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

rhoSimpleFoam vs rhoPimpleFoam, steady state vs transient solver

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

Like Tree10Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 16, 2022, 06:23
Smile rhoSimpleFoam vs rhoPimpleFoam, steady state vs transient solver
  #1
New Member
 
Join Date: May 2018
Posts: 18
Rep Power: 7
Oliver Meng is on a distinguished road
Hi lovely CFD people,

I have a question about steady state solver and transient solver (rhoSimpleFoam vs. rhoPimpleFaom). My case is a train running in a tunnel, with a velocity of 40 m/s. I run the case both with rhoSimpleFoam and rhoPimpleFoam. Of course, I would prefer rhoSimpleFoam if it converges (residuals under 1e-7 or -8).

My questions are:
a.What could be the reasons, why the rhoSimpleFoam does not converge?
b.Can I make the rhoSimpleFoam converge by manipulating fvSchemes or FvSolutions?


Some more information:
My checkMesh shows that the Mesh is 100% ok.
The tunnel and the ground are slip. And the train is no slip. Velocity bc at inlet and pressure bc at outlet.


U:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2106                                  |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    arch        "LSB;label=32;scalar=64";
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (40 0 0);

boundaryField
{
    "tub.*"
    {
        type            slip;
        //value           uniform (0 0 0);
    }
    
    pod
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    
    noSlipGroundPod
    {
        type            slip;
        //value           uniform (0 0 0);
    }

    up
    {
        type            zeroGradient;
    }

    sides
    {
        type            zeroGradient;
    }


    front
    {
        type            fixedValue;
        value           $internalField;
    }


    back
    {
        type            zeroGradient;
    }
    
    "proc.*"
    {
        type    processor;
    }
}


// ************************************************************************* //
p:
Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1e5;

boundaryField
{
 #includeEtc "caseDicts/setConstraintTypes"
    
    "tub.*"
    {
         type           zeroGradient;
    }
    
    pod
    {
         type           zeroGradient;
    }

    noSlipGroundPod
    {
         type           zeroGradient;
    }

    up
    {
        type            zeroGradient;
    }

    sides
    {
        type            zeroGradient;
    }

    front
    {
        type            zeroGradient;
    }

    back
    {
        type            fixedValue;
        value           $internalField;
    }

    "proc.*"
    {
        type    processor;
    }
}


// ************************************************************************* //
k:
Code:
/*--------------------------------*- C++ -*----------------------------------*\

\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// k = 3/2*(I*U)^2
// Re = 4.75e5, U = 70, I = 0.01

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0.24;

boundaryField
{
    "tub.*"
    {
        type            fixedValue;
        value           $internalField;
    }
    
    pod
    {
        type            kqRWallFunction;
        value           uniform 0;
    }

    noSlipGroundPod
    {
        type            kqRWallFunction;
        value           uniform 0;
    }

    up
    {
        type            zeroGradient;
    }
    
    sides
    {
        type            zeroGradient;
    }

    front
    {
        type            fixedValue;
        value           $internalField;
    }

    back
    {
        type            zeroGradient;
    }

    "proc.*"
    {
        type    processor;
    }
    #includeEtc "caseDicts/setConstraintTypes"
}


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

omega:
Code:
/*--------------------------------*- C++ -*----------------------------------*\

\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


dimensions      [0 0 -1 0 0 0 0];

internalField   uniform 2.4e03;

boundaryField
{
    "tub.*"
    {
        type            omegaWallFunction;
        value           $internalField;
    }
    
    pod
    {
        type            omegaWallFunction;
        value           $internalField;
    }

    noSlipGroundPod
    {
        type            omegaWallFunction;
        value           $internalField;
    }

    up
    {
        type            zeroGradient;
    }
    sides
    {
        type            zeroGradient;
    }

    front
    {
        type            fixedValue;
        value           $internalField;
    }

    back
    {
        type            zeroGradient;
    }

    "proc.*"
    {
        type    processor;
    }

    #includeEtc "caseDicts/setConstraintTypes"
}


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

T:
Code:
/*--------------------------------*- C++ -*----------------------------------*\

\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 298;

boundaryField
{
    "tub.*"
    {
        type            fixedValue;
        value           $internalField;
    }
    
    pod
    {
        type            fixedValue;
        value           $internalField;
    }

    noSlipGroundPod
    {
        type            fixedValue;
        value           $internalField;
    }

    up
    {
        type            zeroGradient;
    }

    sides
    {
        type            zeroGradient;
    }

    front
    {
        type            fixedValue;
        value           $internalField;
    }

    back
    {
        type            zeroGradient;
    }

    "proc.*"
    {
        type    processor;
    }

    #includeEtc "caseDicts/setConstraintTypes"
}


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

alphat:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2106                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -1 0 0 0 0];

internalField   uniform 0;

boundaryField
{

    pod
    {
        type            compressible::alphatWallFunction;// calculated; 
        value           uniform 0;
    }
    
    "tub.*"
    {
        type            compressible::alphatWallFunction;// calculated; 
        value           uniform 0;
    }

    noSlipGroundPod
    {
        type            compressible::alphatWallFunction;// calculated; 
        value           uniform 0;
    }

    up
    {
        type            calculated;
        value           uniform 0;
    }
    sides
    {
        type            calculated;
        value           uniform 0;
    }

    front
    {
        type            calculated;
        value           uniform 0;
    }

    back
    {
        type            calculated;
        value           uniform 0;
    }

    "proc.*"
    {
        type    processor;
    }

    #includeEtc "caseDicts/setConstraintTypes"
}


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

nut:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2106                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 0;

boundaryField
{

    "tub.*"
    {
        type            nutUSpaldingWallFunction;
        value           uniform 0;
    }
    
    pod
    {
        type            nutUSpaldingWallFunction;
        value           uniform 0;
    }

    noSlipGroundPod
    {
        type            nutUSpaldingWallFunction;
        value           uniform 0;
    }

    up
    {
        type            calculated;
        value           uniform 0;
    }

    sides
    {
        type            calculated;
        value           uniform 0;
    }

    front
    {
        type            calculated;
        value           uniform 0;
    }

    back
    {
        type            calculated;
        value           uniform 0;
    }

    "proc.*"
    {
        type    processor;
    }

    #includeEtc "caseDicts/setConstraintTypes"
}


// ************************************************************************* //
SIMPLE-fvSchemes:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2106                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;

    limited         cellLimited Gauss linear 1;
    grad(U)         $limited;
    grad(k)         $limited;
    grad(omega)     $limited;
}

divSchemes
{
    default         none;

    div(phi,U)      Gauss linearUpwind limited;

    energy          Gauss linearUpwind limited;
    div(phi,e)      $energy;
    div(phi,K)      $energy;
    div(phi,Ekp)    $energy;

    turbulence      Gauss upwind;
    div(phi,k)      $turbulence;
    div(phi,omega)  $turbulence;

    div(phiv,p)     Gauss upwind;
    div((phi|interpolate(rho)),p) Gauss upwind;

    div(((rho*nuEff)*dev2(T(grad(U)))))    Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

wallDist
{
    method          meshWave;
}


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

SIMPLE-fvSolution:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2106                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        smoother        GaussSeidel;
        tolerance       1e-7;
        relTol          0.01;
    }

    pFinal
    {
        $p;
        relTol          0;
    }

    "(rho|U|k|omega|e)"
    {
        solver          PBiCGStab;
        preconditioner  DILU;
        tolerance       1e-7;
        relTol          1e-3;
    }

    "(rho|U|k|omega|e)Final"
    {
        $U;
        relTol          0;
    }
    
    cellDisplacement
    {
    solver          GAMG;
    smoother        GaussSeidel;
    tolerance       1e-7;
    relTol          0.01;
    }
    
}

SIMPLE
{
    residualControl
    {
        p               1e-8;
        U               1e-8;
        "(k|omega|e|nut)"   1e-8;
    }

    nNonOrthogonalCorrectors 1;
    pMinFactor      0.05;
    pMaxFactor      5;
}

PIMPLE
{
    nCorrectors              2;
    nNonOrthogonalCorrectors 1;
    nOuterCorrectors         1;
    pMinFactor      0.1;
    pMaxFactor      2;
}

relaxationFactors
{
    fields
    {
        p               0.25;
        rho             0.01; //0.01
    }
    equations
    {
        U               0.7;
        "(k|omega)"     0.7;
        e               0.01;
    }
}


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

PIMPLE-fvSchemes:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2106                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         CrankNicolson 0.9;
}

gradSchemes
{
    default         Gauss linear;

    limited         cellLimited Gauss linear 1;
    grad(U)         $limited;
    grad(k)         $limited;
    grad(omega)     $limited;
}

divSchemes
{
    default         none;

    div(phi,U)      Gauss linearUpwind limited;

    energy          Gauss linearUpwind limited;
    div(phi,e)      $energy;
    div(phi,K)      $energy;
    div(phi,Ekp)    $energy;

    turbulence      Gauss upwind;
    div(phi,k)      $turbulence;
    div(phi,omega)  $turbulence;

    div(phiv,p)     Gauss upwind;
    div((phi|interpolate(rho)),p) Gauss upwind;

    div(((rho*nuEff)*dev2(T(grad(U)))))    Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

wallDist
{
    method          meshWave;
}


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


PIMPLE-fvSolution:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2106                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        smoother        GaussSeidel;
        tolerance       1e-8;
        relTol          0.1;
    }

    pFinal
    {
        $p;
        relTol          0.1;
    }

    "(rho|U|k|omega|e)"
    {
        solver          PBiCGStab;
        preconditioner  DILU;
        tolerance       1e-8;
        relTol          1e-3;
    }

    "(rho|U|k|omega|e)Final"
    {
        $U;
        relTol          1e-3;
    }
}

SIMPLE
{
    residualControl
    {
        p               1e-8;
        U               1e-8;
        "(k|omega|e)"   1e-8;
    }

    nNonOrthogonalCorrectors 0;
    pMinFactor      0.01;
    pMaxFactor      5;
}

PIMPLE
{
    nCorrectors              2;
    nNonOrthogonalCorrectors 1;
    nOuterCorrectors         10;
    pMinFactor      0.01;
    pMaxFactor      5;
}

relaxationFactors
{
    fields
    {
        p               0.3;
        rho             0.01; //0.01
    }
    equations
    {
        U               0.7;
        "(k|omega)"     0.7;
        e               0.7;
    }
}


// ************************************************************************* //
Attached Images
File Type: jpg simple_residual.jpg (82.6 KB, 37 views)
File Type: jpg simple_Cd.jpg (65.1 KB, 34 views)
File Type: jpg pimple_residual.jpg (93.4 KB, 31 views)
File Type: png pimple_Cd.png (48.8 KB, 26 views)
Oliver Meng is offline   Reply With Quote

Old   June 17, 2022, 13:26
Default
  #2
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 666
Rep Power: 14
Tobermory will become famous soon enough
One of the difficulties I have observed is that the OpenFOAM solver schemes are very "clean" compared to commercial codes like StarCCM+ of Fluent, and this means that if you have a fine mesh, then there is very little numerical diffusion to stabilise the simulations. This means that flows over bluff bodies will start to show flow unsteadiness & shed turbulent structures into the wake.

I am not sure if this is relevant for your scenario, since we don't have a picture of your geometry, but have a think - is the solver just picking up inherent flow instability? If so, then you won't get full convergence with a steady solver ... unless you coarsen the mesh, which is not ideal! In these circumstances, you may have to run as a transient and field average over a number of shedding cycles.

Also, looking at your relaxation factors, I see you have tightened rho and e down to almost zero ... I know one of the tutorials has 0.01 for rho, but I find it difficult to believe that this is a good way to run the solver, i.e. basically to not update the rho or e equations ...

Good luck!
dlahaye, hogsonik and joshwilliams like this.
Tobermory is offline   Reply With Quote

Old   June 18, 2022, 05:43
Default
  #3
Senior Member
 
Josh Williams
Join Date: Feb 2021
Location: Scotland
Posts: 112
Rep Power: 5
joshwilliams is on a distinguished road
Quote:
Originally Posted by Tobermory View Post
Also, looking at your relaxation factors, I see you have tightened rho and e down to almost zero ... I know one of the tutorials has 0.01 for rho, but I find it difficult to believe that this is a good way to run the solver, i.e. basically to not update the rho or e equations ...

I agree with Tobermory. It seems like a strange concept to use a solver for rho but not really update rho (otherwise, why not just use simpleFoam?).
dlahaye and Tobermory like this.
joshwilliams is offline   Reply With Quote

Old   June 18, 2022, 06:35
Default
  #4
Senior Member
 
Domenico Lahaye
Join Date: Dec 2013
Posts: 722
Blog Entries: 1
Rep Power: 17
dlahaye is on a distinguished road
@tobermory: what criterium have you employed to access how "clean" OpenFoam is? Are you aware of any documentation that shows this "cleanness"?

@joshwilliams: the confusion might be that rho is updated (using equation of state) despite zero iterations for the rho-solve (recorded in the logfile).

Thx.
hogsonik and Tobermory like this.
dlahaye is offline   Reply With Quote

Old   June 18, 2022, 07:00
Default
  #5
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 666
Rep Power: 14
Tobermory will become famous soon enough
Domenico - the numerical cleanliness of OF depends on the schemes (divScheme, etc.) that you choose, of course, but in OF you can at least choose to run with very little artificial stability by using a good quality orthogonal mesh with little or no stretching, second order schemes etc. In the commercial codes even the second order convection schemes are typically blended 2nd/upwind schemes, to ensure stability ... which ofc is often more important in an industrial CFD situation, where a slightly less precise solution is better than no solution.

Indeed, after moving from StarCCM+ to OF, I was shocked at how often my simulations would blow up - it was a real trial at the start!
dlahaye likes this.
Tobermory is offline   Reply With Quote

Old   June 18, 2022, 17:29
Default
  #6
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
Rep Power: 34
arjun will become famous soon enougharjun will become famous soon enough
Quote:
Originally Posted by Tobermory View Post
Domenico - the numerical cleanliness of OF depends on the schemes (divScheme, etc.) that you choose, of course, but in OF you can at least choose to run with very little artificial stability by using a good quality orthogonal mesh with little or no stretching, second order schemes etc. In the commercial codes even the second order convection schemes are typically blended 2nd/upwind schemes, to ensure stability ... which ofc is often more important in an industrial CFD situation, where a slightly less precise solution is better than no solution.

Indeed, after moving from StarCCM+ to OF, I was shocked at how often my simulations would blow up - it was a real trial at the start!

the idea that if the solver is unstable than it must be more accurate compared to stable solver is completely not true.

It is more so not true when you compare OF against StarCCM. CCM does not add sort of artifical dissipation to make it stable and not only that its descretization is actually more accurate.

I personally have never found a case where starccm and of are compared and starccm came out to be less accurate.

Mostly if you benchmark you will find that starccm does better than OF.

I even have a study where most scheme of OF for convection terms were compared in a validation case and starccm was also one of the solver. Guess what there was hardly any scheme that was as good as starccm and around 40 scheme were compared.

Give me email i will send you the results.
dlahaye likes this.
arjun is offline   Reply With Quote

Old   June 19, 2022, 15:10
Default
  #7
Senior Member
 
Domenico Lahaye
Join Date: Dec 2013
Posts: 722
Blog Entries: 1
Rep Power: 17
dlahaye is on a distinguished road
@tobermory: thank you for sharing your thought on the matter. Much appreciated.

@arjun: thank you as well. Is the concern you share related to the fact the starccm is able to take advantage of polyhedral meshes in a way that OF is not?
dlahaye is offline   Reply With Quote

Old   June 20, 2022, 02:05
Default
  #8
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
Rep Power: 34
arjun will become famous soon enougharjun will become famous soon enough
Quote:
Originally Posted by dlahaye View Post
@tobermory: thank you for sharing your thought on the matter. Much appreciated.

@arjun: thank you as well. Is the concern you share related to the fact the starccm is able to take advantage of polyhedral meshes in a way that OF is not?


I used to be developer for starccm and I am probably only one to benchmark its flow model against manufactured solution and study it.


Later when i am writing Wildkatze solver, I am always benchmarking and validating solvers (last 7 years).

Having seen the code myself i know for sure that there is no artifical dissipation added the stability is due to much more accurate schemes used.

We have done lots of benchmarks sometimes we compare OF too just to know how it does.

For example for this case https://fvus.github.io/wildkatze/ver...itverification Tobi (who posts frequently on openfoam forums here too) was kind enough to test many convection schemes. The results do show that openfoam is more dissipative actually (this case actually is the test of it).


Even last two weeks we are testing a test problem and it turned out OF is most dissipative and starccm is least to the point that it ends up generating lots of noise in solution due to it. Starccm tries to maintain the signal while OF pretty much diffuses it.
arjun is offline   Reply With Quote

Old   June 20, 2022, 03:53
Default
  #9
Senior Member
 
Domenico Lahaye
Join Date: Dec 2013
Posts: 722
Blog Entries: 1
Rep Power: 17
dlahaye is on a distinguished road
Dear Arjun,

Thank you so much for your very valuable input.

I am very happy to see more details of the arguments raised so as gain a better understanding.

Are you able to share more details on the benchmarks and the results obtained with both solvers?

Thank you. Domenico.
dlahaye is offline   Reply With Quote

Old   June 20, 2022, 04:30
Default
  #10
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 666
Rep Power: 14
Tobermory will become famous soon enough
Dear Arjun - thanks for your input, and make no mistake - I am a BIG fan of starccm+ ... and have used starccm+ and StarCD before that since the early 90s. My earlier comments about stability were not intended as a discussion of the accuracy of starccm+ over any other code, but I stand by the observation that it (and other leading commercial CFD codes) is much more stable than OF - that must surely come from more robust & forgiving numerical schemes, and perhaps also more forgiving boundary condition coding? Perhaps you can enlighten us, with your experience at CD-Adapco.

Thanks also for the link to Tobi's test case. Regarding validation cases, my view is that you need to be VERY careful about mesh effects - the mesh in the test case, 2 cells across a duct, is clearly not sufficient to resolve anything physical, and so my suggestion is that it is difficult to learn anything real from this test case. I remember a 3D validation case I did against wind tunnel data where brilliant agreement was found from a coarse mesh solution, but the agreement got worse the more I refined the mesh .. until I got to the "real" mesh-independent solution ... that's the one I should have been using at the start to judge the numerical schemes.

Anyway - thank you for the discussion.
Tobermory is offline   Reply With Quote

Old   June 20, 2022, 04:44
Default
  #11
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
Rep Power: 34
arjun will become famous soon enougharjun will become famous soon enough
Quote:
Originally Posted by dlahaye View Post
Dear Arjun,

Thank you so much for your very valuable input.

I am very happy to see more details of the arguments raised so as gain a better understanding.

Are you able to share more details on the benchmarks and the results obtained with both solvers?

Thank you. Domenico.

It was long time ago so give me a day or two to find out his files. It can be useful for people who use openfoam.
arjun is offline   Reply With Quote

Old   June 20, 2022, 04:49
Default
  #12
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
Rep Power: 34
arjun will become famous soon enougharjun will become famous soon enough
Quote:
Originally Posted by Tobermory View Post
Thanks also for the link to Tobi's test case. Regarding validation cases, my view is that you need to be VERY careful about mesh effects - the mesh in the test case, 2 cells across a duct, is clearly not sufficient to resolve anything physical, .

1. The benchmark solution was generated from extremely fine mesh. So it was very physical. This is actually one of the validation cases of Ansys Fluent.

2. In case you did not notice third order solver with those 2 cells width able to reproduce solution generated by very very fine mesh.


3. All solvers used the same mesh. Starccm and Wildkatze did very good but you see if they were as diffusive as you believe they would have done worse.


4. As I said we have done multiple tests. I share you image from last test. OpenFOAM is most diffusive here and Starccm the least. Wildkatze has balanced solution with least amount of noise thanks to new specialised solver in it.
Attached Images
File Type: jpeg Compr01.jpeg (154.8 KB, 37 views)
arjun is offline   Reply With Quote

Old   June 20, 2022, 04:59
Default
  #13
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 666
Rep Power: 14
Tobermory will become famous soon enough
Quote:
Originally Posted by arjun View Post
2. In case you did not notice third order solver with those 2 cells width able to reproduce solution generated by very very fine mesh.
This is the bit that puzzles me - why would anyone run a CFD simulation with just two cells across the domain? That fails the basics of Best Practice. I am not really interested in what that solution gives, since as I said before it contains no real physics. Much more interesting is the grid independent solution ... you should only be comparing grid independent solutions when examining the effects of solver parameters.
Tobermory is offline   Reply With Quote

Old   June 20, 2022, 16:55
Default
  #14
New Member
 
Join Date: May 2018
Posts: 18
Rep Power: 7
Oliver Meng is on a distinguished road
Thanks for your reply.

A little more information about my case. The geometry is actually like a nozzle, wider at the inlet and outlet, very tight in the middle. And the maximum velocity will lead to the chocking effect.

i have tried different cases with different velocities at the inlet. I successfully made all simulations converge (residuals less then 1e-6)with rhoSimplefoam, as long as the max. velocity didn't reach 1 Ma. But for the cases, which should have a higher max. local velocity than 1 Ma (choked), it still did not work.

So my new question is: maybe a steady state solver like rhoSimpleFoam is not capable of a transonic or supersonic compressible case? Which means i really have to switch to rhoPimpleFoam for example?

Quote:
Originally Posted by Tobermory View Post
One of the difficulties I have observed is that the OpenFOAM solver schemes are very "clean" compared to commercial codes like StarCCM+ of Fluent, and this means that if you have a fine mesh, then there is very little numerical diffusion to stabilise the simulations. This means that flows over bluff bodies will start to show flow unsteadiness & shed turbulent structures into the wake.

I am not sure if this is relevant for your scenario, since we don't have a picture of your geometry, but have a think - is the solver just picking up inherent flow instability? If so, then you won't get full convergence with a steady solver ... unless you coarsen the mesh, which is not ideal! In these circumstances, you may have to run as a transient and field average over a number of shedding cycles.

Also, looking at your relaxation factors, I see you have tightened rho and e down to almost zero ... I know one of the tutorials has 0.01 for rho, but I find it difficult to believe that this is a good way to run the solver, i.e. basically to not update the rho or e equations ...

Good luck!
Oliver Meng is offline   Reply With Quote

Old   June 20, 2022, 17:06
Default
  #15
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 666
Rep Power: 14
Tobermory will become famous soon enough
Oliver - it is possible to use rhoSimpleFoam for transonic/sonic cases - see the attached results from a nozzle flow at a pressure ratio of 6.8, run with rhoSimpleFoam. I always prefer to use a steady solver where I can, but as I mentioned in an earlier post, it can sometimes be difficult to get a stable solution.

Incidentally, have you turned on the transonic switch in fvSolution/SIMPLE? I also run with the consistent flag set to yes.
Attached Images
File Type: jpg quadViewTwinned.0028.jpg (43.7 KB, 50 views)
Tobermory is offline   Reply With Quote

Old   June 20, 2022, 17:24
Default
  #16
New Member
 
Join Date: May 2018
Posts: 18
Rep Power: 7
Oliver Meng is on a distinguished road
My pressure ratio should also be round 6.


This is my new fvSolution file with transonic and consistent turning on.


But the simulation crashed at the second iteration with residuals of p ending up at 1e47


Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2106                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        smoother        GaussSeidel;
        tolerance       1e-10;
        relTol          0.1;
    }


    "(rho|U|k|omega|e)"
    {
        solver          PBiCGStab;
        preconditioner  DILU;
        tolerance       1e-10;
        relTol          1e-3;
    }
    
}

SIMPLE
{
    residualControl
    {
        p               1e-10;
        U               1e-10;
        "(k|omega|e|nut)"   1e-10;
    }
    transonic true;
    consistent true;
    nNonOrthogonalCorrectors 1;
    pMinFactor      0.05;
    pMaxFactor      6;
}

PIMPLE
{
    nCorrectors              2;
    nNonOrthogonalCorrectors 1;
    nOuterCorrectors         1;
    pMinFactor      0.05;
    pMaxFactor      6;
}

relaxationFactors
{
    fields
    {
        p               0.2;
        rho             0.1;
        pEqn            0.3;
    }
    equations
    {
        U               0.7;
        "(k|omega)"     0.7;
        e               0.7;
    }
}


// ************************************************************************* //
Code:
DILUPBiCGStab:  Solving for Ux, Initial residual = 0.02137706153, Final residual = 2.082396725e-05, No Iterations 2
DILUPBiCGStab:  Solving for Uy, Initial residual = 0.1155308207, Final residual = 0.0001081439417, No Iterations 2
DILUPBiCGStab:  Solving for Uz, Initial residual = 0.1310687182, Final residual = 0.0001163895147, No Iterations 2
DILUPBiCGStab:  Solving for e, Initial residual = 0.2772536778, Final residual = 0.0001556240328, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.2028451406, Final residual = 3.920168245e+47, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.0337139218, Final residual = 1.233059617e+48, No Iterations 1000
time step continuity errors : sum local = 1.154070612e+101, global = -6.316817843e+100, cumulative = -6.316817843e+100
pressureControl: p max 1.383434598e+104
DILUPBiCGStab:  Solving for omega, Initial residual = 0.004262390935, Final residual = 1.678025594e-06, No Iterations 3
DILUPBiCGStab:  Solving for k, Initial residual = 0.03920934066, Final residual = 2.115743412e-05, No Iterations 3
ExecutionTime = 29.61 s  ClockTime = 30 s
Quote:
Originally Posted by Tobermory View Post
Oliver - it is possible to use rhoSimpleFoam for transonic/sonic cases - see the attached results from a nozzle flow at a pressure ratio of 6.8, run with rhoSimpleFoam. I always prefer to use a steady solver where I can, but as I mentioned in an earlier post, it can sometimes be difficult to get a stable solution.

Incidentally, have you turned on the transonic switch in fvSolution/SIMPLE? I also run with the consistent flag set to yes.
Oliver Meng is offline   Reply With Quote

Old   June 21, 2022, 00:48
Default
  #17
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
Rep Power: 34
arjun will become famous soon enougharjun will become famous soon enough
Quote:
Originally Posted by Tobermory View Post
This is the bit that puzzles me - why would anyone run a CFD simulation with just two cells across the domain? .

To demonstrate that high order solver is more accurate. That was point of that validation no.



Quote:
Originally Posted by Tobermory View Post
I am not really interested in what that solution gives, since as I said before it contains no real physics.
May be this is why you think the way you think since you completely missed that the solution produced was very physical. You just ignore the facts in front of you for the myths you believe in.


Quote:
Originally Posted by Tobermory View Post
Much more interesting is the grid independent solution ... you should only be comparing grid independent solutions when examining the effects of solver parameters.
Not if my higher order solver could get me more accurate results on coarser grids. I am not stupid to keep running simulations for days when higher order would do the same 10 times faster.


BTW the last picture was not some very coarse simulation. That mesh has enough cells and you can see that OpenFOAM was far more diffusive than other two solvers and Starccm was least diffusive. Goes completely against the idea that OpenFOAM is not using any artifical diffusivity while Starccm is using it. Another myth that people keep repeating here.
arjun is offline   Reply With Quote

Old   June 21, 2022, 04:40
Default
  #18
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 666
Rep Power: 14
Tobermory will become famous soon enough
Quote:
Originally Posted by Oliver Meng View Post
My pressure ratio should also be round 6.


This is my new fvSolution file with transonic and consistent turning on.


But the simulation crashed at the second iteration with residuals of p ending up at 1e47
Did you apply the full pressure from the start? I needed to ramp up my pressure over several thousand iterations, to give the pressure solver a chance. I used a uniformTotalPressure condition:

Code:
    upStream {
        type            uniformTotalPressure;
        p0              table (
                            (     0   $p0)
                            (  1000   150000)
                            (  2000   300000)
                            (  3000   $pInlet)
                            (999999   $pInlet)
                        );
    }
and that seemed to do the trick for me, with a totalPressure condition on the downstream outley boundary. For relaxation I had:

Code:
    fields
    {
        p               0.3;
        rho             0.2;
    }
    equations
    {
        velocity        0.5;
        pressure        0.9;
        energy          0.5;
        turbulence      0.7;
        U               $velocity;
        p               $pressure;
        "(k|epsilon|omega)" $turbulence;
        "(h|e)"         $energy;
    }
and I also used fvOptions to constrain T in some of my later simulations:
Code:
    limitT
    {
        type            limitTemperature;
        active          yes;
        selectionMode   all;
        min             50;
        max             750;
    }
to help with some of the early initial transients, where the temperature/h would swing wildly. I hope this helps.
hogsonik likes this.
Tobermory is offline   Reply With Quote

Old   June 21, 2022, 04:46
Default
  #19
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 666
Rep Power: 14
Tobermory will become famous soon enough
Quote:
Originally Posted by arjun View Post
To demonstrate that high order solver is more accurate. That was point of that validation no.
Thank you for giving me a giggle so early on in the morning. I love the idea that you think that two to three cells are enough to resolve fully the complex flow features, including free shear layers and turbulent entrainment, that are required to reproduce the physics involved in your test case.

We are not going to agree on this, so perhaps let us just focus on Oliver's original question, my friend. All the best.
Tobermory is offline   Reply With Quote

Old   June 21, 2022, 06:49
Default
  #20
New Member
 
Join Date: May 2018
Posts: 18
Rep Power: 7
Oliver Meng is on a distinguished road
Thanks you so much! I am trying these methods from you.

Where is exactly your upStream patch in the geometry?

Quote:
Originally Posted by Tobermory View Post
Did you apply the full pressure from the start? I needed to ramp up my pressure over several thousand iterations, to give the pressure solver a chance. I used a uniformTotalPressure condition:

Code:
    upStream {
        type            uniformTotalPressure;
        p0              table (
                            (     0   $p0)
                            (  1000   150000)
                            (  2000   300000)
                            (  3000   $pInlet)
                            (999999   $pInlet)
                        );
    }
and that seemed to do the trick for me, with a totalPressure condition on the downstream outley boundary. For relaxation I had:

Code:
    fields
    {
        p               0.3;
        rho             0.2;
    }
    equations
    {
        velocity        0.5;
        pressure        0.9;
        energy          0.5;
        turbulence      0.7;
        U               $velocity;
        p               $pressure;
        "(k|epsilon|omega)" $turbulence;
        "(h|e)"         $energy;
    }
and I also used fvOptions to constrain T in some of my later simulations:
Code:
    limitT
    {
        type            limitTemperature;
        active          yes;
        selectionMode   all;
        min             50;
        max             750;
    }
to help with some of the early initial transients, where the temperature/h would swing wildly. I hope this helps.
Oliver Meng is offline   Reply With Quote

Reply

Tags
rhopimplefoam, rhosimplefoam, steady state, transient

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
From steady state to transient simulation Mechand FLUENT 0 December 24, 2020 12:17
Will the results of steady state solver and transient solver be same? carye OpenFOAM Running, Solving & CFD 9 December 28, 2019 05:21
Effect of initial condition for steady state vs Transient prasa ANSYS 0 August 22, 2018 04:45
accelarate simulation using steady state solver tjliang OpenFOAM Running, Solving & CFD 0 October 7, 2016 14:42
Constant velocity of the material Sas CFX 15 July 13, 2010 08:56


All times are GMT -4. The time now is 11:14.