Modeling Sandwich Composite using the "skin

[plafortune]

Hi, 

I am trying to model a composite Sandwich panel and compare it with NAFEMS results. 

The sandwich is made out of:

- two skins (shell elements, 2D orthotropic material)

- core (solid elements, 3D orthotropic material)

+ + +

My first modelization approach consists of using the SAME surface for the solid and shell elements. In other words, to create the Idealization of shell surfaces, I directly use the faces of the solid 

Some other software (...abaqus) call this approach "skins". I tough that would be enough, but the results are not good (see table at the end). My hypothesis it that the rotational dof of the shell are not being transferred to the solid. Do you think that makes sense?  

+ + +

My second modelization approach consist of using different surfaces for the skins, and use a bounded contact to "glue" them  to the solid core. Results are better....

Any comments? someone already tried the "skin" element approach? 

Results summary: 

Thanks 

Pierre 

Version: Inventor 2021, Built 138

[viktor_velichko]

Hi, Pierre! Try to use offset bonded contact. Its must to get connect rotate DOF of shell and solid. 

https://forums.autodesk.com/t5/inventor-nastran-forum/bonded-contact-or-offset-bonded-contact/td-p/7...

Why "skin" got worse results I don't know. Can you discribe your task and send your model? I'll try to repead.

[plafortune]

Hi Viktor, 

Thanks for your feedback. 

Actually, in the APPROACH 2 described, I already used the offset bounded contact. 

My question was more about the possibility of directly using the face of a solid to create the skin idealization in a sandwich panel. Indeed, I probably demonstrated that it is not possible to use the face of the solid. It is necessary to "manually" create an offset surface for the skin idealization. 

I was just surprised by this and looked for a confirmation.  

Thanks! 

Pierre

[John_Holtz]

Hi Pierre,

It should not be related to the rotational degree of freedom between the shell and solid in the skin model. It should be related to the area moment of inertia of the shells. What is the moment of inertia of the real shells compared to the moment of inertia of the theoretical "skin" shells versus the moment of inertia of the shells with the gap? That difference would explain some of the differences in the results. (With out doing some calculations, I do not know if that can explain all of the differences.)

For example, if the core is 10 mm thick and the skin is 1 mm thick, the real thickness is 12 mm, the "skin" model thickness is 11 mm, and the "gap" thickness is 12 mm.

For the "skin" model, you can offset the shells by the proper distance to account for the shell thickness. Edit the Idealization, then Advanced Options > Midplane Offset Distance.

[plafortune]

Hi John, 

Yes, interesting comment.

The inertia will not be the same, but I don't expect this effect to be too important (I may be wrong). As you can see on the image, the total thickness of the sandwich is big in comparison to the gap between core and skins. 

But I can explore this (I can "shift" the mean-plane of the shell on the 2nd model to have the same inertia...) 

I am curious: what make you think that "it should not be related to the rotational degree of freedom between the shell and solid in the skin model" ? 

Thanks 

Pierre 

[viktor_velichko]

Pierre, can you send NAFEMS verification test, what you used?

[plafortune]

Hi Viktor, 

It's from this book: https://www.nafems.org/publications/resource_center/r0031/

I only have a hard copy of it. It's protected by copyrights, I don't think it's legal to share it here...

On the other hand, I attached my two models: 

- The one where the skins sharing the faces of the solid core 

- The one with offset separated surfaces for the skins 

Pierre

Pierre 

[plafortune]

@John_Holtz : I tried adding an offset to have to same skin-to-panel-mid-plane distance, ans that doesn't affect the results much. 

Still have a difference between the two modeling approach. When the solid's surfaces are directly used, the panel is softer.

I still wonder what could cause the difference, and if the rotational DOF are transferred or not (...and if that maked any differences in that case). What do you think? 

Pierre  

[viktor_velichko]

Hi, Pierre! I haven’t opened your file yet, because I have Nastran 2020. But it seems I found this nafems test in the ansys documentation. I got a thought. Have you imposed boundary conditions on shells besides than a solid? I mean all DOF, include rotates.

[John_Holtz · Accepted solution]

Hi @plafortune 

I agree that there is something wrong with the "skin" model (where you use the surface of the solid to define the shell elements). I am not sure what the issue is. The two approaches should give the "same" result. It will take some more digging to determine what is causing the difference.

One thought that comes to mind is to try regular, orthotropic shell elements instead of the composites. Since there is only one ply, the analysis should be the same. But this would show if there is something different about the composites that I am not aware of.

Regarding the degree of freedom (DOF) between the shell and solid. If the connection was along a line, then the rotational DOF would be important to transmit a moment into the shell. Since the connection is over an area, the rotational DOF is not important. The shell is still bending. The force between the nodes of the solid and the nodes of the shell are "identical" to the case of analyzing a single shell with a force applied. The load on the single shell is a force at each node; there is no moment in the load. The moment occurs internal to the shell because the deflected shape causes bending. The load and effect are the same in a shell only model as in the skin model.

[plafortune]

@viktor_velichko : thanks for the suggestion. I reviewed that, and the bc are ok 

@John_Holtz :

- Difference of 6% on the displacements between laminate and conventional shells.

- We agree that in this case the rotational DOF are explicitly transferred. 

Changing things here and there (finer mesh, etc), I have a difference of 15% on the displacements between the two models. Well...it's a significant difference, but I didn't expect much better.

Thanks for the help! 

PL