[deji]

Meant u'T', v'T' .

[s-ammarlu]

hi
i guess flow isnt , fully devesloped , and a length needs to be fully developed turbulent flow .

[grandgo]

Originally Posted by gaby

Hello

I'm doing LES calculation for internal flow and results look fine. Now, I need to calculate the energy spectrum turbulence (E(K) vs K)...

Is there any tool in OpenFoam available to calculate this??

Or somebody knows a way to obtain E(K) ??

I'll appreciate any hint...

Gaby

hi gaby,

i'm confronted with the same problem you had. how did you manage it?

i hope you're still visiting the forum from time to time

best regards
grandgo

[gregor]

Hi,
depends how you want to evaluate the energy spectrum (at a specific point, or over the whole domain).

In the dnsFoam the energy spectrum is calculated, so you can simply code your own post processing tool by copying the routines.

#include "fvCFD.H"
#include "Kmesh.H"
#include "UOprocess.H"
#include "fft.H"
#include "calcEk.H"
#include "graph.H"

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

int main(int argc, char *argv[])
{
    #include "setRootCase.H"
    #include "createTime.H"
    #include "createMeshNoClear.H"
    #include "createFields.H"

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

    Info<< nl << "Starting time loop" << endl;
    instantList timeDirs = timeSelector::select0(runTime, args);
    Kmesh K(mesh);

    forAll(timeDirs, timeI)
    {
    runTime.setTime(timeDirs[timeI], timeI);
    Info << "Time =" << runTime.timeName() << endl;
       
    Info<< "Reading field U\n" << endl;
     volVectorField U
     (
         IOobject
         (
             "U",
             runTime.timeName(),
             mesh,
             IOobject::MUST_READ,
             IOobject::AUTO_WRITE
         ),
         mesh
     );

        calcEk(U, K).write(runTime.timePath()/"Ek", runTime.graphFormat());

        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
            << nl << endl;
    }

    Info<< "End\n" << endl;

    return 0;
}

you can use the dnsFoam makefiles
gregor

[grandgo]

Originally Posted by gregor

Hi,
depends how you want to evaluate the energy spectrum (at a specific point, or over the whole domain).

In the dnsFoam the energy spectrum is calculated, so you can simply code your own post processing tool by copying the routines.

#include "fvCFD.H"
#include "Kmesh.H"
#include "UOprocess.H"
#include "fft.H"
#include "calcEk.H"
#include "graph.H"

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

int main(int argc, char *argv[])
{
    #include "setRootCase.H"
    #include "createTime.H"
    #include "createMeshNoClear.H"
    #include "createFields.H"

    Info<< "Reading field U\n" << endl;
    volVectorField U
    (
        IOobject
        (
            "U",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

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

    Info<< nl << "Starting time loop" << endl;
    instantList timeDirs = timeSelector::select0(runTime, args);
    Kmesh K(mesh);

    forAll(timeDirs, timeI)
    {
    runTime.setTime(timeDirs[timeI], timeI);
    Info << "Time =" << runTime.timeName() << endl;

        calcEk(U, K).write(runTime.timePath()/"Ek", runTime.graphFormat());

        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
            << nl << endl;
    }

    Info<< "End\n" << endl;

    return 0;
}

you can use the dnsFoam makefiles
gregor

hi gregor,

thanks for your post.

i'm simulating a pipe flow with LES and i want to measure the energy spectrum "one dimensional" over the radius of the pipe.

in dnsFoam the whole domain ist calculated if i'm right (?). so i could sample the E(k) data with a function in the controlDict file, right?

best regards,
grandgo

[gregor]

Originally Posted by grandgo

in dnsFoam the whole domain ist calculated if i'm right (?).
grandgo

Correct. You can use probes to sample the velocity and then post process your data using matlab or python.

Originally Posted by grandgo

so i could sample the E(k) data with a function in the controlDict file, right?
grandgo

that won't work since E(k) is not a field. It is a scalar representing the energy spectrum of your velocity field. So you can't sample E(k) at a specific position.

gregor

[grandgo]

Originally Posted by gregor

that won't work since E(k) is not a field. It is a scalar representing the energy spectrum of your velocity field. So you can't sample E(k) at a specific position.

oh, i see...stupid question

one more: in what way do i have to change the code from above, so that the utility evaluates the energy spectrum of one specific point?

EDIT:

i used your code to compile a utility but i get this message:

--> FOAM FATAL ERROR: 
calculated number of cells is incorrect

    From function Kmesh::Kmesh(const fvMesh& mesh)
    in file Kmesh/Kmesh.C at line 87.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/sw/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/sw/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  Foam::Kmesh::Kmesh(Foam::fvMesh const&) in "/sw/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/librandomProcesses.so"
#3  
 in "/home/stss8/OpenFOAM/stss8-1.7.x/applications/bin/linux64GccDPOpt/energySpec"
#4  __libc_start_main in "/lib64/libc.so.6"
#5  
 at /usr/src/packages/BUILD/glibc-2.11.2/csu/../sysdeps/x86_64/elf/start.S:116

my mesh is 3D and, since i'm using the utility as post-process, no parallel calculation.

any idea?

[gregor]

Originally Posted by grandgo

one more: in what way do i have to change the code from above, so that the utility evaluates the energy spectrum of one specific point?

well thats not trivial since calcEk(U, K) does a fft in space but you would need to do a fft in time. I am not sure how to easily adapt that. Therefor i would use matlab or numpy.

EDIT:

The error message is because your domain is not a box. If look at the KMesh.C file it is counting all cells along every direction. Then it multiplies the cell numbers and if they do not match the total number of cells it raises an error.

gregor

[grandgo]

Originally Posted by gregor

well thats not trivial since calcEk(U, K) does a fft in space but you would need to do a fft in time. I am not sure how to easily adapt that. Therefor i would use matlab or numpy.

EDIT:

The error message is because your domain is not a box. If look at the KMesh.C file it is counting all cells along every direction. Then it multiplies the cell numbers and if they do not match the total number of cells it raises an error.

gregor

hi gregor,

yes, it was my worry, that it has something do to with my domain not being cube-shaped. thanks anyway.

best regards
grandgo

[grandgo]

hi foamers,

i need your opinions.

i have a LES case with a domain of about 6.5e6 cells, reynolds number is 23000, the courant number is about 1, deltaT 1e-6 sec . i'm using a modified pisoFoam parallel with 16 cores, 2,4ghz each.

the calculation time for one time step is about 200 seconds.

i'm wondering if the calculation time is acceptable or not.

what do you think? within reason or do i have to change anything?

best regards
grandgo

[BernhardGrieser]

Originally Posted by grandgo

hi foamers,

i need your opinions.

i have a LES case with a domain of about 6.5e6 cells, reynolds number is 23000, the courant number is about 1, deltaT 1e-6 sec . i'm using a modified pisoFoam parallel with 16 cores, 2,4ghz each.

the calculation time for one time step is about 200 seconds.

i'm wondering if the calculation time is acceptable or not.

what do you think? within reason or do i have to change anything?

best regards
grandgo

The PISO algorithm requires lower CFL numbers, so if I were you I'd reduce the time step significantly until maxCourant is below 0.1, maybe even less.
You're modeling a pipe flow, don't you? For that given Reynolds number you can go coarser on the grid; maybe reducing the total cell count by a factor of two would be sufficient.
Also, if possible, I recommend you to double your proc number to 32.

Which sgsModel are you using, btw?

[N. A.]

Hello Folks,

I think my question is suited for this post and I am hoping I get to learn more about some of the post-processing of variables in openFOAM.

Following are my questions regarding u'^2, T'^2 andYi'^2.

1) Is u'^2 that we obtained from prime2Mean same as the u_sgs^2? Similarly is T'^2 that we get from prime2Mean also same as T_sgs^2?

2) If not, then how are Tprime2Mean related to T_sgs?

3) I am trying to compare <T_measured> (time averaged mean values) with simulations and heance I compare it with T_mean as obtained from mean suing fieldAverage calculation in OpenFOAM. I am wondering if this is an apple-to-apple comparison, bececause T_mean from openFOAM is mean of the resolved scale values and not the mean of instantaneous values as calulated for measurements.

Please share your thoughts and I think this is an important point for folks using LES and comparison with measurements.

Thanks,
Nir

[s-ammarlu]

hi fomers
i want to simulate , turbulent flow in a square channel with oodles solver , i use LES model with smagorinsky , i want to know what i set for boundary condition for nu Sgs in inlet , outlet , wall , and symmetrry plane ? is zerogradient suitable ?

[yashar.afarin]

Originally Posted by gregor

The error message is because your domain is not a box. If look at the KMesh.C file it is counting all cells along every direction. Then it multiplies the cell numbers and if they do not match the total number of cells it raises an error.

gregor

Hi gregor;

really thanks for your post.
I used LES and I want to draw E(k)-K, but my domian is not a box (a cylinder). how can I use the code in dnsfoam? is it possible?
I would appreciate any help from you.

best regards.

[dhruv]

Hi Alberto,

I downloaded your version of perturbU since I was having the same problem as you described below. However, now it throws up a similar error saying

perturbU.C: In function ‘int main(int, char**)’:
perturbU.C:162: error: ‘mathematicalConstant’ has not been declared
perturbU.C:165: error: ‘mathematicalConstant’ has not been declared
make: *** [Make/linux64GccDPOpt/perturbU.o] Error 1

Can you tell me;
1) What is the mathematical constant?
2) How can I implement it in the code and compile it.
3) What is the significance of the constant?

Thanks in advance,
Dhruv.

Originally Posted by alberto

Compiling perturbU in OpenFOAM 1.3 gives this error:

Making dependency list for source file perturbU.C
could not open file fvCFD.H for source file perturbU.C

due to incomplete options file. Correcting it gives:

perturbU.C: In function 'int main(int, char**)':
perturbU.C:162: error: 'physicalConstant' has not been declared
perturbU.C:165: error: 'physicalConstant' has not been declared

because physicalConstant has been renamed to mathematicalConstant.

I attach the corrected version of the tool.

Best regards,
Alberto

[achinta]

Hello everyone,
I am using OF-2.1.1 OneEqEddy LES model for my case having 6.5 million cells. I imported the mesh from fluent. checkMesh said the mesh is OK but it has non orthogonality:
----------------
Checking geometry...
Overall domain bounding box (-1.47 -0.17 -0.19) (0.384 0.17 0.19)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (9.64958e-17 2.34786e-15 -6.13025e-16) OK.
Max cell openness = 4.58304e-15 OK.
Max aspect ratio = 299.485 OK.
Minumum face area = 3.41806e-11. Maximum face area = 0.000249108. Face area magnitudes OK.
Min volume = 1.22828e-14. Max volume = 4.16394e-07. Total volume = 0.20005. Cell volumes OK.
Mesh non-orthogonality Max: 87.0638 average: 19.2898
*Number of severely non-orthogonal faces: 18931.
Non-orthogonality check OK.
<<Writing 18931 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 2.88371 OK.
Coupled point location match (average 0) OK.
Mesh OK.
----------------


I gave appropriate boundary conditions. I mention some of them which could be wrong(please correct me).

1) There are 4 mass flow inlets where i gave the following in /0/U file:
----
type flowRateInletVelocity;
flowRate constant <value>;
value uniform (0 0 0);
----
There is a velocity inlet for which i gave conditions as usual.
type fixedValue;
value uniform (<value> 0 0);
-----

2) pressure: All patches/walls except outlet(p=0) have 0 gradient.

3) B
Internal field, velocity and mass flow inlets have 0 value.
exit and walls have 0 gradient.

4) k (turbulent kinetic energy)
Internal field has k=0.8 (same as velocity inlet)
mass flow inlets(assumed to have negligible turbulence) have k=1e-2 (arbitrary value)
Velocity inlet has k=0.8
exit: 0 gradient
walls: {type kqRWallFunction; value uniform 0.8;}

5)nuSgs
internalfield: 1e-7 (arbitrary value)
Inlets and exit: 0 gradient
Walls: { type nuSgsUSpaldingWallFunction;
value uniform 1e-7; }

--------------------------------------------------------

For delta, i am using 'cubeRootVol'

fvSchemes and fvSolution are the same as the one used in TUTORIALS "incompressible/pisoFoam/les/pitzDaily".

I am running it on 4 nodes.

After few time steps it diverges. k goes unbound and residuals of p increase:
----------------
Time = 1e-09

Courant Number mean: 3.82832e-07 max: 0.00098636
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 8.89837e-10, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 9.24966e-10, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 1.81297e-09, No Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.0492102, No Iterations 841
time step continuity errors : sum local = 3.97898e-10, global = 7.55946e-12, cumulative = 7.55946e-12
DICPCG: Solving for p, Initial residual = 0.156543, Final residual = 1.67279e-06, No Iterations 1001
time step continuity errors : sum local = 7.68918e-13, global = 7.51877e-15, cumulative = 7.56698e-12
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 1.83321e-06, No Iterations 1
bounding k, min: -3.30181e-05 max: 8.65 average: 1.64454e-06
ExecutionTime = 1372 s ClockTime = 1383 s
..
..
...
...
Time = 5e-09

Courant Number mean: 1.71033e-06 max: 0.089907
DILUPBiCG: Solving for Ux, Initial residual = 0.00110495, Final residual = 7.5732e-09, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.0157435, Final residual = 2.62783e-07, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.0154086, Final residual = 3.92554e-07, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.529496, Final residual = 0.0254955, No Iterations 14
time step continuity errors : sum local = 9.93601e-10, global = 2.7549e-12, cumulative = 1.30333e-11
DICPCG: Solving for p, Initial residual = 0.437915, Final residual = 2.59646e-06, No Iterations 1001
time step continuity errors : sum local = 9.63605e-14, global = 7.5182e-16, cumulative = 1.30341e-11
DILUPBiCG: Solving for k, Initial residual = 0.00816952, Final residual = 1.52233e-06, No Iterations 2
bounding k, min: -0.0225029 max: 319157 average: 0.485327
ExecutionTime = 5485.57 s ClockTime = 5603 s

Time = 6e-09

Courant Number mean: 1.71111e-06 max: 0.126074
DILUPBiCG: Solving for Ux, Initial residual = 0.000781675, Final residual = 3.83783e-08, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.0120933, Final residual = 5.34931e-07, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.0111096, Final residual = 9.24812e-07, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.69218, Final residual = 0.0339392, No Iterations 13
time step continuity errors : sum local = 1.60353e-09, global = 7.22851e-13, cumulative = 1.3757e-11
DICPCG: Solving for p, Initial residual = 0.684253, Final residual = 4.81795e-06, No Iterations 1001
time step continuity errors : sum local = 2.54543e-13, global = 1.56233e-15, cumulative = 1.37585e-11
DILUPBiCG: Solving for k, Initial residual = 0.0184975, Final residual = 2.59942e-07, No Iterations 3
bounding k, min: -6.54063 max: 1.7305e+07 average: 23.2609
ExecutionTime = 6482.16 s ClockTime = 6622 s

Courant Number mean: 1.72122e-06 max: 0.459119
DILUPBiCG: Solving for Ux, Initial residual = 0.000715073, Final residual = 1.65796e-07, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.0119322, Final residual = 2.4439e-06, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.00885946, Final residual = 2.70834e-06, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.853146, Final residual = 1.58563e-05, No Iterations 1001
time step continuity errors : sum local = 1.40116e-12, global = 2.70491e-15, cumulative = 1.37612e-11
DICPCG: Solving for p, Initial residual = 0.842176, Final residual = 2.86118e-05, No Iterations 1001
time step continuity errors : sum local = 3.19604e-12, global = 1.44523e-14, cumulative = 1.37757e-11
DILUPBiCG: Solving for k, Initial residual = 0.0295402, Final residual = 6.14694e-06, No Iterations 4
bounding k, min: -1010.36 max: 1.49557e+09 average: 1435.33
ExecutionTime = 7972.54 s ClockTime = 8197 s

-------------------
THIS IS THE ERROR MESSAGE
-------------------
#0 Foam::error:rintStack(Foam::Ostream&) in "/gt/home/h112812/OpenFOAM/ OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #1 Foam::sigFpe::sigHandler(int) in "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1 .1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #2 __restore_rt at sigaction.c:0
[3] #3 Foam:ILUPreconditioner::calcReciprocalD(Foam::Fi eld<double>&, Foam::ld uMatrix const&) in "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gc cDPOpt/lib/libOpenFOAM.so"
[3] #4 Foam:ILUPreconditioner:ILUPreconditioner(Foam: :lduMatrix::solver con st&, Foam::dictionary const&) in "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platf orms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #5 Foam::lduMatrix:reconditioner::addasymMatrixCons tructorToTable<Foam: ILUPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libO penFOAM.so"
[3] #6 Foam::lduMatrix:reconditioner::New(Foam::lduMatr ix::solver const&, Foa m::dictionary const&) in "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/lin ux64GccDPOpt/lib/libOpenFOAM.so"
[3] #7 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, uns igned char) const in "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64 GccDPOpt/lib/libOpenFOAM.so"
[3] #8 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/gt/home/h112 812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[3] #9 Foam::fvMatrix<double>::solve() in "/gt/home/h112812/OpenFOAM/OpenFOAM-2 .1.1/platforms/linux64GccDPOpt/bin/pisoFoam"
[3] #10 Foam::incompressible::LESModels:neEqEddy::correc t(Foam::tmp<Foam::Geo metricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh> > const&) i n "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libinc ompressibleLESModels.so"
[3] #11 Foam::incompressible::LESModel::correct() in "/gt/home/h112812/OpenFOAM /OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so"
[3] #12 main in "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccD POpt/bin/pisoFoam"
[3] #13 __libc_start_main in "/lib64/tls/libc.so.6"
[3] #14 _start in "/gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64Gc cDPOpt/bin/pisoFoam"

[cubad10269:07980] *** Process received signal ***
[cubad10269:07980] Signal: Floating point exception (8)
[cubad10269:07980] Signal code: (-6)
[cubad10269:07980] Failing at address: 0x11c6c00001f2c
[cubad10269:07980] [ 0] /lib64/tls/libc.so.6 [0x384322e2f0]
[cubad10269:07980] [ 1] /lib64/tls/libc.so.6(gsignal+0x3d) [0x384322e25d]
[cubad10269:07980] [ 2] /lib64/tls/libc.so.6 [0x384322e2f0]
[cubad10269:07980] [ 3] /gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux 64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam18DILUPreconditioner15calcR eciprocalDERNS_ 5FieldIdEERKNS_9lduMatrixE+0xb5) [0x2a97b8eff5]
[cubad10269:07980] [ 4] /gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux 64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam18DILUPreconditionerC1ERKNS _9lduMatrix6sol verERKNS_10dictionaryE+0x159) [0x2a97b8f819]
[cubad10269:07980] [ 5] /gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux 64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam9lduMatrix14preconditioner3 1addasymMatrixC onstructorToTableINS_18DILUPreconditionerEE3NewERK NS0_6solverERKNS_10dictionaryE +0x3c) [0x2a97b8f92c]
[cubad10269:07980] [ 6] /gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux 64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam9lduMatrix14preconditioner3 NewERKNS0_6solv erERKNS_10dictionaryE+0x7ef) [0x2a97b7ebaf]
[cubad10269:07980] [ 7] /gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux 64GccDPOpt/lib/libOpenFOAM.so(_ZNK4Foam5PBiCG5solveERNS_5FieldIdE ERKS2_h+0x6e3) [0x2a97b83853]
[cubad10269:07980] [ 8] /gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux 64GccDPOpt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE5solveERKNS _10dictionaryE+ 0x157) [0x2a969c3df7]
[cubad10269:07980] [ 9] pisoFoam(_ZN4Foam8fvMatrixIdE5solveEv+0xd3) [0x421a13]
[cubad10269:07980] [10] /gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux 64GccDPOpt/lib/libincompressibleLESModels.so(_ZN4Foam14incompress ible9LESModels9 oneEqEddy7correctERKNS_3tmpINS_14GeometricFieldINS _6TensorIdEENS_12fvPatchFieldE NS_7volMeshEEEEE+0x743) [0x2a95d9c443]
[cubad10269:07980] [11] /gt/home/h112812/OpenFOAM/OpenFOAM-2.1.1/platforms/linux 64GccDPOpt/lib/libincompressibleLESModels.so(_ZN4Foam14incompress ible8LESModel7c orrectEv+0x35) [0x2a95d10275]
[cubad10269:07980] [12] pisoFoam [0x418ed4]
[cubad10269:07980] [13] /lib64/tls/libc.so.6(__libc_start_main+0xdb) [0x384321c3 fb]
[cubad10269:07980] [14] pisoFoam [0x41548a]
[cubad10269:07980] *** End of error message ***
--------------------------------------------
Could some please tell me where i went wrong?
1) Is it because of non-orthogonality of the mesh?
2) Domain size is 1.8*0.4*0.4 cubic meters. and it has 6.5 million cells. Is it too refined to use wall functions near the wall?
3) Should i change discretization schemes?

------
ddtSchemes
{
default backward;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss filteredLinear;
div(phi,k) Gauss limitedLinear 1;
div(phi,B) Gauss limitedLinear 1;
div(phi,nuTilda) Gauss limitedLinear 1;
div(B) Gauss linear;
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(DBEff,B) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}
interpolationSchemes
{
default linear;
interpolate(U) linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p ;
}
------

4) Should i change fvSolution? I am using DICPCG for p and DILUPBiCG for U and k with
---
PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
----

Please let me know if you need more details to figure out the problem.

Kind regards,
Achinta

[robbirobocop]

Well, two hints that subsequetly come to my mind when I read your post.

Firstly, try to set nNonOrthogonalCorrectors higher. Your value of 0 won't correct nonOrthogonality... Try to go with 2 since your mesh with about 6.5 million cells will take a lot more with increasing the number of correctors.

Secondly, you should initialise k with a higher value (the internalFields). That might help.

Use GAMG for p. (There are a lot of tutorials on how to change the fvSolution in order to use GAMG.

[achinta]

Hi Rob,
Thanks for the reply.
1) I tried different value for k (updated in the previous thread).
2) I used nNonOrthogonalCorrectors=1 since nNonOrthogonalCorrectors=2 takes lot of time.
3) I have read in some posts that GAMG is good for serial computing and PCG is good for parallel computing So i continued with PCG only.(please check http://www.cfd-online.com/Forums/ope...ure-issue.html )
Please tell me your opinion. Is there a great difference between GAMG and PCG results?

With the above corrections, the solution is diverging again. Do you think nNonOrthogonalCorrectors=2/GAMG can stabilize the results?

I kindly request other users opinion also .

Kind regards,
Achinta

[robbirobocop]

I doubt that GAMG will stabilise your solution.
Maybe you should send someone your case so he or she can check some possibilities...
Or you should at least provide some more information

By the way, I usually use "Euler" instead of "backward" for ddtSchemes.

[JoaoDMiranda]

Does anyone have the compressible LES lowReOneEqEddy reference? I can't find it anywhere?

Thanks a lot for your help.

João.