Hydrothermal convection test case
Prepare case files
To get started we will run the Regular2DBox case from the cookbook directory of HydrothermalFoam. This cookbooks describes how we can simulate a simple hydrothermal convection cell. It resolves hydrothermal convection driven by a gaussian-shaped constant temperature boundary condition at the bottom.
Copy the case into your shared working directory (probably $HOME/HydrothermalFoam_runs). You need to do this within the docker container (your right-hand shell in Visual Studio Code if you followed the recommended setup). Cd into your shared folder and type this:
cd $HOME/HydrothermalFoam_runs
cp -r $HOME/hydrothermalfoam-master/cookbooks/2d/Regular2DBox .
Check out the directory structure shown in Listing 11.
1.
2|-- 0
3| |-- T
4| |-- p
5| -- permeability
6|-- a.foam
7|-- clean.sh
8|-- constant
9| |-- g
10| -- thermophysicalProperties
11|-- run.sh
12 -- system
13 |-- blockMeshDict
14 |-- controlDict
15 |-- fvSchemes
16 -- fvSolution.
The 0 directory now has entries for T (temperature) and p (pressure) our new primary variables, and for permeability, which we will discuss later. In addition, the constant directory has an entry thermophysicalProperties, which describes the solid properties.
Tip
Most OpenFoam cases include scripts like run.sh and clean.sh. The run.sh script is a good starting point for “understanding” a case. It lists all commands that have to be executed (e.g. meshing, setting of properties, etc.) to run a case. The clean.sh script cleans up the case and deletes e.g. the mesh and all output directories. Have a look into these files and see if you understand them!
The 0 directory contains all initial and boundary conditions, the system folder contains all controlling parameter files, and the constant folder contains constant properties like the mesh - which we will create next.
Mesh generation
The case is run on a simple 2-d-box-like geometry and the mesh is build using blockMesh, just like in the previous lecture on cavity flow. Look at blockMeshDict and check that you sill understand the structure. Afterwards, you can create the mesh:
blockMesh
After making the mesh, you can use Paraview to visualize it,
touch a.foam
paraview a.foam
Boundary conditions
Next we need to set boundary conditions. Open the file T inside the 0 directory from your local left-hand shell.
code 0/T
1/*--------------------------------*- C++ -*----------------------------------*\
2| ========= | |
3| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
4| \\ / O peration | Version: 5 |
5| \\ / A nd | Web: www.OpenFOAM.org |
6| \\/ M anipulation | |
7\*---------------------------------------------------------------------------*/
8FoamFile
9{
10 version 2.0;
11 format ascii;
12 class volScalarField;
13 object T;
14}
15// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
16
17dimensions [0 0 0 1 0 0 0];
18
19internalField uniform 278.15; //278.15 K = 5 C
20
21boundaryField
22{
23 left
24 {
25 type zeroGradient;
26 }
27 right
28 {
29 type zeroGradient;
30 }
31 top
32 {
33 //type fixedValue;
34 //value uniform 273.15;
35 type inletOutlet;
36 phi phi;
37 inletValue uniform 278.15;
38 }
39 bottom
40 {
41 type codedFixedValue;
42 value uniform 873.15;
43 name gaussShapeT;
44 code #{
45 scalarField x(this->patch().Cf().component(0));
46 double wGauss=200;
47 double x0=1000;
48 double Tmin=573;
49 double Tmax=873.15;
50 scalarField T(Tmin+(Tmax-Tmin)*exp(-(x-x0)*(x-x0)/(2*wGauss*wGauss)));
51 operator==(T);
52 #};
53 }
54 frontAndBack
55 {
56 type empty;
57 }
58}
59
60// ************************************************************************* //
The boundary conditions are again set for the patches that were defined in the blockMeshDict. Notice how the side are insulating (zeroGradient). The top has a boundary condition called inletOutlet; it sets a constant inflow temperature (recharge of cold seawater) and assumes zeroGradient for the outflow (mimicing free fluid venting). The bottom boundary condition is special, it is set to codedFixedValue. The codedFixedValue BC allows “programming” a boundary condition on the fly. Here a gaussian-shapes constant temperature boundary condition is programmed. Note that x(this->patch().Cf().component(0)) is the x-coordinate of each FV face of the patch “bottom”.
Units are set by the dimensions keyword. The entries refer to the standard SI units [Kg m s K mol A cd]. By having a one in the fourth columns, the units of the defined properties has units of Kelvin.
We also need to set boundary conditions for pressure.
code 0/p
1/*--------------------------------*- C++ -*----------------------------------*\
2| ========= | |
3| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
4| \\ / O peration | Version: 5 |
5| \\ / A nd | Web: www.OpenFOAM.org |
6| \\/ M anipulation | |
7\*---------------------------------------------------------------------------*/
8FoamFile
9{
10 version 2.0;
11 format ascii;
12 class volScalarField;
13 object p;
14}
15// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
16
17dimensions [1 -1 -2 0 0 0 0];
18
19internalField uniform 300e5;
20
21boundaryField
22{
23 left
24 {
25 type noFlux;
26 }
27 right
28 {
29 type noFlux;
30 }
31 top
32 {
33 type submarinePressure;
34 value uniform 300e5;
35 }
36 bottom
37 {
38 type noFlux;
39 }
40 frontAndBack
41 {
42 type empty;
43 }
44}
45
46// ************************************************************************* //
The noFlux boundary conditions, sets the pressure gradient to zero (horizontal direction) and hydrostatic (vertical direction), so that no flow occurs through these boundaries. The submarinePressure boundary condition is provided by HydrothermalFoam and sets the pressure according to water depth. Change it to fixedValue; we will discuss the special boundary conditions later.
Transport properties
In hydrothermal convection simulations, the fluid properties are given by the used EOS (details on this in the next lecture). What we need to set are the solid properties like permeability, solid density, solid specific heat, and porosity. These are set in two different files. Permeabilty is treated as a variable and is set in the 0 directory.
code 0/permeability
1/*--------------------------------*- C++ -*----------------------------------*\
2| ========= | |
3| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
4| \\ / O peration | Version: 5.0 |
5| \\ / A nd | Web: www.OpenFOAM.org |
6| \\/ M anipulation | |
7\*---------------------------------------------------------------------------*/
8FoamFile
9{
10 version 2.0;
11 format ascii;
12 class volScalarField;
13 location "0";
14 object permeability;
15}
16// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
17
18dimensions [0 2 0 0 0 0 0];
19
20internalField uniform 1e-14;
Again, check that you understand the units, which here add up to m^2.
Next we look at the solid properties:
code constant/thermophysicalProperties
Check that you understand the units! Details can be found in the HydrothermalFoam documentation.
Case control
Finally, we need to set some control parameters like the time step, run time, output writing. These kind of parameters are set in system/controlDict. Open it and explore the values
code system/controlDict
1/*--------------------------------*- C++ -*----------------------------------*\
2| ========= | |
3| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
4| \\ / O peration | Version: 5 |
5| \\ / A nd | Web: www.OpenFOAM.org |
6| \\/ M anipulation | |
7\*---------------------------------------------------------------------------*/
8FoamFile
9{
10 version 2.0;
11 format ascii;
12 class dictionary;
13 object controlDict;
14}
15
16application HydrothermalSinglePhaseDarcyFoam;
17startFrom latestTime;
18startTime 0;
19stopAt endTime;
20endTime 16912000000; //86400000000
21deltaT 864000;
22adjustTimeStep yes;
23maxCo 0.8;
24maxDeltaT 86400000;
25writeControl adjustableRunTime;
26writeInterval 86400000;
27purgeWrite 0;
28writeFormat ascii;
29writePrecision 6;
30writeCompression off;
31timeFormat general;
32timePrecision 14;
33runTimeModifiable true;
34libs
35(
36
37 "libHydrothermalBoundaryConditions.so"
38 "libHydroThermoPhysicalModels.so"
39);
The solver we are using is called HydrothermalSinglePhaseDarcyFoam. In addition, we are including two libraries “libHydrothermalBoundaryConditions.so”; these are part of HydrothermalFoam and provide special boundary conditions for submarine hydrothermal flow calculations.
Running the case
Now we are finally ready to run our first test case. Just type this into your docker shell:
HydrothermalSinglePhaseDarcyFoam
Notice how several directories are appearing, which contain the intermediate results. You can postprocess the case by simply opening the a.foam file from paraview.
Fig. 14 Results of the Regular2DBox example calculation.