Problem creating a complex shell

[Anonymous]

I am tearing my hair out trying to create a complex shell to be 3d printed.  It is a helicopter fuselage that I have poured countless hours into modelling.  I have set up loads of profiles and rails, and used the loft command to create a patchwork of individual surfaces.  Then I hit a brick wall - what is the correct workflow here?  I have tried stitching the surfaces together (fine), but the resulting surface will not thicken.  I can thicken individual surfaces and then try to join them together, but this ultimately fails too (some of them will join fine, others not).  I get simple error messages like 'operation failed' and no diagnostics to tell my why this will not work.  It is enormously frustrating.  I really don't want to try merging all of the surfaces in the form environment as it isn't parametric and after it fails or I get weird shapes I cannot go back a step (no timeline in the form edit mode).  There are no tight radii that I can see, and the thicken fails in either direction for any amount  I am just trying to use the wrong tool for this?  Is some other software better?

[TheCADWhisperer]

The image looks pretty rough, especially that one pinch point.

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Overbuild surfaces and trim.

[Anonymous]

Rough?  thanks . . . I have (in later parts of the timeline and project) tried overbuilding and trimming, and also had issues there.  But let's start with the nose as that has the most complex curves - in fact, I did try combining two shapes initially and doing a trim, but got 'compute failed' errors on that too, from what I could only guess was due to the shapes being tangent at one section (where the nose cone and windscreen blend into one).  I have exported a f3z file (doesn't seem to allow exporting of f3d anymore?).  Many thanks for looking at this.

[TrippyLighting]

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@Anonymous wrote:

Rough?  thanks . . . 

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Yep, rough 😉

A surfacing project usually does not involve T-Splines and you should definitely not overbuild and trim T-Spline based NURBS surfaces.

You've got curves and should use surface lofts to create these surfaces.

If you do a design with T-Splines, then the whole fuselage would likely be one T-Spline

[Anonymous]

I have used lots of lofts for this.  Then what?  Stitch and then thicken?  Thicken and then join?  Either approach seems to fail.  By the way Peter, I did successfully get the tail boom done (and printed) by building it from scratch myself instead of going with the imported .obj file and trying to manipulate the resulting messy mesh, so a bit of a victory there.

[TrippyLighting]

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@Anonymous wrote:

I have used lots of lofts for this. 

Yes, but those are T-Spline lofts, not lofts created with the tools in the Surface tab.

[laughingcreek]

It's also not surprising that you can't thicken this, since all of the surfaces are "near tangent" at the edges (which gives fusion a lot of trouble) rather than tangent.

[colinNJB25]

My first Fusion project was guitar necks and learning the software and dealing with all the issues were very frustrating. I spent about 9 months modeling my first neck the was producible. Now, it is a matter of a few hours for me to draw a neck but I also spend 30 to 40 hr a week using Fusion for my day job.

To make this part I agree working in the surface space is the fastest method. When I have designed airplane fuselages I have done a series of sketches as cross sections and lofted between them. Since I build by hand the sketches surfaces the further use as a template for the construction. The nice thing about that is you can pull on the splines and watch the shape in real time. I think I would use 4 or 5 sketches across and 3 down the length that will become rails.

Thickening a surface is much more reliable. 

[Anonymous]

Ok, so I should use the 'surface' loft instead of the form 'loft'.  I have just tried that, then stitched them together, tried to thicken (under the surface menu) and  . . . computer says no.  Actually, the second time it said no.  The first time, the whole laptop went down (not seen that happen before).

What is the difference between the two, given that they both fail?  There is also a 'thicken' under solid and under surface - are they the same?

[Anonymous]

I can see that the surfaces are 'near' tangent.  I have tried my best to make them tangent, but can see no way of forcing a tangency constraint.  What are you proposing as a solution to that?  What am I missing here?  I cannot see a way of doing that when you stitch surfaces together.

[colinNJB25]

Step Through this time line. It is only one way to do it and I have not made any attempt to constrain the sketches. If you turn on the three sketches you can drag the points around till you have the shapes you like. You could also add rails on the other axis to make the curves you want.

[laughingcreek]

have you corrected the surface edge conditions?  You might want to attach your latest attempt.

The accuracy of a form loft is going to be determined by the number of faces you use, and isn't going to be good enough to get good stitched results.  it's also not going to be parametric.  many used to rough out a basic shape that gets further edited by hand.  working with form mode isn't anything like working with any other elements in fusion and requires a whole different approach to pull off.

the thicken's in surface and solid space are the same.  if you edges are still near tangent I would still expect failures.

[laughingcreek]

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@Anonymous wrote:

...  I cannot see a way of doing that when you stitch surfaces together.

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we posted at the same time.

tang-ency is controlled by the way you construct your input curves, and the settings in your loft command, not during stitch.

[Anonymous]

I cannot capture the pop-up menu in a screen shot, but I cannot get what you display there.  My pop up has 'connected' and 'direction' only, this when using loft from the 'surface' menu.  When I create the first three sections using the surface menu, there is still not a tangent join between sections 2 and 3 (see screen shots).

I appreciate the help but I have not advanced my understanding about what is going wrong or how to fix it.  What is the difference between a loft in 'surface' or 'form'?  I can see the surface one is parametric and I like that, but the results are coming out the same (and not working to achieve the thickened shell).

[TrippyLighting]

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@Anonymous wrote:

...I cannot get what you display there.  My pop up has 'connected' and 'direction' only, this when using loft from the 'surface' menu.  

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The reason is that you selected sketch objects as the profiles and rails. Tangency requires another surface. So instead of selecting a sketch object, select the edge of a surface.

[laughingcreek · Accepted solution]

let's back up.

your both working to hard, and not working hard enough.

let's talk about boats for a second.

The boat builder goes out to the yard and makes cross-section frames/ribs, and bends boards across them to make the hull.  it won't be perfectly fair, but it will be close enough that he can get it fair with skill and hand tools.

but

the designer sits down and marks the important design points, like length and width at the widest point, bends a piece of thin flexible wood (use to be called a spline)between the points, and draws curves from that.

THEN he figures out the sizes of the cross section for the builder to use to make frames from.

You have to model from the perspective of the designer, not the builder.  you can't start by laying out a bunch of cross sections off a plan, connect them together with a multi point spline, and expect to get good results.

figure out the important bits.  use those to draw your curves.

ok, enough about boats.

generally speaking, when drawing surfaces you want to make your primary surfaces in a certain order-

1-extrude any thing that makes sense to extrude

2-revolve or sweep anything  that makes sense to revolve or sweep

3-THEN start lofting.

in the attached model, I started with the mid part of the helicopter, because it is a straight section (should have extruded it, I sweeped it here, same difference in this case. )  then used that to build out the nose and canopy.

feel free to step thru it, look at the settings of each feature, and ask questions.

[Anonymous]

Thanks very much for taking the time to do this - there is a lot there for me to pore over and absorb, and I appreciate the lesson using the model that I am trying to build.  How long did it take you to do this?

[laughingcreek]

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@Anonymous wrote:

....  How long did it take you to do this?

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15 -20 min? there about . still rough, and as always there a things I might do differently in hind sight.  I could worry over a model like this for hours (days) if the project called for it.  But I figured this was enough to give you something to chew on.

[TrippyLighting]

So there is something that @laughingcreek has done on that model which is indeed very elegant and not self-evident for folks who just start in surfacing.

Many, users would loft from a profile into a point, which you can do in FUiosn 360 but is rarely a good idea, for example in this case the red curve and the red point (circle) would be the profiles, and the green curves would be the rails:

However, that causes you to loft into a singularity.  The shape of a NURBS surface is controlled by a quadrilateral mesh of control points and their weights. When you loft into a point the control points of that mesh collapse into one point. This causes mathematical problems and the software has to work with approximations casuen curvature problems.

However, by creating these small patches hat problem is completely avoided.

 

[Anonymous]

It has taken me several hours to reproduce (and slightly embellish) this, but the result look great.  Thanks very much @laughingcreek for the help.  A very different approach and yes, as @TrippyLighting says, an elegant solution to lofting to a point (which was something that I was struggling with).  I think that I have a workflow now too, which I shall use for the remainder of the fuselage.  Thanks again!

Randal