Difference between revisions of "Contrib:KeesWouters/shell/plotcoq3d"

Revision as of 17:43, 27 April 2013

Post processing of COQUE-3D calcalation

[under construction]

In this contribution the main (and only) focus is on the postprocessing of the displacements and stresses of shell COQUE-3D elements. The centre nodes of tria7 and quad9 elements used for the discription of the displacements field of COQUE_3D poses some nasty problems in the postprocessing with Salome. To overcome this problem the results are projected on the original quadratic mesh without the centre node.

Definition of the geometry

This time the geometry has been drawn in FreeCAD. It is good enough at this moment (april 2013) to draw some more or less complex geometry, although, in this case, it wouldnot have been much more effort to construct it in Salome. Anyway, I import the brep geometry from FreeCAD into Salome and mesh it there. It is a planar shell with four holes. Main dimensions are Length x Width = 100 x 50. The holes with diameter of 6 are centred along the short centre line of have offset along the long centre line, see picture below. The thickness is defined in the Code Aster *.comm file and can be changed any time: thickness th = 0.02.
As usual no explicit dimensions are used here. But units have to be consistent and will be if you imagine:

• length and displacments [m]
• forces [N] and moments [Nm] and
• Youngs' modulus and stresses [Pa]

Boundary conditions and loads:

• all dof fixed on short side Lxm:
  • (DX=0.0, DY=0.0, DZ=0.0, DRX=0.0, DRY=0.0, DRZ=0.0)
    
• 2 'loads': prescribed in-plane x displacement or out-out-of-plane vertical displacement fixed on short side Lxp:
  • (DZ=Zdisp) or
    
  • (DX=Xdisp)
    

Material:
Material steel

• E = 210e9 Pa
• Nu = 0.28
• rho = 7850 kg/m3 (not needed)

*

A rough discription of the Code-Aster commands

The general flow is as follows:

1. initialise
2. import the initial mesh (initMesh)
3. create a modified mesh (modiMesh)
   • create COQUE_3D elements with centre nodes
   • orient all element in the same direction
4. creaste models with both meshes: iniModel and modModel
5. define Coque_3d characteristics (thickness on group shell)
6. define material (steel)
7. aplly boundary conditions
8. main calculation: RESU=MECA_STATIQUE(...)
9. post process the result RESU:
   • create displacement and stress fields for modified model: CALC_CHAMP
   • create displacement and stress fields for modified model at bottom, centre and top layer: POST_CHAMP
   • create displacement and stress fields for initial model at bottom, centre and top layer: PROJ_CHAMP. This last step is required to remove the data at the centre nodes that Salome is unable to coop with.
   • print results of modified and initial model (results of the modified model are only printed to show that they are not fully what you expect)

Steps 1 to 8 are fairly standard and are not descript in more detail here. We will concentrate on step 9). The stresses can be provided at the top, the centre and the bottom of the shell plane. These layers are denoted by 'SUP', 'MOY', and 'INF' in Code-Aster (superieur, moyenne et inferieur je pense) and depends on the normal vector of the shell elements (see step 3 in the general flow). These can be changed by the ORIENT command. In the next part all the commands could be given for the three layers, but it has been described here only for 'SUP' to keep it tidier. In the *.comm file at the end the complete command file can be downloaded with all layers excecuted.

Calculate the mechanical behaviour of the structure

#main calculation
RESU=MECA_STATIQUE(MODELE=cocModel,
                    CHAM_MATER=material,
                    CARA_ELEM=shellch,
                    OPTION=('SIEF_ELGA'),   ##'SIEF_ELGA','DEPL','SICO_ELNO','SIGM_ELNO','SIEQ_ELNO'
                    EXCIT=(_F(CHARGE=clamped),
                           _F(CHARGE=ApplyPr),),);

Extracting the stresses of the coque_3d model

RESU=CALC_CHAMP(reuse =RESU,
               RESULTAT=RESU,
               CONTRAINTE=('SIEF_ELNO','EFGE_NOEU','EFGE_ELNO',),
               CRITERES='SIEQ_ELNO',
               EXCIT=(_F(CHARGE=clamped),
                      _F(CHARGE=ApplyPr),),);

Extracting the stresses of the coque_3d model on layers

SIEQ_SUP=POST_CHAMP(RESULTAT=RESU,
                   EXTR_COQUE=_F(NOM_CHAM='SIEQ_ELNO',
                                 NUME_COUCHE=1,
                                 NIVE_COUCHE='SUP',),);

SIEF_SUP=POST_CHAMP(RESULTAT=RESU,
                   EXTR_COQUE=_F(NOM_CHAM='SIEF_ELNO',
                                 NUME_COUCHE=1,
                                 NIVE_COUCHE='SUP',),);

SIEQ_SUP=CALC_CHAMP(reuse =SIEQ_SUP,
                   RESULTAT=SIEQ_SUP,
                   CRITERES='SIEQ_NOEU',);

SIEF_SUP=CALC_CHAMP(reuse =SIEF_SUP,
                   RESULTAT=SIEF_SUP,
                   CONTRAINTE='SIEF_NOEU',);

IMPR_RESU(FORMAT='MED',
         UNITE=80,
         RESU=(_F(RESULTAT=RESU,),
               _F(RESULTAT=SIEQ_SUP,),
               _F(RESULTAT=SIEQ_MOY,),
               _F(RESULTAT=SIEQ_INF,),
               _F(RESULTAT=SIEF_SUP,),
               _F(RESULTAT=SIEF_MOY,),
               _F(RESULTAT=SIEF_INF,),),);

Extracting the stresses of the initial model on layers

QSUP_INI=PROJ_CHAMP(RESULTAT=SIEQ_SUP,
                   MODELE_1=cocModel,    # project fields of this model to
                   MODELE_2=iniModel,); # field of model_2

FSUP_INI=PROJ_CHAMP(RESULTAT=SIEF_SUP,
                   MODELE_1=cocModel,    # project fields of this model to
                   MODELE_2=iniModel,); # field of model_2

initRes=PROJ_CHAMP(RESULTAT=RESU,
                   MODELE_1=cocModel,    # project fields of this model to
                   MODELE_2=iniModel,); # field of model_2

IMPR_RESU(FORMAT='MED',
         UNITE=81,
         RESU=(_F(RESULTAT=initRes,NOM_CHAM=('DEPL'),),
               #_F(MAILLAGE=initMesh,RESULTAT=RESU,NOM_CHAM=('DEPL'),),
               _F(RESULTAT=QSUP_INI,),
               _F(RESULTAT=QMOY_INI,),
               _F(RESULTAT=QINF_INI,),
               _F(RESULTAT=FSUP_INI,),
               _F(RESULTAT=FMOY_INI,),
               _F(RESULTAT=FINF_INI,),),);

IMPR_RESU(FORMAT='MED',
         UNITE=82,
         RESU=(_F(RESULTAT=initRes),),);

FIN();

Results of Ux displacement

The load is a displacement of 0.1 in x direction. The calculated Ux displacement (overlayed with the mesh in undeformed state) and the von Mises stresses in the centre layer are shown in the following pictures.
*

Results of pressure load

In the picture below the vector displacement due to a pressure of 1 bar (1e5 Pa) is shown. Note that this is quite an unrealistic case, as the displacements are far too big.

The next pictures show the von Mises and Sxx stresses in the top, centre and bottom layer of the shell. In the picture the centre stress is translated 55 in y direction and the bottom stress is translated 2*55 units. The von Mises stresses in the top and bottom layer are equal. In the centre layer the stress is practically zero. This is what we expect for a shell under pressure.
The stress component Sxx has different sign in the top layer compared to the bottom layer. Again, the centre layer stress is zero.