Fuselage Shell - error
With these areas highlighted, you won't be able to do it unless you make them bigger.
The reason you're having this error, is because you can't shell a body with a thickness value bigger than the smallest thickness value of the body, and that would cause the body to intersect itself causing the error you're facing.
At the top of the areas highlighted above, it gets smaller and smaller, so the 4 mm is too big for the shell command to succeed.
Saeed Hamza
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while there IS weirdness at the area indicated by @SaeedHamza , I'm going to point out the strictly speaking the cause for problem isn't simply that the area is to narrow. if the geometry is clean fusion can generally solve a thicken in a tight area like this. as and example if I take a spline that I I made-
extrude it into a surface-
and thicken it-
you can see fusion did fine with the thicken, even in the area that was narrower than the thicken value.
add some complexity though (just a little short line at the end)-
and things start to fall apart-
which is to say that thicken (and offset, and shell) are very sensitive to how clean the geometry is.
by trying to surface offset individual faces you can often find the problem areas when it come to using shell or thicken. this model has several faces that are problematic. the one I find most intriguing is this big one one-
isolated it mostly looks ok. -
but it won't thicken or offset.
I found that if I trim out this section-
it will thicken or offset. weird.
looking at the curvature comb, at first glance it doesn't look so bad (but not great either)-
however, if you look closely at the comb in the area that I cut out, we see the comb has some flat spots on the red line where I would expect it to be curved-
this is a resolution thing. a limitation of the curvature comb tool. it means at a smaller scale there problems with this edge, but the tool doesn't have enough resolution to really show it. but there is enough of a problem here to cause any type of thicken to fail.
might can be fixed in the original fusion model if you have it. dollars to donuts there is a modeling technique that could be improved to fix this. first place to look will be the underlying sketches.
Thank you for your helpful response. I appreciate your guidance and suggestions.
I have attempted to apply unstitching and thickening the surface, but it did not work for me. I still encountered errors .
I have also tried to cut off the edge of the surface that was causing problems and export it to SolidWorks, but I could only create a 0.5 mm shell there.
I think the issue might be related to the way I created the fuselage body.
The weird thing is that the fuselage body is made from a continuous spline with lofting, but the curvature combs show these strange steps.
I am planning to remodel the fuselage from scratch. If you have any tips or best practices for modeling wing-fuselage joints, please share them with me. I would be very grateful for your input.
I have to say, as in terms of the shell, I am very disappointed with Fusion.
I spent a few hours trying to make the hull as smooth as possible. In between, I kept testing whether the surfaces could still be thickened.
In the end, I extended the wing-fuselage transition again because I thought this was the problem. All the surfaces can be thickened individually - but not all together.
As a last attempt, I exported the solid as a STEP. After importing, it is sometimes possible to shell. But that didn't help either.
Now I was curious whether SolidEdge can shell the STEP.
It worked - and in a matter of seconds!
And now comes the most surprising thing.
The unprocessed part from @RJMathiyazhagan could also be shelled without any problems.
My new version from surfaces
The original from @RJMathiyazhagan
@RJMathiyazhagan wrote:...might alter the aerodynamic properties of the airfoil.
That comment is frequently heard here from modelers struggling with their model and coming here for help.
Did you use a different utility to produce this air foil shape and imported it into fusion? guess what, you already changed the shape of the airfoil. I spline created in any other program will be slightly different after importing into fusion. no getting around that. or maybe this IS the curvature quality your looking for in your air foil?
the following isn't a popular opinion among folks here who are into plane building, but IMO- If the air foil shape is so critical that it can't be redrawn to improve curvature quality causing it to be off .1 mm in places, then you are using both the wrong software for the project and probably the wrong manufacturing process also. the profile is already jacked upon import. basic law of surface work, surface quality will at best stay the same with each operation done to it, but will frequently degrade in quality by a degree. it won't EVER get better. the only way to make it better is to intervene manually and recreate natively.
@RJMathiyazhagan wrote:...I used splines with curvature constraints to create the airfoil edges. However, when I tried to use shell or thicken commands, I got an error message....
look at this screen shot-
you see how there is a peak in the comb at the top, but the rest of the comb has no value? and not note that the scale of the comb is at it's max? again, the issue with this edge is falling outside the resolution limits of the comb tool, so it's not telling the full story. basically the curvature at that point is for all intents and purposes approaching infinity. fusion (and computers generally) don't do infinity. I would hazard to guess that the curve at that point actually curls back on itself at a very small scale. check the sketch for the loft profile closest to this face. your going to find something is up with it.
...I would love to hear any tips or advice you have on how to model this type of fuselage skin more effectively, especially for the shell command....
sometimes getting a critique on what you've already done before restarting can be helpful. you could post your model (export as a .f3d) to get better help.
I have to correct myself.
I have now added the lower part of the fuselage to complete it.
Without much hope, I started the shell command anyway. I already set the clock to see how long it would take until the error message appears.
I think it took about a minute - then success!
Now I'm pretty confused...
@RJMathiyazhagan
Exporting a STEP, whether with Fusion or SolidEdge, should always be a last resort because you lose the history.
