[hsingtzu]

Hi

I followed the instruction at http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam to add temperature to icoFoam. I called the new solver "my_icoFoam." However, when I ran the solver, I got the following error message after t=0.195. I am wondering if anyone knows what they mean and how to solve this problem.Thanks!

#0  Foam::error::printStack(Foam::Ostream&) in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2  Uninterpreted: 
#3  Foam::PBiCG::solve(Foam::Field<double>&,  Foam::Field<double> const&, unsigned char) const in  "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#4  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in  "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#5  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
#6  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
#7  __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#8  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
Floating point exception

[chegdan]

What happened before the error message?

Floating point exception

getting this after a few successful iterations probably means that you were getting some really large numbers...hence causing the floating point exception. Make sure your time steps are scaled properly for Courant number (see the user's guide). However, without more information...I'm just guessing. If you post a log file or discuss the particular case in more detail, then more people will help. Good Luck.

Dan

[hsingtzu]

Thanks, chegdan.

by accident I lost the original code, so I redid it. and it did not work.
I decreased dt, and the courant number did decrease from

Time = 0.005

Courant Number mean: 7.1527 max: 5.99709e+298

to

Time = 5e-60

Courant Number mean: 7.1527e-57 max: 5.99709e+241

I was wondering if I should did some other change...

[chegdan]

Originally Posted by hsingtzu

Thanks, chegdan.

by accident I lost the original code, so I redid it. and it did not work.
I decreased dt, and the courant number did decrease from

Time = 0.005

Courant Number mean: 7.1527 max: 5.99709e+298

to

Time = 5e-60

Courant Number mean: 7.1527e-57 max: 5.99709e+241

I was wondering if I should did some other change...

What does your mesh look like? does it pass the checkMesh -allTopology -allGeometry utility? If you want to post your solver and case, I can take a quick look at it.

Dan

[hsingtzu]

Hello Daniel

Thanks for the quick reply

my blockMeshDict is

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.1;

vertices #codeStream
{
    codeInclude
    #{
        #include "pointField.H"
    #};

    code
    #{
        pointField points(19);
        points[0]  = point(0.5, 0, -133);
        points[1]  = point(1, 0, -133);
        points[2]  = point(2, 0, -133);
        points[3]  = point(2, 0.707107, -133);
        points[4]  = point(0.707107, 0.707107, -133);
        points[5]  = point(0.353553, 0.353553, -133);
        points[6]  = point(2, 2, -133);
        points[7]  = point(0.707107, 2, -133);
        points[8]  = point(0, 2, -133);
        points[9]  = point(0, 1, -133);
        points[10] = point(0, 0.5, -133);
        points[11] = point(-0.5, 0, -133);
        points[12] = point(-1, 0, -133);
        points[13] = point(-2, 0, -133);
        points[14] = point(-2, 0.707107, -133);
        points[15] = point(-0.707107, 0.707107, -133);
        points[16] = point(-0.353553, 0.353553, -133);
        points[17] = point(-2, 2, -133);
        points[18] = point(-0.707107, 2, -133);

        // Duplicate z points
        label sz = points.size();
        points.setSize(3*sz);
        for (label i = 0; i < sz; i++)
        {
            const point& pt = points[i];
            points[i+sz] = point(pt.x(), pt.y(), 0);
        }
        for (label i = 0; i < sz; i++)
        {
            const point& pt = points[i];
            points[i+sz+sz] = point(pt.x(), pt.y(), -pt.z());
        }
        os  << points;
    #};
};


blocks          
(
    hex (5 4 9 10 24 23 28 29) (10 10 1) simpleGrading (1 1 1)
    hex (0 1 4 5 19 20 23 24) (10 10 1) simpleGrading (1 1 1)
    hex (1 2 3 4 20 21 22 23) (20 10 1) simpleGrading (1 1 1)
    hex (4 3 6 7 23 22 25 26) (20 20 1) simpleGrading (1 1 1)
    hex (9 4 7 8 28 23 26 27) (10 20 1) simpleGrading (1 1 1)
    hex (15 16 10 9 34 35 29 28) (10 10 1) simpleGrading (1 1 1)
    hex (12 11 16 15 31 30 35 34) (10 10 1) simpleGrading (1 1 1)
    hex (13 12 15 14 32 31 34 33) (20 10 1) simpleGrading (1 1 1)
    hex (14 15 18 17 33 34 37 36) (20 20 1) simpleGrading (1 1 1)
    hex (15 9 8 18 34 28 27 37) (10 20 1) simpleGrading (1 1 1)
    hex (24 23 28 29 43 42 47 48) (10 10 1) simpleGrading (1 1 1)
     
);

edges           
(
    arc 0 5 (0.469846 0.17101 -0.5)
    arc 5 10 (0.17101 0.469846 -0.5)
    arc 1 4 (0.939693 0.34202 -0.5)
    arc 4 9 (0.34202 0.939693 -0.5)
    arc 19 24 (0.469846 0.17101 0.5)
    arc 24 29 (0.17101 0.469846 0.5)
    arc 20 23 (0.939693 0.34202 0.5)
    arc 23 28 (0.34202 0.939693 0.5)
    arc 11 16 (-0.469846 0.17101 -0.5)
    arc 16 10 (-0.17101 0.469846 -0.5)
    arc 12 15 (-0.939693 0.34202 -0.5)
    arc 15 9 (-0.34202 0.939693 -0.5)
    arc 30 35 (-0.469846 0.17101 0.5)
    arc 35 29 (-0.17101 0.469846 0.5)
    arc 31 34 (-0.939693 0.34202 0.5)
    arc 34 28 (-0.34202 0.939693 0.5)
);

boundary
(
    down
    {
//        type  patch;
        type symmetryPlane;
        faces
        (
            (0 1 20 19)
            (1 2 21 20)
            (12 11 30 31)
            (13 12 31 32)
        );
    }
    right
    {
//        type  symmetryPlane;
        type patch;
        faces
        (
            (2 3 22 21)
            (3 6 25 22)
        );
    }
    up
    {
//        type patch;
        type symmetryPlane;
        faces
        (
            (7 8 27 26)
            (6 7 26 25)
            (8 18 37 27)
            (18 17 36 37)
        );
    }
    left
    {
//        type symmetryPlane;
        type patch;
        faces
        (
            (14 13 32 33)
            (17 14 33 36)
        );
    }
    cylinder
    {
        type patch;
        faces
        (
            (10 5 24 29)
            (5 0 19 24)
            (16 10 29 35)
            (11 16 35 30)
        );
    }
);

mergePatchPairs
(
);

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

my 0/p is

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    down            
    {
        type            symmetryPlane;
    }

    right           
    {
        type            fixedValue;
        value           uniform 0;
    }

    up              
    {
        type            symmetryPlane;
    }

    left            
    {
        type            zeroGradient;
    }

    cylinder        
    {
        type            zeroGradient;
    }

    defaultFaces    
    {
        type            empty;
    }
}

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

my 0/U is

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (1 0 0); 

boundaryField
{
    down
    {
        type            symmetryPlane;
    }
    right
    {
        type            zeroGradient;
    }
    up
    {
        type            symmetryPlane;
    }
    left
    {
        type            fixedValue;
        value           uniform (1 0 0);
    }
    cylinder
    {
        type            zeroGradient;
    }
    defaultFaces
    {
        type            empty;
    }
}


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

and my 0/T is

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 300;

boundaryField
{
    down            
    {
        type            symmetryPlane;
    }

    right           
    {
        type            zeroGradient;
    }

    up              
    {
        type            symmetryPlane;
    }

    left            
    {
        type            zeroGradient;
    }

    cylinder        
    {
        type            fixedValue;
        value           uniform  400;
    }

    defaultFaces    
    {
        type            empty;
    }
}

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

I appreciate your time and help.

[chegdan]

hsingtzu,

I tried your case and there are several issues.
1. I rebuilt your mesh from the blockMeshDict you provided and it looks like the image below. is there something more that you do to create the mesh? you might want to try uploading your whole case to say dropbox (dropbox referral http://db.tt/hbaGBi5) and then post the link here when you put the case in the public folder on your dropbox

2. after running the checkMesh -allTopology -allGeometry command, I get some nasty messages.

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.0.x-5f38cb9e6919
Exec   : checkMesh -allTopology -allGeometry
Date   : Dec 01 2011
Time   : 11:42:32
Host   : aris
PID    : 3637
Case   : /home/dcombest/OpenFOAM/dcombest-2.0.x/run/myIcoFoam/case2
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           4343
    faces:            8430
    internal faces:   4170
    cells:            2100
    boundary patches: 6
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     2100
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
 ***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Topological cell zip-up check OK.
    Face-face connectivity OK.
  <<Writing 6 cells with with two non-boundary faces to set twoInternalFacesCells
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                   Bounding box
    down                60       124      ok (non-closed singly connected)   (-0.2 0 -13.3) (0.2 0 0)
    right               30       62       ok (non-closed singly connected)   (0.2 0 -13.3) (0.2 0.2 0)
    up                  60       122      ok (non-closed singly connected)   (-0.2 0.2 -13.3) (0.2 0.2 0)
    left                30       62       ok (non-closed singly connected)   (-0.2 0 -13.3) (-0.2 0.2 0)
    cylinder            40       82       ok (non-closed singly connected)   (-5.84259 -5.80624 -13.3) (5.84259 5.84259 0.0500826)
    defaultFaces        4040     4262     ok (non-closed singly connected)   (-5.86406 -5.80624 -13.3) (5.86406 5.86406 13.3)

Checking geometry...
    Overall domain bounding box (-5.86406 -5.80624 -13.3) (5.86406 5.86406 13.3)
    Mesh (non-empty, non-wedge) directions (0 0 0)
    Mesh (non-empty) directions (0 0 0)
 ***Number of edges not aligned with or perpendicular to non-empty directions: 5969
  <<Writing 2729 points on non-aligned edges to set nonAlignedEdges
    Boundary openness (4.18677e-19 1.23902e-16 -3.24945e-19) OK.
    Max cell openness = 3.4632e-14 OK.
    Max aspect ratio = 0 OK.
    Minumum face area = 1.85615e-05. Maximum face area = 25.9195.  Face area magnitudes OK.
    Min volume = 2e-300. Max volume = 0.033485.  Total volume = 5.34265.  Cell volumes OK.
    Mesh non-orthogonality Max: 180 average: 74.3256
   *Number of severely non-orthogonal faces: 738.
 ***Number of non-orthogonality errors: 1654.
  <<Writing 2392 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 4522 faces are incorrectly oriented.
  <<Writing 3090 faces with incorrect orientation to set wrongOrientedFaces
 ***Max skewness = 362.256, 1072 highly skew faces detected which may impair the quality of the results
  <<Writing 1072 skew faces to set skewFaces
    Coupled point location match (average 0) OK.
 ***Error in face tets: 8398 faces with low quality or negative volume decomposition tets.
  <<Writing 3508 faces with low quality or negative volume decomposition tets to set lowQualityTetFaces
    Min/max edge length = 0.00382683 13.3 OK.
   *There are 720 faces with concave angles between consecutive edges. Max concave angle = 90 degrees.
  <<Writing 720 faces with concave angles to set concaveFaces
    Face flatness (1 = flat, 0 = butterfly) : average = 0.99583  min = 0.227895
   *There are 46 faces with ratio between projected and actual area < 0.8
    Minimum ratio (minimum flatness, maximum warpage) = 0.227895
  <<Writing 46 warped faces to set warpedFaces
    Cell determinant (wellposedness) : minimum: 0 average: 7.25286e-07
 ***Cells with small determinant found, number of cells: 2100
  <<Writing 2100 under-determined cells to set underdeterminedCells
 ***Concave cells (using face planes) found, number of cells: 1010
  <<Writing 1010 concave cells to set concaveCells

Failed 7 mesh checks.

End

so right now, its a bad mesh. if you post your case completely with everything in it already...then I can just run it and use exactly what you have used. good luck

[mohsen cheraghi]

Hi
I think it returns to your BC. you used zero gradient boundary for velocity on the cylinder which should be fixedValue of (0 0 0) to provide obstruction.
But if you insist on using this BC for the cylinder you must change your solver to simpleFoam.

Good luck

[chegdan]

Originally Posted by mohsen cheraghi

Hi
I think it returns to your BC. you used zero gradient boundary for velocity on the cylinder which should be fixedValue of (0 0 0) to provide obstruction.
But if you insist on using this BC for the cylinder you must change your solver to simpleFoam.

Good luck

Good point!

Also, for walls in your geometry...the patch type in the blockMeshDict should be wall and not patch.
* By setting a zeroGradient for velocity at the cylinder patch with patch type "patch", it is creating an outflow condition (if that is what you wanted).
* For a no-slip boundary, you will need a fixedValue (like you have), but with a patch type of wall.

Hope this helps you.

[calim_cfd]

i'll flood the topic and ask u to work on the mesh quality. Can we have a look at your (desired) mesh?
tried ur dict and i got same pic as daniel

[hsingtzu]

Dear All

Thanks for all the comments. I should have double checked the geometry before copying it from OpenFOAM-2.0.1/run/tutorials/basic/potentialFoam/cylinder/constant/polyMesh. Actually I want to do my_icoFoam on model of "a cylinder inside a box" (please see the attached pic 1). I use the blockMeshDict from OpenFOAM-1.7.1 and it works.

However, when I try a 3D box with 16 cylinders (4x4) inside (please see the attached pic 2),it gives me the following error message. (I have tried dt=0.0005 and dt= 0.000005. Both give me error messages. the following is the one with dt =0.000005. I have replaced "patch" with "wall" and set the BC of cylinder as "fixedValue; uniform (0 0 0);")

Time = 0.005355

Courant Number mean: 6.61656e+94 max: 3.14367e+96
DILUPBiCG:  Solving for Ux, Initial residual = 0.99999, Final residual = 2.96883e-06, No Iterations 135
DILUPBiCG:  Solving for Uy, Initial residual = 0.999964, Final residual = 8.35209e-06, No Iterations 139
DILUPBiCG:  Solving for Uz, Initial residual = 0.99999, Final residual = 6.06657e-06, No Iterations 88
#0  Foam::error::printStack(Foam::Ostream&) in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2  Uninterpreted: 
#3  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#4  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#5  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
#6  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
#7  __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#8  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
Floating point exception

0/p can be found at http://dl.dropbox.com/u/20517550/4x4_3D/0/p
0/U can be found at http://dl.dropbox.com/u/20517550/4x4_3D/0/U
0/T can be found at http://dl.dropbox.com/u/20517550/4x4_3D/0/T
constant/polyMesh/boundary can be found at http://dl.dropbox.com/u/20517550/4x4...yMesh/boundary

please let me know if you would like to have access to some other files.


Thanks
Hsingtzu

[chegdan]

ok, starting to get somewhere.

1. you have some velocity inlets and those need to be type patch, outlets also need to be type patch instead of wall.

2. at pressure outlets, you need a fixedValue condition of type patch.

3. if you zip up everything in one directory and then provide the link to the zip file then we could try it.

4. I solve the same problem all the time with randomly packed cylinders http://www.personal.psu.edu/dab143/O...ombest2_ab.pdf

[calim_cfd]

Originally Posted by hsingtzu

Dear All

Thanks for all the comments. I should have double checked the geometry before copying it from OpenFOAM-2.0.1/run/tutorials/basic/potentialFoam/cylinder/constant/polyMesh. Actually I want to do my_icoFoam on model of "a cylinder inside a box" (please see the attached pic 1). I use the blockMeshDict from OpenFOAM-1.7.1 and it works.

However, when I try a 3D box with 16 cylinders (4x4) inside (please see the attached pic 2),it gives me the following error message. (I have tried dt=0.0005 and dt= 0.000005. Both give me error messages. the following is the one with dt =0.000005. I have replaced "patch" with "wall" and set the BC of cylinder as "fixedValue; uniform (0 0 0);")

Time = 0.005355

Courant Number mean: 6.61656e+94 max: 3.14367e+96
DILUPBiCG:  Solving for Ux, Initial residual = 0.99999, Final residual = 2.96883e-06, No Iterations 135
DILUPBiCG:  Solving for Uy, Initial residual = 0.999964, Final residual = 8.35209e-06, No Iterations 139
DILUPBiCG:  Solving for Uz, Initial residual = 0.99999, Final residual = 6.06657e-06, No Iterations 88
#0  Foam::error::printStack(Foam::Ostream&) in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2  Uninterpreted: 
#3  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#4  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/uiuc/OpenFOAM/uiuc-2.0.1/platforms/linuxGccDPOpt/lib/libfiniteVolume.so"
#5  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
#6  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
#7  __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#8  
 in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/my_icoFoam"
Floating point exception

0/p can be found at http://dl.dropbox.com/u/20517550/4x4_3D/0/p
0/U can be found at http://dl.dropbox.com/u/20517550/4x4_3D/0/U
0/T can be found at http://dl.dropbox.com/u/20517550/4x4_3D/0/T
constant/polyMesh/boundary can be found at http://dl.dropbox.com/u/20517550/4x4...yMesh/boundary

please let me know if you would like to have access to some other files.


Thanks
Hsingtzu

when i run transient cases i usually check my case with a steady-state solver. then if applicable, map the solution to the transient case.

also(then) try setting the initial step to sth rly low, and check the first occurrence of co number and make sure it is below 1. And make sure ur getting fixed time steps by setting runTimeModifiable=no;

startTime       0.0001;

stopAt          endTime;

endTime         10;

deltaT          0.00001;
...
runTimeModifiable no;

maxCo           1;

once u get things stable u can optimize the run..


hope it helps u get ur solver working..

[hsingtzu]

Dear calim_cfd and chegdan

Thanks for your comments. I really appreciate your time and help.
I am sorry for the late reply. I have been working on my final project which is due this Sun. This means that I will work on this problem next week.

[hsingtzu]

To Chegdan:

Thanks for your reply. I have changed the types of all boundary conditions to "patch".
You may find the file at http://dl.dropbox.com/u/20517550/4x4.zip
I appreciate your time and help.

To calim-cfd:

Thanks for your suggestions.

Hsingtzu

[chegdan]

Hsingtzu,

Ok..I glanced at the case file and you have some problems. You have an inlet velocity and then many outflow (zeroGradient) boundary conditions for the velocity field. If you are modeling the flow around bluff bodies then you need some no-slip (ie fixedValue ) boundary conditions in there as was suggested by mohsen. I have something running on my workstation so I can't switch over and try your case immediately. Good Luck.

Dan

[hsingtzu]

Thanks for your kind suggestion, Dan.
I should have paid attention to mohsen cheraghi's suggestion.

Have a nice weekend.
Hsingtzu

[hsingtzu]

Hi

I was trying to apply icoFoam to my model, but the courant # blew up at the first time step.

Time = 5e-05

Courant Number mean: 2.385e+286 max: 4.39836e+286

I had checked the mesh, and it looked fine. Even though I got a lot of warning messages when compiling it with "blockMesh", I had no idea where might be wrong. I also checked my boundary conditions according to the previous suggestions. You may find the file at
http://dl.dropbox.com/u/20517550/cell_3D.zip

and I would appreciate any help.

Thanks
Hsingtzu

[calim_cfd]

first notes

a checkMesh reports:

Checking geometry...
    Overall domain bounding box (-0.0063 -0.0063 0) (0.0063 0.0063 0.0098)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (3.40255e-17 -7.68602e-17 1.21815e-16) OK.
 ***High aspect ratio cells found, Max aspect ratio: 5.83792e+193, number of cells 5000
  <<Writing 5000 cells with high aspect ratio to set highAspectRatioCells
    Minumum face area = 7.11491e-08. Maximum face area = 1.53781e-06.  Face area magnitudes OK.
    Min volume = 2e-300. Max volume = 2e-300.  Total volume = 1e-296.  Cell volumes OK.
    Mesh non-orthogonality Max: 180 average: 170.484
 ***Number of non-orthogonality errors: 13600.
  <<Writing 13600 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 30000 faces are incorrectly oriented.
  <<Writing 16400 faces with incorrect orientation to set wrongOrientedFaces
    Max skewness = 0.548939 OK.
    Coupled point location match (average 0) OK.

so i'm not even sure your case will run. Plus the physics of your case is not properly set (you ziped case) ..

i can see the mesh in paraview and it doesnt look that bad.. maybe you need to review the ordering of faces in blockMeshDict

and if your mesh turns out still being bad then you'll need limited schemes and relaxation factors...

get your mesh right first.. i dont have time to debugg yout blockmeshdict sry

[hsingtzu]

Hi calim_cfd

Thanks for mentioning "checkMesh". I did not think about it. Now I am working on the face pyramids.
You mentioned that "the physics of your case is not properly set". Would you please give me some directions to work on? I used the cavity example of the official guide to make this model.

Thanks
Hsingtzu

[hsingtzu]

Then I solved the problem by giving up blockMesh thing and adopting gmsh.