CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

How to add a passive scalar to the simpleFoam solver

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree6Likes
  • 4 Post By Uyan
  • 1 Post By Sugajen
  • 1 Post By Uyan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 13, 2014, 16:18
Default How to add a passive scalar to the simpleFoam solver
  #1
Member
 
Join Date: Feb 2014
Posts: 61
Rep Power: 8
Uyan is on a distinguished road
Hi all,

I am new to OpenFOAM software. I ran a simulation of a Jet in a crossflow simulation using simpleFoam. I need to add a passive scalar transportation equation to the simpleFoam solver.

I went through the following example.
http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

But my problem of including passive scalar transportation equation with a turbulent Schmidt number is slightly different from this example.

So, How do I add a passive scalar transport equation to the simpleFoam solver?

Appreciate any guidance on this issue.

Thank you.
Uyan is offline   Reply With Quote

Old   February 20, 2015, 12:50
Default For anyone searching for the solution for this problem.
  #2
Member
 
Join Date: Feb 2014
Posts: 61
Rep Power: 8
Uyan is on a distinguished road
For anyone who is trying to solve a problem like this i am posting the method i followed.

create a TEqn as of other UEqn and PEqn for the passive scalar.

Code:
 {
    volScalarField kappaEff
    (
        "kappaEff",
         (turbulence->nut()/Prt) +(turbulence->nu()/Pr)
     );

    fvScalarMatrix TEqn
    (
      fvm::div(phi, T)
      - fvm::laplacian(kappaEff, T)
    );

    TEqn.relax();     

    TEqn.solve();

}
Then add the T field into createFields.H header file.

Code:
    Info<< "Reading field T\n" <<endl;
    volScalarField T
    (
      IOobject
      (
         "T",
         runTime.timeName(),
         mesh,
         IOobject::MUST_READ,
         IOobject::AUTO_WRITE
       ),
      mesh
    );

Then include the TEqn into simpleFoam.C after turbulence correction.

Code:
         turbulence->correct();
          #include "TEqn.H"
Then add a line to read turbulent Prandtl number from transportProperties dictionary.
Code:
   singlePhaseTransportModel laminarTransport(U, phi);
  

     dimensionedScalar Pr(laminarTransport.lookup("Pr"));

     dimensionedScalar Prt(laminarTransport.lookup("Prt"));
Don't forget to rename simpleFoam.C and the change Make/files to get a new application.

This example was also useful.
https://openfoamwiki.net/index.php/H...ure_to_icoFoam
Uyan is offline   Reply With Quote

Old   June 21, 2017, 21:04
Default Solution diverging
  #3
Member
 
Sugajen
Join Date: Jan 2012
Location: Tempe, USA
Posts: 52
Rep Power: 10
Sugajen is on a distinguished road
Hi all,

I followed the procedure as posted by Uyan and found that the scalar transport solution diverging. But the scalar is transported throughout the region as expected. What could be the cause of divergence? It does not make sense to me since the solution looks acceptable, it is the divergence bothering me Below is the output from OF, fvSchemes, fvSolution and U BC. Attached are the solver and case files.

All comments and suggestions are welcome

output
Code:
Time = 101

smoothSolver:  Solving for Ux, Initial residual = 0.00120042, Final residual = 3.7046e-06, No Iterations 4
smoothSolver:  Solving for Uy, Initial residual = 0.00120393, Final residual = 3.70971e-06, No Iterations 4
smoothSolver:  Solving for Uz, Initial residual = 0.000836939, Final residual = 2.79653e-06, No Iterations 4
GAMG:  Solving for p, Initial residual = 4.31652e-05, Final residual = 8.86733e-07, No Iterations 9
time step continuity errors : sum local = 3.83691e-06, global = 4.17804e-07, cumulative = 0.00012566
GAMG:  Solving for CF, Initial residual = 0.685496, Final residual = 0.513947, No Iterations 1000
ExecutionTime = 211.28 s  ClockTime = 212 s


    From function virtual bool Foam::regIOobject::readIfModified()
    in file db/regIOobject/regIOobjectRead.C at line 291
    
    Re-reading object controlDict from file "/home/ipalab/OpenFOAM/ipalab-4.1/simplefoamexample/system/controlDict"
Time = 102

smoothSolver:  Solving for Ux, Initial residual = 0.00118109, Final residual = 3.65892e-06, No Iterations 4
smoothSolver:  Solving for Uy, Initial residual = 0.001184, Final residual = 3.66113e-06, No Iterations 4
smoothSolver:  Solving for Uz, Initial residual = 0.000818525, Final residual = 2.73043e-06, No Iterations 4
GAMG:  Solving for p, Initial residual = 4.16364e-05, Final residual = 8.8246e-07, No Iterations 9
time step continuity errors : sum local = 3.81498e-06, global = 4.26037e-07, cumulative = 0.000126086
GAMG:  Solving for CF, Initial residual = 0.684755, Final residual = 0.514736, No Iterations 1000
ExecutionTime = 214.31 s  ClockTime = 215 s
fvScheme
Code:
ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      bounded Gauss linearUpwind grad(U);
    div(phi,nuTilda) bounded Gauss linearUpwind grad(nuTilda);
    div((nuEff*dev2(T(grad(U))))) Gauss linear;
    div(phi,CF)      bounded Gauss linearUpwind grad(CF);
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

wallDist
{
    method meshWave;
}
fvSolution
Code:
solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0.01;
        smoother        GaussSeidel;
    }

    CF 
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0.01;
        smoother        GaussSeidel;
    };

    U
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-08;
        relTol          0.01;
    }

    nuTilda
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-08;
        relTol          0.01;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;

    residualControl
    {
        p               1e-5;
        U               1e-5;
        nuTilda         1e-5;
	CF		1e-5;
    }
}

relaxationFactors
{
    fields
    {
        p               0.3;
	CF		0.3;
    }
    equations
    {
        U               0.7;
        nuTilda         0.7;
    }
}
U
Code:
dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0.0 0.0 0.1);

boundaryField
{
    inlet
    {
        type            fixedValue;
        value		uniform (0.0 0.0 0.1);
    }

    outlet
    {
        type            zeroGradient;
    }

    xWalls
    {
        type            noSlip;
    }
    
    yWalls
    {
        type            noSlip;
    }
Attached Files
File Type: c my_simpleFoam.C (2.7 KB, 40 views)
File Type: txt transportProperties.txt (1.0 KB, 41 views)
File Type: txt turbulenceProperties.txt (991 Bytes, 23 views)
File Type: txt controlDict.txt (1.2 KB, 19 views)
cathaygrace likes this.
Sugajen is offline   Reply With Quote

Old   June 22, 2017, 10:37
Default
  #4
Senior Member
 
Troy Snyder
Join Date: Jul 2009
Location: Akron, OH
Posts: 198
Rep Power: 14
tas38 is on a distinguished road
Does your solution diverge using the original application, i.e. without transport of the passive scalar? This is the first thing I would check.
tas38 is offline   Reply With Quote

Old   June 22, 2017, 12:32
Default
  #5
Member
 
Join Date: Feb 2014
Posts: 61
Rep Power: 8
Uyan is on a distinguished road
Sugajen,

I think, how do you calculate diffusion term coefficient DS is the problem here.

Change the DS value and see how it affects the solver performance then you'll see it depends on DS value.

But why do you use a user defined diffusion coefficient in the first place?

If you look at my post #2,you'll see i have used the diffusion coefficient as a function of eddy viscosity.
Uyan is offline   Reply With Quote

Old   June 22, 2017, 14:58
Default
  #6
Member
 
Sugajen
Join Date: Jan 2012
Location: Tempe, USA
Posts: 52
Rep Power: 10
Sugajen is on a distinguished road
@Uyan I have constant diffusion coefficient. That is why making it user defined. But why would that matter?

@tas38 That's a good point. It does converge with simpleFoam
Sugajen is offline   Reply With Quote

Old   June 22, 2017, 17:36
Default
  #7
Member
 
Join Date: Feb 2014
Posts: 61
Rep Power: 8
Uyan is on a distinguished road
Sugen,


In my case i did not relax scalar equation , i simply solved the pressure velocity loop and then using that velocity i solved the scalar.

Even if i had used TEqn.relax() in the above code, i have not under relaxed the field. So it was a redundant statement.

Try without under relaxing. No need to under-relax a passive scalar.
Sugajen likes this.
Uyan is offline   Reply With Quote

Reply

Tags
passive scalar, schmidt, simplefoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
whats the cause of error? immortality OpenFOAM Running, Solving & CFD 12 July 11, 2019 17:33
passive scalar with simpleFoam Uyan OpenFOAM Programming & Development 2 March 1, 2016 10:07
compressible flow in turbocharger riesotto OpenFOAM 50 May 26, 2014 01:47
is internalField(U) equivalent to zeroGradient? immortality OpenFOAM Running, Solving & CFD 7 March 29, 2013 01:27
Climbing inlet pressure with simpleFoam and directMappedPatches chegdan OpenFOAM Running, Solving & CFD 1 January 2, 2012 19:35


All times are GMT -4. The time now is 05:45.