
[Sponsors] 
May 29, 2012, 12:54 
Convergence problem.

#1 
New Member
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 7 
Hi
Iīm using the SimpleFoam and buoyantBoussinesqSimpleFoam.at the moment, I donīt consider the turbulence: RASModel laminar; turbulence off; I think that the BC are well defined, so I donīt really understand why i have such a problem in steady case. It could be nice if someone can take a look, maybe you notice where is my mistake(s). fvSolution Code:
solvers { p { solver PCG; tolerance 1e09; relTol 0.0001; maxIter 4000; preconditioner DIC; } "(UTkepsilonR)" { solver PBiCG; preconditioner DILU; tolerance 1e09; relTol 0.0001; maxIter 3000; } } SIMPLE { nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; residualControl { p 1e6; U 1e6; T 1e6; // possibly check turbulence fields "(kepsilonomega)" 1e3; } } relaxationFactors { fields { p 0.8; } equations { U 0.8; T 0.8; "(kepsilonR)" 0.8; } } fvSchemes Code:
ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,T) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p_rgh) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(kappaEff,T) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } Code:
Selecting incompressible transport model Newtonian Selecting RAS turbulence model laminar SIMPLE: convergence criteria field p tolerance 1e06 field U tolerance 1e06 field T tolerance 1e06 field "(kepsilonomega)" tolerance 0.001 Starting time loop Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 9.91822e05, No Iterations 96 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 9.59855e05, No Iterations 56 DILUPBiCG: Solving for Uz, Initial residual = 1.75444e06, Final residual = 9.82385e10, No Iterations 43 DICPCG: Solving for p, Initial residual = 1, Final residual = 9.80756e05, No Iterations 2918 time step continuity errors : sum local = 8.99111e06, global = 1.25301e08, cumulative = 1.25301e08 ExecutionTime = 306.68 s ClockTime = 307 s Time = 2 DILUPBiCG: Solving for Ux, Initial residual = 0.935871, Final residual = 9.05429e05, No Iterations 1863 DILUPBiCG: Solving for Uy, Initial residual = 0.908349, Final residual = 32.7383, No Iterations 3001 DILUPBiCG: Solving for Uz, Initial residual = 0.522177, Final residual = 0.0819383, No Iterations 3001 DICPCG: Solving for p, Initial residual = 0.999559, Final residual = 9.96217e05, No Iterations 3080 time step continuity errors : sum local = 0.0493776, global = 3.04871e06, cumulative = 3.06124e06 ExecutionTime = 2206.47 s ClockTime = 2209 s Time = 3 DILUPBiCG: Solving for Ux, Initial residual = 0.872234, Final residual = 291.137, No Iterations 3001 DILUPBiCG: Solving for Uy, Initial residual = 0.946215, Final residual = 29.1615, No Iterations 3001 DILUPBiCG: Solving for Uz, Initial residual = 0.981871, Final residual = 0.0162036, No Iterations 3001 DICPCG: Solving for p, Initial residual = 0.999723, Final residual = 9.94861e05, No Iterations 3442 time step continuity errors : sum local = 68.092, global = 0.0055498, cumulative = 0.00555286 ExecutionTime = 3928.84 s ClockTime = 3932 s Time = 4 DILUPBiCG: Solving for Ux, Initial residual = 0.999816, Final residual = 0.0411844, No Iterations 3001 DILUPBiCG: Solving for Uy, Initial residual = 0.999753, Final residual = 0.0675664, No Iterations 3001 DILUPBiCG: Solving for Uz, Initial residual = 0.999209, Final residual = 0.0191083, No Iterations 3001 DICPCG: Solving for p, Initial residual = 0.957101, Final residual = 0.000626641, No Iterations 4001 time step continuity errors : sum local = 70089.2, global = 0.784526, cumulative = 0.790079 ExecutionTime = 5648.58 s ClockTime = 5652 s Time = 5 DILUPBiCG: Solving for Ux, Initial residual = 0.998547, Final residual = 656.787, No Iterations 3001 DILUPBiCG: Solving for Uy, Initial residual = 0.998022, Final residual = 59.1156, No Iterations 3001 Iīve been reading in the forum, and a lot of people recommend to use the GAMG preconditioner in order to calculate p, any suggestion? increase the number of iterations and the relaxation factors? . If you think that is necessary i could also show my BC files, I donīt do it know to avoid an excess of information. Thanks a lot, Carles 

May 30, 2012, 03:07 

#2 
Senior Member

Dear CRT,
I would change your relaxation factors to the settings below: The settings you have seem a bit too hard for the solver. If it does not run then, maybe there is some other problem. Cheers, Tom relaxationFactors { fields { p 0.3; } equations { U 0.7; T 0.5; "(kepsilonR)" 0.8; } } 

May 31, 2012, 05:15 

#3  
New Member
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 7 
Dear Tompf,
Thanks for your replay. I've changed the relaxation factors and it doesn't seem to change a lot. What it seems to work is to use the GAMG solver for the pressure, and also whit some nonorthogonal correctors (5). Then the divergence problem appear just in the Ux, Uy, Uz and the time continuity error, but probably the last is a consequence of the velocity divergence, or? Code:
Time = 18 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.000990552, No Iterations 37 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.000665076, No Iterations 181 DILUPBiCG: Solving for Uz, Initial residual = 0.993859, Final residual = 5.52181e+08, No Iterations 6001 GAMG: Solving for p, Initial residual = 1, Final residual = 0.000850571, No Iterations 15 GAMG: Solving for p, Initial residual = 0.0560913, Final residual = 4.81741e05, No Iterations 14 GAMG: Solving for p, Initial residual = 0.00783873, Final residual = 7.67655e06, No Iterations 14 GAMG: Solving for p, Initial residual = 0.00219096, Final residual = 2.16098e06, No Iterations 14 GAMG: Solving for p, Initial residual = 0.000818089, Final residual = 6.0367e07, No Iterations 13 GAMG: Solving for p, Initial residual = 0.000324318, Final residual = 2.75583e07, No Iterations 11 time step continuity errors : sum local = 8.54545e+92, global = 1.55141e+89, cumulative = 1.55007e+89 ExecutionTime = 27290.9 s ClockTime = 27291 s Time = 19 #0 Foam::error::printStack(Foam::Ostream&) in "/home/carles/OpenFOAM/OpenFOAM2.0.x/platforms/linux64Gcc45DPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/carles/OpenFOAM/OpenFOAM2.0.x/platforms/linux64Gcc45DPOpt/lib/libOpenFOAM.so" #2 in "/lib64/libc.so.6" #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/carles/OpenFOAM/OpenFOAM2.0.x/platforms/linux64Gcc45DPOpt/lib/libOpenFOAM.so" #4 in "/home/carles/OpenFOAM/OpenFOAM2.0.x/platforms/linux64Gcc45DPOpt/bin/simpleFoam" #5 in "/home/carles/OpenFOAM/OpenFOAM2.0.x/platforms/linux64Gcc45DPOpt/bin/simpleFoam" #6 in "/home/carles/OpenFOAM/OpenFOAM2.0.x/platforms/linux64Gcc45DPOpt/bin/simpleFoam" #7 __libc_start_main in "/lib64/libc.so.6" #8 at /usr/src/packages/BUILD/glibc2.11.2/csu/../sysdeps/x86_64/elf/start.S:116 Floating point exception 1. http://www.cfdonline.com/Forums/ope...implefoam.html Quote:
http://www.cfdonline.com/Forums/ope...adystate.html Quote:
Do someone know a good book, papers whatever that help me to understand a bite more about the different schemes that i can choose? Any suggestion will be rally appreciated. Thanks! Carles 

May 31, 2012, 05:33 

#4 
Senior Member

Dear Carles,
Well it seems like you problems do lie elsewhere. Did you check your mesh, running checkMesh? Does it look ok? If not, than I think you may need to look into your boundary conditions. I do not think the nonOrthogonalityCorrectors are necessary unless you have nonOrthogonality problems reported by checkMesh. Also in that case I would suggest you use the Code:
Gauss linear limited 0.333 I also do not think it is necessary to have a maxIter larger than the standard 1000. I usually only set it to a lower value if there is some instability in the first couple of iterations, just to speed up the entire process. Furthermore I would suggest in your fvSolution to just use a relTol of 0.01 for p and maybe just 0.1 for the other variables. Than I think your numerics setup should be ok, maybe only play around with lower relaxation factors for the first few iterations. Yes, you can change stuff in the fvSystem/fvSolution file during runtime and it will be taken into account. The initialization may work, but it depends on the problem. First make sure your mesh and boundary conditions are ok, otherwise initialization won't do the trick. So I would suggest to first run checkMesh and maybe check again your boundary conditions, before trying to change your numerics. Good luck, Tom 

May 31, 2012, 10:13 

#5 
New Member
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 7 
Dear Tom,
I think that the mesh is ok. The only prooblems that checkMesh report me is: Code:
***Wedge patch frontAndBackPlanes_pos not planar. Point (0.268943 0.0632487 0.00275887) is not in patch plane by 8.66739e07 meter. Code:
Mesh nonorthogonality Max: 25.1038 average: 4.18976 Nonorthogonality check OK. Thanks, Carles 

May 31, 2012, 10:29 

#6 
Senior Member

Dear Carles,
Ah so it is an axissymmetrical case. How many cells does it have? Not a lot I would guess? Could you maybe post your entire checkMesh result and your boundary conditions for U and p? Also a picture of your geometry (preferably showing the mesh) would help a lot. Regards, Tom 

May 31, 2012, 11:54 

#7 
New Member
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 7 
Dear Tom,
Of course I can, checkMesh Code:
Mesh stats points: 1813894 internal points: 0 faces: 3608735 internal faces: 1784797 cells: 900880 boundary patches: 5 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 889132 prisms: 11748 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 WALL 22104 44211 ok (nonclosed singly connected) INLET 64 129 ok (nonclosed singly connected) GAPTOP 10 22 ok (nonclosed singly connected) frontAndBackPlanes_pos900880 907814 ok (nonclosed singly connected) frontAndBackPlanes_neg900880 907814 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0 0 0.00396936) (0.38 0.091 0.00396936) Mesh (nonempty, nonwedge) directions (1 1 0) Mesh (nonempty) directions (1 1 1) Wedge frontAndBackPlanes_pos with angle 2.49531 degrees ***Wedge patch frontAndBackPlanes_pos not planar. Point (0.268943 0.0632487 0.00275887) is not in patch plane by 8.66739e07 meter. Boundary openness (2.32202e17 9.25979e15 2.14019e14) OK. Max cell openness = 3.31318e16 OK. Max aspect ratio = 4.02019 OK. Minumum face area = 1.74478e09. Maximum face area = 3.16415e06. Face area magnitudes OK. Min volume = 3.8192e13. Max volume = 9.20786e10. Total volume = 0.000124784. Cell volumes OK. Mesh nonorthogonality Max: 25.1038 average: 4.18976 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.621888 OK. Coupled point location match (average 0) OK. Failed 1 mesh checks. Code:
dimensions [0 2 2 0 0 0 0]; internalField uniform 0; boundaryField { WALL { type zeroGradient; } INLET { type zeroGradient; } GAPTOP { type fixedValue; value uniform 0; } frontAndBackPlanes_pos { type wedge; } frontAndBackPlanes_neg { type wedge; } } Code:
dimensions [0 1 1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { WALL { type fixedValue; value uniform (0 0 0); } INLET { type timeVaryingMappedFixedValue; setAverage off; } GAPTOP { type zeroGradient; } frontAndBackPlanes_pos { type wedge; } frontAndBackPlanes_neg { type wedge; } } Code:
// Average (0 0 0) // Data on points 80 ( ( 0.091885373 0 0 ) ( 0.091700472 0 0 ) ( 0.09133745 0 0 ) ( 0.090811901 0 0 ) ( 0.090139844 0 0 ) ( 0.089339107 0 0 ) ( 0.088429593 0 0 ) ( 0.087431565 0 0 ) ( 0.086365201 0 0 ) ( 0.085249819 0 0 ) ( 0.084103227 0 0 ) ( 0.082941331 0 0 ) ( 0.081778221 0 0 ) ( 0.080625713 0 0 ) ( 0.079493508 0 0 ) ( 0.078389108 0 0 ) ( 0.077317581 0 0 ) ( 0.076281399 0 0 ) ( 0.075279854 0 0 ) ( 0.074308395 0 0 ) ( 0.073357597 0 0 ) ( 0.072411761 0 0 ) ( 0.071447313 0 0 ) ( 0.07043115 0 0 ) ( 0.069319129 0 0 ) ( 0.068055138 0 0 ) ( 0.066571429 0 0 ) ( 0.064790532 0 0 ) ( 0.062629394 0 0 ) ( 0.060005635 0 0 ) ( 0.056845449 0 0 ) ( 0.053092379 0 0 ) ( 0.04871482 0 0 ) ( 0.043710824 0 0 ) ( 0.038109064 0 0 ) ( 0.031965468 0 0 ) ( 0.025357356 0 0 ) ( 0.018376643 0 0 ) ( 0.011126214 0 0 ) ( 0.0037204318 0 0 ) ( 0.091885373 0 0 ) ( 0.091700472 0 0 ) ( 0.09133745 0 0 ) ( 0.090811901 0 0 ) ( 0.090139844 0 0 ) ( 0.089339107 0 0 ) ( 0.088429593 0 0 ) ( 0.087431565 0 0 ) ( 0.086365201 0 0 ) ( 0.085249819 0 0 ) ( 0.084103227 0 0 ) ( 0.082941331 0 0 ) ( 0.081778221 0 0 ) ( 0.080625713 0 0 ) ( 0.079493508 0 0 ) ( 0.078389108 0 0 ) ( 0.077317581 0 0 ) ( 0.076281399 0 0 ) ( 0.075279854 0 0 ) ( 0.074308395 0 0 ) ( 0.073357597 0 0 ) ( 0.072411761 0 0 ) ( 0.071447313 0 0 ) ( 0.07043115 0 0 ) ( 0.069319129 0 0 ) ( 0.068055138 0 0 ) ( 0.066571429 0 0 ) ( 0.064790532 0 0 ) ( 0.062629394 0 0 ) ( 0.060005635 0 0 ) ( 0.056845449 0 0 ) ( 0.053092379 0 0 ) ( 0.04871482 0 0 ) ( 0.043710824 0 0 ) ( 0.038109064 0 0 ) ( 0.031965468 0 0 ) ( 0.025357356 0 0 ) ( 0.018376643 0 0 ) ( 0.011126214 0 0 ) ( 0.0037204318 0 0 ) ) 

May 31, 2012, 11:57 

#8 
New Member
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 7 
And some screen shots.


May 31, 2012, 12:22 

#9 
Senior Member

Carles,
I am wondering a bit about the problem you are trying to solve. If I read your checkMesh file correctly you have a patch GAPTOP that has only 10 faces and it seems from your boundary conditions you want to set this as your outlet. From the pictures I can't really tell what way the flow is meant to go. I think you specify an inlet at the bottom left, but I do not see where the outlet is exactly and also I do not see a patch of only 10 faces. Are you sure that this GAPTOP patch is defined correctly? I think you may want to try to first perform a simulation with a fixed inflow value instead of the mapped one, and maybe generate a coarser mesh to find the correct setup for your problem. If that is found gradually increase the complexity of the simulation until you achieve the correct simulation. I won't be near a computer next couple of days, so I hope you can work out your problem, of someone else can help you. Cheers, Tom 

June 1, 2012, 07:47 

#10  
New Member
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 7 
Hi Tom,
Yes you're right about the inlet. itīs at the bottom left. The outlet is located at the top right, I forget to attach a picture. Quote:
Thanks for your time!! greetings, carles 

June 26, 2012, 05:54 

#11 
New Member
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 7 
I could find a solution, the problem was in the fvSolution file. Now iīm using this settings:
Code:
solvers { p_rgh { solver GAMG; tolerance 1e12; relTol 0.001; minIter 5; maxIter 200; smoother GaussSeidel; // DIC; //DICGaussSeidel; //FDIC; nPreSweeps 1; nPostSweeps 3; nFinestSweeps 3; scaleCorrection true; directSolveCoarsest false; cacheAgglomeration on; nCellsInCoarsestLevel 50; // 500 agglomerator faceAreaPair; mergeLevels 1; // 3 } U { solver PBiCG; preconditioner DILU; tolerance 1e09; relTol 0.1; } k { solver PBiCG; preconditioner DILU; tolerance 1e09; relTol 0.1; } epsilon { solver PBiCG; preconditioner DILU; tolerance 1e09; relTol 0.1; } R { solver PBiCG; preconditioner DILU; tolerance 1e09; relTol 0.1; } T { solver PBiCG; preconditioner DILU; minIter 400; tolerance 1e09; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 1; } relaxationFactors { p_rgh 0.7; U 0.7; k 0.7; epsilon 0.7; R 0.7; T 0.7; } 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
convergence problem when use pisoFoam, LES for wind tunnel case  Forrest_Lei  OpenFOAM  3  July 19, 2011 06:00 
convergence problem  commonyue  Main CFD Forum  1  December 1, 2009 04:54 
Convergence of CFX field in FSI analysis  nasdak  CFX  2  June 29, 2009 01:17 
3D Fluid Flow Convergence problem  Emily  FLUENT  2  March 21, 2007 23:18 
Non Convergence of 3D Heat transfer cfd problem  Balraj  Main CFD Forum  3  December 9, 2004 01:24 