[bengir]

Hello everybody.
I am a beginner with Openfoam and I am trying to model the flow past a sphere with an axisymmetric study. I created my mesh with gmsh but when I am using gmshToFoam I have the following error message :

Create time

Starting to read mesh format at line 2
Read format version 2.2  ascii 0

Starting to read physical names at line 5
Physical names:8
    Line 4    axis
    Surface 1    inlet
    Surface 2    outlet
    Surface 3    wall
    Surface 5    sphere
    Surface 6    front
    Surface 7    back
    Volume 8    interior

Starting to read points at line 16
Vertices to be read:22920
Vertices read:22920

Starting to read cells at line 22939
Cells to be read:22685

Unhandled element 1 at line 22941
Unhandled element 1 at line 22942
................
Unhandled element 1 at line 23035
Unhandled element 1 at line 23036
..............
Unhandled element 1 at line 23087
Mapping region 7 to Foam patch 0
Mapping region 8 to Foam cellZone 0
Cells:
    total:11269
    hex  :11137
    prism:132
    pyr  :0
    tet  :0

CellZones:
Zone    Size
    0    11269

Skipping tag  at line 45627
Patch 0 gets name back

--> FOAM Warning : 
    From function Foam::polyMesh::polyMesh(const Foam::IOobject&, const Foam::Xfer<Foam::Field<Foam::Vector<double> > >&, const cellShapeList&, const faceListList&, const wordList&, const wordList&, const Foam::word&, const Foam::word&, const wordList&, bool)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 595
    Found 22906 undefined faces in mesh; adding to default patch.
Finding faces of patch 0

FaceZones:
Zone    Size

Writing zone 0 to cellZone interior and cellSet
End

I don't understand what it the problem.
That is my .geo file so you will probably find the problem (I hope )

cl__1 = 1;


Point(1) = {-100, 0, 0, 1};
Point(2) = {200, 0, 0, 1};
Point(3) = {-100, 100, 0, 1};
Point(4) = {200, 100, 0, 1};
Point(5) = {-7.5, 0, 0, 1.0};
Point(6) = {7.5, 0, 0, 1.0};
Point(7) = {0, 0, 0, 1.0};

Point(11) = {100, 0, 0, 1.0};
Point(12) = {100, 100, 0, 1.0};


//sphere
Point(8) = {5.3033008589, 5.3033008589, 0, 1.0};
Point(9) = {-5.3033008589, 5.3033008589, 0, 1.0};
Point(10) = {5.3033008589, 5.3033008589, 0, 1.0};



//lignes domaine
Line(1) = {3, 1};
Line(2) = {12, 11};
Line(3) = {4, 2};
Line(4) = {3, 12};
Line(5) = {12, 4};
Line(6) = {1, 5};
Line(7) = {6, 11};
Line(8) = {11, 2};
Line(95) = {5, 6};


//sphere
Circle(9) = {5, 7, 9};
Circle(10) = {9, 7, 8};
Circle(11) = {8, 7, 6};

//lignes bloc
Line(12) = {3, 9};
Line(13) = {12, 8};

Transfinite Line {4} = 60 Using Progression 1;
Transfinite Line {5, 8} =15 Using Progression 1;
Transfinite Line {1} = 60 Using Progression 1;
Transfinite Line {2, 3} = 60 Using Progression 0.96;
Transfinite Line {11, 10, 9} = 60 Using Progression 1;
Transfinite Line {10} = 60 Using Progression 1;
Transfinite Line {12} = 60 Using Progression 0.9;
Transfinite Line {13} = 60 Using Progression 0.9;
Transfinite Line {6} = 60 Using Progression 0.9;
Transfinite Line {7} = 60 Using Progression 1.1;


//surfaces
Line Loop(14) = {12, 10, -13, -4};
Plane Surface(15) = {14};
Line Loop(16) = {12, -9, -6, -1};
Plane Surface(17) = {16};
Line Loop(18) = {13, 11, 7, -2};
Plane Surface(19) = {18};
Line Loop(20) = {5, 3, -8, -2};
Plane Surface(21) = {20};
Transfinite Surface {17};
Transfinite Surface {15};
Transfinite Surface {19};
Transfinite Surface {21};
Recombine Surface {17};
Recombine Surface {15};
Recombine Surface {19};
Recombine Surface {21};





Extrude {{1,0,0}, {0,0,0},Pi/36} {
Surface{17, 15, 19, 21}; 
Layers{1};
Recombine; }

Physical Surface("inlet") = {37};//inlet
Physical Surface("outlet") = {89};//outlet
Physical Surface("wall") = {59, 86};//wall haut
Physical Line("axis") = {6, 7, 8, 95};//ligne sym
Physical Surface("sphere") = {51, 72, 33};//sphere
Physical Surface("front") = {38, 60, 77, 94};//front
Physical Surface("back") = {17, 15, 19, 21};//back
Physical Volume("interior") = {1, 2, 3, 4};//interior

Thanks in advance,
Cheers,
Ben

[alexeym]

Hi,

You have two kinds of warnings in your output:

1. Unhandled element type.
2. Standard "Found ... undefined faces in mesh; adding to default patch."

The second should be ignored, you can find explanation of the forum.

The first is caused by "2-node line" elements (type 1 in Gmsh terminology) in MSH file, which are generated due to this line:

Physical Line("axis") = {6, 7, 8, 95};//ligne sym

gmshToFoam indeed can not handle this type of elements. So, you can try to remove above mentioned line.

[bengir]

Thanks for your answer!
I don't have the message "unhandled..." anymore , nevertheless I still have one problem.
When I check my "boundary" file into "poly mesh", I just have 2 zone : "back" and "defaultFaces". I don't know why the other zone are not created.
Do you have any idea?

[alexeym]

Hi,

You have used wrong IDs, when defined physical surfaces. So in resulting MSH there is only physical surface 6 (back) and physical volume 7 (interior). Guess there are other faces, which do not belong to any physical surfaces and they are added to defaultFaces.

[bengir]

Hi,
Thanks, I modified something and so I forgot to change ID's. Obviously, now, I have something wrong again. When I do a checkMesh I have a fatal error :

wedge wedge1 plane aligns with coordinate plane

Does that mean I have to change that plane thanks to a rotate extrusion? I did it before but then there were some fatal error about the normal of wedge plane...

I'm sorry for all that questions but I really want to understand that axisymmetric problem.

Thanks in advance,

Ben.

[alexeym]

Hi,

Wedge-type boundaries should not align with coordinate planes, so before extrusion you need to rotate plane you would like to extrude, since you have constructed geometry in X-Y plane. In general, I rotate plane by -alpha radians and then extrude by 2*alpha radians. 2*alpha should be less than 5 degrees, so usually alpha = Pi/180.

[bengir]

It's working now!
I jus have to launch some calculations now, thanks