[88turbo]

I tried to find a tutorials or test case on using the periodic boundary condition module (SU2_PBC), but didn't have a lot of luck. I saw the periodic markers in the open rotor test case, but I couldn't get it to run. The case I'm running creates a 'mesh_out.su2' file, but I don't know if I need to run that back through the SU2_CFD or not. Any help is appreciated! Thanks!

[shirazbj]

Hi,

I tried this case a while ago, see:
an error when Paraview try to input flow.vtk

I tried with su2_cfd, but not su2_pbc. Under win7@32.

The mesh_openrotor_79k.su2 already has periodic conditions in it. I tried to remove all parts after MARKER_TAG= SEND_RECEIVE in the mesh file and then run su2_pdc.exe, It generate a new mesh file and added the removed parts. Also there is a periodic_halo.vtk, but it looks wired in Paraview. See attached pic.

The new Rev1206 source code can outputs nearly correct mesh in ascii tecplot format whih ghost points removed. The original 2.0 version can't. still expecting the new version of new output.

Regards

Cean

[shirazbj]

this is the result with new 2.0.2 su2_pbc.

still looks wired.

[fpalacios]

The picture doesn't make sense for me... as far I see the periodic_original.plt already has a halo cells created by the PBC?
Maybe you are running PBC twice, or maybe the original grid already has the periodic structure.

Best,
Francisco

[shirazbj]

I see. With the mesh file provided for that case, i also need to remove some points and elements before runing su2_pbc.exe. Not just the send_receive tag parts.

if su2_pbc is combined into su2_cfd, maybe it's easier to output the result.

[Amrita Lonkar]

Hi Steve and Cean,

The procedure to include PBC boundary conditions in your simulation are:

1) Create a regular mesh in .su2 or .cgns format.
2) Use a configuration file which has the option for the periodic marker.

For example,
MARKER_PERIODIC= ( SideWall1, SideWall2, 0,1.0, 0, -60, 0, 0, 0, 0,0, SideWall2, SideWall1, 0,1.0,0, 60, 0,0, 0,0,0 )

where the format of the above quantities is:
% Format: ( periodic marker, donor marker, rotation_center_x, rotation_center_y,
% rotation_center_z, rotation_angle_x-axis, rotation_angle_y-axis,
% rotation_angle_z-axis, translation_x, translation_y, translation_z, ... ).


Use this mesh file and configuration file to run SU2_PBC as:

SU2_PBC configuration.cfg

This will output a new mesh (by default named mesh_out.su2) with a set of halo cells.

Use this mesh file to run a flow simulation. This can be done by just renaming the input mesh file in the configuration file as:
MESH_FILENAME = mesh_out.su2


This should work, let us know if this doesn't. We will soon add a test case to demonstrate this capability. Thanks for highlighting this issue.

Amrita

[shirazbj]

Hi Amrita,

I realised the compilcation of the mesh file: it may be a normal file or a file generated by su2_PBC.

If su2_CFD can hide the su2_PBC detail, it would be more easy to use.

Regards,

Cean

[copeland]

Hi Cean,

Just to follow up, you can always tell if a mesh file has been generated using SU2_PBC by opening the .su2 mesh file and searching for "MARKER_TAG= SEND_RECEIVE". If this send/receive tag is in the file, it has been generated using the periodic module.

Thanks for your suggestion on incorporating PBC into the main CFD module, we are always looking for ways to improve the usability of the code. We'll keep it in mind for future releases.



-Sean