[kaaja]

Hi,

I have trouble getting results for the Reynold's stresses when using the command

simpleFoam -postProcess -func R

Using the above command, I get the following error message

Build  : 4.1
Exec   : simpleFoam -postProcess -func R
Date   : Apr 18 2017
Time   : 07:42:47
Host   : ""
PID    : 10656
Case   : /home/.../run16
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


SIMPLE: convergence criteria
    field p     tolerance 0.01
    field U     tolerance 0.001
    field "(k|epsilon|omega|f|v2)"     tolerance 0.001

turbulenceFields R: storing fields:
    turbulenceProperties:R

Time = 0
Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
    alphaK1         0.85;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.856;
    gamma1          0.555556;
    gamma2          0.44;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    b1              1;
    c1              10;
    F3              false;
}

No MRF models present

--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword boundaryField is undefined in dictionary "/home/.../run16/0/turbulenceProperties:R"

file: /home/.../run16/0/turbulenceProperties:R from line 18 to line 20.

    From function const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&) const
    in file db/dictionary/dictionary.C at line 642.

The file "turbulenceProperties:R " looks like:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volSymmTensorField;
    location    "0";
    object      turbulenceProperties:R;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0.233333 -0 -0 0.233333 -0 0.233333);

Does anyone have a clue to what's going wrong here?

[aow]

Hello Kaaja,

I realize this is roughly a year later, but I was wondering if you figured out your problem (since I believe I'm having a similar one)? My guess after reading the error is that it looks like you were missing boundary condition definitions for the Reynolds stress tensor since all that the command "<solverName> -postProcess -func R" does is to generate a file that has the full field data for each cell without specifying any boundary conditions. If this was the case, what sort of boundary conditions did you apply for R?

Also, do you have to change the file name from "turbulenceProperties:R" (the file name generated by the postProcess command) to "R" in the time directories? After looking at the source code in "LRR.H" and "LRR.C" it looks like they're using "R".

Best regards,
Andrew

PS - In case it matters, I've attached the error report and I am using Pablo Higuera's "olaDyMFoam" solver, which is a modification of the standard "interFoam" solver to allow for dynamic mesh motion for wave generation boundary conditions (I'm trying to model a piston wave maker in a long flume; see https://github.com/phicau/olaFlow for the solver code).

[kaaja]

Hello Andrew,

I am sad to say that I don't remember if I solved that problem, and that I don't have capacity these next 2 months checking it eighter (lot of work).

Probably not the same thing, but I found the following 2 posts I did on somewhat related topics

How to sample turbulenceProperties:R?

https://www.cfd-online.com/Forums/openfoam/187909-reporting-turbulence-fields.html

I hope you will work it out!

[aow]

Thanks kaaja,

I managed to get my LRR simulation working using Rxx = Ryy = Rzz = 2k/3 and Rxy = Rxz = Ryz = 0 for the internalField. I used the following BCs for R in my 0 directory.

For a solid wall boundary...

flumeWall
    {
        type            kqRWallFunction;
        value           uniform (0 0 0 0 0 0);
    }

For an atmosphere boundary at the top of my wave flume...

atmosphere
    {
        type            inletOutlet;
		inletValue      uniform (0 0 0 0 0 0);
		value           uniform (0 0 0 0 0 0);
    }

I also had to adjust my fvSchemes and fvSolution files too since there weren't any entries for R-related calculations.

For fvSchemes I used...

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    div(rhoPhi,U)                                      Gauss limitedLinearV 1;
    div(U)                                                Gauss linear;
    div(phi,alpha)                                     Gauss vanLeer;
    div(phirb,alpha)                                  Gauss interfaceCompression;
    div((muEff*dev(T(grad(U)))))	             Gauss linear;
    div(phi,k)                                           Gauss upwind;
    div(phi,epsilon)                                   Gauss upwind;
    div(phi,omega)                                   Gauss upwind;
    div(phi,R)                                           Gauss upwind;
    div((rhoPhi|interpolate(porosity)),U)     Gauss limitedLinearV 1;
    div(rhoPhiPor,UPor)                              Gauss limitedLinearV 1;
    div(rhoPhi,UPor)                                  Gauss limitedLinearV 1;
    div(rhoPhiPor,U)                                  Gauss limitedLinearV 1;
    div((phi|interpolate(porosity)),k)          Gauss upwind;
    div((phi|interpolate(porosity)),epsilon) Gauss upwind;
    div((phi|interpolate(porosity)),omega)  Gauss upwind;
    div((phi|interpolate(porosity)),R)          Gauss upwind;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p_rgh;
    pcorr;
    alpha.water;
}

wallDist
{
    method meshWave;
}

For fvSolution I used...

solvers
{
    "alpha.water.*"
    {
        nAlphaCorr      1;
        nAlphaSubCycles 2;
        alphaOuterCorrectors yes;
        cAlpha          1;

        MULESCorr       no;
        nLimiterIter    3;

        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-8;
        relTol          0;
    }

    "pcorr.*"
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-5;
        relTol          0;
    }

    pcorrFinal
    {
        $pcorr;
        relTol          0;
    }

    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-07;
        relTol          0.05;
    }

    p_rghFinal
    {
        $p_rgh;
        relTol          0;
    }

    "(U|k|epsilon).*"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-06;
        relTol          0;
    }
	
    R
    {
	solver          smoothSolver;
        smoother     symGaussSeidel;
        tolerance     1e-8;
        relTol          0;
     }
	
     RFinal
     {
		$R;
		tolerance		1e-08;
		relTol		0;
      }
	
    cellDisplacement
    {
        solver                        GAMG;
        tolerance                    1e-5;
        relTol                         0;
        smoother                   GaussSeidel;
        cacheAgglomeration    false;
        nCellsInCoarsestLevel 10;
        agglomerator              faceAreaPair;
        mergeLevels               1;
    }

    cellDisplacementFinal
    {
        $cellDisplacement;
        relTol          0;
    }
}

PIMPLE
{
    momentumPredictor   no;
    nOuterCorrectors    1;
    nCorrectors         3;
    nNonOrthogonalCorrectors 0;
}

relaxationFactors
{
    fields
    {
    }
    equations
    {
        ".*" 1;
    }
}

Finally, it should be noted that I used OpenFOAM-5.0 with Pablo Higuera's OLAFOAM (now called olaFlow; see https://github.com/phicau/olaFlow) solvers added too. The case is a highly-modified version of the wavemakerFlume tutorial that came with OLAFOAM.

[aow]

Also, I forgot to say that I ended up just making a brand new R file in my 0 time directory with the boundary conditions I mentioned previously so I got away with not using the recommended approach of first running a simpler model (kEpsilon) and then changing to the RSM model (LRR).

Since my simulation went so well, I also tried using the SSG model in this same manner at first, which blew up after 0.6 s (my endTime is 25 s). Then I tried using the LRR results at 0.5 s as an initial state for switching to the SSG model, but it also blew up near 1 s so for now I'm just sticking with the LRR model.