Modeling A ==== Workflow of the TP ---- Geometry and meshing with Salome-Meca ~~~~ Under Salomé-Méca, realize the geometry. We can consider a plate centered at the origin, with a finite dimension: :math:`2m` on the side. Make the mesh. Remember that cracks are not meshed, so it is possible to use a regulated mesh of quadrangles that is sufficiently fine everywhere (1D algorithm = Wire discretization + 2D algorithm = Quadrangle). Creating the command file without post-processing the break ~~~~ Reading the healthy mesh and defining the non-enriched model ^^^^ .. csv-table:: "Reading the refined mesh (LIRE_MAILLAGE) in MED format;" "Definition of the finite elements used (AFFE_MODELE, MODELISATION =' D_PLAN ');" "Reorientation of the normals to the elements: we will use MODI_MAILLAGE/ORIE_PEAU_2Dpour to orient all the elements in the same way, with a normal turned towards the outside for the faces on which the load is applied;" Definition of the crack and the elements X- FEM ^^^^ .. csv-table:: "Definition of a single horizontal crack of length :math:`\mathrm{2a}\mathrm{=}\mathrm{0,3}m` (DEFI_FISS_XFEM): preferably use the crack catalog (FORM_FISS =' SEGMENT ')" "Modifying the model to take into account the elements X- FEM (MODI_MODELE_XFEM)," Definition of the material, the conditions and the resolution of the mechanical problem ^^^^ .. csv-table:: "Material definition and assignment (DEFI_MATERIAU and AFFE_MATERIAU);" "Definition of limit conditions and loads (AFFE_CHAR_MECA) on the enriched model: * Blocking rigid modes (DDL_IMPOsur the GROUP_NO 'N_A', 'N_B'); * Applying traction (1 MPa) on 'M_up' and 'M_down' (PRES_REP)" "Solving the elastic problem (MECA_STATIQUE) on the rich model." Post-processing of movements and constraints with X- FEM and visualization with Paravis ^^^^ .. csv-table:: "Creating a visualization mesh (POST_MAIL_XFEM);" "Creating a model for visualization (AFFE_MODELE) on the mesh created for visualization;" "Creation of a results field on the X- FEM visualization mesh (POST_CHAM_XFEM);" "Print results in MED (IMPR_RESU) format." Complete the order file created by taking into account 2 cracks, in the following case: :math:`a\mathrm{=}\mathrm{0,15}` and :math:`b\mathrm{=}\mathrm{0,4}` (i.e. :math:`2a\mathrm{/}b\mathrm{=}\mathrm{0,75}`) :math:`e\mathrm{=}0` It is reminded that every call DEFI_FISS_XFEM produces a crack. For 2 cracks, you have to call this command twice. Add break post-processing to the command file ~~~~ 1. **Calculating K with CALC_G** Calculate the stress intensity factor (K1) (OPTION =' CALC_K_G '). Use the result of MECA_STATIQUE (RESULTAT). Complete the information on field THETA: * the crack bottom, specifying the bottom number (in your case there are 2 crack bottoms A and B) * the radii of the crown of the theta field (R_INF, R_SUP), to be defined according to the mesh used. The CALC_Gproduisant command has a table-like data structure, you have to print the results in a table with IMPR_TABLE. 1. **Calculating K with POST_K1_K2_K3** Calculate K with POST_K1_K2_K3: * use the result of MECA_STATIQUE (RESULTAT) * fill in the bottom of the crack * fill in the ABSC_CURV_MAXI parameter * print the results in a table (IMPR_TABLE) Note: do not take into account the alarm in CALC_CHAMP which states that EXCIT must be added. Compare the results obtained to the Handbook solution. To go further, we can: * extend the charts for :math:`2a\mathrm{/}r>0.9` (for example :math:`2a\mathrm{/}r\mathrm{=}1`), * study the fineness of the mesh, * do a parametric study for :math:`e\mathrm{=}\mathrm{[}\mathrm{0 };\mathrm{2b}\mathrm{]}` (think about using python), * study other configurations (inclined cracks, addition of other cracks...). .. image:: images/Object_17.png :width: 7.1134in :height: 5.7835in .. _RefSchema_Object_17.png: Figure 2.1.3-1: Abacus