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Frustrations with fillets

Question asked by David Sutton on Mar 24, 2019
Latest reply on Mar 27, 2019 by David Sutton

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I'm modelling a bracket that has a 7 degree draft feature applied to each side. I need to add an 0.62" fillet at the base of each drafted side.

The fillet generates without issue on one side but throws an error on the other side. Both sides are identical so I can't figure out why this is happening.

The attached pics show the messages I'm seeing. I also attach the Solidworks file if that helps. Does anyone have any advice for me please? I'd love to get a handle on the conditions required for a fillet to work correctly.

Paul Salvador Mar 25, 2019 10:17 AM

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Hey David,.. seems like a rounding error.. **it happens,.. as a workaround, change the Profile option to "Curvature Continuous" ... done.

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Jeff Holliday Mar 24, 2019 7:20 PM
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Not sure but did you try adding the radius before the draft?
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- David Sutton @ Jeff Holliday on Mar 25, 2019 4:05 AM
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  Thanks for the suggestion Jeff. I've just given it a try but unfortunately it resulted in a concave (carved out) area at the base of the draft.
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Jesse Robbers Mar 24, 2019 7:29 PM
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In sketch2 there is a line that is under defined, was lacking tangent relations to the radius at each end of this line. This doesn't fox your problem, but something to take care of.

For your Draft1, Draft3, & Draft4 features, it results in a funky curved face, is this the intent or desired result? Or can these faces remain planar? If planar is acceptable, then the fillet will resolve on both sides of the part. If this isn't acceptable and you want to keep that funky curved face, then model 1/2 of the part and mirror the body....or make this curved face in another way.

This doesn't solve the problem or behavior we see here, but you could at least get thru it to the other side using one of the above options.My preference would be to make those drafted faces planar which will allow the fillet to terminate better as well.
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- David Sutton @ Jesse Robbers on Mar 25, 2019 4:33 AM
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  Well spotted Jesse, I'll get that fixed. It's the result of another frustration I have - when copying a fully defined sketch, some or all of the relations are lost. The original sketch was fully defined.
  
  In terms of the funky draft, it does indeed look odd but is part of the original design that I'm attempting to recreate (see attached engineering drawing). The strange bulging curves had me confused at first but when you apply a 7 degree taper from the top edge of a wavy profile (changes in height) then the base of the taper does end up like this.
  
  I'll give your mirroring suggestion a try thanks. I'm not sure if I should always be attempting to use mirror when a part is symmetrical? Is that one of the standard good practice rules? I worry a little when the mirror line cuts through a curved area like the filleted horse shoe area in this item. Will the half-filleted part form a smooth curve without an obvious transition point when mirror is applied later?
  
  So much to learn....
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  - Jesse Robbers @ David Sutton on Mar 25, 2019 11:38 AM
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    It seems like you're stuck with this funky bulged side detail. I think you have to muscle thru it. Using any mirror or patterning type feature just saves you work later on, whether it's replicating features in identical way, at different positions, or time/work to repair things as the design changes so that you can focus your time and intent on the seed feature. Things can be mirrored in the sketch, but it's a bit more robust and simple to mirror the feature(s) or the body later on and in your case for this trouble part mirroring the body (the side that the fillet resolves on) would be the way to go to get thru it so you can get onto something else.
    
    For this line where it's mirrored about, sometimes there is a visible line there (not an actual hard line or edge but just a tangent lines visible type of line). Sometimes there isn't this line there, sometimes these lines are convenient on the drawings. If your parts are modeled so that the face/surfaces about this centerline it's mirrored about is good, it is collinear, tangency, etc..., then it should just be a visible line you see and not an actual line or edge on the part. You can use zebra stripes or curvature tool to check things like this across surfaces or throughout surfaces for confirmation.
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    - David Sutton @ Jesse Robbers on Mar 26, 2019 4:47 AM
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      That's very helpful Jesse, thanks for the great explanation. I'll be using much more mirroring in future.
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Paul Salvador Mar 24, 2019 8:03 PM
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..make it simple, create a neutral plane at the crest of Sketch7 and draft the faces (that is, do not use parting lines... image)
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- David Sutton @ Paul Salvador on Mar 25, 2019 4:42 AM
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  Thanks for stepping in again Paul. Please see the original engineering drawing above. The bulged draft does seem like overkill but gives them some extra material which remains after a subsequent milling operation. Maybe it was easier to make the mold pattern that way too? Would be nice to understand why Solidworks has problems creating a feature like this but I'll try the mirror approach to get me past this issue.
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  - Paul Salvador @ David Sutton on Mar 25, 2019 10:17 AM
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    Hey David,.. seems like a rounding error.. **it happens,.. as a workaround, change the Profile option to "Curvature Continuous" ... done.
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    - David Sutton @ Paul Salvador on Mar 26, 2019 4:25 AM
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      Nice one Paul, that fixed the issue nicely. I need to read up on curvature continuous as I'm not sure what it means really. My guess is that it allows the curve to be slightly out-of-round to produce a fit. It's an amazingly complex thing to ask it to do really on wavy edges like this.
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      - Paul Salvador @ David Sutton on Mar 26, 2019 10:28 AM
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        ..it's a workaround, the radii is not "rolling ball" (arc / analytical) but a blend (algebraic curve)... but the draft is not analytical so.. from my perspective/experience.. does it really require a rolling ball fillet?
        btw, as the others suggest, because this part is symmetrical, the mirror is the better/consistent way to model.
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        David Sutton @ Paul Salvador on Mar 27, 2019 1:23 PM
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        Understood Paul, I'm just trying to get as close as possible to the original but the drawing is pretty vague anyway with respect to the fillets.
        Redoing the part using the mirror approach. Thanks again for the pointers.
        
        Dave
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Tateos Tvapanyan Mar 25, 2019 5:36 AM
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It's not answering your question, but you can work around this by splitting the part with the Right Plane and after that mirror the body.
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- David Sutton @ Tateos Tvapanyan on Mar 26, 2019 4:29 AM
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  Thanks for the suggestion Tateos. I gave that a try too and it worked perfectly. Will start using mirroring more often now. Am I supposed to tick the "Knit Surfaces" option when applying the mirror?
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  - Tateos Tvapanyan @ David Sutton on Mar 26, 2019 9:51 AM
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    "Knit Surfaces" is relevant when you mirroring a surface body.
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Steve Labonte Mar 25, 2019 8:38 AM
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Hi David,
under fillet options check curvature continuous. when working with multiple draft angles decimal places aren't carried out far enough causes issues. before you added the .62 rad look at the small feature areas on either side you will notice they measure different
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- David Sutton @ Steve Labonte on Mar 26, 2019 4:33 AM
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  Thanks for the great explanation Steve, that worked a treat.
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Ruben Balderrama Mar 25, 2019 10:04 AM
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Cut half with a surface and mirror
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- David Sutton @ Ruben Balderrama on Mar 26, 2019 4:45 AM
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  Thanks for your assistance Ruben, I'm learning so much from you guys. I'd really be stuck without this forum as I don't find the Solidworks help system particularly helpful.
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David Sutton Mar 26, 2019 4:48 AM
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I've just realised the responses aren't listed in time order so I apologise if my replies seem inappropriate.
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Frustrations with fillets

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