# convergence problems using simpleFoam

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

 November 25, 2009, 14:31 convergence problems using simpleFoam #1 New Member   Sebastian Join Date: Nov 2009 Posts: 2 Rep Power: 0 Hi, I'm trying to simulate a dust enclosure. The first I want to simulate is the closed enclosure. I have one outlet (with a given velocity of about 20 m/s) and 2 or 3 inlets (with a given pressure of 0 Pa). Later I want to simulate with open door (pressure 0 Pa), to look if there is an outflow. For this I had made a model in *.stl. I meshed this model using snappyHexMesh. Now I have the problem, that the solution does not converge. Sometimes it blows up, and sometimes the residuals stay at one point and go up and down slowly (many iterations). So I can't get a right solution. I also viewed the results in paraview, but I can't see a steady solution. For example: Code: ```Time = 815 DILUPBiCG: Solving for Ux, Initial residual = 0.00381937156, Final residual = 5.46407448e-07, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.0039635767, Final residual = 3.38204802e-07, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.00394110401, Final residual = 5.52425189e-07, No Iterations 2 DICPCG: Solving for p, Initial residual = 0.0339215183, Final residual = 3.39079191e-06, No Iterations 260 time step continuity errors : sum local = 1.59943344e-05, global = 6.05402128e-10, cumulative = 1.90916487e-06 ExecutionTime = 3293.45 s ClockTime = 3304 s (has to be about 10 000sec I made a break)``` My checkMesh now looks like this: Code: ```Mesh stats points: 590512 faces: 1672734 internal faces: 1609959 cells: 541732 boundary patches: 8 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 516514 prisms: 10178 wedges: 145 pyramids: 0 tet wedges: 322 tetrahedra: 0 polyhedra: 14573 Checking topology... Boundary definition 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 defaultFaces 0 0 ok (empty) xxxxxx_lalu 2179 2361 ok (non-closed singly connected) xxxxxx_outlet 271 311 ok (non-closed singly connected) xxxxxx_spa_links 2271 2387 ok (non-closed singly connected) xxxxxx_spa_rechts2270 2386 ok (non-closed singly connected) xxxxxx_tuerschl 131 249 ok (non-closed singly connected) xxxxxx_tuer 3168 3337 ok (non-closed singly connected) xxxxxx_walls 52485 54205 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (-0.0495049591 -1.879 0) (1.1265 0 1.87) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (-2.18009372e-18 3.97104586e-19 2.29753118e-19) OK. Max cell openness = 2.59771373e-16 OK. Max aspect ratio = 37.4175372 OK. Minumum face area = 1.79977657e-06. Maximum face area = 0.00207470849. Face area magnitudes OK. Min volume = 2.31921363e-09. Max volume = 7.75293658e-05. Total volume = 2.47929553. Cell volumes OK. Mesh non-orthogonality Max: 64.3808597 average: 5.39379502 Non-orthogonality check OK. Face pyramids OK. Max skewness = 3.82309381 OK. Mesh OK.``` For me it looks good. So I made a set up for a laminar incompressible flow. (I think, the effect of compression is very little and laminar is a good choice for beginnig). My parameters are: Code: ```RASModell laminar turbulence off simulationType laminar nu=13.5e-06 (constant for air)``` For the solver I choose the following: Code: ```p { solver PCG; preconditioner DIC; tolerance 1e-07; relTol 0.001;} U { solver PBiCG; preconditioner DILU; tolerance 1e-05; relTol 0.001; } SIMPLE { nNonOrthogonalCorrectors 0; } relaxationFactors { p 0.3; U 0.2; }``` I also tried lower and higher relaxationFactors GAMG for p and U, but nothing helps. I also use the following schemes: Code: ```div(phi,U) Gauss upwind; interpolate(U) linear; ddt default steadyState;``` The BC is like this: Code: ```U outlet -> fixedValue uniform (0 0 20) inlets -> zeroGradient walls and doors -> fixedValue uniform (0 0 0) p outlet -> zeroGradient inlets -> fixedValue 0 walls and doors -> zeroGradient``` Now I tried to get rid of the problems for two weeks. I tried other BCs (outletInlet), other schemes (linear instead of upwind) and so on. I hope you can help me with this problem and give me an hint to clear the fault I surely made somewhere. If I should give you further informations don't hesitate to ask. Thank you very much. Sebastian

 November 25, 2009, 15:26 #2 Senior Member     Niels Nielsen Join Date: Mar 2009 Location: NJ - Denmark Posts: 483 Rep Power: 17 Hi your skewness is very bad (3.8), best results coming from having it below 0.9. you could also try leastSquares (or faceLimited) as gradSchemes and maybe gammaV 0.2 for div(phi,U). and upwind for the turbulence properties. I would still focus on the grid skewness as my main place of interest. Try using another mesh generator like Netgen, Engrid or Salome. Code: ```ddtSchemes { default steadyState; } gradSchemes { default leastSquares; grad(p) leastSquares; grad(U) leastSquares; // grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) Gauss gammaV 0.2; div(phi,k) Gauss upwind; div(phi,omega) Gauss upwind; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { // default Gauss linear corrected; default Gauss linear limited 0.5; // default Gauss linear limited 0.333; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } // ************************************************************************* //``` Also using smoothSolver for U,k,omega,epsilon would be an idea same as using GAMG for p. Code: ``` solvers { p { solver GAMG; tolerance 1e-7; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; }; U { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; }; k { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; }; omega { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; }; } SIMPLE { nNonOrthogonalCorrectors 0; } relaxationFactors { p 0.3; U 0.7; k 0.7; omega 0.7; } // ************************************************************************* //``` __________________ Linnemann PS. I do not do personal support, so please post in the forums.

 November 25, 2009, 15:37 #3 Senior Member     Niels Nielsen Join Date: Mar 2009 Location: NJ - Denmark Posts: 483 Rep Power: 17 Hi again another thing if you have it write out values often you can open paraview and examine where the solution values blow up. This way you can examine the mesh where this occurs and I bet it is where you have your most skewed cells. I once had one badly skewed cell (4.12) and it made the whole solution crash. So even though checkMesh states the mesh is ok you have to use your common sense to see if "you" accept it to be ok :-). __________________ Linnemann PS. I do not do personal support, so please post in the forums.

 November 25, 2009, 16:27 #4 New Member   Sebastian Join Date: Nov 2009 Posts: 2 Rep Power: 0 Yes you're right, I saw this phenomenon before, that two skewed cells at the inlet make trouble. I refinde the mesh using snappyHexMesh with refinementRegion or sth. like that. The mesh I had bevor was even worse than this. I decided to use sHM cause, the other tools often crash (netgen) or do something for long time without feedback (Salome). But I think I have no other chance and so I'll give Salome a second chance and try it. The schemes you told me, I will try them tomorrow (probably on the new mesh). Thank you for your help

 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 brahim OpenFOAM Running, Solving & CFD 20 June 9, 2015 09:09 Kutti OpenFOAM 16 June 14, 2010 08:12 franzdrs Main CFD Forum 0 June 15, 2009 18:17 schnitzlein OpenFOAM Running, Solving & CFD 6 June 24, 2005 09:51 Chetan FLUENT 3 April 15, 2004 19:13

All times are GMT -4. The time now is 15:32.