CFD Online Logo CFD Online URL
Home > Forums > OpenFOAM Programming & Development

Top-Level Mixing-Plane

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Display Modes
Old   February 26, 2010, 08:41
Default Top-Level Mixing-Plane
Oliver Borm
Join Date: Mar 2009
Posts: 59
Rep Power: 10
deepblue17 is on a distinguished road

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!
Attached Images
File Type: png rotor1_mixingPlane.png (30.5 KB, 54 views)
File Type: png stator1_mixingPlane.png (30.0 KB, 44 views)
File Type: png rotor1_stator1_mixingPlane.png (28.5 KB, 53 views)
Attached Files
File Type: gz extrudePolyMesh.tar.gz (7.0 KB, 27 views)
deepblue17 is offline   Reply With Quote


Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
How to setup mixing plane interface in STAR-CCM+ mrjonezz STAR-CCM+ 3 July 8, 2015 11:51
Turbine stage mixing plane calculation Knut FLUENT 0 December 4, 2007 13:46
Error in flux at Fluent´s mixing plane calculation ales FLUENT 0 February 9, 2005 05:48
Mixing Plane Lee FLUENT 0 August 8, 2003 22:36
Mixing plane geometry definition Hbet FLUENT 0 January 18, 2002 08:16

All times are GMT -4. The time now is 04:16.