
[Sponsors] 
March 1, 2016, 01:15 
simpleFoam convergence issue

#1 
New Member
Harnoor Singh
Join Date: Jan 2016
Posts: 14
Rep Power: 7 
I am new to OpenFoam. I am trying to simulate flow over a 3d wing (sd 6060 airfoil) at Re=80000. I have created my mesh in icemcfd and imported it in Openfoam. I am using k omega SST model and I have specified all boundary conditions to the best of my knowledge. I am using simpleFoam as the solver. The solution does not converge and I am getting completely wrong results. I am pasting my case files below. Can someone please take a look and tell me where the problem is? Any help would be greatly appreciated.
k internalField uniform 2.77e8; boundaryField { near_side { type symmetryPlane; } far_side { type fixedValue; value uniform 2.77e8; } outlet { type fixedValue; value uniform 2.77e8; } inlet { type fixedValue; value uniform 2.77e8; } wing_surface { type kqRWallFunction; value uniform 1e11; } wing_tip { type kqRWallFunction; value uniform 1e11; } } omega internalField uniform 3.28; boundaryField { near_side { type symmetryPlane; } far_side { type fixedValue; value uniform 3.28; } outlet { type fixedValue; value uniform 3.28; } inlet { type fixedValue; value uniform 3.28; } wing_surface { type omegaWallFunction; value uniform 2.688e6; } wing_tip { type omegaWallFunction; value uniform 1.421e3; } } p internalField uniform 86974; boundaryField { inlet { type fixedValue; value uniform 86974; } outlet { type fixedValue; value uniform 86974; } wing_surface { type zeroGradient; } near_side { type symmetryPlane; } far_side { type fixedValue; value uniform 86974; } wing_tip { type zeroGradient; } } U internalField uniform (8.533 0 0); boundaryField { inlet { type fixedValue; value uniform (8.533 0 0); } outlet { type fixedValue; value uniform (8.533 0 0); } wing_surface { type fixedValue; value uniform (0 0 0); } near_side { type symmetryPlane; } far_side { type fixedValue; value uniform (8.533 0 0); } wing_tip { type fixedValue; value uniform (0 0 0); ; } } nut internalField uniform 8.446e9; boundaryField { near_side { type symmetryPlane; } far_side { type calculated; value uniform 8.446e9; } outlet { type calculated; value uniform 8.446e9; } inlet { type calculated; value uniform 8.446e9; } wing_surface { type nutkWallFunction; value uniform 7.73e12; } wing_tip { type nutkWallFunction; value uniform 7.73e12; } } fvSchemes ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) bounded Gauss linearUpwindV grad(U); div(phi,k) bounded Gauss upwind; div(phi,omega) bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } fvSolution solvers { p { solver GAMG; tolerance 1e7; relTol 0.01; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } k { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } omega { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } } SIMPLE { nNonOrthogonalCorrectors 0; } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.2; } equations { U 0.5; k 0.5; omega 0.5; } } cache { grad(U); } controlDict deltaT 0.01; writeControl timeStep; writeInterval 50; Pls tell me where the problem is? 

March 1, 2016, 05:26 

#2 
Senior Member
anonymous
Join Date: Aug 2014
Posts: 205
Rep Power: 9 
Increase NonOrthogonalCorrectors to 1
Change div(phi, U) to upwind Change default gradient scheme to: default cellMDLimited Gauss linear 0.5; Do you think that your mesh has enough quality? Do you have tetrahedral elements on the boundary patches? Which is your expected y+? 

March 5, 2016, 09:17 
3d Wing simulation is simpleFoam

#3 
New Member
Harnoor Singh
Join Date: Jan 2016
Posts: 14
Rep Power: 7 
I have made the changes in non orthogonal correctors, div(U,phi) scheme and default grad scheme. Now, the results are less crazier than last time. But, the solution is still incorrect. The value of Ux sarts becoming increasingly negative after abut 15 seconds. The order of magnitude of U is becoming very large at certain locations near the outlet. Also, while viewing in paraview, I noticed that the errors originate at the outlet boundary and propagate towards the inlet. So, my intuition is that there is a problem in the boundary conditions. Can someone please check the type and value of my BC's.
To answer your previous question, my mesh quality is fine. My expected y+ value is 1.9. I dont know how to check if my patches are surrounded by tetragonal cells. checkMesh yielded that mesh is fine. I have attached an image of my geometry, which can be viewed to get an idea of the location of boundary patches. 

March 5, 2016, 12:47 

#4 
Senior Member
Alex
Join Date: Jan 2014
Posts: 126
Rep Power: 9 
Okay,
just some thoughts you might consider: you are specifying very many conditions for the initial variables. Usually, I define the BCs as follows: U: Inlet: fixedValue Outlet: zeroGradient side walls: slip airfoil fixedValue 0 0 0 p: Inlet: zeroGradient outlet: fixedValue $internalField (value of internal field) side: zeroGradient airfoil: zeroGradient k: Inlet: either fixedValue or turbulentKineticEnergyinlet outlet: zeroGradient side: zeroGradient airfoil: zeroGradient or kqRWallFunction omega: inlet: either fixedValue or turbulentMixingLengthFrequencyInlet outlet: zeroGradient side: zeroGradient airfoil: omegaWallFunction Also, you might want to set the gradSchemes to cellMDLimited Gauss Linear 0.5 That's all I would change for now just to see if it makes something better. You could post 3 steps of your log file or attach the whole file if the problem persists. Sometimes, the behavior of the residuals tell the whole story. Cheers Alex 

March 6, 2016, 09:41 
simpleFoam convergence

#5 
New Member
Harnoor Singh
Join Date: Jan 2016
Posts: 14
Rep Power: 7 
Thanks a ton Alex. It worked like a charm. Just changed the BC's as you suggested.
There was still one slight problem. The pressure wasnt converging completely. After 2 hours, the initial and final residuals were practically constant over time. I stopped the simulation after 3 hours. The pressure results look more or less correct. But, is there something that could be done in this regard? The velocities and other variables have converged without any problem. 

March 6, 2016, 10:26 

#6 
Senior Member
Alex
Join Date: Jan 2014
Posts: 126
Rep Power: 9 
Could you post your current fvSchemes and fvSolution file? Please post it as <Code> for better overview


March 7, 2016, 12:43 
fvsolution

#7 
New Member
Harnoor Singh
Join Date: Jan 2016
Posts: 14
Rep Power: 7 
fvsolution
solvers { p { solver GAMG; tolerance 1e7; relTol 0.01; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } k { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } omega { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } } SIMPLE { nNonOrthogonalCorrectors 1; } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.2; } equations { U 0.5; k 0.5; omega 0.5; } } cache { grad(U); } 

March 7, 2016, 12:44 
fvschemes

#8 
New Member
Harnoor Singh
Join Date: Jan 2016
Posts: 14
Rep Power: 7 
fvschemes
ddtSchemes { default steadyState; } gradSchemes { default cellMDLimited Gauss linear 0.5; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) bounded Gauss upwind; div(phi,k) bounded Gauss upwind; div(phi,omega) bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } 

March 7, 2016, 13:43 

#9 
Senior Member
Alex
Join Date: Jan 2014
Posts: 126
Rep Power: 9 
Okay, again some suggestions. For p, change the solver settings (fvSolution) to tolerance 1e10, nCellsInCoarsestLvl to 120 (speeds up the computation time).
Then, again to the pGAMGsolver, add: maxIter 500; also a good speed boost, and the 500 additional iterations barely help. Also, in the SIMPLE settings, add the line nCorrectors 1 and change the nOrthogonalCorrectors to 3. Then, in fvSchemes, you can change the grad(U) to Gauss Linear and the div(phi,U) term to bounded Gauss linearUpwind grad(U). If none of those suggestions helps you, you can also try setting the laplacian scheme in the fvSchemes to Gauss linear uncorrected or Gauss linear limited 0.5. This should do the job but I wouldn't recommend it until it's necessary. Cheers Alex 

March 11, 2016, 10:32 
simpleFoam convergence

#10 
New Member
Harnoor Singh
Join Date: Jan 2016
Posts: 14
Rep Power: 7 
I tried the changes that you suggested but it didn't make much of a difference.
However, I plotted the coefficient of drag and lift vs time for my simulation. I found out that they are converging beautifully (Plots attached below). All variables except p are completely converging. p gets struck at 1 iteration/time step after 20 seconds and then starts oscillating. Now, I have some questions  1. Since the force coefficients are converging, is it fine to assume that simulation results are correct. Can I neglect the minor issue with p? 2. The values of Coefficient of drag and lift I am getting are 0.025 and 0.123 respectively. The experimental values are 0.018 and 0.121. The coefficient of lift is spot on. But there is a some error in drag coefficient. Can it be attributed to the fact that the experimental free stream turbulence level was 0.5% whereas in the simulation it was 0.001%? How big a deal is this? 3. I cant find out a way to set the free stream turbulence intensity to 0.5% in komega sst model. This is because of the restrictions imposed on the value of nut infinity in komega sst. It must lie between 10^(5) to 10^(2) times nu infinity. nu infinity for our case is 1.6^(5). This restriction puts a bound on the maximum value of TKE and hence on free stream turbulence. Is there any way to solve this problem? 4. After the simulation, I tried to generate the log file by the commands  foamJob simpleFoam foamLog log But, the generated log files only contain the last few timestep data (Around 10 delta t). I have no idea why this is happening. This is the reason that I haven't been able to plot the residuals using gnuplot. Is there anything wrong with my commands? 5. Could the error in the value of drag coefficient be attributed to the fact that I am using a steady state solver? My problem appears to have no transient phenomenon whatsoever. 6. I am trying to simulate flow over a wing on which experiments have already been performed. The paper that I am using only specifies the chord length. It does not specify the wing span. Can I take any arbitrary wing span without effecting the force coefficients? I mean would the end effects (due o wing tips) really have any significant influence on the force coefficients? What is the minimum span that I should keep (In terms of chord length) to avoid errors due to end effects? Thanks in advance. 

March 12, 2016, 13:08 

#11  
Senior Member
Alex
Join Date: Jan 2014
Posts: 126
Rep Power: 9 
Quote:
2. I think the freestream turbulence is a minor issue regarding your simulation results. The problem of OF's kOmegaSST is that it is just in High Re formulation. Can you switch the kwall BC to kLowReWallFunction? Also, if you are including nut in your /0 folder, you can set the wall BC to nutLowReWallFunction. HighRe kOmegaSST tends to overpredict drag even in LowRe meshes. Another possibility would be to use the kkLOmega model as it simulates transitional flow. I found it to be performing well when dealing with a transitional boundary layer (I am not sure if that's the case in your simulation) 3. Read about the turbulentIntensityKineticEnergyInlet BC for 0/k. Maybe this is a way for you to define your turbulence values. Or did I misunderstand the question? 4. I am generating my log file by putting an empty text document named "log" in the case directory and starting the simulation with Code:
simpleFoam >log 5. I am pretty sure that this is not the case. 6. That is actually a tough question since a too short wing produces too much induced drag compared to the regular drag of the middle section of the wing. If you have information about what kind of airplane this wing could be used for you could make a pretty accurate guess by looking at the technical data of the airplane. If there is nothing mentioned I'd look at typical airplane wingspans. Since the lift is also affected by the wing geometry (e.g. washout), you might have already chosen just the right wingspan. What is your yPlus value after the simulation? Code:
yPlus latestTime Cheers Alex 

March 12, 2016, 13:12 

#12 
Senior Member
Alex
Join Date: Jan 2014
Posts: 126
Rep Power: 9 
Oh and for your drag you can also play around with the convection terms:
Code:
div(phi,U) div(p,U) 

March 14, 2016, 01:58 

#13 
New Member
Parth Thakkar
Join Date: Mar 2016
Posts: 7
Rep Power: 6 
Sir, I am working with Harnoor on this project.
1. The pressure residuals are oscillating between values of the order of 1e8 to 1e7. Our number of nOrthogonalCorrectors is 1. 2. We have changed our airfoil, and the values of Cl and Cd at alpha=0 are 0.1 and 0.019 respectively. But, the results we are getting are Cl=0.031 and Cd=0.029. We tried switching the BC's to kLowReWallFunction. There is not much change in the values of our lift and drag coefficients. 3. Sir you misunderstood the question. We are finding difficulty in determining the values of k and omega to be given in initial conditions. Menter's paper in which he proposed the kOmegaSST model, is on this link : https://drive.google.com/open?id=0B3...GEybXNEMXVmY3c Menter has suggested the following values for freestream k and omega in equation (A11) : omegainfinity = e*Uinfinity/L nutinfinity = nuinfinity*d kinfinity = omegainfinity*nutinfinity The values of e and d vary from [1,10] and [1e5,1e2] respectively. I have the following data fixed : Re=235000 c=0.298m Freestream Turbulent Intensity=0.1% How do we choose the values of e,d and L? Also, in equation (A12), what does deltay1 mean? In our simulations, we have chosen the values e=5 and d=1e2. 6. On most of the airfoil, our y+ value is less than 1. Our mesh contains around 800,000 cells. Is it fine enough? Thanks in advance. 

November 16, 2016, 09:23 
C_l and C_d values are incredible high

#14 
New Member
Join Date: Oct 2016
Posts: 22
Rep Power: 6 
Hi all,
I do need help to set up a Simulation of an Airfoil using SimpleFoam and the KOmegaSST model. I created all the files needed and the simulation is running. However the C_l and C_d values are around something 3e88. which definitely makes no sense. Maybe somebody could look through my files and give me some hints what is or could be wrong. I calculated my yPlus which is ~30. CONTROL DICT Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application simpleFoam; startFrom latestTime; //startTime 0; stopAt endTime; endTime 25; deltaT 0.1; writeControl timeStep; writeInterval 10; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; adustTimeStep yes; maxCo 0.9; functions { #include "forceCoeffs" } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // //Tutorial 2D Airfoil solvers { p { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0.1; smoother GaussSeidel; nSweeps 2; } pFinal { $p; relTol 0; } U { solver PBiCG; preconditioner DILU; smoother GaussSeidel; nSweeps 2; tolerance 1e08; relTol 0.1; } nuTilda { solver PBiCG; //preconditioner DIC; smoother GaussSeidel; nSweeps 2; tolerance 1e08; relTol 0.1; } omega { solver PBiCG; preconditioner DILU; smoother GaussSeidel; nSweeps 2; tolerance 1e08; relTol 0.1; } k { solver PBiCG; preconditioner DILU; smoother GaussSeidel; nSweeps 2; tolerance 1e08; relTol 0.1; } } SIMPLE { nCorrectors 2; nNonOrthogonalCorrectors 1; pRefCell 0; pRefValue 0; residualControl { p 1e5; U 1e5; nuTilda 1e5; } } relaxationFactors { fields { p 0.3; } equations { U 0.7; nuTilda 0.7; omega 0.7; } } potentialFlow { nNonOrthogonalCorrectors 15; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default Gauss linear; grad(U) Gauss linear; grad(p) Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,omega) Gauss limitedLinear 1; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(alphaTEff,omega) Gauss linear corrected; laplacian(alphaTEff,kt) Gauss linear corrected; laplacian(nu,kl) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DReff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; laplacian(DomegaEff,omega) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRquired { default no; p ; } wallDist { method meshWave; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object transportProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // transportModel Newtonian; nu [0 2 1 0 0 0 0] 3.087e05; rho [1 3 0 0 0 0 0 ] 1.225; CrossPowerLawCoeffs { nu0 nu0 [ 0 2 1 0 0 0 0 ] 1e06; nuInf nuInf [ 0 2 1 0 0 0 0 ] 1e06; m m [ 0 0 1 0 0 0 0 ] 1; n n [ 0 0 0 0 0 0 0 ] 1; } BirdCarreauCoeffs { nu0 nu0 [ 0 2 1 0 0 0 0 ] 1e06; nuInf nuInf [ 0 2 1 0 0 0 0 ] 1e06; k k [ 0 0 1 0 0 0 0 ] 0; n n [ 0 0 0 0 0 0 0 ] 1; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object turbulenceProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // simulationType RAS; RAS { RASModel kOmegaSST; turbulence on; printCoeffs on; } //kOmegaSSTCoeffs //{ // alphaK1 0.85034; // alphaK2 1.0; // alphaOmega1 0.5; // alphaOmega2 0.85616; // gamma1 0.5532; // gamma2 0.4403; // beta1 0.0750; // beta2 0.0828; // betaStar 0.09; // a1 0.31; // c1 10; //Cmu 0.09; //} //wallFunctionCoeffs //{ // kappa 0.4187; // E 9; //} // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 2 0 0 0 0]; internalField uniform 1; boundaryField { Inlet { type turbulentIntensityKineticEnergyInlet; intensity 0.000002; value uniform 1; } Outlet { type zeroGradient; } Front { type empty;//fixed Value, //value uniform 1e6; } Back { type empty;//fixed Value; // value uniform 1e6; } Wing { type kqRWallFunction; } } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object nut; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 1 0 0 0 0]; internalField uniform 1.54074669e05; boundaryField { Inlet { type fixedValue; value uniform 1.54074669e05; } Outlet { type zeroGradient; } Front { type empty; } Back { type empty; } Wing { type nutkWallFunction; value uniform 1.54074669e05; } } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 1.5   \\ / A nd  Web: http://www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object nuTilda; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 1 0 0 0 0]; internalField uniform 242; boundaryField { Outlet { type zeroGradient; } Inlet { type fixedValue; value uniform 242; } Wing { type fixedValue; value uniform 242; } Front { type empty; } Back { type empty; } } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; object omega; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 1 0 0 0 0]; internalField uniform 30;//5.135822; boundaryField { Inlet { type fixedValue; value uniform 30;//5.135822; } Outlet { type zeroGradient; } Front { type empty; } Back { type empty; } Wing { type omegaWallFunction; value uniform 30;//5.135822; } } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: 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 0; boundaryField { Inlet { type zeroGradient; //freestreamPressure; } Outlet { type fixedValue; value uniform 0; } Front { type empty; } Back { type empty; } Wing { type zeroGradient; } } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 4.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volVectorField; location "0"; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 1 0 0 0 0]; internalField uniform (92.61 0 0); boundaryField { Outlet { type freestream; freestreamValue uniform (92.61 0 0); } //ObenAndUnten //{ // type symmetry; //} Inlet { type freestream; freestreamValue uniform (92.61 0 0); } Wing { type fixedValue; value uniform (0 0 0); } Front { type empty; } Back { type empty; } } // ************************************************************************* // Thanks! 

Tags 
airfoil 3d, k omega sst, simplefoam convergence 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Convergence issue with continuity equation  Jake  FLUENT  8  June 6, 2018 04:41 
convergence issue laplacianFoam  Shakil Masum  OpenFOAM Running, Solving & CFD  1  September 9, 2014 14:03 
Convergence issue for high speed combustion with radiation.  Goutham cet  FLUENT  2  July 30, 2014 08:22 
SimpleFoam convergence problem with really simple simulation  mayank.dce2k7  OpenFOAM Running, Solving & CFD  2  November 19, 2013 06:28 
simpleFoam: simple 1D channel flow, yet very strange convergence behavior  kishpishar  OpenFOAM Running, Solving & CFD  2  June 20, 2013 14:55 