# No convergence because of underdeterminedCells?

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

September 2, 2011, 09:45
No convergence because of underdeterminedCells?
#1
New Member

Join Date: Aug 2011
Posts: 4
Rep Power: 5
Hi,

I have a problem running a case with SimpleFoam. The geometry is quite complex. I'm running the case with turbulence off. I made the mesh with netgen (1.4M cells, no layers). As you can see in the attached File the case doesn't converge although the solution looks physical to me.
My checkMesh complains only about some non-orthogonal Faces and a lot of under-determined Cells.
Could these cells effect the convergence?
Or what can I change in fvSolution / fvSchemes so that the case converge?

Quote:
 Checking geometry... Overall domain bounding box (-876.472 -48 -63.9999) (884.528 48 273) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (2.12129e-17 -1.9514e-16 1.29017e-16) OK. Max cell openness = 3.51972e-16 OK. Max aspect ratio = 33.8371 OK. Minumum face area = 0.146015. Maximum face area = 287.294. Face area magnitudes OK. Min volume = 0.0386411. Max volume = 1541.7. Total volume = 3.29777e+07. Cell volumes OK. Mesh non-orthogonality Max: 84.8534 average: 16.5116 *Number of severely non-orthogonal faces: 42. Non-orthogonality check OK. <
Quote:
 /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default Gauss linear; div(phi,U) Gauss linearUpwindV Gauss linear div(phi,k) Gauss upwind; div(phi,omega) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } // ************************************************** *********************** //
Quote:
 /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p { solver GAMG; tolerance 1e-7; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; //2 cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; //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; } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { p 0.3; U 0.7; k 0.7; omega 0.7; } cache { grad(U); } // ************************************************** *********************** //
Attached Images
 Residuals.jpg (27.8 KB, 43 views)

 September 5, 2011, 14:12 #2 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 8,301 Blog Entries: 34 Rep Power: 84 Greetings Tobi-R and welcome to the forum! You better try removing those undetermined cells: http://openfoamwiki.net/index.php/SetSet The best solution would be for the mesh to be "100% OK" according to checkMesh, but since there are strange cells in it, you would either have to edit the mesh manually to fix it (I don't know how to do that), or you can use the setSet utility to manipulate the mesh based on the sets created by checkMesh. Best regards and good luck! Bruno Alhasan likes this. __________________ OpenFOAM: Frequently Asked Questions | Useful links for building and using Forum: How to ask for help | Posting code and output with [CODE] My to-do list and when I'll be able to come to the forum: http://wyldckat.github.io And please: Read this before sending private messages to me

 September 6, 2011, 12:30 #3 Senior Member     Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 543 Rep Power: 18 Tobi-R I encountered this a lot over the summer and tried to figure out how to remove these. Though i am not exactly sure what under-determined cells can do to the solution (if anyone can answer i would appreciate that as well), i do know that more of them correlated to terrible convergence. The best and possibly quickest solution I can offer is to re-mesh your geometry. I know you say it's a complex one, but you might better off in the long run. I ended up moving to extremely small mesh sizes (with more than 20 million delauney tetrahedral cells) and then converting it to a polyhedral mesh (less than 8 million cells). This of course has its own problems, but you will get better results (from my experience of course). Good luck and I hope this helps. Dan Alhasan likes this.

 September 13, 2011, 03:29 #4 New Member   Join Date: Aug 2011 Posts: 4 Rep Power: 5 Hi, thanks for the answers. Unfortunately none of your hints worked. I tried to work with the setSet utility as well as converting the mesh into a polyhedral mesh but both just made things even worse. I also tried to re-mesh the geometry. I made a finer mesh with Netgen ( ~5 million Cells) an 3 different meshes with EnGrid (1, 2.5, 8 million Cells) . All of them blew up except the mesh made with Engrid with ~8 million Cells and the results looks nearly the same as in the first post, although the checkMesh is better ( only ~ 50 under-determined cells but ~5000 non-orthogonal faces). The other EnGrid meshes had also just ~ 50 under-determined cells and only ~50 non-orthogonal faces. Has anyone another hint what I can do?

 September 13, 2011, 05:02 #5 Senior Member   Aurelien Thinat Join Date: Jul 2010 Posts: 154 Rep Power: 7 Hi Tobi, I didn't face problems with underdetermined cells. But I already faced problems with cells non-orthogonality : you have to change your fvScheme. "divSchemes { default Gauss linear; div(phi,U) Gauss linearUpwindV Gauss linear div(phi,k) Gauss upwind; div(phi,omega) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } " These schemes are used on "perfect" mesh only and you have to use limited 0,5 (or 0,33) schemes, it depends on the mesh's quality. holodeck10 and Alhasan like this.

 Tags convergence, simplefoam, underdetermined

 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 Centurion2011 FLUENT 24 May 9, 2015 08:02 nasdak CFX 2 June 29, 2009 01:17 tippo CFX 2 May 5, 2009 10:55 ganesh Main CFD Forum 4 June 30, 2006 14:20 Chetan FLUENT 3 April 15, 2004 19:13

All times are GMT -4. The time now is 17:51.