[thomas.]

Hello all,

I am trying to simulate a multiphase flow using interFoam and using LES for turbulence modelling. I will try to be as accurate as possible regarding the description of the problem, so I will quote all error/warnings messages from terminal.
I would really appreciate your help. Thanks in advance for your time!

So, the geometry file in gmsh is:

// Gmsh project created on Thu Apr  9 09:24:11 2015
el = 1;
pi = 3.14159265;
theta = (pi/4 + pi/2);
theta2 = (pi/4);
r = 40;
r2 = 40+20*Cos(theta2);

Point(1) = {0, 0, 0, el};
Point(2) = {0, 15, 0, el};
Point(3) = {r2*Cos(theta), 15+r2*Sin(theta), 0, el};
Point(4) = {r*Cos(theta), 35+r*Sin(theta), 0, el};
Point(5) = {0, 35, 0, el};
Point(6) = {0, 40, 0, el};
Point(7) = {120, 40, 0, el};
Point(8) = {120, 35, 0, el};
Point(9) = {160, 35, 0, el};
Point(10) = {160, 15, 0, el};
Point(11) = {120, 15, 0, el};
Point(12) = {120, 0, 0, el};
Line(1) = {1, 2};
Line(2) = {2, 3};
Line(3) = {3, 4};
Line(4) = {4, 5};
Line(5) = {5, 6};
Line(6) = {6, 7};
Line(7) = {7, 8};
Line(8) = {8, 9};
Line(9) = {9, 10};
Line(10) = {10, 11};
Line(11) = {11, 12};
Line(12) = {12, 1};
Line Loop(13) = {6, 7, 8, 9, 10, 11, 12, 1, 2, 3, 4, 5};
Plane Surface(14) = {13};

Extrude {0, 0, 10} {
  Surface{14};
  Layers{1};
  Recombine;
}
Physical Surface("back") = {14};
Physical Surface("front") = {76};
Physical Surface("inlet") = {67};
Physical Surface("outlet") = {43};
Physical Surface("walls") = {59, 63, 71, 75, 31, 35, 39, 43, 47, 55};
Physical Volume("interior") = {1};

After converting the mesh file using gmshToFoam, I get following warning:

--> FOAM Warning : 
    From function polyMesh:polyMesh(... construct from shapes...)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 627
    Found 248400 undefined faces in mesh; adding to default patch.

The resulting boundary file looks like this:

6
(
    back
    {
        type            patch;
        physicalType    patch;
        nFaces          122260;
        startFace       609360;
    }
    walls
    {
        type            patch;
        physicalType    patch;
        nFaces          3496;
        startFace       731620;
    }
    outlet
    {
        type            patch;
        physicalType    patch;
        nFaces          156;
        startFace       735116;
    }
    inlet
    {
        type            patch;
        physicalType    patch;
        nFaces          112;
        startFace       735272;
    }
    front
    {
        type            patch;
        physicalType    patch;
        nFaces          122260;
        startFace       735384;
    }
    defaultFaces
    {
        type            patch;
        nFaces          116;
        startFace       857644;
    }
)

As I change the type and physical type for front and back to "empty" while leaving the defaultFaces type as "patch" and I try to run interFoam, I get following error:

--> FOAM FATAL IO ERROR: 
Cannot find patchField entry for defaultFaces

file: /home/thomas/CFD/OpenFOAM/thomas-2.3.1/run/tutorials/multiphase/interFoam/thomasCaseLES/0/p_rgh.boundaryField from line 25 to line 42.

    From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 209.

FOAM exiting

And if I change the defaultFaces type to "empty", I get following error:

--> FOAM FATAL ERROR: 
Case is not 3D or 2D, LES is not applicable

    From function cubeRootVolDelta::calcDelta()
    in file cubeRootVolDelta/cubeRootVolDelta.C at line 72.

FOAM exiting

Once again, thank you in advance for reading and trying to help!

[alexeym]

Hi,

You have forgotten to add one surface into walls patch (see attached image), so they went into defaultFaces and this ended with final error (as for 2D case only front and back should be empty).

Also, you have to edit boundary dictionary (with changeDictionary utility for example), so front and back have type empty, walls has type wall (or your next question will be about wall functions those complain about walls not being walls ).

And finally, why not make hexagonal mesh using transfinite algorithm? The geometry is very simple.

[thomas.]

Hi,

first of all, thank you very much for responding. Your comment helped me to find where I was messing up: I checked the wall boundaries definition and I noticed, that I had surface 43 defined as an outlet and as a wall. In stead of defining surface 43 as a wall, I have to define surface 51 as a wall.

Regarding the transfinite algoritm: that's the next step!

Thanks again!