Natural convection over a single tube
 

Hey Guys,

I am simulating a single tube of 325 mm length and 25 mm diameter kept inside a closed box of 2 m X 2 m X 2 m dimensions filled with air. I am simulating air as the perfect gas (compressible model). The tube is kept at 350 K temperature and air is at 300 K.

I am using buoyantPimpleFoam solver in Openfoam 2.0.0. The pressure is atmospheric at the tube and at the walls of the container, the velocity is no slip everywhere.

The problem is with the convergence, I am getting a fluctuating residuals for velocity and pressure. The residuals varies from 1e-02 to 1e-04, but it is not converging. The velocity vectors seems ok everywhere but the temperature range is showing 299.97 to 350 K, which should not go below 300 K (ideally).
I am taking a time step of 1e-05, and the meshing is tetrahedral (unstructured). I am using k-epsilon model as well as have tried SSTkOmega.

Please help me if you have any idea about this, I have tried every boundary conditions I could.

Thanks in advance

nonOrthogonalCorrector
 

Hi

How many nonOrthogonalCorrectors do you apply? With tetrahedral mesh you probably have to increase them. Could you post your fvSolution dict?

Regards

Fabian

Hey

Thanks for your reply, I am posting my fvSolutions

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
"rho.*"
{
solver PCG;
preconditioner DIC;
tolerance 0;
relTol 0;
}

p_rgh
{
solver GAMG;
tolerance 1e-09;
relTol 0.001;
smoother GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
minIter 1;
}

p_rghFinal
{
solver GAMG;
tolerance 1e-09;
relTol 0.001;
smoother GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
minIter 1;
}
h
{
solver GAMG;
tolerance 1e-08;
relTol 0.01;
smoother GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
minIter 1;
}
R
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-08;
relTol 0.01;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.01;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.01;
}

omega
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-07;
relTol 0.01;
}


"(U|k|omega|h|R)Final"
{
$U;
relTol 0;
}

}


PIMPLE
{
momentumPredictor yes;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
}

{
p 0.5;
U 0.3;
T 0.5;
k 0.5;
omega 0.5;
nut 0.5;
R 0.5;
nuTilda 0.5;
}

In one of the cases I had some fins on the same tube, I used nNonOrthogonalCorrectors = 4 and air as incompressible fluid, but in that case velocity was converging but p_rgh was not converging.

Plz have a look at it.
// ************************************************** *********************** //

Hello,

Do, something like this and let us know about the convergence.

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

relaxationFactors
{
fields
{
}
equations
{
"(U|T|k|epsilon|R)" 1;
"(U|T|k|epsilon|R)Final" 1;
}
}

You can also have a look at the tutorial/case folder of other heat transfer problems.

Also, try varying the "nNonOrthogonalCorrectors" upto 1 & 2. If still you are not getting the convergence then try to make quality (skewness for unstructured < 0.7) mesh.

:)

outerCorrectors and relaxation
 

Right. These settings look good for me too. Check your mesh quality. If you still have problems you could increase your outer correctors and give some relaxation factors.

Regards

Fabian

Hey

Thanks alot for your replies. I have updated my fvSolution accordingly in an already running case. The velocity residual is 1e-05 and pressure residual is 0.054, pressure residual is coming down with time. Hope to have it converged in some more time. I will post you accordingly after some time.

Once again thanks a lot for the help. One more thing I would like to ask, what is the significance of the outer correctors and non orthogonal correctors.

Ankur

Check this out, for more information...

http://openfoamwiki.net/index.php/Ma...rGuideAddendum

Nice Page
 

Nice, didn't know that page. Thanks.
Any news Ankur?

Regrads

Fabian

You are welcome, even it is mentioned in the user guide of OF by Sir H. Jasak.

:)

Hey

Sorry I got busy in some other work.

I have seen that page..not fully understood though. I will read it again and will let you know.

The case of tube having fins is now converging, the pressure has gone to 0.02 from 0.5..the convergence is slow. The grid quality is the problem I think, because the grid number is 1600000, mesh is tetra, and the skewness is around 1.1. I am using Gmsh 2.3.0 and I am not able to decrease the skewness below this value.

I am very thankful to both of you for your valuable suggestions and time.

I will post back as soon as possible with further updates.

Sometimes quality mesh really have an impact on results, may be with skewness of around 1.1 you may not get good results. Actually, order of >1 means you need to re-mesh your geometry.
So, it is usually advisable to keep skewness upto <0.8. For, that you need to really try hard in meshing. Spend sometime reading the same.
At last, the CFD solution depends on "Geometry meshing + solution algorithms" methods. So, you need to keep a balance between these, knowing only one method may cause problems in the results.

:)

Hey Tushar

Thanks for the suggestion. I have tried a lot to decrease the skewness, and you are right I should try harder to make it good. I am going to do it first. I will let you know once I am done with it.

:)
Ankur

Hey tushar

I am a little late for the reply. I have completed the CFd simulations of a cylinder without fins successfully. I got good results. In some time I will also simulate it with fins, hopefully It will also be done.

This reply is just to let you that its done and thanks for the help. I am facing some other problem wich I am going to post today on forum.

Thanks