[Luca S]

Hi,

I'm studying an inviscid flow (air) on a blade, which is supposed to be one of a series of blades tested in line (instead of rotating). The mesh is unstructured and created with Pointwise (.su2 format).

I would like to know which kind of configuration file to use and how to set a translational periodic condition for my test.

The inlet and outlet conditions are:
- pressure inlet (153960 N/m^2, 348 K )
- pressure outlet (100000 N/m^2 )

See the attached mesh file, where you can find the boundary conditions inlet, outlet, blade, per1 e per2. The distance between the the upper wall (per2) and the lower wall (per1) is 0.71.

Thank you.

[Luca S]

I tried to adapt the configuration file inv_channel.cfg (from the testcase named 'inviscid bump in a channel'):

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Euler wall boundary marker(s) (NONE = no marker)
MARKER_EULER= ( blade, per1, per2 )
%
% Inlet boundary marker(s) (NONE = no marker)
% Format: ( inlet marker, total temperature, total pressure, flow_direction_x,
% flow_direction_y, flow_direction_z, ... ) where flow_direction is
% a unit vector.
% Default: Mach ~ 0.1
MARKER_INLET= ( inlet, 348, 153960.0, 0.8667, 0.5, 0.0 )
%
% Outlet boundary marker(s) (NONE = no marker)
% Format: ( outlet marker, back pressure (static), ... )
MARKER_OUTLET= ( outlet, 100000.0 )
%
MARKER_PERIODIC= ( per1, per2, 0, 0, 0, 0, 0, 0, 0, 0.71,0, per2, per1, 0, 0, 0, 0, 0, 0, 0, -0.71, 0 )


Then I use this mesh file and configuration file to run SU2_MSH as:
SU2_MSH inv_channel.cfg

The output is a new mesh (by default named mesh_out.su2).

Finally I change the input mesh file in the configuration file as:
MESH_FILENAME = mesh_out.su2

Setting 1000 iterations and running 'SU2_CFD inv_channel.cfg' the solver doesn't converge.

Any suggestions?

Thank you.

[Luca S]

I solved the convergence problem setting the convective numerical method Lax-Friedrich:

% -------------------- FLOW NUMERICAL METHOD DEFINITION -----------------------%
%
% Convective numerical method (JST, LAX-FRIEDRICH, CUSP, ROE, AUSM, HLLC,
% TURKEL_PREC, MSW)
CONV_NUM_METHOD_FLOW= LAX-FRIEDRICH


However I can't see the periodicity after plotting Mach contours. See the attached config file that I used and the Mach number contours obtained.

Any ideas?

Thank you.

[salvovitale]

Dear Luca,

specify periodic like this:

MARKER_PERIODIC= ( per1, per2, 0, 0, 0, 0, 0, 0, 0, 0.71,0)

remove the periodic boundary from the MARKER_EULER because what you actually are imposing in you simulation is that your periodic boundaries are symmetry BC and not periodic.

MARKER_EULER= ( blade, per1, per2 ) should be MARKER_EULER= ( blade)


I think if you do this modification your test_case should run also with other schemes and converge to a periodic solution.


Regards


sv

[Luca S]

Hi Salvo,

first I changed the periodic marker, providing the first half of my specification, i.e.,

MARKER_EULER= ( blade, per1, per2 )
MARKER_PERIODIC= ( per1, per2, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, -0.71, 0.0 )

the solver runs but I still can't get a periodic solution.

Then I tried removing per1 and per2 from the euler marker,

MARKER_EULER= ( blade )
MARKER_PERIODIC= ( per1, per2, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, -0.71, 0.0 )

but the solver diverged,

Iter Time(s) Res[Rho] Res[RhoE] CLift(Total) CDrag(Total)
178 0.058369 33.818948 53.467412 -10000.000000 -10000.000000
179 0.058366 33.941822 53.670406 10000.000000 -10000.000000
180 0.058334 34.259249 53.921974 10000.000000 -10000.000000
181 0.058336 34.467027 54.351889 10000.000000 10000.000000
182 0.058333 34.671664 54.904520 10000.000000 10000.000000
183 0.058332 35.136916 55.283411 10000.000000 10000.000000
184 0.058324 35.175393 55.373995 10000.000000 10000.000000
185 0.058325 35.527664 55.746049 -10000.000000 -10000.000000
186 0.058322 35.907650 56.116415 -10000.000000 -10000.000000
187 0.058316 36.114722 57.074697 10000.000000 -10000.000000
188 0.058312 36.495260 57.216966 -10000.000000 -10000.000000

!!! Error: SU2 has diverged. Now exiting... !!!


Thank you very much for your answer.

[salvovitale]

Could you post you cfg file and the original mesh before you run SU_MSH so i can have a look and see what is the problem.

sv

[Luca S]

Dear Salvo,

here you are the config file that I use before running SU2_MSH and the original mesh.

Thank you

[LaSerpe]

Luca I think Salvo means that he needs the SU2 mesh file not the image.

cheers

g

[Luca S]

Sorry, I hope this is the mesh file you wanted.

Thank you.

[Luca S]

I'm trying to adapt the attached config file.

I run SU2_MSH and get the periodic mesh, then when I run SU2_CFD I get this error:

------------------------- Geometry Preprocessing ------------------------
Setting point connectivity.
Renumbering points (Reverse Cuthill McKee Ordering).
Recomputing point connectivity.
Setting element connectivity.
Checking the numerical grid orientation.
Identifying edges and vertices.
Computing centers of gravity.
Errore di segmentazione

Any ideas?

[Luca S]

I modified again the config file 'turb_vki.cfg', I set:

% ------------- DIRECT, ADJOINT, AND LINEARIZED PROBLEM DEFINITION ------------%
%
% Physical governing equations (EULER, NAVIER_STOKES,
% TNE2_EULER, TNE2_NAVIER_STOKES,
% WAVE_EQUATION, HEAT_EQUATION, LINEAR_ELASTICITY,
% POISSON_EQUATION)
PHYSICAL_PROBLEM= EULER
%
% Specify turbulent model (NONE, SA, SA_NEG, SST)
KIND_TURB_MODEL= NONE

% -------------------- BOUNDARY CONDITION DEFINITION --------------------------%
%
% Navier-Stokes wall boundary marker(s) (NONE = no marker)
MARKER_EULER= ( blade, per1, per2 )
%
% Inlet boundary type (TOTAL_CONDITIONS, MASS_FLOW)
INLET_TYPE= TOTAL_CONDITIONS
%
% Inlet boundary marker(s) with the following formats (NONE = no marker)
% Total Conditions: (inlet marker, total temp, total pressure, flow_direction_x,
% flow_direction_y, flow_direction_z, ... ) where flow_direction is
% a unit vector.
% Mass Flow: (inlet marker, density, velocity magnitude, flow_direction_x,
% flow_direction_y, flow_direction_z, ... ) where flow_direction is
% a unit vector.
MARKER_INLET= ( inlet, 348.0, 153960.0, 0.8667, 0.5, 0.0 )
%
% Outlet boundary marker(s) (NONE = no marker)
% Format: ( outlet marker, back pressure (static), ... )
MARKER_OUTLET= ( outlet, 100000.0 )
%
% Periodic boundary marker(s) (NONE = no marker)
% 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, ... )
MARKER_PERIODIC= ( per1, per2, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, 0.0, -0.71, 0.0 )
%
% Marker(s) of the surface to be plotted or designed
MARKER_PLOTTING= ( blade )
%
% Marker(s) of the surface where the functional (Cd, Cl, etc.) will be evaluated
MARKER_MONITORING= ( blade )

I attach the config file and the results obtained running SU2_CFD (without creating the periodic mesh).

Thank you.

[salvovitale]

I tryed to run your cases and I also got some troubles. I think the problem is the quality of your mesh. Look at the images attached and try to imporve the mesh.

cheers
sv

PS good that you start as a template from the turb_vki.cgf

[Luca S]

Dear Salvo.

I try to correct my mesh. In the meantime I attach the last config file that I'm using (without running SU2_MSH). I think it works well.

Thank you very much.

[Luca S]

Salvo, I created a new mesh with the corrections you suggested. However I can run SU2_MSH only removing per1 and per2 from MARKER_EULER, and then when I run SU2_CFD I get again this error:

------------------------- Geometry Preprocessing ------------------------
Setting point connectivity.
Renumbering points (Reverse Cuthill McKee Ordering).
Recomputing point connectivity.
Setting element connectivity.
Checking the numerical grid orientation.
Identifying edges and vertices.
Computing centers of gravity.
Errore di segmentazione

I attach the new mesh file.

Thank you

[Luca S]

To get results with the new mesh I created running SU2_CFD (without creating the periodical mesh), I have to change the Convective numerical method from ROE to LAX-FRIEDRICH

CONV_NUM_METHOD_FLOW= LAX-FRIEDRICH

I attach the new results.

Thank you.

[salvovitale]

You cant get a periodic solution without running SU2_MSH, because you must first create a periodic mesh with halo nodes on one side. With this new mesh I get to drop down 2 order the residuals. However, I think with that trailing-edge it s pretty difficult to get a good convergence with an Euler solver. Anyway your case now works and you can start build up on that. You may still improve your mesh though.

Attached my working cfg file. Change the name of the mesh on the config file, run SU2_MSH, then change again the name of the mesh file and run SU2_CFD.

cheers

sv

[Luca S]

Thank you very much Salvo, I try to work on this to get better residuals.

[Luca S]

I tried to run the viscous case (running SU2_MSH and SU2_CFD) and this time the vki turbine config file worked very well.
I attach the results and the config file.

Of course I modified also the mesh (see attached image) creating a structured zone around the blade.

[Luca S]

Does anyone know if the pressure coefficients values I get in both inviscid and viscous cases are ok?

Maybe it is a pressure coefficient definition problem?

Thank you

[Luca S]

How can I scale the mesh with a scale factor of 0.048?

Thank you