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 steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) 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; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(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; } snGradSchemes { default corrected; } fluxRequired { default no; p; } *************************** The fvSolution file is: *************************** solvers { p GAMG { tolerance 1e6; relTol 0.01; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; }; U smoothSolver { smoother GaussSeidel; nSweeps 2; tolerance 1e8; relTol 0.1; }; k PBiCG { preconditioner DILU; tolerance 1e05; relTol 0.1; }; epsilon PBiCG { preconditioner DILU; tolerance 1e05; relTol 0.1; }; R PBiCG { preconditioner DILU; tolerance 1e05; relTol 0.1; }; nuTilda smoothSolver { smoother GaussSeidel; nSweeps 2; tolerance 1e8; 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 = 5.86040152799e05, No Iterations 4 GAMG: Solving for p, Initial residual = 0.00071885457453, Final residual = 5.72054751809e06, No Iterations 5 GAMG: Solving for p, Initial residual = 0.000126793712278, Final residual = 7.18547241099e07, No Iterations 5 time step continuity errors : sum local = 3.07898278868e11, global = 2.00751370042e14, cumulative = 5.60535949412e11 ExecutionTime = 1826.51 s ClockTime = 1826 s *************************** As we could see the residual for U and p is very large, here I use deltaT=1e02. I struggle at this model, may I ask if some one could give me some idea for this? Thank you. Bin 
Hi,
try changing relaxationFactors: { p 0.4; U 0.6; ... } and wait.... Marco 
Hi Marco,
Thank you for your attention. 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 = 5.6345388581e05, 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 = 3.86452241619e05, No Iterations 4 GAMG: Solving for p, Initial residual = 0.000463156930012, Final residual = 2.50732060428e06, No Iterations 6 GAMG: Solving for p, Initial residual = 7.89315428925e05, Final residual = 6.66690439345e07, No Iterations 4 time step continuity errors : sum local = 2.59918498834e11, global = 2.10847262229e14, cumulative = 3.47871725926e12 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 (nonempty) directions (1 1 0) Mesh (nonempty, nonwedge) dimensions 2 All edges aligned with or perpendicular to nonempty directions. Boundary openness (5.40237466474e20 4.34269087253e18 1.95015090065e14) OK. Max cell openness = 3.18619574257e16 OK. Max aspect ratio = 80.0001195999 OK. Minumum face area = 3.10546639285e05. Maximum face area = 0.0736848781216. Face area magnitudes OK. Min volume = 3.62305447655e07. Max volume = 0.000859659367582. Total volume = 130.215018482. Cell volumes OK. Mesh nonorthogonality Max: 85.6112588833 average: 6.3947096647 *Number of severely nonorthogonal faces: 15. Nonorthogonality check OK. <<Writing 15 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 2.92248322884 OK. Mesh OK. ************************ Is it because "severely nonorthogonal faces"? I use Gmsh to build my model, with local fine meshing method. Welcome again for comment. Bin Quote:

Quote:
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 STARCD? 
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 
Hi Olesen and Marico,
Thank you for your attention. 1. Do you have the same viscosity as the STARCD model? Ans: I set in the file transportProperties : nu [0 2 1 0 0 0 0] 1.51e05; 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 STARCD? 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 19:54. 