2D simulation of flow over a square obstacle using openfoam
Aim : To calculate velocity contour and dragforce on a square obstacle placed in the air field and to automate the simulation process in openfoam
Geometry :
The geometry is created by blockMeshDict file in Openfoam.
Input data :
velocity at inlet = 10 m/sec
Temperature at inlet = 25 deg c
Reynolds number= Re = density*velocity*charecterstic length / dynamic viscosity
At 25 deg
dynamic viscosity of air =1.849 * 10 ^-05
density of air = 1.184
Re= 6.403 * 10^5
So renolds number is greater than 5 * 10^5
Flow is clearly turbulent. In order to capture the turbulence accurately RANS K-epsillon model is used.
BlockmeshDict 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;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(0 0 -0.5)
(3.5 0 -0.5)
(4.5 0 -0.5)
(10 0 -0.5)
(10 1.5 -0.5)
(10 2.5 -0.5)
(10 4 -0.5)
(4.5 4 -0.5)
(3.5 4 -0.5)
(0 4 -0.5)
(0 2.5 -0.5)
(0 1.5 -0.5)
(3.5 1.5 -0.5)
(4.5 1.5 -0.5)
(4.5 2.5 -0.5)
(3.5 2.5 -0.5)
(0 0 0.5)
(3.5 0 0.5)
(4.5 0 0.5)
(10 0 0.5)
(10 1.5 0.5)
(10 2.5 0.5)
(10 4 0.5)
(4.5 4 0.5)
(3.5 4 0.5)
(0 4 0.5)
(0 2.5 0.5)
(0 1.5 0.5)
(3.5 1.5 0.5)
(4.5 1.5 0.5)
(4.5 2.5 0.5)
(3.5 2.5 0.5)
);
blocks
(
hex (0 1 12 11 16 17 28 27) (10 15 1) simpleGrading (1 1 1)
hex (11 12 15 10 27 28 31 26) (10 10 1) simpleGrading (1 1 1)
hex (10 15 8 9 26 31 24 25) (10 15 1) simpleGrading (1 1 1)
hex (15 14 7 8 31 30 23 24) (20 15 1) simpleGrading (1 1 1)
hex (1 2 13 12 17 18 29 28) (20 15 1) simpleGrading (1 1 1)
hex (14 5 6 7 30 21 22 23) (20 15 1) simpleGrading (1 1 1)
hex (13 4 5 14 29 20 21 30) (20 15 1) simpleGrading (1 1 1)
hex (2 3 4 13 18 19 20 29) (20 15 1) simpleGrading (1 1 1)
);
edges
(
);
boundary
(
pressure-outlet
{
type patch;
faces
(
(3 4 20 19)
(4 5 21 20)
(5 6 22 21)
);
}
velocity-inlet
{
type patch;
faces
(
(11 0 16 27)
(10 11 27 26)
(9 10 26 25)
);
}
upper-wall
{
type symmetryPlane;
faces
(
(6 7 23 22)
(7 8 24 23)
(8 9 25 24)
);
}
lower-wall
{
type symmetryPlane;
faces
(
(0 1 17 16)
(1 2 18 17)
(2 3 19 18)
);
}
obstacle-wall
{
type wall;
faces
(
(15 12 28 31)
(14 15 31 30)
(12 13 29 28)
(13 14 30 29)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //
ControlDict 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 simpleFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 1;
deltaT 1e-4;
writeControl timeStep;
writeInterval 200;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //
THe solver used here is simpleFoam solver and the simulation is run for one sec with time step of 1e-4.
Transport properties :
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
transportModel Newtonian;
nu [0 2 -1 0 0 0 0] 1.56165e-05;
// ************************************************************************* //
kinematic viscosity at 25 degree of temperature is taken
Turbulent 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 "constant";
object momentumTransport;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
model kEpsilon;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //
Here KEpsilon model is selected.
The emperical correlations required to find the turbulent properties are
where I is the Intensity
so k and w properties are calculated by using the above emperical relations.
Boundary condtions:
velocity :
/*--------------------------------*- 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 (10 0 0);
boundaryField
{
velocity-inlet
{
type fixedValue;
value uniform (10 0 0);
}
pressure-outlet
{
type zeroGradient;
}
upper-wall
{
type symmetryPlane;
}
lower-wall
{
type symmetryPlane;
}
obstacle-wall
{
type noSlip;
}
}
// ************************************************************************* //
pressure :
/*--------------------------------*- 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
{
velocity-inlet
{
type zeroGradient;
}
pressure-outlet
{
type fixedValue;
value uniform 0;
}
upper-wall
{
type symmetryPlane;
}
lower-wall
{
type symmetryPlane;
}
obstacle-wall
{
type zeroGradient;
}
}
// ************************************************************************* //
k 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 volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.13574;
boundaryField
{
velocity-inlet
{
type fixedValue;
value uniform 0.13574;
}
pressure-outlet
{
type zeroGradient;
}
upper-wall
{
type symmetryPlane;
}
lower-wall
{
type symmetryPlane;
}
obstacle-wall
{
type kqRWallFunction;
value uniform 0.13574;
}
}
// ************************************************************************* //
epsilon :
/*--------------------------------*- 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;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
internalField uniform 0.117167;
boundaryField
{
velocity-inlet
{
type fixedValue;
value uniform 0.117167;
}
pressure-outlet
{
type zeroGradient;
}
upper-wall
{
type symmetryPlane;
}
lower-wall
{
type symmetryPlane;
}
obstacle-wall
{
type epsilonWallFunction;
value uniform 0.117167;
}
}
// ************************************************************************* //
The simpleFoam solver is called and the equations are solved in parallel computing method.
Mesh :
output files:
velocity contour :
velocity vector field:
Drag force calculation :
The obstacle is to be removed from the surface seperately by using ExtractBlock tool
Then the surface is generated by SurfaceExtract
normal vectors should be generated to find the x normals and y normals
now calculator is opened in paraview the product of p*x-Normal is stored as drag
Now its is integrated to obtain the Drag force.
Mesh-refinement strategy:
The mesh can be refined at the obstacle surface by changing the mesh grading factor in the blockMeshDict file. The cell volume is formed according to the grading factor given in that file.
Reduction of Computational time:
The simulation time can be reduced by performing renumberMesh and a proper time scale is to be selected so as to satisfy the courant number criteria.
Automated Allrun file:
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
application=$(getApplication)
runApplication $application
paraFoam
#------------------------------------------------------------------------------
It can be further automated by using function codes.
Conclusion:
simulation is performed sucessfully by using Openfoam