Difficulty Shelling a Sold PArt

[Anonymous]

Hi Community,

I am currently working on improving a the outer body of a vehicle that is to compete in the world solar challenge (Australia)

I am currently unable to shell the part in the attachment: The file was drawn in catia but I do not have access to the programme anymore.

The shell is supposed to go inward at 3mm and the

The error message says:    Could not create a new shell
     NACA 7 Concept5 MODIFIED.ipt: Errors occurred during update
       Shell2: Could not build this Shell
        The attempted Shell operation was unable to solve for a vertex. This may have been caused by thin faces in the input or an overly large thickness. Try with a smaller shell thickness or by removing such thin input faces.

The .ipt file has been attached to this message, can someone please help me or has anyone had any experience with this error

Regards

Adelani

[jakefowler]

Hi Adelani,

Many thanks for posting this issue! The shell operation is having trouble because of some modelling inconsistencies on the imported model. At first glance, these appear to be the result of the Catia modelling workflow, although it's possible that some of these could have resulted during the data translation process (if you are able to post/email the original Catia file, we could investigate this possibility). I've logged the shell operation failure with our development team (Defect ID 1461485), to see if we can get the Shell algorithm to overcome these issues for a future release. 

However, given these problems with the input model, I would actually consider rebuilding this model in Inventor (if resources allowed) if you want to perform extensive downstream operations on this model, since these modelling inconsistencies could well introduce further issues beyond the Shell failure.

Assuming that rebuilding the model may not be a possibility, I was able to work-around the Shell failure with the current model by healing-up some of these issues on the input model before shelling: please see the attached IPT (saved from Inventor 2013 RTM - roll the EoP marker down the feature tree to view the model). The two adjustments I made were:

1. I removed two sliver faces (very thin faces, likely to be introduced accidentally) in the feature Delete Face1. By ticking the 'Heal' option, the surrounding faces were reintersected to maintain this model as a Solid body.

2. I replaced the 'dome'-like face at the top of the model (removed with Delete Face2) with a native Inventor Loft surface. The original face does not align smoothly with the surrounding faces, and has two awkward degenerate points that are likely to make life difficult for downstream operations. I used a copy of your original surface as a visual aid when constructing the new Loft, but the resultant surfaces aren't identical, so you may wish to compare the results to make sure that the new shape meets your specifications.

I hope this helps, and let me know if you have any questions on this. Wish you the best of luck with the competition!

Jake

[Anonymous]

Dear Jake,

That looks awesome, I am also going to perform some CFD so I is very useful to get rid of the slivers as they cause meshing errors. MANY THANKS! I am not sure that the importing process caused the error but I have attached the CATIA file just in case. I am very grateful for your help and thank you very much for my time!

Adelani O  

P.S. I have not been able to attach the CATpart file, appologies 

[JDMather]

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@Anonymous wrote:

P.S. I have not been able to attach the CATpart file, appologies 

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Right click on the filename and select Send to Compressed (zipped) Folder.
Attach the resulting *.zip file here.