[izna]

Hello

I have a PC with 4GB RAM 2 processors..
Ihave run a simulation with pisoFOam and today is 48 hours since i last start.. and still convergence not acheived..!!

Can anyone give me a better way to acheive convergence easier with pisoFoam?

I am attaching my fv solution just so that you may know what i did..

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0.1;
}

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

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

k
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

epsilon
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

R
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

nuTilda
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}
}

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

residualControl
{
p 1e-3;
U 1e-4;
"(k|epsilon|omega)" 1e-3;
}


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

and my control dict

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application pisoFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 10;

deltaT 0.0005;

writeControl timeStep;

writeInterval 100;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression off;

timeFormat general;

timePrecision 6;

runTimeModifiable true;


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

[ngj]

Good evening,

pisoFoam is intended for transient simulations, which does not necessarily have a steady state solution. Also, to my knowledge, the pisoFoam does not check for the residualControls, which you have in your fvSolution file.

For steady state simulations you would probable want to look into e.g. simpleFoam.

Kind regards,

Niels

[izna]

hi..

simpleFoam is not working at all for the case that running... hence am running with pisoFoam, and its working with pisoFoam.. but taking such a long time!!!!

[RodriguezFatz]

Is this a transient simulation or steady state?

[izna]

steady state..

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / 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 ;
}


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

[RodriguezFatz]

You are using the wrong solver. You solve for a transient simulation, time-scheme is Euler and your time-step is 0.5ms.
This is not steady-state.

1) Use simpleFoam! Why do you say "simpleFoam is not working at all for the case that running"? SimpleFoam is a steady state solver.
2) Use GAMG solver for pressure.
3) "Linear" discretization doesn't converge very well. You can try some more dissipative scheme (upwind, linearUpwind,...).

[izna]

i already did all that with simpleFoam.. But after 300 timestep my solution crash.. and when i check in paraView, i see my domain as a blueeee one.. ie no velocity has enter... hence why i was soo desperate...

[RodriguezFatz]

Then you did it wrong
Post your simple solver settings and then the residuals.

[izna]

simple Solver settings..:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver GAMG;
tolerance 1e-7;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 10;
mergeLevels 1;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

epsilon
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
k 0.7;
omega 0.7;
}
}

cache
{
grad(U);
}

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

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss linearUpwindV grad(U);
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

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

[RodriguezFatz]

Can you post the residual plot?
1) What happens, if you set "relTol" for the pressure to 1.0e-3? Do the residuals change?
2) What happens, if you use some gradient limiter? Such as

 
gradSchemes
{
    default            faceLimited edgeCellsLeastSquares 1;
}

3) Write "bounded" at each div(phi,xxx)

 
...
div(phi,k)      bounded Gauss upwind;

[izna]

am sorry for late reply.. but for each of the above mentioned points. My solution crash..
Now am worried....

[RodriguezFatz]

Can you send the whole log-output? So we can try to find the spot...

[izna]

hi..afte changing the fv solution and fv schemes.. I obtain a good simulation which i checked..

.. when arriving at 1760 iteration the solution crashed.. and when i checked in paraView.. I obtain a blue domain..
Why such a nice simulation suddenly crash ?

[RodriguezFatz]

You have to share all relevant data, otherwise no one will be able to help you.

1) log output
2) boundary condition files
3) screenshot of your domain with grid.

Additionally: It seems you use the k-epsilon model. In your fvSolution file you set relaxation factors, but not for k-epsilon but for k-omega. This could be the reason.

[DaSh]

Hi all,

I have a question which is close to the topic. Niels said above, that pisoFoam does not check for residualControls.

Does that mean, that when running a transient turbulent simulation on pisoFoam, the residual output does not indicate the state of convergence of my simulation?

I have the problem at the moment with my simulation. The residual is not dropping anymore, so I have no convergence. (It is LES of Taylor Couette Flow). I use backward time scheme and gauß upwind for U divscheme. My schemes should be fine.

After reading this thread I am just worrying, that the solver is not able to produce what I want.

Can anybody comment on this?

Thx!
Danesh

[haakon]

You are correct. pisoFoam does not obey the residual controls. This is because the solution is time-accurate, i.e. every step is a valid solution of the transient problem. Hence, each step is solved until the specified tolerance level in fvSolution, and not further. Then the time is advances and a new solution is found. The value of the time step is hence important, as the PISO-algorithm cannot handle large time steps.

Remember my earlier comments on fluid flows that generally are transient by nature. I do not feel that you have clearly out-ruled this issue yet.

[DaSh]

I understand what you mean Haakon. Of course the Taylor Couette Flow (in my case) will have a steady state solution at some point, e.g. turbulent taylor vortices. I am pretty sure, that it should work with pisoFoam. My time step is actually large. It is 0,05, which should be ok, looking at the courant number (alway < 0,45).

[izna]

helloo

I am sorry for late reply..

But finally My solution with simpleFoam converge..

I used a fv schemes and fv solution as below.. and attached is my converged results.. As we can all see its not good at all!...

I nEED HELP BADLY

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / 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 ;
}


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

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{

solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}


U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

epsilon
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}


}

SIMPLE
{
nNonOrthogonalCorrectors 0;

residualControl
{
p 1e-2;
U 1e-3;
"(k|epsilon|omega)" 1e-3;
}
}

relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
k 0.7;
epsilon 0.7;
}
}

cache
{
grad(U);
}


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

[RodriguezFatz]

The log output is still missing.

You really can not expect this to converge. You set everything to linear, gradients have no limiters and so on. You need to get a stable, robust setting and then you can try to make it numerically more accurat. But don't start with this second order low diffusion stuff.

[izna]

look can you please post for me a fv scheme and fv solution fiting for this? ANd i assure you it converged..