CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Convergence problem.

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   May 29, 2012, 12:54
Default Convergence problem.
  #1
CRT
New Member
 
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 4
CRT is on a distinguished road
Hi

Iīm using the SimpleFoam and buoyantBoussinesqSimpleFoam.at the moment, I donīt consider the turbulence:
RASModel laminar;
turbulence off;
I think that the BC are well defined, so I donīt really understand why i have such a problem in steady case. It could be nice if someone can take a look, maybe you notice where is my mistake(s).

fvSolution
Code:
solvers
{
    p
    {
        solver          PCG;
        tolerance       1e-09;
        relTol          0.0001;
    maxIter        4000;
        preconditioner  DIC;
    }


    "(U|T|k|epsilon|R)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-09;
        relTol          0.0001;
    maxIter        3000;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;

    residualControl
    {
        p           1e-6;
        U               1e-6;
        T               1e-6;

        // possibly check turbulence fields
        "(k|epsilon|omega)" 1e-3;
    }
}

relaxationFactors
{
    fields
    {
        p          0.8;
    }
    equations
    {
        U               0.8;
        T               0.8;
        "(k|epsilon|R)" 0.8;
    }
}
fvSchemes
Code:
ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss upwind;
    div(phi,T)      Gauss upwind;
    div(phi,k)      Gauss upwind;
    div(phi,epsilon) Gauss upwind;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         none;
    laplacian(nuEff,U) Gauss linear corrected;
    laplacian((1|A(U)),p_rgh) Gauss linear corrected;
    laplacian((1|A(U)),p) Gauss linear corrected;
    laplacian(kappaEff,T) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DepsilonEff,epsilon) Gauss linear corrected;
    laplacian(DREff,R) Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p           ;
}
Thatīs the output of my calculations:
Code:
Selecting incompressible transport model Newtonian
Selecting RAS turbulence model laminar

SIMPLE: convergence criteria
    field p      tolerance 1e-06
    field U      tolerance 1e-06
    field T      tolerance 1e-06
    field "(k|epsilon|omega)"    tolerance 0.001


Starting time loop

Time = 1

DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 9.91822e-05, No Iterations 96
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 9.59855e-05, No Iterations 56
DILUPBiCG:  Solving for Uz, Initial residual = 1.75444e-06, Final residual = 9.82385e-10, No Iterations 43
DICPCG:  Solving for p, Initial residual = 1, Final residual = 9.80756e-05, No Iterations 2918
time step continuity errors : sum local = 8.99111e-06, global = -1.25301e-08, cumulative = -1.25301e-08
ExecutionTime = 306.68 s  ClockTime = 307 s

Time = 2

DILUPBiCG:  Solving for Ux, Initial residual = 0.935871, Final residual = 9.05429e-05, No Iterations 1863
DILUPBiCG:  Solving for Uy, Initial residual = 0.908349, Final residual = 32.7383, No Iterations 3001
DILUPBiCG:  Solving for Uz, Initial residual = 0.522177, Final residual = 0.0819383, No Iterations 3001
DICPCG:  Solving for p, Initial residual = 0.999559, Final residual = 9.96217e-05, No Iterations 3080                                      
time step continuity errors : sum local = 0.0493776, global = -3.04871e-06, cumulative = -3.06124e-06                                      
ExecutionTime = 2206.47 s  ClockTime = 2209 s 
                                                                                                                                     
Time = 3

DILUPBiCG:  Solving for Ux, Initial residual = 0.872234, Final residual = 291.137, No Iterations 3001                                                       
DILUPBiCG:  Solving for Uy, Initial residual = 0.946215, Final residual = 29.1615, No Iterations 3001
DILUPBiCG:  Solving for Uz, Initial residual = 0.981871, Final residual = 0.0162036, No Iterations 3001
DICPCG:  Solving for p, Initial residual = 0.999723, Final residual = 9.94861e-05, No Iterations 3442
time step continuity errors : sum local = 68.092, global = -0.0055498, cumulative = -0.00555286
ExecutionTime = 3928.84 s  ClockTime = 3932 s

Time = 4

DILUPBiCG:  Solving for Ux, Initial residual = 0.999816, Final residual = 0.0411844, No Iterations 3001
DILUPBiCG:  Solving for Uy, Initial residual = 0.999753, Final residual = 0.0675664, No Iterations 3001
DILUPBiCG:  Solving for Uz, Initial residual = 0.999209, Final residual = 0.0191083, No Iterations 3001
DICPCG:  Solving for p, Initial residual = 0.957101, Final residual = 0.000626641, No Iterations 4001
time step continuity errors : sum local = 70089.2, global = -0.784526, cumulative = -0.790079
ExecutionTime = 5648.58 s  ClockTime = 5652 s

Time = 5

DILUPBiCG:  Solving for Ux, Initial residual = 0.998547, Final residual = 656.787, No Iterations 3001
DILUPBiCG:  Solving for Uy, Initial residual = 0.998022, Final residual = 59.1156, No Iterations 3001
The residual start to grow up until the simulation crash.


Iīve been reading in the forum, and a lot of people recommend to use the GAMG preconditioner in order to calculate p, any suggestion?
increase the number of iterations and the relaxation factors? .

If you think that is necessary i could also show my BC files, I donīt do it know to avoid an excess of information.

Thanks a lot,
Carles
CRT is offline   Reply With Quote

Old   May 30, 2012, 03:07
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 133
Rep Power: 7
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Dear CRT,

I would change your relaxation factors to the settings below:
The settings you have seem a bit too hard for the solver. If it does not run then, maybe there is some other problem.

Cheers,
Tom

relaxationFactors { fields { p 0.3; } equations { U 0.7; T 0.5; "(k|epsilon|R)" 0.8; } }
tomf is offline   Reply With Quote

Old   May 31, 2012, 05:15
Default
  #3
CRT
New Member
 
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 4
CRT is on a distinguished road
Dear Tompf,

Thanks for your replay. I've changed the relaxation factors and it doesn't seem to change a lot.
What it seems to work is to use the GAMG solver for the pressure, and also whit some non-orthogonal correctors (5). Then the divergence problem appear just in the Ux, Uy, Uz and the time continuity error, but probably the last is a consequence of the velocity divergence, or?

Code:
Time = 18

DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.000990552, No Iterations 37
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.000665076, No Iterations 181
DILUPBiCG:  Solving for Uz, Initial residual = 0.993859, Final residual = 5.52181e+08, No Iterations 6001
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.000850571, No Iterations 15
GAMG:  Solving for p, Initial residual = 0.0560913, Final residual = 4.81741e-05, No Iterations 14
GAMG:  Solving for p, Initial residual = 0.00783873, Final residual = 7.67655e-06, No Iterations 14
GAMG:  Solving for p, Initial residual = 0.00219096, Final residual = 2.16098e-06, No Iterations 14
GAMG:  Solving for p, Initial residual = 0.000818089, Final residual = 6.0367e-07, No Iterations 13
GAMG:  Solving for p, Initial residual = 0.000324318, Final residual = 2.75583e-07, No Iterations 11
time step continuity errors : sum local = 8.54545e+92, global = -1.55141e+89, cumulative = -1.55007e+89
ExecutionTime = 27290.9 s  ClockTime = 27291 s

Time = 19

#0  Foam::error::printStack(Foam::Ostream&) in "/home/carles/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc45DPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/carles/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc45DPOpt/lib/libOpenFOAM.so"
#2   in "/lib64/libc.so.6"
#3  Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/carles/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc45DPOpt/lib/libOpenFOAM.so"
#4  
 in "/home/carles/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc45DPOpt/bin/simpleFoam"
#5  
 in "/home/carles/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc45DPOpt/bin/simpleFoam"
#6  
 in "/home/carles/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc45DPOpt/bin/simpleFoam"
#7  __libc_start_main in "/lib64/libc.so.6"
#8  
 at /usr/src/packages/BUILD/glibc-2.11.2/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception
Some users advice , itīs important to do somehow a initialization of the problem, such as:
1.
no convergence with simplefoam
Quote:
stawrogin
Hi,
if you are sure that your BCs are okay for U (you can check in paraview) I would try to stabilize the first iterations by using a cellLimited grad schemes and setting the relaxation factors for k and eps to 05. or 0.4
2.
Convergence problem using simpleFoam steady state
Quote:
hani
Initialize the flow as good as possible, set some relevant constant value for k and epsilon in the internal field. Use potentialFoam to initialize the velocity.

Use upwind scheme initially for U,k,epsilon, and later change to a better scheme.
Under-relax as proposed by Hrv.
Decrease the Reynolds number by increasing the viscosity or lower the velocity, and later change back to the real Reynolds number.

Use stabilizing boundary conditions. Typically a Dirichlet condition for the pressure at the outlet seems more stable than a Neumann bc. You can later try to switch back to the bc's you really want.
Is it possible? to make some changes during the calculation in the fvSchemes file and those will be take it into account by the solver?

Do someone know a good book, papers whatever that help me to understand a bite more about the different schemes that i can choose?

Any suggestion will be rally appreciated.

Thanks!
Carles
CRT is offline   Reply With Quote

Old   May 31, 2012, 05:33
Default
  #4
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 133
Rep Power: 7
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Dear Carles,

Well it seems like you problems do lie elsewhere. Did you check your mesh, running checkMesh? Does it look ok? If not, than I think you may need to look into your boundary conditions. I do not think the nonOrthogonalityCorrectors are necessary unless you have nonOrthogonality problems reported by checkMesh. Also in that case I would suggest you use the

Code:
Gauss linear limited 0.333
scheme for your laplacianSchemes.

I also do not think it is necessary to have a maxIter larger than the standard 1000. I usually only set it to a lower value if there is some instability in the first couple of iterations, just to speed up the entire process. Furthermore I would suggest in your fvSolution to just use a relTol of 0.01 for p and maybe just 0.1 for the other variables.

Than I think your numerics set-up should be ok, maybe only play around with lower relaxation factors for the first few iterations.

Yes, you can change stuff in the fvSystem/fvSolution file during runtime and it will be taken into account. The initialization may work, but it depends on the problem. First make sure your mesh and boundary conditions are ok, otherwise initialization won't do the trick.

So I would suggest to first run checkMesh and maybe check again your boundary conditions, before trying to change your numerics.

Good luck,
Tom
tomf is offline   Reply With Quote

Old   May 31, 2012, 10:13
Default
  #5
CRT
New Member
 
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 4
CRT is on a distinguished road
Dear Tom,

I think that the mesh is ok. The only prooblems that checkMesh report me is:
Code:
***Wedge patch frontAndBackPlanes_pos not planar. Point (0.268943 0.0632487 0.00275887) is not in patch plane by 8.66739e-07 meter.
About the non-orthogonality:
Code:
Mesh non-orthogonality Max: 25.1038 average: 4.18976
    Non-orthogonality check OK.
I will try your suggestions and let you know if it works.

Thanks,
Carles
CRT is offline   Reply With Quote

Old   May 31, 2012, 10:29
Default
  #6
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 133
Rep Power: 7
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Dear Carles,

Ah so it is an axis-symmetrical case. How many cells does it have? Not a lot I would guess? Could you maybe post your entire checkMesh result and your boundary conditions for U and p? Also a picture of your geometry (preferably showing the mesh) would help a lot.

Regards,
Tom
tomf is offline   Reply With Quote

Old   May 31, 2012, 11:54
Default
  #7
CRT
New Member
 
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 4
CRT is on a distinguished road
Dear Tom,

Of course I can,

checkMesh
Code:
Mesh stats
    points:           1813894
    internal points:  0
    faces:            3608735
    internal faces:   1784797
    cells:            900880
    boundary patches: 5
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     889132
    prisms:        11748
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing 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                  
    WALL                22104    44211    ok (non-closed singly connected)  
    INLET               64       129      ok (non-closed singly connected)  
    GAPTOP              10       22       ok (non-closed singly connected)  
    frontAndBackPlanes_pos900880   907814   ok (non-closed singly connected)  
    frontAndBackPlanes_neg900880   907814   ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 0 -0.00396936) (0.38 0.091 0.00396936)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 1)
    Wedge frontAndBackPlanes_pos with angle 2.49531 degrees
 ***Wedge patch frontAndBackPlanes_pos not planar. Point (0.268943 0.0632487 0.00275887) is not in patch plane by 8.66739e-07 meter.
    Boundary openness (-2.32202e-17 -9.25979e-15 2.14019e-14) OK.
    Max cell openness = 3.31318e-16 OK.
    Max aspect ratio = 4.02019 OK.
    Minumum face area = 1.74478e-09. Maximum face area = 3.16415e-06.  Face area magnitudes OK.
    Min volume = 3.8192e-13. Max volume = 9.20786e-10.  Total volume = 0.000124784.  Cell volumes OK.
    Mesh non-orthogonality Max: 25.1038 average: 4.18976
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.621888 OK.
    Coupled point location match (average 0) OK.

Failed 1 mesh checks.
p file - 0 folder
Code:
dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    WALL
    {
        type            zeroGradient;
    }
    INLET
    {
        type            zeroGradient;
    }
    GAPTOP
    {
        type            fixedValue;
        value           uniform 0;
    }
    frontAndBackPlanes_pos
    {
        type            wedge;
    }
    frontAndBackPlanes_neg
    {
        type            wedge;
    }

}
U file - 0 folder

Code:
dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    WALL
    {
    type            fixedValue;
        value           uniform (0 0 0);
    }
    INLET
    {
        type            timeVaryingMappedFixedValue;
        setAverage      off;
    }
    GAPTOP
    {
        type            zeroGradient;
    }
    frontAndBackPlanes_pos
    {
    type            wedge;
    }
    frontAndBackPlanes_neg
    {
    type            wedge;
    }
}
U file - boundarydata folder

Code:
// Average
(0 0 0)

// Data on points
80
(
(    0.091885373    0    0    )
(    0.091700472    0    0    )
(    0.09133745    0    0    )
(    0.090811901    0    0    )
(    0.090139844    0    0    )
(    0.089339107    0    0    )
(    0.088429593    0    0    )
(    0.087431565    0    0    )
(    0.086365201    0    0    )
(    0.085249819    0    0    )
(    0.084103227    0    0    )
(    0.082941331    0    0    )
(    0.081778221    0    0    )
(    0.080625713    0    0    )
(    0.079493508    0    0    )
(    0.078389108    0    0    )
(    0.077317581    0    0    )
(    0.076281399    0    0    )
(    0.075279854    0    0    )
(    0.074308395    0    0    )
(    0.073357597    0    0    )
(    0.072411761    0    0    )
(    0.071447313    0    0    )
(    0.07043115    0    0    )
(    0.069319129    0    0    )
(    0.068055138    0    0    )
(    0.066571429    0    0    )
(    0.064790532    0    0    )
(    0.062629394    0    0    )
(    0.060005635    0    0    )
(    0.056845449    0    0    )
(    0.053092379    0    0    )
(    0.04871482    0    0    )
(    0.043710824    0    0    )
(    0.038109064    0    0    )
(    0.031965468    0    0    )
(    0.025357356    0    0    )
(    0.018376643    0    0    )
(    0.011126214    0    0    )
(    0.0037204318    0    0    )
(    0.091885373    0    0    )
(    0.091700472    0    0    )
(    0.09133745    0    0    )
(    0.090811901    0    0    )
(    0.090139844    0    0    )
(    0.089339107    0    0    )
(    0.088429593    0    0    )
(    0.087431565    0    0    )
(    0.086365201    0    0    )
(    0.085249819    0    0    )
(    0.084103227    0    0    )
(    0.082941331    0    0    )
(    0.081778221    0    0    )
(    0.080625713    0    0    )
(    0.079493508    0    0    )
(    0.078389108    0    0    )
(    0.077317581    0    0    )
(    0.076281399    0    0    )
(    0.075279854    0    0    )
(    0.074308395    0    0    )
(    0.073357597    0    0    )
(    0.072411761    0    0    )
(    0.071447313    0    0    )
(    0.07043115    0    0    )
(    0.069319129    0    0    )
(    0.068055138    0    0    )
(    0.066571429    0    0    )
(    0.064790532    0    0    )
(    0.062629394    0    0    )
(    0.060005635    0    0    )
(    0.056845449    0    0    )
(    0.053092379    0    0    )
(    0.04871482    0    0    )
(    0.043710824    0    0    )
(    0.038109064    0    0    )
(    0.031965468    0    0    )
(    0.025357356    0    0    )
(    0.018376643    0    0    )
(    0.011126214    0    0    )
(    0.0037204318    0    0    )
)
Attached Images
File Type: jpg meshwithinpipe.jpg (94.2 KB, 25 views)
File Type: jpg mesh.jpg (98.1 KB, 33 views)
File Type: jpg outletpipe.jpg (98.3 KB, 24 views)
CRT is offline   Reply With Quote

Old   May 31, 2012, 11:57
Default
  #8
CRT
New Member
 
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 4
CRT is on a distinguished road
And some screen shots.
Attached Images
File Type: jpg 1.jpg (97.4 KB, 32 views)
File Type: jpg ggeo.jpg (33.4 KB, 24 views)
File Type: jpg inlet.jpg (75.6 KB, 20 views)
File Type: jpg inletpipe.jpg (95.6 KB, 24 views)
File Type: jpg outletpipe.jpg (98.3 KB, 20 views)
CRT is offline   Reply With Quote

Old   May 31, 2012, 12:22
Default
  #9
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 133
Rep Power: 7
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Carles,

I am wondering a bit about the problem you are trying to solve. If I read your checkMesh file correctly you have a patch GAPTOP that has only 10 faces and it seems from your boundary conditions you want to set this as your outlet. From the pictures I can't really tell what way the flow is meant to go. I think you specify an inlet at the bottom left, but I do not see where the outlet is exactly and also I do not see a patch of only 10 faces. Are you sure that this GAPTOP patch is defined correctly?

I think you may want to try to first perform a simulation with a fixed inflow value instead of the mapped one, and maybe generate a coarser mesh to find the correct setup for your problem. If that is found gradually increase the complexity of the simulation until you achieve the correct simulation.

I won't be near a computer next couple of days, so I hope you can work out your problem, of someone else can help you.

Cheers,
Tom
tomf is offline   Reply With Quote

Old   June 1, 2012, 07:47
Default
  #10
CRT
New Member
 
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 4
CRT is on a distinguished road
Hi Tom,

Yes you're right about the inlet. itīs at the bottom left. The outlet is located at the top right, I forget to attach a picture.

Quote:
I think you may want to try to first perform a simulation with a fixed inflow value instead of the mapped one, and maybe generate a coarser mesh to find the correct setup for your problem. If that is found gradually increase the complexity of the simulation until you achieve the correct simulation.
I will try, but I think itīs well defined. Itīs good to know that this mesh-geometry works in fluent. However i canīt get a solution with OpenFoam. Letīs see if a can find out whatīs wrong.

Thanks for your time!!

greetings,
carles
Attached Images
File Type: jpg outlet.jpg (74.5 KB, 14 views)
CRT is offline   Reply With Quote

Old   June 26, 2012, 05:54
Default
  #11
CRT
New Member
 
Carles
Join Date: Jan 2012
Location: Karlsruhe
Posts: 29
Rep Power: 4
CRT is on a distinguished road
I could find a solution, the problem was in the fvSolution file. Now iīm using this settings:

Code:
solvers
{ 
    p_rgh
    {
        solver           GAMG;
        tolerance        1e-12;
        relTol           0.001;
        minIter          5;
        maxIter          200;
        smoother         GaussSeidel; // DIC; //DICGaussSeidel; //FDIC;
        nPreSweeps       1;
        nPostSweeps      3;
        nFinestSweeps    3;
        scaleCorrection true;
        directSolveCoarsest false;
        cacheAgglomeration on;
        nCellsInCoarsestLevel 50;    // 500
        agglomerator     faceAreaPair;
        mergeLevels      1;    // 3
    }
    U
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-09;
        relTol          0.1;
    }
    k
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-09;
        relTol          0.1;
    }
    epsilon
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-09;
        relTol          0.1;
    }
    R
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-09;
        relTol          0.1;
    }
    T
    {
        solver          PBiCG;
        preconditioner  DILU;
        minIter          400;
        tolerance       1e-09;
        relTol          0.1;
    }
}


SIMPLE
{
    nNonOrthogonalCorrectors 1;
}

relaxationFactors
{
    p_rgh           0.7;
    U               0.7;
    k               0.7;
    epsilon         0.7;
    R               0.7;
    T                0.7;
}
CRT is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
convergence problem when use pisoFoam, LES for wind tunnel case Forrest_Lei OpenFOAM 3 July 19, 2011 06:00
convergence problem commonyue Main CFD Forum 1 December 1, 2009 03:54
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
3D Fluid Flow Convergence problem Emily FLUENT 2 March 21, 2007 23:18
Non Convergence of 3D Heat transfer cfd problem Balraj Main CFD Forum 3 December 9, 2004 00:24


All times are GMT -4. The time now is 22:04.