3. Modeling A#
3.1. Workflow of the TP#
The aim is to conduct the calculation by modeling the concrete using elements \(3D\) and the steel reinforcements with elements GRILLE_MEMBRANE. The*Code_Aster* command file will be generated using AsterStudy.
3.2. Realization of the mesh#
Limited time option: we suggest reading the mesh (forma40a.mmed) that was created with a Salomé script. The file can be retrieved from the salome_meca installation directory (path: XXX /salome_meca/ VYYY /tools/code_aster_stable_ ZZZZ /share/aster/tests).
Option in an unconstrained time: the user can perform the mesh, making sure to pass the mesh through the surfaces where the reinforcement sheets are located.
3.3. Elastic calculation#
The aim is to define the file the command file used to carry out this study. The various steps are indicated below:
Read the mesh in MED (LIRE_MAILLAGE) format. |
Assign models to different mesh groups (AFFE_MODELE/3D and GRILLE_MEMBRANE). |
Define the characteristics of the structural elements (AFFE_CARA_ELEM, keyword GRILLEpour the elements GRILLE_MEMBRANE), namely the section and the coordinate system used to define the local coordinate system. |
Define the material properties of steel and concrete (DEFI_MATERIAU) and affect them (AFFE_MATERIAU). |
Create time discretization using DEFI_LIST_REEL. |
Define boundary conditions and loads (AFFE_CHAR_MECA, keywords DDL_IMPOet PESANTEUR). Note: loading on edge \(B1X\) requires defining a multiplier function using the DEFI_FONCTION command that will be applied to loading via the FONC_MULT keyword under EXCIT or using AFFE_CHAR_MECA_F. |
Use STAT_NON_LINEpour the elastic calculation (COMPORTEMENT/RELATION =” ELAS “) with the instant list defined earlier. |
Print the result in MED format (IMPR_RESU/FORMAT =” MED “). |
Save and start the calculation. |
3.4. Post-treatment#
3.4.1. Basic stripping with Paravis#
Import file MED in*Salomé* under Paravis. |
Trace the deformed (Warp by Vector filter). |
Visualize constraints at Gauss points (filter ELGA field To Point Gaussian). |
Complete the command file by calculating various interesting quantities: deformations (type ELGAou ELNO), stresses and/or equivalent deformations. Start the calculation again and then visualize the different quantities under Salomé. |
3.4.2. Plotting a force-displacement curve in Code_Aster#
By using the initial command file or by defining a new stage, do the post-processing to draw the force-displacement curve.
Calculate nodal forces using command CALC_CHAMP. |
Retrieve the result of the efforts applied using the POST_RELEVE_T command. |
Retrieve the next move \(>\) from edge \(NO2NO3\) using the POST_RELEVE_T command. |
Print both tables to visualize the information contained. |
Plot the force-displacement curve in XMGRACE format using the IMPR_FONCTION command. To do this, retrieve the functions to be traced using RECU_FONCTION by applying the necessary filters. (Do not forget to specify the unit and define the output file to be able to visualize the curve directly). |
3.4.3. Suggestions for other post-treatments#
Retrieve the deformations along a line (for example, from point \((\mathrm{0,2.5}\mathrm{,0})\) to point \((10\text{.}\mathrm{,2}\text{.}5\mathrm{,0})\)) using the command MACR_LIGN_COUP. Print the curve using command IMPR_TABLE. |
Print the maximum stress obtained in concrete and then in steels using the POST_RELEVE_T command (OPERATION =” EXTREMA “). |
3.5. Tested sizes and results#
Value of stress components:
Location |
Identification |
Reference |
Tolerance |
Edge \(B1X\) |
Resulting effort \(DZ\) |
|
|
Maximum stress in the steel sheet \(ACM\) |
|
|
|
Maximum stress in concrete |
\(\mathrm{1,61016}\times {10}^{7}\) |
|