
[Sponsors] 
the value of k and Epsilon is constantly increasing 

LinkBack  Thread Tools  Search this Thread  Display Modes 
February 29, 2020, 11:04 
the value of k and Epsilon is constantly increasing

#1 
New Member
Said
Join Date: Feb 2020
Location: Türkiye
Posts: 14
Rep Power: 2 
Hi, i have a kEpsilon case. I created a geometry (like the attachment) and meshed with salome. Then i did import the mesh with "ideasUnvToFoam to a "pitzDaily" file which is the steadystate turbulent simpleFoam solver. I calculated the k and Epsilon values. When i run the case, the value of k and Epsilon is constantly increasing. What should i do, any suggestion?
I used; Salome 9.3. (NETGEN 1D2D3D, 25k nodes) OpenFoam7 Hdraulic diameter= 5e4 Reynolds= 25000 nu= 2e7 controlDict Code:
application simpleFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 200; deltaT 1e4; writeControl adjustableRunTime; writeInterval 1e4; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; functions { #includeFunc streamlines } Code:
dimensions [0 2 3 0 0 0 0]; internalField uniform 1078.1; boundaryField { inlet { type fixedValue; value uniform 1078.1; } outlet { type zeroGradient; } upperWall { type epsilonWallFunction; value uniform 1078.1; } lowerWall { type epsilonWallFunction; value uniform 1078.1; } frontAndBack { type empty; } } Code:
dimensions [0 2 2 0 0 0 0]; internalField uniform 0.375; boundaryField { inlet { type fixedValue; value uniform 0.375; } outlet { type zeroGradient; } upperWall { type kqRWallFunction; value uniform 0.375; } lowerWall { type kqRWallFunction; value uniform 0.375; } frontAndBack { type empty; } } Code:
dimensions [0 1 1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { inlet { type fixedValue; value uniform (10 0 0); } outlet { type zeroGradient; } upperWall { type noSlip; } lowerWall { type noSlip; } frontAndBack { type empty; } } Code:
dimensions [0 2 2 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } upperWall { type zeroGradient; } lowerWall { type zeroGradient; } frontAndBack { type empty; } } Code:
/**\ =========  \\ / F ield  OpenFOAM: The Open Source CFD Toolbox \\ / O peration  Website: https://openfoam.org \\ / A nd  Version: 7 \\/ M anipulation  \**/ Build : 71ff648926f77 Exec : simpleFoam Date : Feb 29 2020 Time : 17:34:15 Host : "said" PID : 20416 I/O : uncollated Case : /home/said/OpenFOAM/openfoam7/tutorials/denemeler/pitzDeneme1 nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 SIMPLE: Convergence criteria found p: tolerance 0.01 U: tolerance 0.001 "(kepsilonomegafv2)": tolerance 0.001 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting turbulence model type RAS Selecting RAS turbulence model kEpsilon RAS { RASModel kEpsilon; turbulence on; printCoeffs on; Cmu 0.09; C1 1.44; C2 1.92; C3 0; sigmak 1; sigmaEps 1.3; } No MRF models present No finite volume options present Starting time loop streamLine streamlines: automatic track length specified through number of sub cycles : 5 Time = 0.0001 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0350657, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0327314, No Iterations 1 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0728737, No Iterations 8 time step continuity errors : sum local = 0.000345373, global = 1.05665e05, cumulative = 1.05665e05 smoothSolver: Solving for epsilon, Initial residual = 0.999999, Final residual = 0.0693174, No Iterations 5 bounding epsilon, min: 3.3678e+08 max: 1.2544e+10 average: 7.12552e+08 smoothSolver: Solving for k, Initial residual = 1, Final residual = 7.96532e07, No Iterations 1 bounding k, min: 24.3664 max: 702.772 average: 0.386658 ExecutionTime = 34.84 s ClockTime = 35 s streamLine streamlines write: seeded 0 particles Tracks:0 Total samples:0 Time = 0.0002 smoothSolver: Solving for Ux, Initial residual = 0.784733, Final residual = 0.0692963, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 0.815212, Final residual = 0.0663261, No Iterations 1 GAMG: Solving for p, Initial residual = 0.982169, Final residual = 0.088101, No Iterations 1 time step continuity errors : sum local = 2.74335, global = 0.000341709, cumulative = 0.000331142 smoothSolver: Solving for epsilon, Initial residual = 0.0125579, Final residual = 0.000768383, No Iterations 1 bounding epsilon, min: 1.67538e+07 max: 3.7362e+09 average: 3.5674e+07 smoothSolver: Solving for k, Initial residual = 0.748306, Final residual = 0.0705025, No Iterations 20 bounding k, min: 12361.6 max: 88308.7 average: 0.682547 ExecutionTime = 54.37 s ClockTime = 55 s streamLine streamlines write: seeded 0 particles Tracks:0 Total samples:0 Time = 0.0003 smoothSolver: Solving for Ux, Initial residual = 0.809226, Final residual = 0.0099766, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 0.731181, Final residual = 0.0124558, No Iterations 1 GAMG: Solving for p, Initial residual = 0.031464, Final residual = 0.00108104, No Iterations 2 time step continuity errors : sum local = 8.80402e+11, global = 4.86576e+08, cumulative = 4.86576e+08 smoothSolver: Solving for epsilon, Initial residual = 1, Final residual = 0.0887976, No Iterations 3 bounding epsilon, min: 7.93897e+22 max: 6.5463e+23 average: 2.40067e+19 smoothSolver: Solving for k, Initial residual = 0.999996, Final residual = 0.0472814, No Iterations 2 bounding k, min: 3.61155e+17 max: 2.11732e+18 average: 1.10185e+14 ExecutionTime = 70.58 s ClockTime = 71 s streamLine streamlines write: seeded 0 particles Tracks:0 Total samples:0 Time = 0.0004 smoothSolver: Solving for Ux, Initial residual = 0.830135, Final residual = 0.0220289, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.839851, Final residual = 0.0284726, No Iterations 2 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0870518, No Iterations 4 time step continuity errors : sum local = 6.79143e+35, global = 1.49171e+34, cumulative = 1.49171e+34 smoothSolver: Solving for epsilon, Initial residual = 1, Final residual = 0.0892089, No Iterations 2 bounding epsilon, min: 6.69723e+81 max: 1.97989e+98 average: 4.39393e+92 smoothSolver: Solving for k, Initial residual = 1, Final residual = 1.35535e13, No Iterations 1 bounding k, min: 4.75429e+59 max: 2.35257e+60 average: 6.087e+54 ExecutionTime = 88.71 s ClockTime = 89 s streamLine streamlines write: seeded 0 particles Tracks:0 Total samples:0 Time = 0.0005 smoothSolver: Solving for Ux, Initial residual = 0.99729, Final residual = 0.0409, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 0.997922, Final residual = 0.0452263, No Iterations 2 #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const at ??:? #4 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const at ??:? #5 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:? #6 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:? #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam7/platforms/linux64GccDPInt32Opt/bin/simpleFoam" #8 Foam::fvMatrix<double>::solve() in "/opt/openfoam7/platforms/linux64GccDPInt32Opt/bin/simpleFoam" #9 ? in "/opt/openfoam7/platforms/linux64GccDPInt32Opt/bin/simpleFoam" #10 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #11 ? in "/opt/openfoam7/platforms/linux64GccDPInt32Opt/bin/simpleFoam" 

February 29, 2020, 17:52 

#2 
Member
Andrew O. Winter
Join Date: Aug 2015
Location: Seattle, WA, USA
Posts: 77
Rep Power: 7 
Hi Said,
Looking at your values for and , it seems like they might be a bit off. Taking , , , and , where , you get , , , based on the Wikipedia TKE webpage. However, these relatively small differences are probably not what's causing your simulation to diverge. I would try one or both of two things: 1) reduce the relaxation parameters in the fvSolution file for your case, 2) gradually increase the velocity/turbulence instead of starting from rest and immediately trying to jump to extremely high values for a very turbulent flow condition. The best way to do this is probably to ramp up the velocity using the timeVaryingMappedFixedValue boundary condition for your inlet boundary velocity. Reading the header text at the beginning of the source code header file (see https://github.com/OpenFOAM/OpenFOAM...FvPatchField.H) helps to explain what the setup for this BC is like and searching through the forums you'll find references to it as well. Also, have you used the checkMesh utility to check if there are any poorquality cells in your mesh? If not, I would do this first to verify that there are not any severely nonorthogonal or skewed cells. Last edited by aow; February 29, 2020 at 23:04. 

March 1, 2020, 09:22 

#3 
New Member
Said
Join Date: Feb 2020
Location: Türkiye
Posts: 14
Rep Power: 2 
Dear aow,
Thanks for your reply. I did what you said but there is nothing change. And also i change my geometry, mesh, deltaT, Reynolds number but the results still same, k and epsilon is constantly increasing. I did try a lot of things but my case still doesn't working. Any suggestion, what should i do? 

March 1, 2020, 19:21 

#4 
Member
Andrew O. Winter
Join Date: Aug 2015
Location: Seattle, WA, USA
Posts: 77
Rep Power: 7 
Sorry that didn't help at all. Did you use blockMesh and snappyHexMesh or are you importing the mesh entirely from Salome? I've never used Salome so I'm not familiar with what sort of results it produces. Anyway, if you did use blockMesh/snappyHexMesh, could you post your dictionary files for them?
Also, have you tried playing around with the time step? Maybe 1e4 is initially too large. You could try starting with 1e5 and 1e6 instead to see if there is any improvement. Your tolerances for p, U, k, etc... might be a bit large too so maybe try reducing them a bit as well. If you could show your fvSolution and fvSchemes files that might help identify the problem too. 

March 2, 2020, 01:32 

#5  
New Member
Said
Join Date: Feb 2020
Location: Türkiye
Posts: 14
Rep Power: 2 
Quote:
Thanks again. I did import the mesh with salome, I didn't use blockMesh or snappyHexMesh. Do you think this could be a problem? And I tried playing around with deltaT but it diverging same time (like 0.001 sec). Here my other case files: fvSolution Code:
solvers { p { solver GAMG; tolerance 1e6; relTol 1e3; //0.1 smoother GaussSeidel; } "(Ukepsilonomegafv2)" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e6; relTol 1e3; //0.1 } } SIMPLE { nNonOrthogonalCorrectors 0; consistent yes; residualControl { p 1e2; U 1e3; "(kepsilonomegafv2)" 1e3; } } relaxationFactors { equations { U 0.8; // 0.9 is more stable but 0.95 more convergent ".*" 0.8; // 0.9 is more stable but 0.95 more convergent } } Code:
ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) bounded Gauss linearUpwind grad(U); div(phi,k) bounded Gauss limitedLinear 1; div(phi,epsilon) bounded Gauss limitedLinear 1; div(phi,omega) bounded Gauss limitedLinear 1; div(phi,v2) bounded Gauss limitedLinear 1; div((nuEff*dev2(T(grad(U))))) Gauss linear; div(nonlinearStress) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } wallDist { method meshWave; } 

April 23, 2020, 23:18 

#6 
Member
Andrew O. Winter
Join Date: Aug 2015
Location: Seattle, WA, USA
Posts: 77
Rep Power: 7 
Hi Saidc,
Sorry for the slow reply... I've been busy with work and have not paid attention to CFD Online lately. Hmm, well there doesn't seem to be anything obviously wrong with your solution and schemes files to me. What's a bit weird to me is that you only have solution options specified for p and "(Ukepsilonomegafv2)", but I'm not used to running steady state solutions in OpenFOAM and after examining some of the steady state tutorials it looks like you're not doing anything necessarily wrong there. Another thing that I noticed is that it seems like your residual control values are rather large at 1e2 and 1e3. It looks like you copied the pitzDaily tutorial based on comparing the scripts you've posted to the tutorial files. Perhaps reduce the residual control values and try again to force the simulation to go through more iterations and reach a more converged state. For example, the incompressible/simpleFoam/airFoil2D tutorial uses 1e5 as the residual control value for all field variables being solved for in the simulation. Also, have you tried recording and plotting solution residuals for the variables being solved for in your simulation? You should verify they're actually converging to a steady value in each time step if it's an unsteady model, or, that it reaches a single converged value in a steady state model. Otherwise, if your solution and schemes setup are okay and so are your initial/boundary conditions, then the problem most likely lies with your mesh. Is it possible for you to post an image of it or at least of the domain? I'm wondering if you have too coarse of a mesh somewhere or high skew and/or nonorthogonality of some cells. As I mentioned before, you can check this using the checkMesh utility; however, even if all checks pass this is not a foolproof approach of checking your mesh. You may need to refine it in regions of your model, especially where large gradients in pressure, velocity, etc... are expected to occur, but be careful how you do this. If you use snappyHexMesh, it will refine very abruptly with large jumps in cell size. It is better to use uniform grading like blockMesh can do. If you're using Salome, you may need to figure out a way to do this to get smooth cell size variation when refining the mesh. 

April 23, 2020, 23:35 

#7 
Member
Andrew O. Winter
Join Date: Aug 2015
Location: Seattle, WA, USA
Posts: 77
Rep Power: 7 
One more thing I thought I should mention is that your k and epsilon values have already hit "bounding" values on your first solver iteration at time = 0.0001 s, which tells me something is fundamentally wrong with your initial setup. Maybe your outlet boundary conditions for k and epsilon are causing part of this problem? Perhaps you should try changing them to the following example, which should handle backflow better than the zeroGradient BC if that is happening in your simulation. The other BCs for k and epsilon look okay to me, it's just that your initial values are very large compared to what I've seen doing water wave impact simulations and it might be part of the problem. I would verify that they are indeed the values you should be using once more to be sure.
Code:
outlet { type inletOutlet; inletValue $internalField; value $internalField; } 

Tags 
keplison, openfaom7, simple foam, turbulent 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
SimpleFoam k and epsilon bounded  nedved  OpenFOAM Running, Solving & CFD  16  March 4, 2017 09:30 
simpleFoam error  "Floating point exception"  mbcx4jc2  OpenFOAM Running, Solving & CFD  12  August 4, 2015 03:20 
Calculation of k and epsilon freezes  Nigirim  OpenFOAM Running, Solving & CFD  1  November 14, 2012 08:52 
epsilon and K blowing up.  sivakumar  OpenFOAM Running, Solving & CFD  1  October 25, 2012 05:50 
SimpleFoam k and epsilon bounded  nedved  OpenFOAM Running, Solving & CFD  1  November 25, 2008 21:21 