displacements in sol103 (normal modes analysis) 3

[pedrodmar]

Hello everybody,

I have performed a normal modes analysis to my model and I have obtained the first eigenfrecuency at 200Hz, but when I look at the deformation it is very high (20mm).
Does anybody knows if it is normal??? because I have seen other analyses and displacements are lower.

I don´t know if it is important, I´ve used Tonn and mm.

Thanks in advance,

Pedro J. Rodríguez

 

[pedrodmar]

Sorry, I didn´t mention it. I´m using Patran preprocessor.

 

[johnhors]

In a normal modes analysis the value of displacement magnitude is meaningless unless you have requested mass normalised values to be used in a forced vibration analysis. Taken on its own the mode shape is dimensionless, it is the relative displacement of one part of the structure with respect to another part of the structure that has value in describing the mode shape.

http://www.Roshaz.com

 

[ThomasH]

Hi

Since you mentioned units Tonn and mm.

Make sure you have consistent units. Tonn and mm's can be part of a consistent system but since you ask if it's important. It's very important.

And like johnhors says, 20 mm deformation is meaningless. It can be the result of a mass normalised result but 20 mm as deformation is meaningless.

But units are very important. Mass, length and stiffness modules, all must be based on the same base units.

Good Luck

Thomas

 

[pedrodmar]

Thank you very much to both of you,

I knew that results from modal were only to get frecuencies and mode shapes but I didn´t know why, now I know. I think that my units are consistent, because I used mm, tonns, MPa, N.

Pedro.

 

[BlasMolero]

Dear Pedro,
Just as add-on as told by others correctly to you: in a SEMODES (SOL 103) analysis displacement results are meaningless. And regarding units, the system used is correct: density in Tons/mm3, and length in mm. Simply use the trick: value of mass density in kg/m3 x 1e-12. For instance, mass density of steel = 7850e-12 = 7.85 e-9 T/mm3. Revise your numbers.

Regarding the value of 1st eigenvalue, f1=200 Hz means that your model is very, very, very stiff. The only word I can tell you is to check your boundary conditions.

Best regards,
Blas.

 

[pedrodmar]

Thank you Blas.

I know that the first eigenvalue of 200Hz means a high stiffness, but I need it because ESA asks for a first mode >140 Hz. Anyway I will check the boundary conditions because I have suposed the fixation points as embeeded (0 dof in the central node of the MPC).

Thanks again,
Pedro.