[kartonvcvete740]

Greetings friends! I have a problem reproducing the experiment (https://www.cfd-online.com/Wiki/RAE2822_airfoil), although the task is quite simple. I do not get results similar to an experiment, in particular the pressure distribution over the wing surface. This can be seen in the graphs. To put it in simple words: A shock wave does not want to form on the surface of my model, although it should be there, and I understand that.

For the SST turbulence model, I chose the y + parameter in the range of ~ 1.5-2.5, I tried other turbulence models (and the y + parameter), the result does not change. How much does this situation depend on the fact that my grid is not structured (I think that taking into account the number of cells this does not play any role at all except the calculation speed)? Could this be the main reason? I attach screenshots in which you can see my settings. Thank!

[ghorrocks]

Please attach your output file.

But some comments on the information you have posted:
* You have the viscous work option selected. It is not going to be significant so turn it off.
* You have transitional turbulence selected. This case is going to be fully turbulent so turn it off.
* You have a very rapid change in mesh size from the inflation layers to the bulk mesh. If you look at your reference wiki page you will see the transition there is far more gradual.
* To get shock waves you need a material properties model with variable density. I cannot confirm you have done this correctly - that is why you need to attach the output file.

[kartonvcvete740]

Thanks for the answer! I apologize for not immediately attaching the desired file.

[ghorrocks]

You will also probably need to use double precision numerics.

What does the mesh look like in the area where you expect the shock? You will need a fine mesh to resolve the shock, a coarse mesh will blur it.

[kartonvcvete740]

Today I thickened the grid, and also made changes to the settings you mentioned above. The result can be seen in the images. I understand that it is not structured and perhaps I cannot get high accuracy with it. Then why, when increasing the speed to a value of 247.86, I get a distinct shock wave, both on the upper and lower surfaces of the profile. Pay attention to the screenshots, there is no shock wave on the grid of 4.5 million elements, and two shock waves of 1.5 million elements. Think the matter is in the grid? Using a ICEM CFD fix the situation?

[ghorrocks]

You will have the explain what you are doing better for us to explain the differences. I don't know what conditions those images were taken from. Details are important, things like the mesh size, convergence, numerical scheme and all sorts of other details are important. But remember the forum is not suitable for detailed analysis of problems. The forum works best to answer specific questions. Open questions like "why are these different?" are not really suitable for the forum.

The only comment I can make at the moment is that CFX can only model a shock spanning 3 to 8 elements due to the way it does the numerics. It cannot model a shock as an instantaneous change. So you need to make sure your mesh in the area of the shock is fine enough that 3 to 8 elements is a small enough distance that you will capture the shock sharply enough for you to be happy. The image of the mesh you show has the mesh getting pretty coarse as you travel away from the foil, and that means the shock cannot be resolved sharply.

[kartonvcvete740]

In a previous post, I provided images in which I get a shock wave using a similar grid. I'll try to build a grid in a ICEM CFD.