
[Sponsors] 
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 = 5.46407448e07, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.0039635767, Final residual = 3.38204802e07, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.00394110401, Final residual = 5.52425189e07, No Iterations 2 DICPCG: Solving for p, Initial residual = 0.0339215183, Final residual = 3.39079191e06, No Iterations 260 time step continuity errors : sum local = 1.59943344e05, global = 6.05402128e10, cumulative = 1.90916487e06 ExecutionTime = 3293.45 s ClockTime = 3304 s (has to be about 10 000sec I made a break) 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 (nonclosed singly connected) xxxxxx_outlet 271 311 ok (nonclosed singly connected) xxxxxx_spa_links 2271 2387 ok (nonclosed singly connected) xxxxxx_spa_rechts2270 2386 ok (nonclosed singly connected) xxxxxx_tuerschl 131 249 ok (nonclosed singly connected) xxxxxx_tuer 3168 3337 ok (nonclosed singly connected) xxxxxx_walls 52485 54205 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0.0495049591 1.879 0) (1.1265 0 1.87) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (2.18009372e18 3.97104586e19 2.29753118e19) OK. Max cell openness = 2.59771373e16 OK. Max aspect ratio = 37.4175372 OK. Minumum face area = 1.79977657e06. Maximum face area = 0.00207470849. Face area magnitudes OK. Min volume = 2.31921363e09. Max volume = 7.75293658e05. Total volume = 2.47929553. Cell volumes OK. Mesh nonorthogonality Max: 64.3808597 average: 5.39379502 Nonorthogonality check OK. Face pyramids OK. Max skewness = 3.82309381 OK. Mesh OK. Code:
RASModell laminar turbulence off simulationType laminar nu=13.5e06 (constant for air) Code:
p { solver PCG; preconditioner DIC; tolerance 1e07; relTol 0.001;} U { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.001; } SIMPLE { nNonOrthogonalCorrectors 0; } relaxationFactors { p 0.3; U 0.2; } Code:
div(phi,U) Gauss upwind; interpolate(U) linear; ddt default steadyState; 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 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: 472
Rep Power: 16 
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; } // ************************************************************************* // Code:
solvers { p { solver GAMG; tolerance 1e7; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; }; U { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; }; k { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; }; omega { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; 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: 472
Rep Power: 16 
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  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
SimpleFoam convergence problems  brahim  OpenFOAM Running, Solving & CFD  20  June 9, 2015 09:09 
Convergence Problems SimpleFOAM  Kutti  OpenFOAM  16  June 14, 2010 08:12 
Problems with convergence with an easy system  franzdrs  Main CFD Forum  0  June 15, 2009 18:17 
SimpleFoam convergence problems  schnitzlein  OpenFOAM Running, Solving & CFD  6  June 24, 2005 09:51 
Convergence problems  Chetan  FLUENT  3  April 15, 2004 19:13 