[mjavrincon]

Hi guys,

I am trying to set up an LES simulation with turbulentDFSEMInlet boundary condition. In order to do so, I run a precursor RANS simulation with uniform inlet conditions and k-omega SST model of the same geometry. During the RANS simulation I extract the data at the outlet with the following code in controlDict:

    sampledPlanes
    {
        type                     surfaces;
        functionObjectLibs ( "libsampling.so" );
        outputControl        timeStep;
        outputInterval       1000;
        enabled                true;
        surfaceFormat       boundaryData;
        fields                    ( U turbulenceProperties:R turbulenceProperties:L );
        interpolationScheme cellPatchConstrained;
        surfaces                ( outlet { type patch ; patches ( outlet ) ; interpolate false ; } );
    }

Afterwards, I edit the case to adjust it for LES, take the data of U, R, L under postProcessing/sampledPlanes/ and copy it with the right format under constant/boundaryData. The problem is that I always get the following error when trying to decompose or run the case with turbulentDFSEMInlet:

Time = 0
Turbulent DFSEM patch inlet: interpolating field R from "/data/MJRP/fullCases/LES/constant/boundaryData/inlet/0/R"
Turbulent DFSEM patch inlet: interpolating field L from "/data/MJRP/fullCases/LES/constant/boundaryData/inlet/0/L"
Turbulent DFSEM patch inlet: interpolating field U from "/data/MJRP/fullCases/LES/constant/boundaryData/inlet/0/U"


--> FOAM FATAL ERROR:
Reynolds stress (2.3018333e-31 7.4816001e-32 -1.3597915e-31 -3.9599454e-32 -2.22473e-32 -1.2211324e-31) at face 1 leads to an invalid Cholesky decomposition due to the constraint R_yy - sqr(a_xy) >= 0

    From static bool Foam::turbulentDFSEMInletFvPatchVectorField::checkStresses(const symmTensorField&)
    in file fields/fvPatchFields/derived/turbulentDFSEMInlet/turbulentDFSEMInletFvPatchVectorField.C at line 992.

FOAM exiting

I have tried everything that I know including improving the mesh and extract the data in different ways at the outlet. I have not seen any solution to the problem online and perhaps I have an error of concept on how the BC works, but I hope that you could help me.

Thus, does anyone faced the same problem and knows what is failing here?

Thanks in advance!

[HPE]

Hi,

One of the input Reynolds stress tensor element contains only zero-valued elements.

That's physically not possible. Therefore, OpenFOAM complains.

Hope this helps.

[mjavrincon]

Thank you for your reply.

I have found the issue and I finally made it work.

The main problem is that I was extracting the data exactly at the inlet patch, where the Reynolds Stress tensor is zero.

I had to extract the simulation data from RANS at a certain distance from the inlet, where the flow is fully developed in my case. Doing so and then adjusting the case before running the LES in constant/boundaryData gives no problems when decomposing the case. Here you can see the function in controlDict to sample a plane:

sampledSurface
    {
        type            surfaces;
        executeControl  runTime;
        executeInterval 0.15;
        writeControl    runTime;
        writeInterval   500;
        enabled         true;
        surfaceFormat   boundaryData;
        interpolationScheme none;
        interpolate     false;
        triangulate     false;
        fields          ( U turbulenceProperties:R turbulenceProperties:L UPrime2Mean );
        surfaces        ( inletSurface { 
                                     type plane ; 
                                     planeType pointAndNormal ; 
                                     pointAndNormalDict { 
                                              point ( -0.07 0 0 ) ; 
                                              normal ( 1 0 0 ) ; 
                                              interpolate false ; 
                                              triangulate false ; 
                                              } 
                                      } );
    }

As a reference, attached you can see the difference between having uniform inlet conditions and using DFSEM. I hope it helps if anyone else find themselves in trouble.

[Sandeep lamba]

hi Mario Javier Rincón, It is of great help for me. Thanks for sharing.

[HPE]

- sorry posted as a mistake -

[XJ_Wang]

Hi Mario,

Thanks for sharing.

I also found a problem in the old version of OpenFOAM.com

For example in v1912,
OpenFOAM-v1912/src/finiteVolume/fields/fvPatchFields/derived/turbulentDFSEMInlet/turbulentDFSEMInletFvPatchVectorField.C
line 995:

scalar a_yz = (R.yz() - a_xy*a_xz)*a_yy;

this should be:

scalar a_yz = (R.yz() - a_xy*a_xz)/a_yy;

I have found it has been corrected in v2112.(not sure in which version it was corrected for the first time)

Hope this will be helpful if other foamers encounter this problem.