
[Sponsors] 
October 7, 2015, 05:46 
No convergence issue

#1 
New Member
Join Date: Sep 2015
Posts: 9
Rep Power: 2 
Hello everybody
I am trying to run a simulation of a reactor with the sst k omega, however I have some problems with convergence. I use the simpleFoam solver with 12 processors. fvSolution Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.2   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p { solver GAMG; tolerance 1e7; relTol 0.0; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 1000; mergeLevels 1; } pFinal { $p; tolerance 1e7; relTol 0; } "(Ukomegaepsilon)" { solver PBiCG; preconditioner DILU; tolerance 1e8; relTol 0.0; } "(Ukomegaepsilon)Final" { $U; relTol 0; } } SIMPLE { nNonOrthogonalCorrectors 1; residualControl { p 1e5; U 1e5; } } relaxationFactors { fields { p 0.1; } equations { U 0.1; k 0.05; omega 0.05; epsilon 0.1; } } cache { grad(U); } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.2   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //ddtSchemes { default steadyState;//Euler;// } gradSchemes { default cellMDLimited Gauss linear 0.5; grad(U) cellMDLimited Gauss linear 0.5; grad(omega) cellLimited leastSquares 1.0; grad(epsilon) cellLimited leastSquares 1.0; } /*divSchemes { div(phi,U) bounded Gauss linearUpwind grad(U); //bounded Gauss upwind; // div(phi,omega) bounded Gauss linearUpwind default; //bounded Gauss upwind; // div(phi,epsilon) bounded Gauss linearUpwind default; // bounded Gauss upwind; // div(phi,k) bounded Gauss linearUpwind default; //bounded Gauss upwind; // div((nuEff*dev(T(grad(U))))) Gauss linear; //Gauss linear; // }*/ divSchemes { div(phi,U) bounded Gauss linearUpwindV grad(U); // div(phi,omega) bounded Gauss upwind; //bounded Gauss linearUpwind default; // div(phi,epsilon) bounded Gauss upwind; //bounded Gauss linearUpwind default; // div(phi,k) bounded Gauss upwind; //bounded Gauss linearUpwind default; // div((nuEff*dev(T(grad(U))))) Gauss linear; //Gauss linear; // } laplacianSchemes { default Gauss linear limited 1; } snGradSchemes { default limited 0.777; } interpolationSchemes { default linear; } fluxRequired { default no; p; } // ************************************************************************* // 

October 7, 2015, 05:59 

#2 
New Member
Join Date: Sep 2015
Posts: 9
Rep Power: 2 
U
Code:
outlet { type inletOutlet; inletValue uniform (0 0 0); value uniform (0 0 0); } volume_CFD { type fixedValue; value uniform (0 0 0); } inlet1 { type fixedValue; value uniform ( 3.1337499 0 7.3826288); } inlet2 { type fixedValue; value uniform (0 0 0); //( 3.1337499 0 7.3826288); } Code:
boundaryField { // Set patchGroups for constraint patches outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } volume_CFD { type kqRWallFunction; value uniform 0; } inlet1 { type turbulentIntensityKineticEnergyInlet; intensity 0.038; value uniform 1; } inlet2 { type turbulentIntensityKineticEnergyInlet; intensity 0.038; value uniform 1; } } Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.2   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; object nut; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 1 0 0 0 0]; internalField uniform 0.11; boundaryField { inlet1 { type calculated; value uniform 0; } inlet2 { type calculated; value uniform 0; } outlet { type calculated; value uniform 0; } volume_CFD { type nutUSpaldingWallFunction; value uniform 0; } } // ************************************************************************* // Code:
CMA: no RDMA devices found CMA: no RDMA devices found CMA: no RDMA devices found CMA: no RDMA devices found CMA: no RDMA devices found CMA: no RDMA devices found  [[30462,1],5]: A highperformance Open MPI pointtopoint messaging module was unable to find any relevant network interfaces: Module: OpenFabrics (openib) Host: node045 Another transport will be used instead, although this may result in lower performance.  CMA: no RDMA devices found CMA: no RDMA devices found CMA: no RDMA devices found CMA: no RDMA devices found CMA: no RDMA devices found CMA: no RDMA devices found /**\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.x   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ Build : 2.2.x61b850bc107b Exec : checkMesh parallel Date : Oct 07 2015 Time : 11:44:56 Host : "node045" PID : 11530 Case : /CALCULS/maione1/CFDEM/tutorials/cfdemSolverIB/MeshMedia nProcs : 12 Slaves : 11 ( "node045.11531" "node045.11532" "node045.11533" "node045.11534" "node045.11535" "node037.14144" "node037.14145" "node037.14146" "node037.14147" "node037.14148" "node037.14149" ) Pstream initialized with: floatTransfer : 0 nProcsSimpleSum : 0 commsType : nonBlocking polling iterations : 0 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Disallowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 [node045:11519] 11 more processes have sent help message helpmpibtlbase.txt / btl:nonics [node045:11519] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages Time = 0 Mesh stats points: 3454052 faces: 7085734 internal faces: 4910183 cells: 1891053 faces per cell: 6.3435 boundary patches: 5 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 1534837 prisms: 51297 wedges: 0 pyramids: 0 tet wedges: 1871 tetrahedra: 69 polyhedra: 302979 Breakdown of polyhedra by number of faces: faces number of cells 4 17986 5 21538 6 65018 7 13858 8 947 9 137048 10 596 11 242 12 29823 13 917 14 28 15 11336 16 194 17 15 18 3148 19 4 20 5 21 260 24 16 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 basic patch addressing... Patch Faces Points inlet1 4140 5053 inlet2 4122 5031 volume_CFD 703841 852716 outlet 4338 4956 Checking geometry... Overall domain bounding box (0.18 0.18 0.010004) (0.18 0.18 2.5) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (1.1211e15 4.3906e18 7.4201e18) OK. Max cell openness = 1.6134e15 OK. Max aspect ratio = 32.143 OK. Minimum face area = 4.0523e09. Maximum face area = 0.00031261. Face area magnitudes OK. Min volume = 9.7672e12. Max volume = 5.0375e06. Total volume = 0.22924. Cell volumes OK. Mesh nonorthogonality Max: 65.006 average: 12.563 Nonorthogonality check OK. Face pyramids OK. ***Max skewness = 19.309, 917 highly skew faces detected which may impair the quality of the results <<Writing 917 skew faces to set skewFaces Coupled point location match (average 0) OK. Failed 1 mesh checks. End Finalising parallel run the geometry consist on a pipe with many holes on its wall, releasing air in the main core of the reactor which is cylindrical can somebody help me on that? thank you all 

October 7, 2015, 06:06 

#3 
New Member
Join Date: Sep 2015
Posts: 9
Rep Power: 2 
I attach also some slice where you can see the main pipe on the left and the differents holes of injection


October 8, 2015, 03:05 

#4 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,296
Rep Power: 19 
Hi,
1) Can you make a better mesh without these skewed cells? 2) I don't really understand the geometry. Maybe it is not important, but could you try to post a picture of the whole thing, with highlighted inlets and outlets? 3) Can you post some log output? 4) In your residual plot you see some convergence finally at the end. Why did you stop calculating and what did you change at it=12000?
__________________
The skeleton ran out of shampoo in the shower. 

October 8, 2015, 03:37 

#5 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,296
Rep Power: 19 
As I understand it your solver settings are not very good. If there is no special reason you should not deactivate the relTol in SIMPLE. In SIMPLE it is not needed that every single linear equation is solved to a very low residual (what you do by just using the "tolerance"). This is, because you do the outer (SIMPLE) iterations anyway and you just need the inner interations solved in a way that the outer algorithm remains stable. Thus, I usually use relTol=0.1 and set the tolerance to some very low value, such as 1e18.
Secondly, you set the laplacian scheme to "limited 1", which means you use the corrected scheme. This is not the most stable one. Begin with "limited 0", this is the uncorrected scheme and if that works you can start to increase the numer to 0.3, 0.5, ...
__________________
The skeleton ran out of shampoo in the shower. 

October 8, 2015, 05:58 

#6 
New Member
Join Date: Sep 2015
Posts: 9
Rep Power: 2 
thank you very much I will try your suggestions, i noticed there was something not right about the solvers. I will post here my results.
The problem is I do this mesh with snappy because is a really complicated mesh. Sorry I cannot post the entire mesh however the inlet is on the pipe on the left. Sorry I don't really remember what I've changed. I will post the log output when I go back to my office tomorrow. however thank you very much for your help, is really appreciated 

October 10, 2015, 17:00 

#7 
Senior Member
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 742
Rep Power: 9 
Hello, Kurdt89,
Im not very familar with the your simulation. But looks like you are simulating a reactor(is there bubbles of droplets?). As we know SST komega is highly appropriate for strong adverse pressure gradient. In my simulations, such as stirred tanks, bubble columns, I just use kepsilon. Could you please share some experience with SST komega model in your reactor simulaiton? Thanks.
__________________
Im the translator of OpenFOAM User Guide Chinese Edition! But always newbie on CFD. http://dyfluid.com/en.html 

October 12, 2015, 02:36 

#8 
New Member
Join Date: Sep 2015
Posts: 9
Rep Power: 2 
In my case the problem is that I cannot control the global value of y+ inside the whole thing and also that different regimes exhist, there are laminar regions in which the kepsilon family would certainly crush (already tested).
So i use k omega sst with scalable functions, which is fine but highly unstable, I still have problems with convergence. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
convergence issue for transonic turbulent case  aeroiitkgp  SU2  5  May 12, 2015 16:44 
convergence issue with turbulence  mar  CDadapco  5  February 2, 2015 03:42 
Convergence issue  dhaya400  FLUENT  1  December 5, 2014 10:58 
Convergence issue  Jake  FLUENT  3  June 30, 2005 04:12 
Convergence issue with continuity equation  Jake  FLUENT  6  June 15, 2005 16:14 