Simulation of flow through backward facing step using icoFoam solver
Aim: To perform a simulation of flow in bacward facing step using openFoam software.
Objective:
1) To generate mesh using BlockMeshdict file for three grading factors.
Case 1, grading factor = 0.2
Case 2, grading factor = 0.5
Case 3, grading factor = 0.8
2) To solve the case using icoFoam solver.
3) To plot the velocity and pressure variation near backward facing step.
Geometry:
Calculating Minimum cell size (dx), Time step (dt) and end time of simulation (t):
Minimum cell size
Time step value
End time for simulation
The minimum cell size for non-uniform mesh is determined and time step value for max CFL number is calculated and the end time for simulation is calculated.
Initial condition:
Velocity initial condition
/*--------------------------------*- C++ -*----------------------------------*
========= |
/ F ield | OpenFOAM: The Open Source CFD Toolbox
/ O peration | Website: https://openfoam.org
/ A nd | Version: 8
/ 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 (0.5 0 0);
}
Outlet
{
type zeroGradient;
}
Front
{
type empty;
}
Back
{
type empty;
}
Noslip
{
type noSlip;
}
}
Pressure initial condition
/*--------------------------------*- C++ -*----------------------------------*
========= |
/ F ield | OpenFOAM: The Open Source CFD Toolbox
/ O peration | Website: https://openfoam.org
/ A nd | Version: 8
/ 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;
}
Front
{
type empty;
}
Back
{
type empty;
}
Noslip
{
type zeroGradient;
}
}
// ************************************************************************* //The initial condition of flow velocity and pressure is provided in the 0 zero directory in openfoam. For inlet boundary, velocity of 0.5 m/s is specified as the initial condition, this type of boundary condition is dirichlet boundary condition. For outlet boundary, kinematic pressure of zero gradient is specified as boundary condition, this type of boundary is known as neumann boundary condition.
Simulation time parameters:
Control dict file
/*--------------------------------*- C++ -*----------------------------------*
========= |
/ F ield | OpenFOAM: The Open Source CFD Toolbox
/ O peration | Website: https://openfoam.org
/ A nd | Version: 8
/ M anipulation |
*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application icoFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 0.4;
deltaT 6e-4;
writeControl timeStep;
writeInterval 100;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //The controldict file contains the simulation parameters such as time step value, simulation start time, end time and interval for writing output.
Fluid property
/*--------------------------------*- C++ -*----------------------------------*
========= |
/ F ield | OpenFOAM: The Open Source CFD Toolbox
/ O peration | Website: https://openfoam.org
/ A nd | Version: 8
/ M anipulation |
*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
nu [0 2 -1 0 0 0 0] 1.86e-5;
// ************************************************************************* //The transport properties file contains the fluid viscosity which defines the reynold's number. In this case, air is taken as fluid whose viscosity is 1.86e-5 m^2/s at 300K.
Mesh generation:
Case 1
BlockMeshDict file for grading factor 0.2
/*--------------------------------*- C++ -*----------------------------------*
========= |
/ F ield | OpenFOAM: The Open Source CFD Toolbox
/ O peration | Website: https://openfoam.org
/ A nd | Version: 8
/ M anipulation |
*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.001;
vertices
(
(0 0 0)
(100 0 0)
(100 5 0)
(0 5 0)
(100 10 0)
(0 10 0)
(200 10 0)
(200 5 0)
(200 0 0)
(200 -5 0)
(100 -5 0)
(0 0 1)
(100 0 1)
(100 5 1)
(0 5 1)
(100 10 1)
(0 10 1)
(200 10 1)
(200 5 1)
(200 0 1)
(200 -5 1)
(100 -5 1)
);
blocks
(
hex (0 1 2 3 11 12 13 14) (100 3 1) simpleGrading (0.2 5 1)
hex (3 2 4 5 14 13 15 16) (100 3 1) simpleGrading (0.2 0.2 1)
hex (2 7 6 4 13 18 17 15) (100 3 1) simpleGrading (5 0.2 1)
hex (1 8 7 2 12 19 18 13) (100 3 1) simpleGrading (5 5 1)
hex (10 9 8 1 21 20 19 12) (100 4 1) simpleGrading (5 5 1)
);
edges
(
);
boundary
(
Inlet
{
type patch;
faces
(
(0 11 14 3)
(3 14 16 5)
);
}
Outlet
{
type patch;
faces
(
(7 6 17 18)
(8 7 18 19)
(9 8 19 20)
);
}
Front
{
type empty;
faces
(
(12 13 14 11)
(13 15 16 14)
(18 17 15 13)
(19 18 13 12)
(20 19 12 21)
);
}
Back
{
type empty;
faces
(
(3 5 4 2)
(0 3 2 1)
(2 4 6 7)
(1 2 7 8)
(10 1 8 9)
);
}
Noslip
{
type wall;
faces
(
(15 4 5 16)
(17 6 4 15)
(21 12 1 10)
(11 0 1 12)
(21 10 9 20)
);
}
);
mergePatchPairs
(
);
Mesh for grading factor 0.2 :
Case 2
Blockmeshdict file for grading factor 0.5
/*--------------------------------*- C++ -*----------------------------------*
========= |
/ F ield | OpenFOAM: The Open Source CFD Toolbox
/ O peration | Website: https://openfoam.org
/ A nd | Version: 8
/ M anipulation |
*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.001;
vertices
(
(0 0 0)
(100 0 0)
(100 5 0)
(0 5 0)
(100 10 0)
(0 10 0)
(200 10 0)
(200 5 0)
(200 0 0)
(200 -5 0)
(100 -5 0)
(0 0 1)
(100 0 1)
(100 5 1)
(0 5 1)
(100 10 1)
(0 10 1)
(200 10 1)
(200 5 1)
(200 0 1)
(200 -5 1)
(100 -5 1)
);
blocks
(
hex (0 1 2 3 11 12 13 14) (100 3 1) simpleGrading (0.5 2 1)
hex (3 2 4 5 14 13 15 16) (100 3 1) simpleGrading (0.5 0.5 1)
hex (2 7 6 4 13 18 17 15) (100 3 1) simpleGrading (2 0.5 1)
hex (1 8 7 2 12 19 18 13) (100 3 1) simpleGrading (2 2 1)
hex (10 9 8 1 21 20 19 12) (100 4 1) simpleGrading (2 2 1)
);
edges
(
);
boundary
(
Inlet
{
type patch;
faces
(
(0 11 14 3)
(3 14 16 5)
);
}
Outlet
{
type patch;
faces
(
(7 6 17 18)
(8 7 18 19)
(9 8 19 20)
);
}
Front
{
type empty;
faces
(
(12 13 14 11)
(13 15 16 14)
(18 17 15 13)
(19 18 13 12)
(20 19 12 21)
);
}
Back
{
type empty;
faces
(
(3 5 4 2)
(0 3 2 1)
(2 4 6 7)
(1 2 7 8)
(10 1 8 9)
);
}
Noslip
{
type wall;
faces
(
(15 4 5 16)
(17 6 4 15)
(21 12 1 10)
(11 0 1 12)
(21 10 9 20)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //Mesh for grading factor 0.5 :
Case 3
Blockmeshdict file for grading factor 0.8
/*--------------------------------*- C++ -*----------------------------------*
========= |
/ F ield | OpenFOAM: The Open Source CFD Toolbox
/ O peration | Website: https://openfoam.org
/ A nd | Version: 8
/ M anipulation |
*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.001;
vertices
(
(0 0 0)
(100 0 0)
(100 5 0)
(0 5 0)
(100 10 0)
(0 10 0)
(200 10 0)
(200 5 0)
(200 0 0)
(200 -5 0)
(100 -5 0)
(0 0 1)
(100 0 1)
(100 5 1)
(0 5 1)
(100 10 1)
(0 10 1)
(200 10 1)
(200 5 1)
(200 0 1)
(200 -5 1)
(100 -5 1)
);
blocks
(
hex (0 1 2 3 11 12 13 14) (100 3 1) simpleGrading (0.8 1.25 1)
hex (3 2 4 5 14 13 15 16) (100 3 1) simpleGrading (0.8 0.8 1)
hex (2 7 6 4 13 18 17 15) (100 3 1) simpleGrading (1.25 0.8 1)
hex (1 8 7 2 12 19 18 13) (100 3 1) simpleGrading (1.25 1.25 1)
hex (10 9 8 1 21 20 19 12) (100 4 1) simpleGrading (1.25 1.25 1)
);
edges
(
);
boundary
(
Inlet
{
type patch;
faces
(
(0 11 14 3)
(3 14 16 5)
);
}
Outlet
{
type patch;
faces
(
(7 6 17 18)
(8 7 18 19)
(9 8 19 20)
);
}
Front
{
type empty;
faces
(
(12 13 14 11)
(13 15 16 14)
(18 17 15 13)
(19 18 13 12)
(20 19 12 21)
);
}
Back
{
type empty;
faces
(
(3 5 4 2)
(0 3 2 1)
(2 4 6 7)
(1 2 7 8)
(10 1 8 9)
);
}
Noslip
{
type wall;
faces
(
(15 4 5 16)
(17 6 4 15)
(21 12 1 10)
(11 0 1 12)
(21 10 9 20)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //Mesh for grading factor 0.8 :
The blockmeshdict file contains the details of geometry, boundaries, number of cells and mesh grading factor.
Results:
Velocity plot for Case 1
Velocity plot for Case 2
Velocity plot for Case 3
Pressure plot for Case 1
Pressure plot for Case 2
Pressure plot for Case 3
Velocity contour
Pressure contour
Velocity streamline contour
Flow separation and vortex formation
The contours obtained in the case 1 provides more detail compared to other two cases, hence the velocity contour from case 1 is selected for observing the flow separation, point of separation, point of reattchment and vortex formation.
From the above figure, it can be observed that the stream of fluid starts to dettach itself near the step and this point is known as the point of flow separation. And at a certain length after the backward facing step, the stream of fluid flow stop recirculating and joins the rest of the flow, this point is known as point of reattachment. A region of low pressure is created just after the backward facing step where recirculating and backward flow occurs, this region is called as separated flow region. In the separated flow region, formation of circulating fluid structures takes place and these structures are known as vortices.