# Fluent works... OF not?

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

January 9, 2015, 06:01
Fluent works... OF not?
#1
New Member

Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
Hi everybody,
I'm studying Mechanical Engineering at Politecnico di Bari (Italy). I'm writing a thesis analyzing incompressible flow over an airfoil. (turbulence model: k-omega; flow velocity: 20 m/s; nu=10^-4 m^2/s; rho= 1 kg/m^3)

I made the mesh with Pointwise. I run it first with Fluent and it worked.

I tried to run the analysis in OpenFOAM so I adapted the "motorbike" tutorial to my case. But it doesn't work.

Quote:
 Create time Create mesh for time = 0 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting RAS turbulence model kOmegaSST kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; gamma1 0.5532; gamma2 0.4403; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; c1 10; } No field sources present SIMPLE: no convergence criteria found. Calculations will run for 500 steps. Starting time loop Time = 1 #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 at smoothSolver.C:0 #4 Foam::smoothSolver::solve(Foam::Field&, Foam::Field const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam" #6 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam" #7 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam" #8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #9 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam" Floating point exception (core dumped)
Which is the problem? The smoothSolver? Boundary conditions? Mesh?

 January 9, 2015, 06:06 #2 Senior Member   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,688 Rep Power: 27 Hi, As the solver crashes during the first iteration, it can be mesh, schemes, ICs and BCs. So please post: 1. checkMesh output 2. fvSchemes file 3. 0 folder

January 9, 2015, 07:06
#3
New Member

Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
CheckMesh
Quote:
 /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.0.1-51f1de99a4bc Exec : checkMesh Date : Jan 09 2015 Time : 11:58:32 Host : ime048 PID : 16607 Case : /home/tesisti/Togati/9-1-15/riferimento nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 207080 internal points: 0 faces: 411979 internal faces: 204899 cells: 102813 boundary patches: 4 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 102813 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 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 frontAndBack 205626 207080 ok (non-closed singly connected) inlet 797 1596 ok (non-closed singly connected) outlet 258 518 ok (non-closed singly connected) wall 399 798 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (-8.99996 -10 0) (20.037 10 1) Mesh (non-empty, non-wedge) directions (1 1 0) Mesh (non-empty) directions (1 1 0) All edges aligned with or perpendicular to non-empty directions. Boundary openness (1.52339e-17 4.52257e-18 7.30337e-15) OK. ***High aspect ratio cells found, Max aspect ratio: 91679.8, number of cells 4620 <

fvSchemes
Quote:
 FoamFile { version 2.0; format ascii; class dictionary; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) Gauss linearUpwindV grad(U); div(phi,k) Gauss upwind; div(phi,omega) 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; }
I attached the 0 folder.
Attached Files
 0.zip (3.3 KB, 3 views)

 January 9, 2015, 09:23 #4 Senior Member   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,688 Rep Power: 27 Hi, I was not able to find errors in the settings, my suggestions will be quite generic: 1. Change smoothSolver to PBiCG. Dictionary for the solver you can find in \$FOAM_TUTORIALS/heatTransfer/buoyantBoussinesqPimpleFoam/hotRoom/system/fvSolution. 2. As your mesh has highly non-orthogonal faces, consider using cellMDLimited modifications of schemes for gradients. Examples can be found in \$FOAM_TUTORIALS/incompressible/pisoFoam/les/motorBike/motorBike/system/fvSchemes (though not quite sure it will be there in 2.1.1, I don't have this version installed). 3. Add bounded to divergence schemes. Example can be found in \$FOAM_TUTORIALS/incompressible/simpleFoam/pitzDailyExptInlet/system/fvSchemes.

 January 9, 2015, 18:46 #5 Senior Member   anonymous Join Date: Aug 2014 Posts: 204 Rep Power: 6 Your does seem to be the problem. Are you sure you changed frontAndBack to empty in the boundary file?

January 10, 2015, 08:12
#6
New Member

Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
@alexeym

1) I changed the solver for U, k, omega from smoothSolver to PBiCG.

2) I used cellMDLimited

Quote:
 gradSchemes { default cellMDLimited Gauss linear 1; }
3) In fvSchemes file of pitzDailyExptInlet tutorial I found this:

Quote:
 divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; }
and when i tried to add "bounded" like this

Quote:
 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))))) bounded Gauss linear; }
or like this

Quote:
 divSchemes { default bounded; }

it gaves me an error:

Quote:
 --> FOAM FATAL IO ERROR: unknown div scheme bounded Valid div schemes are : 1 ( Gauss )

So I tried to run with only modifications 1 and 2.
Results:
Quote:
 Starting time loop Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 6.09293e-05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.000172088, No Iterations 1 #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 Foam::GAMGSolver::scalingFactor(Foam::Field&, Foam::Field const&, Foam::Field const&, Foam::Field const&) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam::GAMGSolver::scalingFactor(Foam::Field&, Foam::lduMatrix const&, Foam::Field&, Foam::FieldField const&, Foam::UPtrList const&, Foam::Field const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 Foam::GAMGSolver::Vcycle(Foam::PtrList const&, Foam::Field&, Foam::Field const&, Foam::Field&, Foam::Field&, Foam::Field&, Foam::PtrList >&, Foam::PtrList >&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #6 Foam::GAMGSolver::solve(Foam::Field&, Foam::Field const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #7 Foam::fvMatrix::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #8 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam" #9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #10 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam" Floating point exception (core dumped)
@ssss
Yes, boundary conditions are ok.

Any more tips? Should be the problem the GAMGSolver (which is the selected solver for p)?

 January 10, 2015, 09:27 #7 Senior Member   anonymous Join Date: Aug 2014 Posts: 204 Rep Power: 6 In order to use bounded in the fvSchemes you need Openfoam2.2.0 or greater, you are using of2.1.1 Are you sure your boundary conditions are correct? Maybe there is a variable whith initial value of 0 (omega...)?

 January 10, 2015, 09:30 #8 Senior Member   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,688 Rep Power: 27 Hi, Well, guess bounded was not implemented in 2.1.1. According to the output, this time FPE happens in pEqn.H, so you've got two options: 1. Change solver for pressure to PCG. 2. Increase number of cell in coarsest level for GAMG solver (nCellsInCoarsestLevel). In general I set this value to nCellsInMesh^(1/3) (for 2D case it could be nCellsInMesh^(1/2), so for ~100,000 cells in your mesh the value should be around 320) Also I've noticed this line in the output: Code: SIMPLE: no convergence criteria found. Calculations will run for 500 steps. I think you should add residualControl to the SIMPLE dictionary in fvSolution file. You can find example in \$FOAM_TUTORIALS/incompressible/simpleFoam/pitzDaily/system/fvSolution. Though in general final residuals should be around 1e-6 (in the example 1e-2/1e-3 were used).

January 10, 2015, 12:14
#9
New Member

Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4

@ssss
omega value is 1.78 everywhere. I uploaded the 0 folder in a precedent post so you can check it.

I increased the number of cell in coarsest level

Quote:
 p { solver GAMG; tolerance 1e-7; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 320; mergeLevels 1; }
but i had the same error.

So I changed the GAMG solver
Quote:
 p { solver PCG; preconditioner DIC; tolerance 1e-6; relTol 0; }
It run. I set endTime=500 in order to monitorate the situation. When I tried to open the results in paraView i had a problem:

Quote:
 created temporary '17-cfd.OpenFOAM' Segmentation fault (core dumped)
So I couldn't visualize the results.

Looking to last outputs I think that something went wrong

Quote:
 Time = 499 DILUPBiCG: Solving for Ux, Initial residual = 0.0176025, Final residual = 8.92661e-06, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.022828, Final residual = 8.31351e-06, No Iterations 1 DICPCG: Solving for p, Initial residual = 3.92221e-07, Final residual = 3.92221e-07, No Iterations 0 time step continuity errors : sum local = 2.19464e+34, global = 9.28582e+31, cumulative = 9.09985e+32 DILUPBiCG: Solving for omega, Initial residual = 0.119754, Final residual = 2.62773e-05, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.160839, Final residual = 5.17799e-05, No Iterations 1 ExecutionTime = 851.27 s ClockTime = 854 s forceCoeffs output: Cd = -3.43866e+69 Cl = -3.51752e+53 Cm = -1.71933e+69 Cl(f) = 1.71933e+69 Cl(r) = -1.71933e+69 Time = 500 DILUPBiCG: Solving for Ux, Initial residual = 0.0153715, Final residual = 7.43431e-06, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.0209576, Final residual = 1.01333e-05, No Iterations 1 DICPCG: Solving for p, Initial residual = 4.0874e-07, Final residual = 4.0874e-07, No Iterations 0 time step continuity errors : sum local = 2.21535e+34, global = 1.02473e+32, cumulative = 1.01246e+33 DILUPBiCG: Solving for omega, Initial residual = 0.112249, Final residual = 9.26829e-06, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.152886, Final residual = 4.04e-05, No Iterations 1 ExecutionTime = 859.41 s ClockTime = 862 s forceCoeffs output: Cd = -3.43851e+69 Cl = -3.51762e+53 Cm = -1.71925e+69 Cl(f) = 1.71925e+69 Cl(r) = -1.71925e+69 End
Force coefficients have impossible values. And what about the time step continuity errors?

Any more tips before updating OF in order to use the bounded divSchemes?

 January 10, 2015, 13:59 #10 Senior Member   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,688 Rep Power: 27 Hi, "relTol 0" in pressure solver is too strict. Let it be 1e-2 or 0.1. Don't know what values of tolerance and relTol you have for velocity. As you can see from residuals, solution is far from convergence. Increase endTime to say 25000. If solution converge earlier, it will just stop at the point of convergence. Don't know the reason for the core dump, though as solution diverges, maybe certain values in result files lead to this behavior. Try using paraview's build-in OpenFOAM reader (paraFoam -builtin).

January 10, 2015, 14:43
#11
New Member

Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
I fixed the fvSolution file

Quote:
 solvers { p { solver PCG; preconditioner DIC; tolerance 1e-6; relTol 0.1; } U { solver PBiCG; preconditioner DILU; tolerance 1e-6; relTol 0.1; } k { solver PBiCG; preconditioner DILU; tolerance 1e-6; relTol 0.1; } omega { solver PBiCG; preconditioner DILU; tolerance 1e-6; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 0; } residualControl { p 1e-6; U 1e-6; k 1e-6; omega 1e-6 } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.3; } equations { U 0.7; k 0.7; omega 0.7; } } cache { grad(U); }
I set endTime to 25000.

Results:

Quote:
 Time = 826 DILUPBiCG: Solving for Ux, Initial residual = 0.459715, Final residual = 0.0100426, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.506025, Final residual = 0.0107321, No Iterations 1 DICPCG: Solving for p, Initial residual = 1.09289e-05, Final residual = 1.25529e-08, No Iterations 1 time step continuity errors : sum local = 4.44341e+58, global = 1.99964e+53, cumulative = 5.47876e+55 DILUPBiCG: Solving for omega, Initial residual = 0.533658, Final residual = 1.7975e-09, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.373316, Final residual = 1.61836e-07, No Iterations 1 ExecutionTime = 1028.32 s ClockTime = 1032 s forceCoeffs output: Cd = -1.33784e+122 Cl = -1.28579e+108 Cm = -6.68919e+121 Cl(f) = 6.68919e+121 Cl(r) = -6.68919e+121 Time = 827 DILUPBiCG: Solving for Ux, Initial residual = 0.507959, Final residual = 0.00769252, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.511595, Final residual = 0.00614268, No Iterations 1 DICPCG: Solving for p, Initial residual = 8.71646e-05, Final residual = 9.2361e-08, No Iterations 1 time step continuity errors : sum local = 4.93263e+58, global = 4.62504e+51, cumulative = 5.47922e+55 DILUPBiCG: Solving for omega, Initial residual = 0.517434, Final residual = 1.72607e-06, No Iterations 1 #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 Foam::PBiCG::solve(Foam::Field&, Foam::Field const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam::fvMatrix::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #5 Foam::fvMatrix::solve() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #6 Foam::incompressible::RASModels::kOmegaSST::correc t() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #7 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam" #8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #9 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam" Floating point exception (core dumped)

 January 10, 2015, 14:56 #12 Senior Member   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,688 Rep Power: 27 Hi, 1. Increase number of non-orthogonal correctors. nNonOrthogonalCorrectors in SIMPLE dictionary. Set it to 3-4. 2. If solution still diverges. Relax more. Set relaxation factor for velocity to 0.3.

January 12, 2015, 10:55
#13
New Member

Angelo Ugenti
Join Date: Dec 2014
Location: Bari
Posts: 8
Rep Power: 4
I set the number of non-orthogonal correctors to 4.

Quote:
 Time = 24999 DILUPBiCG: Solving for Ux, Initial residual = 1.57507e-05, Final residual = 2.77971e-07, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 8.88111e-05, Final residual = 3.18473e-06, No Iterations 2 DICPCG: Solving for p, Initial residual = 0.000894356, Final residual = 8.78172e-05, No Iterations 9 DICPCG: Solving for p, Initial residual = 9.23095e-05, Final residual = 9.02085e-06, No Iterations 94 DICPCG: Solving for p, Initial residual = 9.77823e-06, Final residual = 9.6372e-07, No Iterations 55 DICPCG: Solving for p, Initial residual = 1.04882e-06, Final residual = 6.18521e-07, No Iterations 1 DICPCG: Solving for p, Initial residual = 6.19302e-07, Final residual = 6.19302e-07, No Iterations 0 time step continuity errors : sum local = 4.35178e-08, global = 8.0513e-09, cumulative = 1.09825e-05 DILUPBiCG: Solving for omega, Initial residual = 8.58339e-07, Final residual = 8.58339e-07, No Iterations 0 DILUPBiCG: Solving for k, Initial residual = 1.79678e-05, Final residual = 4.7525e-07, No Iterations 1 ExecutionTime = 9546.81 s ClockTime = 9575 s forceCoeffs output: Cd = 0.0370108 Cl = 5.52511e-19 Cm = 0.0185054 Cl(f) = -0.0185054 Cl(r) = 0.0185054 Time = 25000 DILUPBiCG: Solving for Ux, Initial residual = 1.57509e-05, Final residual = 2.77264e-07, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 8.88113e-05, Final residual = 3.18471e-06, No Iterations 2 DICPCG: Solving for p, Initial residual = 0.000875004, Final residual = 7.37109e-05, No Iterations 10 DICPCG: Solving for p, Initial residual = 9.25738e-05, Final residual = 8.82807e-06, No Iterations 90 DICPCG: Solving for p, Initial residual = 2.34116e-05, Final residual = 2.25928e-06, No Iterations 32 DICPCG: Solving for p, Initial residual = 1.41847e-05, Final residual = 1.23549e-06, No Iterations 2 DICPCG: Solving for p, Initial residual = 1.30288e-05, Final residual = 1.02704e-06, No Iterations 1 time step continuity errors : sum local = 7.21817e-08, global = -8.91159e-09, cumulative = 1.09736e-05 DILUPBiCG: Solving for omega, Initial residual = 8.58635e-07, Final residual = 8.58635e-07, No Iterations 0 DILUPBiCG: Solving for k, Initial residual = 1.79674e-05, Final residual = 4.85255e-07, No Iterations 1 ExecutionTime = 9552.63 s ClockTime = 9581 s forceCoeffs output: Cd = 0.0370012 Cl = 5.52454e-19 Cm = 0.0185006 Cl(f) = -0.0185006 Cl(r) = 0.0185006 End
Why lift coefficient is so small? (Fluent result for Cl was 0.8)

 January 12, 2015, 11:19 #14 Senior Member   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,688 Rep Power: 27 Hi, If you take a look at forceCoeffs.C: Code: // lift, drag and moment coeffs[0] = (totForce & liftDir_)/(Aref_*pDyn); coeffs[1] = (totForce & dragDir_)/(Aref_*pDyn); coeffs[2] = (totMoment & pitchAxis_)/(Aref_*lRef_*pDyn); scalar Cl = sum(coeffs[0]); scalar Cd = sum(coeffs[1]); scalar Cm = sum(coeffs[2]); If your Cd is OK, then, I guess, you've made a mistake in liftDir_ vector.

 January 12, 2015, 11:39 #15 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 20 Angelo please try: Code: p { solver GAMG; tolerance 1e-12; relTol 0.1; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 1; nFinestSweeps 2; scaleCorrection true; directSolveCoarsestLevel false; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 500; mergeLevels 1; maxIter 100; } and for all others: Code: "(U|k|omega)" { solver smoothSolver; preconditioner DILU; smoother DILUGaussSeidel; tolerance 1e-12; relTol 0.1; nSweeps 1; maxIter 100; } and post the log output. __________________ The skeleton ran out of shampoo in the shower.

 January 12, 2015, 11:40 #16 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 20 Also one very clever person in this forum wrote you should never limit the pressure gradient. __________________ The skeleton ran out of shampoo in the shower.

 January 12, 2015, 12:03 #17 Senior Member   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,688 Rep Power: 27 In fact it was here: http://www.openfoam.org/mantisbt/view.php?id=1410#c3246

 January 13, 2015, 02:18 #18 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 20 Right there, henry... very clever. __________________ The skeleton ran out of shampoo in the shower.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post spaceprop FLUENT 5 September 2, 2014 09:43 yuyuxuan FLUENT 0 December 3, 2013 23:56 opehterinar81 FLUENT 0 August 19, 2011 11:55 ibex7 FLUENT 7 April 18, 2011 02:44 Freeman FLUENT 4 April 14, 2006 05:58