5. C modeling#

In the case of shell element modeling, meshing consists in discretizing the average area of the pipe. Since the geometry is symmetric with respect to plane \((A,X,Y)\), we mesh only half a surface.

Boundary conditions and loading: embedment at both ends of the pipe, and pressure at the internal surface.

_images/100000000000033C000001D7B34283E122499990.png

A1

PPPP

5.1. Geometry#

We can create this geometry by defining the points \(A1\), \(P\) and \(\mathrm{A2}\), then the arc of a circle \(\mathit{Base}\) (Menu New Entity → Basic → Point/Arc) .Then simply create the first straight pipe \(\mathrm{AC}\) from the arc of a circle \(\mathrm{Base}\) by using the New Entity → Generation → Extrusion menu: Vector = OY, Height = 3.

To create the elbow, you need to retrieve the end of pipe \(\mathrm{AC}\) by applying the MenuNewEntity→Explode (Edge), then create a vector parallel to the Z axis and passing the point O \((\mathrm{0.6,}\mathrm{3.0,}0.)\). Then generate the elbow geometry using the New Entity → Generation → Revolution menu.

Finally, apply the same approach for pipe \(\mathrm{DB}\) (Explode then Extrusion).

Create a « compound » (New Entity Menu → Build → Compound) by selecting the three parts of the pipe.

We will then create the mesh groups where we want to set limit conditions: Base, Symmetry, Background and pipe surface (Menu New Entity → Group → Create Group).

We will also create the group point \(\mathrm{A1}\).

5.2. 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 discretization hypothesis by dimension:

  • 2D Quadrangle: Mapping.

  • 1D Wire Discretization with the basic Number of Segment hypothesis (15 segments per edge).

Then calculate the mesh (Menu Mesh → Compute).

To allow different refinement depending on the edges, we will create a sub-mesh (Menu Mesh → Create Sub-mesh) defining the basic hypothesis Number of Segment on the circumference, for example 10 segments on \(\mathit{base}\) and the additional hypothesis « Propagation of 1D hypothesis on Opposite Edges ».

Then calculate the mesh (Menu Mesh → Compute).

Create the mesh groups corresponding to the geometric groups (Menu Mesh→Create Groups from Geometry).

Export the mesh in MED format.

5.3. 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 main steps of this mechanical calculation 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. The pipe will be modeled by shell elements (DKT).

  • Orient normals to elements: Command MODI_MAILLAGE/ORIE_NORM_COQUE to orient all elements in the same way, with a normal facing the inside of the pipe (given the sign convention on pressure) in order to give a positive value to the pressure (use the surface group).

  • Define material: Command DEFI_MATERIAU: E, NU, ALPHA

  • Assign material: Command AFFE_MATERIAU. The mechanical characteristics are identical throughout the structure.

  • Affect the characteristics of shell elements: Command AFFE_CARA_ELEM/COQUEpour define the thickness.

  • Affect mechanical boundary conditions and loads: Command AFFE_CHAR_MECA:

    • There is an embedment on the group of elements \(\mathrm{Base}\) and \(\mathrm{Efond}\), and symmetry conditions (normal displacement \(\mathrm{DZ}\) zero and rotations \(\mathrm{DRX}\) and \(\mathrm{DRY}\) zero) on the group of elements \(\mathrm{Symetrie}\): DDL_IMPO.

    • Internal pressure \(P\): PRES_REP. It is necessary to convert the pressure P at the inner surface into the pressure at the mean surface.

  • Solving the elastic problem: Command MECA_STATIQUE: CARA_ELEM,, CHAM_MATER, EXCIT, MODELE.

  • Print displacements and constraints in format MED: Command IMPR_RESU..

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