Offset surface for shel elements

[alessandro_introiniED9PA]

Good morning,

I write here to ask for a support in Nastran. I am making a FEM simulation of a vessel cover. This cover has a 4m diameter disk with a central hole and different welded ribs to reinforce its structure above the disk. In attached I share some screenshots.

I have to assess two simulation cases: over pressure (+0,065barg) and vacumm (-0,065barg). In order to make calculations faster, I would like to convert the main disk in a thin surface and to mesh it with shell elements. In addition, I would be sure to keep the contact between the disk and the ribs, avoiding eventual troubles with the contact type "Offset bonded" and the "Max activation distance". For this reason, I have used the "Offset Surfaces", insert 0 like offset and insert 6mm like thickness.

Then, I am wondering if the software is able to understand which direction the thickness has to be considered to (in this case downwards). Thanks in advance.

Alessandro

[John_Holtz]

Hi @alessandro_introiniED9PA 

A thickness of 6 mm is insignificant to the diameter of 4 m. In my opinion, the results are going to be the same whether the shell is at the true midsurface or the bottom face.

I do not understand what you are doing with the ribs and how you intend to avoid using some type of contact. Once you have that figured out, the answer of what to do with the top plate will become more obvious.

John

[alessandro_introiniED9PA]

Good morning Mr. Holtz,

thank you for your support. I agree with you for what concerns the low impact of 6mm thickness on a 4m disk. For this reason I use shell elements. My idea is to use shell elements for the disk and tetrahedal elemets for the ribs. 

But, as you know, if I create a mesh using the midsurface method, a gap will be generated between ribs and disk mid-plane. Consequently, I have to choose the right contact type and in this case the "OFFSET BONDED" should be the right one. But, how do I calculate the maxumimun activation distance ?

So, in order to avoid this issue and to settle it once and for all, I thought that "offset surface" could have been a good solution.

So, my question is: the software is able to understand the right direction of the disk thickness, if I insert 0 like offset and insert 6mm like thickness?

Thanks.

Alessandro

[John_Holtz]

Hi Alessandro,

For the answer to your question about the maximum activation distance, see tips 16, 18 and 19 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks.

I want to clarify my previous answer:

• If the location of the shells is the midsurface, the answer you get will be X. If the location of the shells is the top or bottom face, the answer will be Y. The difference will be small, such as X/Y = 0.99. That is, just a 1% difference or something insignificant like that. 
• Because you are making the ribs with solid elements and using contact (and all the other factors), I think the results will be accurate to within 10%. In other words, the position of the shell is insignificant compared to the other approximations you are making.

Actually, it looks like you have a single part model. I predict that you cannot create a combination shell and solid element analysis using the current model. You need an assembly to so that the solid mesh is only the pieces that you want to be a solid mesh.

The better way to do the analysis is to follow Tip 3. The plate and ribs should be surfaces created in Inventor. This model would have the surfaces at the proper location (at the midplane of each part), would have no gaps between the surfaces and edges, and can be meshed using "Continuous Meshing" in order to avoid contact between the shells. Only the center ring which is thick would be a  solid part and use contact to connect it to the shell.

John

[alessandro_introiniED9PA]

Thank you very much Mr Holtz. I would like to share my file, so that you can see my CAD file and my simulation settings. May I ask you to give me your mail address? My file is 113MB and I cannot send it to you through the forum.

Alessandro

[John_Holtz]

Hi Alessandro,

The model in the image does not look too complex. If the image shows the entire model, the 113 MB file size is due to the mesh. I suggest you delete the mesh (from all the analyses if you have more than one analysis setup). Then the file should be small enough to attach to the forum.

John

[alessandro_introiniED9PA]

Good morning Mr Holtz, here attached I send you two files:

- "Coperchio AP_v3-1": here I used thesheel elements only for the 4m disk

- "Tentativo Coperchio AP_v4-1": I generated this file following the solid-surface procedures for the disk and the ribs

Which of the two assemblies is correct? Are the two simulations equivalent?

Let me know your comments, please.

Best regards

[John_Holtz]

Hi Alessandro,

The assembly version of the model is missing the three part files that are included in the assembly. (See What files to provide when the model is needed - Autodesk Community for steps to provide all the files needed for an assembly.)

Regarding the two analyses, I assume you have results from both analyses and can compare the results. Are the two results approximately the same? If the results are not the same, you can look at all the results to better understand why the results are different. For example,

• Are the reaction forces the same? If not, a load is not applied properly.
• Is the contact force appearing everywhere it should be? If not, contact may be missing somewhere, or the maximum activation distance is too large or too small to create the correct contact. (See tips through 22 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks.)
• Is the displacement the same? If yes, the stiffness is the same in both models. If no, why is the stiffness different? Is the mesh too large? (Smaller mesh sizes give better estimations of the stiffness.)
• Finally, are the stresses the same at locations away from joints? (In other words, ignore the stress "hot spots" that occur at corners or joints where parts are bonded together. The points with the maximum stress are not accurate if the max stress is isolated to one node.)

John

[alessandro_introiniED9PA]

Hi John, I send you the right files. I cannot add Nastran files, because they are too big. I have checked the results and, although the settings are the same (constraints, loads, materials,...) the displacement are different. In the case with disk and ribs meshed with shell elements ("Tentativo Coperchio AP_v4" file), the displacements are about 1,6 bigger than in the other file.

Unfortunately, I don't know if simulations have reached the convergence, because the plot is  always flat. So, I don't know which results are reliable.

May I ask to tell me if the pre-processing step, so the two models, are correct? 

In "Tentativo Coperchio AP_v4" file I have noticed that Nastran does not give me the contacts automatically. I have been forced to select each face and edge to set contacts. Is it normal?

Thanks.

Regards

[John_Holtz · Accepted solution]

Hi,

Did you check the reaction forces?

• The assembly file where the ribs and main plate are modeled with shell: reaction = 74403
• The part file where the ribs are modeled with solids, main plate with shell: reaction = 45090. The applied pressure is different than in the other model. (Also, the pressure should not be applied to the solid ribs because that load is already included by applying pressure to the entire plate/shell.)

I'm not sure if the mesh convergence does anything when the model includes shell elements. It might refine the mesh in the solid, but it definitely does not refine the shell. You should just use the old-fashion approach of refining the mesh manually if needed. When the load is corrected, the shell model with 20 mm mesh gives the same displacement as the solid model with 10 mm mesh (5.225 mm versus 5.295 mm).

John

[alessandro_introiniED9PA]

Thank you very much John. I have refined both the shell mesh and the solid mesh to your advised values and I deleted the pressure loads on the ribs surfaces. Now the results (displacements and reaction forces) are equivalent between the two models. Thank you again for your support and patience. See you to the next analysis.

Best regards

Alessandro