Hinge mechanism in Code_Aster

vishwas

Hello,
I am trying to simulate a bar hinged at one end and falling under gravity. A hole in the bar represents the hinge.

I modeled the bar as solid elements and created a POI1 element at hole location. Then I conneted the center node to some nodes on hole surface with K_TR_D_L elements.
I assigned necessary charecteristics of M_TR_D_N, K_TR_D_N, K_TR_D_L and M_TR_D_L most of them zero to make the 0D element and springs massless.
However, the software gives simgularity matrix error.
Attaching the case in google drive as uploading here in forum seems not possible.
https--://drive.google.com/file/d/1RAXufDhsAakGh117EoiH7lgk8XafSYUa/view?usp=sharing
What could be wrong here?

Thanks and Regards

Sound_Spinning

vishwas
Nodes on solids do not have/understand rotations, you may be hitting rigid body modes, a guess.
Try modelling a 'soft' coupling via liaison_RBE3 between the POI1 and the nodes set on the bore. Then you get 6DoF at ref_node (POI1) and can have a 6DoF spring-to-ground or whatever you need to hold things up properly.
For the hinge effect you just make the rot DoF on that spring zero or very low, and the other values high, depending on what you want to model.

vishwas

Hello,
I tried using RBE3 constraint but still getting singular matrix error.
Also, previously upto Code aster version 15.4, GROT_GDEP used to work for solid elements taking into account large rotations but now it seems only working with COQUE_3D models.

I dont know if GREEN_LAGRANGE can do large rotations as efficiently as before. SIMO_MIEHE can do it but it is computationally expensive.It is so easy to apply cylindrical support in other software.
I attach study here:

Regards
Anirudh
https: //drive.google.com/file/d/1zEUYO-40HNkET6N_bv8qvp1rFbgb-WVd/view?usp=drive_link

Sound_Spinning

vishwas
Do a linear model 1st, if that doesn't work, don't turn any non-linear stuff on till understood with a linear model.

jeanpierreaubry

vishwas
this is my rewording of the problem
https://transfert.free.fr/cdP5zLG

vishwas

jeanpierreaubry
Hi,
Good news the simulation is runnung fine for both static and dynamic cases. Surely GREEN_LAGRANGE worked well for lage rotations.
However, I have a few questions:
Why did you create a new POI1 named n1p when a 0D element n1 already existed on the node 1. Isn't 0D element added in mesh module same as POI1 created by CREA_MAILLAGE?
Also, obs 0D element doesn't seem to do anything.
Why didn't we need to create all faces of boundary elements and assign them 3D modelisation?
I see no modelisation is applied to 'int' group of faces. Why doesn't the solver complain that no modelisation is applied to these elements. Do the 3d elements (magenta colour) 'own' their boundary 2d faces (blue faces) and automatically assign them the 3D modelisation).
This is important to know because in another hyperelastic study that I have shared , If a face group/SEG2 group is included in AFFE_CHAR_MECA, the software complaints that it needs to be assigned some modelisation(although it is sub part(boundary faces/lines) of same 3d solid elements).
I Manually replaced kk with 0 for DRZ(no stiffness) in Dynamic calculation still working fine. Also enabled gravity full from start.

DEBUT()

kk = 1.0 * 10000

mesh0 = LIRE_MAILLAGE(FORMAT='MED',
UNITE=2)

mesh = CREA_MAILLAGE(CREA_POI1=_F(GROUP_MA='n1',
NOM_GROUP_MA=('n1p', )),
INFO=1,
MAILLAGE=mesh0)

mesh = DEFI_GROUP(reuse=mesh,
CREA_GROUP_NO=(_F(GROUP_MA='n1',
NOM='n1'),
_F(GROUP_MA='obs',
NOM='obs'),
_F(GROUP_MA='int',
NOM='int')),
MAILLAGE=mesh)

model = AFFE_MODELE(AFFE=(_F(GROUP_MA='Cut_1_1',
MODELISATION='3D',
PHENOMENE='MECANIQUE'),
F(GROUP_MA=('n1p', ),
MODELISATION=('DIS_TR', ),
PHENOMENE='MECANIQUE')),
MAILLAGE=mesh)
elemprop = AFFE_CARA_ELEM(DISCRET=F(CARA='K_TR_D_N',
GROUP_MA=('n1p', ),
VALE=(10000.0, 10000.0, 10000.0, 0.0, 10000.0, 10000.0)),
MODELE=model)

mater = DEFI_MATERIAU(ELAS=_F(E=200000000000.0,
NU=0.33,
RHO=7800.0))

fieldmat = AFFE_MATERIAU(AFFE=_F(MATER=(mater, ),
TOUT='OUI'),
MODELE=model)

listr = DEFI_LIST_REEL(DEBUT=0.0,
INTERVALLE=_F(JUSQU_A=5,
PAS=0.1))

times = DEFI_LIST_INST(DEFI_LIST=F(LIST_INST=listr),
ECHEC=F(SUBD_NIVEAU=3,
SUBD_PAS=4),
METHODE='MANUEL',
MODELE=model)

load0_m = DEFI_FONCTION(NOM_PARA='INST',
PROL_DROITE='CONSTANT',
PROL_GAUCHE='CONSTANT',
VALE=(0, 0, 1, 1))

lsolid = AFFE_CHAR_MECA(LIAISON_RBE3=_F(COEF_ESCL=1.0,
DDL_ESCL=('DX-DY-DZ', ),
DDL_MAIT=('DX', 'DY', 'DZ', 'DRX', 'DRY', 'DRZ'),
GROUP_NO_ESCL='int',
GROUP_NO_MAIT='n1'),
MODELE=model)

load = AFFE_CHAR_MECA(DDL_IMPO=_F(DRY=0.0,
DRZ=0.0,
DX=0.0,
DY=0.0,
DZ=0.0,
GROUP_NO=('n1', )),
MODELE=model)

load0 = AFFE_CHAR_MECA(MODELE=model,
PESANTEUR=F(DIRECTION=(0.0, 0.0, -1.0),
GRAVITE=10.0))
try:
#comment: resnonl = STAT_NON_LINE(CARA_ELEM=elemprop,
#comment: CHAM_MATER=fieldmat,
#comment: COMPORTEMENT=(F(DEFORMATION='GREEN_LAGRANGE',
#comment: GROUP_MA='Cut_1_1'),
#comment: F(DEFORMATION='PETIT',
#comment: GROUP_MA='n1p')),
#comment: CONVERGENCE=F(ITER_GLOB_MAXI=20,
#comment: RESI_GLOB_RELA=0.001),
#comment: EXCIT=(_F(CHARGE=lsolid),
#comment: _F(CHARGE=load),
#comment: F(CHARGE=load0)),
#comment: INCREMENT=F(LIST_INST=times),
#comment: MODELE=model,
#comment: NEWTON=F(MATRICE='TANGENTE',
#comment: PREDICTION='TANGENTE',
#comment: REAC_ITER=1),
#comment: SOLVEUR=F(NPREC=-1))

resnonl2 = DYNA_NON_LINE(CARA_ELEM=elemprop,
	                 CHAM_MATER=fieldmat,
	                 COMPORTEMENT=_F(DEFORMATION='GREEN_LAGRANGE',
	                                 TOUT='OUI'),
	                 CONVERGENCE=_F(ITER_GLOB_MAXI=10,
	                                RESI_GLOB_MAXI=1.0,
	                                RESI_GLOB_RELA=0.01),
	                 EXCIT=(_F(CHARGE=lsolid),
	                        _F(CHARGE=load),
	                        _F(CHARGE=load0)),
	                 INCREMENT=_F(LIST_INST=times),
	                 MODELE=model,
	                 NEWTON=_F(MATRICE='TANGENTE',
	                           PREDICTION='TANGENTE',
	                           REAC_INCR=1,
	                           REAC_ITER=1),
	                 SCHEMA_TEMPS=_F(FORMULATION='DEPLACEMENT',
	                                 SCHEMA='HHT'))

except:
pass
#comment: IMPR_RESU(FORMAT='RESULTAT',
#comment: RESU=_F(FORMAT_R='1PE12.3',
#comment: GROUP_NO=('n1', 'obs'),
#comment: NOM_CHAM='DEPL',
#comment: RESULTAT=resnonl),
#comment: UNITE=8)

IMPR_RESU(FORMAT='MED',
RESU=_F(RESULTAT=resnonl2),
UNITE=80)

FIN()

Thanks and Regards
Anirudh

jeanpierreaubry

vishwas
nice to know it works as expected

Why did you create a new POI1 named n1p when a 0D element n1 already existed on the node 1. Isn't 0D element added in mesh module same as POI1 created by CREA_MAILLAGE?

if a node is not linked by a physical element to the rest of the structure one has to create a POI1 so as to be able to assign if some stiffness
at least this the way it works if the mesh is created with Gmsh, i do not know for salome as i never use it

Also, obs 0D element doesn't seem to do anything.

it is used to print the displacement in ASCII IMPR_RESU to quickly view the DEPL without opening a graphic post pro window

I see no modelisation is applied to 'int' group of faces.

because i use LIAISON_RBE3 with a node to node relation

Why doesn't the solver complain that no modelisation is applied to these elements. Do the 3d elements (magenta colour) 'own' their boundary 2d faces (blue faces) and automatically assign them the 3D modelisation).

we have to specify surface or lines with 3D MODELISATION only if these faces or lines carry some boundary conditions

If a face group/SEG2 group is included in AFFE_CHAR_MECA, the software complaints that it needs to be assigned some modelisation(although it is sub part(boundary faces/lines) of same 3d solid elements).

as i say just above

if any other questions do not hesitate

k_zurawski

Hi,
I don't understand the 'link' group in your code. You assigned K_TR_D_L and M_TR_D_L to the group. Why haven't you used LIAISON_SOLIDE to make a rigid connection between the 'n1' and hole surface?

vishwas

k_zurawski
Hi,
I didn't use them in latest version. See command file above.
I initially created them as some sort of link between center node and edge nodes of hole. Don't need particularly after using RBE3 .
LIASION_SOLIDE is not implemented in DYNA_NON_LINE. As this mechanism is to be dynamic in nature, so not used.

Regards
Anirudh