Fillet not behaving as expected with extruded sketch and loft command

[Anonymous]

I'm new to Fusion 360 and I am currently trying to understand if I am using the Fillet command properly or if I have hit a limitation of the software.

In the video, you will see that I have create 2 sketches. The first one that is extruded and lofted, already contains a Fillet that I made in the Sketch. After extruding the sketch, copying it 2 times and lofting together the resulting bodies, the edge are properly aligned between the 3 lofted bodies.

In the second example, this is where I am having the issue with the Fillet command. This sketch doesn't have any fillets. I extrude it, copy the result 3 time and use the loft command to connect the bodies and then apply the Fillet

command on some of the top edges. The result is not correct, the edges created by the fillet command are misaligned and don't connect properly. The resulting topology is not smooth as I would expect (and like it should be compared to the first example). This is even more visible if I convert the body to a mesh, there's a lot of extra triangles when the edges are supposed to connect after the Fillet operation.

Is my workflow correct and what I am trying to do possible in this order of operation? I know that I can create the desired shape from a Sketch that contains already the fillets, but my goal is to do it later in the process, like in the example number 2 (the sketch that doesn't have any fillet initially).

Can anyone replicate the issue? Or please tell me what I am doing wrong.

Thank you.

Edit: Please give me a moment to insert the screencast. It was inserted when I posted it, and now it's not showing. I get the following error:

"Your post has been changed because invalid HTML was found in the message body. The invalid HTML has been removed. Please review the message and submit the message when you are satisfied."

Edit2: Here's the direct link. I can't insert it in the post.

https://knowledge.autodesk.com/community/screencast/fab0bb03-6b9b-4e77-8364-bf8af1687cb6

[jhackney1972]

Please attach your model that you showed in the Screencast.

[Anonymous]

Hi,

Here it is

[laughingcreek]

maybe this clears things up for you-

[laughingcreek · Accepted solution]

FWIW-loft isn't really the ideal choice for this situation.  (usually isn't for strait and/or flat objects).  sweep is what you want here. it will maintain the shape of the profile.  see attached.

[Anonymous]

Thank you for your workflow solution (sweep operation approach). It's working perfectly!

[Anonymous]

I've just made some more tests today, using the Sweep method suggested, and I found out that it only works when using the perpendicular orientation. When using the Parallel orientation mode, I get the same issue where edges don't align properly. Do you think that it should be reported as a bug or something that they should fix or improve?

[laughingcreek]

of course the angle changes when using the parallel orientation.  for the same reason it did when lofting it.  your moving the profile along at a skewed angle to it's path.  no, it's not a bug.  it' doing exactly what your telling it to do.

look at the attached.  only difference is the perpendicular/parallel setting in the sweep.

[Anonymous]

I understand and thank you for your answer. In terms of workflow, would it be realistic to hope that the fillet command handles this in the way I am expecting it to do it? I've posted the question in the Support forum (because I thought it was a bug, but also suggested improving the feature if it's possible and if it's not a bug like you've just explained to me).

I would love the Fillet command to create clean topology automatically, from extruded Sketches and lofted objects or with the sweep method using the parallel or perpendicular mode, if that's realistic of course. The resulting workflow would be really straightforward.

Again, thank you for taking the time to answer my questions, greatly appreciated.

[laughingcreek]

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@Anonymous wrote:

... In terms of workflow, would it be realistic to hope that the fillet command handles this in the way I am expecting it to do it?

No, it's not realistic.  the geometry created would be undesirable in many cases.  Particularly if your a machinist.   or even if your modeling and expecting that "filleted edge" to have an arc for a cross-section.  when the angle between the faces changes, somethings got to give.  if you look at the cross -section of the fillet sweeped at an angle you would see it is no longer an arc, but parabolic in shape (1/4 of an ellipse to be more precise). 

fillet isn't really a modeling tool.  it's a finishing tool used at the end.  any other needs should be addressed with other tools.