Static structural analysis for rotating wheel

  • Zach
  • Topic Author
  • Offline
  • Junior Member
  • Junior Member
More
8 years 10 months ago #8079 by Zach
Hi,
I checked this problem of stress concentration with another geometry and compared it with ansys results.
Ansys: www.dropbox.com/s/t193n1iwn74oj5k/9243-5ansys.png?dl=0 - look realistic (at 1000 RPM)
Aster: www.dropbox.com/s/aqjzvxrs3wczvo9/9243-5aster.png?dl=0 - not realistic. Seems like it is analysed as one detail, however - it should be with circular symmetry.
Here are study files:
www.dropbox.com/s/691c5khxxzgih6v/9243-5_1.1.comm?dl=0
www.dropbox.com/s/18ba1hf460fmjxo/9243-5_1.1.hdf?dl=0
www.dropbox.com/s/40bpsaxy2xb6qz9/9243-5_1.1Case.mess?dl=0
www.dropbox.com/s/xinejx860qq2mkz/9243-5_1.1Case.rmed?dl=0
www.dropbox.com/s/d8iq5l1h6dj86z9/9243-5_1.1Mesh.med?dl=0

What is the reason of such strange results?
Is there smth wrong with circular symmetry definition?

Please Log in or Create an account to join the conversation.

  • Zach
  • Topic Author
  • Offline
  • Junior Member
  • Junior Member
More
8 years 10 months ago #8080 by Zach
So, I made the same analysis without circular symmetry ie for full wheel:
www.dropbox.com/s/s4ssndbs1m9fpxu/9243-5asterFULL.png?dl=0 - result is more realistic (although max is ~30% higher then in ansys, do not know why...).
It means, that there is really smth wrong in command file with circular symmetry definition.
Could someone help to solve it?

Please Log in or Create an account to join the conversation.

More
8 years 10 months ago - 8 years 10 months ago #8081 by Claus
Please have a look at my tutorial regarding plasticity on the wiki here. There is a section on handling symmetry, specifically:
BC=AFFE_CHAR_MECA(MODELE=Model,
                  DDL_IMPO=(_F(GROUP_NO='PLAN_XOY',
                               DZ=0.0,),
                            _F(GROUP_NO='suprt1',
                               DY=0.0,),),
                  LIAISON_OBLIQUE=_F(GROUP_NO='PLAN_120',
                                     ANGL_NAUT=(0,-120,0,),
                                     DZ=0.0,),);

Regarding precision: It might have to do with mesh refinement and mesh quality etc. Are you using a quadratic mesh for the simulation? (I haven't checked the mesh, only .comm)

/C

Code_Aster release : STA11.4 on OpenSUSE 12.3 64 bits - EDF/Intel version
Last edit: 8 years 10 months ago by Claus.

Please Log in or Create an account to join the conversation.

More
8 years 10 months ago - 8 years 10 months ago #8083 by RichardS
Hello Claws,

are you sure that the code you provided really does a cyclic BC, I think not (at least not for general geometries)?


Hello ZachJa,
you made a simple mistake, you defined the cyclic boundary condition, but didn't assign it to the static analysis!
After this is fixed the simulation almost runs, you just have now a few nodes overconstrained (the ones that are on the edge between 'fix' and 'SLAVE').
I modified the SLAVE group by removing the overconstrained nodes and now the results should look good.
Attached is the modified command file.

Best regards,
Richard

/EDIT:
Upload seems to not work so I'll pollute the thread with it:
DEBUT();

MA=DEFI_MATERIAU(ELAS=_F(E=2.1e+11,
                         NU=0.3,
                         RHO=7800,),
                      );    

MAIL=LIRE_MAILLAGE(FORMAT='MED',);

MAIL=MODI_MAILLAGE(reuse=MAIL,
                   MAILLAGE=MAIL,
                   ORIE_PEAU_3D=_F(GROUP_MA=('fix',),),
                   );

# create node groups fom element groups 'SLAVE' and 'fix' with the same names
MAIL=DEFI_GROUP(reuse=MAIL,
		MAILLAGE=MAIL,
		CREA_GROUP_NO=_F(GROUP_MA=('SLAVE','fix')),
		);

# create a node group which is the difference of SLAVE with fix named SLAVE_OK
MAIL=DEFI_GROUP(reuse=MAIL,
		MAILLAGE=MAIL,
		CREA_GROUP_NO=_F(DIFFE=('SLAVE','fix'), NOM='SLAVE_OK'),
		);

MODE=AFFE_MODELE(MAILLAGE=MAIL,
                 AFFE=_F(TOUT='OUI',
                         PHENOMENE='MECANIQUE',
                         MODELISATION='3D',),);

MATE=AFFE_MATERIAU(MAILLAGE=MAIL,
                   AFFE=_F(TOUT='OUI',
                           MATER=MA,),);

CHAR=AFFE_CHAR_MECA(MODELE=MODE,
                    ROTATION=_F(GROUP_MA='rot',
                                VITESSE=104.7,
                                AXE=(0,0,1,),),
                    DDL_IMPO=_F(GROUP_MA=('fix',),
                                DX=0.0,
                                DY=0.0,
                                DZ=0.0,),);

CYCL=AFFE_CHAR_MECA(MODELE=MODE,
                    LIAISON_MAIL=_F(GROUP_MA_MAIT='rot',
                                    GROUP_NO_ESCL='SLAVE_OK',
                                    ANGL_NAUT=(18.0,0.0,0.0,),
                                    CENTRE=(0.0,0.0,0.0,),),
                    );	

RESU=MECA_STATIQUE(MODELE=MODE,
                   CHAM_MATER=MATE,
                   EXCIT=(_F(CHARGE=CHAR,),
			  _F(CHARGE=CYCL,),),);

RESU=CALC_CHAMP(reuse =RESU,
               MODELE=MODE,
               CHAM_MATER=MATE,
               RESULTAT=RESU,
               CONTRAINTE=('SIGM_NOEU','SIGM_ELGA','SIGM_ELNO',),
               CRITERES=('SIEQ_NOEU','SIEQ_ELGA','SIEQ_ELNO',),
               );

IMPR_RESU(FORMAT='MED',
          UNITE=80,
          RESU=_F(RESULTAT=RESU,
                  NOM_CHAM=('SIGM_NOEU','SIEQ_NOEU','DEPL','SIGM_ELGA','SIGM_ELNO',),),);

FIN();

SimScale - Engineering Simulation in your browser!
Last edit: 8 years 10 months ago by RichardS.

Please Log in or Create an account to join the conversation.

  • Zach
  • Topic Author
  • Offline
  • Junior Member
  • Junior Member
More
8 years 10 months ago #8084 by Zach
Thank you RichardS,
could you please specify what do you mean with: "a node group which is the difference of SLAVE with fix" - I am not sure that got it clear (may be you could send/upload mesh file). Is it a group that includes all nodes except groups of nodes "SLAVE" and "fix"?

Please Log in or Create an account to join the conversation.

More
8 years 10 months ago #8085 by RichardS

ZachJa wrote: Thank you RichardS,
could you please specify what do you mean with: "a node group which is the difference of SLAVE with fix" - I am not sure that got it clear (may be you could send/upload mesh file). Is it a group that includes all nodes except groups of nodes "SLAVE" and "fix"?


Hello ZachJa,
I didn't change the mesh file,
all additional groups were created with Code-Aster inside the comm file that I posted.
Perhaps its easier to put it as mathematical expression:
SLAVE_OK = SLAVE - fix
"SLAVE_OK are all nodes that are in SLAVE but NOT in fix".

Best,
Richard

SimScale - Engineering Simulation in your browser!

Please Log in or Create an account to join the conversation.

Moderators: catux
Time to create page: 0.171 seconds
Powered by Kunena Forum