Week 8 - Simulation of a backward facing step in OpenFOAM

Aim :- Simulation of a backward facing step in OpenFOAM

Objective :-

• To simulate an incompressible-laminar-viscous flow through the backward facing step geometry and perform a transient simulation. The solver can be chosen based on the described physics of the flow. To explain the entire simulation procedure. To provide explanations to every change you make inside the reference case files obtained from OpenFOAM tutorials.
• To perform 2 case studies as described below and compare the results.

Case 1 - Simulate the flow without using any grading factor (i.e., GF = 1)

Case 2 - Simulate the flow with grading factor of 0.2. The cells should be finer near the walls (including the step wall).

Incompressible Flow :-

The flow in which there is no change in the density is called the Incompressible flow.

Laminar flow :-

A Laminar flow is one where the fluid motion is regular is no mixing. It can be visualised by the path lines that do not intersect each other. In fluid dynamics, laminar flow is characterized by fluid particles following smooth paths in layers, with each layer moving smoothly past the adjacent layers with little or no mixing.

At low velocities, the fluid tends to flow without lateral mixing and adjacent layers slide past one another. There are no cross-currents perpendicular to the direction of flow nor eddies or swirls of fluids mathematically. Reynolds number is the ratio of inertial force to the viscous force.

Viscous Flow :-

A type of fluid flow in which there is a continuous steady motion of the particles, the motion at a fixed point always remains constant. Also called streamline flow, laminar flow, steady flow.

Mesh specification :-

1. Number of cells along the x direction (longer dimension) = 200
2. Number of cells along the longer y direction = 20

Boundary Conditions :-

The domain specifications are provided in the following figure

Desired output :-

To measure the velocity profile at 0.085 m from the inlet of the geometry for both case studies and compare by using plot over line tool.

To explain why Grading/Growth factor is essential for meshing.

Procedure :-

To open the run folder in OpenFOAM in which we are going to run our simulations.

To open the tutorial by using the command- cd $FOAM_TUTORIALS"/incompressible/

To copy the cavity folder to the run folder so that the official file of OpenFOAM remain untouched.

To find out blockMesh script file to create domain space and provide mesh specification. In this case there are 21 vertices and 5 blocks. While creating the blocks we need to specify the number of mesh points needed along the x,y and z direction and also the simple grading should be done along the boundaries.

convertToMeters 0.01;

vertices
(
(0 0 0) //vertex 0
(8 0 0) //vertex 1
(8 0.5 0) //vertex 2
(0 0.5 0) //vertex 3
(8 1 0) //vertex 4
(0 1 0) //vertex 5
(20 1 0) //vertex 6
(20 0.5 0) //vertex 7
(20 0 0) //vertex 8
(20 -1 0) //vertex 9
(8 -1 0) //vertex 10
(0 0 1) //vertex 11
(8 0 1) //vertex 12
(8 0.5 1) //vertex 13
(0 0.5 1) //vertex 14
(8 1 1) //vertex 15
(0 1 1) //vertex 16
(20 1 1) //vertex 17
(20 0.5 1) //vertex 18
(20 0 1) //vertex 19
(20 -1 1) //vertex 20
(8 -1 1) //vertex 21
);

Code :-

BlockMesh dict :-

For the grading size 1 :

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.01;

vertices
(
    (0 0 0) //vertex 0
    (8 0 0) //vertex 1
    (8 0.5 0) //vertex 2
    (0 0.5 0) //vertex 3
    (8 1 0) //vertex 4
    (0 1 0) //vertex 5
    (20 1 0) //vertex 6
    (20 0.5 0) //vertex 7
    (20 0 0) //vertex 8
    (20 -1 0) //vertex 9
    (8 -1 0) //vertex 10
    (0 0 1) //vertex 11
    (8 0 1) //vertex 12
    (8 0.5 1) //vertex 13
    (0 0.5 1) //vertex 14
    (8 1 1) //vertex 15
    (0 1 1) //vertex 16
    (20 1 1) //vertex 17
    (20 0.5 1) //vertex 18
    (20 0 1) //vertex 19
    (20 -1 1) //vertex 20
    (8 -1 1) //vertex 21
);

blocks
(
    hex (0 1 2 3 11 12 13 14) (50 5 1) simpleGrading (1 1 1)
    hex (3 2 4 5 14 13 15 16) (50 5 1) simpleGrading (1 1 1)
    hex (2 7 6 4 13 18 17 15) (150 5 1) simpleGrading (1 1 1)
    hex (1 8 7 2 12 19 18 13) (150 5 1) simpleGrading (1 1 1)
    hex (10 9 8 1 21 20 19 12) (150 20 1) simpleGrading (1 1 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
        (
            (4 5 16 15)
            (6 4 15 17)
            (0 1 12 11)
            (10 9 20 21)
            (10 21 12 1)
        );
    }
);

mergePatchPairs
(
);

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

For grading size 0.2 :

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.01;

vertices
(
    (0 0 0) //vertex 0
    (8 0 0) //vertex 1
    (8 0.5 0) //vertex 2
    (0 0.5 0) //vertex 3
    (8 1 0) //vertex 4
    (0 1 0) //vertex 5
    (20 1 0) //vertex 6
    (20 0.5 0) //vertex 7
    (20 0 0) //vertex 8
    (20 -1 0) //vertex 9
    (8 -1 0) //vertex 10
    (0 0 1) //vertex 11
    (8 0 1) //vertex 12
    (8 0.5 1) //vertex 13
    (0 0.5 1) //vertex 14
    (8 1 1) //vertex 15
    (0 1 1) //vertex 16
    (20 1 1) //vertex 17
    (20 0.5 1) //vertex 18
    (20 0 1) //vertex 19
    (20 -1 1) //vertex 20
    (8 -1 1) //vertex 21
);

blocks
(
    hex (0 1 2 3 11 12 13 14) (50 5 1) simpleGrading (1 5 1)
    hex (3 2 4 5 14 13 15 16) (50 5 1) simpleGrading (1 0.2 1)
    hex (2 7 6 4 13 18 17 15) (150 5 1) simpleGrading (5 0.2 1)
    hex (1 8 7 2 12 19 18 13) (150 5 1) simpleGrading (5 5 1)
    hex (10 9 8 1 21 20 19 12) (150 20 1) simpleGrading (5 10 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
        (
            (4 5 16 15)
            (6 4 15 17)
            (0 1 12 11)
            (10 9 20 21)
            (10 21 12 1)
        );
    }
);

mergePatchPairs
(
);

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

Control dict :-

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     icoFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         20;

deltaT          1e-2;

writeControl    timeStep;

writeInterval   20;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;


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

Pressure File :-

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    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;
    }
}

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

Velocity File :-

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    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 (0.02 0 0);
    }

    outlet
    {
        type            zeroGradient;
    }

    walls
    {
        type            noSlip;
    }
}

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

Transport properties :-

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    location    "constant";
    object      transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

nu              [0 2 -1 0 0 0 0] 1e-5;


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

Results :-

Results are acquired after solving using the icofoam solver.

Grading Factor of 1 :

Mesh :

Velocity Field :

This filed is acquired by using the paraFoam command.

Pressure field :

Velocity profiles before and after time steps :

The plots are acquired by using the plot over line tool.

This graph predicts that the maximum velocity profile has decreased because of the change in area.

Grading Factor of 0.2 :

Mesh :

The cells are finer near the wall.

Velocity Field :

Pressure Field :

Velocity Field before the step :

Velocity profile after the step :

Velocity profile before and after the step :

Results :

If the mesh is not fine it gives average results because of capturing less elements at each node, To capture accurate results its required for finer mesh to capture flow properties of fluid. By comparing both the plots G.F-0.2 gives better reults than simple grading 1

Velocity magnitude profiles gives similar results for both cases in general at 0.085m there is an decrease in velocity but with a mesh grading factor finer results are obtained with accurate results at step height and boundary walls.

A graded mesh determines the element density in each region of the model based on the complexity of the geometry.More complex geometry with more angles and cuts will have a higher density of elements to better capture the topographical features. The mesh density grades away from the complex regions.