[thomas.]

Hello all,

I would really appreciate if someone could help me out with this one.

I have been trying for a while now to simulate an internal turbulent vortex flow (air) within a suction-diffuser with k-omega SST with no success: I am getting extreme high values for omega (10^6) and very high values for k (10^2). I am using OF 3.0.x.

I tried both resolving the boundary layer (y+ near 1) and using scalable wall functions (1 < y+ < 300), according to:
http://www.dicat.unige.it/guerrero/o...turbulence.pdf
Every time I get the mentioned k and omega values.

I attached two screenshots from the geometry. It consists of two inlet tubes, one suction (bottom part of the geometry), an outlet tube and walls. Both inlet tubes are supposed to generate an internal vortex, so the sucked air from the atmosphere finds its way up to the outlet close to the cone-shaped wall. The suction is supposed to be generated due to the pressure drop due to the high velocity of the inlet flow and due to the negative pressure of the outlet.

I meshed with snappyHexMesh starting from a 100x100x75 blockMesh (that´s why there is only one surfaceRefinement step).

In the next post (I couldn´t attach everything to this post, due to the 20000 characters limit), you will find the code of snappyHexMesh and the boundary conditions (in this case, for resolving the boundary layer).

Once again, I would REALLY appreciate if someone could help me out with this.

Thanks in advance!

[thomas.]

snappyHexMesh:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      snappyHexMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Which of the steps to run
castellatedMesh true;
snap            true;
addLayers       true;
geometry //Prescribe geometry entities for meshing
{
    CAD_patch0.stl
    {
        type triSurfaceMesh;
 name outlet;
    }
    CAD_patch1.stl
    {
 type triSurfaceMesh;
 name wall_outlet_cylinder;
    }
    CAD_patch2.stl
    {
 type triSurfaceMesh;
 name wall_inlet_cone;
    }
    CAD_patch3.stl
    {
 type triSurfaceMesh;
 name wall_top;
    }
    CAD_patch4.stl
    {
 type triSurfaceMesh;
 name atm;
    }
    CAD_patch5.stl
    {
 type triSurfaceMesh;
 name inlet2;
    }
    CAD_patch6.stl
    {
 type triSurfaceMesh;
 name inlet1;
    }
    duese.stl
    {
 type triSurfaceMesh;
 name volumen;
    }
    //refinementBox
    //{
    //    type searchableBox;
    //    min (-1.0 -0.7 0.0);
    //    max ( 8.0  0.7 2.5);
    //}
};

// Settings for the castellatedMesh generation. Prescribe feature,
// surface and volume mesh refinements
castellatedMeshControls
{
    // Refinement parameters
    // ~~~~~~~~~~~~~~~~~~~~~
    // If local number of cells is >= maxLocalCells on any processor
    // switches from from refinement followed by balancing
    // (current method) to (weighted) balancing before refinement.
    maxLocalCells 1000000;
    // Overall cell limit (approximately). Refinement will stop immediately
    // upon reaching this number so a refinement level might not complete.
    // Note that this is the number of cells before removing the part which
    // is not 'visible' from the keepPoint. The final number of cells might
    // actually be a lot less.
    maxGlobalCells 20000000;
    // The surface refinement loop might spend lots of iterations refining just a
    // few cells. This setting will cause refinement to stop if <= minimumRefine
    // are selected for refinement. Note: it will at least do one iteration
    // (unless the number of cells to refine is 0)
    minRefinementCells 0;
    // Allow a certain level of imbalance during refining
    // (since balancing is quite expensive)
    // Expressed as fraction of perfect balance (= overall number of cells /
    // nProcs). 0=balance always.
    maxLoadUnbalance 0.10;

    // Number of buffer layers between different levels.
    // 1 means normal 2:1 refinement restriction, larger means slower
    // refinement.
    nCellsBetweenLevels 3;
 
    // Explicit feature edge refinement
    // ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
    // Specifies a level for any cell intersected by its edges.
    // This is a featureEdgeMesh, read from constant/triSurface for now.
    features
    (
        {
            file "CAD_patch0.eMesh";
            level 6;
        }
        {
            file "CAD_patch1.eMesh";
            level 6;
        }
        {
            file "CAD_patch2.eMesh";
            level 6;
        }
        {
            file "CAD_patch3.eMesh";
            level 6;
        }
        {
            file "CAD_patch4.eMesh";
            level 6;
        }
        {
            file "CAD_patch5.eMesh";
            level 6;
 }
        {
            file "CAD_patch6.eMesh";
            level 6;
 }
    );
 
    // Surface based refinement
    // ~~~~~~~~~~~~~~~~~~~~~~~~
    // Specifies two levels for every surface. The first is the minimum level,
    // every cell intersecting a surface gets refined up to the minimum level.
    // The second level is the maximum level. Cells that 'see' multiple
    // intersections where the intersections make an
    // angle > resolveFeatureAngle get refined up to the maximum level.
    refinementSurfaces
    {
  atm
   {
    level (1 1);
   }
  wall_inlet_cone
   {
    level (1 1);
   }
  wall_outlet_cylinder
   { 
    level (1 1);
   }
  wall_top
   {
    level (1 1);
   }
  inlet1
   {
    level (1 1);
   }
  inlet2
   {
    level (1 1);
   }
  outlet
   {
    level (1 1);
   }
            // Optional specification of patch type (default is wall). No
            // constraint types (cyclic, symmetry) etc. are allowed.
            //patchInfo
            //{
            //   type wall;
            //   inGroups (motorBikeGroup);
            //}
     //}
        //}
    }
    // Resolve sharp angles
    resolveFeatureAngle 30;

    // Region-wise refinement
    // ~~~~~~~~~~~~~~~~~~~~~~
    // Specifies refinement level for cells in relation to a surface. One of
    // three modes
    // - distance. 'levels' specifies per distance to the surface the
    //   wanted refinement level. The distances need to be specified in
    //   descending order.
    // - inside. 'levels' is only one entry and only the level is used. All
    //   cells inside the surface get refined up to the level. The surface
    //   needs to be closed for this to be possible.
    // - outside. Same but cells outside.
    refinementRegions
    {
       // refinementBox     {volume {mode distance; levels ((0.0006 4) (0.002 3) (0.01      2));}} // was ((0.001 4) (0.003 3) (0.01 2))
       //{
       //     mode inside;
       //     levels ((1E15 4));
       // }
    }

    // Mesh selection
    // ~~~~~~~~~~~~~~
    // After refinement patches get added for all refinementSurfaces and
    // all cells intersecting the surfaces get put into these patches. The
    // section reachable from the locationInMesh is kept.
    // NOTE: This point should never be on a face, always inside a cell, even
    // after refinement.
    locationInMesh (0 0 0.04);

    // Whether any faceZones (as specified in the refinementSurfaces)
    // are only on the boundary of corresponding cellZones or also allow
    // free-standing zone faces. Not used if there are no faceZones.
    allowFreeStandingZoneFaces true;
}
 
// Settings for the snapping. 
snapControls
{
    //- Number of patch smoothing iterations before finding correspondence
    //  to surface
    nSmoothPatch 3;
    //- Relative distance for points to be attracted by surface feature point
    //  or edge. True distance is this factor times local
    //  maximum edge length.
    tolerance 2.0;
    //- Number of mesh displacement relaxation iterations.
    nSolveIter 30;
    //- Maximum number of snapping relaxation iterations. Should stop
    //  before upon reaching a correct mesh.
    nRelaxIter 5;
    // Feature snapping
        //- Number of feature edge snapping iterations.
        //  Leave out altogether to disable.
        nFeatureSnapIter 10;
        //- Detect (geometric only) features by sampling the surface
        //  (default=false).
        implicitFeatureSnap false;
        //- Use castellatedMeshControls::features (default = true)
        explicitFeatureSnap true;
        //- Detect points on multiple surfaces (only for explicitFeatureSnap)
        multiRegionFeatureSnap false;
}
 
// Settings for the boundary layer addition.
addLayersControls
{
    // Are the thickness parameters below relative to the undistorted
    // size of the refined cell outside layer (true) or absolute sizes (false).
    relativeSizes false;
    // Per final patch (so not geometry!) the layer information
    layers
    {
        atm
        {
            nSurfaceLayers 10;
        }
 wall_inlet_cone
        {
            nSurfaceLayers 10;
        }
 wall_outlet_cylinder
        {
            nSurfaceLayers 10;
        }
 wall_top
        {
            nSurfaceLayers 10;
        }
    }
    firstLayerThickness 5e-05;//1.8
    // Expansion factor for layer mesh
    expansionRatio 1.15;
    // Wanted thickness of final added cell layer. If multiple layers
    // is the thickness of the layer furthest away from the wall.
    // Relative to undistorted size of cell outside layer.
    // See relativeSizes parameter.
    //finalLayerThickness 0.3;
    // Minimum thickness of cell layer. If for any reason layer
    // cannot be above minThickness, do not add layer.
    // Relative to undistorted size of cell outside layer.
    minThickness 1.0e-05;//1.5
    // If points get not extruded do nGrow layers of connected faces that are
    // also not grown. This helps convergence of the layer addition process
    // close to features.
    // Note: changed(corrected) w.r.t 17x! (didn't do anything in 17x)
    nGrow 0;
    // Advanced settings
    // When not to extrude surface. 0 is flat surface, 90 is when two faces
    // are perpendicular
    featureAngle 180;
    // At non-patched sides allow mesh to slip if extrusion direction makes
    // angle larger than slipFeatureAngle.
    slipFeatureAngle 30;
    // Maximum number of snapping relaxation iterations. Should stop
    // before upon reaching a correct mesh.
    nRelaxIter 5;
    // Number of smoothing iterations of surface normals
    nSmoothSurfaceNormals 1;
    // Number of smoothing iterations of interior mesh movement direction
    nSmoothNormals 3;
    // Smooth layer thickness over surface patches
    nSmoothThickness 10;
    // Stop layer growth on highly warped cells
    maxFaceThicknessRatio 0.5;
    // Reduce layer growth where ratio thickness to medial
    // distance is large
    maxThicknessToMedialRatio 1;
    // Angle used to pick up medial axis points
    // Note: changed(corrected) w.r.t 17x! 90 degrees corresponds to 130 in 17x.
    minMedianAxisAngle 90;

    // Create buffer region for new layer terminations
    nBufferCellsNoExtrude 0;

    // Overall max number of layer addition iterations. The mesher will exit
    // if it reaches this number of iterations; possibly with an illegal
    // mesh.
    nLayerIter 50;
}
 
// Generic mesh quality settings. At any undoable phase these determine
// where to undo.
meshQualityControls
{
    maxNonOrtho 65;
    maxBoundarySkewness 20;
    maxInternalSkewness 4;
    maxConcave 80;
    minFlatness 0.5;
    minVol 1e-13;
    minTetQuality -1e+30;
    minArea -1;
    minTwist 0.02;
    minDeterminant 0.001;
    minFaceWeight 0.02;
    minVolRatio 0.01;
    minTriangleTwist -1;
    // Advanced
    nSmoothScale 4;
    errorReduction 0.75;
}

// Advanced
debug 0;

// Merge tolerance. Is fraction of overall bounding box of initial mesh.
// Note: the write tolerance needs to be higher than this.
mergeTolerance 1e-6;

// ************************************************************************* //;

k:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -2 0 0 0 0];
internalField   uniform 6.1;
boundaryField
{
    inlet1
    {
        type            fixedValue;
 value  uniform 6.1;
    }
    inlet2
    {
        type            fixedValue;
 value  uniform 6.1;
    }
    outlet
    {
        type            zeroGradient;
    }
    wall_inlet_cone
    {
        type            kqRWallFunction;
 value  uniform 1e-10;
    }
    wall_outlet_cylinder
    {
        type            kqRWallFunction;
 value  uniform 1e-10;
    }
    wall_top
    {
        type            kqRWallFunction;
 value  uniform 1e-10;
    }
    atm
    {
        type            inletOutlet;
        inletValue      uniform 0.01;
        value           uniform 0.01;
    }
}

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

omega:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 0 -1 0 0 0 0];
internalField   uniform 8.7e+03;
boundaryField
{
    inlet1
    {
        type            fixedValue;
 value  uniform 8.7e+03;
    }
    inlet2
    {
        type            fixedValue;
 value  uniform 8.7e+03;
    }
    outlet
    {
         type            zeroGradient;
    }
    wall_inlet_cone
    {
        type            omegaWallFunction;
        value           uniform 6.8e+01;
    }
    wall_outlet_cylinder
    {
        type            omegaWallFunction;
        value           uniform 6.8e+01;
    }
    wall_top
    {
        type            omegaWallFunction;
        value           uniform 6.8e+01;
    }
    atm
    {
        type            inletOutlet;
        inletValue      uniform 0.1;
        value           uniform 0.1;
    }
}

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

nut:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -1 0 0 0 0];
internalField   uniform 46; 
boundaryField
{
    inlet1
    {
        type            calculated;
        value           uniform 1;
    }
    inlet2
    {
        type            calculated;
        value           uniform 1;
    }
    outlet
    {
        type            calculated;
        value           uniform 1;
    }
    wall_inlet_cone
    {
        type            nutUSpaldingWallFunction;
        value           $internalField;
    }
    wall_outlet_cylinder
    {
        type           nutUSpaldingWallFunction;
        value           $internalField;
    }
    wall_top
    {
        type            nutUSpaldingWallFunction;
        value           $internalField;
    }
    atm
    {
        type            calculated;
        value           uniform 1;
    }
}
// ************************************************************************* //

U:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 1 -1 0 0 0 0];
internalField   uniform (1e-09 1e-09 1e-09);
boundaryField
{
    inlet1
    {
        type           fixedValue;
 value  uniform (0 40 0);
    }
    inlet2
    {
        type           fixedValue;
 value  uniform (0 -40 0);
    }

    outlet
    {
        type            zeroGradient;
    }
    wall_inlet_cone
    {
        type            fixedValue;
        value           $internalField;
    } 
    wall_outlet_cylinder
    {
        type            fixedValue;
        value           $internalField;
    }
    wall_top
    {
        type            fixedValue;
        value           $internalField;
    }
    atm
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
 inletDirection uniform (0 0 1);
    }
}

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

p:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -2 0 0 0 0];
internalField   uniform 0;
boundaryField
{
    inlet1
    {
        type            totalPressure;
        p0              uniform 0;
        U               U;
        gamma           1.4;
        value           uniform 0;
    }
    inlet2
    {
        type            totalPressure;
        p0              uniform 0;
        U               U;
        gamma           1.4;
        value           uniform 0;
    }
    outlet
    {
        type            totalPressure;
        p0              uniform -2500;
        U               U;
        gamma           1.4;
        value           uniform 0;
    }
    wall_inlet_cone
    {
        type            zeroGradient;
    }
    wall_outlet_cylinder
    {
        type            zeroGradient;
    }
    wall_top
    {
        type            zeroGradient;
    }
    atm
    {
        type            totalPressure;
        p0              uniform 0;
        U               U;
        gamma           1.4;
        value           uniform 0;
    }
}
// ************************************************************************* //

[alexeym]

Hi,

Could you also post output of checkMesh? Are you sure you have converged? How do you calculate IC for k and omega?

[thomas.]

Hi!

first of all, thanks for your reply.

Unfortunately, I don´t have access right now to the Linux-session and PC from which I am doing the simulation, so I can´t post the checkMesh output right now (I will post it tomorrow early). Nevertheless, the mesh parameters read in checkMesh are quite fine, as far as I am concerned: non-orthogonality under 65, normal skewness, 80% hexahedral cells, 20% prism cells and all the meshQualityControls parameters are satisfied.

I calculated the IC´s according to http://www.dicat.unige.it/guerrero/o...turbulence.pdf and also according to the CFD-online tool. I tried also with numerical zero and/or with very high values.

I have run 5000 iterations and the residuals stabilize around iteration number 200 at 0.01 (not opitmal, I know). I also checked continuity (the value bounces around 0 +/- 0.02).

Also, the high values for omega and k are just present in a few cells (10 or so) in the sharp corner in the outlet tube and/or in the inlet patches.

I really don´t know what else to try. Help would be really appreciated!

[msuaeronautics]

Why such high omega inflow conditions?

[alexeym]

@thomas.

Why stop at 5000 iterations?

Since anyway you will add checkMesh output, could you also add fvSchemes and fvSolution files?

I calculated the IC´s according to http://www.dicat.unige.it/guerrero/o...turbulence.pdf and also according to the CFD-online tool. I tried also with numerical zero and/or with very high values.

Why not try CONSISTENT values? For example, turbulentIntensityKineticEnergyInlet and turbulentMixingLengthFrequencyInlet with corresponding turbulence intensity and hydraulic diameter.

[thomas.]

Hi,

once again, thank you very much for taking the time to try to help.

Checking the checkMesh info, I noticed that I had several thousand of polyhedra cells with more than 15 faces. I could fix that by starting from a coarse blockMesh and then doing a region refinement (refinementRegions => mode inside). By doing that and playing around with the blockMesh/refinementRegions parameters, I reduce polyhedra cells to a maximum of 5 faces. Maybe that´s a source of those extremely high omega values.

Regarding the turbulent boundary and initial conditions: I used fixedValues according to the formulas of the calculated inlet values given by the boundary conditions Alexey proposed:
http://foam.sourceforge.net/docs/cpp/a02692.html#details
http://foam.sourceforge.net/docs/cpp/a02689.html#details

The values are so high, because I calculated them using the diameter of the inlet tubes as the characteristic lenght, i.e., 4 [mm].
I will try those boundary conditions, though.



Here, my new checkMesh:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 3.0.1-119cac7e8750
Exec   : checkMesh
Date   : Mar 30 2016
Time   : 10:12:04
Host   : "thomas-Lenovo-G710"
PID    : 3293
Case   : /home/thomas/OpenFOAM/thomas-3.0.1/run/duese_turb_2inlets
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:           919587
    faces:            2709299
    internal faces:   2659690
    cells:            899859
    faces per cell:   5.9664781
    boundary patches: 13
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     879553
    prisms:        6948
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     13358
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            4   9859
            5   3499

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
                    maxY        0        0                        ok (empty)
                    minX        0        0                        ok (empty)
                    maxX        0        0                        ok (empty)
                    minY        0        0                        ok (empty)
                    minZ        0        0                        ok (empty)
                    maxZ        0        0                        ok (empty)
                  outlet      120      139  ok (non-closed singly connected)
    wall_outlet_cylinder     6217     6680  ok (non-closed singly connected)
         wall_inlet_cone    25581    35411  ok (non-closed singly connected)
                wall_top    17145    17271  ok (non-closed singly connected)
                     atm      484      513  ok (non-closed singly connected)
                  inlet2       31       39  ok (non-closed singly connected)
                  inlet1       31       39  ok (non-closed singly connected)

Checking geometry...
    Overall domain bounding box (-0.059998797 -0.059999725 0) (0.059999999 0.059998673 0.090000004)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (-2.7304679e-16 -1.026775e-16 1.0133647e-15) OK.
    Max cell openness = 3.2339666e-16 OK.
    Max aspect ratio = 4.6956445 OK.
    Minimum face area = 7.5996014e-08. Maximum face area = 1.5246158e-06.  Face area magnitudes OK.
    Min volume = 8.1169095e-11. Max volume = 8.1982517e-10.  Total volume = 0.00047691756.  Cell volumes OK.
    Mesh non-orthogonality Max: 55.790767 average: 2.7985153
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.2066045 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

fvSchemes

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
    grad(U)         cellLimited Gauss linear 1;
}

divSchemes
{
    default         none;
    div(phi,U)      bounded Gauss linearUpwindV 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 corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

wallDist
{
    method meshWave;
}


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

fvSolution:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
    p
    {
        solver           GAMG;
        tolerance        1e-7;
        relTol           0.01;
        smoother         GaussSeidel;
        nPreSweeps       0;
        nPostSweeps      2;
        cacheAgglomeration on;
        agglomerator     faceAreaPair;
        nCellsInCoarsestLevel 10;
        mergeLevels      1;
    }

    Phi
    {
        $p;
    }

    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 0;
    consistent yes;
    residualControl
    {
        p               1e-3;
        U               1e-3;
        "(k|omega)"     1e-3;
    }
}

potentialFlow
{
    nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
    equations
    {
        U               0.75; // 0.9 is more stable but 0.95 more convergent
    omega        0.75;
    k        0.75;
        ".*"            0.75; // 0.9 is more stable but 0.95 more convergent
    }
}

cache
{
    grad(U);
}

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

[c_dowd]

Can you see in your result visualisations where the turbulence values get too high? That could give you some hints as to whether its a meshing problem or not, if it's happening in a region with highly skewed or non-orthogonal cells it's probably a mesh problem.

[alexeym]

@thomas.

1. You have got 56 degrees of maximum non-orthogonality, yet have 0 non-orthogonal corrector iterations. Usually it is 1 or 2 for your value of non-orthogonality.

2. What were the values of residuals after 5000 iterations? Maybe you just far from convergence, so those high values of k and omega are just intermediate result.

[thomas.]

Uops, you´re right!

Thank you all for your help. I will try those out and let you know how it went, in the case, someone else has the same problem in the future.

One further question: when trying to insert layers, the quality-parameters of the mesh get lower, i.e., from 56° non-ortho I get to 65° of non ortho and I get once again the polyhedra with 18 faces. Any idea how I can get passed this?

Thanks!