CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

OpenFOAM - Validation of Results

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By Ahmed
  • 1 Post By niklas

Reply
 
LinkBack Thread Tools Display Modes
Old   August 8, 2009, 13:21
Default OpenFOAM - Validation of Results
  #1
Senior Member
 
Ahmed
Join Date: Mar 2009
Location: NY
Posts: 250
Rep Power: 9
Ahmed is on a distinguished road
Being unhappy/disappointed with the results obtained by OpenFOAM after my first tutorial ( The cavity Tutorial ) 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
Attached Images
File Type: jpg Mesh1.jpg (22.5 KB, 145 views)
File Type: jpg Mesh1-inlet.jpg (57.9 KB, 139 views)
File Type: jpg U-magnitude-Inlet.jpg (18.0 KB, 190 views)
File Type: jpg U-magnitude-Outlet.jpg (17.1 KB, 167 views)
Ahmed is offline   Reply With Quote

Old   August 9, 2009, 03:01
Default
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by Ahmed View Post
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.
You just did the same: posted pictures

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 live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   August 9, 2009, 03:38
Default
  #3
Senior Member
 
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 275
Rep Power: 9
henrik is on a distinguished road
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 11:38.
henrik is offline   Reply With Quote

Old   August 9, 2009, 11:00
Default
  #4
Senior Member
 
Ahmed
Join Date: Mar 2009
Location: NY
Posts: 250
Rep Power: 9
Ahmed is on a distinguished road
Quote:
Originally Posted by alberto View Post
You just did the same: posted pictures

Out of joke, the idea of posting validation cases is surely interesting.
That is correct, I posted the code and pictures hoping that readers can repeat the analysis and share their results and comments with the rest of us (Check the above post by Henrik Rusche)
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
immortality likes this.
Ahmed is offline   Reply With Quote

Old   August 9, 2009, 11:03
Default
  #5
Senior Member
 
Ahmed
Join Date: Mar 2009
Location: NY
Posts: 250
Rep Power: 9
Ahmed is on a distinguished road
Quote:
Originally Posted by henrik View Post
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 to get better than this and it completely transparent - down to the last line of code.

Henrik
Henrik
Thanks for the information, I hope to see more validation cases on this forum
Good Luck
Ahmed is offline   Reply With Quote

Old   August 10, 2009, 09:11
Default
  #6
Member
 
Andrew King
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 81
Rep Power: 8
andersking is on a distinguished road
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
andersking is offline   Reply With Quote

Old   August 10, 2009, 09:28
Default
  #7
Member
 
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 8
paulo is on a distinguished road
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
paulo is offline   Reply With Quote

Old   February 11, 2010, 20:13
Default
  #8
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by lbuckley View Post
And if anyone knows of a good site for some fundamental examples, I would greatly appreciate it.
For the basic solvers (compressible/incompressible) the examples in the tutorial folder are relatively easy, even if I am well aware of the time it takes to learn OF ;-)

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 live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   May 11, 2010, 04:50
Default
  #9
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
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
mali likes this.
niklas is offline   Reply With Quote

Old   June 22, 2011, 18:59
Default
  #10
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
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.
Martin Hegedus is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
OpenFoam validation ranas OpenFOAM Running, Solving & CFD 0 July 7, 2009 05:56
OpenFOAM Training in Europe and USA hjasak OpenFOAM 0 August 8, 2008 05:33
Adventure of fisrst openfoam installation on Ubuntu 710 jussi OpenFOAM Installation 0 April 24, 2008 14:25
Second OpenFOAM Workshop in Zagreb Croatia 79Jun2007 hjasak OpenFOAM 5 June 10, 2007 12:33
OpenFOAM Training and Workshop Hrvoje Jasak Main CFD Forum 0 October 7, 2005 07:14


All times are GMT -4. The time now is 00:12.