[kkpal]

hi everyone!
I've been doing simulation about flow around cylinder recently.
Some information about the case is listed below.

2D simulation;
U=1, D=1, rho=1, nu=0.01, so Re=100;
domain size: upstream 20D, downstream 40D, topwall and bottom wall 20D.
mesh size: about 40000 vertices

The problem is that no matter how I tried, I can not get the accurate result in terms of strouhal number, which in my case is 1.44. An accurate St for RE100 should be 1.65.

Could someone send me a similar case file which has been verified and yields accurate results so I can check what went wrong in my own case? I will be very grateful!
my email address is kai-zhang-kf@ynu.ac.jp

[sasanghomi]

Hi ,
I think you use icoFoam as a solver. So I think two parameters have vital role for getting the exact result : 1) discretization method of terms in equations 2)Mesh generation.
So change your fvSchemes and fvSolution as below :

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM Extend Project: Open Source CFD        |
|  \\    /   O peration     | Version:  1.6-ext                               |
|   \\  /    A nd           | Web:      www.extend-project.de                 |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver           PCG;
        preconditioner   DIC;
        tolerance        1e-06;
        relTol           0;
    };

    U
    {
        solver         BiCG;
        preconditioner   DILU;
        tolerance        1e-05;
        relTol           0;
    };
}


PISO
{
   nCorrectors    2;
   nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
 }

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM Extend Project: Open Source CFD        |
|  \\    /   O peration     | Version:  1.6-ext                               |
|   \\  /    A nd           | Web:      www.extend-project.de                 |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default backward;
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss GammaV 0.5 ;

}

laplacianSchemes
{
    default         Gauss linear limited 0.5;
    laplacian(nu,U) Gauss linear limited 0.5;
    laplacian(rUA,pcorr) Gauss linear limited 0.5;
    laplacian(rAU,p) Gauss linear limited 0.5;
}

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

snGradSchemes
{
    default         limited 0.5;
}

fluxRequired
{
    default         no;
    pcorr;
    p;
}

Hope this helps,
Sasan.

[kkpal]

dear sasan
thanks very much! your post solved the problem, I used icoFoam this time, now my St number is 1.62, which is much better than the previous ones. Now it is clear that it is not the problem of my mesh, but the discretization method of terms in equations that is giving me bad results.

However, in my previous simulations, I used pimpleFoam because for the long run I need to do much higher Re simulations, for which icoFoam is not appropriate.

Here is my fvschemes and fvsolutions, which is for pimpleFoam and did not give right result.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0.01;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    pFinal
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    "(U|k|epsilon)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }

    "(U|k|epsilon)Final"
    {
        $U;
        tolerance       1e-05;
        relTol          0;
    }
}

PIMPLE
{
    nOuterCorrectors 1;
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
}

relaxationFactors
{
    fields
    {
    }
    equations
    {
        "U.*"           0.9;
        "k.*"           1;
        "epsilon.*"     1;
    }
}


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

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    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;
    grad(p)         Gauss linear;
    grad(U)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss limitedLinearV 1;
    div(phi,k)      Gauss limitedLinear 1;
    div(phi,epsilon) Gauss limitedLinear 1;
    div(phi,R)      Gauss limitedLinear 1;
    div(R)          Gauss linear;
    div(phi,nuTilda) Gauss limitedLinear 1;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         none;
    laplacian(nuEff,U) Gauss linear corrected;
    laplacian((1|A(U)),p) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DepsilonEff,epsilon) Gauss linear corrected;
    laplacian(DREff,R) Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

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

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}


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

It seems that settings in pimpleFoam is much more complex than those in icoFoam, can you guide me how to make adjustment to these files?

[kkpal]

I just tried changing the settings in pimpleFoam to the ones you provided, hoping that it would also give good result, but it did not.
It seems in my case ,icoFoam does a better job than pimpleFoam.

or pimpleFoam requires something other different settings?

[kkpal]

dear sasan
I think I found the cause for the inaccuracy of the Str number in pimpleFoam.

http://www.cfd-online.com/Forums/openfoam-solving/94785-icofoam-vs-pisofoam-laminar.html

in this thread it is noted that relaxation may affect the Str number. So I removed the relaxation parameters and magically the good result came out!! Though I don't know what is the particular reason for this improvement.

it is found out that for unsteady cases relaxation is more than necessary. however, in pimpleFoam relaxation is allowable, should we never use relaxation in pimpleFoam when dealing with unsteady cases?

[sasanghomi]

Hi kia ,
You are welcome .
I tried to simulate turbulent flow around a cylinder with pisoFoam 6-7 month ago.But I had some problems and the case didn't converge and amplitude of Lift didn't get a fix value(oscillation was not regular ). Actually I didn't succeed to simulate the flow accurately.
About relaxation factor I should say that I have heard when you use PISO algorithm for solving equations if you use relaxation factor only final result (after convergence) is accurate.
Anyway I am interested in simulation of turbulent flow around a cylinder and I will try to do it.
Let me know your progress.

Thanks and best regards,
Sasan.

[sherandlock]

Hi Sasan,

Thank you for your help very much.

This is my error. When time is 1.45s. I have no idea why this is happenning, Would you like to enlighten me a little bit?

Courant Number mean: 1.11225e+91 max: 2.80651e+96
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/yzhou/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/home/yzhou/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/yzhou/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#4 Foam::fvMatrix<Foam::Vector<double> >::solve(Foam::dictionary const&) in "/home/yzhou/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/bin/icoFoam"
#5 Foam::fvMatrix<Foam::Vector<double> >::solve() in "/home/yzhou/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/bin/icoFoam"
#6 main in "/home/yzhou/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/bin/icoFoam"
#7 __libc_start_main in "/lib64/libc.so.6"
#8 Foam::UOPstream::write(char) in "/home/yzhou/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/bin/icoFoam"
Floating exception

[sasanghomi]

Hi sherandlock ,

Your case has diverged . The Courant number is very high . So I only have one idea ,
Try to use adjustTimeStep in the controlDict. Add below lines in the controlDict :

adjustTimeStep  yes; 
 
maxCo           0.5; 
 
maxDeltaT       0.01;

Hope this helps.

[Maimouna]

Dear Sasan,

I'm try to implement flow past circular cylinder in pimpleFoam solver. I attached the case that I'm looking for (pdf file). I blocked and checked mesh everything was fine. I run the case without any problem. But, when I plotted drag and lift forces (using Matlab), it gave me inconvenience result. I don't know where is my mistake.

Anyway, I attached my case if you could please go through all files and checked please what are my mistakes.

NT: D = 1, Re = 100. I'm trying to fix nu in transportProperties file and change u in the attached file because I didn't know where are my errors so I'm trying to do different ways. Also, might blockMeshDict affects my results if you could check please.

Many thanks in advanced.

[sasanghomi]

Hi,

There is no attached file, honestly!

best regards.

[Maimouna]

Hi Sasan,

sorry, I attached them again.

Looking forward for your help.

[kkpal]

I think at Re=100, turbulence model will jeopardize your result. In this regime the flow is mainly 2 dimensional and could be regarded as not turbulent.

Originally Posted by Maimouna

Dear Sasan,

I'm try to implement flow past circular cylinder in pimpleFoam solver. I attached the case that I'm looking for (pdf file). I blocked and checked mesh everything was fine. I run the case without any problem. But, when I plotted drag and lift forces (using Matlab), it gave me inconvenience result. I don't know where is my mistake.

Anyway, I attached my case if you could please go through all files and checked please what are my mistakes.

NT: D = 1, Re = 100. I'm trying to fix nu in transportProperties file and change u in the attached file because I didn't know where are my errors so I'm trying to do different ways. Also, might blockMeshDict affects my results if you could check please.

Many thanks in advanced.

[Maimouna]

Dear Kai Zhang,

I'm working in laminar not turbulence model.

Have I changed my solver from pimpleFoam to another solver or that does not affect?

What other changes would be supposed?

Regards

[alexeym]

Originally Posted by Maimouna

I'm working in laminar not turbulence model.

According to your case files, you're working with oneEqEddy LES model for the turbulence. If you'd like to run simulation for laminar case you need to:

1. Put RASModel in constant/turbulenceProperties
2. Put

RASModel        laminar;

turbulence      off;

printCoeffs     on;

in constant/RASProperties.

Also I'd suggest you to change fvSolution:

PIMPLE
{
    nOuterCorrectors 10;
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;

    residualControl
    {
        "(U|p)"
        {
             tolarance 1e-4;
             relTol 0;
        }
    }
}

to be sure that you have converged solution on every time step.

[Maimouna]

Dear Alexey,

many thanks for your reply. I did all changes that you supposed. After typing pimpleFoam in the command window, I got this error
[QUOTE]

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | foam-extend: Open Source CFD |
| \\ / O peration | Version: 3.0 |
| \\ / A nd | Web: http://www.extend-project.de |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 3.0-8d34057e525d
Exec : pimpleFoam
Date : Mar 04 2014
Time : 10:40:09
Host : maimouna-desktop
PID : 3105
CtrlDict : /home/maimouna/foam/foam-extend-3.0/etc/controlDict
Case : /home/maimouna/foam/foam-extend-3.0/tutorials/incompressible/pimpleFoam/circularCylinderModified
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0.000000e+00

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RASModel
Selecting RAS turbulence model laminar


--> FOAM FATAL IO ERROR:
keyword turbulence is undefined in dictionary "/home/maimouna/foam/foam-extend-3.0/tutorials/incompressible/pimpleFoam/circularCylinderModified/constant/RASProperties"

file: /home/maimouna/foam/foam-extend-3.0/tutorials/incompressible/pimpleFoam/circularCylinderModified/constant/RASProperties from line 18 to line 82.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 395.

FOAM exiting

maimouna@maimouna-desktop:~/foam/foam-extend-3.0/tutorials/incompressible/pimpleFoam/circularCylinderModified$

What does this error mean?

[alexeym]

Well,

Post your RASProperties file, otherwise I can only suggest that RASProperties file is incorrect

[Maimouna]

This is RASProperties file

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

RASModel laminar; //oneEqEddy;

delta cubeRootVol;

printCoeffs on;

cubeRootVolCoeffs
{
deltaCoeff 1;
}

PrandtlCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

maxDeltaRatio 1.1;
}

Cdelta 0.158;
}

vanDriestCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

maxDeltaRatio 1.1;
}

Aplus 26;
Cdelta 0.158;
}

smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

maxDeltaRatio 1.1;
}


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

Regards

[alexeym]

Well, can you please tell me the difference between what you've posted and what I've suggested to put into RASProperties?

Can you create a file with just

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.2                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

RASModel        laminar;

turbulence      off;

printCoeffs     on;


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

?

The error you've got tells you that there's no turbulence keyword in RASProperties files, and in fact there's no such keyword in your file.

[Maimouna]

Dear Alexey,

sorry for that mistakes.

I is running now. I will let you know about the result.

Many thanks

[Maimouna]

Dear Alexy,

the running is done.
I have two questions please
1. in cotrolDict file (attached)
startTime 0;
endTime 25.0;
deltaT 0.01;

but the running is completed after 1.4, why?

 /*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     pimpleFoam;

startFrom       latestTime;

startTime       0;

stopAt          endTime;

endTime         25.0;

deltaT          0.01; //1e-04

writeControl    adjustableRunTime;

writeInterval   0.1; //5.0e-1

purgeWrite      0;

writeFormat     binary;

writePrecision  6;

writeCompression uncompressed;

timeFormat      scientific;

timePrecision   6;

runTimeModifiable yes;

adjustTimeStep    yes;

maxCo             0.5;

maxDeltaT         2.0e-3;

functions
{
    probes
    {
        type            probes;
        functionObjectLibs ("libsampling.so");
        enabled         true;
        outputControl   timeStep;
        outputInterval  1;
        probeLocations
        (
            ( 0.05   0.0   0.002 )
            ( 0.05   0.01  0.002 )
            ( 0.05   0.01  0.002 )
            ( 0.05   0.01  0.002 )
            ( 0.05   0.01  0.002 )
            ( 0.05   0.01  0.002 )
            ( 0.05   0.01  0.002 )
        );

        fields
        (
            p
        );
    }

    forces
    {
        type        forceCoeffs;
        functionObjectLibs ( "libforces.so" );
        outputControl timeStep;
        outputInterval 1;
        patches
        (
            walls
        );
            directForceDensity no;

        pName       p;
        UName       U;
        rhoName     rhoInf;
        //log         true;
        rhoInf      994.5;
        CofR        ( 0 0 0 );
        liftDir     ( 0 1 0 );
        dragDir     ( 1 0 0 );
        pitchAxis   ( 0 0 1 );
        magUInf     1.787e-4; //1; //0.54
        lRef        0.04;
        Aref        0.0157;
        Aref1        0.004;
        rhoRef      994.5;
    }

    fieldAverage1
    {
        type            fieldAverage;
        functionObjectLibs ("libfieldFunctionObjects.so");
        enabled         true;
        outputControl   outputTime;
        fields
        (
            U
            {
                mean        on;
                prime2Mean  on;
                base        time;
            }

            p
            {
                mean        on;
                prime2Mean  on;
                base        time;
            }
        );
    }
}


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

2. the drag chart is given as attached. Why? I know the drag coefficient figure is tottaly different, whats the wrong?

Best regards