[Publicity]

Hello. I am an undergrad student (year 1) beginning my studies as an aerospace engineer. I started using SU2 about a week ago and have gone through the tutorials. I am using gmsh and have created my own mesh for an oblique shock example.

The angles I have been testing are 10º - 35º with increments of 5º. The simulation converges for small angles but diverges when I go to above 20º (at 20º the RMS plateaus at around -3). The inlet conditions are specified in my config file.

MACH_NUMBER= 2.0
MARKER_SUPERSONIC_INLET= ( inlet, 300.0, 100000.0, 695.4290761825, 0.0, 0.0 )
MARKER_OUTLET= ( outlet, 10000.0 )

I noticed that there are some angles at which MACH 2 is not sufficient to generate an oblique shock. I have tried to use a higher mach number (up to 10). Furthermore, I have tried to use a progression of 1.05 to make the mesh finer around the ramp.

Below is my gmsh geo file. Thanks for your help!

// Gmsh project created on Sun Jul 28 20:22:19 2024
lc = 1.0;
//+
Point(1) = {0, 0, 0, lc};
//+
Point(2) = {0.5, 0, 0, lc};
//+
Point(3) = {1.5, 0.3640, 0, lc};
//+
// 1763
// 2679
// 3640
// 4663
// 5774
// 7002
Point(4) = {1.5, 1, 0, lc};
//+
Point(5) = {0, 1, 0, lc};
//+
Line(1) = {1, 2};
//+
Line(2) = {2, 3};
//+
Line(3) = {3, 4};
//+
Line(4) = {4, 5};
//+
Line(5) = {5, 1};
//+
Curve Loop(1) = {5, 1, 2, 3, 4};
//+
Plane Surface(1) = {1};
//+
Physical Curve("inlet", 6) = {5};
//+
Physical Curve("outlet", 7) = {3};
//+
Physical Curve("wall", 8) = {4, 2, 1};
//+
Transfinite Surface {1} = {5, 4, 3, 1};
//+
Transfinite Curve {5, 3} = 201 Using Progression 1;
//+
Transfinite Curve {4} = 151 Using Progression 1;
//+
Transfinite Curve {1} = 51 Using Progression 1;
//+
Transfinite Curve {2} = 101 Using Progression 1;
//+
Mesh.RecombinationAlgorithm = 1;
Recombine Surface {1};

Mesh 2;
Mesh.Format = 42; // specifies the .su2 format
Mesh.SaveAll= 1; // 0= No (default), 1= Yes
Save "tutorial.su2";

[R.K]

Its difficult to comment, why its not converging without the config settings. Looking at the mesh, I assume you are using the Euler solver. Supersonic flows usually require a low back pressure, I think yours should be fine, but you can try reducing it further or use the 'MARKER_SUPERSONIC_OUTLET'. For the numerical scheme use the JST scheme to start with, then play around with the upwind schemes once JST converges. You could also change the top 'wall' boundary condition to a farfield condition. I would also change the top boundary condition to a farfield condtion rather than wall. For the Euler solver, this wont have a big difference, but may help.

[bigfootedrockmidget]

People have a limited amount of time. But it takes less than 2 minutes to download a mesh and a config file, inspect it and run it and see if something is off. You can also post pictures, that takes even less time to inspect.
Sometimes that's all the time it takes for somebody to find an issue. Anything more complicated than changing a setting requires more analysis. You should make the effort for the reader as small as possible, especially when they are not engaged in the conversation yet.

[Publicity]

Originally Posted by bigfootedrockmidget

People have a limited amount of time. But it takes less than 2 minutes to download a mesh and a config file, inspect it and run it and see if something is off. You can also post pictures, that takes even less time to inspect.
Sometimes that's all the time it takes for somebody to find an issue. Anything more complicated than changing a setting requires more analysis. You should make the effort for the reader as small as possible, especially when they are not engaged in the conversation yet.

Thanks for the advice. I will post the mesh and config file as a file attachment next time.

[R.K]

Currently, the top surface is a wall making the shock reflect off it, If this is what you are trying to simulate, you may need to play with the domain as the outlet is too close to the reflection point.

If you are trying only simulate the oblique shock forming on the wedge, keep the top surface (Line 4) to be a farfield condition (MARKER_FAR). This change alone gets the simulation to converge in under 900 iterations. With a few more changes you can get it to converge much quicker, best I could do was 104 iterations (on 18 cores):
1. Use BCGSTAB for the linear solver, this will allow you to use a much higher CFL number for JST. You can find more information about linear solvers here: https://su2code.github.io/docs_v7/Li...econditioners/
2. Set CFL_ADAPT to YES, you can monitor what the average CFL number being used is if you add AVG_CFL in your screen output
3. You can play around with the NEWTON_KRYLOV parameters to make it even faster.
4. Lastly, set MARKER_PLOTTING /_MONITORING to 'wall', this will give the lift and drag values.

[Publicity]

Originally Posted by R.K

Currently, the top surface is a wall making the shock reflect off it, If this is what you are trying to simulate, you may need to play with the domain as the outlet is too close to the reflection point.

If you are trying only simulate the oblique shock forming on the wedge, keep the top surface (Line 4) to be a farfield condition (MARKER_FAR). This change alone gets the simulation to converge in under 900 iterations. With a few more changes you can get it to converge much quicker, best I could do was 104 iterations (on 18 cores):
1. Use BCGSTAB for the linear solver, this will allow you to use a much higher CFL number for JST. You can find more information about linear solvers here: https://su2code.github.io/docs_v7/Li...econditioners/
2. Set CFL_ADAPT to YES, you can monitor what the average CFL number being used is if you add AVG_CFL in your screen output
3. You can play around with the NEWTON_KRYLOV parameters to make it even faster.
4. Lastly, set MARKER_PLOTTING /_MONITORING to 'wall', this will give the lift and drag values.

Thank you so much! I tried out your suggestions and things converged quite well. I added some progression to my mesh, changed up some far fields. I didn't do anything with the NEWTON_KRYLOV parameters, I'm studying them now.

However, now when I try for higher angles and higher mach numbers, I am starting to see divergence again. I am going to see if I can use pressure / velocity far fields instead of a supersonic inlet. Not sure if that will make any difference.

[R.K]

If you are increasing the wedge angle and Mach number, the shock will become detached from the wedge quicker; you can check any aerodynamics book for a chart which shows at what angles shocks detach.


But given that you have 2 walls on the bottom (one completely horizontal and one for the wedge), the shock probably can't separate; because of the horizontal wall. I would extend the domain so that the wedge is hovering in the domain like an airfoil is simulated, rather than connected with a wall. You can also push the far field further to see the shocks fully develop. The cost shouldn't increase too much with this.