6. D modeling#

6.1. Geometry#

Geometry can be created by defining the points \(A,C,D,B\), then the two lines \(\mathrm{AC}\) and \(\mathrm{DB}\), and the arc of a circle \(\mathrm{CD}\). This can be done in several ways:

  • By defining the coordinates of each point, including the midpoint of arc \(\mathit{CD}\) (Menu New Entity → Basic →…);

  • In a simpler way using the « Sketcher » tool (New Entity Menu → Basic→2D Sketch).

After building the entire line, you must define the groups under this « Wire »: for this practical work, it will suffice to create the groups \(A\), \(B\), \(\mathrm{AC}\), \(\mathrm{CD}\), and \(\mathrm{DB}\) (Menu New Entity → Group → Create Group) (Menu New Entity → Group → Create Group).

6.2. Meshing#

Launch the Mesh module of the Salome-Meca platform.

The mesh is defined by the Mesh → Create Mesh menu. Select the geometry to be meshed, then the algorithm and the hypothesis of discretization by dimension: 1D Wire Discretization with the hypothesis of 15 segments per edge.

6.3. Creation and launch of the calculation case (via asterStudy)#

Launch the AsterStudy module from the Salome-Meca platform.

Then in the left column, click on the Case View tab.

The command file for the calculation case is defined.

Note: Add orders using the Commands menu → Show All.

The study requires a first transitory thermal calculation followed by a mechanical calculation.

The main steps for creating and launching the calculation case are as follows:

  • Read the mesh in MED format: Command LIRE_MAILLAGE.

  • Define the finite elements used: Command AFFE_MODELE.

  • Define material: Command DEFI_MATERIAU.

  • Assign material: Command AFFE_MATERIAU.

  • Affect the characteristics of the beam elements: Command AFFE_CARA_ELEM.

  • Affect mechanical boundary conditions and loading: Command AFFE_CHAR_MECA/Enforce DOF (DDL_IMPO). Point \(A\) is embedded.

  • Define the elastic problem matrices: Command ASSEMBLAGE/MASS_MECA and RIGI_MECA.

  • Calculate the first 5 natural modes: Command CALC_MODES.

  • Print the specific modes in format MED: Command IMPR_RESU. We will print the mesh and the modes.

To launch the calculation case, in the left column, click on the History View tab.

Transient analysis:

  • Construction of the point force

        • Assign the load « force to point \(B\) »: Command AFFE_CHAR_MECA/FORCE_NODALE.

        • Calculate the elementary force vectors: Command CALC_VECT_ELEM.

        • Build a field at the nodes by assembling the force vector: Command ASSE_VECTEUR.

        • Define the time evolution function: Command FORMULE.

  • Transitional on a modal basis

  1. Projection of the assembled problem based on the specific modes: Command PROJ_BASE.

  2. Calculate the transient by modal recombination: Command DYNA_VIBRA.

  3. Extract the moves in \(Y\) in \(B\): Command RECU_FONCTION.

  4. Print these functions in format TABLEAU: Command IMPR_FONCTION.