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

You are not logged in.

#1 2019-03-09 10:14:37

nirmaljoshi
Member
From: Japan
Registered: 2018-10-12
Posts: 186

[solved]linear tranlation in contact

Hi all,
How do we allow the translation of one object embedded in another object using contact? I tried (a steel rod is pulled out from concrete block), but could not succeed. Help and suggestions required as I am doing contact realted problem in Codeaster for first time.

Last edited by nirmaljoshi (2019-03-12 02:12:01)


Attachments:
contact.zip, Size: 47.13 KiB, Downloads: 108

Offline

#2 2019-03-09 12:04:50

jeanpierreaubry
Guru
From: nantes (france)
Registered: 2009-03-12
Posts: 3,638

Re: [solved]linear tranlation in contact

hello

if a remeber well
contact is between two 2D faces and not 3D volumes

jean pierre aubry


consider reading my book
freely available here https://framabook.org/beginning-with-code_aster/

Offline

#3 2019-03-11 02:03:15

nirmaljoshi
Member
From: Japan
Registered: 2018-10-12
Posts: 186

Re: [solved]linear tranlation in contact

Thanks for resoponding.
Now I used surface for contact-interaction instead of nodes in   LIAISON_MAIL and the simulation ran smoothly. But the output were quite strange when I visualized in Paravis.


Attachments:
Stage_1.comm, Size: 5.73 KiB, Downloads: 133

Offline

#4 2019-03-11 02:09:29

nirmaljoshi
Member
From: Japan
Registered: 2018-10-12
Posts: 186

Re: [solved]linear tranlation in contact

I tried the example in your book too that describes Columb contact. There also I got strange result. i.e. instead of the levers rotating, it got embedded with each other (I suppose that is not the expected result?).


Attachments:
wrenchcontact.zip, Size: 475.29 KiB, Downloads: 109

Offline

#5 2019-03-11 08:25:02

jeanpierreaubry
Guru
From: nantes (france)
Registered: 2009-03-12
Posts: 3,638

Re: [solved]linear tranlation in contact

regarding the contact problem

with 'glue' you are gluing the steel part to the concrete part
with 'contact' you for these two part to slide one over the other
but they are already glued together
i do not understand what you want!

regarding the wrench
the file part1.med in the archive is probably corrupted


consider reading my book
freely available here https://framabook.org/beginning-with-code_aster/

Offline

#6 2019-03-11 09:06:00

nirmaljoshi
Member
From: Japan
Registered: 2018-10-12
Posts: 186

Re: [solved]linear tranlation in contact

jeanpierreaubry wrote:

with 'glue' you are gluing the steel part to the concrete part

I tried without using 'glue' (just removed the 'glue' part in analysis, in which case, I got error.

What i want is as follows:
The steel bar should be pulled out from the concrete. While doing so, the resistance force should be generated by the contact surface between the steel and concrete. This is a simple pull out test to check the bonding. Something similar to attached animation (only the concrete and steel part).

Last edited by nirmaljoshi (2019-03-11 09:06:29)


Attachments:
pull test animation.gif, Size: 79.43 KiB, Downloads: 330

Offline

#7 2019-03-11 09:24:53

mecour
Member
From: Ostrava (Czech)
Registered: 2011-04-04
Posts: 155

Re: [solved]linear tranlation in contact

Hello,

it is not good to simulate this problem with conctact. There is no adhesion, cohesion and other aspects of steel concrete connection only friction. Maybe better to use some cohesive elements. As starting point I can recommend you the JOINT_MECA_RUPT model. The usage is quite simple with good results.

Offline

#8 2019-03-11 09:39:01

jeanpierreaubry
Guru
From: nantes (france)
Registered: 2009-03-12
Posts: 3,638

Re: [solved]linear tranlation in contact

@mecour
you are right  there is no force to generate friction here
contact could be used if we dilated the steel rod so as to increase the diameter
or cooling down the concrete
something like that may happen when the concrete dries out
i overlooked that point
regarding JOINT_MECA_RUPT i have no experience

@nirmaljoshi

I tried without using 'glue' (just removed the 'glue' part in analysis, in which case, I got error.

while the trial and error method is sometimes quite useful
one has nevertheless to apply realistic conditions


consider reading my book
freely available here https://framabook.org/beginning-with-code_aster/

Offline

#9 2019-03-11 10:02:28

nirmaljoshi
Member
From: Japan
Registered: 2018-10-12
Posts: 186

Re: [solved]linear tranlation in contact

@jeanpierreaubry, @mecor
Thanks for your suggestions. I changes some boundary condition and as you guys indicated, the pulling force was zero. The comm file is listed below.

DEBUT(LANG='EN')

meshC = LIRE_MAILLAGE(FORMAT='MED',
                      UNITE=4)

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

mesh = ASSE_MAILLAGE(MAILLAGE_1=meshC,
                     MAILLAGE_2=meshS,
                     OPERATION='SUPERPOSE')

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

steelGC = DEFI_MATER_GC(ACIER=_F(E=2e+11,
                                 NU=0.3,
                                 SY=400000000.0))

concGC = DEFI_MATER_GC(MAZARS=_F(CODIFICATION='BAEL91',
                                 FCJ=35900000.0,
                                 UNITE_CONTRAINTE='Pa'))

fieldmat = AFFE_MATERIAU(AFFE=(_F(GROUP_MA=('Group_steel', ),
                                  MATER=(steelGC, )),
                               _F(GROUP_MA=('Group_concrete', ),
                                  MATER=(concGC, ))),
                         MODELE=model)

fload = DEFI_FONCTION(INTERPOL=('LIN', ),
                      NOM_PARA='INST',
                      PROL_DROITE='LINEAIRE',
                      PROL_GAUCHE='LINEAIRE',
                      VALE=(0.0, 0.0, 80.0, 80.0))

listr = DEFI_LIST_REEL(DEBUT=0.0,
                       INTERVALLE=(_F(JUSQU_A=5.0,
                                      PAS=0.5),
                                   _F(JUSQU_A=20.0,
                                      PAS=1.0),
                                   _F(JUSQU_A=50.0,
                                      PAS=2.0),
                                   _F(JUSQU_A=100.0,
                                      PAS=5.0),
                                   _F(JUSQU_A=200.0,
                                      PAS=10.0)))

support = AFFE_CHAR_MECA(DDL_IMPO=_F(GROUP_MA=('Group_supportFace', ),
                                     LIAISON='ENCASTRE'),
                         MODELE=model)

load1 = AFFE_CHAR_MECA(DDL_IMPO=_F(DX=0.0,
                                   DY=0.0,
                                   DZ=1e-05,
                                   GROUP_MA=('Group_loadingFace', )),
                       MODELE=model)

contact = DEFI_CONTACT(FORMULATION='CONTINUE',
                       FROTTEMENT='COULOMB',
                       MODELE=model,
                       ZONE=_F(ALGO_CONT='PENALISATION',
                               ALGO_FROT='PENALISATION',
                               COEF_PENA_CONT=40000000.0,
                               COEF_PENA_FROT=400000.0,
                               COULOMB=0.45,
                               GROUP_MA_ESCL=('Group_contConc', ),
                               GROUP_MA_MAIT=('Group_contSteel', )))

resnonl = STAT_NON_LINE(CHAM_MATER=fieldmat,
                        COMPORTEMENT=(_F(DEFORMATION='PETIT',
                                         GROUP_MA=('Group_steel', ),
                                         RELATION='VMIS_CINE_LINE'),
                                      _F(GROUP_MA=('Group_concrete', ),
                                         RELATION='MAZARS')),
                        CONTACT=contact,
                        CONVERGENCE=_F(ARRET='NON',
                                       ITER_GLOB_MAXI=200,
                                       RESI_GLOB_MAXI=0.001),
                        EXCIT=(_F(CHARGE=support),
                               _F(CHARGE=load1,
                                  FONC_MULT=fload)),
                        INCREMENT=_F(LIST_INST=listr),
                        METHODE='NEWTON',
                        MODELE=model,
                        NEWTON=_F(MATRICE='TANGENTE',
                                  PREDICTION='TANGENTE',
                                  REAC_ITER=1),
                        SOLVEUR=_F(METHODE='MULT_FRONT'))

rxn = CALC_CHAMP(CONTRAINTE=('SIGM_ELNO', ),
                 DEFORMATION=('EPSI_ELNO', ),
                 FORCE=('REAC_NODA', ),
                 RESULTAT=resnonl)

table = POST_RELEVE_T(ACTION=(_F(GROUP_NO=('Group_steelFibreNode', ),
                                 INTITULE='disp',
                                 NOM_CHAM='DEPL',
                                 OPERATION=('EXTRACTION', ),
                                 RESULTANTE=('DZ', ),
                                 RESULTAT=resnonl),
                              _F(GROUP_NO=('Group_loadingFace', ),
                                 INTITULE='eqLoad',
                                 NOM_CHAM='REAC_NODA',
                                 OPERATION=('EXTRACTION', ),
                                 RESULTANTE=('DZ', ),
                                 RESULTAT=rxn),
                              _F(GROUP_NO=('Group_steelFibreNode', ),
                                 INTITULE='strain',
                                 NOM_CHAM='EPSI_ELNO',
                                 NOM_CMP=('EPZZ', ),
                                 OPERATION=('EXTRACTION', ),
                                 RESULTAT=rxn),
                              _F(GROUP_NO=('Group_steelFibreNode', ),
                                 INTITULE='stress',
                                 NOM_CHAM='SIGM_ELNO',
                                 NOM_CMP=('SIZZ', ),
                                 OPERATION=('EXTRACTION', ),
                                 RESULTAT=rxn)))

IMPR_RESU(FORMAT='MED',
          RESU=(_F(RESULTAT=resnonl),
                _F(RESULTAT=rxn)),
          UNITE=2)

IMPR_TABLE(FORMAT='TABLEAU',
           SEPARATEUR=' ,',
           TABLE=table,
           UNITE=8)

FIN()
jeanpierreaubry wrote:

you are right  there is no force to generate friction here
contact could be used if we dilated the steel rod so as to increase the diameter
or cooling down the concrete
something like that may happen when the concrete dries out

You are exactly describing my next step. i.e. I need to dilate the concrete (effect due to ASR). Any further suggestions would be of great help.

Last edited by nirmaljoshi (2019-03-11 13:09:27)

Offline

#10 2020-08-25 16:26:56

Duc Vu
Member
Registered: 2020-04-03
Posts: 19

Re: [solved]linear tranlation in contact

Hi nirmaljoshi, mecour and JP,

I'm performing the same problem with yours except the steel rod is pulled out by a horizontal force (DY and DX instead of DZ as describe in your mesh). So If you solved this problem with contact, could you provide your .comm file, if not, did you tried to play with cohesive element as the suggest of @mecour? As I never used cohesive element, can you give me some indication?

Offline