Comparing Strain Engery from different Modal Analysis 2

[hanspeter]

Hello Dear community,

during a modal analysis (2..Modal/Eigenvalue) the question occured, if it is possible to compare the strain energy values (especially their distribution) on a plate 1 with the strain energy values from a modal analysis of another plate 2 with slightly different geometry.
I had read, that the scaling of these values is somehow arbitrary per mode. So if I understood right, if the scaling per mode and part is arbitrary, you can not compare mode 1 with mode 2 or part 1 with part 2 in terms of eg strain energy. Is that right??

Example A start:
There are two plates with plate elements: Plate A with 2mm, and plate b with 3mm. diameter and mesh is equal.

I want to know if the strain energy of node X Plate A in mode 1 is comparable with the strain energy of node XPlate B Mode 1. (not if it is equal, just if it is comparable).
So can I say in a relative way that the strain energy is eg. 2times higher on X Plate 1 than on X Plate 2.
Is that possible?

Example A end.

Example B start:
There are two plates with plate elements: Plate A with 2mm, and plate b with 3mm. diameter and mesh is equal.

I investigated the drop between highest and lowest strain energy on Plate A. Then I did the same for Plate B.
Now I want to compare these 2 drops and say, if drop B is higher, then I go for Plate 1, because I want to reduce the strain energy per mode.
So I computed the drop ratio between both plates.
Are relative modal value factors comparable?

Example B end.

Maybe someone can help me out with that would be very interesting!!!
Your

Hans Peter

 

[BlasMolero]

Dear Hans,
The element strain energy output in MODAL ANALYSIS (SOL103) is an extremely useful tool in helping you to identify the most efficient locations for structural modifications to improve stiffness in the model in order to meet stringent design criteria. I use it a lot because is an excellent tool for identifying areas of modification that will reap the most benefits for design changes.

In Modal Analysis for me the most interesting value to plot using contours in FEMAP more than strain energy is STRAIN ENERGY PERCENT. In the following picture you have a FE model of an aluminum car frame Shell. According both the plot and listing results element number 627 has the highest element strain energy among all elements. In fact, it contains 1.547% of the total strain energy of the whole structure. In other words, element number 627 is the most effective element to modify if you wish to increase the stiffness of the structure for the same amount of weight increase.

      EIGENVALUE =  2.590527E+04
      CYCLES =  2.561617E+01
                                           [b]E L E M E N T   S T R A I N   E N E R G I E S[/b] 
                ELEMENT-TYPE = QUAD4               * TOTAL ENERGY OF ALL ELEMENTS IN PROBLEM     =   1.295263E+04
                   MODE               1            * TOTAL ENERGY OF ALL ELEMENTS IN SET      -1 =   1.295263E+04
                                    ELEMENT-ID          STRAIN-ENERGY           PERCENT OF TOTAL    STRAIN-ENERGY-DENSITY
                                           [b]627          2.003210E+02                 1.5466              8.082329E+01[/b]

In summary, this is the way I take advanced of Strain Energy results with FEMAP & NX NASTRAN running Modal Analysis.

Back to your problem:
1.- Element strain energy is basically the elastic energy stored in the structural element.
2.- Strain energy is the area underneath of the load vs. displacement curve. But in Modal Analysis we don't have loadings, neither displacements, only play with mass and stiffness, then if you look for "quantitative" values of strain energy better runs a linear static analysis. But you can compare.
3.- Also, if you want to know which model is more stiff, directly use eigenvalue results, because the comparison includes not only stiffness but also mass. Compare 1st mode eigenvalue results, the bigger the stiffer!!.

Hope to be of help!!.
Best regards,
Blas.



~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[hanspeter]

Hi Mr. Hidalgo,

very clear and good answer, thank you!

In your answer you showed the results of one model.
My problem is considering 2 seperate models A and B.
What about a strain energy value on node n = 10 on model A and value n=20 on model B.
Can you compare them directly? So can you say my modifications i made in model B result in 2 times higher strain than in A?

Is that comparable? Or are that arbitrary scaled values which are just valid for one mode and one model? (eg, your example)
Because the theory guide writes, that scaling per mode is arbitrary (because there are no forces as you mentioned right).

Do you have informations, if you can compare the values through different models and modes and if yes, how can you achieve a uniform scaling (which you need for comparison, arbitrary can be anything...).

Thanks again!!!

Best greetings Hans Peter

 

[BlasMolero]

Dear Hans,
Yes, you can compare the maximum elemental strain energy between two models, being "A" the original model, and "B" the modified model. But do not mix "apples with oranges", compare strain results fixing the 1st mode, do not compare mode 1st with 10th.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[hanspeter]

Hi,

just trying to end confusion:

I just got an answer from the Femap distributor and they wrote me that there is no way of comparing two different modells. Like mode 1 from Model A and mode 1 from Model B.
I made also some tests:
If you test and compare different Modes of a 1mm and a 2mm plate and a 3mm plate you wont find any corelation between the strain Energy of each Mode (always comparing the same mode , of course).

But anyway, thank you.
Best regards

HP