Shell operation failing

[asdFletcher]

Windows 7 64bit / NX7.5

Currently I've got a solid model that has been successfully sewn together from faces. My goal is to simply shell this feature. Unfortunately I can't post any images -- but imagine an eight of a basketball and you're basically there. The inside will get bored out and it doesn't have to be pretty or adhere closely to the outside surface. All I need is an approximation. Ideally it would be associative.

To get my solid the order of operations were:
imported faces (STEP) --> repair,sew,repeat --> export parasolid --> import parasolid --> attempt shell

Things I've tried so far:
Shell (both: Remove all Faces, Then Shell & Shell all Faces)
Errors: "Preview could not be computed." / "Cannot apply Shell."

Offset Face
Errors: "Cannot offset face. The offset distance might be greater than the curvature of the face or the offset face might intersect itself."

Offset Surface
(with varied parameters)
Errors: "Cannot offset face. The offset distance might be greater than the curvature of the face or the offset face might intersect itself."

The best option so far has been:
Extract body --> scale to 95% --> translate --> boolean subtract
But this is not associative, and requires a manual translate to get my scaled shape to the "center" since scale is based off the origin of my coordinate system. Is there any way to control the point about which Scale is centered? Without this my translate is manual and results in varied wall thickness.

I believe the problem arises from small surfaces and regions of high curvature (which do not need to be preserved on the inner contour). I've played around with the options/tolerances on the above settings and have not been able to pull together anything that wouldn't require less work than the original sew, which was considerable.

Does anyone have any ideas?

Thank you for reading

 

[jnikolauk]

you could try offsetting the edge curves the approimate thickness you want and create a through cureves (or a N sided surface if you only have 3 sides if I'm reading you correctly)

 

[cowski]

Before you export a parasolid, you should run Analysis -> Examine Geometry (turn on all the body and face checks) to make sure you have a valid solid. If you start with a bad model, there may not be any tricks that work for you.

www.nxjournaling.com

 

[asdFletcher]

jnikolauk:
Thank you, this is a good idea. I'll work this angle and see if I can get a solution.

cowski:
Thanks for the reply. I did indeed do Examine Geometry on the original faces and until everything passed it would only create a sheet body. Is it possible that the solid body created is somehow afflicted by small imperfections that flew beneath the tolerances on Examine Geometry?

I've seen Mr. Baker mention that sew tolerances can affect downstream actions. Could I be experiencing this? Or is it a deeper issue with offsetting small surfaces with high curvature?

 

[cowski]

If you changed the sew tolerance during the operation just to get the sheets to sew; then yes, the tolerances could be the problem. If examine geometry didn't report errors and you didn't open up the sew tolerance, then the "offset face" error message is probably the true cause. You say the small faces and high curvature don't need to be preserved on the inside faces: since this is the case, you might try
[ol 1]
[li]create a copy of the body you have (extract body at timestamp)[/li]
[li]model away the small faces and high curvature[/li]
[li]offset this new body the desired distance[/li]
[li]subtract the new body from the original[/li]
[/ol]

www.nxjournaling.com

 

[RyanVLee]

i have run into similar problems if you didn't change your sew tolerances then offset the surfaces wear small blends come into play basically you need to rebuild the inside of the model then simple subtract

Ryan Lee
Design Engineer

If you can think it it can be modeled

 

[asdFletcher]

Thank you cowski. I ended up doing something similar and it worked.

My process was as follows:
1. Extract replica solid-body
2. Replace & approximate the entire thing with through curve meshes
3. Sew the through curve meshes from step 2 into a solid (default tolerances)
4. Shell the resulting solid
5. Extract the faces from the inside of the shell
6. Sew the extracted faces (from step 5) together to make a solid
7. Subtract this solid from my original geometry

 

[capnhook]

In conclusion, the shell operation FAILED, eh?

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]