Beginner's question about shell

[kdrector]

I have questions about the shell command.   Is shell supposed to work with a non trivial model composed of several features?

The link below will get you to my design.

https://a360.co/2BttjDI

This design is composed of a series of revolves, extrusion, and a loft. 

You can see in the screencast, I selected the body from the menus and set the thickness.  I also tried selecting a face on the body, instead of from the menu.

My attempts at shell result in the error message, " The operation could not create a valid result.  Try adjusting the values or changing the inputs.".

This is not a useful error message at all.  I tried adjusting the thickness value from very small to very large, to no avail.  I can't see how to change the input and still have my model.

 Is shell supposed to work with non trivial models composed of several features?

System Mac OSX 10.13.6 

Fusion 360  2.0.5103

[I_Forge_KC · Accepted solution]

There are two problem areas that need to be addressed before the shell will work - and even then it is tenuous because of some of your feature sizes.

1.

The first issue is likely an oversight on the extrusion to make that boss.

The second issue is a result of very poor sketching on the side view sketch. It's obvious this likely came from a 2D print that was dropped in. If you're going to work with questionable geometry like that, I tend to put them as a master sketch, fix everything, make it construction geometry, and then add individual sketches with projections for the relevant features. This makes tracking down individual failures much easier.

[I_Forge_KC · Accepted solution]

You can actually edit the revolve to grab that minute sketch profile as well.

[kdrector]

I appreciate your help and I hate to bother you about something I might eventually work out, but could you clarify this a little more.

What do you consider questionable geometry?  If you could set me straight it will really help me in the long run.

And which is the minute sketch profile? Could it be the missing chunk in the extrude feature? Probably not because thats an extrude and you said edit the revolve?

[I_Forge_KC]

Both errors I highlighted are caused by not selecting all the relevant geometry to fully form the feature. There is a small teardrop in the extrusion and a small triangle in the revolution that were not added to the feature during creation.

When you look at both of your sketches, there is a ton of info there and none of it is constrained. This means you can pick any line or point and drag it around at will. Invariably, this will change shape through no direct fault of your own. You need to do something to tie everything down.

You'll also see around the forums that the sketching egine of Fusion (and any solid modeler, really) is the weakest link. With this in mind, it is best to work from simple sketches when possible and to always ALWAYS fully constrain the geometry. For example, the revolve with the issue is of a really funky profile that builds in unnecessary complications into the solver. 

Since this is an imported bunch of lines, I would use the FIX constraint (the padlock) to lock everything in place, then use new sketches to create the various shapes for revolving and extruding. Back to that problematic revolve, I would make a new sketch, project a few important points, and then draw a basic rectangle to achieve that shape. No extra data, no small areas, no opportunities for missed profiles.