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 :math:`(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.


.. image:: images/100000000000033C000001D7B34283E122499990.png
    :width: 5.5654in
    :height: 3.2319in


.. _RefImage_100000000000033C000001D7B34283E122499990.png:

A1

PPPP


Geometry
----

We can create this geometry by defining the points :math:`A1`, :math:`P` and :math:`\mathrm{A2}`, then the arc of a circle :math:`\mathit{Base}` (Menu New Entity → Basic → Point/Arc) .Then simply create the first straight pipe :math:`\mathrm{AC}` from the arc of a circle :math:`\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 :math:`\mathrm{AC}` by applying the MenuNewEntity→Explode (Edge), then create a vector parallel to the Z axis and passing the point O :math:`(\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 :math:`\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 :math:`\mathrm{A1}`.


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 :math:`\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.


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


    *   Internal pressure :math:`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.