.. role:: xml(code)
  :language: xml

.. _Sec:tuto:splitDomains:

**********************************************
Split physical domains for unstructured meshes
**********************************************

ECOGEN is able to initialize fluid domains according to geometrical physical domains for Gmsh_ unstructured mesh (see :ref:`Sec:tuto:generatingMeshes`). Of course, it is also possible to initialize the computational domain with predefined type domain as described in the section :ref:`Sec:input:InitialConditions`. However, in this tutorial, we will focus on how to initialize fluid physical domains in ECOGEN according to geometrical domains defined in the geometry file of Gmsh *.geo*.

For the purpose of this tutorial, we will use a 2D single-phase shock tube of 1m length and 1m height (more information about this setup can be found at :ref:`Chap:TestCases`). The tube is filled with air (:math:`\rho = 1.225 \, kg /m^3`) initially at rest, the left chamber pressure is :math:`P_L = 5 \, bar` and the right chamber pressure is fixed at :math:`P_R = 1 \, bar`.

Geometry and mesh
=================

The 2D tube is defined by a 1x1 square. To design the initial interface between the left and right chamber we create two points on the upper and lower part (**Point(5)** and **Point(6)**) of the domain, that are connected by **Line(7)**:


.. figure:: ./_static/tutos/splitPhysicalDomains/meshTube.png
  :scale: 30%
  :align: center

  Geometry and mesh (triangular elements) of the 2D shock tube on Gmsh_ software.

The complete geometry configuration file (*.geo*) is the following:

.. code-block:: none

	//Mesh size
	dx = 0.05;

	// Physical domains number
	walls = 1;
	leftChamber = 2;
	rightChamber = 3;

	// Geometry definition
	Point(1) = {0, 0, 0, dx};
	Point(2) = {1, 0, 0, dx};
	Point(3) = {1, 1, 0, dx};
	Point(4) = {0, 1, 0, dx};
	Point(5) = {0.5, 0, 0, dx};
	Point(6) = {0.5, 1, 0, dx};

	Line(1) = {1, 4};
	Line(2) = {4, 6};
	Line(3) = {6, 3};
	Line(4) = {3, 2};
	Line(5) = {2, 5};
	Line(6) = {5, 1};

	Line(7) = {5,6}; // Interface between chambers

	// Boundary conditions
	Physical Line(walls) = {1, 2, 3, 4, 5, 6};

	// Left Chamber domain
	Line Loop(8) = {1, 2, -7, 6};
	Plane Surface(9) = {8};
	Physical Surface(leftChamber) = {9};

	// Right chamber domain
	Line Loop(10) = {3, 4, 5, 7};
	Plane Surface(11) = {10};
	Physical Surface(rightChamber) = {11};

Setup of the test case
======================

Let's start with the *main.xml* file. We use an *XML* output mode with time control set to *iterations* and a *CFL* number of *0.8*: 

.. code-block:: xml

	<?xml version = "1.0" encoding = "UTF-8" standalone = "yes"?>
	<computationParam>
		<run>shockTubeUnstructured</run>
		<outputMode format="XML" binary="false" precision="15"/>
		<timeControlMode iterations="true">
			<iterations number="100" iterFreq="10"/>
			<physicalTime totalTime="1e-3" timeFreq="5.e-5"/>
		</timeControlMode>
		<computationControl CFL="0.8"/>
	</computationParam>

To solve this flow we use the model *Euler* with air considered as ideal gas. Thus, the *model.xml* file is:

.. code-block:: xml

	<?xml version = "1.0" encoding = "UTF-8" standalone = "yes"?>
	<model>
		<flowModel name="Euler"/>
		<EOS name="IG_air.xml"/>
	</model>

Reading of the unstructured mesh is done throught the *mesh.xml* file:

.. code-block:: xml

	<?xml version = "1.0" encoding = "UTF-8" standalone = "yes"?>
	<mesh>
		<type structure="unStructured"/>
		<unstructuredMesh>
			<file name="libMeshes/myMeshFolder/tube2d.msh"/>
		</unstructuredMesh>
	</mesh>

All that remains to be done is to initialize the chambers with the corresponding fluid states. To this end, we define two :xml:`physicalDomains` of type *entireDomain*, one for each chamber. The link between the physical domains of the geometry file *.geo* and ECOGEN is made by the attribute :xml:`physicalEntity`. As given above on the *.geo* file, the left chamber has the physical entity number 2 and the right chamber has the number 3. Therefore, the *initialConditions.xml* file is:

.. code-block:: xml

	<?xml version = "1.0" encoding = "UTF-8" standalone = "yes"?>
	<CI>
	    <!-- LIST OF GEOMETRICAL DOMAINS  -->
	    <physicalDomains> 
	        <domain name="leftChamber" state="leftChamber" type="entireDomain" physicalEntity="2"/>
	        <domain name="rightChamber" state="rightChamber" type="entireDomain" physicalEntity="3"/>
	    </physicalDomains>

	    <!-- LIST OF BOUNDARY CONDITIONS -->
	    <boundaryConditions>
	        <boundCond name="walls" type="wall" number="1" />
	    </boundaryConditions>
	    
	    <!--  LIST OF STATES  -->
	    <state name="leftChamber">
	        <material type="fluid" EOS="IG_air.xml">
	            <dataFluid density="1.225" pressure="5.e5">
	                <velocity x="0." y="0." z="0."/>
	            </dataFluid>
	        </material>
	    </state>

	    <state name="rightChamber">
	        <material type="fluid" EOS="IG_air.xml">
	            <dataFluid density="1.225" pressure="1.e5">
	                <velocity x="0." y="0." z="0."/>
	            </dataFluid>
	        </material>
	    </state>
	</CI>

Add the new test case to the main input file *ECOGEN.xml*: :xml:`<testCase>./libTests/myTest/</testCase>`. 

Run the test case simulation with **XX** cores:

.. code-block:: console

	./ECOGEN
	mpirun -np XX ECOGEN

.. important::

	Be aware to partition the mesh file with the corresponding number of cores used for the simulation if parallel computation is desired. Gmsh pre-treatment attribute :xml:`GMSHPretraitement` of the *mesh.xml* file might be set to *true* in this case.

Results
=======

Initially, the configuration of the shock tube is as follows:

.. figure:: ./_static/tutos/splitPhysicalDomains/postProcessInit.png
  :scale: 30%
  :align: center

  Pressure visualization (left) and 1D plot of pressure and velocity along the length of the tube (right) at the initial time. Visualization using Paraview_ software.

It is clearly visible that the addition of the line along the interface makes it possible to obtain a mesh with a straight separation at this location. In the absence of this line, the initialization of the fluid states using a :xml:`halfSpace` leads to an initial interface deformed by the cells position:

.. figure:: ./_static/tutos/splitPhysicalDomains/halfSpaceInit.png
  :scale: 40%
  :align: center

  Pressure visualization at the initial time. Visualization using Paraview_ software.

Of course, for this test case configuration, it is possible to obtain an equivalent result without declaring two physical domains in the geometry file. By keeping the middle line of the geometry file, the straight separation is ensured and it is therefore possible to define in the *initialConditions.xml* file an :xml:`entireDomain` domain for the left chamber and a :xml:`halfSpace` domain located at :math:`x = 0.5 \, m` with a positive direction for the right chamber.

However, it can be particularly interesting to use an initialization of the fluid states with the definition of the physical domains from the geometry, in case the fluid regions are too complex to define with the predefined ECOGEN domains.

After few timesteps, the flow is the following:

.. figure:: ./_static/tutos/splitPhysicalDomains/postProcess.png
  :scale: 30%
  :align: center

  Pressure visualization (left) and 1D plot of pressure and velocity along the length of the tube (right) after few timesteps. Visualization using Paraview_ software.

.. _Gmsh: http://gmsh.info/
.. _Paraview: https://www.paraview.org/