrorWithPartDesignWB.FCStd
(448.17 KiB) Downloaded 7 times
drmacro
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Re: How to fillet mirrored part

Post by drmacro »

MobiusStrip wrote: Sat Jun 10, 2023 10:19 am ...
I opened mainOutline_sketch and set all the arcs tangent and viola:
Screenshot_20230610_071914.png
Screenshot_20230610_071914.png (82.94 KiB) Viewed 1035 times
Fillet does NOT like non-tangents, end of story, full stop, ... :mrgreen:
Attachments
ring_mirrorWithPartDesignWB-mac.FCStd
(473.64 KiB) Downloaded 9 times
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
MobiusStrip
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Re: How to fillet mirrored part

Post by MobiusStrip »

Thanks, I appreciate you taking the time to try that. But... if FreeCAD refuses to fillet shapes containing non-tangent curves, it's pretty useless. This means you simply can't make a great many simple shapes. Also, up above in the thread, I posted a shape that has several neighboring curves, sharp angles, and not a single tangency... and it fillets fine.

Forcing the user to make the curves tangent forces him to change the shape, which is unacceptable: https://youtu.be/2Mu4MhHRFlM
drmacro
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Re: How to fillet mirrored part

Post by drmacro »

MobiusStrip wrote: Sat Jun 10, 2023 9:06 pm Thanks, I appreciate you taking the time to try that. But... if FreeCAD refuses to fillet shapes containing non-tangent curves, it's pretty useless. This means you simply can't make a great many simple shapes. Also, up above in the thread, I posted a shape that has several neighboring curves, sharp angles, and not a single tangency... and it fillets fine.

Forcing the user to make the curves tangent forces him to change the shape, which is unacceptable: https://youtu.be/2Mu4MhHRFlM
There are situations that don't need tangency. And, a simple change can make those you point to fail as well.

As for the error shown in your video. Box select the vertexes, not the edges. And learn how to determine why it is redundant and how to deal with the condition. You might want to get hold of the Sketcher Lecture linked in @chrisb forum posts signature. It is very helpful for learning how to use the Sketcher workbench.

Unfortunately, FreeCAD has no control over improving the fillet tool until it is fixed in OCCT the modeling kernel which is an OpenCASCADE product.

The fillet tool and it's limitations is a long known and much lamented issue.

Everything you point out has been said hundreds of times here and in other social media.

You can expect similar issues with chamfer and thickness.

Sorry
Star Trek II: The Wrath of Khan: Spock: "...His pattern indicates two-dimensional thinking."
MobiusStrip
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Re: How to fillet mirrored part

Post by MobiusStrip »

Thanks for the reply and the reference to the tutorial. I do know why it's redundant; the only reason I deliberately showed that dialog is to illustrate that the points already had a coincident constraint.

What does applying tangency to two vertices do differently? I don't know what the word "tangent" even means in that context, or how the resulting constraint differs from coincident. Not trying to be lazy; I will see if I can find out as soon as I get done typing this...
chrisb
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Re: How to fillet mirrored part

Post by chrisb »

MobiusStrip wrote: Sun Jun 11, 2023 2:47 am I don't know what the word "tangent" even means in that context, or how the resulting constraint differs from coincident.
Point-to-point tangency means: make the points coincident plus the connected edges tangent, i.e. if we look at what we know as tangents on both endpoints of the connected edges are identical.
What does applying tangency to two vertices do differently?
Mathematically there is no difference. However, the solver doesn't solve the sketch algebraically but numerically. And the algorithm isn't stable for coincidence plus tangency on the participating edges.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
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