1.4.1. Lid Driven Cavity¶

Problem Specification
Pre-Processing
Viewing the Mesh
Running the Application
Post-processing
Increased Mesh Resolution

1.4.1.1. Problem Specification ¶

For the open cavity, what is the influence of:

Increased mesh resolution?
Increased mesh grading?
Reynolds Number?
Turbulent flow?

The open cavity is defined as shown below:

Case 1 - icoFoam Solver:

Laminar
Isothermal
Incompressible

Case 2 - pisoFoam Solver:

Turbulent
Isothermal
Incompressible

1.4.1.2. Pre-Processing ¶

I use Kate for processing the text files. I have set $FOAM_RUN = /home/andrew/Dropbox/7_OpenFOAM/run. Now I copy the files from the tutorial directory:

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity
$ cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity .
$ cd cavity

This copies the following ascii dictionaries into cavity (the case directory):

0
- p (ics and bcs values)
- U (ics and bcs values)
constant
- transportProperties (viscosity)
system
- blockMeshDict (mesh, domain and bcs application)
- controlDict (parameters for solver)
- fvSchemes (time and space numerical schemes)
- fvSolution (parameters for numerical schemes)

1.4.1.2.1. Mesh Generation¶

OpenFOAM always uses a 3D system, but 2D can be used by specifying an empty bc on the 3rd dimension. The right-hand rule for node numbering:

The components of the blockMeshDict are given below.

1.4.1.2.1.1. Header information¶

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

1.4.1.2.1.2. File information¶

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

1.4.1.2.1.3. Scaling factor for the vertex coordinates¶

All the coordinates given in the vertices section are multiplied by 0.1, or whatever factor is given. Looking at the vertices coordinates, this sets the sides of the cavity to 0.1m x 0.1m and it’s depth to 0.01m.

convertToMeters 0.1;

1.4.1.2.1.4. Vertices¶

Ordering of vertices is 0, 1, 2, 3, 4, 5, 6, 7 as per the figure above.

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)
);

1.4.1.2.1.5. Block¶

Ordered list of vertex labels, number of nodes in three directions (x, y, z) and grading in three directions (x, y, z).

blocks
(
    hex (0 1 2 3 4 5 6 7) (20 20 1) simpleGrading (1 1 1)
);

1.4.1.2.1.6. Edges¶

This is blank because it is used to describe arc or spline edges.

edges
(
);

1.4.1.2.1.7. Boundary Conditions¶

This is a description of the boundary patches, using the vertex numbers.

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)
        );
    }
);

1.4.1.2.1.8. Merge Patch Pairs¶

This is blank because there is only one block, so no merging is needed.

mergePatchPairs
(
);

1.4.1.2.1.9. How to generate a mesh?¶

The mesh is generated by running

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavity
$ blockMesh

This creates the following subfolder:

constant
- polyMesh
  
  boundary
  
  faces
  
  neighbours
  
  owner
  
  points

1.4.1.2.2. Boundary and Initial Conditions¶

The ICs and BCs are set in this folder:

0
- p
- U

The components of the p and U files:

1.4.1.2.2.1. Dimensions¶

This specifies that kinematic pressure $m^2/s^2$ is being used, i.e. kinematic pressure $P = p/\rho_0$. The dimensions for u are m/s according to [M L T Temp Quantity Current Luminosity].

dimensions      [0 2 -2 0 0 0 0];

dimensions      [0 1 -1 0 0 0 0];

1.4.1.2.2.2. Internal Field¶

The internal field in given a value, a uniform value of 0 in this case for the scalar pressure and (0 0 0) for the velocity vector.

internalField   uniform 0;

internalField   uniform (0 0 0);

1.4.1.2.2.3. Boundary Field¶

This specified that the pressure gradient is zero on the moving and fixed walls. The fixed walls have a noslip condition and the moving wall as a velocity of 1m/s. On the front and back the 2D condition is specified i.e. empty.

boundaryField
{
    movingWall
    {
        type            zeroGradient;
    }

    fixedWalls
    {
        type            zeroGradient;
    }

    frontAndBack
    {
        type            empty;
    }
}

boundaryField
{
    movingWall
    {
        type            fixedValue;
        value           uniform (1 0 0);
    }

    fixedWalls
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    frontAndBack
    {
        type            empty;
    }
}

1.4.1.2.3. Physical Properties¶

The physical properties are located in this folder:

constant
- transportProperties

The Reynolds Number is 10, such that the kinematic viscosity must be 0.01, if the velocity is 1 and the characteristic length is 0.1m.

nu              [0 2 -1 0 0 0 0] 0.01;

1.4.1.2.4. Control¶

The control dictionary is located here:

system
- controlDict

This dictionary controls the time and reading and writing of the solution data and is described as follows:

1.4.1.2.4.1. Solver¶

This selects the incompressible, isothermal and laminar solver.

application     icoFoam;

1.4.1.2.4.2. Start and End Times¶

This sets the start and end times of the simulation. Usually the solution runs for 10 circulation times, which would be 10 x (0.1m / 1m/s) = 1s, however with hindsight, 0.5s is sufficient.

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         0.5;

1.4.1.2.4.3. Timestep¶

The timestep is set according to the Counrant Number. For a Courant Number of 1, a velocity of 1, a spatial step of 0.1/20 = 0.005m, the timestep is 0.005s.

deltaT          0.005;

1.4.1.2.4.4. Write Interval¶

In order to write out the data (U and p for the icoFoam solver) every 0.1s, we must specify a write interval of 20.

writeInterval   20;

1.4.1.2.4.5. Additional Settings¶

The additional settings are given below for the control dictionary, and are probably not changed very much from case to case.

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

1.4.1.2.5. Finite Volume Discretisation Schemes¶

The finite volume discretisation scheme selection is made in fvSchemes:

system
- fvSchemes

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear orthogonal;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         orthogonal;
}

1.4.1.2.6. Finite Volume Solvers¶

The selection of the finite volume solvers is made in fvSolution. In a closed incompressible system such as the cavity, pressure is relative: it is the pressure range that matters not the absolute values. In cases such as this, the solver sets a reference level by pRefValue in cell pRefCell. In this example both are set to 0. Changing either of these values will change the absolute pressure field, but not, of course, the relative pressures or velocity field.

system
- fvSolution

solvers
{
    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-06;
        relTol          0.05;
    }

    pFinal
    {
        $p;
        relTol          0;
    }

    U
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-05;
        relTol          0;
    }
}

PISO
{
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
}

1.4.1.3. Viewing the Mesh ¶

ParaView is loaded

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavity
$ paraFoam

Load the mesh:

cavity.OpenFOAM is loaded.
Properties > Mesh Parts > Click X by Mesh Parts
Properties > Apply

Change the colors:

Properties > Display > Representation > Wireframe
Properties > Coloring > Solid Color > Edit > Black
Properties > View > Background > Single color > White

Change the representation:

Layout > Toggle to 2D (if 3D)
Click in white area

1.4.1.4. Running the Application ¶

Run the application

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavity
$ icoFoam

Or with the optional case argument

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavity
$ icoFoam -case $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavity

The progress of the job is written to the terminal window. It tells the user the current time, maximum Courant number, initial and final residuals for all fields.

1.4.1.5. Post-processing ¶

1.4.1.5.1. Contours¶

ParaView is loaded

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavity
$ paraFoam

Load the mesh:

cavity.OpenFOAM is loaded.
Properties > Mesh Parts > Click X by Mesh Parts
Properties > Apply

Colours:

Properties > Representation > Surface
Last Frame
Properties > Coloring > Rescale
Properties > Background = White
Properties > Coloring > Edit > Choose Preset > Blue to Red Rainbow
Properties > Coloring > Edit > Save Current Colormap as default
Properties > Coloring > Edit > Edit Color Legend Properties > Title Text = Pressure (Pa)
Properties > Lighting > Specular = 1
Move legend to central position

1.4.1.5.2. Slice¶

Hold left mouse button to rotate view
Filters > Slice (icon)
Properties > Origin = 0.05, 0.05, 0.005
Properties > Normal = 0, 0, 1
Properties > Apply
Filters > Contour (icon) I’m not sure this adds anything
Properties > Contour by > p I’m not sure this adds anything
Isosurfaces > Range = 10 I’m not sure this adds anything

1.4.1.5.3. Vectors, slice¶

Outline:

Remove the eye from Slice and Contour filters
cavity.OpenFOAM > Representation > Outline
cavity.OpenFOAM > Coloring > Solid Colour > Black
cavity.OpenFOAM > Orientation Axes > Orentiation Axes Labrl Color > Black

Cell Centres:

Filter > Alphabetical > Cell Centres
CellCenters1 > Coloring > U
Apply

Arrows:

Filter > Alphabetical > Glyph
Glyph1 > scalars: p, vectors: U
Apply

To Save State:

File > Save State > contours_vectors.pvsm

1.4.1.5.4. Streamlines¶

Streamlines:

Filter > Alphabetical > Stream Tracer
Properties > Seeds > Seed Type > High Res Line Source
P1 = 0.05 0 0.005, P2 = 0.05 0.1 0.005
Resolution = 21
Max step = 0.5
Initial step = 0.2
Direction = BOTH
Type = Runge-Kutta-4-5
Properties > Coloring > U
Apply

Tube:

Filter > Alphabetical > Tube
Tube1 > Radius Factor = 10, Number of Sides = 6, Radius = 0.0003
Apply

1.4.1.6. Increased Mesh Resolution ¶

Increase mesh density by a factor of 2
Map results of coarser mesh onto finer mesh
Compare results of fine and coarse mesh

1.4.1.6.1. Create new case from existing case¶

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity
$ mkdir cavityFine
$ cp -r cavity/constant cavityFine
$ cp -r cavity/system cavityFine
$ cd cavityFine

1.4.1.6.2. Create fine mesh - How to re-generate a mesh?¶

Open blockMeshDict file and change (20 20 1) to (40 40 1), i.e.

blocks
(
    hex (0 1 2 3 4 5 6 7) (40 40 1) simpleGrading (1 1 1)
);

Now run blockMesh to generate the constant folder:

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavityFine
$ blockMesh

1.4.1.6.3. How to map the coarse mesh results onto the fine mesh?¶

Open controlDict file and change startTime 0 to startTime 0.5

startTime       0.5;

Check the predicates of mapFields

mapFields -help

Now map coarse to fine grid (consistent is used because the boundary conditions, boundary types and geometry are identical):

mapFields ../cavity -consistent

1.4.1.6.4. Control adjustments - How to maintain a Courant number of 1?¶

To maintain a Courant number of 1, the timestep must be halved, as the spatial step was halved.

Open controlDict file and change deltaT 0.005 to deltaT 0.0025

deltaT       0.0025;

Also specify output every 0.1 seconds by changing writeControl timeStep to writeControl runTime and writeInterval 20 to writeInterval 0.1:

writeControl    runTime;
writeInterval   0.1;

Also specify an end time of 0.7 seconds, by changing endTime 0.5 to endTime 0.7;

endTime    0.7;

1.4.1.6.5. How to run the code in the background?¶

This will send the output to a file called log and then view it with cat.

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavityFine
$ icoFoam > log &
$ cat log

1.4.1.6.6. How to do a vector plot comparing unrefined with a refined mesh?¶

Create files with .OpenFOAM extension:

$ cd $FOAM_RUN/1_tutorials/1_lid_driven_cavity/cavity
$ paraFoam -touch
$ cd ../cavityFine
$ paraFoam -touch
$ paraFoam