Correct way to Fillet?

[atrueresistance]

I'm trying to apply a fillet that folds shield down at edges, but can't seem to get it to work without some type of error. Any suggestions? 

I'd like to get all the edges for everything folded so it is a smooth transition for full 3D CNC milling. 

[kellings]

Try to start with a really small value like .005. If that works, then you can start to increase the value of the fillet until it fails again. I might try .005 and then if that works, I would try .01, then .05, and so on until you get as close to the .125 fillet that you were trying to place. 

I wonder if the issues are in the places where the profile creats the v shapes. It may be too tight in those places to work. It may help to add a vertical fillet at those interesections first and then you can try to add that .125" fillet again. 

[Anonymous]

Yeah, those sharp v areas look suspect.  I would, from within the sketch that made the extrusion, try filleting those sharp corners/angles.  If you have real difficulty finding the problem, you could create a sketch on the top or bottom of the shield and draw some lines that can then be used as tools for Split body, so that you can then try filleting different sections of the shield. 

Good luck!

Jesse

[kellings]

Its a little bit 6 of one, half a dozen of the other when it comes to the fillet method. If the fillets are added to the sketch and it doesn't help and the original profile is desired, you have to go and do some work in the sketch to fix things. If you add the fillets to the solid model as a feature, you can just delete the feature in the tree and no extra work is involved to get back to the original extruded profile. 

I try to stay away from sketch fillets unless it is necessary to do the fillets in a sketch. 

[Anonymous]

It's interesting you mention that, as I was just remembering someone else say something similar and was wondering why.  Using the 3D model fillets are certainly fine, but I just tried something that also seems to work.  I just used a user created parameter for the radius of all the sketch fillets.  Then if you want to quickly modify OR remove the sketch fillets, simply reduce the user parameter to an infinitesimal value, such as .01 or .001 inch. 

I'm curious if there are other reasons not to go the route of creating fillets in sketches, but this workaround seems like an interesting thought.

Jesse

[kellings]

I haven't been using Fusion as much as I would like to the past couple of months. I've been focusing on the CAM portion of the product instead of the modeling. I'm more experienced with Inventor. So I haven't doug into parameters much yet. In Inventor pretty much anything that can have a dimensional value can be controled with a named parameter including features. 

Maybe someone from the Autodesk team can speak to this subject, but features seem cause less of a performance hit than adding things at a sketch level (especially when the sketch gets very complex). The rule of thumb I learned is that if the feature can be added as a feature instead of in a sketch and you end up with the exact same result, it should be created as a feature instead of a sketch.

The other reason I do it this way is for future part variations. If you add things like fillets at the sketch level and later you want to create a variation of that part that doesn't have fillets, or not all of the fillets, it is easier to edit the feature to remove the fillets you don't want. Otherwise you have to go into your sketch an do it and depending how that sketch was built, it could take a little bit of work to fix things up. 

[JamieGilchrist]

This is a great discussion around best practices in modeling.  I certainly advocate for not putting fillets in sketches whenever possible.  That's not to say "never", for instance if part of the design intent in the sketch requires a fillet then by all means put them in the sketch.  If, however, the filets are only secondary or tertiary level of detail/transitions required for manufacturing, I almost exclusively use fillets as features rather thank sketch entities.  Two reasons:

1.  In the event that you find yourself working with a problematic model, the simpler the feature set that defines the geometry, the easier it will be to diagnose and fix any problems.  Sketches should be distilled down to be as simple as possible, the definition of "simple" is entirely up to the designer or the standards set by a company.  This principle helps reduce the burden of corners <pun> one can paint themselves into in a parametric modeler (this is not unique to Fusion; Inventor, PTC, Solidworks, etc. all can support poor modeling practices that end up with a model that can become riddled with problems and errors).    A very simple illustration of this is say I have a shelled part, the primary shape is built from a  sketch with all the fillet details necessary to create my finished plastic part design.  If that shell fails to meet the requirements of the thckness that you as the user needs to determine "where" that failure is occurring.  Experience tells me that the failure will likely be in the radii of one or more of the fillets.  now I have to edit my sketch to find the problem and the potential for downstream features to be compromised greatly increase and you'll often end up "hacking" the modle to get it to just work so you can move on.

2.  If you are working on somebody elses model and need to "fix" a problem area or add additional detail, say add some reference to a theoretical corner that is filleted, if that geometry exists in the sketch, but not the model, It's pretty easy to make the necessary reference.  If your collaborator adheres to this modeling principle then your job can get done much faster and subsequent users won't be looking at "hacky" models.

good talk.

[Anonymous]

Great points, I'm taking notes 🙂

[JamieGilchrist]

hi atrueresistance,

try turning off tangent chain in the fillet tool and gradualy add more sections.  You'll quickly find where the fillet is failing ( I agree with the others, it's likely around the sharp "v"s in your design).  try going toa 0.06" radius and shee how that works.  If the "v"s are in fact where the problems are you may have to live with a smaller radius fillet or alter the design to accomodate the larger fillet.  I'm curious to hear what you find.

hope this helps.

[JamieGilchrist]

if you can share your model I' can also take a look to see where the fillet is failing to build.