Simulating the Flow over backward facing step using icoFoam solver

We shall modify the cavity tutorial folder of icoFoam solver to solve the given problem.

The files are modified as shown below

control/

blockMeshDict file:

/*--------------------------------*- C++ -*----------------------------------*\\
  =========                 |
  \\\\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\\\    /   O peration     | Website:  https://openfoam.org
    \\\\  /    A nd           | Version:  7  
     \\\\/     M anipulation  |
\\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

vertices
(
    (0 0 0)//0
    (0.08 0 0)//1
    (0.08 0.005 0)//2
    (0 0.005 0)//3
    (0.08 0.01 0)//4
    (0 0.01 0)//5
    (0.2 0.01 0)//6
    (0.2 0.005 0)//7
    (0.2 0 0)//8
    (0.2 -0.01 0)//9
    (0.08 -0.01 0)//10

    (0 0 0.002)//11
    (0.08 0 0.002)//12
    (0.08 0.005 0.002)//13
    (0 0.005 0.002)//14
    (0.08 0.01 0.002)//15
    (0 0.01 0.002)//16
    (0.2 0.01 0.002)//17
    (0.2 0.005 0.002)//18
    (0.2 0 0.002)//19
    (0.2 -0.01 0.002)//20
    (0.08 -0.01 0.002)//21
);

blocks
(
    hex (0 1 2 3 11 12 13 14) (80 5 1) simpleGrading (0.2 5 1)
    hex (3 2 4 5 14 13 15 16) (80 5 1) simpleGrading (0.2 0.2 1)
    hex (2 7 6 4 13 18 17 15) (120 5 1) simpleGrading (5 0.2 1)
    hex (1 8 7 2 12 19 18 13) (120 5 1) simpleGrading (5 5 1)
    hex (10 9 8 1 21 20 19 12) (120 10 1) simpleGrading (5 5 1)
);

edges
(
);

boundary
(
    inlet
    {
        type patch;
        faces
        (
            (0 11 14 3)
            (3 14 16 5)
        );
    }
    outlet
    {
        type patch;
        faces
        (
            (9 8 19 20)
            (8 7 18 19)
            (7 6 17 18)
        );
    }
    walls
    {
        type wall;
        faces
        (
            (5 16 15 4)
            (4 15 17 6)
            (11 0 1 12)
            (21 10 9 20)
            (1 10 21 12)
        );
    }
    frontAndBack
    {
        type empty;
        faces
        (
            (0 3 2 1)
            (3 5 4 2)
            (2 4 6 7)
            (1 2 7 8)
            (10 1 8 9)
            (11 12 13 14)
            (14 13 15 16)
            (13 18 17 15)
            (12 19 18 13)
            (21 20 19 12)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //

controlDict file:

deltaT should be chosen such that the courant number would not go above 1 over the entire simulation.

Courant number is given by

`C=U*(∆t)/(∆x+∆y)`

/*--------------------------------*- C++ -*----------------------------------*\\
  =========                 |
  \\\\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\\\    /   O peration     | Website:  https://openfoam.org
    \\\\  /    A nd           | Version:  7  
     \\\\/     M anipulation  |
\\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    \"system\";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     icoFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         0.1;

deltaT          0.0001;

writeControl    timeStep;

writeInterval   1;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;


// ************************************************************************* //

Initial conditions are located in 0/

p file: (Kinematic pressure)

/*--------------------------------*- C++ -*----------------------------------*\\
  =========                 |
  \\\\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\\\    /   O peration     | Website:  https://openfoam.org
    \\\\  /    A nd           | Version:  7  
     \\\\/     M anipulation  |
\\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }

    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }

    walls
    {
        type            zeroGradient;
    }

    frontAndBack
    {
        type            empty;
    }
}

// ************************************************************************* //

U file: (Velocity)

/*--------------------------------*- C++ -*----------------------------------*\\
  =========                 |
  \\\\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\\\    /   O peration     | Website:  https://openfoam.org
    \\\\  /    A nd           | Version:  7  
     \\\\/     M anipulation  |
\\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 0);

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

    outlet
    {
        type            zeroGradient;
    }

    walls
    {
        type            noSlip;
    }

    frontAndBack
    {
        type            empty;
    }
}

// ************************************************************************* //

./Allrun command in the terminal solves the problem

We also need to post-process the results using paraFoam command

OUTPUT:

Velocity contours for different grading factors near walls

Grading factor = 0.2

Grading factor = 0.5

Grading factor = 0.8

• Flow seperation at the step is smooth for grading factor 0.8 than 0.5 than 0.2
• This may be due to the fact that grading 0.2 at the bottom wall increased the size of the cell near the step in Y direction
• Grading factor of 1 would have given even better results

Velocity profile plots at x = 0.085 for various grading factors:

• Velocity profile for grading factor of 0.8 is smooth because the cells are finer than those in other cases
• Grading should be done in such a way that the cells surrounding the step are finer
• Velocity at the surface of walls is zero