TUTORIAL 04: CFD ANALYSIS OF WATER FALLING ON CYLINDRICAL SURFACE USING INTERFOAM SOLVER
Tutorial 04: CFD analysis of water falling on cylindrical surface using interfoam solver of OPENFOAM.
Figure 4.1 (a) Initial volume fraction (VF) of water Contour of free water falling with BCs
Figure 4.1 (b) Meshed domain of water falling
Problem Identification
In this problem investigation of free water falling using OPENFOAM is proposed for multi phase modeling (free water falling cooling), in which water is flow in free water falling from prescribed location section from top initial condition (see figure), which is assumed at surface of top side wall (See the following figure). Air and water properties are selected from literature available in digital medium. Outlet is at top of the domain which is selected for continuity effect of free water falling system. Some assumptions are applied in this problem like initial room temperature is assumed at constant value for this problem (ISOTHERMAL). Air and water properties are also assumed constant for this problem.
“interFoam” is selected as solver for this problem. Open Foam software is installed on Win 7, provided by FSD blueCAPE Lda: http://bluecfd.com/
Note: This tutorial is not endorsed/ supported by provider of software's which are used in this tutorial. This tutorial is made for educational purpose only.
Figure4.2 Different Boundary Conditions
The simulation is solved for ambient conditions at transient flow scheme available in selected solver.
Pre-Processing
This problem is selected as laminar flow problem, so the solver must have capability to solve laminar flow conditions, that’s why “interFoam” is selected as solver. The very first step is import suitable mesh file in open-foam software. There are various methods available in software to read mesh file, but we use “fluentMeshToFoam” command to read *.msh file generated by Ansys Fluent® software. It is required to make a folder in home directory (Folder Name wflow) of your open-foam software, where important sub-folders are already presented (see the following figure). At starting only three folders are availble 0, constant and system, which is copied from open foam tutorial. In this case folders are copied from interFoam tutorials.
Figure 4.3 Folder in home directory for this tutorial
After desired folder creation, run open-foam software (see the following figure)
Figure 4.4 Run Open-Foam using blueCFD terminal
Run “ls” command in this terminal to verify the user created folder (see the following figure)
Figure 4.5 ls command to check the folders in home directory
After verification of user folder (wflow), run “cd” command to enter in this folder (see the following figure)
Figure 4.6 cd command to enter desired folder
Run “fluentMeshToFoam” command in terminal (see the following figure), it must be ensure by user that msh file is available in main folder by run command “ls” again, in this tutorial wflow.msh file is used (copy from tutorial available in Google drive link)
Figure 4.7 ls command to verify msh file
Figure 4.8 mesh command to convert msh file in poly mesh file
This command create a sub-folder named polymesh in sub-folder constant which we create in starting phase of problem. (see the following figure )
In polymesh folder various files are created. These files have geometry information of wflow.msh but our consideration is on boundary file (red highlighted in figure)
Figure 4.9 Polymesh folder created by “fluentMeshToFoam” command
Note down all boundary names created from msh file can be see by open the boundary file available in polymesh folder using word-pad/notepad (see the following figure)
Boundary Conditions
After creation of polymesh in constant folder, its time to create boundary files in directory 0 created by user in starting part of the problem. The boundary files depend on governing equations which will be solved during numerical simulation, for this problem the main variables(total four variables) which must be solved are present in the following figure
Figure 4.11 Boundary conditions for present problem
There are large number of boundary conditions are available, which must be provide to boundary conditions for every problems, the selection is depend on type of boundary conditions useful for particular problem. In this tutorial some important boundary conditions are used all detail information is provided in last of this tutorial book. All files are created using note-pad-2 (provided in software package)
Note: We copy these files from tutorial available in open-foam program files (see the following figure)
Figure 4.12 Copy pee-generated files for present problem
Now edit these boundary files as per given details for all boundary conditions:
Alpha.water.orig boundary condition for free water falling problem
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
leftwall
{
type zeroGradient;
}
rightwall
{
type zeroGradient;
}
lowerwall
{
type zeroGradient;
}
balls
{
type zeroGradient;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
frontAndBackPlanes
{
type empty;
}
}
// ************************************************************************* //
P_rgh boundary condition for free water falling problem
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
leftwall
{
type fixedFluxPressure;
value uniform 0;
}
rightwall
{
type fixedFluxPressure;
value uniform 0;
}
lowerwall
{
type fixedFluxPressure;
value uniform 0;
}
balls
{
type fixedFluxPressure;
value uniform 0;
}
atmosphere
{
type totalPressure;
p0 uniform 0;
}
frontAndBackPlanes
{
type empty;
}
}
// ************************************************************************* //
U boundary condition for free water falling problem
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
leftwall
{
type noSlip;
}
rightwall
{
type noSlip;
}
lowerwall
{
type noSlip;
}
balls
{
type noSlip;
}
atmosphere
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
frontAndbackPlanes
{
type empty;
}
}
// ************************************************************************* //
Fluid Flow Properties (Transport and Turbulence)
These properties are present in directory constant where polymesh is available, the process is same like previous section. For simplicity copy these files from tutorial available in open-foam program files path for selected solver.
Source code for g
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class uniformDimensionedVectorField;
location "constant";
object g;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -2 0 0 0 0];
value (0 -9.81 0);
// ************************************************************************* //
Source code for Transport Properties
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
phases (water air);
water
{
transportModel Newtonian;
nu 1e-06;
rho 1000;
}
air
{
transportModel Newtonian;
nu 1.48e-05;
rho 1;
}
sigma 0.07;
// ************************************************************************* //
Source code for Turbulence Properties
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType laminar;
// ************************************************************************* //
Time/Solver (Input-Output)
Like other CFD software, Open-Foam is also required time size as per requirement of problem. This task is fulfill by creating controlDict file in directory “system”
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application interFoam;
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 5;
deltaT 0.0005;
writeControl adjustableRunTime;
writeInterval 0.02;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression uncompressed;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep yes;
maxCo 1;
maxAlphaCo 1;
maxDeltaT 1;
// ************************************************************************* //
decomposeParDict is not required in this problem so no need to discuss here
Numerical Schemes
The numerical schemes are defined in file fvSchemes available in directory system created by user in starting phase of problem.
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
div(rhoPhi,U) Gauss linearUpwind grad(U);
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss linear;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
// ************************************************************************* //
Solution Control
Solution is controlled by making file fvSolution in directory system
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"alpha.water.*"
{
nAlphaCorr 2;
nAlphaSubCycles 1;
cAlpha 1;
MULESCorr yes;
nLimiterIter 5;
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-8;
relTol 0;
}
"pcorr.*"
{
solver PCG;
preconditioner DIC;
tolerance 1e-5;
relTol 0;
}
p_rgh
{
solver PCG;
preconditioner DIC;
tolerance 1e-07;
relTol 0.05;
}
p_rghFinal
{
$p_rgh;
relTol 0;
}
U
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-06;
relTol 0;
}
}
PIMPLE
{
momentumPredictor no;
nOuterCorrectors 1;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
equations
{
".*" 1;
}
}
// ************************************************************************* //
setFieldsDict
This command is used for initialize the secondary phase (in this problem water is secondary phase) in fluid domain. As seen in figure, water is initially at top of the domain, so a boxtocell command is used to set water volume fraction to 1 using this command.
Figure set fields
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 5 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
defaultFieldValues
(
volScalarFieldValue alpha.water 0
);
regions
(
boxToCell
{
box (0.05 0.75 -1) (0.45 0.95 1);
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
);
// ************************************************************************* //
Run this command using
cp 0/alpha.water.orig 0/alpha.water
Alpha water command
After run this command, alpha.water is created in 0 folder
Solver Running
After created the all desired source files for present problem only last step is to run the solver by provide the command “” (see the following figure)
Figure 4.13 command for run the solver
Figure 4.14 Solver running in open-foam code
After successful ending of solver running condition, various sub-folders are created in user directory free water falling for different time conditions
Post-Processing
In this step solved problem is analysis by using para-foam software available with open-foam software. To run this software run command “para-foam” in terminal of open-foam software. It must take care that terminal selected free water falling folder before run this command.
Figure 4.15 para-foam for post-processing of problem
Para-view is very large software for post-processing of CFD simulation files so in this tutorial we skip this software at this stage. Only some important results are present here.
Water Volume Fraction Contours
Velocity Contours
This offering is not approved or endorsed by OpenCFD Limited, producer and distributor of the OpenFOAM software and owner of the OPENFOAM® and OpenCFD® trade marks.
END
Comments
Post a Comment