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How To Evenly Fillet Complex Surfaces In Solidworks?

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I'm currently blanking out on how to solve this problem in Solidworks:

 

If you take a look at the image attached, you will a few random wavy surfaces, with a yellow highlighted fillet between two of them. My problem is that this fillet is terribly uneven. If you look to the left of the picture, it fills out the gap between the two blue lines I placed, but to the right in the picture it's so small it almost disappears.

 

Now, those blue lines are actually my second problem as well, because I had to manually place them there, and I know that they are not perfectly offset compared to each other, when they end up being projected onto the surface. I could probably generate an example where those blue lines converge as extremely as the fillet does, but perhaps by now you understand my problem and have encountered this before and know a solution?

 

I have a third and fourth problem to discuss as well, if we can get this topic going. :)

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Surface_fillet_tests.zip

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Can somthing like this be used... Just unsupress the files in the sw file since it was over 1mb...

 

Ah, thank you! I spotted my mistake now... I didn't do the split lines, which enabled me to select an edge when using the boundary surface tool, and that's why I didn't see the tangency/curvature options (since I was selecting the whole face), which had me stumped.

 

And I just tried the same thing on the middle part of the surfaces with those other two lines I put there, and it worked brilliantly (much better than my whole surface rebuild, which was a very, very bad solution). So that answers question one.

 

Anyone for the second problem now?

 

When you delete the faces to make room for that boundary fillet in the pictures above, you can really see that even those two split lines wave quite a bit back and forth. The distance isn't constant between them. So, is there a trick to making them constant, even between these very irregular surfaces?

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Guest schwinndk

hmmm.. I haven´t seen that kind of Isoparametric Curve tool in sw before. I know that Rhino has it dough.. But there might be a way around it. I will post somthing if I think of it..

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Solidworks does have the ability to create this type of blend, it's under fillet -> face fillet, and the option checkbox "Constant Width" makes this happen. For some reason however the feature fails on this geometry.

 

Not to worry. I suggest you open up a 3DSketch and create a spline-on-surface. Click on the left edge, twice on the surface, and on the right edge - making a 4 point spline. Do this for the top surface, and for the bottom surface.

 

Attempt to space them apart roughly equidistant from each other.

Then drag the spline points and tangent/weight handles until they match up.

 

This isn't "mathematically" perfect but when the the maths fail, you've got to do it manually, just keep working on them - trim 'em and boundary surface with "Curvature to Face" and watch the purple curvature combs for a smooth comb, adjust the "Tangent Length" box to attain it.

 

Hope this helps!

Kevin.

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You ask a lot my friend.

 

You could try an equal distance Fillet - otherwise this is an approximation.

 

Holy crap! That's an amazingly impressive solution, and it doesn't look like an approximation at all, but actually correct!

 

I have only one question: The 3D sketch in "Oberfläche-Ausformung3"... how did you do it? I assume it is some sort of projection, but how was it made?

 

Solidworks does have the ability to create this type of blend, it's under fillet -> face fillet, and the option checkbox "Constant Width" makes this happen. For some reason however the feature fails on this geometry.

 

I suspected that was the case by looking in the help files, but I've not actually yet managed to create a surface on which the tool works. Quite poor, imo. Perhaps they'll make a new one that's more flexible some day, like when they went from loft to boundary surface and surface fill...

 

Not to worry. I suggest you open up a 3DSketch and create a spline-on-surface. Click on the left edge, twice on the surface, and on the right edge - making a 4 point spline. Do this for the top surface, and for the bottom surface.

 

Attempt to space them apart roughly equidistant from each other.

Then drag the spline points and tangent/weight handles until they match up.

 

Thanks for the tip. Very interesting tool, but ouch. Yes, I can see myself doing it for these completely organic shapes, but if it would have been a curve built with arcs or ellipses it sounds like a nightmare to match up.

 

But perhaps eezydo did use that spline-on-surface to create his solution somehow... I'm very interested to see his answer.

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Guest eezydo

I think its called "Face curves" in english. - the little Grid icon in the sketch toolbar.

It gives you the Isoparms.

Check "position" at 50% to make it run along the middle of the surface.

post-9393-1253797492.jpg

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Guest eezydo

If you make the gap very large though its likely to deviate , as the cut relates to the

surface shape near the edge.

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I want to add: Spline-on-Surface isn't my favourite way to go either usually, but what it gives you though is a lot of control. It's almost like a feature that you can use to "trick" Solidworks into allowing you direct editing capabilities.

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I think its called "Face curves" in english. - the little Grid icon in the sketch toolbar.

It gives you the Isoparms.

Check "position" at 50% to make it run along the middle of the surface.

 

Really cool, that's the second new thing I've learned today. Thank you!

 

However, it is really unfortunate that you are using an old version of Solidworks, because while it works on your example, it doesn't on mine. See, my example is deliberately extremely wavy and twisty (see attached images... I call it "wave surfacing" :) ) and any surface offset I attempt either self intersects or intersects with the other surface.

 

Now, I instead tried to draw a normal at the center of each surface (using the face curves I've just learned) and move a copy of them using that as a workaround, but even though it to the naked eye looks rather good, when measured it's still off.

 

I'll continue to experiment to see if I can find a correct solution, but again, thank you for all your tips so far!

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Absolutely bloody wonderful! Thank you for that solution!

 

When measured, the distances only differ about a fraction of a millimeter, and that's good enough for me right now (Solidworks doesn't do proper Class A surfaces anyway, I believe).

 

As long as you can offset the stiched surfaces, the solution works. If anyone can find a complicated enough surface where it fails, I'd be interested to see it, but as far as I'm concerned:

 

Solidworks now has "chordal fillets", just like Catia V5 and Alias Automotive 2010. :)

post-526-1253879474.png

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Guest eezydo

Glad it worked.

I did make it fail and be less precise - have to play with the offset distance.

But after all its just a workaround.

 

.... Yeah sometimes Catia would be nice.

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