CFD Online Discussion Forums - convergence problem in using incompressible transient solvers.

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - convergence problem in using incompressible transient solvers. (https://www.cfd-online.com/Forums/openfoam-solving/94642-convergence-problem-using-incompressible-transient-solvers.html)

convergence problem in using incompressible transient solvers.

Dear Foarmers,

Hello, I'd like to simulate the 3D half-wing which is mounted on the symmetry plane.

Recently, I applied pisoFoam and pimpleFoam to get the unsteady solutions but the solutions have been diverged.

I tried to apply those solvers with lower tolerance criteria, various solver types and schemes but they generally weren't helpful at all.

Please give me an advice on using the transient solvers.

Here I attached the control, fvSolution and fvSchemes files recently used.

controlDict :

Code:

  1 /*--------------------------------*- C++ -*----------------------------------*\

  2 | =========                 |                                                 |

  3 | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

  4 |  \\    /   O peration     | Version:  1.7.1                                 |

  5 |   \\  /    A nd           | Web:      www.OpenFOAM.com                      |

  6 |    \\/     M anipulation  |                                                 |

  7 \*---------------------------------------------------------------------------*/

  8 FoamFile

  9 {

 10     version     2.0;

 11     format      ascii;

 12     class       dictionary;

 13     location    "system";

 14     object      controlDict;

 15 }

 16 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

 17 

 18 //application     simpleFoam;

 19   application     pimpleFoam;

 20 //application     pisoFoam;

 21 

 22 startFrom       latestTime;

 23 

 24 startTime       0;

 25 

 26 stopAt          endTime;

 27 

 28 endTime         200;

 29 

 30 deltaT          1e-5;

 31 

 32 writeControl    timeStep;

 33 

 34 writeInterval   100;

 35 

 36 purgeWrite      0;

 37 

 38 writeFormat     ascii;

 39 

 40 writePrecision  6;

 41 

 42 writeCompression uncompressed;

 43 

 44 timeFormat      general;

 45 

 46 timePrecision   6;

 47 

 48 runTimeModifiable yes;

 49 

 50 adjustTimeStep yes;

 51 

 52 maxCo 5;

 53 

 54 functions

 55 {

 56         forces

 57         {

 58                 type            forceCoeffs;

 59                 functionObjectLibs      ( "libforces.so" );

 60                 outputControl           timeStep;

 61                 outputInterval          1;

 62                 patches         ( wing flap );

 63                 rhoName         rhoInf;

 64                 log             true;

 65                 rhoInf          1.225;

 66                 CofR            ( 45.89 0 0 );

 67                 liftDir         ( 0 1 0 );

 68                 dragDir         ( 1 0 0 );

 69                 pitchAxis       ( 0 0 1 );      // PITCH

 70                 magUInf         2;

 71                 lRef            53.97;

 72                 Aref            3006.1;

 73         }

 74 }

 75 

 76 

 77 // ************************************************************************* //

fvSolution :

Code:

  1 /*--------------------------------*- C++ -*----------------------------------*\

  2 | =========                 |                                                 |

  3 | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

  4 |  \\    /   O peration     | Version:  1.7.1                                 |

  5 |   \\  /    A nd           | Web:      www.OpenFOAM.com                      |

  6 |    \\/     M anipulation  |                                                 |

  7 \*---------------------------------------------------------------------------*/

  8 FoamFile

  9 {

 10     version     2.0;

 11     format      ascii;

 12     class       dictionary;

 13     object      fvSolution;

 14 }

 15 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

 16 

 17 solvers

 18 {

 19     p

 20     {

 21                 solver                  GAMG;

 22                 tolerance               1e-07;

 23                 relTol                  0.001;

 24                 smoother                GaussSeidel;

 25                 cacheAgglomeration      true;

 26                 nCellsInCoarsestLevel   10;

 27                 agglomerator            faceAreaPair;

 28                 mergeLevels             1;

 29     };

 30 

 31     pFinal

 32     {

 33                 solver                  GAMG;

 34                 tolerance               1e-07;

 35                 relTol                  0.001;

 36                 smoother                GaussSeidel;

 37                 cacheAgglomeration      true;

 38                 nCellsInCoarsestLevel   10;

 39                 agglomerator            faceAreaPair;

 40                 mergeLevels             1;

 41     };

 42 

 43     U

 44     {

 45                 solver                  PBiCG;

 46                 preconditioner  DILU;

 47                 tolerance               1e-08;

 48                 relTol                  0;

 49     };

 50 

 51     UFinal

 52     {

 53                 solver                  PBiCG;

 54                 preconditioner  DILU;

 55                 tolerance               1e-08;

 56                 relTol                  0;

 57     };

 58 

 59     k

 60     {

 61                 solver                  PBiCG;

 62                 preconditioner  DILU;

 63                 tolerance               1e-08;

 64                 relTol                  0;

 65     };

 66 

 67     omega

 68     {

 69                 solver                  PBiCG;

 70                 preconditioner  DILU;

 71                 tolerance               1e-08;

 72                 relTol                  0;

 73     };

 74 }

 75 

 76 SIMPLE

 77 {

 78     nNonOrthogonalCorrectors 1;

 79     pRefCell        0;

 80     pRefValue       0;

 81 }

 82 

 83 PISO

 84 {

 85         nCorrectors 5;

 86     nNonOrthogonalCorrectors 0;

 87     pRefCell        0;

 88     pRefValue       0;

 89 }

 90 

 91 PIMPLE

 92 {

 93         nOuterCorrectors 10;

 94         nCorrectors 2;

 95         nNonOrthogonalCorrectors 0;

 96     pRefCell        0;

 97     pRefValue       0;

 98 }

 99 

100 relaxationFactors

101 {

102     U           1;

103     k           1;

104     omega       1;

105 //  p  0.01;

106 //  U  0.1;

107 //  k  0.1;

108 //  omega 0.1;

109 }

110 

111 // ************************************************************************* //

fvSchemes :

Code:

  1 /*--------------------------------*- C++ -*----------------------------------*\

  2 | =========                 |                                                 |

  3 | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

  4 |  \\    /   O peration     | Version:  1.7.1                                 |

  5 |   \\  /    A nd           | Web:      www.OpenFOAM.com                      |

  6 |    \\/     M anipulation  |                                                 |

  7 \*---------------------------------------------------------------------------*/

  8 FoamFile

  9 {

 10     version     2.0;

 11     format      ascii;

 12     class       dictionary;

 13     object      fvSchemes;

 14 }

 15 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

 16 

 17 ddtSchemes

 18 {

 19 //      default steadyState;

 20 //      default         CrankNicholson 0.5;

 21 //      default backward;

 22         default Euler;

 23 }

 24 

 25 gradSchemes

 26 {

 27     default         Gauss linear;

 28     grad(p)         Gauss linear;

 29     grad(U)         Gauss linear;

 30 //    grad(U)         cellLimited Gauss linear 1;

 31 }

 32 

 33 divSchemes

 34 {

 35     default         Gauss upwind;

 36 //  div(phi,U)      Gauss linearUpwindV Gauss linear;

 37 //  div(phi,k)      Gauss linearUpwind Gauss linear;

 38 //  div(phi,omega)  Gauss linearUpwind Gauss linear;

 39     div((nuEff*dev(grad(U).T()))) Gauss linear;

 40 }

 41 

 42 laplacianSchemes

 43 {

 44     default         Gauss linear corrected;

 45 //  default         Gauss linear limited 0.5;

 46 //  default         Gauss linear limited 0.333;

 47 }

 48 

 49 interpolationSchemes

 50 {

 51     default         linear;

 52     interpolate(U)  linear;

 53 }

 54 

 55 snGradSchemes

 56 {

 57     default         corrected;

 58 }

 59 

 60 fluxRequired

 61 {

 62     default         no;

 63     p;

 64 }

 65 

 66 // ************************************************************************* //

Regards,
Geon-Hong.

Your maximum Courant number is 5, too high. Set it to something less than 1.

Dear alberto,

Thanks for your reply.

Of course I tried lower value of Courant number, which was set to be 0.5 or unity. However the problem was the same.

Regards,
Geon-Hong.

One possible reason is a mistake in BC's,

To investigate this, I am looking for examples and using their BC's... Or I am looking in the log file what is the diverging variable and trying to find the error there.

Another approach is to try to simplify the case. Start from a working example and add feature after feature... and when you will know the step which is causing your troubles you can deal with it.

Martin.

Dear Holecek,

Thank you for your reply.

I tried other boundary conditions which are used in tutorial cases.

Still it doesn't work at all.

By the way, what log file should I check?

Thank you very much.

Regards,
Geon-Hong.

Did you check the mesh for problems (checkMesh)?

Dear Alberto,

Of course I did.

However, there is a awkward thing that,

High aspect ratio cells found

and

Failed 1 mesh checks.

But I can't find what is problem. The checkMesh result is as below,

Code:

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  1.7.1                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : 1.7.1-03e7e056c215

Exec   : checkMesh

Date   : Nov 24 2011

Time   : 14:03:27

Host   : adlc11

PID    : 10513

Case   : /home/users/kgb/Work/flap/ucav1303/flap10c10b975p

nProcs : 1

SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

 

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time

 

Create polyMesh for time = 0

 

Time = 0

 

Mesh stats

    points:           6933336

    faces:            20575358

    internal faces:   20351362

    cells:            6821120

    boundary patches: 8

    point zones:      0

    face zones:       1

    cell zones:       1

 

Overall number of cells of each type:

    hexahedra:     6821120

    prisms:        0

    wedges:        0

    pyramids:      0

    tet wedges:    0

    tetrahedra:    0

    polyhedra:     0

 

Checking topology...

    Boundary definition OK.

    Point usage OK.

    Upper triangular ordering OK.

    Face vertices OK.

    Number of regions: 1 (OK).

 

Checking patch topology for multiply connected surfaces ...

    Patch               Faces    Points   Surface topology                  

    flap                6172     6174     ok (closed singly connected)      

    bottom              20060    20382    ok (non-closed singly connected)  

    top                 20060    20382    ok (non-closed singly connected)  

    side                29244    29508    ok (non-closed singly connected)  

    outflow             36816    37209    ok (non-closed singly connected)  

    inflow              47200    47637    ok (non-closed singly connected)  

    symPlane            28860    29223    ok (non-closed singly connected)  

    wing                35584    35685    ok (non-closed singly connected)  

 

Checking geometry...

    Overall domain bounding box (-247.502 -270 0) (900 270 358.535)

    Mesh (non-empty, non-wedge) directions (1 1 1)

    Mesh (non-empty) directions (1 1 1)

    Boundary openness (-1.03703e-16 1.14641e-15 -2.58996e-15) OK.

 ***High aspect ratio cells found, Max aspect ratio: 13183.7, number of cells 260418

  <<Writing 260418 cells with high aspect ratio to set highAspectRatioCells

    Minumum face area = 5.15158e-07. Maximum face area = 2886.02.  Face area magnitudes OK.

    Min volume = 4.04901e-08. Max volume = 71036.  Total volume = 1.94209e+08.  Cell volumes OK.

    Mesh non-orthogonality Max: 89.7243 average: 28.048

   *Number of severely non-orthogonal faces: 767159.

    Non-orthogonality check OK.

  <<Writing 767159 non-orthogonal faces to set nonOrthoFaces

    Face pyramids OK.

    Max skewness = 2.69123 OK.

 

Failed 1 mesh checks.

 

End

It seems you have 260418 cells with high aspect ratio, and at least one of them has an aspect ratio of 13183.7, which is extremely high.

Code:

***High aspect ratio cells found, Max aspect ratio: 13183.7, number of cells 260418   <<Writing 260418 cells with high aspect ratio to set highAspectRatioCells

The checkMesh utility should write a file listing the affected cells.

checkMesh results

Dear Alberto,

Yes, I checked the high aspect ratio cells from the file highAspectRatioCells in constant/polyMesh/sets.

What can I do with this cell-set? Is there any way to improve this problem?

I guess those high-aspect-ratio cells are generated from the cells adjacent to the wall.

The wing I want to simulate is tapered, which means that the wing tip has smaller chord length than the root. Furthermore, I generated the structured grid over the wing. Thus the wing has the same number of grid points along the chord at both wing tip and root. This might cause such problems, I guess.

Regeneration of the grid is only hope? ToT

Quote:

Originally Posted by Geon-Hong (Post 333371)

Regeneration of the grid is only hope? ToT

What program did you use to generate the geometry as well as the grid?
It seems that you would have to regenerate the grid. If you have done it with sHM - it will not take you too long ^^

about grid problems

I've noticed just before that the problems have been occurred far from the wing, not adjacent to the wing.

The problem is that the grid has been generated in structured manner and the grid size along in the downstream was stretched while thin layer of grid for resolving the boundary layer near the wall is maintained.

Now I am considering a hybrid grid arrangement : structured near the wall and unstructured at far field.

Rob / I used gambit to generate the grid. Now I'd like to try Ansys instead. I have no idea about sHM. What is it?

One more thing that I'd like to mention is that I ran the same case(mesh) with the FLUENT but it provided converged transient solution. At least, FLUENT may provide a transient solution though the mesh have extremely high aspect ratio cells which have order of 1e4 as my case.

From following thread, Mads Reck also referred that

aspect ratios of more than 1000 is by no means insane - we have it in airfoil aerodynamics all the time - and on wind turbine blades.

Aspect ratios of 1e5 or even higher is usual business when you want to have a first cell height of around 1e-6 chordLengths.

http://www.cfd-online.com/Forums/ope...e-comment.html

I hope to resolve this problem as soon as possible.

Quote:

Originally Posted by Geon-Hong (Post 333403)

Fluent starccm+ etc apply lots of tricks (trade secrets) to keep solver stable. The main difficulty with high respect ratio is that it makes pressure correction equation very difficult to converge, which could make solver unstable.
OpenFOAM does not apply such tricks so things should be more difficult with it. For this reason you would need good quality meshes with openFOAM.

Hi,

You have some cells with high nonorthogonality (90 starts to be a high value imo). You should used "limited 0,333" schemes and not "corrected" schemes (snGrad).
I don't know if it would solve your problem, but it should be a start.

Aurelien