[anonygoat]

Hi!

I am trying to perform a supersonic compressor cascade simulation with CFX. My inlet is one blade of the cascade like this:


I have gotten some results that look good to me, such as with a supersonic inlet with Mach 2.5. I use transnational periodicity to simulate multiple (technically infinite, I guess) blades in a cascade. Here are the post-CFX results with a final transformation performed to show the multiple blades:


I have been trying to lower the Mach number, but have been issues getting convergence (cannot get an inlet Mach below 2.1 to work). I have tried much of the troubleshooting in the CFX documentation. I think a problem is that the blade geometry is too aggressive, it attempts to turn the flow too much.

I tried reducing the change in the blade geometry by 10 degrees to give a 10 degree change in angle (before the blade had a 20 degree change in angle):


This did not help with the convergence at lower Mach numbers, so I tried a wind tunnel (vertical configuration) to verify I am not messing up something simple. This works fine at inlet Mach of 2.5, 2.0 and 1.5. Here is the Mach contour for 1.5:


I then tried tilting the sides of the wind tunnel 70 degrees with the inlet and outlet horizontal still, leaving everything else in the configuration the same. I input the x and y velocity components manually (cos(20) and sin(20)) for u and v components) to make the flow hit the airfoil with 0 incidence angle. This run does not converge however. Here is an image of the geometry that does not converge at an inlet Mach of 2.5:


I do not understand why this image with the tilted wind tunnel does not converge and the vertical wind tunnel does. I realize that the inlet/outlet are normal in one case and not the other (and that this is the only difference I can think of between it and a direct rotation, and therefore the cause), but I don't understand why this matters. I could modify the geometry to have inlets normal to the sides, but then when I add a turn to the blade the sides would not be the same lengths and therefore I could not add a transnational periodic boundary condition.

Any thoughts on what I am doing wrong or why tilting the wind tunnel 70 degrees (and leaving the inlets and outlets horizontal) matters is appreciated! I can provide more configuration information, but everything is the same except the geometry file.
The two geometries.
Converges:

Does not converge:

[ghorrocks]

Transonic simulations are very difficult because the equations are elliptic in some regions and hyperbolic in others. Purely subsonic and purely supersonic simulations are much easier as they are all one class of flow and far more numerically stable. So this agrees with what you report.

Some of your other comments appear to agree with mesh quality issues. The more you skew the mesh the worse the quality becomes, and this will become very important especially for supersonic flows. It you redraw your geometry to improve mesh quality convergence should improve.

[anonygoat]

Got it, thank you!

I have not been paying that much to mesh quality for the different simulations (I have been using the same default element size for the geometries without assessing the quality from case to case). I will start refining the mesh!

Thank you again!

[ghorrocks]

Mesh quality and mesh size are different things. Don't get them confused.

When you skew your mesh you don't change the mesh size (well, you don't change it much, anyway) but you do affect the quality. Alternately, if you have a mesh and you subdivide the elements then you change the mesh size but the quality is unchanged.

[anonygoat]

I have looked at the mesh skewness for the case that is not converging and it doesn't seem horrible.

For the case that does not converge, the max skewness is 0.69738 and the average skewness is 1.96e-2 with a standard deviation of 6.09e-2.

The ANSYS 19.2 help says that 0.5 -0.75 is fair and 0.25 - 0.5 is good. It says that in 2D, all cells should be good or better. I know that CFX can't do true 2D... I'm guessing that I should aim for the 2D skewness goals (good or better) even though the model is 3D simulating 2D (1 cell thickness currently).

There are only about 4 cells that are fair. Could these be causing the problem still? Or is it possible that the shocks/interactions/flow near Mach will make it not converge regardless?

I am debating whether I should try to fix the skewed cells (not really sure how to go about this) or if I should try increasing the spacing/increasing the amount of distance upstream/downstream of the blade. Not really sure if this would help, but I feel like it would cause less complex interactions.

I tried the model in Fluent (have been using CFX due to past projects in CFX) but it does not seem to converge any better. I'm guess this means the problems I am having are because of the geometry/mesh and independent of the solver.

Any advice/recommendations are appreciated!

[ghorrocks]

The mesh quality comments in the output file are just a guide. Some simulations are not sensitive you mesh quality (and so work fine on pretty bad meshes) and some are highly sensitive. Transonic simulations are definitely extremely sensitive to mesh quality, and much more sensitive than the guide comments. If you want to really know your sensitivity to mesh quality produce a few meshes with different qualities and run them and see the difference in results.

I am debating whether I should try to fix the skewed cells

It is ALWAYS worth the effort to improve mesh quality. In cases which are difficult to converge and super-sensitive to quality it becomes imperative.

(not really sure how to go about this)

In your case a very simple structured mesh will produce an excellent mesh, at least in the cases you do not skew too much. For the heavily skewed geometries it will require some thought.

or if I should try increasing the spacing/increasing the amount of distance upstream/downstream of the blade. Not really sure if this would help, but I feel like it would cause less complex interactions.

This is an independent problem to mesh quality. For an accurate simulation you need the mesh quality to be acceptable AND the upstream/downstream distance to be correct. It is not one or the other, you need both.