[vignesh.sankarn]

Hi guys,
I am analysing a 3d full scale wing for a project and for some reason the values of Cl isn't decreasing. I am not able to obtain the stall point at all. The values keeps rising with alpha. Would really appreciate if someone could help

[sbaffini]

Stall is really about correctly computing a lot of stuff. It might be due to your grid, turbulence model, also probably needs some unsteady approach, certainly not wall functions, even inflow/outflow conditions, etc. etc.

You need to give us some more info. But, in general, it is something for experienced users in that specific field to correctly predict flow fields near stall conditions

[vignesh.sankarn]

Sorry about the lack of information. So I am trying to analyze a full-scale wing and study the lift and drag coefficients. I have a mesh with about 1.7 million nodes and I have also assigned an inflation layer based on the y+ range of 30-300. I am using K-e model realizable model and the issue I am facing is the coefficient of lift continues to increase with alpha with no signs of reaching a peak value. I am using an unstructured mesh for the analyses. I am not trying to study the flow characteristics near the stall but would like to understand at what angle stall occurs

[sbaffini]

The general idea is that you should pick up a reference paper that does something similar to what you're trying to do and you first try to replicate that. You can so learn how your code works for this sort of problems and devise a strategy for your specific case. You also learn the details of how certain problems are solved.

I still don't know how much wrong we are talking about here. Lift curve still linear at 45°, 20°, 15°? But a fully unstructured mesh (full tetra?) with wall functions and a k-epsilon model is a set of 3 wrong choices here. Also, you don't say this, but I suspect you might also be using a first order scheme.

K-omega SST, no wall functions (y+<1-2) and a structured mesh (at least near the wall) are the starting points for a good job here.

Of course, no wall functions implies, at least, a factor 10-30 more cells. So, the feasibility of all this largely depends from the why you're doing it. If it is for learning purposes, you could still do the rest of the improvements and stay with large y+ (might not get very accurate results, but should get the qualitative behavior)

[vignesh.sankarn]

So I am using second order scheme. and yes I am using a fully unstructured tetra mesh. I am doing this as part of my project work. The problem I am facing is with the mesh
I am not able to create a structured mesh on the surface. The quality of the mesh does down significantly when I apply an inflation layer as well. I am unable to improve it due to computational limitations. Yes the value of coefficient of lift is still increasing at 30 degrees. My free stream velocity is 70 m/s and my chord is 6.4m.

[sbaffini]

Let's start with the k-omega sst then. But I still suspect that the mesh might need improvements.

The point is that the stall part of the curve bends because the flow starts separating. So to get that correctly you can't get the viscous part at the wall wrong.

I am also wondering if you get the linear slope of the CL curve right, as getting a linear one all the way to 30° without separation suggests a very viscous solution

[vignesh.sankarn]

I have added a link to the graph that I obtained with the current setup
https://drive.google.com/file/d/1D6a...ew?usp=sharing

[sbaffini]

Could you also share a relevant contour section of the flow field?

You are indeed getting the stall, I think. Just, possibly, very wromg

[vignesh.sankarn]

https://drive.google.com/drive/folde...h5?usp=sharing
I have attached the contours for 30 degrees aoa

[sbaffini]

Ok, this looks definitely not like a stall, and seems wrong and weird to me. Try at least with the k-omega SST, and maybe try to have at least an uniform y+ all over the surface, possibly the low end (i.e., 50).

A relevant aspect here is also what boundary conditions you are using for the turbulence model at inlet. What sort of values you get for the turbulent viscosity ratio in the domain?

[vignesh.sankarn]

My inlet is a velocity inlet and outlet is pressure outlet and I have a symmetry condition on the near field and wall on the far field.
I do get the turbulent viscosity ratio exceeded 1e5 error whilst solving

[sbaffini]

What values are you using for k and epsilon at inlet and what is the resulting turbulent viscosity ratio? Does it stay so up to the wing or does it decay before reaching it?

Turb. Visc. Ratio limited at 100k may signal that something is wrong. Do you still have it at convergence?

I don't understand what you mean by near and far field. Top and bottom boundaries of the domain? Boundaries relative to the root and tip of the wing?

However, the flow looked generally plausible. You need to:

1) switch to k-omega sst with plausible inlet values for turbulent quantities and be sure that the inlet turbulent viscosity remains sustained up to the wing

2) improve mesh quality (the fact that you can't even produce a structured surface mesh for a wing just tells me how little effort you put on that)

3) possibly reduce y+ to be at least everywhere below 100

4) be sure to get fully converged results with no warnings on this or that

In general, you don't need to invent anything, just look for papers dealing with similar problems. Onera M6 is probably the most tested wing in CFD, just look for "RANS Onera M6" or variations on that

[vignesh.sankarn]

I have added images with all the parameters below to the link. The far-field is near the wing's tip, which is a wall condition. The nearfield is at the root of the wing and I have set that to symmetry condition. I have one major problem when it comes to the mesher. When I put my wing to a structured mesh, the inflation layer fails to generate on the surface. Do you have any suggestions for that?
I will also try running the k-omega model to see if that changes anything. Thank you for your suggestions.
https://drive.google.com/drive/folde...h5?usp=sharing