4. B modeling#
4.1. 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.
4.2. 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 \(270\mathit{MPa}\)): 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.
4.3. Tested sizes and results#
Value of the stress components (SIGM_NOEU) with the initial mesh and after an adaptation:
Mesh |
Location |
Identification |
Reference (Analytics) |
Tolerance |
1 |
Node \(B\) |
Constraint \(\mathrm{SIYY}\) |
303.0 |
|
1 |
Node \(A\) |
Constraint \(\mathit{SIXX}\) |
-100.0 |
|
2 |
Node \(B\) |
Constraint \(\mathrm{SIYY}\) |
303.0 |
|
2 |
Node \(A\) |
Constraint \(\mathit{SIXX}\) |
-100.0 |
|
These tests on analytical values are supplemented by non-regression tests.