First CFD Case
2. First Simulation by OpenFOAM
a. Problem definition
The first problem we work on is the well known ''Cavity Problem'' (see for exapmle). Here, the lid (top wall) of a square model moves by $ U=1~\mathrm{m/s} $ to the right side. Accordingly, the fluid (water in this case) moves with the lid owing to the no-slip condition.
Figure: Cavity Problem definition
You can find the documentation of this problem in doc folder in OpenFOAM installation directory. Open a terminal window by ctrl+t and run the command below in the terminal
evince -i 19 /opt/openfoam10/doc/Guides/OpenFOAMUserGuide-A4.pdf &
to open the ''Tutorials'' on page 19. Then you can close the terminal window.
b. Pre-processing
We can find this study in the tutorials directory of our OpenFOAM installation. Copy it in lecture02 folder.
cd ~/OpenFOAM/lecture02/
cp -r /opt/openfoam10/tutorials/incompressible/icoFoam/cavity/cavity .
''blockMesh'' is a mesh generation tool for creating simple block meshes in OpenFOAM.
The cavity problem geometry and mesh is set in system/blockMeshDict file.
This file generates the geometry below.
Figure: Cavity Problem computational domain
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.1;
vertices
(
(0 0 0)
(1 0 0)
(1 1 0)
(0 1 0)
(0 0 0.1)
(1 0 0.1)
(1 1 0.1)
(0 1 0.1)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (20 20 1) simpleGrading (1 1 1)
);
boundary
(
movingWall
{
type wall;
faces
(
(3 7 6 2)
);
}
fixedWalls
{
type wall;
faces
(
(0 4 7 3)
(2 6 5 1)
(1 5 4 0)
);
}
frontAndBack
{
type empty;
faces
(
(0 3 2 1)
(4 5 6 7)
);
}
);
// ************************************************************************* //
The mesh can be generated by running
blockMesh
command in the cavity folder. Then, you can visualize the mesh running
paraFoam
Figure: ParaView visualization of the blockMesh of Cavity Problem
We can find the mesh files, such as
~/OpenFOAM/lecture02/cavity/constant/polyMesh
├── boundary
├── faces
├── neighbour
├── owner
└── points
c. Solver setup
0 (zero) directory
In setting up the solver,
the first step is to define the boundary and initial conditions (BCs and ICs).
These are specified within the 0 folder in the working directory.
~/OpenFOAM/lecture02/cavity/0
├── p
└── U
Here the p and U are the condition files for pressure and velocity.
Besides the pressure field $ p $ and velocity field $ U $, which are almost always present,
the contents of the 0 directory can vary
significantly depending on the physics of the problem
being solved and the specific solver being used.
Here are some common examples:
T: Temperature field, used in heat transfer and compressible flow simulations.k: Turbulent kinetic energy, used in simulations involving turbulence models like k-epsilon or k-omega.epsilonoromega: Specific dissipation rate (for the k-epsilon model) or specific rate of dissipation (for the k-omega model), used in turbulence modeling.nut: Turbulent viscosity, used in turbulence modeling.alpha: Volume fraction of one phase in multiphase flow simulations, used in solvers like interFoam and multiphaseInterFoam.rho: Density, used in compressible flow simulations and sometimes in multiphase flow simulations.phi: Flux field, used in various solvers.
In the pressure file below, dimensions [0 2 -2 0 0 0 0] part is important. These numbers are
| Dimension | Represents | Numbers |
|---|---|---|
| Mass | kilograms (kg) | 0 |
| Length | meters (m) | 2 |
| Time | seconds (s) | -2 |
| Temperature | kelvin (K) | 0 |
| Quantity of Substance | mole (mol) | 0 |
| Electric Current | ampere (A) | 0 |
| Luminous Intensity | candela (cd) | 0 |
Therefore, the unit is $ \mathrm{m^2/s^2} $. However, actual unit of the pressure is
$$ \mathrm{Pa} = \frac{\mathrm{N}}{\mathrm{m^2}} = \frac{\mathrm{kg}}{\mathrm{m~s}^2}. $$
In OpenFOAM, the pressure $ \mathrm{p} $ is defined actually as ''pressure per unit density''. Density unit is $ \mathrm{kg/m^3} $. So the
$$ \dfrac{\mathrm{m^2}}{\mathrm{s^2}} = \dfrac{\frac{\mathrm{kg}}{\mathrm{m~s}^2}}{\frac{\mathrm{kg}}{\mathrm{m^3}}} . $$
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii; // The file format is ASCII, meaning it's human-readable
class volScalarField; // This file describes a scalar field variable (as opposed to a vector field)
object p; // The name of the field defined in this file, which is pressure 'p'
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0]; // The dimensions of pressure in terms of basic dimensions (mass, length, time, etc.)
internalField uniform 0; // Sets a uniform initial condition for pressure throughout the domain, which is zero in this case
boundaryField
{
movingWall
{
type zeroGradient; // The pressure gradient at the boundary is zero, meaning no change in pressure across this boundary
}
fixedWalls
{
type zeroGradient; // Same as above, no pressure gradient across the boundary
}
frontAndBack
{
type empty; // Specifies there's no domain in this direction, used in 2D simulations
}
}
// ************************************************************************ //
In the velocity file below, the unit is $ \mathrm{m/s} $ as it is mentioned above.
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii; // File format: ascii (human-readable) or binary
class volVectorField; // Means it's a vectoral field variable defined over the volume of the mesh
object U; // Object name: 'U' typically represents the velocity field in OpenFOAM
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0); // This sets the initial condition for the velocity field inside the domain to a uniform value, which in this case is a vector field with all components being zero (no initial velocity).
boundaryField
{
movingWall
{
type fixedValue; // The type of boundary condition: 'fixedValue' means the value is set and does not change.
value uniform (1 0 0); // The value of velocity on this boundary: a uniform velocity in the x-direction.
}
fixedWalls
{
type noSlip; // 'noSlip' condition means the velocity is zero relative to the wall (the fluid sticks to the wall).
}
frontAndBack
{
type empty; // 'empty' is used in 2D simulations to specify that there is no flow normal to these boundaries.
}
}
// ************************************************************************ //
constant directory
Check the constant folder which we define the
- physicalProperties
- transportProperties
- turbulenceProperties
- g (gravity)
- polyMesh
- solidProperties
- environmentalProperties
- fvSchemes and fvSolution
and so on. In this example, we only have the physicalProperties which is shown as follows.
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii; // The file format is ASCII, meaning it's human-readable
class dictionary; // This file is a dictionary, which is a set of key/value pairs in OpenFOAM
location "constant"; // The directory where this dictionary is located, typically 'constant' for physical properties
object physicalProperties; // The name of the object this file describes, in this case, 'physicalProperties'
}
nu [0 2 -1 0 0 0 0] 0.01; // Defines the kinematic viscosity 'nu' with dimensions and a value of 0.01 m^2/s
Here, nu [0 2 -1 0 0 0 0] 0.01 part is important. These numbers are
| Dimension | Represents | Number in nu Above |
|---|---|---|
| Kinematic Viscosity | meter square per second ($ \mathrm{m^2/s} $) | nu |
| Mass | kilograms (kg) | 0 |
| Length | meters (m) | 2 |
| Time | seconds (s) | -1 |
| Temperature | kelvin (K) | 0 |
| Quantity of Substance | mole (mol) | 0 |
| Electric Current | ampere (A) | 0 |
| Luminous Intensity | candela (cd) | 0 |
| Kinematic Viscosity | meter square per second ($ \mathrm{m^2/s} $) | 0.01 |
Here in our case, the 0.01 represents the $ \nu = 0.01~\mathrm{m^2/s} $. We can reach the Reynolds Number ($ \mathrm{Re} $) of the flow from this.
$$ \mathrm{Re} = \dfrac{DU}{\nu}, $$
where $D$ is the length of our model which is $0.1~\mathrm{m}$, $U$ is the velocity of our lid model which is $1~\mathrm{m/s}$, hence,
$$ \mathrm{Re} = \dfrac{0.1~\mathrm{m}~1~\mathrm{m/s}}{0.01~\mathrm{m^2/s}} = 10. $$
Therefore, we can understand that our flow is a low-Re flow. This is important to chose the solvers and turbulence models in OpenFOAM.
system directory
The system directory contains configuration files that define the overall behavior of the simulation. Key files in this directory typically include:
- controlDict: Controls the start and end times of the simulation, time step size, data writing frequency, and the format of the written data.
- fvSchemes: Defines the numerical schemes used for spatial and temporal discretization in the simulation.
- fvSolution: Specifies the solution algorithms for the linear system of equations, solver settings, and tolerances.
- transportProperties: (In some cases, though often found in the constant directory) Describes the transport properties like viscosity and diffusivity.
- decomposeParDict: Configuration for domain decomposition when running simulations in parallel.
- blockMeshDict: (If using blockMesh) Defines the mesh in terms of vertices, blocks, and boundary patches.
- meshQualityDict: Settings for mesh quality controls during meshing operations.
- snappyHexMeshDict: (If using snappyHexMesh) Configures the mesh generation process for complex geometries.
These files collectively determine how the simulation is set up, solved, and written out. They need to be configured correctly for the simulation to run as intended.
In ''cavity'' case the directory contains
~/OpenFOAM/lecture02/cavity/system
├── blockMeshDict
├── controlDict
├── fvSchemes
└── fvSolution
We studied on the blockMeshDict earlier. The controlDict is explained as follows.
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application icoFoam; // Specifies the solver to be used
startFrom startTime; // Specifies the starting point of the simulation, 'startTime' means from the beginning
startTime 0; // Sets the simulation start time to 0 seconds
stopAt endTime; // Determines the stopping criterion, 'endTime' means stop at a specified time
endTime 0.5; // Sets the simulation end time to 0.5 seconds
deltaT 0.005; // Sets the time step for the simulation to 0.005 seconds
writeControl timeStep; // Determines when to write data, 'timeStep' means write every fixed number of time steps
writeInterval 20; // Sets the interval at which data is written to 20 time steps
purgeWrite 0; // Specifies the number of past time directories to keep; 0 means keep all
writeFormat ascii; // Specifies the data format for writing, 'ascii' is human-readable
writePrecision 6; // Sets the precision (number of significant digits) for writing data to 6
writeCompression off; // Specifies whether to compress the output files, 'off' means no compression
timeFormat general; // Specifies the format for time values, 'general' is a flexible format
timePrecision 6; // Sets the precision for writing time values to 6 significant digits
runTimeModifiable true; // Allows certain parameters to be modified while the simulation is running
// ************************************************************************* //
The fvSchemes file defines numerical schemes used in an OpenFOAM simulation for different mathematical operations.
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes // Time differentiation schemes.
{
default Euler;
}
gradSchemes // Gradient calculation schemes.
{
default Gauss linear;
grad(p) Gauss linear;
}
divSchemes // Divergence calculation schemes for convective transport.
{
default none;
div(phi,U) Gauss linear;
}
laplacianSchemes // Schemes for solving Laplacian (diffusion) terms.
{
default Gauss linear orthogonal;
}
interpolationSchemes // Methods for interpolating values between mesh cells.
{
default linear;
}
snGradSchemes // Schemes for calculating surface-normal gradients.
{
default orthogonal;
}
// ************************************************************************* //
Other option names for each scheme category in OpenFOAM might include:
- ddtSchemes: CrankNicolson, backward, steadyState
- gradSchemes: leastSquares, cellLimited Gauss linear
- divSchemes: upwind, vanLeer, limitedLinear
- laplacianSchemes: Gauss linear corrected, cellMDLimited Gauss linear
- interpolationSchemes: cubic, faceLimited cubic
- snGradSchemes: corrected, limited
These are just a few examples, and OpenFOAM provides a wide range of schemes for each category. Each scheme has its own use cases and is chosen based on the requirements of the simulation for accuracy and stability.
The fvSolution file configures solvers,
tolerances, and algorithms for solving the equations in an OpenFOAM simulation.
It specifies solver settings for pressure (p),
a final pressure correction step (pFinal),
and velocity (U), along with the PISO algorithm parameters.
The file in this case is explained with other alternative methods below.
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p
{
solver PCG; // Other solvers: GAMG, PBiCG, BiCGStab
preconditioner DIC; // Other preconditioners: DILU, GAMG
tolerance 1e-06;
relTol 0.05;
}
pFinal
{
$p;
relTol 0; // Final tolerance reset to zero for accuracy
}
U
{
solver smoothSolver; // For velocity
smoother symGaussSeidel; // Other smoothers: GaussSeidel, DICGaussSeidel
tolerance 1e-05;
relTol 0;
}
}
PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0; // Additional corrections for non-orthogonality
pRefCell 0; // Reference cell for pressure level
pRefValue 0; // Reference value for pressure in pRefCell
// Additional PISO option: nOuterCorrectors for outer correctors
// Additional PISO option: residualControl for controlling residuals
}
// ************************************************************************* //
d. Computing
The solver we use in this case is the icoFoam. It is one of the basic solvers in OpenFOAM. You can find some information by typing
foamInfo icoFoam
This command will print the output below.
File
/opt/openfoam10/applications/solvers/incompressible/icoFoam/icoFoam.C
Description
Transient solver for incompressible, laminar flow of Newtonian fluids.
Examples using "icoFoam"
/opt/openfoam10/tutorials/incompressible/icoFoam/cavity/cavityGrade
/opt/openfoam10/tutorials/incompressible/icoFoam/cavity/cavityClipped
/opt/openfoam10/tutorials/incompressible/icoFoam/cavity/cavity
/opt/openfoam10/tutorials/incompressible/icoFoam/elbow
To compute the ''cavity'' case, run the following command.
icoFoam
That's all. We have set a simulation using OpenFOAM and computed it.
e. Post-processing
Now, in the ~/OpenFOAM/lecture02/cavity folder there are some other files.
~/OpenFOAM/lecture02/cavity
├── 0
├── 0.1
├── 0.2
├── 0.3
├── 0.4
├── 0.5
├── constant
└── system
We know the 0, constant and system folders. The other folders include the solution. For example 0.5 folder is as follows.
~/OpenFOAM/lecture02/cavity/0.5
├── p # Pressure field data at this time step.
├── phi # Flux field data, often representing the face fluxes for velocity or other scalar fields.
├── U # Velocity field data, containing the vector field of fluid velocities.
└── uniform
└── time # A special directory indicating that certain data (like time) is uniform across the domain or doesn't change with position.
Run
paraFoam
to visualize the results in ParaView.
Figure: Cavity Problem velocity contours and streamtraces with a set colorbar
Figure: Cavity Problem pressure contours and streamtraces with a set colorbar