Thick shell for FEA modes analysis 2

[jungi]

Hallo everbody,

i'm looking for someone, who has experience in using thick shell elements in FEA normal modes extraction. I've just compared volume to thin shell and it's a dissaster .

Especially using quadrilateral shell elements (!) i obtain different results computing the same mesh using Lanczos solvers from different commercial packages (ideas, Ansys) I get discrepancies up to 40Hz!. I wonder if thick shell formulation would be a better substitute for volume modelling (computational time) than thin shell meshes?

thanks in advance for any suggesrtions!

greetings

Artur

 

[pja]

So are you using a thick shell element and these results are a disaster? Or are you trying to model a thick shell using thin shell elements? If it is the latter than of course your results won't match with theory/full 3d elasticity results. Shear deformation becomes important. I can't decipher your message to tell which one it is....

 

[jungi]

Hallo pja,

Sorry I'm not a native speaker. Let's say I have a cast aluminum part, relatively thick. I'm going to perform a normal modes calculation using fea. I don't know how to prepare the model. I have two options: volume with tetraeder elements and more computation time effective shell model with thin shell elements.
I compared the results of normal mode extraction from the volume model and from the equivalent THIN shell mesh model.
I expected to obtain similar results, but the discrepancies are up to 40Hz between corresponding normal modes from those two analysis.

The thickness could have influence on the shear stiffness, that's why I considered using thick shell formulation. The problem is there is a certain programming effort for me if I decide to use thick shell formulation, that's why I’m looking for someone who could give me some advice for what kind of structure is the thick shell formulation appropriate

artur

 

[Spirit]

jungi,


are you using linear (4 nodes) or quadratic (10 nodes) tetrahedra? This alone does make a big difference in the results, the linear tetrahedra being overly (and artificially) stiffer than quadratic.

Cheers

DS



'Ability is 10% inspiration and 90% perspiration.'

 

[GregLocock]

How big a percentage error is 40 Hz? Does your static stiffness analysis agree? Do your weights agree?



Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[jungi]

Hi,

I’ve checked the mass, all my FEA models "weight" the same - the mass of the models also fits the mass of the real part.

The percentage of the difference in Eigen frequency is not an issue in my case, since the objective of my work is to exactly predict them. I mean, it won’t help me if the percentage difference is 1% when the absolute difference is 5 Hz.

I've already made some more comparisons:

Case1. Volume - shell

I’ve modeled my part as a second order tetraeder volume and second order quadrilateral shell model; of course I’ve corrected the mass, so the both of them weight the same. Max. Difference ~ 40Hz.


Case 2. Shell - shell

I took the shell model from the case1 and solved it using Lanczos solvers from two commercial packages ideas and ansys. I have the possibility to start both analyses from my preprocessor, so I’m sure, that the models are in both cases the same. I’ve modeled the part as a second order quadrilateral shell mesh. Max. Difference ~40 Hz!!!

Case 3. Shell - shell

I’ve modeled the part from case 1 and 2 using second order triangular elements. Now the comparison between the normal mode extraction results from ideas and ansys differ no more than 1 Hz except for two switched modes where the discrepancies are up to 5 Hz.

I’ve also made the calculations directly in ansys and ideas, so I can be sure that my preprocessor delivers them the proper data. The preprocessor is ok! No data gets lost during export!

My OLD experience is:
1. Quadrilateral second order mesh is "better" then triangular second order mesh, although stiffer.
2. Lanczos solvers have the same algorithm in all the commercial fea packages no matter what kind of elements you use as long as you use identical models for comparison.

Both cases won't work!!!

Have anyone ever done similar comparison?

greetings and thanks for support!!

 

[GregLocock]

Try comparing static stiffness, under self weight, or an applied load, for the different element types, and if you like, the different solvers.

Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[pja]

Number 1 make sure that both your solid and shell models are mesh converged. Specifically make sure you have enough elements through the thickness for the solid model. Second, as I stated before, using a thin shell element for models which are thick(ie perhaps when the L/t ratio is less than 10-20) will not give good results. Many FEM books have results which give comparisons thin and thick shell formulations.

 

[jungi]

hi,


pja, the meshes had converged and i have 4 second order tetra over the thickness. Do you have any particular book in mind?

thx

artur

 

[pja]

Ok if you are sure that both of your solutions are converged with respect to the discretization then your results are telling you that a thin shell element isn't going to work. What are the dimensions of the body you are looking at?

Chapter 8 of J.N. Reddy's Energy Principles and Variational Methods in Applied Mechanics, 2nd Edition has some comparisions of classical and shear deformation theory solutions.

 

[jungi]

hallo pja,

thx for the tip on that book, I’ve already ordered it.

Dimensions? I've encountered these problems by almost all my parts, but here are two examples:

1. Aluminum cast, semicircular plate with concentric ridges

Plate:
Radius of 1800mm
Thickness 90mm

Ridges:
Height 100mm
Thickness 50mm

2. Rolled steel, semi cylinder shell
Radius of 1800mm
Height 2000mm
Thickness 15mm

Both deliver strange results, if computed for normal modes using different packages. And I know that thin shell formulation is not really properly, especially for the aluminum cast part, but for now I have no clue how to deal with thick shell formulation. Another problem I have to clear is why ansys, ideas and now abaqus and our homemade software deliver so different results (i've made some extra tests for a simple rolled steel plate 1700x900x16 mm).

Greetings,

artur

 

[pja]

I am not familiar with ideas or abaqus. I do however use ANSYS. So your thin shell results from the four different codes differ signficantly? Is that what you are saying? You have to make sure you are comparing apples to apples..are the formulations the same for the elements you are comparing?

 

[jungi]

yes, the mesh is the same for all of the cases, i start all the simulations from one program alwys using the same model!

 

[pja]

Not the mesh the element formulations..ie in ANSYS if you are you using SHELL63 elements then they are DKT type elements? Are the thin shell elements which you are using in the other codes also DKT elements?

 

[jungi]

yes, the shell element are SHELL63. What does DKT mean?

 

[mgk12345]

HI JUNGI
ARE U TRYING TO REPLACE THE SOLID PLATE LIKE STRUCTURE WITH SHELL ELEMENT TO GET THE EQUIVALENT MODEL.

MILIND

 

[jungi]

hi milind,

yes, thats my goal volume models are precise but require mor computational time - problem is that volume and shell model results doesnt' fit...

 

[mgk12345]

hi
i am working on the same problem. i do also have the same problem but i got the results for natural frequency of the shell model and solid model between 10%. that is fine enough and i am going to optimize the shell thickness to reduce the % error to get between 1-2 %.
i have one problem in that. when we take the solid perpendicular plates and fixed that on one horizontal area and apply unit load on the vertical plate at the middle node in x,y,z direction we get the stiffness Kx,KY<KZ in that direction.
but when we do that with the shell model of the same thickness and applying same load on the same node point, the % error in KX,KY,KZ is more than 20%.
i have used the shell element 63 and solid 185.
i am trying to use solid shell element instead of shell but meshing is not possible in ansys.
if u do have the suggestions for my problem and if i can help u in any matter i will be happy.
please give me ur valuable suggestions regrading the same as u are working from long time.
bye.
milind

 

[jungi]

Hi milind,

For now, I have no clue how to generally overcome the differences between solid and shell. I've only figured out that solid fits the measurement much better, so I use "model updating" and so correct the shell element’s stiff nesses... and so the results obtained from shell model better fit those from solid modeling... for the shells, I still have problems in obtaining same results for a mesh calculated with different packages (ideas, ansys, abaqus) that’s irrational to me... I believed that a mesh should deliver same results no matter what software I use and as I said before I got differences up to 40Hz!!! my last tests show that a fine triangular second order shell mesh delivers "best" results calculated on different solvers, but it still happens that I get 2 or 3 switched modes in frequency band 0-500Hz. so the only thing I can suggest is: get yourself a model updating software (I use femtools) and work with two models solid and shell, just fit the shell to the solid... I hope I’ll help…

Best regards

 

[pja]

As I said before, if the shell element formulations are different for the different codes you can expect that the results won't match up perfectly. This shouldn't be surprising...you have check the theoretical background for each of the shell elements which you are using in the codes.