CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (http://www.cfd-online.com/Forums/openfoam-programming-development/)
-   -   Top-Level Mixing-Plane (http://www.cfd-online.com/Forums/openfoam-programming-development/73095-top-level-mixing-plane.html)

deepblue17 February 26, 2010 08:41

Top-Level Mixing-Plane
 
4 Attachment(s)
Hello,

I would like to present a "top-level" mixing-plane for turbomachines. The basic idea is to use several hexahedral cells with polygonal faces. These cells are arranged in normal direction (either radial, axial or mixed - depends on the machine type). Every "dummy" cell therefore spans in the complete azimuthal direction (compare attached figures). As each cell has only one value, the azimuthal averaging is done indirectly. The spacing of the cells in normal direction could be different for the rotor and stator dummy cells (cf. figure 3). In order ro create these hexahedral cells I've modified the extrudeMesh utility, which I've called now extrudePolyMesh, which is attached and does work with OF-1.6. In oder to couple the different mesh parts, one could use the following approaches:

rotorMesh <-> ggi or stitchMesh <-> dummyRotorCells <-> overlapGgi / ggi / stitchMesh <-> dummyStatorCells <-> ggi / stitchMesh <-> statorMesh

If the spacing (number of blades in each bladerow) is different between the rotor and stator, one needs the overlapGgi BC between the rotor and stator dummy cells.

The following procedure could be applied in order to generate the rotor dummy cells:

* extrudeMesh ; from rotorMesh exit patch with extrudeModel = linearNormal

* autoPatch 45 ; in order to get all 6 boundary patches -> search for the right BC patch (green faces in figure 1 and 2)

* extrudePolyMesh ; from the green patch (e.g. auto 3) with extrudeModel = wedge

* autoPatch 45 ; in order to get all 6 boundary patches, maybe you want to rename them in oder to avoid name clashes when you merge the meshes afterwards and remove patches with zero faces in the boundary file

* checkMesh ; make sure there are no problems with the dummy cells, maybe you have to change the flipNormals in the extrudeProperties file "on" or "off" in order that no negative cells are generated. In the worst cases you may also need to modify the extrudePolyMesh utility for your specific case!

The same procedure has to be applied for the stator dummy cells.

Afterwards one can merge the two meshes with the dummy cells from rotor and stator:

mergeMeshes . fubar_rotorPolyMesh . fubar_statorPolyMesh

The new mesh is stored in an new time directory, maybe one wants to move the polyMesh directory under the constant directory. Then one should merge the dummy cells with the original case:

mergeMeshes . fubar . fubar_rotorStatorPolyMesh

Now you have the complete mesh with all the "dummy" cells, compare attached figure 3. This mesh should now run with incompressibel and compressibel; laminar or turbulent solvers. But only if the checkMesh utility does NOT fail!


All times are GMT -4. The time now is 11:38.