# Contrib:KeesWouters/shell/plotcoq3d

## Contents

**Post processing of COQUE-3D results**

This contribution is only usefull for Code-Aster version 11.3 (maybe earlier version as 11.1 and 11.2 but certainly no previous releases).

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 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 assume:

- length and displacements [m]
- forces [N] and moments [Nm] and
- Youngs' modulus and stresses [Pa]

**Boundary conditions and loads:**

Two loads and boundary conditions have been applied:

- all DOFs fixed on short side Lxm and a prescribed in-plane x displacement on other short side end:
- on short side Lxm: DX=0.0, DY=0.0, DZ=0.0, DRX=0.0, DRY=0.0, DRZ=0.0
- o short side Lxp: DX=Xdisp

- on short side Lxm: DX=0.0, DY=0.0, DZ=0.0, DRX=0.0, DRY=0.0, DRZ=0.0
- all DOFs fixed on short sides Lxm, DZ at Lxp and out-out-of-plane pressure load:
- on short side Lxm: DX=0.0, DY=0.0, DZ=0.0, DRX=0.0, DRY=0.0, DRZ=0.0
- on short side Lxp: DZ=0.0 and
- pressure on shell area p=1e5 (imagine 1 bar))

- on short side Lxm: DX=0.0, DY=0.0, DZ=0.0, DRX=0.0, DRY=0.0, DRZ=0.0

**Material:**

Material steel

**A rough discription of the Code-Aster commands**

The general flow is as follows:

- initialise
- import the initial mesh (initMesh)
- create a modified mesh (modiMesh)
- create COQUE_3D elements with centre nodes
- orient all element in the same direction

- creaste models with both meshes: iniModel and modModel
- define Coque_3d characteristics (thickness on group
*shell*) - define material (steel)
- aplly boundary conditions
- main calculation: RESU=MECA_STATIQUE(...)
- 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 equivalent fields for modified model at bottom, centre and top layer: CALC_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.

**Short description of CALC_CHAMP, POST_CHAMP and PROJ_CHAMP**

We will use the commands CALC_CHAMP, POST_CHAMP and PROJ_CHAMP several times. Now a short description from the C-A-documentation is given:

- Short description of CALC_CHAMP, from U4.81.04.pdf:
- Create or supplement a result by computing fields by element or with the nodes (forced, strains, ...). The produced result concept either is created, or modified, i.e. the call to CALC_CHAMP is done in the following way:
- resu = CALC_CHAMP(RESULTAT = resu..., reuse = resu,...), or
- resu1 = CALC_CHAMP(RESULTAT = resu,...)

- this last means that POST_CHAMP returns and extend its original field (resu) or create a new field (resu1). POST_CHAMP is not re-entrance.

- Create or supplement a result by computing fields by element or with the nodes (forced, strains, ...). The produced result concept either is created, or modified, i.e. the call to CALC_CHAMP is done in the following way:

- Short description of POST_CHAMP, from U4.81.05.pdf:
- specific Post-processing for the structural elements (shells, beams,...):
- extraction of a field for a subpoint
- computation of the minimum/maximum on all of the subpoints of a point taken into account of the eccentring of the plates for computation of the force

- Short description of PROJ_CHAMP, from U4.72.05.pdf:
- the goal of the operator is to project the fields of a data structure result on another mesh. Eg. this command can be used to transfer the result of a thermal computation carried out on a “thermal” mesh to a different "mechanical" mesh. [In this case we want to get rid of the centre node of the coque-3d mesh that carries no displacements and just carry out a mechanical to mechanical projection.]

The normal direction of the shell can be easily verified by

- selecting the group of faces
*shell*in the mesh module - in the VTK viewer right click and
- select
*orientation of the Faces*- see figure below

**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**

Use the commands POST_CHAMP and again CALC_CHAMP to extract the local stresses Sxx, Syy, Szz, Sxy, Sxz and Syz and the equivalent stresses (VMIS, S1, S2, S3,TRESCA) from the result RESU issued in the previous command: SIEQ_SUP (equivalent stresses) and SIEF_SUP. POST_CHAMP only retrieves the local stresses (to be checked) and the subsequent CALC_CHAMP retrieves the equivalent stresses (to be checked). Note the all commands can be extended for the centre (MOY) and bottom (INF) layer additional to the top layer (SUP) shown here. Finally the retrieved stresses and displacements are written to file (IMPR_RESU, all layers are choosen, add additionnal POST_CHAMP and CALC_CHAMP for the others layers if you want to use this).

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',); # ...... # add SIEF/EQ_MOY, SIEF/EQ_INF # ......

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,),),);

**Mapping the stresses to layers of the initial model**

Alright, when using Salome the above results are disappointing (you may check the file written to unit 80 above, but be warned). To get really nice picture (and that is what FEM is all about, isnot it?) we have to get ride of the centre node of the mesh node. That is now fairly easy: project the results from the coque_3d model to the initial model by using PROJ_CHAMP. Then check the file written to unit 81, et voila, nice pictures. *Unit*e 82 is there to show that displacements and forces are written to the file by default.

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();

That's about it. Except for saying grace to TdS, jeanpierreaubry and Theobolt for asking and supplying help in the C-A-forum: [Stresses from COQUE_3D and DKT elements]

**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 total displacement (sum, vector) due to a pressure of 1 bar (1e5 Pa) is shown. Note that this is quite an unrealistic case wrt to load parameters.

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 (green axis) 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.

**Input files for the FE Analysis and references**

Input files:

- FreeCAD geometry file plane4holes.brep
- Python script for defining the geometry and mesh (kw_plane_geom_mesh_v06.py), load by File --> load script (cntrl T in the object browser), refresh (F5) after running

- the mesh file
*Mshell*will be saved by the previous script

- the mesh file
- ASTK file (shellist_v22.astk, you need to edit the path and filenames to your requirements ...)
- command file (shell_static_v26.comm)

Download the files here:

References:

[manuel CALC_CHAMP]

[manuel POST_CHAMP]

[manuel PROJ_CHAMP *french*]

[forum: Stresses from COQUE_3D and DKT elements]

April 2013 Enjoy - kees