CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Low pressure drop with the same model (http://www.cfd-online.com/Forums/openfoam-solving/65434-low-pressure-drop-same-model.html)

 zhoubinwx June 15, 2009 04:56

Low pressure drop with the same model

Dear foamers,

I am simulating on a model, which has already simulated by my professor using StarCD. With the same model and same inlet velocity, my professor's pressure drop is 168Pa. While I use simpleFoam in OF, I could not get converged results, and the simulated pressure drop is only 0.004993Pa.

The fvScheme file is:
***************************
ddtSchemes
{
}
{
default Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
}
laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}
interpolationSchemes
{
default linear;
interpolate(U) linear;
}
{
default corrected;
}
fluxRequired
{
default no;
p;
}
***************************
The fvSolution file is:
***************************
solvers
{
p GAMG
{
tolerance 1e-6;
relTol 0.01;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};
U smoothSolver
{
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-8;
relTol 0.1;
};
k PBiCG
{
preconditioner DILU;
tolerance 1e-05;
relTol 0.1;
};
epsilon PBiCG
{
preconditioner DILU;
tolerance 1e-05;
relTol 0.1;
};
R PBiCG
{
preconditioner DILU;
tolerance 1e-05;
relTol 0.1;
};

nuTilda smoothSolver
{
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-8;
relTol 0.1;
};
}
SIMPLE
{
nNonOrthogonalCorrectors 3;
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
p 0.3;
U 0.7;
k 0.7;
epsilon 0.7;
R 0.7;
nuTilda 0.7;
}
***************************
The log file is:
***************************
Time = 2.3

smoothSolver: Solving for Ux, Initial residual = 0.0039317624097, Final residual = 0.00028429926006, No Iterations 4
smoothSolver: Solving for Uy, Initial residual = 0.00575887542213, Final residual = 0.000439263248628, No Iterations 4
GAMG: Solving for p, Initial residual = 0.0604334923612, Final residual = 0.000305639970335, No Iterations 5
GAMG: Solving for p, Initial residual = 0.00991415857267, Final residual = 5.86040152799e-05, No Iterations 4
GAMG: Solving for p, Initial residual = 0.00071885457453, Final residual = 5.72054751809e-06, No Iterations 5
GAMG: Solving for p, Initial residual = 0.000126793712278, Final residual = 7.18547241099e-07, No Iterations 5
time step continuity errors : sum local = 3.07898278868e-11, global = -2.00751370042e-14, cumulative = -5.60535949412e-11
ExecutionTime = 1826.51 s ClockTime = 1826 s
***************************

As we could see the residual for U and p is very large, here I use deltaT=1e-02.

I struggle at this model, may I ask if some one could give me some idea for this? Thank you.

Bin

 marico June 15, 2009 05:32

Hi,

try changing relaxationFactors:
{
p 0.4;
U 0.6;
...
}

and wait....

Marco

 zhoubinwx June 16, 2009 02:17

Hi Marco,

Now I have set in fvSolution file:
************************
relaxationFactors
{
p 0.4;//0.3;
U 0.6;//0.7;
k 0.7;
epsilon 0.7;
R 0.7;
nuTilda 0.7;
}
************************
I still get low pressure drop (0.00904) with simpleFoam solver.
Now the log file is:
************************
Time = 35.43
smoothSolver: Solving for Ux, Initial residual = 0.00203370891239, Final residual = 5.6345388581e-05, No Iterations 4
smoothSolver: Solving for Uy, Initial residual = 0.00356242994235, Final residual = 0.000104210543403, No Iterations 4
GAMG: Solving for p, Initial residual = 0.0364082592636, Final residual = 0.000304828677232, No Iterations 4
GAMG: Solving for p, Initial residual = 0.00478820727082, Final residual = 3.86452241619e-05, No Iterations 4
GAMG: Solving for p, Initial residual = 0.000463156930012, Final residual = 2.50732060428e-06, No Iterations 6
GAMG: Solving for p, Initial residual = 7.89315428925e-05, Final residual = 6.66690439345e-07, No Iterations 4
time step continuity errors : sum local = 2.59918498834e-11, global = -2.10847262229e-14, cumulative = -3.47871725926e-12
ExecutionTime = 19303.1 s ClockTime = 19303 s
************************
Now I post my checkMesh log here, I wonder if the mesh quality of fine enough.
************************
Checking geometry...
Overall domain bounding box (-120 0 -0.007) (470 20.001 0.0046667)
Mesh (non-empty) directions (1 1 0)
Mesh (non-empty, non-wedge) dimensions 2
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (5.40237466474e-20 -4.34269087253e-18 -1.95015090065e-14) OK.
Max cell openness = 3.18619574257e-16 OK.
Max aspect ratio = 80.0001195999 OK.
Minumum face area = 3.10546639285e-05. Maximum face area = 0.0736848781216. Face area magnitudes OK.
Min volume = 3.62305447655e-07. Max volume = 0.000859659367582. Total volume = 130.215018482. Cell volumes OK.
Mesh non-orthogonality Max: 85.6112588833 average: 6.3947096647
*Number of severely non-orthogonal faces: 15.
Non-orthogonality check OK.
<<Writing 15 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 2.92248322884 OK.
Mesh OK.
************************
Is it because "severely non-orthogonal faces"? I use Gmsh to build my model, with local fine meshing method.

Welcome again for comment.

Bin

Quote:
 Originally Posted by marico (Post 219315) Hi, try changing relaxationFactors: { p 0.4; U 0.6; ... } and wait.... Marco

 olesen June 16, 2009 02:23

Quote:
 Originally Posted by zhoubinwx (Post 219305) While I use simpleFoam in OF, I could not get converged results, and the simulated pressure drop is only 0.004993Pa.
1. Do you have the same viscosity as the STAR-CD model?
2. Are you sure about the units of pressure 'p', or do they perhaps include the viscosity (since you are using an incompressible solver 'simpleFoam').
3. Is it possible that you have a different scaling (eg, mm vs. m) when you imported the model from STAR-CD?

 marico June 16, 2009 02:44

Hi,

what is about the turbulence model? You seem to use laminar, since there are no turbulence equations solved... Did your Prof also?
And what about the yPlus values? You could check them to see whether your mesh is appropriate for the case with yPlusRAS..

Marco

 zhoubinwx June 16, 2009 05:10

Hi Olesen and Marico,

1. Do you have the same viscosity as the STAR-CD model?
Ans: I set in the file transportProperties :
nu [0 2 -1 0 0 0 0] 1.51e-05;

2. Are you sure about the units of pressure 'p', or do they perhaps include the viscosity (since you are using an incompressible solver 'simpleFoam').
Ans: in 0/p file, dimension of p is [0 2 -2 0 0 0 0];
I set 0 for internal field and pressure outlet;

3. Is it possible that you have a different scaling (eg, mm vs. m) when you imported the model from STAR-CD?
Ans: ***** This is the reason******

When I check by the sequence of the post, I find that I use mm instead of micrometer when I convert my mesh.

Therefore I didn't check Marco's suggestions, Hi, sorry Marco :)

Thank you again for your enthusiasm and kindness.

Grazie.

Bin

 All times are GMT -4. The time now is 22:41.