[SOLVED] Big Error on Modal Analysis

urshelfenstein

Hello,

I faced a big error in a modal analysis. To investigate this issue a very simple model was used based on a test case (v2.08.011).

What I found is that the resulting frequencies are strongly related to the mesh size. This looks very strange to me because according to my understanding the mesh size should not have such a big influence to the result in a modal analysis. By running modal analysis on other FEM software I never experienced such an effect.

The resulting resonance frequency of the first mode should be in both directions 167.62 Hz. Even with a fine mesh size (cf. the attached PDF which summarizes the results) I got a deviation more than 6%.

Here you find the used code:

DEBUT(LANG='en',);

#---------------------------------------------------
# MESH
#---------------------------------------------------

mesh=LIRE_MAILLAGE(	FORMAT='MED',									# read in string						
						UNITE=21,
						INFO=1,);
   

#---------------------------------------------------
# MODEL
#---------------------------------------------------

model1=AFFE_MODELE(MAILLAGE=mesh,										# define the model
                   AFFE=_F(TOUT='OUI',
                           PHENOMENE='MECANIQUE',
                           MODELISATION='3D',),);
								
								

#---------------------------------------------------
# LOAD AND BC
#---------------------------------------------------

BC=AFFE_CHAR_MECA(MODELE=model1,										
                  DDL_IMPO=(_F(GROUP_MA=('fix',),						
                               DX=0.0,
                               DY=0.0,
                               DZ=0.0,),),);
                               
CuBe2A=DEFI_MATERIAU(ELAS=_F(E=210000.0,								
                             NU=0.3,	
                             RHO=7.8e-09,
                             ALPHA=0.01,),);



matfield=AFFE_MATERIAU(MAILLAGE=mesh,
                       AFFE=_F(TOUT='OUI',
                                MATER=CuBe2A,),
	);
                                    
                                    
ASSEMBLAGE(MODELE=model1,
           CHAM_MATER=matfield,
           CHARGE=BC,
           NUME_DDL=CO('NUM'),
           MATR_ASSE=(_F(MATRICE=CO('Stiffn'),
                         OPTION='RIGI_MECA',),
                      _F(MATRICE=CO('Mass'),
                         OPTION='MASS_MECA',),
                      _F(MATRICE=CO('Damping'),
                         OPTION='AMOR_MECA',),),);


#---------------------------------------------------
# MODAL SOLVER 
#---------------------------------------------------

reig0000=CALC_MODES(OPTION='BANDE',
                    SOLVEUR_MODAL=_F(METHODE='SORENSEN',),
                    MATR_RIGI=Stiffn,
                    MATR_MASS=Mass,
                    CALC_FREQ=_F(FREQ=(0.0,30000.0,),),
                    VERI_MODE=_F(STOP_ERREUR='NON',),
                    AMELIORATION='NON',);



IMPR_RESU(FORMAT='MED',
          UNITE=80,
          RESU=_F(RESULTAT=reig0000,),);



FIN();

Any ideas how to make sure that the resulting frequencies will not change with the mesh size? For me it looks like a bug.

Thank you for any support,

Urs

Attached file:
Grid_Refinment_Study.pdf, 64616kb

jeanpierreaubry

hello

this seems pretty normal to me

you need to have enough element along the span to clearly represent the mode shape

in addition with not enough element you will just simply miss high order mode shapes

jean pierre aubry

urshelfenstein

Hello Everybody,

@jeanpierreaubry: Thank you for your fast reply.

For me the deviation is much to high. To prove this I run the same case in the FEM module included to our CAD (Inventor). This is easy to use FEM for quick and dirty solutions.

With just about 10 elements over the beam length I got a resonance frequency of the first mode of 167.8 Hz. This is compared to the expected value (167.6 Hz) a deviation of 0.1%.

With about the same mesh size I got from Code Aster a resonance frequency of the first mode of about 220 Hz which is about a deviation of 30%.

According this comparison the result of CA is 300 times worse! What is wrong?

Reagards,

Urs

jeanpierreaubry

can you show the mode shape of this frequency?

as your model seems quite simple

what are the analytical figures?

boyere

Urs,

May I ask a question ?

Do you know which kind of elements your CAD solver uses ?

Emmanuel

urshelfenstein

Good Morning,

The analytical calculation, the comparison with the result of FORMA11, and the deformed shapes you will find in the attached file.

Because the solver of the CAD uses a tetra mesh I also change from a hex-mesh to a tetra-mesh and the error became as expected bigger. I do not have much information of the CAD solver and the elements there. I found that with 4995 elements it has 8088 nodes. Therefore, I guess it is a linear tet-mesh.

One observation is that the first mode in the CAD and also in the FORMA11 showed a diagonal displacement. The 3D tetra mesh solution in CA shows only a displacement in one direction.

I am very confused.

Best regards,

Urs

Attached file:
ModalComparision.pdf, 451149kb

RichardS

hi urs,

doesn't inventor use 2nd order elements by default (or even 3rd order for some simulations)?

Did you also use 2nd order tets for the modal analysis?

Best,

Richard

RichardS

I did a quick test with SalomeMeca2015.2

and got 168.2Hz with 102 2nd order Tet elements. With the same mesh size and 1st order elements I get 260Hz.

I guess its all about the elements, obviously Code-Aster modal analysis calculation is perfectly fine.

Best,

Richard

urshelfenstein

Hey Richard,

You are right. I changed the elements to second order elements and got for a mesh with 120 elements an a mesh with 2871 elements exactly the same frequency of 167.24 Hz. Therefore, if I use second order elements the result is accurate and also not depending on the mesh size.

So I have now found a way to get good results. But one question remains. Why is there such a big difference between linear and second order elements.

Even with a very fine mesh of such a simple geometry (2781 Elements) I had with linear elements a Error of almost 10% when I used linear elements. So far I used second order elements for complex and curved geometries. Is that in general a bad approach and I should use second order elements as default?

Especially for a modal analysis I never thought that the order of the element creates such a big difference. According my understanding the result depends on the mass and the stiffness and on this simple beam the geometry is perfectly approximated with simple linear tetra elements. Where is my understanding wrong.

Thanks a lot for your support,

Urs

paster

Hello

The geometry yes, the mass yes but the stiffness NO!

Good luck with the Finite element Method

boyere

I can't say more: linear 3d elements converge very slowly when computing bending or normal modes.

It has already been discussed in this forum.

So it's strongly advised to use quadratic elements (or structural elements).

But I may add one point: the general philosophy with Code_Aster is that the user should always control his calculation. If he asks for linear element, he gets linear elements. Code_Aster doesn't secretly change them in quadratic ones to improve the results.

Emmanuel

urshelfenstein

Hi Everybody,

Thanks for your answers. I will follow this strongly advise to use quadratic elements.

It is good that Code_Aster does what it is told to do. It is much better than to use a black box and hoping that the right stuff is done.

BR,

Urs