3D Windturbine simulation in SU2
3 Attachment(s)
Dear All,
I'm trying to simulate a single blade 120deg axi-symmetric model of the CX100 turbine using the incompressible RANS solver in SU2. The 3D grid was made in Pointwise using this webinar - https://www.youtube.com/watch?v=_o0KOJ7RJXc. The SU2 configuration file is also attached. You can download the grid using the link below or if this link expires, feel free to contact me. If anyone knows, please let me know if you know a place where I can share this indefinitely.. https://we.tl/Nz7L2hjxrv The attached images shows the boundary patches. With the current set-up I'm not able to even reach one iteration. I've tried using the SU2_MSH processor and running the simulation with 'CX100_pre.su2' grid, which also fails. Could anyone please have a look at this case and suggest improvements that can actually enable me to run this problem. The .cfg file: Code:
% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------% Any advice is greatly appreciated Thanks in advance, Kind regards, Kishore |
hey,
Could you please elaborate what error you got. |
Quote:
Code:
------------------------------------------------------------------------- If I use SU2_MSH to adapt the CX100.su2 grid file for periodic boundary conditions the output is: Code:
------------------------------------------------------------------------- Code:
------------------------------------------------------------------------- Kind regards, Kishore |
Hi Kishore,
as far as I know, the incompressible solver is currently not able to handle a rotating frame (at least the additional terms are not included in the flux computation). You could try to use the compressible solver. However, this will not solve your problem with the periodic boundaries. What exactly is the difference between the first run and the third one ? Tim |
Quote:
Many thanks for your reply. The differences are that the first run was performed with the grid directly from pointwise 'CX100.su2' without any pre-processing for SU2 periodic simulation (halo cells, renumbering etc.), while the second run was performed with the grid outputted from the SU2_MSH 'CX100_pre.su2' - grid adapted for periodic boundaries. Have you or anyone successfully simulated a 3D periodic problem in SU2 using the grid from pointwise? Kind regards, Kishore |
Hi,
I tried to run your grid, but the file seems different, as there are only 5 markers and they are named: MARKER_TAG= Blade MARKER_ELEMS= 34994 MARKER_TAG= Farfield MARKER_ELEMS= 8944 MARKER_TAG= Per1 MARKER_ELEMS= 7393 MARKER_TAG= Per2 MARKER_ELEMS= 7393 MARKER_TAG= Spinner MARKER_ELEMS= 5388 I modified cfg file accordingly and the output of SU2_MSH gave log similar to yours with the following ending lines: Quote:
I'm using release 4.1.2 |
Quote:
I realised that I uploaded the wrong grid file and updated the link above this morning with the grid shown in the images, maybe you were using the old link. Regardless as you've already found out, they only vary in the boundary names. Its interesting that your are getting up to the angular velocity output from SU2_CFD, so the SU2_MSH in v4.1.2 is better at adapting periodic boundaries for this grid than the v4.1.1. Because my run failed on "The surface element (1, 1325) doesn't have an associated volume element.". Did you get bad matches too from SU2_MSH? I'm glad we got progress with handling the grid, maybe as Tim said we need to try the compressible solver to get the rotating frame and the periodic BCs to work? My next step will be to get v4.1.2 and set-up a compressible case..maybe with very low mach numbers to skip any compressibility effects? - adjust the fluid models so it computes the same density for all pressure and temperatures perhaps. maybe I can do isothermal compressible simulation? where we change the fluid model to set same density for all pressures...I'm sure there is more to it than that... Has anyone tried to compute a incompressible solution using the compressible SU2 solver? Please let me know your thoughts and if any other results.... Thanks a lot, Kind regards, Kishore |
Quote:
For the bad matches in SU2_MSH, since the nearest donor distance is about 1e-8 level, which is close to the truncation error of single precision, I think you could try to output the mesh with double-precision in Pointwise. Besides,you could also adjust the tolerance in function CPhysicalGeometry::SetPeriodicBoundary,which is currently 1e-10, and changing it to 1e-8 may be helpful in this case. Muchen |
Quote:
Many thanks for your advice. The grids were generated with double double-precision, so maybe that is the maximum matches I could get from Pointwise? So from what I understand if I have grids with 1e-8 or more bad match I can set CPhysicalGeometry::SetPeriodicBoundary to higher values to not allow CFD_MSH to modify the location of the grid elements but still renumber them for periodic BC? Kind regards, Kishore |
Quote:
Actually, no matter what the tolerance is, for each point on the periodic boundaries, the SU2_MSH command would still find its nearest point after the transformation defined in the config file and set it as the donor point . Since this is a point-to-point approach, it is best to create identical meshes on the two periodic boundaries, which means that these two meshes could completely overlap with each other after certain translation or rotation. Besides, you could always check the "periodic_halo.dat" to see if the halo cells are created successfully. Muchen |
Quote:
In Pointwise, I did make surface mesh for both periodic boundaries to be identical (1:1) - the surface mesh from one side was rotated and the volumes were generated between them to make it easy for SU2_MSH. Maybe there is some tolerance issue with the copy/rotation in pointwise... Still haven't tried the compressible solver with this grid, hopefully with the newer version V4.2 everything run smoothly.... Kind regards, Kishore |
Hi Kishore,
I am also working on the 3d Periodic BCs for rotor simulation using SU2. the link to download your grid isn't available anymore, could you please update it again? And I want try your run to see what happen. Thanks! |
Quote:
I've uploaded it again: https://we.tl/peNWItztZt Maybe you know a better place to permanently share this file.... Can you please post your configuration file that we already have for a 3D periodic rotor cases? and any improvements you suggest for this case. Any help is greatly appreciated, Kind regards, Kishore |
Hi Kishore,
Now I am trying to run the Caradonna&Tung case using 3D rotating periodic BC, the procedures are: 1. Output the su2 mesh from pointwise. 2. Set up the configuration file, the periodic boundary and grid adaption parts are: % Periodic boundary marker(s) (NONE = no marker) % Format: ( periodic marker, donor marker, rot_cen_x, rot_cen_y, rot_cen_z, rot_angle_x-axis, rot_angle_y-axis, rot_angle_z-axis, translation_x, translation_y, translation_z) MARKER_PERIODIC= ( per1, per2, 0.0, 0.0, 0.0, 0.0, 0.0, 180.0, 0.0, 0.0, 0.0) % ------------------------- GRID ADAPTATION STRATEGY --------------------------% % % Kind of grid adaptation (NONE, PERIODIC) KIND_ADAPT= PERIODIC 3. Execute the SU2_MSH to output su2 grid with periodic halo element 4. Running the SU2_CFD using new su2 grid from step 3. However, there are two types of error are occurred at the last step. The first one is new halo element boundary surface cannot find associated element, the error information is "Checking the numerical grid orientation. The surface element (1, 10691) doesn't have an associated volume element. " This surface (1,10691) is a new boundary surface created in step 3. I have tested several grids for this case, and some grids could pass the step where the first error was occurred, but still cannot be start running. I think the second error is about MPI sending/receiving, the error information is segmentation fault when I executed the SU2_CFD in parallel. And the code can run several steps in serial execution, but the segmentation error will be occurred when the master node merge coordinates at solution writing out step. These are the errors and information I got using 3d rotation periodic BC, and maybe we can discuss about it. Thanks! |
Final report on modelling Wind turbine using SU2 and OpenFOAM
Hi All,
I've managed to put together the steps and settings for wind turbine simulation using SU2 and OpenFOAM. It also includes some validation for the mexico rotor. http://publications.tno.nl/publicati...018-R11648.pdf https://www.slideshare.net/slideshow...n9VMov6E11jeAd I hope you find it useful, Kind regards, Kishore |
Quote:
|
All times are GMT -4. The time now is 15:58. |