How to Trim two Surfaces and apply a Edge Fillet

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mark1791
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How to Trim two Surfaces and apply a Edge Fillet

Postby mark1791 » Thu Sep 13, 2018 5:08 am

Hi All

I am trying to see if i can trim two surfaces created using two sketches, then apply a edge Fillet. This is easy in Catia, but trying to do this in FreeCad has me stumped, i can create the two surfaces but trying to trim them is to me next to impossible.

Catia:-
Trim-Two-Surfaces-and-apply-EdgeFillet.jpg
Trim-Two-Surfaces-and-apply-EdgeFillet.jpg (175.47 KiB) Viewed 716 times
FreeCad:- Get as far as the two surfaces then stumped.
Free-Cad-Create-two-surfaces-Trim-and-apply-Edgefillet.jpg
Free-Cad-Create-two-surfaces-Trim-and-apply-Edgefillet.jpg (413.66 KiB) Viewed 716 times
Why this way?, work in Automotive BIW world where we design the panels in Catia GSD and then offset the panel gauge to create solid, so seeing whether i can replicate the design methodology in FreeCad.

Mark
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Surface-trim-two-Surfaces-and-apply-edgefillet.FCStd
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freecad-heini-1
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby freecad-heini-1 » Thu Sep 13, 2018 7:47 am

Hi Mark,
face trim at a sketch line can be done with Part split / slice:
face_trim_at_sketch_line_1.png
face_trim_at_sketch_line_1.png (24.22 KiB) Viewed 699 times
face_trim_at_sketch_line_2.png
face_trim_at_sketch_line_2.png (17.68 KiB) Viewed 699 times
face_trim_at_sketch_line_3.png
face_trim_at_sketch_line_3.png (15.19 KiB) Viewed 699 times
Then use boolean fusion.
But I have no idea how to fillet the edge.
Best regards
Wilfried
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saso
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby saso » Thu Sep 13, 2018 7:52 am

For surfacing you will probably want to have a look at some of this addons Curves, nurbs and Silk. They can be installed from Tools -> Addon manager (restart FreeCAD after you install them). Understand that we are still developing FreeCAD, if you stay around the project you can help to push it further :)

https://github.com/tomate44/CurvesWB
https://github.com/microelly2/freecad-nurbs
https://github.com/edwardvmills/Silk

Edit: not exactly what you want but in that direction... A second, updated trimmed version :)

Sketch.png
Sketch.png (33.22 KiB) Viewed 680 times
Attachments
Surface-trim-two-Surfaces-and-apply-edgefillet_sweep_trim.FCStd
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby freecad-heini-1 » Thu Sep 13, 2018 10:03 am

Fillets are weak in OpenCascade.

Please have a look how Creo fillet this edge:
two_face_fillet_creo.gif
two_face_fillet_creo.gif (66.02 KiB) Viewed 663 times
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DeepSOIC
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby DeepSOIC » Thu Sep 13, 2018 11:31 am

Done!
trim-connect-fillet.png
trim-connect-fillet.png (109.44 KiB) Viewed 639 times
trim-connect-fillet.FCStd
(45.74 KiB) Downloaded 19 times
1. Part Section, to get face intersection edge
2. Sketch on the big face. Extend the intersection line.
3. Part Slice the big face with sketch.
4. Part CompoundFilter to get rid of one of the pieces.
5. Part Connect remainings of the big face with small face.
-> the small face is trimmed automatically
6. Fillet.

It's similar to Wilfried's approach. But Part Fuse doesn't connect faces into shells. Connect does. When the shell is properly connected, fillet works.
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saso
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby saso » Thu Sep 13, 2018 11:50 am

I have updated mine a bit more, its manual, but actually gives you quite a lot of options to play with all the corners and make them as you want.
GIF.gif
GIF.gif (47.82 KiB) Viewed 601 times
Attachments
surface.FCStd
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Last edited by saso on Thu Sep 13, 2018 12:58 pm, edited 4 times in total.
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby freecad-heini-1 » Thu Sep 13, 2018 11:56 am

DeepSOIC wrote:
Thu Sep 13, 2018 11:31 am
Done!
trim-connect-fillet.pngtrim-connect-fillet.FCStd

1. Part Section, to get face intersection edge
2. Sketch on the big face. Extend the intersection line.
3. Part Slice the big face with sketch.
4. Part CompoundFilter to get rid of one of the pieces.
5. Part Connect remainings of the big face with small face.
-> the small face is trimmed automatically
6. Fillet.

It's similar to Wilfried's approach. But Part Fuse doesn't connect faces into shells. Connect does. When the shell is properly connected, fillet works.
Hi Viktor,
thank you so much for this good instruction. I'm happy to see that every day I can learn more about Freecad.
Connect is the helpful thing here, because it fuses the two faces. Good to know. 8-)
One small improvement. There exists a tool in the Curves-wb to extend the section curve. Location both, lenght 40mm.
Best regards
Wilfried
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saso
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby saso » Thu Sep 13, 2018 12:59 pm

freecad-heini-1 wrote:
Thu Sep 13, 2018 11:56 am
thank you so much for this good instruction. I'm happy to see that every day I can learn more about Freecad.
Connect is the helpful thing here, because it fuses the two faces. Good to know. 8-)
True! :)
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saso
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby saso » Thu Sep 13, 2018 6:08 pm

freecad-heini-1 wrote:
Thu Sep 13, 2018 7:47 am
face trim at a sketch line can be done with Part split / slice:
@freecad-heini-1 did you also use the CompoundFilter after the Slice command in this images or something else? Personally I guess I prefer the Curves -> Trim face tool for this...

But watching your video and playing a bit more around with this it seems to me that Part -> Join, could have another mode (Trim? additionally to the Connect, Embed and Cutout) that would do the direct Trim of both faces, then it would be indeed very much like shown in the above catia example...
DeepSOIC wrote:
Thu Sep 13, 2018 11:31 am
ping
What do you think Viktor? :roll:
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DeepSOIC
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Re: How to Trim two Surfaces and apply a Edge Fillet

Postby DeepSOIC » Thu Sep 13, 2018 6:34 pm

saso wrote:
Thu Sep 13, 2018 6:08 pm
But watching your video and playing a bit more around with this it seems to me that Part -> Join, could have another mode (Trim? additionally to the Connect, Embed and Cutout) that would do the direct Trim of both faces, then it would be indeed very much like shown in the above catia example...
DeepSOIC wrote:
Thu Sep 13, 2018 11:31 am
ping
What do you think Viktor? :roll:
I don't know. Sounds doable for single faces, but that's a rather special situation. If you want it for something more complex, I don't know how it's going to extend the trim.
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