
[Sponsors] 
January 24, 2014, 06:23 
wrong results ...

#21 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
Hello everyone :)
The results of my simulation are not as satisfying as they could be. I compared my cpvalues over the Blade with a simulation performed with fluent and got much bigger results! Furthermore my power coefficient is nearly as high as the Betz coefficient what seems very unrealistic. In a post above it was mentioned that SRFSimpleFoam is not very good for high rpm! Does anyone know some alternatives to SRFSimpleFoam for my simulation of one Blade of the HAWT? What about the DYMFoam solver? Or maybe someone can share some setup files with me, or would like to discuss mine? I īd like to get satisfying results before I start the next step of my BachelorThesis and simulate the whole Turbine with the mast. Thanks in advance for your help Tobias 

January 24, 2014, 06:35 

#22 
Member
Julian Langowski
Join Date: May 2011
Location: Bremen, Germany
Posts: 91
Rep Power: 6 
Hi,
I am working on a rotor blade simulation (MRF approach, 1.5 MW class), too. I have got a simulation running right now, if the results are promising, I am glad to get in contact with you. Bye Julian
__________________
πάντα ῥεῖ  Heraclitus 

January 24, 2014, 07:15 

#23 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
Hi Julian,
do you simulate three blades or just one? Iīd like to test the MRF solver for my case too! At least when I start the big simulation with mast and rotor! Iīm doing the simulation on an experimental Turbine of my University. But the setup for the cases should be the same! Greets Tobias 

January 24, 2014, 07:33 

#24  
Member
Julian Langowski
Join Date: May 2011
Location: Bremen, Germany
Posts: 91
Rep Power: 6 
Quote:
I am simulating 1 blade without nacelle etc., as I already am at 10 Mio. cells and can`t afford more. If you want to simulate the whole HAWT including tower etc. I guess MRF isn`t the right approach, as the blade isn`t really moving, so interaction between blade and tower will not be calculated. Best regards Julian
__________________
πάντα ῥεῖ  Heraclitus 

January 24, 2014, 08:20 

#25 
Senior Member

Hi,
a little bit off topic to those other post, First Symposium on OpenFOAM in Wind Energy http://www.forwind.de/sowe/Site/Program.html 

April 1, 2014, 09:54 
Simulation of horizontalaxiswindturbine

#26 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
Hello dear Elvis
Did you already simulate a Windturbine? I would like to get some tips and tricks ore some guidelines from your experience, or some setup files of simulations you already performed so that I could compare your case with mine. My SRFSimpleFoam and SimpleFoam cases poorely donīt converge and I donīt really know why... I'd be glad for any answer! Best reagards Tobias 

April 1, 2014, 09:57 

#27 
Member
Julian Langowski
Join Date: May 2011
Location: Bremen, Germany
Posts: 91
Rep Power: 6 
Dear Tobias,
how do your residuals (and probe values of U or p) look like over the simulation iterations? As you know, I am working on MRF WT simulation, too. My simulation does not converge perfectly, as well (residuals around 10^4). I am quite sure, it is because of the partly unsteady nature of the flow (separation in root region, ...) which is not considered in SIMPLE. Best regards Julian
__________________
πάντα ῥεῖ  Heraclitus 

April 7, 2014, 07:15 

#28 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
Hey Julian ,
With MRF I got jumping and fluctuating Residuals for omega and k. First it just does not converge, later it crashes because of these parameters... SRF does converge very well, but gives nonphysical results... Did you ever try Pimple with fvoptions? Best regards Tobi 

April 7, 2014, 07:38 

#29 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
Hey Julian :)
With MRF I got jumping and fluctuating Residuals for omega and k. First it just does not converge, later it crashes because of these parameters... SRF does converge very well, but gives nonphysical results... Did you ever try Pimple with fvoptions? Best regards Tobi 

April 7, 2014, 08:24 

#30 
Member
Julian Langowski
Join Date: May 2011
Location: Bremen, Germany
Posts: 91
Rep Power: 6 
Yes,
yes, I did use PIMPLE in PISOmode with fvOptions. However, for SIMPLE I have quite low relaxation factors (0.01) for k and omega. Best regards Julian
__________________
πάντα ῥεῖ  Heraclitus 

April 8, 2014, 03:39 

#31 
Member
Thorsten Grahs
Join Date: Oct 2009
Posts: 48
Rep Power: 8 
Hi Tobias,
a) Use upwind scheme for the turbulent quantaties (the convective terms i.e. div is essential) b) The mesh is essential...chekc y+ like I already mentioned. c) Most ESSENTIAL... right initialisation for the turbulent quantaties, f.i. http://http://www.cfdonline.com/For...nmodel2.html http://support.esicfd.com/esiusers/turb_parameters/ cheers ThG 

May 12, 2014, 05:39 

#32 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
Hello
Actually I got quite good results with a first case that had a very small enclosure. On the next simulation with a bigger enclosure the flow looks good in paraview, but the residuals for p stay very high ~0,06. @ Julian: Did you finish your thesis? Would you mind to share your Pimple/Pisosettings with me? Best regards Tobi Last edited by Tobias Adam; May 12, 2014 at 08:36. 

May 16, 2014, 06:04 

#33 
Member
Julian Langowski
Join Date: May 2011
Location: Bremen, Germany
Posts: 91
Rep Power: 6 
Dear Tobi,
yes, I finished my thesis. Here is my fvSchemes file: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.2   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes // Zeitliche Ableitung { default steadyState; //backward; //alternativ CrankNicholson //steadyState } gradSchemes { default none; grad(p) cellMDLimited Gauss linear 0.5; //cellMDLimited Gauss linear 0.5; grad(U) cellMDLimited Gauss linear 0.5; grad(omega) cellMDLimited Gauss linear 0.5; grad(k) cellMDLimited Gauss linear 0.5; curl(U) cellMDLimited Gauss linear 0.5; } divSchemes { default none; div(phi,U) bounded Gauss linearUpwind grad(U); //bounded Gauss upwind; //bounded Gauss linearUpwind grad(U); div(phi,k) bounded Gauss linearUpwind grad(k); //bounded Gauss upwind; //bounded Gauss linearUpwind grad(k); div(phi,omega) bounded Gauss linearUpwind grad(omega); //bounded Gauss upwind; //bounded Gauss linearUpwind grad(omega); div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default none; laplacian(DomegaEff,k) Gauss linear corrected; laplacian(DomegaEff,omega) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; } interpolationSchemes { default none; //linear bei PIMPLE interpolate(HbyA) linear; interpolate(U) linear; } snGradSchemes { default none; } fluxRequired { default no; p ; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.2   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p { solver GAMG; tolerance 1e7; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; nSweeps 1; tolerance 1e8; relTol 0.1; } k { solver smoothSolver; smoother GaussSeidel; nSweeps 1; tolerance 1e8; relTol 0.1; } omega { solver smoothSolver; smoother GaussSeidel; nSweeps 1; tolerance 1e8; relTol 0.1; } /* pFinal { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0; } "(Ukomega)Final" { $U; tolerance 1e6; relTol 0; }*/ } SIMPLE { nNonOrthogonalCorrectors 5; //8 residualControl { p 1e10; U 1e9; k 1e8; k 1e8; } } relaxationFactors { fields { p 0.3; } equations { U 0.7; k 0.01; omega 0.01; } } /* PIMPLE { nOuterCorrectors 1; nCorrectors 3; nNonOrthogonalCorrectors 3; }*/ // ************************************************************************* // Best regards Julian
__________________
πάντα ῥεῖ  Heraclitus 

June 4, 2014, 07:57 
MRF and Literature

#34 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
Thank you very much Julian,
I allready got this from you earlier, but it helped me a lot for my simulations. A question to everyone: Does anybody have got literature explaining the Mrfprinciple ( like corriolisterm added to NSequations and so on) I want to explain it and compare it with the pympledymfoamsolver. A further question: Does it make sense to use MRF for bladetower interaction as start solution for pympledym or is a steady state solution for a very unsteady too bad? Best Regards Tobi 

June 5, 2014, 09:36 

#35 
New Member
Fatih Ertinaz
Join Date: Feb 2011
Location: Istanbul
Posts: 20
Rep Power: 6 
Hi Tobias,
this document contains brief explanation for the steady and unsteady simulations with rotating regions: http://www.slideshare.net/fumiyanoza...usingopenfoam I guess using converged results of a steadystate solver as an initial condition for the transient case is not a bad idea. If that was what you asked. // Fatih. 

June 24, 2014, 10:01 

#36 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
Hi Fatih,
sorry for my late reply... Thanks for this paper, itīs very helpful. I would have been really happy if I got it at the beginning of my thesis:) Yes, this was what I asked, and itīs definitely a good idea. The pimpleDymsolver is much slower than simple. One question to transient simulations: Is there a general guideline for the maximal possible courant number or is it case dependent at which conumber the case becomes instable? Best regards Tobi P.s. I use SimpleFoam+fv options even for SingleRotatingFrames, because SRFSimple did not give good results for my case. 

June 24, 2014, 18:08 

#37 
New Member
Fatih Ertinaz
Join Date: Feb 2011
Location: Istanbul
Posts: 20
Rep Power: 6 
There is no general rule for determining the max. Courant number as far as I know since it is mesh dependent.
What I would do is to set maxCo as 1 and select a small enough timestep initially and then let OpenFoam adjust it during runTime. You can then try to increase maxCo gradually to figure out what would really be the upperlimit you can use without losing the stability. 

July 24, 2014, 08:57 

#38 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
I found out something new, which might help others.
I tried to map fields from my steady state case to the transient case. It didnīt work, so I just copied the time folder from steadystate and put it to the transient case. I thought it should work, as it has the same mesh. But it didnīt, because the rotatingmeshdict rotates the area of the blade if it does not start with time 0. So the startfield for the transient simulation was useless! To solve the problem, one easily can change the name of the time folder to 0 and delete the uniformfolder inside of this folder. Then the transient simulation starts with the right starting position, with converged results as initial condition. Best Tobi 

August 5, 2014, 10:07 
PimpleDym Simulation

#39 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 4 
They PimpleDymSimulation runs quite good, but the longer the simulation goes the bigger the moment of the blade becomes.
The residuals look very good, the stay low in each time step. I used Co=4 as it seemed to be stable. The only thing bothering me is the Moment increasing more and more. From startvalue ~10Nm to 15Nm over a very long time to ~30Nm now in a very short time... Is it possible that the numerical schemes are wrong, and therefore the moment is calculated wrong? The setting and Boundary conditions are similar to the simple case, I just changed fv schemes and fv solutions .... Best regards Tobi 

September 1, 2014, 06:58 

#40 
Member
Ye Zhang
Join Date: Dec 2009
Location: Delft,Netherland
Posts: 92
Rep Power: 8 
Dear mad,
Could you please send me this paper? I can not download it though the link. Thanks a lot! Best regards Ye 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Wind turbine simulation  Saturn  CFX  45  February 8, 2016 05:42 
Compute the power of small wind turbine.  Luolin  FLUENT  9  May 27, 2013 14:52 
Sliding mesh vs MRF in axial turbine simulation  Vito  FLUENT  3  December 21, 2011 05:57 
Wind turbine domains and boundaries  siardica  CFX  3  July 20, 2009 22:34 
Wind Turbine Modelling  Neil Campbell  Main CFD Forum  1  November 10, 1998 20:03 