
[Sponsors] 
Finally starting to explore OpenFOAM, questions on icoFoam solver... 

LinkBack  Thread Tools  Display Modes 
July 22, 2010, 13:04 
Finally starting to explore OpenFOAM, questions on icoFoam solver...

#1 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
I have finally began exploring OpenFOAM, and trying to evaluate if the software will meet my needs in terms of functionality. I plan to attend one of the future training courses, but in the mean time I am trying to see how far I can get on my own.
The current model is a section of internal passages in a structure. I attempted to place a prismatic boundary layer on the surfaces that have flow across them, which admittedly I am still learning and not sure about the appropriate layer dimensions that this model calls for. I was attempting to look at a laminar incompressible case using the icoFoam solver. The outlet velocity is known, and I wish to determine what the pressure drop is through the passage. My main goal is to view the steady state condition pressure drop, and I can accept some loss of resolution to improve computing time. I found that I can not maintain a courant number less than 1 unless my timestep is at least 1e7. I let this iterate over the course of 2 days, and it appeared to be converging. Then, the pressure residual started oscillating around 8e6 and 1e5. Eventually, it finally started to diverge and the courant number went very high. Here are my initial conditions: " FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 2 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type fixedValue; value uniform 0; } outlet { type zeroGradient; } boundary { type zeroGradient; } } // ************************************************** *********************** //" FoamFile { version 2.0; format ascii; class volVectorField; object U; } "// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { outlet { type fixedValue; value uniform (0 0 .998); } inlet { type zeroGradient; } boundary { type fixedValue; value uniform (0 0 0); } } // ************************************************** *********************** //" Attached is a picture of the mesh and pressure/velocity plots prior to divergence. I am not sure if I have specified a boundary condition incorrectly, an improper mesh, or if I am using the wrong solver. I greatly appreciate any help. Thanks. 

July 22, 2010, 13:06 

#2 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
Also, is there a simple way to specify boundary conditions to a face based on a local coordinate system. The inlet face is not perfectly aligned with the global Cartesian, but I suppose I could transform the velocity vector if I knew the angle it was misaligned.


July 22, 2010, 13:14 

#3 
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 253
Rep Power: 14 
Hi Jason,
you can try simpleFoam. It's much faster and more stable... In the following thread are some hints how to speed up simpleFoam: http://www.cfdonline.com/Forums/ope...nvergence.html Martin 

July 22, 2010, 13:57 

#4  
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
Quote:


July 22, 2010, 14:12 

#5 
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 253
Rep Power: 14 
No, you don't need to specify other values/Parameters/fields than U and p.
Just select Code:
RASModel laminar; turbulence off; 

July 22, 2010, 14:41 

#6 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
Thanks again, I am going to give that a try on simplified passage.


July 22, 2010, 15:17 

#7 
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 253
Rep Power: 14 
Try this "system/fvSolution":
Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 1.6.x   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { U // linear equation system solver for U { solver smoothSolver; // solver type smoother GaussSeidel; // smoother type tolerance 1e06; // solver finishes if either absolute relTol 0.01; // tolerance is reached or the relative // tolerance here nSweeps 1; // setting for smoothSolver maxIter 100; // limitation of iterations number } p // linear equation system solver for p { solver GAMG; // very efficient multigrid solver tolerance 1e07; // solver finishes if either absolute relTol 0.001; // tolerance is reached or the relative // tolerance here minIter 3; // a minimum number of iterations maxIter 100; // limitation of iterions number smoother DIC; // setting for GAMG nPreSweeps 1; // 1 for p, set to 0 for all other! nPostSweeps 2; // 2 is fine nFinestSweeps 2; // 2 is fine scaleCorrection true; // true is fine directSolveCoarsestLevel false; // false is fine cacheAgglomeration on; // on is fine; set to off, if dynamic // mesh refinement is used! nCellsInCoarsestLevel 500; // 500 is fine, // otherwise sqrt(number of cells) agglomerator faceAreaPair; // faceAreaPair is fine mergeLevels 1; // 1 is fine } } SIMPLE { nNonOrthogonalCorrectors 1; // 0 is fine for perfect mesh; increase // to 1 or 2 for non orthogonal mesh convergence 1e5; // convergence criteria steady state } relaxationFactors { p 0.3; // 0.3 is stable, decrease for bad mesh U 0.7; // 0.7 is stable, decrease for bad mesh } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 1.6.x   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; // no time dependence here } gradSchemes { default Gauss linear; // Gauss linear or leastSquares grad(p) faceLimited leastSquares 0 1; // these entries overwrite grad(U) Gauss linear; // the "default" setting } divSchemes { default none; div(phi,U) Gauss upwind; // stable: Gauss upwind //div(phi,U) Gauss linearUpwind Gauss; // faster linearUpwind Gauss // div(phi,k) Gauss upwind; // for turbulent flow only // div(phi,epsilon) Gauss upwind; // for turbulent flow only // div(phi,R) Gauss upwind; // for turbulent flow only // div(R) Gauss linear; // for turbulent flow only // div(phi,nuTilda) Gauss upwind; // for turbulent flow only div((nuEff*dev(grad(U).T()))) Gauss linear; // this scheme is not used for // steady and laminar flow, but // it is read by the solver, so // it must be defined. } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; // for good meshes //laplacian(nuEff,U) Gauss linear limited 0.7; // for bad meshes laplacian((1A(U)),p) Gauss linear corrected; // for good meshes //laplacian((1A(U)),p) Gauss linear limited 0.7; // for bad meshes // for turbulent flow only: // 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; // linear is fine U linear; } snGradSchemes { default corrected; // limited 0.7; for bad meshes; // must fit to laplacianSchemes } fluxRequired { default no; p ; phi ; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 1.6.x   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application simpleFoam; // which solver (for documentation) startFrom startTime; // firstTime, startTime, latestTime startTime 0; // set > 0 to continue stopAt endTime; // writeNow, endTime, nextWrite, ... endTime 600; // Latest timestep allowed deltaT 1; // simple counter for steadyState writeControl adjustableRunTime; // or uncommon: cpuTime, clockTime writeInterval 50; // time step write interval purgeWrite 0; // 1 recycles time steps storage // 0 keeps all time steps on disk writeFormat ascii; // ascii: readable, binary: smaller writePrecision 6; // precision for ascii format writeCompression uncompressed; // compressed for gzipped files timeFormat general; // fixed, scientific or general timePrecision 6; // precision for time handling runTimeModifiable yes; // yes: OF reads dictionaries each // time step graphFormat raw; // raw, gnuplot, xmgr, jplot //libs() for user libraries, p.e. user boundary conditions //functions() for special functions // ************************************************************************* // I suppose simpleFoam will solve your simulation in a couple of minutes ;) Martin 

July 22, 2010, 15:29 

#8 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
Wow, thanks alot! Yes, I know I am only running on a core 2 duo with 5gb of ram, but felt 2 days was a bit much!


July 22, 2010, 15:45 

#9 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
Right now it is at Time= 180, but the residuals are slowly dropping. I think for now I'll let it solve through in the background for a bit and see if it reaches convergence, attached are some initial plots.


July 22, 2010, 21:11 

#10 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
I left the solution to run over night at work, but decided to restart it on my home pc. So far, it is very very slowly dropping the residual; much like the icoFoam did just before it went unstable.
I feel that some of the sharp corners with overly dense mesh concentration may be causing some of the flow instability. I am at least learning, that I have much to learn when switching from a standard structural approach to fluids . Here is an excerpt of the log file: Time = 1596 smoothSolver: Solving for Ux, Initial residual = 5.04376e05, Final residual = 9.87483e07, No Iterations 6 smoothSolver: Solving for Uy, Initial residual = 5.51604e05, Final residual = 5.5295e07, No Iterations 7 smoothSolver: Solving for Uz, Initial residual = 2.065e05, Final residual = 7.26189e07, No Iterations 5 GAMG: Solving for p, Initial residual = 0.00138633, Final residual = 8.14647e07, No Iterations 5 GAMG: Solving for p, Initial residual = 0.0016717, Final residual = 8.46325e07, No Iterations 5 GAMG: Solving for p, Initial residual = 0.00174926, Final residual = 6.99528e07, No Iterations 5 time step continuity errors : sum local = 0.000138876, global = 2.97148e07, cumulative = 6.34467e05 ExecutionTime = 1416.44 s ClockTime = 1423 s Time = 1603 smoothSolver: Solving for Ux, Initial residual = 4.989e05, Final residual = 9.76406e07, No Iterations 6 smoothSolver: Solving for Uy, Initial residual = 5.40616e05, Final residual = 5.39811e07, No Iterations 7 smoothSolver: Solving for Uz, Initial residual = 2.02852e05, Final residual = 7.14789e07, No Iterations 5 GAMG: Solving for p, Initial residual = 0.00136729, Final residual = 5.67102e07, No Iterations 5 GAMG: Solving for p, Initial residual = 0.00167996, Final residual = 1.14624e06, No Iterations 4 GAMG: Solving for p, Initial residual = 0.00162179, Final residual = 7.83107e07, No Iterations 5 time step continuity errors : sum local = 0.000155448, global = 1.93752e07, cumulative = 6.60641e05 ExecutionTime = 1455.49 s ClockTime = 1463 s 

July 22, 2010, 22:34 

#11 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Hi,
may I ask you to run a checkMesh on your case? What is the number of cells you are using and what is the size of the system? Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

July 23, 2010, 03:16 

#12 
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 253
Rep Power: 14 
I think, Alberto is right:
run a "checkMesh allTopology allGeometry" I suppose that there are cell determinant problems... Martin 

July 23, 2010, 08:24 

#13 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
Here is the output generated from the above command:
Code:
Build : 1.7.0279cc8e8233b Exec : checkMesh allTopology allGeometry Date : Jul 23 2010 Time : 08:21:33 Host : jasondesktop PID : 7142 Case : /home/jason/OpenFOAM/jason1.7.0/run/testing/pipe_test_2 nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 60110 internal points: 53412 edges: 294764 internal edges: 275060 internal edges using one boundary point: 7452 internal edges using two boundary points: 0 faces: 425684 internal faces: 412676 cells: 191029 boundary patches: 3 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 0 prisms: 74244 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 116785 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Topological cell zipup check OK. Face vertices OK. Faceface connectivity OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology Bounding box boundary 12374 6219 ok (nonclosed singly connected) (0.03277 0.00680315 0.0723646) (0.0184584 0.0211148 0.0500063) inlet 284 248 ok (nonclosed singly connected) (0.03277 0.00680315 0.0563375) (0.0294114 0.0101618 0.0516125) outlet 350 295 ok (nonclosed singly connected) (0.0267988 0.0144653 0.0723646) (0.0214612 0.0198247 0.0723646) Checking geometry... Overall domain bounding box (0.03277 0.00680315 0.0723646) (0.0184584 0.0211148 0.0500063) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (3.64353e19 2.55572e19 5.58326e19) OK. Max cell openness = 2.04311e16 OK. Max aspect ratio = 14.7891 OK. Minumum face area = 5.09213e12. Maximum face area = 3.86097e07. Face area magnitudes OK. Min volume = 1.08791e17. Max volume = 7.96135e11. Total volume = 8.08761e07. Cell volumes OK. Mesh nonorthogonality Max: 60.2802 average: 19.3085 Nonorthogonality check OK. Face pyramids OK. Max skewness = 3.16024 OK. Min/max edge length = 1.10157e06 0.001065 OK. All angles in faces OK. Face flatness (1 = flat, 0 = butterfly) : average = 0.999739 min = 0.895423 All face flatness OK. Cell determinant (wellposedness) : minimum: 0.0383356 average: 1.54342 Cell determinant check OK. Mesh OK. End 

July 23, 2010, 09:09 

#14 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
I was also wondering if it might be appropriate to loosen up on my pressure and maybe velocity tolerance. For these initial stages I am attempting to show comparative pressure drops between designs, and 510% within the converged result may be adequate.


July 23, 2010, 09:30 

#15 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Hi,
the mesh passes all the tests without errors or warnings. About tolerances, try to plot the residuals, and check if they became flat or the keep dropping, and stop the simulation after they stayed flat for a while. That should be the converged solution. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

July 23, 2010, 09:53 

#16 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
I thought the solution couldn't be assumed converged until the tolerance set is met, is a steady mean residual over time more important than hitting the tolerance?


July 23, 2010, 09:58 

#17 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
The tolerance is an arbitrary value, and it is not necessarily something you can reach, especially if very low.
Usually residuals are an indication of convergence that has to me considered together with other elements, both numerical and physical. For example, your residuals can be high, but never change for a high number of iterations, and that means your solution is not changing at all.
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

July 23, 2010, 10:01 

#18 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
Thanks again, this has been very helpful. I am relieved to know this case will not require 3 days to run .


July 23, 2010, 10:04 

#19 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
It should really take less thank 1 hour! :)
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

July 23, 2010, 10:18 

#20 
Member
Jason G.
Join Date: Sep 2009
Location: Clemmons, NC
Posts: 78
Rep Power: 10 
Yes, looking at the plot I think I could have killed it after 200500 iterations which would be 2040mins .


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Working directory via command line  Luiz  CFX  4  March 6, 2011 21:02 
AMG solver in Openfoam  gonski  Main CFD Forum  0  November 25, 2007 06:20 
questions concerning solver and multigrid methodes  youradvice  Main CFD Forum  1  August 6, 2007 15:27 
Solver exits before starting....WHY?  ali  CFX  0  February 17, 2006 04:46 
compressible two phase flow in CFX4.4  youngan  CFX  0  July 1, 2003 23:32 