[Jiricbeng]

Hi there,

please help me with the following:
I wish to calculate 3D geometry as an incompressible k-epsilon model with boundary conditions - velocity inlet and pressure outlet (which is likely the most humble task).
Below you can see the individual files. I would be very grateful for any help. I think the problem is especially in settings of k and epsilon..
Thank you very much


wall-4 is inlet
wall-5 is outlet.


The folder 0/p:


internalField uniform 0;
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
wall-4
{
type zeroGradient;
}
wall-5
{
type fixedValue;
value uniform 0;
}
wall-3
{
type zeroGradient;
}
wall-6
{
type zeroGradient;
}
wall-7
{
type zeroGradient;
}
}
***************



The folder 0/U:

internalField uniform (0 0 0);
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
wall-4
{
type fixedValue;
value uniform (0 0 1);
}
wall-5
{
type zeroGradient;
}
wall-3
{
type zeroGradient;
}
wall-6
{
type zeroGradient;
}
wall-7
{
type zeroGradient;
}
}
**********************




The folder 0/epsilon:


dimensions [0 2 -3 0 0 0 0];

internalField uniform 8.87;
boundaryField
{
wall-3
{
type zeroGradient;
value uniform 8.87;
}
wall-4
{
type freestream;
freestreamValue uniform 8.87;
}
wall-5
{
type zeroGradient;
}
wall-6
{
type zeroGradient;
value uniform 8.87;
}
wall-7
{
type zeroGradient;
value uniform 8.87;
}
}
*******************



The folder 0/k:


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

internalField uniform 0.0158;
boundaryField
{
wall-3
{
type zeroGradient;
value uniform 0.0158;
}
wall-4
{
type freestream;
freestreamValue uniform 0.0158;
}
wall-5
{
type zeroGradient;
}
wall-6
{
type zeroGradient;
value uniform 0.0158;
}
wall-7
{
type zeroGradient;
value uniform 0.0158;
}
}



The folder 0/nut:

dimensions [0 2 -1 0 0 0 0];

internalField uniform 0.14;
boundaryField
{
wall-4
{
type calculated;
value $internalField;
}
wall-5
{
type calculated;
value $internalField;
}
wall-3
{
type nutkWallFunction;
value $internalField;
}
wall-6
{
type nutkWallFunction;
value $internalField;
}
wall-7
{
type nutkWallFunction;
value $internalField;
}
}
****************




The folder system/controlDict:

libs
(
"libOpenFOAM.so"
"libincompressibleTurbulenceModel.so"
"libincompressibleRASModels.so"
);
application simpleFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 150;

deltaT 1;

writeControl timeStep;

writeInterval 10;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression uncompressed;

timeFormat general;

timePrecision 6;

runTimeModifiable true;
**************************




The folder system/fvSchemes:

ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss limitedLinearV 1;
div(phi,k) bounded Gauss limitedLinear 1;
div(phi,epsilon) bounded Gauss limitedLinear 1;
div(phi,R) bounded Gauss limitedLinear 1;
div(R) Gauss linear;
div(phi,nuTilda) bounded Gauss limitedLinear 1;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p ;
}
*********************





The folder system/fvSolution:

solvers
{
p
{
solver GAMG;
smoother GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
tolerance 1e-06;
relTol 0.05;
}
pFinal
{
$p;
tolerance 1e-06;
relTol 0;
}

"(U|k|epsilon)"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-05;
relTol 0.1;
}

"(U|k|epsilon)Final"
{
$U;
tolerance 1e-05;
relTol 0;
}
nuTilda
{
solver smoothSolver;
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-08;
relTol 0.1;
}
}
PIMPLE
{
nOuterCorrectors 4;
nCorrectors 1;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
residualControl
{
p 1e-2;
U 1e-3;
"(k|epsilon)" 1e-3;
}
}
relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
k 0.7;
"epsilon.*" 0.7;
}
}
cache
{
grad(U);
}

[gonpe]

Check your syntax for the inlet k and epsilon. You can just use the fixedValue type as you did in the velocity specification.

Check out the pitzDaily tutorial under the /tutorials/incompressible/simpleFoam directory.

[Jiricbeng]

Thank you for reply. Although I amended the setting according to the Pitzdaily case, solution still fails and vectors in the domain are of zero size.
Have you another idea?

[gonpe]

What do you mean by fails?

What does your output look like?

[Jiricbeng]

I mean it goes down in 32nd iteration, writing "floating point exception, core dumped". I know the trouble is there is division by zero somewhere, but I do not know where. And if I look at the results from 20th iteration, the velocity vectors in the domain are zero sized. Therefore I assume a boundary condition must be wrong, but I cannot find out where as I created the text files in accordance with pitzDaily case.. I appreciate any help.

[Jiricbeng]

Obviously the trouble I am coming across:

time step continuity errors : sum local = 2.61612e+11, global = 3.17086e+09, cumulative = 3.17084e+09

and

bounding epsilon, min: -3.46871e-10 max: 1.19867e+08 average: 964.697

In the first 10 iterations velocity in the domain is non-zero but after 20 iterations velocities in the domain (as well as on the boundaries) are entirely of zero size, there is just no flux.

[gonpe]

Is this a simple channel? If so, what does the grid look like? Did you generate it with blockMesh?

Are you able to run a potentialFoam to set up the initial solution? See the potentialFoam tutorial directory.

[Jiricbeng]

This is a draft tube. Mesh is created in gridpro and is fully hexagonal. It was generated by using "fluentMeshToFoam Mymesh.msh". I am going to try out potentialFoam.

[CFDnewbie147]

Hello,

did you check the mesh with "checkMesh"? Are there any failures?

Another question: Is it right that you've the only velocity component in the z direction? Does this fit to your tube geometry? 1 m/s?

Did you try it without a turbulence model (laminar)? If it works laminar, you've to look for the failure while using a turbulence model.

Best regards
CFDNewbie147

[Jiricbeng]

I ve already solved out the problem, it was likely caused by a very high value of epsilon, beside that I deleted CrossPowerLawCoeffs from transportProperties and changed divSchemes in fvSchemes from bounded Gauss upwind to Gauss upwind. CheckMesh worked before the changes.
However, comparing results of the draft tube computed in OF and Fluent, although the setting is the same (k-epsilon etc), the results are different. Total pressure decrease in OF is 352Pa and in Fluent it is 297Pa.

[CFDnewbie147]

Do you use the same mesh or did you make one in OF with snappyHexMesh?

If it's not the same mesh you've used, the mesh could cause the difference. Did you make a mesh-refinement study?

[Jiricbeng]

It was the same mesh. I do not use snappyHexMesh, I create meshes in ansys. The problem was obviously caused by the boundary k epsilon values. I recommend using this calculation
http://www.cfd-online.com/Tools/turbulence.php