Problem about variable fillet on curved surfaces

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tanderson69
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Re: Problem about variable fillet on curved surfaces

Postby tanderson69 » Wed Jun 13, 2018 1:31 am

I finally got something that passes the bopcheck(occt 7.3). It has some sloppy tolerances and is not too pretty, but I am calling it done.
faucetBlendTA01.png
faucetBlendTA01.png (31.31 KiB) Viewed 137 times
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faucetBlendTA01.brep.zip
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freecad-heini-1
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Re: Problem about variable fillet on curved surfaces

Postby freecad-heini-1 » Wed Jun 13, 2018 5:13 am

NormandC wrote:
Tue Jun 12, 2018 10:06 pm
Man, I can't wait for the OCC people to recode the fillet algo from scratch. :roll:
+1

Fillets and thickness.
hebelmischer.gif
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tanderson69
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Re: Problem about variable fillet on curved surfaces

Postby tanderson69 » Wed Jun 13, 2018 2:27 pm

Blend order: Most modeling veterans know this, but I put together an example for noobs. See picture below. In the 'favorable' method the vertical edge gets blended away then in another feature the top gets blended. The order is reversed in the 'unfavorable' method. The top 2 edges get blended first and then the vertical. You can see the difference in the surface type, bspline vs torus, and you can see the effect on tolerances. The bspline is 3 sided with 1 edge degenerated to a point. This degenerated edge can be pain point, especially with offsets. Another thing to keep in mind is: that you can assign different radii to different edges inside the same blend/fillet feature. When you do this to my example, occ builds the favorable method. So the modeling kernel knows which method to prefer.

That being said, the real world is not so simple. In the context of this part, there is a tendency to use the 'unfavorable' method as that is how it was originally done. However, we don't know why it was done that way. I am guessing that was the only way to get it through the modelling kernel. So with that, I would use the 'favorable' method, as long as I can build a valid model, and discuss it with the person responsible for the $.

I am wondering if it wouldn't be better to change the underside surface of the handle so the handle gets thicker naturally. This way the blend wouldn't be responsible for adding the thickness to the handle as it approaches the main cylindrical body. I might try that just for fun.


blendOrder.png
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ppemawm
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Re: Problem about variable fillet on curved surfaces

Postby ppemawm » Wed Jun 13, 2018 3:43 pm

Another take on creating a complete handle (less fillets) only in PartDesign that passes geometry check. I surprised myself on how easy this was to do in V0.17. The sweep sketches can be reused on each of the Booleans with minor modifications.

Picture1.jpg
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faucet_handle.FCStd
(601.09 KiB) Downloaded 9 times
.
Now I just need to conquer the filleting problem following freecad-heini-1 and tanderson69 advice. :?

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13519 (Git)
Build type: Release
Branch: releases/FreeCAD-0-17
Hash: 1a8b868018f45ea486c0023fdbfeb06febc1fb89
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)
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tanderson69
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Re: Problem about variable fillet on curved surfaces

Postby tanderson69 » Wed Jun 13, 2018 4:10 pm

I moved the surface underneath the handle 10mm away from main cylindrical body. This made the handle approx 2mm thicker at the start of the 15mm blend. I am guessing this won't compromise the ergonomics. It sure makes the blends work better and passes the bopcheck(occt 7.3).

faucetBlendTA02.png
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oldmachine
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Re: Problem about variable fillet on curved surfaces

Postby oldmachine » Wed Jun 13, 2018 4:17 pm

...was following this post... previously mentioned is to "Split it" - thanks for that tip! I didn't construct it with all the details, just enough to do it quickly then made a simple cut to cut it in half - then was able to add the 15mm radius without problems (then mirror it)... Good Tip!
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NormandC
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Re: Problem about variable fillet on curved surfaces

Postby NormandC » Wed Jun 13, 2018 4:19 pm

ppemawm wrote:
Wed Jun 13, 2018 3:43 pm
Now I just need to conquer the filleting problem following freecad-heini-1 and tanderson69 advice. :?
The residual edges on your model will prevent fillets from succeeding. I tried OpenSCAD Refine Shape on your Body. It does not succeed. Maybe because you used sweeps which create B-spline surfaces that the removeSplitter() algo cannot treat.

tanderson69 wrote:
Wed Jun 13, 2018 4:10 pm
faucetBlendTA02.brep
Unfortunately a brep solid does not tell us how you made the model and in which order you made the fillets.
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NormandC
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Re: Problem about variable fillet on curved surfaces

Postby NormandC » Wed Jun 13, 2018 4:20 pm

oldmachine wrote:
Wed Jun 13, 2018 4:17 pm
then was able to add the 15mm radius without problems
Your screenshot looks very shiny but does not tell us much with the edges hidden. Did you make the R15 fillet on the joint between the handle and the cylinder on the side, or only the one underneath? That's when it goes south for me.
Last edited by NormandC on Wed Jun 13, 2018 4:24 pm, edited 1 time in total.
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Re: Problem about variable fillet on curved surfaces

Postby freecad-heini-1 » Wed Jun 13, 2018 4:23 pm

In the original pictures it looks like more than this:
fillet_15mm..gif
fillet_15mm..gif (300.82 KiB) Viewed 79 times
fillet_15_and_2mm..gif
fillet_15_and_2mm..gif (974.99 KiB) Viewed 79 times
But the 15mm fillet with the triangle looks not correct to me.
oldmachine
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Re: Problem about variable fillet on curved surfaces

Postby oldmachine » Wed Jun 13, 2018 4:30 pm

Your screenshot looks very shiny but does not tell us much with the edges hidden. Did you make the R15 fillet on the joint between the handle and the cylinder on the side, or only the one underneath? That's when it goes south for me.
Did not intend to make it exactly as the drawing shows - just enough to learn about the filleting tip. 15mm radius on top-front and underside. File attached
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