3. Modeling A#
3.1. Workflow of the TP#
The aim is to carry out the elastic calculation by generating the geometry, the mesh and the AsterStudy command file using the Salome-Meca platform.
Modeling is C_PLAN elastic. A quarter of the plate is modelled. We will also define the commands necessary for the analysis (plot of curves and graphic post-processing).
3.1.1. Geometry#
We will create the flat face of the top right quarter of the plate.
Start the Geometry module.
The main steps to build this geometry are as follows:
To define the contours of the plate, you can, for example, use the « Sketcher » tool (Menu New Entity → Basic → 2D Sketch). It is easier to start with the point \(B\) with coordinates \((\mathrm{10,}0)\). Starting with \(B\), for the arc of a circle, use Element Type (Arc) and Destination (Direction/Perpendicular), and define radius 10 and the angle and radius 90°. We get point \(A\). Then use Element Type (Line) and give the other points (\(G\), \(F\), \(D\)) by their absolute coordinates. Finish with Sketch Closure.
We then get a closed outline (Sketch_1) on which we must build a face (Menu New Entity →Build →Face). The geometry of the plate is then complete.
Build groups that are useful for calculation. Here we build the 3 groups of edges on which the boundary conditions (symmetries and loading) will be based: left for edge \(\mathit{AG}\), top for edge \(\mathit{GF}\) and bottom for edge \(\mathit{BD}\). Menu New Entity →Group →Create Group: Select the type of geometric entity (here the line, edge) and select the edge directly in the graphics window, then click on Add, an object number should then appear. You can change the name of the group before validating it by Apply.
3.1.2. Meshing#
A plane mesh of the upper right quarter of the plate will be created, in elements of order 2, to have sufficient precision.
Start the Mesh module.
The main steps to generate the mesh are as follows:
Build the mesh (Menu Mesh → Create Mesh). Select the geometry to mesh Face_1, then choose Algorithm → NETGEN 1D - 2Den adding Hypothesis → NETGEN 2D Parameters. In this case, select Fineness → Fine and check the Second Order box before Applying.
Calculate the mesh (Mesh → Compute menu). A mesh information window should appear, and a free mesh is then obtained.
Create the mesh groups corresponding to the geometric groups (Menu Mesh → Create Groups from Geometry). Select all 3 edge groups under the Geometry module and then Apply. We obtain 3 groups of edges on the mesh.
To obtain better precision, we will change the mesh from linear to quadratic, using the « Modification -> Convert to/from quadratic » tool. The most curious can compare the differences in results between the two types of elements.
(Optional) Export the mesh in MED format: select Mesh_1 and right click, then choose Export/MED file.
Notes:
This mesh is fine enough (with quadratic elements) to have a good approximation of the elastic solution: for example if we compare \({\mathrm{\sigma }}_{\mathrm{\theta }\mathrm{\theta }}\) on the edge of the hole with respect to the analytical solution, we obtain a difference of less than 5% .
The geometry and mesh parameters are defined in the forma01a.datg*file associated with the test. The mesh produced is stored in the* forma01a.mmed*file .*
3.2. Creation and launch of the calculation case (via asterStudy)#
Start the AsterStudy module.
Then in the left column, click on the Case View tab. In the Data Settings box, right-click CurrentCase and choose Add Stage. It is in Stage_1 where we define the command file for the calculation case.
Note: Search for commands by Menu Commands → Show All or by the 10 calculation categories: Mesh, Model Definition, Material, Functions and Lists, BC and Load, Pre Analysis, Pre Analysis, Post Processing, Post Processing, Post Processing, Fracture and Fatigue, Output.
The main steps for creating and launching the calculation case are as follows:
Read the mesh in format MED: Category Mesh/Command LIRE_MAILLAGE. The mesh in module MESH is available in the list. Otherwise the button behind allows you to choose a mesh in the directories.
Orient the normal of the edge on which the traction load will be applied: Category Mesh/Command MODI_MAILLAGE/ORIE_PEAU_2Den affecting the top group in GROUP_MA. We keep the same mesh name using reuse.
Define the finite elements used: Model Definition category/Command AFFE_MODELE for 2D plane stress modeling (C_PLAN). Add a term in AFFE. In this term, assign OUI to TOUT elements, and choose the phenomenon MECANIQUE, and add the 2D plane constraints term (C_PLAN) in the modeling
Define material: Material category/Order DEFI_MATERIAU .Choose ELAS and enter values for Young’s modulus and Poisson’s ratio.
Assign material: Material category/Order AFFE_MATERIAU .Define at least one option between MAILLAGE and MODELE. Add a term in AFFE, and assign the material set to TOUT.
Affect mechanical boundary conditions and loading: Category BC and Load/Order AFFE_CHAR_MECA:
for traction: PRES_REP. For the top, enter the pull at PRES (so it’s negative).
Solve the linear static mechanical problem: Category Analysis/Command MECA_STATIQUE by giving the material (CHAM_MATER), modeling (MODELE), boundary conditions, and loading (EXCIT).
Calculate the field: Post Processing Category/Order CALC_CHAMP by activating reuse (to keep the same name of the input object in the order). In other words, we will enrich the concept from MECA_STATIQUE by using the same name.
for calculating the equivalent stress field: CRITERES/SIEQ_ELNO (by elements at the nodes), SIEQ_ELGA (by elements at the Gauss points), SIEQ_NOEU (global to the nodes).
Print the results of a calculation in format MED: Output Category/Command IMPR_RESU .Add a term in RESU, and choose the results to be printed. Set the output file (.rmed) to UNITE.
To start the calculation case, in the left column, click on the History View tab. You must save the study first, and select CurrentCase. Add Stage_1 by selecting run (green cross). Before starting, check the desired calculation parameters in the Run Parameters box: calculation time limit, memory, code_aster version etc.
3.3. Post-processing of results#
To visualize the results, two choices are currently available: the Results tab in AsterStudy, and the ParAvis module.
Choice 1: In the Results tab in Aster Study:
The following post-treatments are proposed:
Import the result file (CaseCase View → Data Files), right click on the output file and choose post-process.By default, the coloring of the plate by the displacement field DEPL, an automatic amplification is applied to the deformation of the plate. To clearly visualize the difference between the initial shape and the deformed, right-click on the window and choose Show as/Wireframe.
Double click the desired field, use the Probe values on one or more points or cells button (cross symbol) to check the values at points A and B.
(optional) go to the Paravis module, we find the current visualization state and also all the historical actions.
Choice 2: In the ParAvis module:
The following post-treatments are proposed:
Import the result file (CaseCase View → Data Files), right click on the output file and choose Open in by Avis.
Download the results: In the Properties tab the column on the left, first choose the fields you want to import, and check the GenerateVectors option, then apply Apply.
Visualize the initial mesh (switch to Surface With Edges representation).
Visualize the deformation of the plate (Menu Filters → Common → Warp By Vector with optionsVectors = results_ DEPL_VectoretScaleFactor = 100 before Apply).
Visualize the constraint field by elements at the nodes or at Gauss points: select the imported result, then in the Filters → Mechanics Menu, choose the desired visualization option.
Check the value of the stresses at node B: if we find a ratio 3 between the stress \({\mathrm{\sigma }}_{\mathrm{\theta }\mathrm{\theta }}\) (= \({\mathrm{\sigma }}_{\mathit{yy}}\)) at the edge of the hole and the force applied. To visualize the results on a node, activate Hover points on (like the photo below), and move the mouse to the desired node.
3.4. Tested sizes and results#
Value of stress components:
Location |
Identification |
Reference (Analytics) |
Tolerance |
Node \(B\) |
Constraint \(\mathit{SIYY}\) |
303.0 |
|
Knot \(A\) |
Constraint \(\mathit{SIXX}\) |
-100.0 |
|
These tests on analytical values are supplemented by non-regression tests.