Validation studies of Symmetry vs Wedge in Open FOAM vs Analytical H.P equation
AIM:
The aim of this project is to simulate the fully developed Hagen Poiseuille’s flow (Re = 2100) through a circular pipe and compare the effect of the type of boundary used in the solution obtained.
PROCEDURE:
The assumptions for Hagen Poiseuille equations are to be considered here as well. Referenced from FM white’s fluid mechanics. Le = 0.06 x Re x D. Where D is the diameter of the pipe.
Le = 0.06 x 2100 x 0.01
Le = 1.26m
The hydrodynamic entrance length is the length of the pipe through which a fluid travels before becoming a fully developed flow. The flow would have the velocity profile as shown.
The above picture is taken from a Wikipedia article.
We assume that the pipe length is greater than the hydrodynamic entrance length. Lippe = 1.5 m
And since the fluid inside the pipe is water, we take the properties of water at NTP
C and 1atm
Density `rho=998frac{kg}{m^3}`
Dynamic Viscosity `mu=0.00089frac{Ns}{m^2}`
Kinematic Viscosity `nu = 1.005e-6 m^2/s`
`V_{avg}=frac{Re. mu}{rho.D}`= 0.187 m/s
`V_{max}=2.V_{avg}`= 0.374 m/s
`Delta P=frac{8.mu.L.V_{avg}}{r^2}` = 101.583 pa
`DeltaP_k=frac{Delta P}{rho}`= 0.101 (m/s) ^2
`tau=mu.frac{dx}{dy}`
We use the post-processing software i.e., Para View to plot shear stress graph
In the blockmeshdict file, we change the type to symmetry from wedge.
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)//0
(0.004981 0.000436 0)//1
(0.004981 -0.000436 0)//2
(0 0 1.500000)//3
(0.004981 0.000436 1.500000)//4
(0.004981 -0.000436 1.500000)//5
);
blocks
(
hex (0 2 1 0 3 5 4 3) (30 1 300)simpleGrading(0.2 1 1)
);
edges
(
arc 1 2 (0.005000 0 0)
arc 4 5 (0.005000 0 1.500000)
);
boundary
(
inlet
{
type patch;
faces
(
(0 2 1 0)
);
}
outlet
{
type patch;
faces
(
(3 5 4 3)
);
}
top
{
type wall;
faces
(
(2 1 4 5)
);
}
front
{
type symmetry;
faces
(
(0 3 4 1)
);
}
back
{
type symmetry;
faces
(
(0 2 5 3)
);
}
axis
{
type empty;
faces
(
(0 3 3 0)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //
The controlDict file should look something like this
/*--------------------------------*- 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 10;
deltaT 0.001;
writeControl timeStep;
writeInterval 20;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //
Now we need to set up the initial conditions, we make the same changes as we did in blockmeshdict here as well.
Once coded the files should look like this
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
{
inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0.0800;
}
axis
{
type empty;
}
top
{
type zeroGradient;
}
front
{
type symmetry;
}
back
{
type symmetry;
}
}
// ************************************************************************* //
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 (0 0 0.1874);
boundaryField
{
inlet
{
type fixedValue;
value uniform (0 0 0.1874);
}
outlet
{
type zeroGradient;
}
axis
{
type empty;
}
top
{
type fixedValue;
value uniform (0 0 0);
}
front
{
type symmetry;
}
back
{
type symmetry;
}
}
// ************************************************************************* //
To specify the type of fluid flowing inside the pipe we edit the transport properties file in the constant folder. In the transport properties file, we edit the nu value using a standard text editor and set it to 1.005e-6 m^2/s. Once edited the transport properties file should look like this.
/*--------------------------------*- 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] 1.005e-6;
// ************************************************************************* //
Now we run the following commands in the terminal
$blockMesh
$checkMesh (not required mostly but just to be sure)
$icoFoam
$paraFoam
In the Paraview once our geometry is loaded it should look like this.
10 degree 25 degree
45 degree
After running the simulation, the velocity profile would look like this. We used the plot over line tool in Para view to plot at the required location.
10 degree
symmetry wedge
25 degree
symmetry wedge
45 degree
symmetry wedge
To calculate the shear stress, we use the calculator tool in paraview to calculate the gradients and then multiply the gradients with mu to get the shear stress. The generated shear stress plot would look like this.
10 degree
symmetry wedge
25 degree
symmetry wedge
45 degree
symmetry wedge
CONCLUSION.
The results obtained are as follows
10 degree
| Parameters | Symmetry | Wedge | Analytical HP equation solution |
| Velocity (max) | 0.371963 | 0.371963 | 0.374m/s |
| shear stress (max) | 0.135149 | 0.13539 | 0.135 N/m2 |
25 degree
| Parameters | Symmetry | Wedge | Analytical HP equation solution |
| Velocity (max) | 0.372234 | 0.372233 | 0.374m/s |
| shear stress (max) | 0.137835 | 0.137835 | 0.135 N/m2 |
45 degree
| Parameters | Symmetry | Wedge | Analytical HP equation solution |
| Velocity (max) | 0.372795 | 0.372795 | 0.374m/s |
| shear stress (max) | 0.145382 | 0.145382 | 0.135 N/m2 |
- From the above results, we can say that the results obtained for both wedge type and symmetry type do not have much difference between them and they comply with the analytical solution.
- Also, both the conditions seem to be grid-independent. While execution time changes with the grid size, it is also observed that on running both the conditions in OpenFOAM, the execution time needed for the symmetry condition is more than the wedge condition.