Fillet bug on a simple shape (video included).
Neither of these fillets should be part of that sketch.
Apply the fillets as solid features.
Less work.
Better computing performance.
More stable model behavior.
My language makes sense to those who are not completely new to CAD 😉
It is your choice whether or not to follow that tutorial or take the advice of a degreed engineer with 30 years of professional experience in 3D modeling and CAD.
What I was trying to convey is to sketch the rectangle and maybe the two holes.
Then extrude the piece.
Then in the "solid" tab use Modify->Fillet and select the edges you want to be filleted.
Applying fillets in sketches is sometimes needed but when it can be avoided such as in this case it should be avoided.
Would you be able to do a quick screen capture showing how you would do that?
@davebYYPCU wrote:First the upright end of you Part has at least two upright lines, one remains in position,
Your fillet trims some of the line not needed after the command. Your line length was not the same as the fillet radius, so Fusion stretched the left over portion. If you were filleting with a half block radius it would not happen.
in other words, if the blue line was constrained to not move, (vertical) it would have left you with a really short line connection to the lower upright line, but because the resulting really short line does not have to be vertical, it stretched.
I'm not understanding you. As far as I can see I do have a constraint.
The reason that does not work is that none of the sketch objects are fully defined (constrained or dimensioned) and that allows the sketch objects to move within the few contains that do exist.
That is EXACTLY one of the reasons why you don't apply such fillets in a sketch.
Have you considered asking the author over Linkedin why this does not work as expected?
Also, I'd love to see what the final piece is supposed to look like. If what you are doing would actually work you'd have a full round fillet. But, in that case, you would sketch a 10 mm half circle and not first make a rectangle and the 2 fillets.
Also, please share your design so far. Export as .f3d and attach to next post.
To replicate the sketch from your video, I get the weirdest results, I cant get anything like normal behaviour when starting from the rectangle..
Two sets of concentric circles and horizontal tangent lines does work.
Might help.....
Hi luckymethod,
I'm going to address your questions in two ways.
1. Yes, I believe this is a bug and I've forwarded your video and a file on to our sketch development team. I'm able to easily replicate this.
2. And, as for much of the advice in this thread, There are better, more stable methods to build this type of geometry in Fusion. While the lessons author shows a method that I understand you're attempting to follow, his method is not one I would promote as a best or even good practice for parametric modeling sketches.
Here's some different approaches to consider:
Starting at the bottom of the attached image, is the tutorial authors method, which I would not advocate for. Advice I like to give people is:
- always keep your sketches as simple as possible
- distill your sketches down to their most basic geometric description whenever possible, i.e. if you don't need to trim a circle, don't
- the simpler the sketch, the easier time you'll have troubleshooting problems with models and assemblies when the arise.
- If possible leave details, such as fillets and chamfers (as @TrippyLighting suggests), out of the sketch, unless absolutely necessary for them to be there. Those details are far more robust as model geometry than sketch geometry.
- Always remember there's more than one way to achieve what you're working on.
Jamie Gilchrist
Senior Principal Experience Designer
