SU2 for Turbomachinery
 

Can we let this be the thread for all sorts of turbomachinery related questions?

My questions are:
If I wanted to do a 2-D blade to blade calculation (euler) I assume I would use the MARKER_EULER, MARKER_PERIODIC for the top and bottom but for the inlet and outlet I remember from the 2.0 release notes that there was mention of "New inlet-outlet boundary conditions". Can you describe what type of boundary conditions these are? Are they Riemann invariants, Thompson style characteristic or something else? I assume the config file options are still the same but for the INLET_TYPE = MASS_FLOW option what do you specify?

On a separate note for external flows is there an option to run to a fixed lift coefficient and if so how do you set it up? Are axisymmetric analyses now available for all governing equations?

Can you add some more Sample/Tutorials for internal flow/turbomachinery and free surface examples?

thanks

Thanks for getting this thread started - we are currently developing many of the capabilities required to perform complex turbomachinery simulations (including design), and much of this functionality is starting to come online.

To answer your first question, the improved inlet/outlet boundary conditions are indeed characteristic-based, and they use Riemann invariants to update the conditions at the inlet/outlet depending on the sign of the eigenvalues.

Along with the improvements to the implementation, we have also added the ability to specify mass flow directly (density & velocity components) in addition to stagnation quantities (total temp, total pressure, flow direction). The format for both is nearly the same and appears as follows in the template configuration file:

%
% 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= ( NONE )

By default, it is assumed that stagnation quantities are given at the inlet, unless the INLET_TYPE is set to MASS_FLOW. In this case, the density and velocity magnitude along with a flow direction are given as seen in the format specification above.

For the question concerning external flows (correct me if I am misunderstanding), we do have a type of convergence criteria that will terminate the computation once an integrated quantity such as lift or drag reaches a certain level of convergence (i.e., it stops changing more than a specified tolerance over a specified number of iterations). It is called the CAUCHY criteria and can be used instead of the default RESIDUAL criteria. This has been particularly useful in the past for design problems where one might be more interested in the convergence of some objective function rather than residuals (which can sometimes behave oddly).

The first tutorial in the online documentation contains some detail on the inlet & outlet BCs, and we will be adding more tutorials and examples to the documentation as we go. In the meantime, is there a particular case that you are interested in trying? We would be delighted to help, and perhaps it could become a test case for the rest of the SU2 community.

Yes. I may have stated it poorly. Other codes have the ability to target a given lift coefficient by varying the angle of attack or other means but I don't think SU2 has this capability or am I mistaken?

No, at the moment, SU2 does not have the capability to adaptively vary the angle of attack during a simulation.