How to Trim two Surfaces and apply a Edge Fillet
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How to Trim two Surfaces and apply a Edge Fillet
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:- FreeCad:- Get as far as the two surfaces then stumped. 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
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:- FreeCad:- Get as far as the two surfaces then stumped. 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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Re: How to Trim two Surfaces and apply a Edge Fillet
Hi Mark,
face trim at a sketch line can be done with Part split / slice: Then use boolean fusion.
But I have no idea how to fillet the edge.
Best regards
Wilfried
face trim at a sketch line can be done with Part split / slice: Then use boolean fusion.
But I have no idea how to fillet the edge.
Best regards
Wilfried
Re: How to Trim two Surfaces and apply a Edge Fillet
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
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
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- 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
Fillets are weak in OpenCascade.
Please have a look how Creo fillet this edge:
Please have a look how Creo fillet this edge:
- DeepSOIC
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Re: How to Trim two Surfaces and apply a Edge Fillet
Done!
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.
1. Part Section, to get face intersection edge2. 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.
Re: How to Trim two Surfaces and apply a Edge Fillet
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.
- Attachments
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- 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
Hi Viktor,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.
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.
One small improvement. There exists a tool in the Curves-wb to extend the section curve. Location both, lenght 40mm.
Best regards
Wilfried
Re: How to Trim two Surfaces and apply a Edge Fillet
True!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.
Re: How to Trim two Surfaces and apply a Edge Fillet
@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...freecad-heini-1 wrote: ↑Thu Sep 13, 2018 7:47 am face trim at a sketch line can be done with Part split / slice:
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...
What do you think Viktor?
- DeepSOIC
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Re: How to Trim two Surfaces and apply a Edge Fillet
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.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...
What do you think Viktor?