Loft operation won't allow me to shell a part

[retzcay7N6SV]

All solutions I've been able to find online refer to checking that all geometry is constrained and that often being what causes issues when trying to use the shell operation after a loft. However, all the geometry in my case is constrained and all other features aren't interfering with the shell (I know this because the moment I suppress or delete the loft the shell works perfectly).

[chris]

I've mentioned this on a few other posts, if you run into something that Inventor can't handle and you don't need the part to have a feature tree or be parametric, then you can build it in "Plasticity". it should have no problem shelling that out. can you post up .stp or .iges version on your part?

[cadman777]

I rarely use Shell b/c it causes too many problems down-stream.

But if you must use it, as in your application, the main causes that I've found for Shell failures is that the resultant surface offset has joints that are impossible to build. One cause of that is too small inside radii (less than the Shell thickness) between surfaces or corners that will collide into other features. Another problem is disappearance of a feature due to too thin a bridge with another feature. This is the kind of thing to look for.

In order to make your shell work, it must be able to offset your surface so that the shell thickness won't cause modeling impossibilities towards the side of the shell that's being created.

Like Chris said, post a STEP or other kind of surface file for us to look at and make suggestions.

If your model is based on calculations (like fluid-flow) then some modifications to it might change the results of your computations and void your project. Just something to think about.

[chris]

@retzcay7N6SV @cadman777  Something that I've found that works as an alternative to "shell" is to Loft out what you don't want. create your outside loft and once that is done, project the profiles from the original sketches, offset to the "shell" thickness and then do a negative loft to create the shell, it's the same principle behind how I lofted my iLogic "non-curve" reducer template(two extrusions, two lofts), one loft to create the "reducer", the second loft to create the "shell", this was in order to avoid a revolve which would make the template unable to work.

[cadman777]

@chris, your method works similar to another method I've used. They are ways we 'trick' the software into doing what we want. The method I'm referring to is constructing the difficult piece of the part first as already shelled, and then adding the other parts as solids and using other features to 'hole it out'. No use of Shell with that method.

[chris]

https://www.youtube.com/watch?v=j2IBH0Y8b68

[kacper.suchomski · Accepted solution]

Hi

The thickness of the shell is too large to keep the offset geometry of all faces.
Check the shell at 0.05 in - it works.

If you need a thicker shell, you can work around this manually.
Create a thin shell, then try to thicken successive surfaces (or groups of surfaces) one at a time. Combined with the Delete face tool at intersections of surfaces too small to offset, you should be able to get the desired effect.

[retzcay7N6SV]

Never used plasticity before so I'll have to look into that. As far as the step file, I attached the file

[retzcay7N6SV]

Makes sense although I don't quite understand where there would be a radius that would cause issues would be inside that loft feature. I attached the STEP file if that helps.

[cadman777]

Thanks.

What shell thickness?

[retzcay7N6SV]

0.1 inches

[cadman777]

Thanks.

Right off I can see that the thin edge along the side is .151" wide.

So if you offset the adjacent surfaces, you subtract .1*2 from .151 = -.049.

That means Inventor is trying to offset the 2 adjacent surfaces .049" into each other.

That's a collision, so the Shell won't work if you shell to the inside.
But if you shell to the outside, it'll probably work.

You have to plan ahead as much as possible when you use Shell.

See the below screen_cap from Rhino3D showing which edge is too narrow to allow the shell.

If you make a Parameter for your shell thickness and then use that parameter to make sure that strip is slightly wider than twice the thickness, it'll probably shell. That's t*2+.01 or something like that.

[retzcay7N6SV]

So, I did get it working before but now I've made more changes to the part and even in plasticity it's not shelling (or in this case, hollowing) the part. Although it could be ignorance on my behalf since I've not used plasticity before, it doesn't seem to want to do the operation either even after watching a video on how to hollow something in plasticity. I attached the updated .stp file, any suggestions you may have would be incredibly helpful.

[cadman777]

I deleted the 2 capped ends and then offset 0.1 to the inside, and this is the result in Rhino3D:

It failed on that sharp edge at the transition.

Do you have a spec that you need to follow based on fluid dynamics?
Or are you just developing this for a hobby project so it fits into a pre-existing area?

IOW, do you have pre-determined geometric parameters that you must follow for this?

[retzcay7N6SV]

The tight radius there is kind of necessary for it to fit in what little space it has, but it’s helpful to know that is one of the problem areas along with the sharp transition. However, what I struggle with is that if I suppress that sharp transition in the nozzle and make that curve you mentioned larger, it still refuses to shell for me in autodesk

[cadman777]

I took a quick look at rev 5 of your STEP file and found a number of things that will kill your shell.

If I have time tomorrow I'll look closer at it and make some changes to show you how I would make it so it stands a chance of shelling or thickening. I found that it's nearly always easier to shell or thicken outwards instead of inwards in most cases.

My first suggestion and your best bet is to shell it outward, which means you have to design the inside surface instead of the outside surface. 

[retzcay7N6SV]

Thank you for being willing to take the time to look into it, I’ve spent more hours than I’m willing to admit stumped on this thing. I have tried shelling outward as well as inward and just about any other thing I can think of with no luck. The furthest I’ve gotten is being able to shell inwards at 0.00001in of thickness while suppressing the loft from the half-circle to the rest of the shape

[johnsonshiue]

Hi! Another approach in Inventor to get this kind of geometry shelled is to convert the faces to Freeform. Then replace the existing face with the Freeform body surface. Sometimes it could help smoothen the kinks.

Many thanks!

[cadman777]

Find attached a surface model that I scrubbed in Rhino3d.

It's not finished yet, b/c I need further input on what I can and can't do to fix the problem areas.

You can try to shell it in Inventor, but it won't shell in my version (2010).

The problem with Inventor is it doesn't have the tools that Rhino has that you need for checking the edges, surfaces and all that stuff, so you're basically 'shooting in the dark' when trying to fix surfaces in Inventor. But try to shell it anyway and see what happens. Rhino's ShowNakedEdges goes a long way to showing where the problems are.

[cadman777]

Here it is 'shelled' in Rhino (OffsetSurface).

It should come into Inventor as a solid.

If not, then copy it to Construction environment and fix the few things that need attention.

In order to get it to this point, I deleted my new transition surfaces (from main body to skewed nozzle) and re-used your original surfaces. After a bit of scrubbing there were about a dozen junk surfaces that needed to be deleted and re-worked, and that did it. I also tried MatchSurface on the mitered edge connection but it caused too many problems with the transition to be of any use. I just didn't want to spend more time on it at this point.

In sum, I think:

1. you did an good job of constructing your design intent in your model.

2. Inventor did a good enough job to get a prototype created.

3. Rhino was needed to do the surface analysis and repair.

Let me know what you think...