Welcome to the forums. Please post in English or French.

You are not logged in.

#1 2018-10-12 13:18:17

Anirudh
Member
Registered: 2017-09-11
Posts: 252

NO force/pressure acting in D_PLAN

Hello everyone,
I am trying to impose a pressure load/edge force/nodal force on a edge in this model below.
However all of them cause singular matrix error. Only nodal displacement load(DDL_IMPO) or Edge displacement(FACE_IMPO) are working. But I need pressure load to work to rotate the body around center.
I would be very grateful If someone can find the error.
Here is my command file:

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

mesh = MODI_MAILLAGE(reuse=mesh,
                     MAILLAGE=mesh,
                     ORIE_PEAU_2D=_F(GROUP_MA=('e1', )))

model = AFFE_MODELE(AFFE=(_F(MODELISATION=('D_PLAN', ),
                             PHENOMENE='MECANIQUE',
                             TOUT='OUI'),
                          _F(GROUP_MA=('od1', ),
                             MODELISATION=('2D_DIS_TR', ),
                             PHENOMENE='MECANIQUE'),
                          _F(GROUP_MA=('r1', ),
                             MODELISATION=('2D_DIS_T', ),
                             PHENOMENE='MECANIQUE')),
                    MAILLAGE=mesh)

elemprop = AFFE_CARA_ELEM(DISCRET_2D=(_F(CARA='K_TR_D_N',
                                         GROUP_MA=('od1', ),
                                         VALE=(10.0, 10.0, 0.0001)),
                                      _F(CARA='M_TR_D_N',
                                         GROUP_MA=('od1', ),
                                         VALE=(0.01, 0.01, 0.01, 0.01)),
                                      _F(CARA='K_T_D_N',
                                         GROUP_MA=('r1', ),
                                         VALE=(10.0, 10.0))),
                          MODELE=model)

mater = DEFI_MATERIAU(ELAS=_F(E=2e+11,
                              NU=0.33,
                              RHO=8000.0))

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

listr = DEFI_LIST_REEL(DEBUT=0.0,
                       INTERVALLE=_F(JUSQU_A=1.0,
                                     PAS=0.01))

unnamed0 = DEFI_FONCTION(NOM_PARA='INST',
                         VALE=(0.0, 0.0, 1.0, 1.0))

load = AFFE_CHAR_MECA(MODELE=model,
                      PRES_REP=_F(GROUP_MA=('e1', ),
                                  PRES=10.0))

load2 = AFFE_CHAR_MECA(DDL_IMPO=_F(DX=0.0,
                                   DY=0.0,
                                   GROUP_NO=('n1', )),
                       MODELE=model)

resnonl = STAT_NON_LINE(CARA_ELEM=elemprop,
                        CHAM_MATER=fieldmat,
                        COMPORTEMENT=_F(DEFORMATION='GROT_GDEP',
                                        RELATION='ELAS',
                                        TOUT='OUI'),
                        CONVERGENCE=_F(ITER_GLOB_MAXI=100,
                                       RESI_GLOB_RELA=1e-05),
                        EXCIT=(_F(CHARGE=load2,
                                  TYPE_CHARGE='DIDI'),
                               _F(CHARGE=load,
                                  FONC_MULT=unnamed0,
                                  TYPE_CHARGE='FIXE_CSTE')),
                        INCREMENT=_F(INST_FIN=0.5,
                                     LIST_INST=listr),
                        MODELE=model,
                        NEWTON=_F(MATRICE='TANGENTE',
                                  PREDICTION='ELASTIQUE',
                                  REAC_INCR=1,
                                  REAC_ITER=1))

Attaching all other files.

Much Thanks and Regards
Anirudh

Last edited by Anirudh (2018-10-12 13:29:48)


Attachments:
pressure_load.png, Size: 90.03 KiB, Downloads: 185

Offline

#2 2018-10-12 13:25:38

Anirudh
Member
Registered: 2017-09-11
Posts: 252

Re: NO force/pressure acting in D_PLAN

Hi,
Attaching Mess file and med file.

Thanks
Anirudh


Attachments:
med&mess_files.zip, Size: 11.34 KiB, Downloads: 117

Offline

#3 2018-10-12 14:05:03

Anirudh
Member
Registered: 2017-09-11
Posts: 252

Re: NO force/pressure acting in D_PLAN

Hello again,
I am getting a feeling that the Rotational stiffness of 2d_Discrete_TR on the 0D element at center node is not affected/usable.

Thanks
Anirudh

Offline

#4 2018-10-14 08:09:07

konyaro
Member
From: Genève
Registered: 2016-04-02
Posts: 237

Re: NO force/pressure acting in D_PLAN

Hello Anirudh,
The D_PLAN elements have no rotational DOF. That means that the rotational stiffness of your od1 element doesn't exist for your D_PLAN elements.

For instance, if I apply a rotation to a node of your D_PLAN elements, the translationnel stiffness of your r1 elements is seen by your D_PLAN elements but not the rotational one of your od1:

Rotation

Konyaro

Last edited by konyaro (2018-10-14 08:09:22)


Attachments:
rotation.png, Size: 38.68 KiB, Downloads: 278

失敗は成功のもと (L'échec est la base de la réussite)

Offline

#5 2018-10-15 06:15:01

Anirudh
Member
Registered: 2017-09-11
Posts: 252

Re: NO force/pressure acting in D_PLAN

Hi Konyaro,
Thanks for the informative result.
So, to use 0d1 stiffness, we should try this:
>>Create a duplicate node at center(on 0d1 node)
>>Reassign 0d1 on the new node created
>>Use discrete 2DIST_TR on the reassigned od1 element.
>>create Liasion DDL between the reassigned od1 and the triangle node.
>>Try applying pressure again.

Would that work?

Thanks a lot.

Anirudh

Last edited by Anirudh (2018-10-15 06:15:45)

Offline

#6 2018-10-16 06:20:16

konyaro
Member
From: Genève
Registered: 2016-04-02
Posts: 237

Re: NO force/pressure acting in D_PLAN

I don't think that will work as your D_PLAN elements don't have rotational DOF you won't be able to link the rotation with LIAISON_DDL. I would link the 0d1 node to the triangle with POU_D_T_GD.


失敗は成功のもと (L'échec est la base de la réussite)

Offline

#7 2018-11-03 13:38:02

Thomas DE SOZA
Guru
From: EDF
Registered: 2007-11-23
Posts: 3,066

Re: NO force/pressure acting in D_PLAN

Hello,

As explained by Konyaro, it is impossible to apply only pressure to a 2D model without blocking the rotational degree of freedom (with the center node, you are only blocking X and Y translations but in two 2D, there are three rigid body movements).

One solution would also be to use a LIAISON_ELEM=‘2D_POU’ linking a 2D_DIS_TR discrete element with for example an edge of the triangle transformed into a rectangle (e.g. replace the summit of the triangle with an edge of the rectangle whose center coincides with the discrete element).
The rotational stiffness of the discrete element must be input accordingly to your physical model. That’s this rotational stiffness that will mainly determine the rotation of the structure when submitted to the pressure.

TdS

Offline