Create shell from whole solid

[pics.munmun]

I have a solid model created from Different extrusion. I want whole solid to be a shell of thickness 50mm so that I can Analyze water flow in Autodesk CFD. 

Refer to attached model

Other method i followed is to create a shell from bottom pipe and top structure. and then tried to loft it. But at that time loft was not able to generate. so i decided to make a solid model first and then make it shell. Still i was not able to accomplish it.

Which workflow is better in these kind of solids?

1) create top and bottom shells and then loft as per sketches

2) loft top and below sections and then create shell 

Thank you

[Alexander_Chernikov]

Yes, the main problem is in the loft element.

I would suggest to create the top element and the pipe as separate bodies, and create shells from them.

Then create a loft element and a shell over it, removing only the top face (there is an error with bottom one) .

For the bottom - make a hole.

Then combine all three bodies into one volume.

The updated part attached (IV2023).

PS. Check the sweep path - there is no tangent btw line and arc.

[pics.munmun]

@Alexander_Chernikov Thank you so much for your reply.

I request you share screencast demonstrating the method yo have mentioned. 

Thank you in advance

[pics.munmun]

@Alexander_Chernikov 

[cadman777 · Accepted solution]

Usually when the Shell feature fails, it's b/c somewhere in the model there is geometry that is trying to become smaller than is possible due to the ShellThickness offset value. So the software can't shell less than that thickness.

One example would be where 2 surfaces join and the distance between inside edges is less than the thickness value. Another example is an outside radius that's trying to be smaller than 0 when the surface offsets too far.

To solve that, check your inside edge distances or inside radii before shelling. Find where they are less than 50mm (or what a 50mm offset surface would cause a failed feature), and then fix it. To fix it, start at a very thin shell value, and then increase the thickness incrementally until your part fails to shell. Then reduce to the last good thickness value, and look for near collisions of inside edges or radii that want to disappear. When you locate the 'offending' geometry, change it to suit your shell thickness, or adjust your shell thickness to suit. That may solve your problem.

Or, you can do like @Alexander_Chernikov showed you, and Shell the top and bottom parts, but use a Hole to finish the job. The Hole feature is a work-around to the conflicting geometry.

[Alexander_Chernikov]

Hi, you can use Loft with Subtract to delete this element.

The result model and video added

[Alexander_Chernikov · Accepted solution]

The Video added

[johnsonshiue · Accepted solution]

Hi! This is an interesting model. The Shell failure is related to the irregular profile in the Loft. The geometry is just way too complicated to have precise offset faces.

To avoid such geometry, you may want to simplify the Extrusion profile (omitting the small circular cut). I used Surface Modeling technique to do it quickly without having to rework the profile. Essentially, you want to do the small circular cut at last. Shell can work up to 90mm. Please take a look at the attached part.

The quickest way to get to your destination may not be a straight line. Loft is powerful but it can make geometry unnecessarily complicated. It is always a good idea simplifying the geometry whenever possible.

Many thanks!