Code_Aster forums
Welcome on the forums. Please post in English or French.
You are not logged in. You won't be able to post until you register and log in using the top-right bar.
#1 2012-03-15 10:35:22
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
periods and forms of natural vibrations
Hi! Iam interested how calculate periods and forms of natural vibrations and form and reserves the loss of stability in attached beam case?
What commands I need to use?
file
https://docs.google.com/open?id=0B9BlA0 … UHFFcEkzdw
Code:
DEBUT();
#Read mesh
Mesh=LIRE_MAILLAGE(FORMAT='MED',);
Mesh=DEFI_GROUP(reuse =Mesh,
MAILLAGE=Mesh,
CREA_GROUP_MA=_F(NOM='TOUT',
TOUT='OUI',),);
#Assign a beam model - POU_D_E denotes a Euler/Bernoulli
Model=AFFE_MODELE(MAILLAGE=Mesh,
AFFE=_F(TOUT='OUI',
PHENOMENE='MECANIQUE',
MODELISATION='POU_D_E',),);
Material=DEFI_MATERIAU(ELAS=_F(E=66000,
NU=0.3,),);
MatField=AFFE_MATERIAU(MAILLAGE=Mesh,
AFFE=_F(TOUT='OUI',
MATER=Material,),);
A = 27400.0;
I_y = 712000000.0;
I_z = 283000000.0;
J = 6180000.0;
RY = 197;
RZ = 187;
AY = 1.46472;
AZ = 4.64168;
CARA_POU=AFFE_CARA_ELEM(MODELE=Model,
POUTRE=_F(GROUP_MA='TOUT',
SECTION='GENERALE',
CARA=('A','IY','IZ','JX','RY','RZ','AY','AZ',),
VALE=(A,I_y,I_z,J,RY,RZ,AY,AZ,),),);
#Boundary conditions
#Point 1 : Fixed
Hold=AFFE_CHAR_MECA(MODELE=Model,
DDL_IMPO=_F(GROUP_NO='fixx2',
LIAISON='ENCASTRE',),);
#Load
#Point 2 : Point load
Load=AFFE_CHAR_MECA(MODELE=Model,
FORCE_NODALE=_F(GROUP_NO='loadd',
FZ=-10000,),);
# Linear elastic solution
RESU1=MECA_STATIQUE(MODELE=Model,
CHAM_MATER=MatField,
CARA_ELEM=CARA_POU,
EXCIT=(_F(CHARGE=Hold,),
_F(CHARGE=Load,),),);
# Calculate forces etc.
RESU1=CALC_ELEM(reuse =RESU1,
RESULTAT=RESU1,
OPTION=('EFGE_ELNO_DEPL','SIPO_ELNO_DEPL','SIGM_ELNO_DEPL',),);
RESU1=CALC_NO(reuse =RESU1,
RESULTAT=RESU1,
OPTION=('REAC_NODA','EFGE_NOEU_DEPL','SIPO_NOEU_DEPL','FORC_NODA',),);
# Write to .med file
IMPR_RESU(MODELE=Model,
FORMAT='MED',
RESU=_F(MAILLAGE=Mesh,
RESULTAT=RESU1,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','REAC_NODA','SIPO_NOEU_DEPL','FORC_NODA',),),);
#Write to .resu file
IMPR_RESU(MODELE=Model,
FORMAT='RESULTAT',
RESU=_F(RESULTAT=RESU1,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','SIPO_NOEU_DEPL','REAC_NODA','SIGM_ELNO_DEPL',),
VALE_MAX='OUI',
VALE_MIN='OUI',),);
FIN();Offline
#2 2012-03-16 14:16:22
- jeanpierreaubry
- Ex-Guru
- From: nantes (france)
- Registered: 2009-03-12
- Posts: 1717
- Website
Re: periods and forms of natural vibrations
hello
you can find that in this
http://www.caelinux.org/wiki/index.php/ … ierreaubry
jean pierre aubry
Offline
#3 2012-04-01 22:08:50
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
Any idea, Any help?
Code:
DEBUT();
#Read mesh
Mesh=LIRE_MAILLAGE(FORMAT='MED',);
Mesh=DEFI_GROUP(reuse =Mesh,
MAILLAGE=Mesh,
CREA_GROUP_MA=_F(NOM='TOUT',
TOUT='OUI',),);
#Assign a beam model - POU_D_E denotes a Euler/Bernoulli
Model=AFFE_MODELE(MAILLAGE=Mesh,
AFFE=_F(TOUT='OUI',
PHENOMENE='MECANIQUE',
MODELISATION='POU_D_E',),);
Material=DEFI_MATERIAU(ELAS=_F(E=66000,
NU=0.3,RHO=1200),);
MatField=AFFE_MATERIAU(MAILLAGE=Mesh,
AFFE=_F(TOUT='OUI',
MATER=Material,),);
A = 27400.0;
I_y = 712000000.0;
I_z = 283000000.0;
J = 6180000.0;
RY = 197;
RZ = 187;
AY = 1.46472;
AZ = 4.64168;
CARA_POU=AFFE_CARA_ELEM(MODELE=Model,
POUTRE=_F(GROUP_MA='TOUT',
SECTION='GENERALE',
CARA=('A','IY','IZ','JX','RY','RZ','AY','AZ',),
VALE=(A,I_y,I_z,J,RY,RZ,AY,AZ,),),);
#Boundary conditions
#Point 1 : Fixed
Hold=AFFE_CHAR_MECA(MODELE=Model,
DDL_IMPO=_F(GROUP_NO='fixx2',
LIAISON='ENCASTRE',),);
#Load
#Point 2 : Point load
Load=AFFE_CHAR_MECA(MODELE=Model,
FORCE_NODALE=_F(GROUP_NO='loadd',
FZ=-10000,),);
# Linear elastic solution
RESU1=MECA_STATIQUE(MODELE=Model,
CHAM_MATER=MatField,
CARA_ELEM=CARA_POU,
EXCIT=(_F(CHARGE=Hold,),
_F(CHARGE=Load,),),);
# Calculate forces etc.
RESU1=CALC_ELEM(reuse =RESU1,
RESULTAT=RESU1,
OPTION=('EFGE_ELNO_DEPL','SIPO_ELNO_DEPL','SIGM_ELNO_DEPL',),);
RESU1=CALC_NO(reuse =RESU1,
RESULTAT=RESU1,
OPTION=('REAC_NODA','EFGE_NOEU_DEPL','SIPO_NOEU_DEPL','FORC_NODA',),);
#######################
Me=CALC_MATR_ELEM(OPTION='MASS_MECA',
MODELE=Model,
CHAM_MATER=MatField,
CHARGE=Load,);
Ke=CALC_MATR_ELEM(OPTION='RIGI_MECA',
MODELE=Model,
CHAM_MATER=MatField,
CHARGE=Load,);
NU=NUME_DDL(MATR_RIGI=Ke,);
M=ASSE_MATRICE(MATR_ELEM=Me,
NUME_DDL=NU,);
K=ASSE_MATRICE(MATR_ELEM=Ke,
NUME_DDL=NU,);
MODE=MODE_ITER_SIMULT(MATR_A=K,
MATR_B=M,
CALC_FREQ=_F(OPTION='PLUS_PETITE',
NMAX_FREQ=10,),);
Resul=EXTR_MODE(FILTRE_MODE=_F(MODE=MODE,
NUME_MODE=(1,2,3,4,5,6,7,8,9,10,),),);
IMPR_RESU(MODELE=Model,
FORMAT='MED',
RESU=_F(MAILLAGE=Mesh,
RESULTAT=Resul,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','REAC_NODA','SIPO_NOEU_DEPL','FORC_NODA',),),);
#############
# Write to .med file
IMPR_RESU(MODELE=Model,
FORMAT='MED',
RESU=_F(MAILLAGE=Mesh,
RESULTAT=RESU1,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','REAC_NODA','SIPO_NOEU_DEPL','FORC_NODA',),),);
#Write to .resu file
IMPR_RESU(MODELE=Model,
FORMAT='RESULTAT',
RESU=_F(RESULTAT=RESU1,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','SIPO_NOEU_DEPL','REAC_NODA','SIGM_ELNO_DEPL',),
VALE_MAX='OUI',
VALE_MIN='OUI',),);
FIN();!----------------------------------------------------------------------------------------------------!
! <EXCEPTION> <CALCULEL2_71> !
! !
! on ne trouve pas dans les arguments de la routine CALCUL de champ а associer au parametre: PCAORIE !
! - option: MASS_MECA !
! - !
! type_element: MECA_POU_D_E !
!----------------------------------------------------------------------------------------------------!
!-------------------------------------------------------!
! <EXCEPTION> <DVP_1> !
! !
! Erreur de programmation : condition non respectйe. !
! !
! !
! !
! Il y a probablement une erreur dans la programmation. !
! Veuillez contacter votre assistance technique. !
!----------------------------------------------------------------!
! <A> <CALCULEL3_39> !
! !
! le modиle contient des йlйments de structure !
! il faut probablement utiliser le mot-clй CARA_ELEM. !
! !
! !
! Ceci est une alarme. Si vous ne comprenez pas le sens de cette !
! alarme, vous pouvez obtenir des rйsultats inattendus ! !
!----------------------------------------------------------------!
!----------------------------------------------------------------------------------------------------!
! <EXCEPTION> <CALCULEL2_71> !
! !
! on ne trouve pas dans les arguments de la routine CALCUL de champ а associer au parametre: PCAORIE !
! - option: MASS_MECA !
! - !
! type_element: MECA_POU_D_E !
!---------------------------------------------
!-------------------------------------------------------!
Offline
#4 2012-04-01 22:44:12
- RichardS
- Member
- Registered: 2010-09-28
- Posts: 232
Re: periods and forms of natural vibrations
Hello,
you forgot to use the key word CARA_ELEM in CALC_MATR_ELEM.
Regards,
Richard
Offline
#5 2012-04-02 07:43:13
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
RichardS wrote:
Hello,
you forgot to use the key word CARA_ELEM in CALC_MATR_ELEM.
Regards,
Richard
Thanks, Richard!
I have
new problems
!------------------------------------------------------------------------------!
! <EXCEPTION> <ALGELINE5_49> !
! !
! nombre de valeurs propres convergйes 0 < nombre de frйquences demandйes 10 !
! erreur ARPACK numйro : 1 !
! --> le calcul continue, !
! la prochaine fois !
! --> augmenter DIM_SOUS_ESPACE = 20 !
! --> ou NMAX_ITER_SOREN = 20 !
! --> ou PREC_SOREN = 0.000000 !
!------------------------------------------------------------------------------!
!---------------------------------------------------------------------------!
! <EXCEPTION> <ALGELINE3_78> !
! !
! Aucune valeur propre а la prйcision requise !
! --> augmenter PREC_SOREN ou NMAX_ITER_SOREN ou augmenter DIM_SOUS_ESPACE !
!---------------------------------------------------------------------------!
!-----------------------------------------------------------------------!
! Liste des alarmes йmises lors de l'exйcution du
calcul. !
! !
! Les alarmes que vous avez
choisies d'ignorer sont prйcйdйes de (*). !
! Nombre d'occurrences pour chacune des alarmes : !
! aucune alarme !
!-----------------------------------------------------------------------!
Code:
DEBUT();
#Read mesh
Mesh=LIRE_MAILLAGE(FORMAT='MED',);
Mesh=DEFI_GROUP(reuse =Mesh,
MAILLAGE=Mesh,
CREA_GROUP_MA=_F(NOM='TOUT',
TOUT='OUI',),);
#Assign a beam model - POU_D_E denotes a Euler/Bernoulli
Model=AFFE_MODELE(MAILLAGE=Mesh,
AFFE=_F(TOUT='OUI',
PHENOMENE='MECANIQUE',
MODELISATION='POU_D_E',),);
Material=DEFI_MATERIAU(ELAS=_F(E=66000,
NU=0.3,RHO=1200),);
MatField=AFFE_MATERIAU(MAILLAGE=Mesh,
AFFE=_F(TOUT='OUI',
MATER=Material,),);
A = 27400.0;
I_y = 712000000.0;
I_z = 283000000.0;
J = 6180000.0;
RY = 197;
RZ = 187;
AY = 1.46472;
AZ = 4.64168;
CARA_POU=AFFE_CARA_ELEM(MODELE=Model,
POUTRE=_F(GROUP_MA='TOUT',
SECTION='GENERALE',
CARA=('A','IY','IZ','JX','RY','RZ','AY','AZ',),
VALE=(A,I_y,I_z,J,RY,RZ,AY,AZ,),),);
#Boundary conditions
#Point 1 : Fixed
Hold=AFFE_CHAR_MECA(MODELE=Model,
DDL_IMPO=_F(GROUP_NO='fixx2',
LIAISON='ENCASTRE',),);
#Load
#Point 2 : Point load
Load=AFFE_CHAR_MECA(MODELE=Model,
FORCE_NODALE=_F(GROUP_NO='loadd',
FZ=-10000,),);
# Linear elastic solution
RESU1=MECA_STATIQUE(MODELE=Model,
CHAM_MATER=MatField,
CARA_ELEM=CARA_POU,
EXCIT=(_F(CHARGE=Hold,),
_F(CHARGE=Load,),),);
# Calculate forces etc.
RESU1=CALC_ELEM(reuse =RESU1,
RESULTAT=RESU1,
OPTION=('EFGE_ELNO_DEPL','SIPO_ELNO_DEPL','SIGM_ELNO_DEPL',),);
RESU1=CALC_NO(reuse =RESU1,
RESULTAT=RESU1,
OPTION=('REAC_NODA','EFGE_NOEU_DEPL','SIPO_NOEU_DEPL','FORC_NODA',),);
#######################
Me=CALC_MATR_ELEM(OPTION='MASS_MECA',
MODELE=Model,
CHAM_MATER=MatField,
CARA_ELEM=CARA_POU,
CHARGE=Load,);
Ke=CALC_MATR_ELEM(OPTION='RIGI_MECA',
MODELE=Model,
CHAM_MATER=MatField,
CARA_ELEM=CARA_POU,
CHARGE=Load,);
NU=NUME_DDL(MATR_RIGI=Ke,);
M=ASSE_MATRICE(MATR_ELEM=Me,
NUME_DDL=NU,);
K=ASSE_MATRICE(MATR_ELEM=Ke,
NUME_DDL=NU,);
MODE=MODE_ITER_SIMULT(MATR_A=K,
MATR_B=M,
CALC_FREQ=_F(OPTION='PLUS_PETITE',
NMAX_FREQ=10,),);
Resul=EXTR_MODE(FILTRE_MODE=_F(MODE=MODE,
NUME_MODE=(1,2,3,4,5,6,7,8,9,10,),),);
IMPR_RESU(MODELE=Model,
FORMAT='MED',
RESU=_F(MAILLAGE=Mesh,
RESULTAT=Resul,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','REAC_NODA','SIPO_NOEU_DEPL','FORC_NODA',),),);
#############
# Write to .med file
IMPR_RESU(MODELE=Model,
FORMAT='MED',
RESU=_F(MAILLAGE=Mesh,
RESULTAT=RESU1,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','REAC_NODA','SIPO_NOEU_DEPL','FORC_NODA',),),);
#Write to .resu file
IMPR_RESU(MODELE=Model,
FORMAT='RESULTAT',
RESU=_F(RESULTAT=RESU1,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','SIPO_NOEU_DEPL','REAC_NODA','SIGM_ELNO_DEPL',),
VALE_MAX='OUI',
VALE_MIN='OUI',),);
FIN();Offline
#6 2012-04-10 10:23:10
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
up
Offline
#7 2012-04-10 13:04:27
- Thomas DE SOZA
- Guru
- From: EDF
- Registered: 2007-11-23
- Posts: 2121
Re: periods and forms of natural vibrations
Just follow the advice in the error message :
Code:
! --> augmenter PREC_SOREN ou NMAX_ITER_SOREN ou augmenter DIM_SOUS_ESPACE !
Usually increasing NMAX_ITER_SOREN is enough. If not, then increase DIM_SOUS_ESPACE.
TdS
Offline
#8 2012-04-14 12:11:48
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
Thomas DE SOZA wrote:
Just follow the advice in the error message :
Code:
! --> augmenter PREC_SOREN ou NMAX_ITER_SOREN ou augmenter DIM_SOUS_ESPACE !Usually increasing NMAX_ITER_SOREN is enough. If not, then increase DIM_SOUS_ESPACE.
TdS
Thanks, Thomas.
MODE=MODE_ITER_SIMULT(MATR_A=K,
MATR_B=M,
METHODE='SORENSEN',
## PREC_SOREN=0.000001,
NMAX_ITER_SOREN=80,
CALC_FREQ=_F(OPTION='PLUS_PETITE',
NMAX_FREQ=10,
DIM_SOUS_ESPACE=80,
## COEF_DIM_ESPACE=8,
),);
I have new problems.
!-------------------------------------------------!
! <EXCEPTION> <ALGELINE5_23> !
! !
! pour le concept MODE !
! !
! dans l'intervalle ( -0.010025 , 0.010025 ) !
! il y a thйoriquement 176 frequence(s) !
! et on en a calculй 10 !
!-------------------------------------------------!
!----------------------------!
! <EXCEPTION> <ALGELINE2_74> !
! !
! erreur de vйrification !
!----------------------------!
If I increase NMAX_FREQ=176,
I have many problems
Code:
!----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 98 ! ! ! ! de frequence 0.002285 ! ! ! ! a une norme d'erreur de 0.000001 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 108 ! ! ! ! de frequence 0.002793 ! ! ! ! a une norme d'erreur de 0.000003 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 109 ! ! ! ! de frequence 0.002797 ! ! ! ! a une norme d'erreur de 0.000002 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 110 ! ! ! ! de frequence 0.002797 ! ! ! ! a une norme d'erreur de 0.000003 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 111 ! ! ! ! de frequence 0.002800 ! ! ! ! a une norme d'erreur de 0.000003 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 115 ! ! ! ! de frequence 0.003259 ! ! ! ! a une norme d'erreur de 0.000002 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 116 ! ! ! ! de frequence 0.003260 ! ! ! ! a une norme d'erreur de 0.000004 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 117 ! ! ! ! de frequence 0.003262 ! ! ! ! a une norme d'erreur de 0.000001 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 118 ! ! ! ! de frequence 0.003262 ! ! ! ! a une norme d'erreur de 0.000007 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 121 ! ! ! ! de frequence 0.003556 ! ! ! ! a une norme d'erreur de 0.000011 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------! !----------------------------------------------------------------------------------! ! <EXCEPTION> <ALGELINE5_15> ! ! ! ! pour le concept MODE le mode numйro 122 ! ! ! ! de frequence 0.003556 ! ! ! ! a une norme d'erreur de 0.000008 supйrieure au seuil admis 0.000001 ! ! ! ! Conseil: Si vous utiliser la mйthode 'TRI_DIAG' ou ! ! 'SORENSEN' vous ! ! pouvez amйliorer cette norme en: ! ! - augmentant la valeur de COEF_DIM_ESPACE (par dйfaut valeur 4 pour TRI_DIAG ! ! ! ! et 2 pour SORENSEN), ! ! - rйduire le nombre de valeurs propres recherchйes (NMAX_FREQ ou taille de ! ! la BANDE). ! !----------------------------------------------------------------------------------!
Last edited by tomaiilyk (2012-04-14 17:18:50)
Offline
#9 2012-04-21 12:37:00
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
up
Offline
#10 2012-04-21 16:15:46
- Johannes_ACKVA
- Member
- From: Ingenieurbüro für Mechanik, DE
- Registered: 2009-11-04
- Posts: 322
- Website
Re: periods and forms of natural vibrations
tomaiilyk,
"...a une norme d'erreur de 0.000001 supйrieure au seuil admis 0.000001"
means that the eigenvalue is less precise than requested (Default is SEUIL=1E-06). You can lower this precision:
MODE_ITER_SIMULT(.....
VERI_MODE=_F( . .
STURM='OUI',
SEUIL=1E-04),
Also, the error should not occur, if You renounce on the Sturm, STURM='NON',
Regards Johannes Ackva
______________________________________________________________________
Ingenieurbüro für Mechanik
Dr.-Ing. Johannes Ackva
Markgrafenstr. 21
D 91717 Wassertrüdingen
______________________________________________________________________
next CODE-ASTER-courses
*** Code-Aster QuickStart, 8-9 of May 2012, at Gompute User meeting in Göteborg, Sweden
www.simdi.se
CODE-ASTER-courses at Ingenieurbüro für Mechanik, Germany
*** SALOME and CODE-ASTER for beginners and nearly-beginners
4 days, Wed 19 Sep- Sat 22 Sep 2012
*** DYNAMIC ANALYSIS WITH CODE-ASTER
2 days, Thursday 18 Oct- Fri 19 Okt 2012
www.code-aster.de
Ingenieurbüro für Mechanik
D 91717 Wassertrüdingen / Germany
www.code-aster.de Training & Support for NASTRAN and CODE-ASTER
Offline
#11 2012-04-22 16:57:48
- jeanpierreaubry
- Ex-Guru
- From: nantes (france)
- Registered: 2009-03-12
- Posts: 1717
- Website
Re: periods and forms of natural vibrations
hello
Johannes_ACKVA wrote:
means that the eigenvalue is less precise than requested (Default is SEUIL=1E-06). You can lower this precision:
MODE_ITER_SIMULT(.....
VERI_MODE=_F( . .
STURM='OUI',
SEUIL=1E-04),
Also, the error should not occur, if You renounce on the Sturm, STURM='NON',
another work around is
Code:
VERI_MODE=_F(
STOP_ERREUR='NON',
),jean pierre aubry
Last edited by jeanpierreaubry (2012-04-22 16:58:41)
Offline
#12 2012-04-24 19:20:50
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
Thanks! Some questions about result.
How can be negative result of frequence? What physical meaning?
NUMERO FREQUENCE (HZ) NORME D'ERREUR
5 0.00000E+00 0.00000E+00
4 -4.44674E-10 7.10857E-20
3 -6.28864E-10 1.48138E-19
6 7.10860E-10 2.63168E-19
2 -1.05854E-09 3.40535E-19
1 -1.13853E-09 3.18442E-19
7 6.78576E-06 1.32313E-11
8 6.04989E-05 1.36749E-09
9 6.05101E-05 1.78640E-09
10 6.08722E-05 1.49796E-09
11 6.08722E-05 2.28594E-09
12 6.84768E-05 2.10293E-09
13 1.22776E-04 4.06290E-09
14 1.22776E-04 5.10838E-09
15 1.23146E-04 5.83950E-09
16 1.23504E-04 4.89884E-09
17 1.28561E-04 2.97486E-09
18 1.79621E-04 6.14595E-09
19 1.79621E-04 5.01659E-09
20 1.80703E-04 9.49856E-09
21 1.82854E-04 5.92908E-09
22 1.85906E-04 9.98350E-09
23 1.88662E-04 8.27244E-09
24 1.89363E-04 1.29534E-08
25 1.89363E-04 9.17185E-09
26 2.05922E-04 1.22786E-08
27 2.48543E-04 1.08941E-08
28 2.48613E-04 8.85719E-09
29 2.54975E-04 1.49844E-08
30 2.55026E-04 1.86272E-08
31 2.61026E-04 1.81095E-08
32 2.61148E-04 2.19163E-08
33 2.78420E-04 1.77250E-08
34 2.78601E-04 2.16955E-08
35 2.82380E-04 1.75706E-08
36 3.27681E-04 2.41488E-08
37 3.39389E-04 3.78929E-08
38 3.39389E-04 3.82463E-08
39 3.40190E-04 3.26992E-08
40 3.54054E-04 2.78621E-08
41 4.23283E-04 5.72370E-08
42 4.23293E-04 5.56193E-08
43 4.24457E-04 3.91431E-08
44 4.24460E-04 4.49572E-08
45 5.06512E-04 4.12881E-08
46 5.06519E-04 6.67597E-08
47 5.07123E-04 9.13207E-08
48 5.07719E-04 8.90278E-08
49 5.31545E-04 2.62971E-08
50 5.46698E-04 3.41461E-08
Offline
#13 2012-04-25 01:16:06
- Johannes_ACKVA
- Member
- From: Ingenieurbüro für Mechanik, DE
- Registered: 2009-11-04
- Posts: 322
- Website
Re: periods and forms of natural vibrations
Your frequencies are not negative but 'numerical zero'. Your system has as many rigid body modes (or mechanism-degrees-of-freedom) as You have zero-eigenfrequencies,
Regards Johannes Ackva
______________________________________________________________________
Ingenieurbüro für Mechanik
Dr.-Ing. Johannes Ackva
Markgrafenstr. 21
D 91717 Wassertrüdingen
______________________________________________________________________
next CODE-ASTER-courses
*** Code-Aster QuickStart, 8-9 of May 2012, at Gompute User meeting in Göteborg, Sweden
www.simdi.se
CODE-ASTER-courses at Ingenieurbüro für Mechanik, Germany
*** SALOME and CODE-ASTER for beginners and nearly-beginners
4 days, Wed 19 Sep- Sat 22 Sep 2012
*** DYNAMIC ANALYSIS WITH CODE-ASTER
2 days, Thursday 18 Oct- Fri 19 Okt 2012
www.code-aster.de
Ingenieurbüro für Mechanik
D 91717 Wassertrüdingen / Germany
www.code-aster.de Training & Support for NASTRAN and CODE-ASTER
Offline
#14 2012-06-09 18:46:21
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
As a result of calculations I got the right values of the frequencies coinciding with rhe theoretical values/ But the forms of the vibrations and the Ansys forms did not match together ? and they have wrong physical sense- steady ends of the beam are dislocated.
What' wrong?
files https://docs.google.com/open?id=0B9BlA0 … VN6TUoxd1U
Code:
#Units in mm, MPa, N
DEBUT();
#Read mesh
Mesh=LIRE_MAILLAGE(FORMAT='MED',);
Mesh=DEFI_GROUP(reuse =Mesh,
MAILLAGE=Mesh,
CREA_GROUP_MA=_F(NOM='TOUT',
TOUT='OUI',),);
#Assign a beam model - POU_D_E denotes a Euler/Bernoulli
Model=AFFE_MODELE(MAILLAGE=Mesh,
AFFE=_F(TOUT='OUI',
PHENOMENE='MECANIQUE',
MODELISATION='POU_D_E',),);
Material=DEFI_MATERIAU(ELAS=_F(E=66000000000,
NU=0.3,RHO=2700),);
MatField=AFFE_MATERIAU(MAILLAGE=Mesh,
AFFE=_F(TOUT='OUI',
MATER=Material,),);
A = 0.0001;
I_y = 8.3E-10;
I_z = 8.3E-10;
J = 14E-10;
RY = 0.005;
RZ = 0.005;
AY =1.5;
AZ =1.5 ;
CARA_POU=AFFE_CARA_ELEM(MODELE=Model,
POUTRE=_F(GROUP_MA='TOUT',
SECTION='GENERALE',
CARA=('A','IY','IZ','JX','RY','RZ','AY','AZ',),
VALE=(A,I_y,I_z,J,RY,RZ,AY,AZ,),),);
#Boundary conditions
#Point 1 : Fixed
Hold=AFFE_CHAR_MECA(MODELE=Model,
DDL_IMPO=_F(GROUP_NO='fixx2',
DX=0.0,
DY=0.0,
DRY=0.0,
DRZ=0.0,
DRX=0.0,
DZ=0.0,),);
#Load
#Point 2 : Point load
Load=AFFE_CHAR_MECA(MODELE=Model,
FORCE_NODALE=_F(GROUP_NO='loadd',
FZ=0.0,),);
# Linear elastic solution
RESU1=MECA_STATIQUE(MODELE=Model,
CHAM_MATER=MatField,
CARA_ELEM=CARA_POU,
EXCIT=(_F(CHARGE=Hold,),
_F(CHARGE=Load,),),);
# Calculate forces etc.
RESU1=CALC_ELEM(reuse =RESU1,
RESULTAT=RESU1,
OPTION=('EFGE_ELNO_DEPL','SIPO_ELNO_DEPL','SIGM_ELNO_DEPL',),);
RESU1=CALC_NO(reuse =RESU1,
RESULTAT=RESU1,
OPTION=('REAC_NODA','EFGE_NOEU_DEPL','SIPO_NOEU_DEPL','FORC_NODA',),);
#######################
Me=CALC_MATR_ELEM(OPTION='MASS_MECA',
MODELE=Model,
CHAM_MATER=MatField,
CARA_ELEM=CARA_POU,
CHARGE=Load,);
Ke=CALC_MATR_ELEM(OPTION='RIGI_MECA',
MODELE=Model,
CHAM_MATER=MatField,
CARA_ELEM=CARA_POU,
CHARGE=Load,);
NU=NUME_DDL(MATR_RIGI=Ke,);
M=ASSE_MATRICE(MATR_ELEM=Me,
NUME_DDL=NU,);
K=ASSE_MATRICE(MATR_ELEM=Ke,
NUME_DDL=NU,);
MODE=MODE_ITER_SIMULT(MATR_A=K,
MATR_B=M,
METHODE='SORENSEN',
# PREC_SOREN=0.00005,
NMAX_ITER_SOREN=80,
VERI_MODE=_F(PREC_SHIFT=5.0000000000000001E-3,
STOP_ERREUR='OUI',
STURM='OUI',
SEUIL=1E-04),
CALC_FREQ=_F(OPTION='BANDE',
FREQ=(0.00001,100000,),
# DIM_SOUS_ESPACE=1,
# COEF_DIM_ESPACE=20,
),);
Resul=EXTR_MODE(FILTRE_MODE=_F(MODE=MODE,
NUME_MODE=(1,2,3,4,5,6,7,8,9,10,11,12,13,14,15,),),);
IMPR_RESU(MODELE=Model,
FORMAT='MED',
RESU=_F(MAILLAGE=Mesh,
RESULTAT=Resul,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','REAC_NODA','SIPO_NOEU_DEPL','FORC_NODA',),),);
#############
# Write to .med file
#IMPR_RESU(MODELE=Model,
# FORMAT='MED',
# RESU=_F(MAILLAGE=Mesh,
# RESULTAT=RESU1,
# NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','REAC_NODA','SIPO_NOEU_DEPL','FORC_NODA',),),);
#IMPR_RESU(FORMAT='GMSH',
# UNITE=38,
# RESU=_F(RESULTAT=RESU1,
# TOUT_ORDRE='OUI',),);
#Write to .resu file
IMPR_RESU(MODELE=Model,
FORMAT='RESULTAT',
RESU=_F(RESULTAT=Resul,
NOM_CHAM=('DEPL','EFGE_NOEU_DEPL','SIPO_NOEU_DEPL','REAC_NODA','SIGM_ELNO_DEPL',),
VALE_MAX='OUI',
VALE_MIN='OUI',),);
FIN();Why dz,dx for N1 N2 <>0 ?
NOEUD DX DY DZ DRX DRY DRZ
N1 -2.15180E-01 2.95060E-10 -1.63310E-01 7.58946E-01 5.48746E-09 -1.00000E+00
N2 -2.15180E-01 2.95016E-10 -1.63310E-01 -7.58946E-01 6.50853E-09 1.00000E+00
Last edited by tomaiilyk (2012-06-10 13:54:17)
Offline
#15 2012-06-10 21:12:13
- Johannes_ACKVA
- Member
- From: Ingenieurbüro für Mechanik, DE
- Registered: 2009-11-04
- Posts: 322
- Website
Re: periods and forms of natural vibrations
tomaiilyk wrote:
I got the right values of the frequencies coinciding with rhe theoretical values;
OK. So also the mode shapes of Ansys and Code-Aster should be the same.
tomaiilyk wrote:
But the forms of the vibrations and the Ansys forms did not match together ? and they have wrong physical sense- steady ends of the beam are dislocated
I do not completely understand what You mean, I just try to give some hints:
(1) You did not add the boundary condition Hold=AFFE_CHAR_MECA to the calc of Your elm matrices for the modal analysis. So the modal analysis is done for an unconstrained structure, no node is fixed to zero.
(2) modal shapes are scalable. Multiplying a modal shape with any factor unequal zero means the same modal shape. So the sign of the shape from Ansys and Code-Aster can be different.
For You next contribution: could You please post the .mess-file instead of the .comm-file? Because it contains informations which make it easier to see problems in You Code-Aster-run,
Regards Johannes Ackva
______________________________________________________________________
Ingenieurbüro für Mechanik
Dr.-Ing. Johannes Ackva
Markgrafenstr. 21
D 91717 Wassertrüdingen
______________________________________________________________________
CODE-ASTER-courses at Ingenieurbüro für Mechanik, Germany
*** SALOME and CODE-ASTER for beginners and nearly-beginners
4 days, Wed 19 Sep- Sat 22 Sep 2012
*** DYNAMIC ANALYSIS WITH CODE-ASTER
2 days, Thursday 18 Oct- Fri 19 Okt 2012
www.code-aster.de
Ingenieurbüro für Mechanik
D 91717 Wassertrüdingen / Germany
www.code-aster.de Training & Support for NASTRAN and CODE-ASTER
Offline
#16 2012-06-28 13:40:33
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
Thanks ,Johannes. Another question. If I have multiple beams fastened together what modelisation should I use and how calculate ('A','IY','IZ','JX','RY','RZ','AY','AZ',) for each of them ?
Johannes_ACKVA wrote:
Last edited by tomaiilyk (2012-06-28 13:42:13)
Offline
#17 2012-07-14 19:07:22
- tomaiilyk
- Member
- Registered: 2009-10-22
- Posts: 64
Re: periods and forms of natural vibrations
Up!
Offline
