3. TP implementation#

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.

This TP allows you to:

Implement a standard non-linear calculation in the AsterStudy module: management of loading, materials, behavior and parameters of STAT_NON_LINE;
Understand and implement the concept of steering;
Do « advanced » post-treatments (in particular draw curves).

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 point \(B\) with coordinates \((\mathrm{10,}0)\). Starting with \(B\), for the arc, 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 5 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 \(\mathit{BD}\), right for edge, right for edge \(\mathit{FD}\) and hole for arc \(\mathit{AB}\). 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.
You can also create node groups, which will be useful for post-processing or management (Menu New Entity → Group → Create Group): five summit groups \(A\), \(B\), \(D\),,, \(F\) and \(G\).

We will create a plane mesh of the upper right quarter of the plate, in quadratic elements, 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 → NETGEN2D Parameters. In this case, select Fineness → Fine and check the Second Order box before Applying.
Calculate the mesh (Menu Mesh → Compute). A mesh information window should appear, and we then get a refined mesh near the hole with large elements at the top of the plate.
To refine this mesh, right-click on the mesh and choose Edit Mesh, then edit the NETGEN 2D Parameters parameters:
- You can reduce Max Size by choosing \(10\) for example.
- If you want to refine around the hole, you can in the Local sizes tab add the group hole \(\mathit{AB}\) with the On edge button, and then just modify the associated value. By reducing it (for example \(2\)), the mesh will be refined around the hole.
Calculate the mesh (Mesh → Compute menu).
To change the mesh from linear to quadratic: « Modification -> Convert to/from quadratic ».
Create the mesh groups corresponding to the geometric groups (Menu Mesh → Create Groups from Geometry). Select all geometric groups.
Export the mesh in MED format.