Shell function doesn´t work with complex objects

[Jan-RickmerLuth]

Through a process of creating 3D-Splines and lofting between them I created a rather complex shape of a hull of a ship.

But as I stitched everything together to a body, I can´t seem to get any kind of body manipulation tool to work for me.

The shape needs to be hollowed out to a wall thickness of about 2mm and the shell function doesn´t even let me click the body.

Thickening the original combination of t-spline faces doesn´t work either as i can only select individual faces

(The combine function doesn´t let me combine the two mirrored bodys as well)

Link to my Design

http://a360.co/27ylvLa

Thanks in advance

[PhilProcarioJr]

@Jan-RickmerLuth

The first problem I noticed when opening your file is you have warnings that need fixed. (all the steps in the timeline that are in a yellow box)

Next problem I noticed is your model is still a patch model, when you did the stitch you didn't set the tolerance high enough. You have it at 0.01mm set it to 1mm and it will give you a solid. A solid is what you need for the shell command to work. It still will not shell because of the sharp edge on the bottom of the boat so at this stage if you want it shelled you will have to do it manually by modeling the inside and cutting it out. I fixed the not being a solid part in the file below.

[Jan-RickmerLuth]

Thank you very much!!

This seems to fix some of my problems and give me something I can work with. Have you got any suggestions on how the shelling process could be made easier than modelling/approximating everything again? (I dont really care whether it is done in Fusion 360 or it violates any best practices. I just want to avoid returning to modeling the hull)

Thanks again

[PhilProcarioJr]

@Jan-RickmerLuth

If it were me I would do a body split and separate the sharp edge of the boat from the rest, then shell the main body and combine the results afterwards.

I would do this for you to show you how but I'm at work and can't.

[Jan-RickmerLuth]

Would be great if you could get that to work for me. I was actually thinking about doing the same thing you suggested, but splitting the object with a "sharp" construction plane only introduces more sharp edges (for me)

[vex]

If I'm invisioning your design correctly (can't really download right now), you might be able to use the shell command:

From your solid model,

Create a profile that is colinear with CL but extends out passed either port or starboard (but not both).
Extrude that profile to remove either the port or starboard portion of the vessel.
Shell the remaining solid, selecting the centerline face and the top face (or leave the top face if you have shear or camber you wish to retain), adjust thickness as necessary.
Mirror along CL

[jeff_strater]

@Jan-RickmerLuth:  I took a look at your design, and I have some recommendations that may help.

Your method of using Boundary Patch to construct the hull is interesting, but has some potential problems, which I think are the root of your shell problem.  Boundary Patch is really intended more as a repair tool for small gaps than a modeling creation tool.  The main problem with Boundary Patch is that it sometimes generates what we internally call "tolerant edges", due to the math used to build them.  This means that the edge isn't quite 100% lined up with the input geometry, but is "close enough".  This is OK for some things, but the more tolerant edges you have, the more the inaccuracy compounds itself.  And, this will show up problems in later modeling operations, in this case Shell.

This is also why your stitch requires such a huge tolerance.  If you have to stitch with a tolerance of 1mm, that's a bad sign.  Usually, Fusion's modeling tries to model to 1.0e-6 (cm) accuracy.  So, having to stitch to a big tolerance is a sign of future trouble, and I think your shell problems show that this is true.

I would probably try to model this using Loft or maybe even Sculpt/Form Features, as a single solid body.  Or, even using surfaces but using the more-precise Loft, and then stitch it all together.

Sorry not to have a better answer that would leverage all your current effort.

Jeff

[Jan-RickmerLuth]

It seems to me that you are correct. Although I used the loft tool for the main faces of the hull (as you can seed by the large curved faces) The Patch method for some remaining faces was actually never planned and those faces should have been made with the loft tool as well, but even though I was pretty happy with the results of the loft in the "lower part" of the model, the T-Spline faces didn´t seem to snap to the rails I selected, when modeling the upper part. The "fix" using Patches was actually just out of desperation

I just tried splitting the model with a construction plane and tried to shell the part of the body that wasn´t created using patches .... I didn´t work

Again, If anyone has got any kind solution that works, regardless of how bad it is, feel free to suggest

(I honestly thought about exporting as an STL file and performing the shelling function in meshmixer .... And I am not desperate enough ... yet)

EDIT:

The large tolerances seem to show up in the regions created with the loft tool as well. (According to the stitching feature in my timeline)

[Jan-RickmerLuth]

Can anyone suggest a possible solution?

Sadly my hard drive died yesterday, so my ability to try any new solutions is very limited. But I ran out of ideas on what to try anyway...