Losing our minds over rigid modes frequency

gigi_proiettili

Hi everyone, me and my fellow colleagues are trying to reproduce rigid modes of vibration of an engine comparing them to Optistruct.
Our model is composed of block head and the 4 bracket that hold the structure to ground via springs, all the pieces are linked via LIAISON_MAILL. The springs are DIS_T formulization and K_T_D_L inside AFFE_CARA_ELEM.
The rigid modes simply won't converge to the Optistruct ones both in frequency and in mode shape.
The model is the same between the two, same mass and inertia and mesh.
Springs are defined in the same way in both softwares.
The rotational rigid modes seem to be the most affected with more than 90% error.
We tried K_TR_D_L assigning 0 stiffness value to the rotational DOF, nothing changed.
We changed the springs in optistruct and nothing changed.
We tried changing to Tri diag solver and nothing changed.
We tried reducing the stiffness of our springs by 99% just to send the rigid modes out of the way for the following dinamic simulation and the 3 rotational rigid modes now had similar frequency to optistruct ones, the 2 traslational mode were all under 3Hz though.
We tried the same springs formulation with a simple cube and 3 springs with a compensation mass linked via rbe3 and the two softwares converged.
Somewhere between the simple cube stage and the full engine model the softwares diverge and we just can't seem to find the reason for it.
By the way the bending modes are reproduced exceptionally good so this is our only concern right now.

If someone has any idea we would very glad to hear it since we have none left.
thanks everyone for your time.

Sound_Spinning

gigi_proiettili
Does the engine model have shells? if yes ==> can be odd with rots modes.
Is the cube test model with solids? if yes ==> that should agree vs OptiStruct.
Have you tried a free-free modal 1st; i.e. comment out all constraints? You should get 6 near 0Hz rigid body modes; if not ==> nothing to do with springs, but maybe shells if you use them in the engine model.

There is an entry on a similar subject to yours (maybe) here:
shells-with-tied-contacts-over-constrain-the-body-rotational-dof

gigi_proiettili

thanks for your reply.
The model does not have shells both the engine and the cube. Also both engine and cube are modelled as solids.
To be honest we never managed to run free-free modal analyses with this large models. Would you mind giving us your way to do them? we just set tri diag and flag the rigid modes box.

anyway this rigid modes mistery is yet to be solved.
if it helps i will list all the loads used for this analysis:
DDL_IMPO
LIAISON_MAIL
LIAISON_MAIL
LIAISON_SOLIDE

Sound_Spinning

gigi_proiettili
free-free modal, remove constraints, see comments:

# ---------------------------------
# STEP_2: Structural Modal Analysis
# ---------------------------------

# Setting the right matrices for a modal STEP
ASSEMBLAGE(
    MODELE = model_assy,
    CHAM_MATER = materials, 
    CARA_ELEM = element_props,
    # CHARGE = (fix_STEP_1, rigid_coups, soft_coups, ),
    ### use below for a free-free modal; i.e. check for 6 RBModes at ~0Hz.
    CHARGE = (rigid_coups, soft_coups, ),  
    MATR_ASSE = (
        _F( MATRICE = CO('MASS'), OPTION = "MASS_MECA", ),
        _F( MATRICE = CO('RIGI'), OPTION = "RIGI_MECA", ),
    ),
    NUME_DDL = CO('numdof'),
);

# Modal analysis setup
modes = CALC_MODES(
    MATR_RIGI = RIGI,
    MATR_MASS = MASS,
    OPTION = "PLUS_PETITE",
    CALC_FREQ = _F( 
        NMAX_FREQ = 12,       ### Number of modes
        NMAX_ITER_SHIFT = 3,
        PREC_SHIFT = 0.05,
        ### Below Important! to capture negative (~0Hz) rigid body modes.
        SEUIL_FREQ = 10,     ### Shift freq parameter, will turn to -10 in solve.
    ),
    SOLVEUR_MODAL = _F( METHODE = 'SORENSEN') ,    ### faster than Lanczos
    # SOLVEUR_MODAL = _F( METHODE = 'TRI_DIAG', MODE_RIGIDE = 'OUI',) ,   ### Lanczos solver
    SOLVEUR = _F(
        RESI_RELA = -1, NB_RHS = 10,
        METHODE='MUMPS', GESTION_MEMOIRE = 'AUTO', PCENT_PIVOT = 10, 
    ),
    VERI_MODE = _F(
        PREC_SHIFT = 0.05, SEUIL = 1e-06,
        STOP_ERREUR = 'NON', STURM = 'NON', 
    ),
    STOP_BANDE_VIDE = 'NON',
);

Those you listed are not loads, but constraints, very different. Any of them not setup properly will over-constrain rots rigid body motion on an assembly. Feel free to share your input deck and/or model?

PierluigiP29

Hello gigi,
Since I never worked on engines, could you explain better what do you mean exactly with 'rigid mode', and what is your goal? In my mind if I think about a rigid shape the frequency is 0 and it is related to an underconstrained model.

Anyway... A while ago I tried a free-free modal analysis found in the FORMA11B testcase, with a sphere used as an example to compare different modal solvers (Lanczos, Sorensen, QZ). I recommend having a look at it.
The only method that gave exactly 0Hz for the first 6 modes was Lanczos with the TRI_DIAG option, the others gave like XE-04/XE-05 Hz which is reasonable.

Also, in the beginning you say that the parts are linked by LIAISON_MAIL, but in the last reply I see you're using also LIAISON_SOLIDE. Have you tried using only LIAISON_SOLIDE?

gigi_proiettili

PierluigiP29
laczos didn't show any difference in mode frequency

gigi_proiettili

hi Pierluigi.
basically we ground the engine using springs attached to the engine brackets that would connect the engine to the chassis.
The modal analysis made in this way show the first 6 modes are rigid traslations or rotations. They are not properly rigid modes.
We tried TRI_DIAG before but the results didn't converge. we will try again with this current model that runs quickly and let you know.
We model bolt joints using liaison mail and the liaison solide are used to connect the spring heads to the brackets. using liaison solide for each bolt head tends to create numerical problems due to the planarity of the nodes groups

gigi_proiettili

Sound_Spinning

yes you are right those are not loads, i think something was lost in traslation.
here you go with the code:
`DEBUT(LANG='FR')

mesh = LIRE_MAILLAGE(FORMAT='MED',
UNITE=20)

model = AFFE_MODELE(AFFE=(_F(MODELISATION=('3D', ),
PHENOMENE='MECANIQUE',
TOUT='OUI'),
_F(GROUP_MA='molle',
MODELISATION='DIS_TR',
PHENOMENE='MECANIQUE'),
_F(GROUP_MA=('Compensation_CONM2', ),
MODELISATION='DIS_TR',
PHENOMENE='MECANIQUE')),
MAILLAGE=mesh)

elemprop = AFFE_CARA_ELEM(DISCRET=(_F(CARA='K_TR_D_L',
GROUP_MA='molle',
VALE=(300.0, 300.0, 400.0, 1000, 1000, 1000)),
_F(CARA='A_TR_D_L',
GROUP_MA=('molle', ),
VALE=(0.3, 0.3, 0.3, 0.3, 0.3, 0.3)),
_F(CARA='M_TR_D_N',
GROUP_MA=('Compensation_CONM2', ),
VALE=(0.1278943, 7799.711, 6871.534, 6053.892, 822.6508, -399.331, -413.313, 0, 0, 0))),
MODELE=model)

Al_Compressor = DEFI_MATERIAU(ELAS=F(E=73500,
NU=0.32,
RHO=2.7e-09))
...various material
Steel_COmpressor_Pulley = DEFI_MATERIAU(ELAS=F(E=200000,
NU=0.28,
RHO=5e-09))

materfl = AFFE_MATERIAU(AFFE=(_F(GROUP_MA='BODY_7.2',
MATER=(Steel_dyno_setup, )),
_F(GROUP_MA=('BLOCK', ),
MATER=(GMW4M, )),
_F(GROUP_MA=('ADAPTER', ),
MATER=(GMW5M, ))),
MODELE=model)

mecabc = AFFE_CHAR_MECA(DDL_IMPO=F(DRX=0.0,
DRY=0.0,
DRZ=0.0,
DX=0.0,
DY=0.0,
DZ=0.0,
GROUP_NO=('bc', )),
LIAISON_MAIL=(F(DISTANCE_MAX=10.0,
GROUP_MA_MAIT=('BLOCK', ),
GROUP_NO_ESCL=('toBLOCK3', )),
F(GROUP_MA_MAIT=('BODY_7.2', ),
GROUP_NO_ESCL=('tofrontjoined', ))),
LIAISON_RBE3=F(DDL_ESCL=('DX-DY-DZ', ),
DDL_MAIT=('DX', 'DY', 'DZ', 'DRX', 'DRY', 'DRZ'),
GROUP_NO_ESCL=('dist_1800502', ),
GROUP_NO_MAIT=('Compensation_CONM2_n', )),
LIAISON_SOLIDE=_F(GROUP_NO=('rigid_1689033bc', 'rigid_1689031bc', 'rigid_1689032bc', 'm_mounts_sx')),
MODELE=model)

ASSEMBLAGE(CARA_ELEM=elemprop,
CHAM_MATER=materfl,
CHARGE=(mecabc, ),
MATR_ASSE=(_F(MATRICE=CO('rigidite'),
OPTION='RIGI_MECA'),
_F(MATRICE=CO('masse'),
OPTION='MASS_MECA')),
MODELE=model,
NUME_DDL=CO('numeddl'))

result = CALC_MODES(CALC_FREQ=F(NMAX_FREQ=6),
MATR_MASS=masse,
MATR_RIGI=rigidite,
OPTION='PLUS_PETITE',
VERI_MODE=F(STOP_ERREUR='NON'))`

Could you please tell me something more about this suggestion of yours? "Any of them not setup properly will over-constrain rots rigid body motion on an assembly"

Sound_Spinning

gigi_proiettili
E.g. on a TIED contact, I see you have a large tolerance=10mm.
If your slave surfaces extend quite a bit away from the master and/or you have large gaps/overlaps between the slave : master you can easily over-constraint rots body motion from pure maths on the constraints. Same with equations or any other hard constraints.

It's very hard to tell more w/out looking at your 3D model and how things are constrained in the modal.