Modeling A: FEM 3D
====


Workflow of the TP
----


Meshing
~~~~

The quadratic mesh of the structure is provided in format MED: forma07a.mmed. Taking into account some symmetries of the problem, only a quarter of the structure is represented. We could only represent :math:`1\mathrm{/}{8}^{\mathit{ème}}` of the structure. The mesh was generated with the GIBI software, and tori are defined around the crack bottom:


*   radius of the smallest torus: :math:`\mathrm{0,12}m`,


*   radius of the largest torus: :math:`\mathrm{0,53}m`.


    .. image:: images/100000000000053F000004190B4A398D53CDC10F.png
        :width: 5.5945in
        :height: 4.3701in


    .. _RefImage_100000000000053F000004190B4A398D53CDC10F.png:

FACE_SUP

FACE_AV
**Figure** 3.1.1-a **: Mesh**

FACE_INF

FACE_LAT
The middle nodes of the edges of the elements touching the bottom of the crack are moved to a quarter of these edges.


Creating the batch file without post-processing the break
~~~~

.. csv-table::

    "Start Salome_Meca, then choose the AsterStudy module. Add the following steps to your case:"
    "**Read a mesh** (**LIRE_MAILLAGE**). Select the forma07a.mmed mesh and the MED" format
    "**Modify a mesh** (**MODI_MAILLAGE**). Choose the mesh read earlier and select reuse. Select the ORIE_PEAU_3Dpour action to reorient the normals to the faces outside of the mesh (element groups FACE_AV, FACE_LAT, FACE_SUP, FACE_INF, LEV_INF, and LEV_SUP)."
    "Assign finite element (AFFE_MODELE). Choose the mechanical phenomenon and the modeling of 3D continuous media (3D)"
    "Material definition and assignment: **Define a material (** **DEFI_MATERIAU** ****) **)** and **Assign a material (** **AFFE_MATERIAU** **** **)**) **"
    "Definition of limit conditions and loads: **Assign mechanical load** **** **(** **AFFE_CHAR_MECA** **)**:
    *   Symmetry on the symmetry plane 'FACE_LAT' (Enforce DOF);
    *   Symmetry on the symmetry plane 'FACE_AV' (Enforce DOF);
    *   Blocking rigid modes (Enforce DOFsur the GROUP_NO 'D');
    *   Applying traction on 'FACE_SUP' and 'FACE_INF' (PRES_REP)"
    "Elastic problem solving: **Static mechanical analysis** **** (**** MECA_STATIQUE **);"
    "For visualization with Paravis:
    *   Calculation of the extrapolated constraint field to the nodes (CALC_CHAMP, option 'CONTRAINTE' with the field 'SIGM_NOEU')
    *   Calculation of the equivalent stress field (CALC_CHAMP, option 'CRITERES' with the field 'SIEQ_NOEU')
    To do this, we will enrich the concept resulting from MECA_STATIQUE by using the same concept name."
    "Printing results in format MED: Results output (IMPR_RESU)."
    "Visualize the displacement fields and constraints obtained in Paravis"



Post-treatment for breakup
~~~~

.. csv-table::

    "In order to separate calculation and post-processing, you can add a new stage to your case study."
    "**Define the crack bottom** **(** **DEFI_FOND_FISS** ****) .** Define the crack background in DEFI_FOND_FISSà from the mesh group at the bottom LFFet the lips LEV_INFet LEV_SUP."
    "**Calculation of** **G** **** and****K****with with**** CALC_G ** (OPTION =( 'G', 'K'))).
    Complete the information on field THETA:
    *   the description of the crack using the keyword FISSURE
    *   the radii of the crown of the theta field (R_INF, R_SUP) (,), to be defined according to the mesh used.
    Print G values (IMPR_TABLE)."
    "**Calculation** **of** **K and G with** POST_K1_K2_K3:
    *   fill in the bottom of the crack
    *   fill in the ABSC_CURV_MAXI parameter
    *   print the results in a table (IMPR_TABLE)"
    "Plot the values of G and K1 from CALC_Get from POST_K1_K2_K3 as a function of the curvilinear abscissa of the crack front (column 'ABSC_CURV') in a spreadsheet."



****
    *


To go further: Study of the influence of 3D discretization
~~~~

In CALC_G, enter the keyword DISCRETISATION of the keyword factor THETA with the keywords to the value LEGENDRE Compare the values with those obtained previously. As a reminder, when DISCRETISATION is not entered, its value by default is LINEAIRE.

In a second step, add the keyword NB_POINT_FOND =5 to the keyword factor THETAà the discretization LINEAIRE and observe the values of G or K1 along the front. Also compare the calculation times of CALC_G with and without NB_POINT_FOND entered.


Tested sizes and results
----


.. csv-table::

    "**Identification**", "**Reference**", "**% tolerance**"
    ":math:`{K}_{I}` of POST_K1_K2_K3 ", "1.5957 106"," 0.8%"