Dear Yuanning Mao

As you know, only [K] and [M] matrices are effective in calculating eigenvalues. You probably did not export the mentioned matrices correctly and these matrices are different in ANSYS and MATLAB which cause different eigenvalues.

So either there is a problem with how to export [K] and [M] matrices or you used the initial [K] matrix in Matlab, while the used [K] matrix in ANSYS which led to given natural frequencies, has some changes compared to the initial [K] matrix. These changes can be for various reasons, including structural analysis, loading, element type, cross section (fiber, elastic, etc.), mesh type and other factors affecting the stiffness of the structure.

Dear Majid Tavakolinia ,

Thanks for your comments and I strongly believe your points make sense. As I was moving forward, I found out that using the Harwell-Boeing (HB) method to export the structural matrix [M] and [K] in ANSYS instead will provide consistent natural frequencies in MATLAB.

There is another question I don't understand is that it seems like the total mass calculated from the exported [M] matrix does not equal the total mass that ANSYS calculated. At this point, I have the unit checked so that the deviation is not caused by unit difference. Indeed, if I simply multiply the corresponding ratio between these two quantities in both [M] and [K] matrix in MATLAB, I still get the same natural frequencies as it supposes to be.

I am happy if anyone who has similar experience can explain this deviation.

Can you share a *.cdb file of your finite element model?

I am not an ANSYS user... but numerical precision can be an issue when exporting Matrices...e.g. in ASCII text format instead of binary format. Quite well known issue for Nastran users. Regards.

Hi Nils Wagner ,

Yes, for sure.

Please find the attachment for the required file. I have already exported a sample [K] and [M] matrix (which only the lower half has been stored as they are symmetric) in the "dp0\SYS\MECH" file in case you need it.

Please beware that I have made some modification on the model so that the corresponding natural frequencies are deviate with the previous presented natural frequencies.

The updated natural frequencies are 537.2, 537.2, 729.6, 1283, 1419.5Hz.

As the results from ANSYS and matlab are not quite discrepant, I guess the errors might be caused by the numerical errors of the computer. I guess the exported matrices are not completely symmetric due to the numerical errors in the computer. You can use (M+M')/2 and (K+K')/2 to replace M and K to ensure their symmetry in matlab.

Hi Wei Tian ,

Thanks for the quick response. I am sorry that I forgot to mention the model I uploaded was slightly modified so that it has slightly different natural frequencies compared with the one I presented in the main question.

The exported matrices are symmetric and both MATLAB and ANSYS provide consistent natural frequency results. It is just the ratio issue I mentioned in Aug 6th remains unsolved.

Anyway, thanks for the point of averaging the matrix, which I do believe is quite helpful in many other applications.

Hi Yuanning,

The *.cdb file is missing in your zip archive. You might use the Ansys command

CDWRITE, ALL

to create that format.

https://www.simutechgroup.com/tips-and-tricks/fea-articles/221-fea-tips-tricks-post-processing-apdl-ansys-workbench

Best regards,

Nils

Hi Nils Wagner ,

I find the link you provided is very helpful and I appreciate it. Please find the *cdb file in the attachment.

Regards.

Hi Yuanning

Based on your sharing files, I got the same results. The first 14 natural frequencies are computed by the exported matrices from ANSYS Mechanical ADPL 17.0. The results are provided in the attachment and the Matlab commands are list as follow

clc,clear

K=hb_to_msm('K');

K=K+K'-diag(diag(K'));

M=hb_to_msm('M');

M=M+M'-diag(diag(M'));

[V,D]=eigs(K,M,14,'SM');

D=sqrt(D)/2/pi;

Hi Yuanning,

I have converted your cdb file to PERMAS dat format.

Almost the same results with PERMAS.

[ 537.34379837 537.34379944 729.70692706 1283.17426412 1419.70827845

1419.70828741 1750.2395307 2073.01769613 2158.711457 2206.47148057

2211.16967721 2211.16968791 2339.62906657 2450.96005171]

You can check that your FE results calculated based on integration points however, your matlab calculation is based on nodal stiffness matrix. I think your FE result is an average number between different nodes in a same plane. Thefore, this slightly difference is reasonable.

I do a lot of natural frequency calculations with a lot of different programs as we try and match known data.

Even what seems minor changes in the matrices can lead to changes in the natural frequency, changing a solver version such as PARDISO can lead to changes, you will be extremely unlikely to match unless you are prepared to work really hard and the results are till somewhat meaningless unless you have measured data.

A FEM mesh is never going to match reality, it is just not fine enough. Have alook a Harrisons book from 1973 on structural analysis to see the possible subsequent steps.