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Unable to Fillet Lines for Creating a Curve Radius

23 REPLIES 23
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Message 1 of 24
wallmachine
769 Views, 23 Replies

Unable to Fillet Lines for Creating a Curve Radius

anyone able to confirm why I can't fillet these lines to create a curve radius and a solution.
23 REPLIES 23
Message 2 of 24

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_0-1691323432909.png

 

@wallmachine 

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?

Message 3 of 24

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_0-1691323432909.png


@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?


hoop.png

Message 4 of 24

@wallmachine 

Examine the Attached file...

TheCADWhisperer_0-1691362153240.png

...not quite right, but with just a bit more work...

Message 5 of 24

@TheCADWhisperer

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.

error.png

Message 6 of 24

@wallmachine 

It is best to stop and resolve each issue as it occurs.

TheCADWhisperer_0-1691427295953.png

Click and drag these 2 Points (the most powerful tip in all of Parametric CAD - not just Fusion 360).

What do you observe?

Message 7 of 24
wallmachine
in reply to: wallmachine

@TheCADWhisperer 

Apologies, not sure how to explain it but when moving those paths the move tool can only move in one direction so I think the other axis is not constrained and I need to create a construction line to be able to constrain it on the other axis.

 

I did managed to get each sketch fully constrained, after fiddling about, whether its right way...

Message 8 of 24

@wallmachine 

Follow along on the next few steps...

TheCADWhisperer_1-1691495183546.png

How will you measure these dimensions in the real world - and why are there any repeated dimensions?

Message 9 of 24

@wallmachine 

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.

TheCADWhisperer_0-1691495330988.png

 

So we add those two missing constraints.

TheCADWhisperer_1-1691495374765.png

Now the left side is not where we intended...

Message 10 of 24

TheCADWhisperer_0-1691495518933.png

@wallmachine 

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).

 

TheCADWhisperer_1-1691495643107.png

 

Message 11 of 24

This short line at the left is missing a Vertical constraint (this should all be automatic) or a Perpendicular constraint to the Construction line.

TheCADWhisperer_0-1691495736055.png

 

Message 12 of 24

We Click and Drag test again and notice that these two lines are missing Tangent Constraints.

TheCADWhisperer_0-1691495846218.png

 

Message 13 of 24

...but we notice that there is a "strange" angle dimension...

TheCADWhisperer_0-1691495922419.png

 

Double click on it and it is even stranger...

TheCADWhisperer_1-1691495949673.png

 

Let's delete that.

Message 14 of 24

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.

 

TheCADWhisperer_0-1691496183493.png

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.

 

TheCADWhisperer_1-1691496275546.png

I add the missing Concentric constraint and all is constrained with only 4 dimensions.

 

Fix up your file and Attach it here again.

Message 15 of 24
wallmachine
in reply to: wallmachine

@TheCADWhisperer 

Thanks for the step by step.

 

Everything seemed to be okay until I got to "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 did not get this arc.

Message 16 of 24


@wallmachine wrote:

@TheCADWhisperer 

- I notice there is this arc - it is missing a Concentric constraint to the circle.


At 1:03 in your video you add a Coincident constraint between the centerpoint of the arc and the Origin.
This is essentially the same as adding the Concentric constraint and why it is a little bit different for you.  The end result is the same.

I am not at my Fusion machine at the moment to check your Sketch 2.

I will look at that when I get a chance and also answer your question about Project>Include geometry in the 3D sketch.

Message 17 of 24

@wallmachine 

Blue lines and white dots should keep you awake at night.

TheCADWhisperer_0-1691583400913.png

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.

Message 18 of 24

@TheCADWhisperer 
With the latest update. I used the project feature, a constraint and sketch dimensions, would it have been best to use construction lines?

Message 19 of 24

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.

TheCADWhisperer_0-1691600365854.png

 

You don't have to use construction lines (they merely make Design Intent obvious), but you have to do things right.

Message 20 of 24
wallmachine
in reply to: wallmachine

@TheCADWhisperer 

Thank you for the tip re 8 decimals I will switch up the design to be a whole number or +/- 0.00. I also followed along with your suggestions re- the constraints, much simpler 👍 

 

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