B modeling
====


Workflow of the TP
----

The aim is to implement mesh adaptation following an elastic calculation.

We will therefore start again with the study carried out during modeling A.


Mesh adaptation
----

After launching the AsterStudy module, we modify the command file to add the calculation of the error indicator:


*   Add error results with the CALC_ERREUR command in the Post Processing category: choose option ERME_ELEM using reuse.


*   Restart the calculation.

To visualize the constraint and error fields (component ERREST, total error), you can perform post-processing in the Results tab (highly recommended) or in the ParAvis module. The steps in the ParaVis module are as follows:


*   Check the fields to be displayed to load them before applying GenerateVectors: SIEF_ELGA, ERME_ELEM


*   To visualize the component SIYYdu field SIEF_ELGA, especially at the edge of the hole: Menu Filters → Mechanics → ELGA field To Surface and switch to Surface With Edges representation. To find the position of the maximum value (in the order of :math:`270\mathit{MPa}`): Edit → Find Data menu: Edit → Find Data and choose the Cells option in the field created ELGAfieldToSurface, select SIEF_ELGA_Vector (1) representing SIYY and the formula is max.


*   Visualize the error indicator map (field ERME_ELEM, component ERREST, total error).

We go back to the AsterStudy module, we modify the command file to perform a mesh adaptation and then directly calculate the new error indicator value:


*   Post Processing category/command MACR_ADAP_MAIL for a RAFFINEMENT mesh adaptation: name the new mesh by MAILLAGE_NP1 = MAIL2, select the element criterion (option CRIT_RAFF_PE) at 10% for the adaptation parameter: RESULTAT_IN/NOM_CHAM = ERME_ELEM/its component NOM_CMP = ERREST.


*   Then string together the commands AFFE_MODELE, AFFE_MATERIAU, AFFE_CHAR_MECA,, MECA_STATIQUE,, CALC_CHAMP and CALC_ERREUR on this new mesh MAIL2 (Duplicate the commands by modifying the mesh and other relevant terms).**Caution**: The concept names in these commands should not be the same as before, and they should not exceed 8 characters in length.


*   Print the new calculation results in format MED: Command IMPR_RESU.


*   Start the calculation.

To visualize the constraint and error fields, you can perform post-processing in the Results tab (highly recommended) or in the ParAvis module.


Tested sizes and results
----

Value of the stress components (SIGM_NOEU) with the initial mesh and after an adaptation:


.. csv-table::

    "**Mesh**", "**Location**", "**Identification**", "**Reference (Analytics)**", "**Tolerance**"
    "1", "Node :math:`B` ", "Constraint :math:`\mathrm{SIYY}` ", "303.0"," 5.0%"
    "1", "Node :math:`A` ", "Constraint :math:`\mathit{SIXX}` ", "-100.0"," 15.0%"
    "2", "Node :math:`B` ", "Constraint :math:`\mathrm{SIYY}` ", "303.0"," 2.0%"
    "2", "Node :math:`A` ", "Constraint :math:`\mathit{SIXX}` ", "-100.0"," 3.0%"


These tests on analytical values are supplemented by non-regression tests.