|
[Sponsors] |
August 19, 2010, 07:09 |
bubbleFoam validation case
|
#1 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
I faced the following difficulty.
I switch off the dispersed phase volume fraction at inlet . That is inlet alpha = uniform 0 and also the dispersed phase velocity . I keep my continuous phase velocity Ub = 0.1 m/s . Continuous properties are rho = 1000 kg/m3 , nu = 1e-06 m2/s . This means now i am studying single phase flow . I compared the results to simpleFoam results and have found a problem with the velocity plots in the plane z=0.2 on the same timestep . Specifically on the line joining (0 0.5 0.2) and (1 0.5 0.2) . Can someone help me resolve this issue .... My blockMeshDict is as follows : Code:
/*--------------------------------*- C++ -*----------------------------------* \ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 1; vertices ( (0 0 0) (0.25 0 0) (0.25 0.25 0) (0 0.25 0) (0 0.75 0) (0.25 0.75 0) (0 1 0) (0.25 1 0) (0.75 0 0) (0.75 0.25 0) (1 0 0) (1 0.25 0) (0.75 0.75 0) (1 0.75 0) (0.75 1 0) (1 1 0) (0 0 2) (0.25 0 2) (0.25 0.25 2) (0 0.25 2) (0 0.75 2) (0.25 0.75 2) (0 1 2) (0.25 1 2) (0.75 0 2) (0.75 0.25 2) (1 0 2) (1 0.25 2) (0.75 0.75 2) (1 0.75 2) (0.75 1 2) (1 1 2) ); blocks ( hex (0 1 2 3 16 17 18 19) (10 10 10) simpleGrading (1 1 1) hex (3 2 5 4 19 18 21 20) (10 10 10) simpleGrading (1 1 1) hex (4 5 7 6 20 21 23 22) (10 10 10) simpleGrading (1 1 1) hex (1 8 9 2 17 24 25 18) (10 10 10) simpleGrading (1 1 1) hex (2 9 12 5 18 25 28 21) (10 10 10) simpleGrading (1 1 1) hex (5 12 14 7 21 28 30 23) (10 10 10) simpleGrading (1 1 1) hex (8 10 11 9 24 26 27 25) (10 10 10) simpleGrading (1 1 1) hex (9 11 13 12 25 27 29 28) (10 10 10) simpleGrading (1 1 1) hex (12 13 15 14 28 29 31 30) (10 10 10) simpleGrading (1 1 1) ); edges ( ); patches ( patch inlet ( (2 5 12 9) ) patch outlet ( (16 19 18 17) (19 20 21 18) (20 22 23 21) (17 18 25 24) (18 21 28 25) (21 23 30 28) (24 25 27 26) (25 28 29 27) (28 30 31 29) ) wall fixedWalls ( (0 16 19 3) (3 19 20 4) (4 20 22 6) (6 22 23 7) (7 23 30 14) (14 30 31 15) (15 31 29 13) (13 29 27 11) (11 27 26 10) (10 26 24 8) (8 24 17 1) (1 17 16 0) (0 3 2 1) (3 4 5 2) (4 6 7 5) (5 7 14 12) (12 14 15 13) (9 12 13 11) (8 9 11 10) (1 2 9 8) ) ); mergePatchPairs ( ); // ************************************************************************* // Last edited by balkrishna; August 19, 2010 at 07:50. |
|
August 20, 2010, 03:09 |
|
#2 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
How is the model set up in bubbleFoam? Are you using the turbulence model or performing a laminar simulation?
Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
August 20, 2010, 03:12 |
|
#3 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
I am performing a laminar simulation .
|
|
August 20, 2010, 03:23 |
|
#4 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Ignore my previous answer (removed). I generated the mesh, and run the case, noticing you have an expansion. Could you post your case setup?
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. Last edited by alberto; August 20, 2010 at 03:51. Reason: Corrected answer |
|
August 20, 2010, 03:52 |
|
#5 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
Thanks for the reply ...
I was unable to place an image of the mesh in the post ... I have uploaded the image of the mesh on the link ... Sorry for the inconvienience .... Secondly , I am not seeking convergence ... All that I am saying is if I switch off my dispersed phase , my equations reduce to those solved by simpleFoam and hence should give the same results at the same time on the same mesh . Do clarify me if I am wrong somewhere .... Last edited by balkrishna; August 20, 2010 at 04:10. |
|
August 20, 2010, 04:20 |
Case setup
|
#6 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
Alpha :
Code:
/*--------------------------------*- C++ -*----------------------------------* \ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object alpha; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 0 0 0 0]; internalField uniform 0 ; boundaryField { inlet { type fixedValue; value uniform 0; } outlet { type zeroGradient; } fixedWalls { type zeroGradient; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -2 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } fixedWalls { type buoyantPressure; value uniform 0; } defaultFaces { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object Ub; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { inlet { type fixedValue; value uniform (0 0 0.1); } outlet { type zeroGradient; } fixedWalls { type fixedValue; value uniform (0 0 0); } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object Ua; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0) ; boundaryField { inlet { type fixedValue; value uniform (0 0 0); } outlet { type zeroGradient; } fixedWalls { type fixedValue; value uniform (0 0 0); } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 1e-8; boundaryField { inlet { type fixedValue; value uniform 1e-8; } outlet { type inletOutlet; inletValue uniform 1e-8; value uniform 1e-8; } fixedWalls { type zeroGradient; } defaultFaces { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object epsilon; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -3 0 0 0 0]; internalField uniform 0.1; boundaryField { inlet { type fixedValue; value uniform 0.1; } outlet { type zeroGradient; } fixedWalls { type zeroGradient; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application bubbleFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 2; deltaT 0.001; writeControl runTime; writeInterval 0.5; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression uncompressed; timeFormat general; timePrecision 6; runTimeModifiable yes; // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phia,Ua) Gauss limitedLinearV 1; div(phib,Ub) Gauss limitedLinearV 1; div(phib,k) Gauss limitedLinear 1; div(phib,epsilon) Gauss limitedLinear 1; div(phi,alpha) Gauss limitedLinear01 1; div((-nuEffa*grad(Ua).T())) Gauss linear; div((-nuEffb*grad(Ub).T())) Gauss linear; } laplacianSchemes { default none; laplacian(nuEffa,Ua) Gauss linear corrected; laplacian(nuEffb,Ub) Gauss linear corrected; laplacian((rho*(1|A(U))),p) Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p { solver PCG; preconditioner DIC; tolerance 1e-10; relTol 0; } Ua { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0; } Ub { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0; } alpha { solver PBiCG; preconditioner DILU; tolerance 1e-10; relTol 0; } beta { solver PBiCG; preconditioner DILU; tolerance 1e-10; relTol 0; } k { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0; } epsilon { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0; } } PISO { nCorrectors 2; nNonOrthogonalCorrectors 0; nAlphaCorr 2; correctAlpha no; pRefCell 0; pRefValue 0; } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class uniformDimensionedVectorField; location "constant"; object g; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -2 0 0 0 0]; value ( 0 0 -9.81 ); // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object RASProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // RASModel laminar; turbulence off; printCoeffs off; // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object transportProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // rhoa rhoa [ 1 -3 0 0 0 0 0 ] 1; rhob rhob [ 1 -3 0 0 0 0 0 ] 1000; nua nua [ 0 2 -1 0 0 0 0 ] 1.6e-05; nub nub [ 0 2 -1 0 0 0 0 ] 1e-06; da da [ 0 1 0 0 0 0 0 ] 0.003; db db [ 0 1 0 0 0 0 0 ] 0.0001; Cvm Cvm [ 0 0 0 0 0 0 0 ] 0.5; Cl Cl [ 0 0 0 0 0 0 0 ] 0; Ct Ct [ 0 0 0 0 0 0 0 ] 1; // ************************************************************************* // |
|
August 20, 2010, 04:47 |
|
#7 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
You are correct. The result should be the same.
Did you use the same numerical schemes and the same tolerances in the linear solvers also in simpleFoam? Also, set to zero the lift (Cl), virtual mass coefficients (Cvm) and Ct (not necessary in theory, since bubbleFoam uses a formulation depending on alpha, so these term should be zero automatically). Best, Alberto
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. Last edited by alberto; August 20, 2010 at 04:58. Reason: precised question and added clarification |
|
August 20, 2010, 04:50 |
|
#8 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
Will recheck on the same .... Thanks for the help ...
Last edited by balkrishna; August 20, 2010 at 05:16. |
|
August 20, 2010, 05:38 |
|
#9 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
Yes checked it .... the schemes are the same ....
|
|
August 20, 2010, 06:17 |
|
#10 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
But they should not matter as alpha or the dispersed phase is 0 . Those equations are written for the dispersed phase ....
|
|
August 20, 2010, 13:32 |
|
#11 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Yes that's correct. I was just removing everything term that makes the two equations different.
The only additional difference I see in your files is g. There is no g in simpleFoam. Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
August 20, 2010, 13:34 |
|
#12 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
inclusion of g is only going to affect the pressure contours ... not the velocity plots ...
thanks ... |
|
August 20, 2010, 13:45 |
|
#13 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
I did not imply this is going to cause a difference in the velocity plot, just that the only physical element of difference is that one in the equations.
The difference in the two solutions is located essentially at the walls, and the rest of the profile adapts as a consequence. At what tolerance is the solution converged? Would you share a case so I can take a look at it (I sent my email address if you cannot upload)? Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
August 20, 2010, 17:36 |
|
#14 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Since I was a bit puzzled by the problem, because I did a similar validation in the past, I run a simpler case of a flow between two parallel plates.
You find the cases here: http://dl.dropbox.com/u/659842/bubbl...bleFoam.tar.gz And as you can see in the attached picture, the velocity profiles are identical. Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
August 21, 2010, 04:15 |
|
#15 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
your test case works great . have you found any problem in my case setup ?
|
|
August 21, 2010, 04:33 |
|
#16 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Hi,
the case you sent me stops at 2 seconds, which is not enough for the solution to reach convergence. You might want to run the case with a larger time step (0.1 for example, or a bit smaller if you want residuals to be low) until t = 1000. Additionally, the contour plots show quite a clear influence of the mesh on the solution, mainly due to the non-uniformity and the jumps in grid size between the different blocks. I hope this helps. Best,
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
August 27, 2010, 04:40 |
modifying bubbleFoam
|
#17 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
I wish to modify bubble Foam of 2 phases to n phase and add heat transfer and species mixing to it .. One stumbling block i came across was the way the alpha equation was programmed .
it consists of the following line in the header file alphaEqn.H Code:
word scheme("div(phi,alpha)"); surfaceScalarField phir = phia - phib; |
|
August 27, 2010, 04:50 |
|
#18 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Silva and Lage did it and have a conference paper on this topic. Check your email :-)
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
August 27, 2010, 05:00 |
|
#19 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
thanks a lot .....
|
|
August 30, 2010, 02:46 |
|
#20 |
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 17 |
Thanks for the link .... Can i get the source code of the solver ?? The implementation of the algorithm is the tough aspect in OpenFOAM .....
|
|
Tags |
bubble, bubblefoam, foam |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Comparison of axisymmetric case, Starccm+ and OpenFOAM | linnemann | OpenFOAM Running, Solving & CFD | 12 | June 16, 2011 06:43 |
Need help to open an OpenFoam case with Paraviw | aaurouss | OpenFOAM | 2 | July 6, 2009 14:18 |
Validation Case | Ruben | Main CFD Forum | 0 | November 1, 2005 11:50 |
Validation case for turbulent flow | Ratan | Main CFD Forum | 0 | October 4, 2005 04:03 |
Validation case for turbulent flow | Ratan | Main CFD Forum | 0 | October 4, 2005 04:02 |