CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Convergence Problem icoFoam steady flow over an airfoil (http://www.cfd-online.com/Forums/openfoam-solving/83636-convergence-problem-icofoam-steady-flow-over-airfoil.html)

Lucas January 5, 2011 22:18

Convergence Problem icoFoam steady flow over an airfoil
 
Hi everyone,

I am trying to simulate steady flow over an airfoil and I'm having problems converging to the solution with icoFoam.

I'm using a ICEM mesh that i exported to fluent format (msh) and converted with
fluentMesh3DToFoam:

I am working with a comparation between OpenFOAM and CFX,
but i am new at OF.

The utility checkMesh set Mesh OK.

This is my case:
http://uploaddearquivos.com.br/downl...o/PROIC.tar.gz

Thank you.

Lucas January 6, 2011 09:49

I tried this morning some changes in the fvschemes fvsolution
I also tried to run in simpleFoam

and i got this:

Code:

Time = 52

Lookup gradScheme for grad(U)
Lookup divScheme for div((nuEff*dev(grad(U).T())))
Lookup laplacianScheme for laplacian(nuEff,U)
Lookup fluxRequired for U
Lookup gradScheme for snGradCorr(U)
Lookup gradScheme for snGradCorr(U)
Lookup gradScheme for snGradCorr(U)
Lookup divScheme for div(phi,U)
Find relax for U
Lookup relaxationFactor for U
Lookup gradScheme for grad(p)

    From function solution::solverDict(const word&)
    in file matrices/solution/solution.C at line 241
    Lookup solver for U
smoothSolver:  Solving for Ux, Initial residual = 0.0237871, Final residual = 0.000128133, No Iterations 1
smoothSolver:  Solving for Uy, Initial residual = 0.317853, Final residual = 0.00208853, No Iterations 1
smoothSolver:  Solving for Uz, Initial residual = 8.9633e-05, Final residual = 4.39538e-07, No Iterations 1
Lookup interpolationScheme for interpolate(U)


--> FOAM FATAL ERROR:
Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux              : 3.36963e+38
Specified mass inflow  : 1.60459e+38
Specified mass outflow  : 0
Adjustable mass outflow : 4.20186e+20


    From function adjustPhi(surfaceScalarField& phi, const volVectorField& U,const volScalarField& p
    in file cfdTools/general/adjustPhi/adjustPhi.C at line 115.

FOAM exiting

hear is my system files:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.7.1                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.com                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application    simpleFoam;  //  which solver (for documentation)

startFrom      startTime;              //  firstTime, startTime, latestTime

startTime      0;                      //  set > 0 to continue

stopAt          endTime;                //  writeNow, endTime, nextWrite, ...

endTime        600;                    //  Latest timestep allowed

deltaT          1;                      //  simple counter for steadyState

writeControl    adjustableRunTime;      //  or uncommon: cpuTime, clockTime

writeInterval  50;                    //  time step write interval

purgeWrite      0;                      //  1 recycles time steps storage
                                        //  0 keeps all time steps on disk

writeFormat    ascii;                  //  ascii: readable, binary: smaller

writePrecision  6;                      //  precision for ascii format

writeCompression uncompressed;          //  compressed for gzipped files

timeFormat      general;                //  fixed, scientific or general

timePrecision  6;                      //  precision for time handling

runTimeModifiable yes;                  //  yes: OF reads dictionaries each
                                        //  time step

graphFormat    raw;                    //  raw, gnuplot, xmgr, jplot

//libs()        for user libraries, p.e. user boundary conditions
//functions()  for special functions

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.7.1                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.com                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default        steadyState;
}

gradSchemes
{
    default        Gauss linear;
    grad(p)        faceLimited leastSquares 0 1;
    grad(U)        Gauss linear;
}

divSchemes
{
    default        none;
    div(phi,U)      Gauss upwind;
    div(phi,nuTilda) Gauss linearUpwind Gauss linear;
    div((nuEff*dev(grad(U).T()))) Gauss linear;
}

laplacianSchemes
{
    default        none;
    laplacian(nuEff,U) Gauss linear limited 0.7;
    laplacian((1|A(U)),p) Gauss linear limited 0.7;
    laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
    laplacian(1,p)  Gauss linear corrected;
}

interpolationSchemes
{
    default        linear;
    interpolate(U)  linear;
}

snGradSchemes
{
    default        limited 0.7;
}

fluxRequired
{
    default        no;
    p              ;
}


// ************************************************************************* //

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.7.1                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.com                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        tolerance      1e-07;
        relTol          0.001;
        smoother        GaussSeidel;
        nPreSweeps      1;
        nPostSweeps    2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 500;
        agglomerator    faceAreaPair;
        mergeLevels    1;
    }

    U
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps        2;
        tolerance      1e-08;
        relTol          0.01;
    nSweeps        1;              // setting for smoothSolver
        maxIter        100;            // limitation of iterations number

    }

    nuTilda
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps        2;
        tolerance      1e-08;
        relTol          0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 6;
    convergence        1e-5;
    pRefCell        0;
    pRefValue      0;
}

relaxationFactors
{
    default        0;
    p              0.003;
    U              0.007;
    nuTilda        0.007;
}


// ************************************************************************* //


tcarrigan January 6, 2011 12:08

For the gradSchemes try:
default cellLimited leastSquares 1.0;

For the divSchemes try:
div(phi,U) Gauss linearUpwindV Gauss linear;
div(phi,nuTilda) Gauss upwind;

For pressure solver:
p GAMG tolerance 1e-8 and relTol 0

For other solvers:
PBiCG using DILU preconditioner with tolerances 1e-8 and relTol 0 rather than using smoothSolver

Try also dropping the nNonOrthogonalCorrectors down to 2, and increase the relaxation factors:
p 0.2
U 0.5
nuTilda 0.5

Lucas January 10, 2011 15:24

thanks for your reply, but the problem was the mesh, i changed the mesh and
everything works fine.

billynoe February 17, 2011 18:24

Quote:

Originally Posted by Lucas (Post 289911)
thanks for your reply, but the problem was the mesh, i changed the mesh and
everything works fine.

what did you change in your mesh? smaller cell sizes?

Lucas February 18, 2011 13:46

In fact i made a complete new mesh, because the last was horrible, with high number of non-orthogonal cells.


All times are GMT -4. The time now is 00:51.