[dnsuman]

I am new to OpenFoam. I am trying to simulate flow over an aircraft fuselage at Re=36000000. I have created my mesh in ansys meshing using cutcell method with inflation layers and y+ ~ 30 and imported it in Openfoam. I am using k omega SST model and I have specified all boundary conditions to the best of my knowledge. I am using simpleFoam as the solver. The solution does not converge and I am getting completely wrong results. I am pasting my case files below. Can someone please take a look and tell me where the problem is? Any help would be greatly appreciated.



K

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

internalField   uniform 18.37479;

boundaryField
{
    inlet
    {
      type            fixedValue;
      value          uniform 18.37479;
    }

    outlet
    {
      type            zeroGradient;
    }
    wall
    {
        type            zeroGradient;
    }
    fuselage
    {
        type            kqRWallFunction;
    value        uniform 18.37479;
    }
    symmetry
    {
        type            symmetry;
    }
}

nut

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 1.6496e-5;

boundaryField
{
    inlet
    {
        type            freestream;
        freestreamValue uniform 1.6496e-5;
    }

    outlet
    {
        type            freestream;
        freestreamValue uniform 1.6496e-5;
    }

    wall
    {
        type            nutkWallFunction;
        value           uniform 1.6496e-5;
    }

    fuselage
    {
        type            nutkWallFunction;
        value           uniform 1.6496e-5;
    }

    symmetry
    {
        type            symmetry;
    }
}

omega

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

internalField   uniform 5.4941;

boundaryField
{
    inlet
    {
      type            fixedValue;
      value          uniform 5.4941;
    }

    outlet
    {
      type            zeroGradient;
    }  
  
    wall
    {
        type            zeroGradient;
    }

    fuselage
    {
        type            omegaWallFunction;
    value        uniform 5.4941;
    }

    symmetry
    {
        type            symmetry;
    }
}

p

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

internalField   uniform 0;

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }
    outlet
    {
        type            freestreamPressure;
        freestreamValue $internalField;
    }

    wall
    {
        type            zeroGradient;
    }

    fuselage
    {
        type            zeroGradient;
    }

    symmetry
    {
        type            symmetry;
    }
}

U

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

internalField   uniform (70 0 0);

boundaryField
{
    inlet
    {
        type            freestreamVelocity;
        freestreamValue $internalField;
    }

    outlet
    {
        type            zeroGradient;
    }

    wall
    {
        type            slip;
    }

    fuselage
    {
        type            noSlip;
    }

    symmetry
    {
        type            symmetry;
    }
}

fvSolution

solvers
{
    p
    {
        solver             GAMG;
        tolerance         1e-10;
        relTol             0.01;
        smoother         GaussSeidel;
        nPreSweeps         0;
        nPostSweeps     2;
        cacheAgglomeration on;
        agglomerator faceAreaPair;
        nCellsInCoarsestLevel 120;
        mergeLevels     1;
        maxIter            500;
    }

    U
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-8;
        relTol          0.1;
        nSweeps         1;
    }

    k
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-8;
        relTol          0.1;
        nSweeps         1;
    }

    omega
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-8;
        relTol          0.1;
        nSweeps         1;
    }

}

SIMPLE
{       
    nNonOrthogonalCorrectors 3;
    nCorrectors 1; 
}

potentialFlow
{
    nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
    fields
    {
        p               0.2;
    }    
    equations
    {
        U               0.5;
        k               0.5;
        omega           0.5;
    }
}

cache
{
    grad(U);
}

fvSchemes

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         cellMDLimited Gauss linear 0.5;
    grad(U)         Gauss linear;
}

divSchemes
{
    default         none;

    div(phi,U)      bounded Gauss linearUpwind grad(U);
    div(phi,k)      bounded Gauss upwind;
    div(phi,omega)  bounded Gauss upwind;
    div((nuEff*dev2(T(grad(U))))) Gauss linear;

}


laplacianSchemes
{
    default         Gauss linear uncorrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default no;
    p;
}

wallDist
{
    method meshWave;
} 


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

ControlDict

application     simpleFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         1000;

deltaT          1;

writeControl    timeStep;

writeInterval   50;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

functions
{
    forces
    {
        type            forceCoeffs;
        libs            ("libforces.so");
        writeControl    writeTime;

        patches
        (
            fuselage
        );

    rho        rhoInf;
        rhoInf      1.0556;

        CofR        (0.4127 0 0);
        liftDir     (0 0 1);
        dragDir     (1 0 0);
        pitchAxis   (0 1 0);
        magUInf     70;
        lRef        8.669;
        Aref        5.01095;
    }
}

Please let me know where the problem is.

[mAlletto]

did you run checkMesh to check if the quality of your mesh is Ok? Can you post snapshot of you mesh. I had the experience that if there are a lot of thetrahedra in the mesh you use openfoam has convergence problems

[mAlletto]

by the way are you sure you want to use an incompressible solver for an inflow velocity of 70m/s. I would guess that in some parts of your domain you will reach velocities where the Ma number is above the limit where the flow can be regarded as incompressible

[dnsuman]

Hi

I have attached the snapshot of the mesh and after giving the check mesh I have got

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : 7-6ef561967074
Exec   : checkMesh
Date   : Nov 28 2019
Time   : 10:12:13
Host   : "freedom"
PID    : 4545
I/O    : uncollated
Case   : /home/leapaero/OpenFOAM/leapaero-7/run/tutorials/incompressible/simpleFoam/fuselage
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

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

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           1854705
    faces:            5569374
    internal faces:   5433716
    cells:            1853250
    faces per cell:   5.93719
    boundary patches: 5
    point zones:      0
    face zones:       1
    cell zones:       1

Overall number of cells of each type:
    hexahedra:     1614876
    prisms:        192058
    wedges:        0
    pyramids:      4933
    tet wedges:    16
    tetrahedra:    5274
    polyhedra:     36093
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            5   252
            6   8929
            7   7546
            8   291
            9   12017
           10   83
           11   255
           12   4974
           13   9
           15   1710
           18   25
           21   2

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
                fuselage    41276    33202  ok (non-closed singly connected)
                   inlet     5202     5356  ok (non-closed singly connected)
                    wall    41616    42025  ok (non-closed singly connected)
                symmetry    42362    43443  ok (non-closed singly connected)
                  outlet     5202     5356  ok (non-closed singly connected)

Checking geometry...
    Overall domain bounding box (-130 -0.000285276 -65) (130 65 65)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (7.31581e-16 4.9481e-15 -8.75319e-16) OK.
    Max cell openness = 5.31195e-15 OK.
    Max aspect ratio = 185.675 OK.
    Minimum face area = 1.22156e-06. Maximum face area = 1.62551.  Face area magnitudes OK.
    Min volume = 7.9565e-09. Max volume = 2.07182.  Total volume = 2.197e+06.  Cell volumes OK.
    Mesh non-orthogonality Max: 82.2994 average: 6.16104
   *Number of severely non-orthogonal (> 70 degrees) faces: 445.
    Non-orthogonality check OK.
  <<Writing 445 non-orthogonal faces to set nonOrthoFaces
    Face pyramids OK.
    Max skewness = 2.57593 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

Also I had not thought about the mach number limit thanks for reminding about that but would you be able to help me out in terms of setting the case for compressible or any inputs that would help me a lot.


Thank You

[dnsuman]

Also after around a 150 iterations the solution used to give a error and i suspect the mesh would be the reason for that error

[mAlletto]

The mesh seems ok. Did you try to write out the solution a few iterations before it converges. This may give you a hint what's going wrong

[mAlletto]

Why do you use so many non orthogonal correctors. The mesh quantity does non require this from my experience

[dnsuman]

Should I set both of the non orthogonal correctors to 0 one in potential flow and SIMPLE and try running the case?

[mAlletto]

Only for simple. For potentialflow it is fine since I assume you use potentialfoam to initialize the flow field

[dnsuman]

Sure thank you I'll run the case and post the updates

[dnsuman]

I made the non orthogonal correctors 0 and ran the simulation please go through the logs attached.


log.txt

[Bazinga]

If mesh and boundary conditions are fine and initialization with potentialFoam does not help, you might want to consider running a case with more numerical diffusion first. For example, use a coarser mesh, and choose 1st order upwind for the div terms of the momentum equations. If this one converges use mapFields to initialize your simulation with 2nd order schemes and finer mesh.

[HPE]

Some ideas from my bed:
- numerical predictions might not be time-invariant. might be there appears considerable extent time-variant patterns.
- relaxation factors: increase p to 0.9 and the rest 0.7.
- might use simplec instead of simple. if you use simplec, remove relaxation factor for p completely (delete those lines)
- find alternative boundary conditions to freestream bpundary conditions, and do the tests.
- depending on Ma number might consider to use an equivalent compressible solver