Help Using Fillet Tool On 2D Sketch

[sebastiao_s_freire]

Greetings,

Real newbie here, trying to learn hot to use Fusion by completing practical examples and sort of get the hang of it that way.

I've found a lot of questions, here, and on other places with people having issues using Fillet, but they are all 3D Fillets, and complicated examples, and mine is a simple "problem" that I'm running into. The Fillet tool is behaving in a 'weird' way(maybe it's just weird for me bc I don't understand). I have a sketch on the ground(XY) plane that has a continuous outline. 

After doing some digging and asking chatgpt(ofc) I think the problem originates in this part, I take the outline, by double clicking a section of it, and it selects all of it, they I offset if "outwards" by, let's say 10mm(from what I could gather id this offsetting that makes fillet behave strangely afterwards). Then, I want to fillet some corners of this new outline that's the offset of the original one. 

When I select the Fillet and hover the corner, the preview shows fine:

However, when I actually click, to apply the fillet, it results in this:

Where the endpoints of the fillet curve don't even touch the lines...

Can anyone help me? Explain what's happening, or why(preferred, as this way I learn, but optional). And how I could go about fixing it.

Thanks in Advance

[kacper.suchomski]

Hi

First and foremost, you shouldn't use fillets in your sketches. This is bad practice.

Sketches must contain a minimal amount of information.

Fillets should be added during the modeling stage.

[g-andresen]

Hi,

Please share the file for reply.

File > export > save as f3d on local drive > attach to post

günther

[sebastiao_s_freire]

This is the file. I'm following a tutorial to making lightboxes based on a vector image

[sebastiao_s_freire]

Ok, I can understand why, however, I'm not sure how I'd achieve this without doing it in the sketch, since the part of the model I'm trying to do, is basically an Xmm thick plate based on the svg image on the sketch(so basically just extruding Xmm each section between the outlines and then coloring them in the slicer), and the fillets are to, when 3D Printing, be smoother for the printer, without so many sharp corners. Never tried to fillet after extruding in this case, but would the other sections near the line I'd be filleting into a curve, also follow said curve?

[TrippyLighting]

You downloaded a file to follow a tutorial, but as a complete beginner you don't have the knowledge and skill set to evaluate the quality of what you have downloaded.

This forum hosts thousands of thread where folks - very often other beginners - run into trouble with imported files. .dxf and .svg are often created by vector graphics software, which does not meet the requirements of Fusion's sketch engine. Often imported sketch objects do not meet the requirements for coincidence and or tangency. Sometimes they contain overlapping identical sketch objects. All of that frequently leads to problems.

These problems can be avoided using Fusion's native sketch and modeling tools.

Then following tutorials of other passionate hobbyists, often created in good faith and good intentions, but unfortunately questionable techniques lead to further problems. 

My recommendation is to follow the advice and instructions you receive in this thread. Fillets rarely belong in sketches. This isn't a rare case 😉

[g-andresen]

Hi,

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@sebastiao_s_freire  schrieb:

... but would the other sections near the line I'd be filleting into a curve, also follow said curve?

---

might help

günther

[Warmingup1953]

Give it a try as others have suggested. The fillet tool in the Design Workspace Solid Tab is easy and you can select multiple edges.

 

[TheCADWhisperer]

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@sebastiao_s_freire wrote:

 I'm following a tutorial...

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@sebastiao_s_freire 

What is the link to the Tutorial?

The geometry is a Control Point Spline (Degree 3) (both the original and the offset).  If you sketch a circle note that you cannot add a Tangent Constraint between the splines and the circle.  I am curious to see what the original Tutorial demonstrates.

[sebastiao_s_freire]

@TrippyLighting The tutorial, which I'll put the link down below, is just a guy following his usual workflow when creating lightboxes(which he does a lot), the SVG I downloaded myself as the 'image' for the lightbox, and when opening the .svg in both a text editor and inkscapes it seemed to be well-formatted which is why I went forward with it. As for your other comment, I wasn't in the slightest doubting what @kacper.suchomski said about being bad practice doing these operations on sketches and that it should preferably be done on the object, I was merely questioning if it would be applicable to the use case, and the reasoning behind that "good practice"(I'm not in manufacturing or modeling, but am also an engineer and have an habit of wanting to know things and the why's, guess that's just my engineering mindset taking over). Thanks for reinforcing and confirming that only in rare cases do fillets belong in sketches and this is not one of those 😉
@g-andresen Thanks for taking the time to record the video, it's going to be really helpful.
@TheCADWhisperer this is the link for the tutorial I was following: https://www.youtube.com/watch?v=6VUHmFcwIGM he starts with a png and uses vectorizer to create the svg, but in my case, I started with the svg already.
'@everyone who helped, thanks, I'll try to follow the tutorial, but an "adapted" version where I leave the Filleting to when the object is already extruded and in 3D.

PS: The 'solution' that chatGPT came up with, prior to me asking here, if you're curious, was that the offset lines and points did not have the same geometry as the original outline, and to transform the offset into construction lines and then redraw with splines along those lines, It did work but it was a mess ^^
I'll post the results 😉 Thanks once again to everyone that helped.

[TheCADWhisperer]

@sebastiao_s_freire 

As a general rule you want to keep sketches as simple as possible.  Each sketch Fillet creates two Tangent Constraints (except in this case because of the geometry type), two Coincident Constraints, and trims the original geometry.  All of this adds complexity to the sketch solver.

Depending on what you are doing with the sketch Offset, it might not even be needed.

There is a relatively new tool Extrude - Thin Feature that negates the need for many sketch Offsets.

As you continue your Fusion endeavors you will also learn to simplify sketches by avoiding (where possible and practical) sketch mirror and sketch pattern.  

It is more computationally efficient to mirror/pattern bodies, faces, features or components.  These techniques transcend across all parametric CAD softwares, not unique to Fusion use.

Of course, there are use cases where sketch Fillets, Mirror, Pattern are appropriate but first consider other techniques that simplify the compute of the sketch solver.