
[Sponsors] 
January 17, 2008, 20:13 
I'm currently trying to do a s

#1 
Member
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 10 
Sponsored Links
The mesh is a simple tetrahedral mesh made with gmsh to the tune of around 1 million cells, the checkmesh results are as follows: Checking geometry... Domain bounding box: (44.104 16.605 15.21) (184.676 16.605 18) Boundary openness (5.39114e17 5.56627e18 1.00736e17) OK. Max cell openness = 1.75755e16 OK. Max aspect ratio = 590.305 OK. Minumum face area = 4.02e08. Maximum face area = 10.9795. Face area magnitudes OK. Min volume = 8.9847e10. Max volume = 12.1966. Total volume = 252267. Cell volumes OK. Mesh nonorthogonality Max: 89.6816 average: 21.2003 *Number of severely nonorthogonal faces: 149. Nonorthogonality check OK. <<Writing 149 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 3.76367 OK. *Edges too small, min/max edge length = 1e05 5.86748, number too small: 1 <<Writing 2 points on short edges to set shortEdges All angles in faces OK. All face flatness OK. Mesh OK. End  Granted the mesh isn't exactly great but this is more due to the complexity of the object I'm trying to generate the flow around. My scheme and solution setups are as follows:  ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear limited 0.5; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } solvers { p GAMG { tolerance 1e07; relTol 0; smoother GaussSeidel; nCellsInCoarsestLevel 200; mergeLevels 1; agglomerator faceAreaPair; cacheAgglomeration off; nPreSweeps 1; nPostSweeps 2; nFinestSweeps 2; scaleCorrection true; directSolveCoarsest false; }; U PBiCG { tolerance 1e07; relTol 0.1; preconditioner DILU; }; k PBiCG { tolerance 1e07; relTol 0.1; preconditioner DILU; }; epsilon PBiCG { tolerance 1e07; relTol 0.1; preconditioner DILU; }; R PBiCG { tolerance 1e07; relTol 0.1; preconditioner DILU; }; nuTilda PBiCG { tolerance 1e07; relTol 0.1; preconditioner DILU; }; } SIMPLE { nNonOrthogonalCorrectors 5; pRefCell 0; pRefValue 0; } relaxationFactors { p 0.2; U 0.5; k 0.3; epsilon 0.3; R 0.7; nuTilda 0.7; }  As things are currently, the solution diverges right from the start, after 2 iterations my lift and drag forces are in the order of 1e8 or so and my local continuity errors increase until eventually the system crashes, here's the readout from the first few iterations of the solution.  Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0470618, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0263094, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0251062, No Iterations 1 GAMG: Solving for p, Initial residual = 1, Final residual = 8.6099e08, No Iterations 18 GAMG: Solving for p, Initial residual = 0.0975858, Final residual = 8.43973e08, No Iterations 16 GAMG: Solving for p, Initial residual = 0.0248457, Final residual = 9.02797e08, No Iterations 13 GAMG: Solving for p, Initial residual = 0.00976953, Final residual = 5.16382e08, No Iterations 13 GAMG: Solving for p, Initial residual = 0.00536754, Final residual = 6.71377e08, No Iterations 12 GAMG: Solving for p, Initial residual = 0.00330867, Final residual = 7.83699e08, No Iterations 11 time step continuity errors : sum local = 0.013064, global = 3.73088e05, cumulative = 3.73088e05 Total pressure Force = (0.534847 2.01937 7.96596) Total viscous Force = (0.00165139 0.00937387 0.0347963) Total turbulent Force = (0 0 0) Total Force = (0.536499 2.02875 8.00076) ExecutionTime = 116.99 s ClockTime = 117 s Time = 2 DILUPBiCG: Solving for Ux, Initial residual = 0.33876, Final residual = 0.0240347, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.419772, Final residual = 0.0253754, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.41666, Final residual = 0.0234304, No Iterations 1 GAMG: Solving for p, Initial residual = 1, Final residual = 9.54611e08, No Iterations 25 GAMG: Solving for p, Initial residual = 0.0179724, Final residual = 6.66377e08, No Iterations 14 GAMG: Solving for p, Initial residual = 0.00555565, Final residual = 6.90765e08, No Iterations 14 GAMG: Solving for p, Initial residual = 0.00274587, Final residual = 6.89308e08, No Iterations 12 GAMG: Solving for p, Initial residual = 0.00169177, Final residual = 7.81096e08, No Iterations 12 GAMG: Solving for p, Initial residual = 0.00125716, Final residual = 7.1114e08, No Iterations 12 time step continuity errors : sum local = 0.102613, global = 7.33632e05, cumulative = 3.60544e05 Total pressure Force = (5.78598e+06 8.6209e+06 2.9444e+07) Total viscous Force = (23.9807 11.6406 33.9165) Total turbulent Force = (0 0 0) Total Force = (5.78601e+06 8.62091e+06 2.94441e+07) ExecutionTime = 233.26 s ClockTime = 234 s Time = 3 DILUPBiCG: Solving for Ux, Initial residual = 0.278798, Final residual = 0.00263389, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.274962, Final residual = 0.0194582, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.281969, Final residual = 0.0142537, No Iterations 1 GAMG: Solving for p, Initial residual = 0.149281, Final residual = 8.71556e08, No Iterations 23 GAMG: Solving for p, Initial residual = 0.00644011, Final residual = 8.54485e08, No Iterations 11 GAMG: Solving for p, Initial residual = 0.00191251, Final residual = 7.56476e08, No Iterations 12 GAMG: Solving for p, Initial residual = 0.000863805, Final residual = 6.18423e08, No Iterations 11 GAMG: Solving for p, Initial residual = 0.00051502, Final residual = 7.79148e08, No Iterations 11 GAMG: Solving for p, Initial residual = 0.000364454, Final residual = 7.7788e08, No Iterations 11 time step continuity errors : sum local = 0.245931, global = 6.00056e06, cumulative = 3.00538e05 Total pressure Force = (3.12704e+07 1.20367e+08 4.65635e+08) Total viscous Force = (28.0773 10.4569 33.8212) Total turbulent Force = (0 0 0) Total Force = (3.12704e+07 1.20367e+08 4.65635e+08) ExecutionTime = 340.78 s ClockTime = 341 s Time = 4 DILUPBiCG: Solving for Ux, Initial residual = 0.256524, Final residual = 0.00287552, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.212373, Final residual = 0.0138832, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.209775, Final residual = 0.0157668, No Iterations 1 GAMG: Solving for p, Initial residual = 0.0282568, Final residual = 9.9138e08, No Iterations 33 GAMG: Solving for p, Initial residual = 0.00410752, Final residual = 8.15701e08, No Iterations 17 GAMG: Solving for p, Initial residual = 0.00116876, Final residual = 7.89225e08, No Iterations 13 GAMG: Solving for p, Initial residual = 0.000591451, Final residual = 8.9654e08, No Iterations 9 GAMG: Solving for p, Initial residual = 0.000380289, Final residual = 7.98343e08, No Iterations 9 GAMG: Solving for p, Initial residual = 0.000275326, Final residual = 9.12885e08, No Iterations 8 time step continuity errors : sum local = 0.286709, global = 0.000247643, cumulative = 0.000277697 Total pressure Force = (1.14291e+08 4.25839e+07 7.23494e+08) Total viscous Force = (31.085 10.3115 52.0479) Total turbulent Force = (0 0 0) Total Force = (1.14291e+08 4.25839e+07 7.23494e+08) ExecutionTime = 459.04 s ClockTime = 460 s  It's my understanding that OpenFoam is more sensitive to bad meshes than commercial solvers, however this is probably the best mesh I'm going to be able to generate with gmsh, so is there any way I can increase the stability of my solution? 

Sponsored Links 
January 20, 2008, 19:45 
So nobody has any ideas?

#2 
Member
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 10 
So nobody has any ideas?


January 21, 2008, 01:39 
FOAM is senssitive to mesh as

#3 
Member
Mojtaba Shahmohammadian
Join Date: Mar 2009
Posts: 73
Rep Power: 10 
FOAM is senssitive to mesh as much as others or even less.
instead you must focus on cfd method to stabilize solution by means of relaxation or so. 

January 21, 2008, 17:51 
That's all well and good but I

#4 
Member
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 10 
That's all well and good but I've run down to a pressure relaxation factor of 0.01 and 10 orthagonal correctors and still my solution explodes to infinity in a few iterations. Clearly something is wrong because I can get other meshes to work just fine, the only difference is this time gmsh can't really cope with the geometry and so I have a fairly poor mesh.


January 21, 2008, 18:09 
Sorry for being stupid, but wh

#5 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,802
Rep Power: 24 
Sorry for being stupid, but where is your turbulence model being updated? There's no solver calls for kepsilon, RSM or similar...
If it's not that, you probably messed up the boundary conditions. Your mesh is criminally bad, but the solver should still run. Which turbulence model are you using? Did you try running potentialFoam and looking at the velocity field? This will give you an idea if the mesh is usable and give you a quick check on the boundary conditions. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 21, 2008, 18:19 
The turbulence is set to lamin

#6 
Member
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 10 
The turbulence is set to laminar and switched off in simplefoam. I ran a potential foam solution and it too could not reach a stable solution however I don't think my boundary conditions are incorrect, I made sure to open the mesh in paraview and check that all the patches are what I want them to be.


January 21, 2008, 18:34 
If you cannot get a stable sol

#7 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,802
Rep Power: 24 
If you cannot get a stable solution with potentialFoam, your mesh is simply not good enough. What does the velocity feel look like? Is it horrid + where?
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 21, 2008, 19:21 
Yeah I don't think gmsh is goi

#8 
Member
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 10 
Yeah I don't think gmsh is going to let me mesh this thing. If you catch a look at the velocity field before it blows up it's horribly splotchy, after the solution blows up it doesn't make any sense anyway.
Thanks for the help anyway, I guess I'll have to look into other ways of meshing. 

January 22, 2008, 04:23 
Why are you using laminar flow

#9 
Member
Michele Vascellari
Join Date: Mar 2009
Posts: 70
Rep Power: 10 
Why are you using laminar flow with high Re number flow? Probably your flow is not laminar, but turbulent, try to use a turbulence model in order to dump the instabilities of the flow.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Reach p from fvmotionsolver  erik023  OpenFOAM Running, Solving & CFD  9  January 11, 2009 17:13 
struggling with interpretation of UDF in fluent  Suman Kandula  FLUENT  0  August 9, 2007 12:56 
How to reach steady state solution  Sally  FLUENT  10  June 14, 2007 09:26 
Intermittent Problems to Reach CFD Online?  Jonas Larsson  Main CFD Forum  4  May 28, 2006 16:26 
Struggling to converge!  John  FLUENT  2  December 21, 2005 03:29 
Sponsored Links 