
[Sponsors] 
question regarding LES of pipe flow  pimpleFoam 

LinkBack  Thread Tools  Search this Thread  Display Modes 
November 9, 2014, 01:00 
question regarding LES of pipe flow  pimpleFoam

#1 
Member
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 8 
Dear Foamers,
I have started doing an LES of pipe flow using pimpleFoam with cyclic boundary conditions in the streamwise direction to generate turbulent statistics and feed them into a premixed jet flame simulation. Some parameters of the pipe: D = 15mm L = 5*D Ubar = 9.2 m/s Re = 9000 Re_tau = 287 Turbulence model = oneEqEddy delta = vanDriest In the wall normal direction I have resolved the mesh with a y+ = 1. My axial mesh has a resolution of \Deltaz+ = 15. The mesh front view is attached herewith https://www.dropbox.com/s/3ed02j8ojj..._mesh.png?dl=0 Here is my fvOptions file for the pressureGradientExplicitSource Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvOptions; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // momentumSource { type pressureGradientExplicitSource; active on; //on/off switch selectionMode all; //cellSet // points //cellZone pressureGradientExplicitSourceCoeffs { fieldNames (U); Ubar (0 0 9.2); } } Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default CrankNicolson 1; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss linear; div(phi,k) Gauss limitedLinear 1; div(phi,B) Gauss limitedLinear 1; div(B) Gauss linear; // div(phi,nuTilda) Gauss limitedLinear 1; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DBEff,B) Gauss linear corrected; // laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0.05; } pFinal { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0; } "(Uk)" { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } "(Uk)Final" { $U; tolerance 1e05; relTol 0; } } PIMPLE { nOuterCorrectors 2; nCorrectors 2; nNonOrthogonalCorrectors 1; pRefCell 1001; pRefValue 0; } // ************************************************************************* // I ran my code for 0.05 seconds (approximately 5 flow through times without averaging the results) and looked at the Uz (streamwise velocity profile) at the end time using ParaView. The figure is attached herewith. My question is why does the instantaneous velocity have such a smooth laminar like structure? Why cant I see any eddies ?? Would be glad if anyone can help 

November 10, 2014, 03:10 

#2 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Hey Daniel,
1) Please post some of the log output of your run. 2) What is the x+ resolution of your mesh? 3) With y+=1, I guess, you don't use any wall functions?
__________________
The skeleton ran out of shampoo in the shower. 

November 10, 2014, 22:57 

#3 
Member
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 8 
Hi Philipp,
I just realized that the reason I was not getting any turbulence generated was because I wasnt specifying any manually generated turbulence at the inlet (pardon me. really stupid on my part ) I am now trying to generate turbulence using the boxTurb16 utility and then map it to my pipe for initial turbulence. A couple of questions I have are: 1. Why does the box grid in the boxTurb utility have to be in powers of 2^k? 2. In the transportProperties and the turbulenceProperties file are defined variables : Code:
Ea 10; k0 5; UOsigma 0.090295; UOalpha 0.81532; UOKupper 10; UOKlower 7; 

November 11, 2014, 02:52 

#4 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Daniel, you don't need to initialize the turbulence... it should be just much faster to get convergence. I didn't initialize it and get some nice LES of a periodic pipe.
I can recommend to track the kinetic energy in the logoutput. If you plot it over time, you can see, if your simulation is converged. I will post some pictures in a minute.
__________________
The skeleton ran out of shampoo in the shower. 

November 11, 2014, 03:30 

#5 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
This is a picture of a pipe flow just as you do, but with higher Re and wall modeled LES. It was initialized without any turbulence.
U.jpg This is a picture of the kinetic energy (perpendicular to the main flow) to track the convergence of the case. You see, it is not fully converged after 40000 time steps. This means after 1.6s or about 100 flow through times. Of course, this is due to very bad initial guess, but you see, this can take some time. kEn.jpeg I track the energy by putting this in my controlDict: Code:
functions ( AverageResolvedKineticEnergyVxVy { type swakExpression; valueType cellZone; zoneName FLUID; accumulations ( average ); expression "U.x*U.x + U.y*U.y"; verbose true; } );
__________________
The skeleton ran out of shampoo in the shower. 

November 11, 2014, 22:47 

#6 
Member
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 8 
Thanks for your post Philipp. I am really curious to know how you achieve turbulence without initializing any at the beginning of the simulation.
What turbulence model do you use and what is the Reynolds number for your flow?? Is the tradeoff with your technique a longer run time? (I ask because the result I posted in my first post was for just 5 flow through times without initializing turbulence and I couldnt observe any turbulent structures in my flowfield ) 

November 12, 2014, 02:35 

#7 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Daniel,
1) Turbulence is produced by the flow. So there is no need for any special initialization to get turbulence at all. The only exception that I know is, when you solve equations for turbulence and the production rate is proportional to some turbulence parameter (such as "k"). If you initialize "k" with zero everywhere, you are doomed, because the production rate will be zero for all time. I was using Smagorinsky model. 2) Two post above (#4) I wrote that it took more than 100 flow through times and it still is not converged. 3) Your problems can have many reasons. You need to answer the questions of post #2 if you want any help to solve them. Maybe the answer is just: "Wait even longer".
__________________
The skeleton ran out of shampoo in the shower. 

November 12, 2014, 22:15 

#8 
Member
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 8 
Hi Philipp,
Refering to your post#2 here is the log output of my run: Code:
Courant Number mean: 0.318167 max: 0.49787 deltaT = 1.04167e05 Time = 0.0999792 PIMPLE: iteration 1 DILUPBiCG: Solving for Ux, Initial residual = 0.0160958, Final residual = 0.000505205, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.0150424, Final residual = 0.000417883, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1.10966e05, Final residual = 1.06779e07, No Iterations 1 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9431 DICPCG: Solving for p, Initial residual = 0.362879, Final residual = 0.0159966, No Iterations 16 DICPCG: Solving for p, Initial residual = 0.016784, Final residual = 0.000816065, No Iterations 104 time step continuity errors : sum local = 9.65187e11, global = 1.35337e11, cumulative = 1.9175e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9424 DICPCG: Solving for p, Initial residual = 0.0733988, Final residual = 0.00325182, No Iterations 6 DICPCG: Solving for p, Initial residual = 0.00358734, Final residual = 0.000172535, No Iterations 223 time step continuity errors : sum local = 2.8346e11, global = 1.35337e11, cumulative = 1.91614e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9424 PIMPLE: iteration 2 DILUPBiCG: Solving for Ux, Initial residual = 0.000610097, Final residual = 4.07385e06, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.000570686, Final residual = 3.67736e06, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 3.10073e09, Final residual = 3.10073e09, No Iterations 0 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9424 DICPCG: Solving for p, Initial residual = 0.00980145, Final residual = 0.000418088, No Iterations 4 DICPCG: Solving for p, Initial residual = 0.000437694, Final residual = 2.17607e05, No Iterations 245 time step continuity errors : sum local = 1.53838e11, global = 1.35337e11, cumulative = 1.91479e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9425 DICPCG: Solving for p, Initial residual = 0.00173541, Final residual = 8.43401e05, No Iterations 3 DICPCG: Solving for p, Initial residual = 8.7379e05, Final residual = 9.85646e07, No Iterations 271 time step continuity errors : sum local = 1.36178e11, global = 1.35337e11, cumulative = 1.91344e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9425 DILUPBiCG: Solving for k, Initial residual = 2.96381e05, Final residual = 3.65235e07, No Iterations 1 bounding k, min: 0 max: 0.122827 average: 0.0593156 ExecutionTime = 8980.11 s ClockTime = 9035 s Courant Number mean: 0.318167 max: 0.497882 deltaT = 1.04167e05 Time = 0.0999896 PIMPLE: iteration 1 DILUPBiCG: Solving for Ux, Initial residual = 0.015843, Final residual = 0.000523452, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.0143468, Final residual = 0.000436435, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1.10947e05, Final residual = 1.06753e07, No Iterations 1 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9421 DICPCG: Solving for p, Initial residual = 0.340204, Final residual = 0.0165366, No Iterations 16 DICPCG: Solving for p, Initial residual = 0.0178719, Final residual = 0.000870718, No Iterations 226 time step continuity errors : sum local = 8.40756e11, global = 7.37073e12, cumulative = 1.91417e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9416 DICPCG: Solving for p, Initial residual = 0.0748232, Final residual = 0.00314183, No Iterations 7 DICPCG: Solving for p, Initial residual = 0.00334815, Final residual = 0.000161511, No Iterations 89 time step continuity errors : sum local = 2.30996e11, global = 7.37072e12, cumulative = 1.91491e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9416 PIMPLE: iteration 2 DILUPBiCG: Solving for Ux, Initial residual = 0.000584867, Final residual = 4.24894e06, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.000545387, Final residual = 3.90244e06, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 3.04409e09, Final residual = 3.04409e09, No Iterations 0 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9416 DICPCG: Solving for p, Initial residual = 0.00976526, Final residual = 0.000399203, No Iterations 4 DICPCG: Solving for p, Initial residual = 0.000416475, Final residual = 2.03138e05, No Iterations 242 time step continuity errors : sum local = 9.11331e12, global = 7.37073e12, cumulative = 1.91565e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9416 DICPCG: Solving for p, Initial residual = 0.00170644, Final residual = 8.18023e05, No Iterations 3 DICPCG: Solving for p, Initial residual = 8.49119e05, Final residual = 9.48026e07, No Iterations 312 time step continuity errors : sum local = 7.45187e12, global = 7.37073e12, cumulative = 1.91638e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9416 DILUPBiCG: Solving for k, Initial residual = 2.96352e05, Final residual = 3.65196e07, No Iterations 1 bounding k, min: 0 max: 0.122824 average: 0.0593149 ExecutionTime = 8981.2 s ClockTime = 9036 s Courant Number mean: 0.318167 max: 0.497894 deltaT = 1.04167e05 Time = 0.1 PIMPLE: iteration 1 DILUPBiCG: Solving for Ux, Initial residual = 0.0170933, Final residual = 0.000506882, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.0157762, Final residual = 0.000423149, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1.10933e05, Final residual = 1.06765e07, No Iterations 1 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9414 DICPCG: Solving for p, Initial residual = 0.362403, Final residual = 0.0157429, No Iterations 16 DICPCG: Solving for p, Initial residual = 0.0165154, Final residual = 0.000787541, No Iterations 230 time step continuity errors : sum local = 8.10639e11, global = 6.68959e12, cumulative = 1.91705e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9408 DICPCG: Solving for p, Initial residual = 0.0734679, Final residual = 0.00324997, No Iterations 6 DICPCG: Solving for p, Initial residual = 0.00359747, Final residual = 0.000178054, No Iterations 238 time step continuity errors : sum local = 2.2006e11, global = 6.68959e12, cumulative = 1.91772e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9408 PIMPLE: iteration 2 DILUPBiCG: Solving for Ux, Initial residual = 0.000607425, Final residual = 4.14948e06, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.00057021, Final residual = 3.84362e06, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 3.0812e09, Final residual = 3.0812e09, No Iterations 0 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9408 DICPCG: Solving for p, Initial residual = 0.00974758, Final residual = 0.00039325, No Iterations 4 DICPCG: Solving for p, Initial residual = 0.000411935, Final residual = 1.98099e05, No Iterations 111 time step continuity errors : sum local = 8.16657e12, global = 6.68959e12, cumulative = 1.91839e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9408 DICPCG: Solving for p, Initial residual = 0.00173266, Final residual = 7.96663e05, No Iterations 3 DICPCG: Solving for p, Initial residual = 8.25938e05, Final residual = 9.99876e07, No Iterations 308 time step continuity errors : sum local = 6.77497e12, global = 6.68959e12, cumulative = 1.91906e08 Pressure gradient source: uncorrected Ubar = 9.2, pressure gradient = 33.9408 DILUPBiCG: Solving for k, Initial residual = 2.96323e05, Final residual = 3.65171e07, No Iterations 1 bounding k, min: 0 max: 0.122821 average: 0.0593141 ExecutionTime = 8982.74 s ClockTime = 9038 s End 3. My minimum y+ resolved at the wall is 1. I am not using any wall functions. In fact I had made a mistake of assigning k to 0 using oneEqEdy model so that there wont be any production of turbulence. But later I changed the turbulence model to Smagorinsky that does not use a an k equation but is calculated. Here is the boundary condition file for k Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ 0 2 2 0 0 0 0 ]; internalField uniform 0; boundaryField { Side { type fixedValue; value uniform 0; } Inlet { type cyclic; } Outlet { type cyclic; } } // ************************************************************************* // 

November 13, 2014, 02:38 

#9  
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Quote:
Code:
volScalarField G(GName(), 2.0*nuSgs_*magSqr(symm(gradU))); When I started my case with Smagorinsky, I had an internal nuSgs field of "0" everywhere. That worked! Remember if you compare the pictures: I had a Reynolds number of 820000. Not 9000. You can also have a look at nuSgs in paraview, just as you plot the velocity. If there is anything to plot, the model started to work. You need to change your solver settings. Firstly change pressure solver, the one you use currently takes too many iterations. Code:
p { solver GAMG; tolerance 1e6; relTol 0.1; maxIter 100; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 1; nFinestSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 50; agglomerator faceAreaPair; mergeLevels 1; }; pFinal { solver GAMG; tolerance 1e6; relTol 1.0e2; maxIter 100; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 1; nFinestSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 50; agglomerator faceAreaPair; mergeLevels 1; }; Then, put the code I posted in your controlDict to track the turbulent energy. You can create a plotscript like this: Code:
set title "Kinetic Energy  Pipe LES" set ylabel 'Kinetic Energy' set xlabel 'time step' set key off set grid plot "< cat log  grep 'Expression AverageResolvedKineticEnergyVxVy :'  cut d'=' f2" title 'kEn' with dots Edit: One last thing: If you want to see turbulent structures in the picture, it is much better to plot a velocity that is perpendicular to the main flow. Because it's average is zero and you can see small structures much easier.
__________________
The skeleton ran out of shampoo in the shower. 

November 14, 2014, 01:42 

#10 
Member
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 8 
Thanks a ton for your insight and help Philipp. I input your code from post#3 in my controlDict and I got the following error:
Code:
[0] [1] [2] [3] [1] [1] > FOAM FATAL ERROR: [1] Unknown function type swakExpression Btw here is my checkMesh output. The number of nonorthogonal faces were high which is why I have used a nonortho correcter in fvSolution. Even then, please let me know your thoughts on this output (dont want to make a run on a bad mesh). Code:
Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology Inlet 3036 3081 ok (nonclosed singly connected) Outlet 3036 3081 ok (nonclosed singly connected) Side 21912 22000 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0.0075 0.0075 0) (0.0075 0.0075 0.075) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (2.93937e17 3.05889e17 3.25725e16) OK. Max cell openness = 1.0304e15 OK. Max aspect ratio = 21.0616 OK. Minimum face area = 3.01205e09. Maximum face area = 1.64985e07. Face area magnitudes OK. Min volume = 1.7177e12. Max volume = 4.96941e11. Total volume = 1.32423e05. Cell volumes OK. Mesh nonorthogonality Max: 180 average: 6.23511 ***Number of nonorthogonality errors: 6072. <<Writing 6072 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 1.10262 OK. Coupled point location match (average 1.38778e17) OK. Failed 1 mesh checks. End 

November 14, 2014, 01:53 

#11 
Member
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 8 
I tried including the following library files in my control dict:
Code:
libs ( "libOpenFOAM.so" "libsimpleSwakFunctionObjects.so" "libswakFunctionObjects.so" "libgroovyBC.so" ); Code:
[1] From function getCellZoneID(const fvMesh &mesh,const word &name) [1] in file CellZoneValueExpressionDriver.C at line 63. [1] FOAM parallel run exiting [1] [2] [2] [2] > FOAM FATAL ERROR: [2] The cellZone FLUID was not found in 

November 14, 2014, 03:15 

#12  
Senior Member

Hi,
I guess this Code:
functions ( AverageResolvedKineticEnergyVxVy { type swakExpression; valueType cellZone; zoneName FLUID; accumulations ( average ); expression "U.x*U.x + U.y*U.y"; verbose true; } ); Code:
functions ( AverageResolvedKineticEnergyVxVy { type swakExpression; valueType internalField; accumulations ( average ); expression "U.x*U.x + U.y*U.y"; verbose true; } ); About your question Quote:


November 14, 2014, 03:23 

#13 
Member
davide basso
Join Date: Jan 2012
Posts: 48
Rep Power: 10 
Code:
Mesh nonorthogonality Max: 180 average: 6.23511 ***Number of nonorthogonality errors: 6072. <<Writing 6072 nonorthogonal faces to set nonOrthoFaces Try to improve it in order to keep the max orthogonality below 7080 

November 14, 2014, 03:30 

#14 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Yes, indeed. For a simple pipe like you meshed it you should get something like:
Mesh nonorthogonality Max: 39.1121 average: 6.23583 Nonorthogonality check OK.
__________________
The skeleton ran out of shampoo in the shower. 

November 14, 2014, 12:10 

#15  
Member
davide basso
Join Date: Jan 2012
Posts: 48
Rep Power: 10 
Quote:
It seems like you used some OGridbased blocking techinque for your mesh ( is it ICEM by any chance? ): Inside the red circles that's where I suspect your orthogonality goes. Since you want a lot of nodes on the edge of the ogrid, which is good, you probably should "relax" the transition of the mesh along the diagonal by reducing the size of the internal square like the one I drew in pink. Hope this helps! 

November 16, 2014, 22:54 

#16  
Member
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 8 
Quote:
So I tried my case with the Smagorinsky model. I initialized k and nuSgs with nonzero values in the internalField. Following is the BC file for k Code:
internalField uniform 1; boundaryField { Side { type zeroGradient; } Inlet { type cyclic; } Outlet { type cyclic; } } I even tried your script for the kinetic energy. However unlike your case, in mine the KE is of the order of 1e10 throughout the run, which means that that there is no production in the x and y direction. I have attached my figures for k, nuSgs and U below. Dont know where the problem lies Quote:
I even tried a test of running checkMesh for a 16 X 16 X 16 cube with cyclic patches and it gives me the same error of orthogonality. I wonder if there is an issue exporting periodic meshes from Pointwise to OF. I even posted it on the forum http://www.cfdonline.com/Forums/ope...ityerror.html please let me know if you have any information regarding the same. Thanks! 

November 17, 2014, 07:10 

#17 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
As far as I know, mesh orthogonality shows the maximum angle between two cellface and cellcenter lines. Yours shows an angle of 180 degree, which means that something is really fucked up. Not just some regular bad cells.
Ok, you can try this: Export a complete regular mesh from your meshing tool. No special "periodic" boundary conditions. Just name the one side "inlet" and one side "outlet". You can change everything you need for periodic b.c. in the files in openFoam. Your /constant/polyMesh/boundary file should be edited to something like this: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.x   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 3 ( PIPE_INLET { type cyclic; nFaces 21285; startFace 19012158; neighbourPatch PIPE_OUTLET; } PIPE_OUTLET { type cyclic; nFaces 21285; startFace 19033443; neighbourPatch PIPE_INLET; } PIPE_WALL { type wall; nFaces 118404; startFace 19054728; } ) // ************************************************************************* // This works for me (mesh comes from ICEM). Edit: Can you upload the case?
__________________
The skeleton ran out of shampoo in the shower. 

November 17, 2014, 07:28 

#18 
Member
davide basso
Join Date: Jan 2012
Posts: 48
Rep Power: 10 
Dan I'm no expert of Pointwise (I've read your other post) but I definitely agree with Philipp.
I suspect your problem may arise because of the mesh periodicity you defined. For your case you don't need mesh periodicity but only b.c. Periodicity, which you can fully define in OF dictionaries 

November 17, 2014, 23:40 

#19  
Member
Daniel
Join Date: Jun 2014
Posts: 60
Rep Power: 8 
Quote:
I have uploaded my case here. You can have a look. 

November 18, 2014, 03:16 

#20 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Daniel, at least for the oneEquation model: You try to do wall resolved LES, right? I am not an expert for that, but I don't think you can set k to zeroGradient at the walls, you need k=0.
For the Smagorinsky model I am not sure... is nuSgs boundary condition used at all? Anyway, is nuSgs zerogradient correct at lowRe walls?
__________________
The skeleton ran out of shampoo in the shower. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Issues on the simulation of highspeed compressible flow within turbomachinery  dowlee  OpenFOAM Running, Solving & CFD  8  October 25, 2016 19:48 
setup problems  LES pipe flow with cyclic BC (1) and direct mapped inlet (2)  florian_krause  OpenFOAM  22  June 13, 2013 21:25 
Pipe flow with pressureinlet  lummz  FLUENT  3  October 13, 2012 13:29 
Question regarding Fluent's Turbulent Pipe Flow Problem  clueless  Main CFD Forum  0  May 15, 2009 03:59 
Question regarding Fluent's Turbulent Pipe Flow Problem  clueless  FLUENT  0  May 15, 2009 03:33 