|
[Sponsors] |
August 8, 2009, 14:21 |
OpenFOAM - Validation of Results
|
#1 |
Senior Member
Ahmed
Join Date: Mar 2009
Location: NY
Posts: 251
Rep Power: 18 |
Being unhappy/disappointed with the results obtained by OpenFOAM after my first tutorial ( http://www.cfd-online.com/Forums/ope...-tutorial.html ) I decided to search for validation cases.
Searching the internet provides a good number of examples, but, in most of these cases, the results of OpenFOAM are presented as images, and comparing the results with those obtained by commercial solvers. 'This actually is not the correct way of validating a programme. When doing CFD analysis, the design engineer is looking for numerical values not pictures. I decided to open this thread looking for your help. I hope the so many users of openFOAM can share their results with new users like me. As a starter, I have prepared a case for the well documented flow over a flat plate, since we have the well known solution of Blasius. Here is the blockMesh Dictionary /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.6 | | \\ / A nd | Web: http://www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 1; vertices ( (0 0 0) (1 0 0) (1 0.1 0) (0 0.1 0) (0 0 0.1) (1 0 0.1) (1 0.1 0.1) (0 0.1 0.1) ); blocks ( hex (0 1 2 3 4 5 6 7) (100 50 1) simpleGrading (1 15 1) ); edges ( ); patches ( patch inlet ( (0 4 7 3) ) patch outlet ( (1 5 6 2) ) wall fixedWall ( (0 1 5 4) ) patch top ( (3 2 6 7) ) empty frontAndBack ( (0 1 2 3) (4 5 6 7) ) ); mergePatchPairs ( ); // ************************************************** *********************** // and the transport properties /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.6 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object transportProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // nu nu [ 0 2 -1 0 0 0 0 ] 15.08e-06; // ************************************************** *********************** // here we have the controlDictionary /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.6 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application icoFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 0.01; deltaT 1e-06; writeControl runTime; writeInterval 0.00015; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression uncompressed; timeFormat general; timePrecision 6; runTimeModifiable yes; // ************************************************** *********************** // here we have the initial conditions /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.6 | | \\ / A nd | Web: http://www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 101325; boundaryField { inlet { type fixedValue; value uniform 101325; } outlet { type zeroGradient; } fixedWall { type zeroGradient; } top { type fixedValue; value uniform 101325; } defaultFaces { type empty; } } // ************************************************** *********************** // and the U file /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.6 | | \\ / A nd | Web: http://www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (100.0 0.0 0); boundaryField { inlet { type fixedValue; value uniform (100.0 0 0); } outlet { type zeroGradient; } fixedWall { type fixedValue; value uniform (0 0 0); } top { type fixedValue; value uniform (100.0 0 0); } defaultFaces { type empty; } } // ************************************************** *********************** // I also attach images of the mesh and the results. I am looking for your comments and corrections, but most importantly, I hope the readers will add their own validation cases |
|
August 9, 2009, 04:01 |
|
#2 | |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Quote:
Out of joke, the idea of posting validation cases is surely interesting.
__________________
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 9, 2009, 04:38 |
|
#3 |
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Wernigerode, Sachsen-Anhalt, Germany
Posts: 281
Rep Power: 18 |
Dear Ahmed,
the Special Interest Group Turbomachinery is doing exactly what you describe. http://openfoamwiki.net/index.php/Sig_Turbomachinery They picked well-known validation cases http://openfoamwiki.net/index.php/Si...ion_test_cases ran the problem in different academic and commercial CFD groups compared the results with experimental data and presented the results at the workshop. The case setups and codes are available from sourceforge - So everybody can redo the exercise. Validation does not get better than this and it completely transparent - down to the last line of code. Henrik Last edited by henrik; August 9, 2009 at 12:38. |
|
August 9, 2009, 12:00 |
|
#4 | |
Senior Member
Ahmed
Join Date: Mar 2009
Location: NY
Posts: 251
Rep Power: 18 |
Quote:
You see, the U magnitude reported by my solution is greater than what I specified as the free stream condition, is my set up giving reasonable answers or is it the programme itself that is accumulating too much rounding errors? Good luck and waiting to see your comments soon |
||
August 9, 2009, 12:03 |
|
#5 | |
Senior Member
Ahmed
Join Date: Mar 2009
Location: NY
Posts: 251
Rep Power: 18 |
Quote:
Thanks for the information, I hope to see more validation cases on this forum Good Luck |
||
August 10, 2009, 10:11 |
|
#6 |
Member
Andrew King
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 82
Rep Power: 17 |
Dear Ahmed,
I believe your solution is correct. You have imposed a uniform fixed velocity at the inlet, and a fixed velocity on the top wall. As the boundary layer develops, the fluid within it slows down, and therefore to maintain mass continuity the fluid in the freestream region must speed up, above the 100m/s you have specified. If you were to increase the height of your domain, then this "error" would be decreased. (also, you will likely observe a velocity gradient between the top surface, and the bulk flow). Regards, Andrew
__________________
Dr Andrew King Fluid Dynamics Research Group Curtin University |
|
August 10, 2009, 10:28 |
|
#7 |
Member
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 17 |
Dear Ahmed and All,
You can find a nice validation case here: http://openfoamwiki.net/index.php/Bl...Flow_Benchmark Hope that helps. Best Regards, Paulo Rocha |
|
February 11, 2010, 20:13 |
|
#8 | |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Quote:
You can find some additional information on the wiki, but unfortunately explained tutorial are not many. 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. |
||
May 11, 2010, 05:50 |
|
#9 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
New case added, LES around a square cylinder from the QNet-Ercoftac database,
Underlying Flow Regime 2-02. http://openfoamwiki.net/index.php/Be...coftac_ufr2-02 |
|
June 22, 2011, 19:59 |
|
#10 |
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 500
Rep Power: 19 |
I've started a similar thread here. http://www.cfd-online.com/Forums/ope...nfoam-v-v.html
A question that came up for me on that thread is what should one expect for the convergence of residual for steady viscous runs for incompressible external aerodynamics. It seems that one should not necessarily expect the pressure equation to converge lower than 1e-6. So my question here is, how far did the residual converge for flat plate example given at the beginning of this thread? It's been a while since this thread was active, but thought I would give it a try. |
|
May 13, 2018, 19:28 |
|
#11 |
Senior Member
Yuehan
Join Date: Nov 2012
Posts: 142
Rep Power: 14 |
Are there more validation cases recently?
Thank you! |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
OpenFoam validation | ranas | OpenFOAM Running, Solving & CFD | 0 | July 7, 2009 06:56 |
OpenFOAM Training in Europe and USA | hjasak | OpenFOAM | 0 | August 8, 2008 06:33 |
Adventure of fisrst openfoam installation on Ubuntu 710 | jussi | OpenFOAM Installation | 0 | April 24, 2008 15:25 |
Second OpenFOAM Workshop in Zagreb Croatia 79Jun2007 | hjasak | OpenFOAM | 5 | June 10, 2007 13:33 |
OpenFOAM Training and Workshop | Hrvoje Jasak | Main CFD Forum | 0 | October 7, 2005 08:14 |