[LB76]

Dear all,
I am trying to validate LES approach for openfoam on the turbulent channel flow at retau=395.
The problem is that the results are far from that of the DNS reference.
By inspecting some possibilities we decided to run the case with no model on an LES grid. The results shows that the code is hyper dissipative without any SGS model. Inspecting the u+ profile shows that it is completely above that of the DNS meaning an overediction of the debit. This is linked to the dissipation errors produced by the code. We tried a less severe case with two vortices in a box and no molecular viscosity. With the linear central scheme, this must conserve kinetoc energy for a while.... We lost 20%.... on the initial level.
In these conditions, adding a SGS model will results in a deterioration of the results. I did not found relevant literature on this. Could someone help me?
Nobody published LES performed with a state of the art model e.g. Wale model and showed good agreement with DNS data.
We performed the DNS at lower Retau 180 and that works fine as it can be also found in literature. I am planning to use OF for LES in turbomachinery | engine applications. What if a simple turbulent flow between two plates cannot be predicted ? If someone can help I would appreciate

[niklas]

not much useful info in here to work with...
can you post the fvSolution and fvSchemes dicts

[LB76]

Hi, thank you for reply, my fvSchemes file looks like this:
ddtSchemes
{
default backward;
}

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

divSchemes
{
default none;
div(phi,U) Gauss linear; //linear; //upwind;
}

laplacianSchemes
{
default none;
laplacian(nu,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
}

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

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p ;
}
fvSolution:
solvers
{

p
{
solver GAMG;
smoother DICGaussSeidel;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 100;
preconditioner DIC;
mergeLevels 1;
tolerance 1e-06;
relTol 0.05;
}

pFinal
{
solver GAMG;
smoother DICGaussSeidel;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 100;
preconditioner DIC;
mergeLevels 1;
tolerance 1e-06;
relTol 0.05;
}

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

PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 1001;
pRefValue 0;
}


Best regards LB

[niklas]

It looks like you are using pisoFoam.
your pressure convergence criteria is quite large.
set the relTol to 0 on all and reduce the tolerance to 1.0e-8 on pressure...
and for U as well.
If you are really accounting for the energies I would be careful at looking for the best
possible convergence.

Also, I would try pimpleFoam.
and then set
nOuterCorrectors to at least 5,
plus all relTol for the *Final to zero.

Not sure what Courant number you have set to calculate the time step, but
if you are above 1, this could also partly explain your results.

hope this makes it better

[Cotten]

What mesh are you using?
I did some channel flows during my Msc and the grid was the most influacting part and the SGS model didn't do much...

[LB76]

Hi

The suggestions provided by Niklas seems to bring some improvements.
I am still investigating thisand trying to find the best coefficient for the WALE model. Could you provide me a pdf of your msc thesis?

Best regards

LB