
[Sponsors] 
September 3, 2012, 01:29 
Electric Car [simpleFoam] Case does not converge

#1 
New Member
Serena
Join Date: Aug 2012
Location: Tokyo
Posts: 7
Rep Power: 5 
Hello,
This is my first post! I have the model of an electric motor that is mounted right next to the wheel of a car. My final objective is to model the heat generation of the motor and to see if the incoming airflow is sufficient to dissipate the heat. Having little experience with OpenFOAM, I decided as a first step, to obtain just the pressure and velocities of the air around the motor and the wheel. But the case diverges. Very high velocities, unrealistic pressures... All the data [original mesh file (261front10side5fin.Valentino.ccm), files of system, 0, constant, directories] are saved in DROPBOX https://www.dropbox.com/sh/gg1ypj0c1sftemx/Ct7derbpHh in the OpenFOAM directory. Please open the file Output.console to see the full list of outputs and iterations. feel free to share and inspect them, hope you'll find the error. Here I just summarize the principal steps followed: 1) CONVERSION OF THE MESH USING ccm26ToFoam the mesh was generated in Star CCM+. In StarCCM+ I checked the mesh and no error was found. Ccm26ToFoam converts the mesh with no major problem. 2) CHECKING THE MESH CheckMesh find 3 errors: ***Number of nonorthogonality errors: 4. <<Writing 1788 nonorthogonal faces to set nonOrthoFaces ***Error in face pyramids: 48 faces are incorrectly oriented. <<Writing 48 faces with incorrect orientation to set wrongOrientedFaces ***Max skewness = 115.832, 84 highly skew faces detected which may impair the quality of the results <<Writing 84 skew faces to set skewFaces Coupled point location match (average 0) OK. Failed 3 mesh checks. End[/CODE]From another thread (nonorthogonality errors, incorrectly oriented faces), I read that the wrong oriented faces can be one reason of the non convergence . But I have no idea how to repair the wrong elements. Within Paraview? or with some OpenFOAM mesh utilities? I don't understand if the cause of no convergence is caused by those failed mesh checks or if the reason resides in the some wrong choices of the following steps (setting boundaries conditions and turbulent model) 3) PREPARATION OF the CASE DIRECTORIES [System, Constant, 0] I took the tutorial motor bike as guideline and copied all the files and substitute in them my new geometry: inwheel_BODY inwheel_TIRE inwheel_MOTOR inwheel_BRACKET inwheel_SUS inwheel_ARM zeroleft zerobottom zeroinlet zerooutlet zeroright zerotop inwheel_WHEEL_MAIN inwheel_FIN the six "zero*" are the surfaces of boundary condition (the external box), the "inwheel_*" are the surfaces surrounding the internal components (the tire, the motor, the SUS =suspension, ect). I applied to my "inwheel_*" the same types and values of "motorBike_.*" found in the motorbike tutorial ( > /home/serena/OpenFOAM/serena2.1.x/run/tutorials/incompressible/simpleFoam/motorBike/) 4) Launch of the ANALYSIS with simpleFOAM the iterations seem to go smooth, but after clearly diverges. Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting RAS turbulence model kOmegaSST kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; gamma1 0.5532; gamma2 0.4403; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; c1 10; } No field sources present SIMPLE: no convergence criteria found. Calculations will run for 500 steps. Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0934226, No Iterations 3 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0946569, No Iterations 3 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0943101, No Iterations 3 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0671126, No Iterations 3 time step continuity errors : sum local = 0.317996, global = 0.0441847, cumulative = 0.0441847 smoothSolver: Solving for omega, Initial residual = 0.198648, Final residual = 0.0150328, No Iterations 2 bounding omega, min: 4.21225e+06 max: 1.01861e+09 average: 17688.8 smoothSolver: Solving for k, Initial residual = 1, Final residual = 0.0992753, No Iterations 67 ExecutionTime = 8.88 s ClockTime = 9 s ..... .... Time = 500 smoothSolver: Solving for Ux, Initial residual = 0.739258, Final residual = 0.0543138, No Iterations 4 smoothSolver: Solving for Uy, Initial residual = 0.689198, Final residual = 0.0452885, No Iterations 4 smoothSolver: Solving for Uz, Initial residual = 0.749222, Final residual = 0.0557543, No Iterations 4 GAMG: Solving for p, Initial residual = 0.000150562, Final residual = 5.88119e06, No Iterations 2 time step continuity errors : sum local = 1.51389e+24, global = 7.6719e+21, cumulative = 4.16417e+22 smoothSolver: Solving for omega, Initial residual = 0.261228, Final residual = 0.0235003, No Iterations 6 smoothSolver: Solving for k, Initial residual = 0.636562, Final residual = 0.0634246, No Iterations 7 bounding k, min: 2.14769e+45 max: 3.1141e+55 average: 1.11945e+52 ExecutionTime = 1032.31 s ClockTime = 1034 s End 5) Paraview postprocessing The results are poor. Is it a mesh problem, or my boundaries conditions are wrong, or is my turbulent model or something else? Observations: I have noticed that if I put "turbulence off;" in the constant\RasProperties file, at least in the first iterations results don't seem so bad. But still after velocities are too high, not realistic. Code:
Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0934226, No Iterations 3 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0946569, No Iterations 3 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0943101, No Iterations 3 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0671126, No Iterations 3 time step continuity errors : sum local = 0.317996, global = 0.0441847, cumulative = 0.0441847 ExecutionTime = 7.12 s ClockTime = 7 s Time = 2 smoothSolver: Solving for Ux, Initial residual = 0.440356, Final residual = 0.0357597, No Iterations 4 smoothSolver: Solving for Uy, Initial residual = 0.555957, Final residual = 0.0404236, No Iterations 4 smoothSolver: Solving for Uz, Initial residual = 0.579449, Final residual = 0.0440795, No Iterations 4 GAMG: Solving for p, Initial residual = 0.345033, Final residual = 0.0144896, No Iterations 2 time step continuity errors : sum local = 0.17027, global = 0.0219908, cumulative = 0.0661755 ExecutionTime = 8.37 s ClockTime = 9 s ... Time = 9 smoothSolver: Solving for Ux, Initial residual = 0.0512727, Final residual = 0.00394622, No Iterations 4 smoothSolver: Solving for Uy, Initial residual = 0.129337, Final residual = 0.00857934, No Iterations 4 smoothSolver: Solving for Uz, Initial residual = 0.127992, Final residual = 0.00912636, No Iterations 4 GAMG: Solving for p, Initial residual = 0.69351, Final residual = 0.0459734, No Iterations 2 time step continuity errors : sum local = 0.182883, global = 0.023035, cumulative = 0.0058053 ExecutionTime = 17.07 s ClockTime = 17 s Time = 10 smoothSolver: Solving for Ux, Initial residual = 0.0278722, Final residual = 0.00182727, No Iterations 4 smoothSolver: Solving for Uy, Initial residual = 0.0781596, Final residual = 0.00476132, No Iterations 4 smoothSolver: Solving for Uz, Initial residual = 0.0742209, Final residual = 0.00448103, No Iterations 4 GAMG: Solving for p, Initial residual = 0.558621, Final residual = 0.0504483, No Iterations 2 time step continuity errors : sum local = 0.200628, global = 0.00653344, cumulative = 0.0123387 ExecutionTime = 18.3 s ClockTime = 18 s ... Time = 500 smoothSolver: Solving for Ux, Initial residual = 0.0026294, Final residual = 0.000257185, No Iterations 3 smoothSolver: Solving for Uy, Initial residual = 0.0989776, Final residual = 0.00675909, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 0.0245168, Final residual = 0.0023348, No Iterations 3 GAMG: Solving for p, Initial residual = 0.273924, Final residual = 0.00853, No Iterations 2 time step continuity errors : sum local = 0.0532629, global = 0.00939804, cumulative = 0.111357 ExecutionTime = 625.82 s ClockTime = 627 s With regards, Serena 

September 4, 2012, 02:09 

#2  
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ  Denmark
Posts: 472
Rep Power: 16 
Hi
Quote:
If I were you I would remake the mesh using snappyHexMesh. Best
__________________
Linnemann PS. I do not do personal support, so please post in the forums. 

September 5, 2012, 00:16 

#3 
New Member
Serena
Join Date: Aug 2012
Location: Tokyo
Posts: 7
Rep Power: 5 
Thank you very much for your reply.
I'm trying to recreate the mesh with snappyHexMesh as you adviced me. My problem now is that in the help guide I read I should insert the STL inside a box created with blockMesh. In my case, the STL file comes already with the surrounding box. The 6 external surfaces (Top Bottom inlet outlet right left) are connected with the surfaces of the model. Is it possible to use those external surfaces for creating the background hex mesh? or do I have to cancel them, leave just the model surfaces and recreate a new box from scratch? I was trying to import the STL file in Engrid and try to find some tools to cancel what I don't need. Does it make sense to you or am I on the wrong road? 

September 7, 2012, 04:44 

#4 
New Member
Serena
Join Date: Aug 2012
Location: Tokyo
Posts: 7
Rep Power: 5 
You were right, the mesh was the culprit.
I have still problem getting the new mesh using snappyhexmesh, but I managed to get a mesh with no errors using the tetrahedral mesher of Star CCM+ instead of the polyhedral. I loose the prism boundary layer, so I tried to compensate that using smaller tetrahedral elements near the wall surface (4million cells in total). The pressure and velocities given by simpleFoam seem reasonable. I used a delta T quite small, the iterations weren't quick. Not knowing too much about CFD, maybe I have mistaken some parameters. Do you see any not so reasonable settings in my files or anything that can be changed in order to get results quicker? > k: internalField uniform $turbulentKE; > nut : internalField uniform 0; > omega : internalField uniform $turbulentOmega; > pressure : internalField uniform 0; > RASModel kOmegaSST; > transportModel Newtonian; nu nu [0 2 1 0 0 0 0] 1.5e05; > ControlDict startTime 0; stopAt endTime; endTime 10; deltaT 0.005; writeControl timeStep; writeInterval 5;  ddtSchemes { default steadyState; } gradSchemes { default cellLimited Gauss linear 1; //default Gauss linear; } divSchemes { default none; div(phi,U) Gauss linearUpwindV grad(U); div(phi,k) Gauss upwind; div(phi,omega) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; }  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; } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.3; } equations { U 0.7; k 0.0:// 0.7; omega 0.0; // 0.7; } } cache { grad(U); }  last step : Time = 10 smoothSolver: Solving for Ux, Initial residual = 0.0007681, Final residual = 4.04672e05, No Iterations 4 smoothSolver: Solving for Uy, Initial residual = 0.00634906, Final residual = 0.000340722, No Iterations 4 smoothSolver: Solving for Uz, Initial residual = 0.00681167, Final residual = 0.000369204, No Iterations 4 GAMG: Solving for p, Initial residual = 0.0418852, Final residual = 0.0040769, No Iterations 1 time step continuity errors : sum local = 0.00021217, global = 1.0422e06, cumulative = 0.0308522 smoothSolver: Solving for omega, Initial residual = 0.00115887, Final residual = 0.000114091, No Iterations 15 smoothSolver: Solving for k, Initial residual = 0.0117018, Final residual = 0.00115757, No Iterations 30 ExecutionTime = 52168.6 s ClockTime = 52529 s End 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Boundary Conditions  Thomas P. Abraham  Main CFD Forum  20  July 7, 2013 05:05 
Car park ventilation and impulse fans  guillaume  Main CFD Forum  12  June 27, 2011 11:16 
Free surface boudary conditions with SOLAVOF  Fan  Main CFD Forum  10  September 9, 2006 12:24 
Turbulent Flat Plate Validation Case  Jonas Larsson  Main CFD Forum  0  April 2, 2004 10:25 
Body force  Does it work?  Jan Rusås  CFX  5  August 27, 2002 09:50 