Problem about variable fillet on curved surfaces

[NormandC]

You seem to have used additional workbenches; please list them here

The Report view gives some info, but not the specific add-on names.

<unknown exception traceback><type 'exceptions.ImportError'>: No module named CompoundFilter2
<unknown exception traceback><type 'exceptions.ImportError'>: No module named CompoundFilter2
<unknown exception traceback><type 'exceptions.ImportError'>: No module named lattice2SubLink
<unknown exception traceback><type 'exceptions.ImportError'>: No module named CompoundFilter2
<unknown exception traceback><type 'exceptions.ImportError'>: No module named CompoundFilter2
<unknown exception traceback><type 'exceptions.ImportError'>: No module named CompoundFilter2
<unknown exception traceback><type 'exceptions.ImportError'>: No module named lattice2SubLink
<unknown exception traceback><type 'exceptions.ImportError'>: No module named CompoundFilter2
<unknown exception traceback><type 'exceptions.ImportError'>: No module named CompoundFilter2
<unknown exception traceback><type 'exceptions.ImportError'>: No module named CompoundFilter2

I'm pretty sure they are from lattice2 and Part-o-Magic.

I think it's possible to work with solids rather than surfaces. I'll give it a try. I certainly agree that not having a split edge at the top is key.

[NormandC]

Screenshot taken from freecad-heini-1's video:

FC_freecad-heini-1_einhandhebelmischer_sketch_01.png (129.53 KiB) Viewed 1363 times

There is no need to use vertical construction lines here. Make the two end points of the R 100 mm arc vertically aligned with a vertical constraint (use on points is available since v0.17), then add an equal length constraint between the two lines.

FC017_faucet_handle_sketch_01.png (21.33 KiB) Viewed 1363 times

Most of the time, people use construction lines as crutches when you can walk without them.

P.S. I didn't split my sketch because I do not plan on doing half the handle. I'm not convinced the radius between the cylinder and the handle is variable. At least, we are missing views telling us so.

[pmlee]

My way to create this part including the fillets:

phpBB [video]

einhandhebelmischer_fh-1_v1.fcstd

Code: Select all

OS: Ubuntu 16.04.4 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13959 (Git)
Build type: None
Branch: master
Hash: 2f18182b6dff87f8857787c854e39ca4d441f993
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: German/Germany (de_DE)

Best regards
Wilfried

OMG!! freecad-heini-1 you are really the man!! I did not expect that fillet can be done by this way. I really appreciate your video!! I'll try your approach. Thank you very much for your tutorial video!!

By the way, this drawing are actually quizzes from the Skill Evaluation Center of Taiwan. The drawing can be download as a practice purpose. You can download the file from the following link. And you can also find some very interesting schematic in it.

http://www2.wdasec.gov.tw/uploaddowndoc ... f&flag=doc

[pmlee]

simply wait until OCC has a better fillet engine.

Are you willing to wait years? Because that's what's going to take. As far as I know, the company that develops OCC does not have any immediate or future plans to improve the filleting engine.

NormanC,

I have done some homework myself. And I find this video regarding variable fillet:

https://www.youtube.com/watch?v=qG8cEEjz-EM

Perhaps this approach can solve my problem. However, it still needs some effort to use this approach in my model. In addition, I wonder why FreeCAD won't `borrow` fillet function from blender or from other open source 3D project. I know it won't be easy. Just curious.

[NormandC]

You can download the file from the following link.

Thanks for the link. For others interested, the PDF is almost 25MB, download speed was slow for me, but I am on the other side of the planet from Taiwan.

Perhaps this approach can solve my problem.

Interesting method. Worth pursuing, but only if you can't replicate freecad-heini-1's method.

I wonder why FreeCAD won't `borrow` fillet function from blender or from other open source 3D project. I know it won't be easy. Just curious.

FreeCAD and Blender are completely different. FreeCAD (like most CAD programs) is based on a method called Boundary representation, or B-rep. Blender is a polygonal modeller. Therefore the functions cannot be shared.

[NormandC]

Unfortunately the PDF does not have complete drawings of the faucet handle. The only page available is the one pmlee posted, which is insufficient to understand the full shape of the handle.

We get more info on the final shape from images in the document.

FC_faucet_handle_02.png (147.88 KiB) Viewed 1350 times

FC_faucet_handle_03.png (123.04 KiB) Viewed 1350 times

Very nice models in that PDF by the way!

[freecad-heini-1]

Hi NormandC,
you are right, it' possible to create the sketch more easy and nothing speaks about to start with a solid and split it with the sweep surface. Thanks for the pictures in different view. The 15mm radius between the handle and the cylinder was wrong, I corrected it and I'm happy to see how great Freecad creates the fillets. Very nice. Freecad is a brave and amazing fullparametric 3D CAD program.

hebelmischer1.png (43.76 KiB) Viewed 1338 times

hebelmischer2.png (23.75 KiB) Viewed 1338 times

hebelmischer3.png (22.14 KiB) Viewed 1338 times

Best regards
Wilfried

[NormandC]

The 15mm radius between the handle and the cylinder was wrong, I corrected it

Well I'm not having much success myself.

The trouble starts with refining the solid:

FC_faucet_handle_04.png (15.08 KiB) Viewed 1331 times

The refine process breaks the solid:

FC_faucet_handle_05.png (63.49 KiB) Viewed 1331 times

And I'll add that your own model has the same issue:

FC_freecad-heini-1_einhandhebelmischer_02.png (67.93 KiB) Viewed 1331 times

But while I can't apply fillets to my model, you were able to with yours. This puzzles me.

I used a different process (PartDesign Body) but the end result is the same. The main difference is that I used a Revolution instead of a Sweep. Maybe I should try a sweep.

[freecad-heini-1]

But while I can't apply fillets to my model, you were able to with yours. This puzzles me.

Hi Normand,
In the German section was a discussion about the style from fillets, s-shape versus straight. Creo and Solidworks and others are using straight, Freecad uses s-shape. The trick is to split the model in the middle or design it as a half from the beginning. Please try this out and you will see that much more fillets are possible as expected.

By the way to recognize symmetry will safe a lot of time and features.

Best regards
Wilfried

[NormandC]

Even splitting the model in half, I don't get reliable results. Some values work, some others don't. Can't make 15mm under the handle, but I can make 14,90mm with PD Fillet - but only if I start small then change the value by small increments. Part Fillet won't work. I make a fillet, then the next one crashes FreeCAD.

Man, I can't wait for the OCC people to recode the fillet algo from scratch.