[CUAero]

Hi all! It will be clear to everyone that I am fairly new to the CFD realm.

My research group has decided to use SU2 for full aircraft configuration CFD and more specifically Euler (so no viscous effects) just to get a ballpark of the CD/CL of the air vehicle to aid the conceptual design initial iterations.

I have developed a very complicated process for turning our in-house geometry into an STL which I am later meshing in GMSH to produce a Farfield-Body mesh as described in tutorials.

I am using the Euler solver tutorial CFG found in the SU2 website.

I have tried a lot of different things with regards to multigrids, CFL numbers, linear solvers etc. to no avail.
Very coarse meshes of around 50 to 100K volume elements usually converge but the finer the mesh gets residuals either stagnate or diverge after thousands of iterations.

I am trying to model full aircraft configurations of various civil and not configurations with nacelles and other attachments (intakes, stabilizers, canards etc).
I would greatly appreciate if someone could help me… I am stuck on this for months….

We also developed a separate mesh which does converge and I don’t know why.
According to the mesh quality metrics that SU2 outputs:

CONVERGING MESH
595030 grid points
3308915 volume elements
Orthogonality angle (deg.) Min 22.3508 Max 86.9945 >20
CV Face Area Aspect Ratio = Min 1.01667 Max 15448.7
CV Sub - Volume Ratio = Min 1 Max 190464

EXAMPLE OF NON CONVERGING MESH
182983 grid points
970152 volume elements
Orthogonality angle (deg.) Min 24.6522 Max 87.7547
CV Face Area Aspect Ratio Min 1.08176 Max 50.0858
CV Sub - Volume Ratio Min 1 Max 567.171


I am using SU2 7.5.1 ”Blackbird” and I am attaching both the mesh file and 2D mesh STL in case anyone wants to generate the volume mesh themselves.

Please find resources HERE because I was not able to upload them directly to the forum


Thank you all for any help, I trully appreciate it!!!

[bigfootedrockmidget]

Adding the settings below worked, it starts converging after 350 iterations and was pretty much converged after 1000 iterations. I used the Roe scheme since it converges very fast. I did a quick test with JST but that one did not converge with the setting below.

LINEAR_SOLVER_ERROR= 0.1 
LINEAR_SOLVER_ITER= 5 
 % 

MGLEVEL= 0

NEWTON_KRYLOV= YES 
NEWTON_KRYLOV_IPARAM= (10, 3, 2)  
NEWTON_KRYLOV_DPARAM= (1.0, 0.1, -6.0, 1e-5)  
% 
CFL_ADAPT= YES 
CFL_NUMBER= 10.0 
CFL_ADAPT_PARAM= ( 0.9, 1.05, 5, 200 )  
% 
CONV_NUM_METHOD_FLOW= ROE

[CUAero]

Thank you so very much for your reply and help!

I have tried this and it does converge at around 1000 iterations.

I am trying to come up with a sort of “universal” cfg for running any air vehicle at (ideally) any speed/AoA regime. For that reason, I have experimentally run the same mesh at M=0.5 / AoA=1.0 and it does converge at around 1100 iterations.

I tried M=1.5/ AoA=1.0 and its still going at 4000+ with the residual stagnated about -3.0.

I would like to ask, if there is anything I should adapt/change in the cfg depending on the conditions? I am also very lost when it come to the strategy I need to use.

How does one decide on which convective scheme to use? How does that affect the results.

Same for CFL, to me it appears that the lower the cfl is the more you “force” the solver to converge, but how does this usually affect the solution? Why not select the lest possible CFL all the time amd restrict the range to a minimum?

During the design process, aircraft models may need to be analysed at a wide range of conditions (e.g. +- 20⁰ and 0.1<M<3.0+) is that something we could realistically expect to get out of su2 in this mode?


All the help is extremely appreciated!! Best Regards and happy holidays!

[rn86j]

Originally Posted by CUAero

Thank you so very much for your reply and help!

I have tried this and it does converge at around 1000 iterations.

I am trying to come up with a sort of “universal” cfg for running any air vehicle at (ideally) any speed/AoA regime. For that reason, I have experimentally run the same mesh at M=0.5 / AoA=1.0 and it does converge at around 1100 iterations.

I tried M=1.5/ AoA=1.0 and its still going at 4000+ with the residual stagnated about -3.0.

I would like to ask, if there is anything I should adapt/change in the cfg depending on the conditions? I am also very lost when it come to the strategy I need to use.

How does one decide on which convective scheme to use? How does that affect the results.

Same for CFL, to me it appears that the lower the cfl is the more you “force” the solver to converge, but how does this usually affect the solution? Why not select the lest possible CFL all the time amd restrict the range to a minimum?

During the design process, aircraft models may need to be analysed at a wide range of conditions (e.g. +- 20⁰ and 0.1<M<3.0+) is that something we could realistically expect to get out of su2 in this mode?


All the help is extremely appreciated!! Best Regards and happy holidays!

Please could you share the gmsh input file for converting the stl file into a Volume mesh inside half Wind tunnel box
Thanks
rn86j

[CUAero]

Hello! The volume mesh script is nothing fancy just a simple physical surface definition and HTX selection. in a .geo script. Please see the code below:

Merge "2DMesh.stl";
Physical Surface("VEHICLE") = {3};
Physical Surface("SYMPLANE") = {1};
Physical Surface("FARFIELD") = {2};

Surface Loop(4) = {2}; // FARFIELD
Surface Loop(5) = {1}; //SYMPLANE
Surface Loop(6) = {3}; //VEHICLE
Volume(6) = {4, 5, 6};

Mesh.Algorithm3D =10;Mesh 3;
OptimizeMesh "Gmsh";
OptimizeMesh "Netgen";
Mesh.SaveAll = 1;
Save "OutputToSU2.su2";

[rn86j]

Originally Posted by CUAero

Hello! The volume mesh script is nothing fancy just a simple physical surface definition and HTX selection. in a .geo script. Please see the code below:

Merge "2DMesh.stl";
Physical Surface("VEHICLE") = {3};
Physical Surface("SYMPLANE") = {1};
Physical Surface("FARFIELD") = {2};

Surface Loop(4) = {2}; // FARFIELD
Surface Loop(5) = {1}; //SYMPLANE
Surface Loop(6) = {3}; //VEHICLE
Volume(6) = {4, 5, 6};

Mesh.Algorithm3D =10;Mesh 3;
OptimizeMesh "Gmsh";
OptimizeMesh "Netgen";
Mesh.SaveAll = 1;
Save "OutputToSU2.su2";

================

Thanks - but do not understand where the FARFIELD & SYMPLANE geometries ae introduced from in the geo script file. I understand the merging of the stl file .......

Part of difficulty in convergence may be due to blunt faces on the nacelle, Inlet and outlet.
For conceptual design work
Try your geometry with proper control faces and pre-specified flow values.

or perhaps as smoothed bodies

or as straight through open nacelles. You will need to introduce nacelle pylons connecting with the wing.
Complexity !! yes....
rn86j

[CUAero]

The physical surfaces are originally in the 2D mesh script. I agree that some nacelle blunt faces may introduce complex instabilities which may not be picked up by Euler but are enough to hinder convergence. Nevertheless, I have tried running it without the nacelle and got the same problems.

I am still trying to fuigure out how does one come up with a scheme strategy and how to fine tune it according to the flow regime and AoA to obtain convergence and accuracy (as much as possible).

This CFD run to estimate the aerodynamic coefficients will be part of an optimization process which will automatically run in a loop.

So ideally the user should not have to manually take care of the mesh and cfg every time.

So just to-reiterate the ROE scheme suggested above does work for the small to medium AoA at mild mach numbers (i.e. 0.5) but does not converge at higher and lower mach numbers.

I have used MGLEVEL =0 and NEWTON_KRYLOV parameters with HLLC at higher Mach numbers and looks like it is converging. Dont know for smaller M.

Still trying to figure out what sort of trategy to use. At this point I have meshed and remeshed the geometry so many times that I dont think its a mesh problem. Does the CV Face Aarea Aspect ratio affect convergence that much? This is the main difference with the "mostly convergent" mesh that we got.


Thank you all for yout time and help!!