How to using moving mesh scheme
 

Hi,

I read your paper in AIAA. It is mentioned that moving mesh scheme is available in SU2.
I am trying to solve a forwarding rotating problem.
The rotating frame in the cfg file and the case looks that it is only for steady problem.
I am wondering how to solve the transient rotating problem.
In the unsteady section, I see the type of mesh motion, and rigid motion parameters. How to use that?

Thanks.

Hi Sean,

SU2 is capable of performing unsteady simulations with dynamic meshes (both rigid and deforming mesh transformations). The rigid mesh motion capabilities are currently more advanced than those for the deforming meshes, although we are actively working in that area too.

To run a time-accurate simulation with a rigidly rotating mesh for the rotating NACA 0012 problem, you can use the following config options, for example:

% ------------------------- UNSTEADY SIMULATION -------------------------------%
%
% Unsteady simulation (NO, TIME_STEPPING, DUAL_TIME_STEPPING-1ST_ORDER,
% DUAL_TIME_STEPPING-2ND_ORDER, TIME_SPECTRAL)
UNSTEADY_SIMULATION= DUAL_TIME_STEPPING-2ND_ORDER
%
% Time Step for dual time stepping simulations (s)
UNST_TIMESTEP= 0.01
%
% Total Physical Time for dual time stepping simulations (s)
UNST_TIME= 1.0
%
% Number of internal iterations (dual time method)
UNST_INT_ITER= 500
%
% Mesh motion for unsteady simulations (NO, YES)
GRID_MOVEMENT= YES
%
% Type of mesh motion (NONE, FLUTTER, RIGID_MOTION, FLUID_STRUCTURE)
GRID_MOVEMENT_KIND= RIGID_MOTION
%
% Coordinates of the rigid motion origin
MOTION_ORIGIN_X= 0.5
MOTION_ORIGIN_Y= -32.0
MOTION_ORIGIN_Z= 0.0
%
% Angular velocity vector (rad/s) about x, y, & z axes (RIGID_MOTION only)
ROTATION_RATE_X = 0.0
ROTATION_RATE_Y = 0.0
ROTATION_RATE_Z = 8.25

Note that you will need to set your own physical time step, total time for the simulation, and a number of internal iterations for the dual time method. The important parameters here are the (x,y,z) coordinates for the center of rotation (MOTION_ORIGIN) and the rotation rate in radians per second (ROTATION_RATE). Please feel free to give this a try in the config file for the rotating NACA 0012 case, and don't forget to turn off the rotating frame option (ROTATING_FRAME= NO).

Cheers,
Tom

Thanks, Tom.
It works and help me finish my project.

There are two problems:
1. How to save the intermediate results, my step is 10, but I only get two results with _0 and _10.
2. How to output paraview .vtk file for domain flow in SU2 2.0.3?

There are two problems:
1. How to save the intermediate results, my step is 10, but I only get two results with _0 and _10.
2. How to output paraview .vtk file for domain flow in SU2 2.0.3?

Please try setting WRT_UNSTEADY=YES in the config file. This causes solution files to be written for unsteady problems with the frequency specified in the WRT_SOL_FREQ option. As an aside, the WRT_UNSTEADY option will likely be deprecated in a near-term release, but is needed for V2.0.3.

Starting with V2.0.3, we are no longer supporting the Paraview format directly and are working to provide CGNS format as our open format. Many visualization packages, including Paraview, can read CGNS files. The Paraview format is still available in previous releases of SU2, and further updates to the output routines are on the way in upcoming releases.

Cheers,
Tom

Thanks for the reply. I am looking forward to the formal release of new versions.

Might be worth mentioning in the web page describing the configuration file that the PITCHING_AMPLitudes should be given in degrees, not rads.

Hi Aldo,

Thanks for the feedback - a little more detail has been added to the configuration file template that can be found with the source code (config_template.cfg).

Hope this helps clear it up a little and cheers,
Tom

Hi, Tom

I have two questions,
1)
Can SU2V2.0.5 solve the RANS with moving mesh scheme.
I tried a case,
but the residual returns NAN.
I did not find the test case in the package.
Can you tell me how to do that.

2) I want the output file is cgns format.
But SU2_CFD can not be complied in parallel with CGNS support.
How to solve this problem.

Thanks.

Dear Sean,

This capability is in the process of verification and validation. We have recently been implementing and testing both the ALE and non-inertial version of the RANS equations (and their corresponding adjoint). V2.0.5 likely does not contain the updated (or validated implementations), but a version in the near future should. Please stay tuned...

We are still ironing out some of the changes to the I/O routines. A simple work around for the time being is to simply retain the restart_flow.dat file from the end of a parallel simulation, and then run the SU2_SOL executable separately (even in serial) to create a CGNS output file based on the solution data in the restart file.

Hope this helps!
Tom