Unable to Fillet Lines for Creating a Curve Radius
First thing I notice is that there are no dimensions on your sketch.
Second thing I notice is that the sketch is not making use of obvious symmetry about the Origin.
Third thing I notice is that you have a 3D sketch...
What is your end goal - what do you want to design?
Do you have a picture of something similar from the real world?
What radius of Fillet do you want?
Can you add the Fillet to the solid feature rather than to the sketch?
Thanks for the tips I'll work on these. Thought by having the 3D sketch enabled it would allow me to visualise it better.
@TheCADWhisperer wrote:First thing I notice is that there are no dimensions on your sketch.
Second thing I notice is that the sketch is not making use of obvious symmetry about the Origin.
Third thing I notice is that you have a 3D sketch...
@TheCADWhisperer wrote:What radius of Fillet do you want?
Can you add the Fillet to the solid feature rather than to the sketch?
Was trying to test some radiuses out, to get the desired result. minimum I was going to start at was 10mm.
Not sure I can add the fillet to the solid pipe/sweep.
@TheCADWhisperer wrote:What is your end goal - what do you want to design?
Do you have a picture of something similar from the real world?
Thank you for the example. I tried to follow your steps. However, I kept having issues with constraints and trying to get it fully constrained, any tips?
Also, would you know how I can get this curve to project to surface? I get the error below.
It is best to stop and resolve each issue as it occurs.
Click and drag these 2 Points (the most powerful tip in all of Parametric CAD - not just Fusion 360).
What do you observe?
Follow along on the next few steps...
How will you measure these dimensions in the real world - and why are there any repeated dimensions?
What you should have observed from the click and drag test is that this line is
1. Missing a Vertical constraint.
2. Not constrained to the Origin.
So we add those two missing constraints.
Now the left side is not where we intended...
Sketch a construction line from the Origin to the Midpoint of the line at left.
Now add a Horizontal constraint to the line (this should have all been done at the outset).
This short line at the left is missing a Vertical constraint (this should all be automatic) or a Perpendicular constraint to the Construction line.
We Click and Drag test again and notice that these two lines are missing Tangent Constraints.
...but we notice that there is a "strange" angle dimension...
Double click on it and it is even stranger...
Let's delete that.
After deleting we notice that the geometry at the left slides horizontally left to right (the old Click and Drag test - the most powerful tip in all of parametric CAD).
So surely in the real world there is a regulation distance between the center of the hoop and the mounting face of the backboard.
I try to add the dimension but when I change it - I notice there is this arc - it is missing a Concentric constraint to the circle.
I add the missing Concentric constraint and all is constrained with only 4 dimensions.
Fix up your file and Attach it here again.
Blue lines and white dots should keep you awake at night.
The click and drag technique reveals some obvious issues with your sweep sketch.
You need to tie together the sweep sketch with the rim sketch using Project (mash p on your keyboard) and select relevant points.
None of those dimensions are needed (they have already been defined in the rim sketch.
And two of the dimensions do are repeated, do not make logical sense (cannot measure anything in the real world out to 8 decimal place) and put the circle in the wrong location to boot.
You don't have to use construction lines (they merely make Design Intent obvious), but you have to do things right.
