Buckling analysis and imperfection

Konst73

Hello everyone, I am an old-school structural engineer but always focused on being able to navigate FEM analyses. Clearly, I turned to an open-source software like CODE-ASTER, and currently, I am learning through video tutorials. At the moment, my focus is on buckling analyses. Having acquired the procedure for determining critical loads for an idealized structure (free of imperfections/defects), I would like to take the next step by introducing such imperfections/defects into my analysis. To this end, I refer to the guidelines of certain technical standards, which suggest that imperfections can be introduced into the structure by considering specific equivalent loads. To better explain my intention, I am sharing an explanatory image (I hope I uploaded the image link well without violating the forum rules).

https://ibb.co/tJPC42c

I would like to apply the load q and find the deformed shape. Then, this deformation should serve as the domain for performing the buckling analysis to determine the critical load using the multiplier lambda, which should only interact with the exploratory load P, not with the load q. This is where I get stuck. I tried adapting the commands from a video that dealt with sub-model studies, where displacements were "projected," as well as commands from a tutorial on thermo-mechanical analysis where the temperature field was assigned to a different mesh (logically, for my study, I was attempting to project the displacement field obtained with the load q), but I failed. Can anyone suggest a resolution path for this issue? Thank you in advance for your suggestions and your time.
By the way, I apologize for my English, but it's the translator's fault…

ing.nicola

With command

depl0 = CREA_CHAMP( INST=0.0, NOM_CHAM='DEPL', OPERATION='EXTR', RESULTAT=reslin, TYPE_CHAM='NOEU_DEPL_R' )

you can extract the displacement.

Can use command

mesh = MODI_MAILLAGE( DEFORME=_F( DEPL=depl0, OPTION='TRAN' ), MAILLAGE=mesh )
to obtain the mesh in deformed state.,

If you want applicate a "x" percentage of DEPL , you have to use CREA_CHAMP ( AFFE ... VALE_F= x ) for manipulate DEPL champ where x is a FORMULE or FONCTION or you can use CREA_CHAMP ( COMB .... COEF_R = x )

Document U2.08.04 explain the procedure for buckling calculation.

Konst73

First of all, thank you very much for the suggestions that I wanted to apply to a model of a cantilever beam with dimensions of 1000x30x50 mm, discretized with hexahedral elements of 5 mm side length, and loaded on the 50x1000 face from the positive X side with a positive lateral load of 0.1 N/mm². The suggested procedure appears to work, and I am including it (complete) at the end of this comment. However, I would like to make some considerations, in case they might be of interest to someone and they may want to challenge them.

It seems that assigning the direction of the lateral load opposite (negative) to the shape of the first mode slightly increases the value of the critical load (in reality, I can explain this, but not from the standpoint of the mathematical model). Does this imply that we must start from a buckling analysis where the model is free of imperfections?
The values of the critical load between the condition of a perfect bar (without lateral load) and that of an imperfect bar (with lateral load to simulate imperfections) differ by only a few N, even though I have verified that the node coordinate on the upper face of the modified mesh differs from the displacement value obtained in the perfect bar model with lateral load.
Furthermore, I expected that using a lateral load of 0.5 N/mm² compared to 0.1 N/mm² would result in a significant variation in the critical load. However, this did not occur, as the final difference is only a few N. By the way, the maximum displacement of the bar with a lateral load of 0.1 N/mm² is approximately 26 mm (almost the length of the beam's shorter side). Could it be that this condition has no effect on the critical load value?
If anyone notices any major errors in the following command list, I don’t mind if I’m criticized, as long as they point it out. Thank you.

DEBUT()
#STAGE1
mesh = LIRE_MAILLAGE(UNITE=20)
model = AFFE_MODELE(AFFE=F(MODELISATION='3D',
PHENOMENE='MECANIQUE',
TOUT='OUI'),
MAILLAGE=mesh)
mater = DEFI_MATERIAU(ELAS=F(E=210000.0,
NU=0.3))
fieldmat = AFFE_MATERIAU(AFFE=F(MATER=(mater, ),
TOUT='OUI'),
MODELE=model)
BC = AFFE_CHAR_MECA(DDL_IMPO=F(DX=0.0,
DY=0.0,
DZ=0.0,
GROUP_MA=('Fix', )),
MODELE=model)
load1 = AFFE_CHAR_MECA(FORCE_FACE=F(FX=0.5,
GROUP_MA=('Load1', )),
MODELE=model)
reslin = MECA_STATIQUE(CHAM_MATER=fieldmat,
EXCIT=(F(CHARGE=BC),
F(CHARGE=load1)),
MODELE=model,
OPTION='SIEF_ELGA')
IMPR_RESU(RESU=F(RESULTAT=reslin),
UNITE=2)

#STAGE 2
field = CREA_CHAMP(NOM_CHAM='DEPL',
NUME_ORDRE=1,
OPERATION='EXTR',
RESULTAT=reslin,
TYPE_CHAM='NOEU_DEPL_R')
mesh = MODI_MAILLAGE(reuse=mesh,
DEFORME=F(DEPL=field,
OPTION='TRAN'),
MAILLAGE=mesh)
model2 = AFFE_MODELE(AFFE=F(MODELISATION='3D',
PHENOMENE='MECANIQUE',
TOUT='OUI'),
MAILLAGE=mesh)
fieldma2 = AFFE_MATERIAU(AFFE=F(MATER=(mater, ),
TOUT='OUI'),
MODELE=model2)
BC2 = AFFE_CHAR_MECA(DDL_IMPO=F(DX=0.0,
DY=0.0,
DZ=0.0,
GROUP_MA=('Fix', )),
MODELE=model2)
Load_N = AFFE_CHAR_MECA(FORCE_NODALE=F(FZ=-1.0,
GROUP_NO=('Load3', )),
MODELE=model2)
reslin2 = MECA_STATIQUE(CHAM_MATER=fieldma2,
EXCIT=(F(CHARGE=BC2),
F(CHARGE=Load_N)),
MODELE=model2,
OPTION='SIEF_ELGA')
IMPR_RESU(RESU=F(RESULTAT=reslin2),
UNITE=80)

#STAGE3
field1 = CREA_CHAMP(NOM_CHAM='SIEF_ELGA',
NUME_ORDRE=1,
OPERATION='EXTR',
RESULTAT=reslin2,
TYPE_CHAM='ELGA_SIEF_R')
ASSEMBLAGE(CHAM_MATER=fieldma2,
CHARGE=(BC2, ),
MATR_ASSE=(_F(MATRICE=CO('K_Rigi'),
OPTION='RIGI_MECA'),
F(MATRICE=CO('G_Rigi'),
OPTION='RIGI_GEOM',
SIEF_ELGA=field1)),
MODELE=model2,
NUME_DDL=CO('dofs'))
modes = CALC_MODES(MATR_RIGI=K_Rigi,
MATR_RIGI_GEOM=G_Rigi,
OPTION='PLUS_PETITE',
TYPE_RESU='MODE_FLAMB')
IMPR_RESU(RESU=F(RESULTAT=modes),
UNITE=3)
FIN()