Hello everybody: I am trying to obtain the drag force for a NACA0012 airfoil (2D model) and I get the drag over predicted compare to the experimental data (for about 30% or more) even in angle of attack of zero! The problem is with the viscous drag which is really over predicted. Although it looks a very simple problem, but I am not able to obtain an acceptable drag for turbulent flows. I have ensured the following facts:

1. The Reynolds number matches the experiments and is not in transition Reynolds numbers (Re=2-5 million) 2. I have used all the turbulence models and wall functions available in 2ddp solver 3. I am using a fine grid close to the airfoil and I keep the y+ value in the proper range for different wall functions 4. I have verified the reference values 5. I am using a very high quality structured grid with a maximum skewness of 0.12 6. The domain is large enough, so it has no effect on the flow field around the foil 7. The flow is incompressible (M=0.085). Both pressure farfield and velocity inlet have been tried.

I really appreciate it if anyone can help.

Thanks

Yasser

Q: How the drag is calculated? A: Integrating the wall shear stress over the area Q: How the wall shear stress is calculated? A: Using the law of the wall

check your Y+, adapt your mesh using the Y+........... You are the one in control of the solution,

Experience is gained by asking the right questions and searching for the correct answers (i.e. you have to read books about fluid dynamics, the help system, user guide,....etc.

Hi Ahmed: Thanks for your help. In fact, I am keeping a proper y+ by using the adaptation, but it still does not work. Apparently, the shear stress is very large around the leading edge. Do you have any idea that helps more? Thanks again

Yasser

I strongly advise you to dump this practice of adapting by y+ value, IT'S NO GOOD! Why? Because hanging-node adaption in structured meshes generates high cell volume gradient and irregular point distribution exactly where you need very uniform grid: BOUNDARY LAYER! What is the effect of this? Increased numerical dissipation. Already drag prediction is very hard to obtain even with excellent meshes, so making this kind of mistake is strongly not recommended.

USE A UNIFORM (constant, low growth ratio, max 1.1) GRID IN B-L!!!

y+ mean value must be near 1. Do not bother about low values for y+ at the leading edge, it is more important to have the correct value of y+ from 25 to 100 percent of chord.

Anyway, I must warn you that even if you use such a mesh, the best precision you can expect is around 20 percent! This is not a problem of FLUENT, this is an all CFD softwares problem.

Good luck, Razvan

You say you are calculating the drag force, and it is a 2D problem, in this case, FLUENT takes a default reference depth of 1.0 M (you can change this value) in order to calculate areas. May be you need to check that parameter such that you are comparing the drag on the same areas. If this is not the case just forget what I have written.

Hi Ahmed: The thing is that if you increase the depth the drag would increase. The drag force you get from FLUENT is the drag force per unit depth. By the way, when you non-dimensionalize the forces, it would be independent of area. Thanks for your help again.

Yasser

Hi Razvan: Thanks alot for your help. In fact, I am using a Boundary Layer with a growth ratio of 1.05 but I still get the drag high. If I could get the drag something like 20% off, I would be satisfied!

Now, I am suspicious to the leading edge. When I plot the skin friction coefficient over the foil it is a huge jump on the leading edge and it becomes relatively low after like 20% of the chord. I do not know the reason of this phenomenon anyways.

Do you know what does Fluent do in cases that the flow is laminar at the begining of the foil and becomes turbulent on the foil? I mean the flow over the foil includes the laminar, transition and turbulent flow? Because if the flow is laminar on the leading edge, the skin friction would be much lower and we may get rid of this high drag. I do not know to what extent you agree with me. I appreciate your response.

Yasser

There is no turbulence model in Fluent capable of predicting transition from laminar to turbulent. All models are exactly what their name says: turbulence models. They are valid only in turbulent flows. But, they can be used for jobs like airfoil drag prediction, with proper care.

The problem could be just that: friction coefficient in laminar flow is significantly lower then in turbulent one. So, accurately predicting transition might solve the problem of overpredicted drag.

In Fluent, there is an undirect way to achieve this: forced transition. If you know the exact position of the transition point on the airfoil for a specific flow regime, you could split your grid in Gambit in two different fluid regions: one around the airfoil's leading edge, from inlet to the transition location, and the second from the transition location to the outlet region. Then, in Fluent you will specify that the first fuid zone is a laminar zone, and the other will be turbulent by default. You got it now: practically, Fluent deactivates turbulence model in the first zone, forcing it to be laminar! It is pretty simple, but you must know precisely the transition point. The main disadvantage of this approach is of course the need to redefine grid zones if you would like to change Re or even the angle-of-attack!!

Also be carefull about turbulence boundary conditions at inlet regions. For example, if you specify turbulent viscosity ratio (TVR) to be 1 and use S-A model or SST-kw, you will notice that TVR does not increase immediately on the airfoil! At Re=5*10^5, TVR starts increasing only at about 10% of chord lenght. This could be interpreted as some kind of transition, isn't it?

You might also consider trying LES or even DES. I never used them for this kind of job, so I cannot tell you exactly if they are better or not. But my guess is YES.

Razvan

Searching in my old case data base, I found a NACA 0012 airfoil. It is a 60.000 nodes, fully structured mesh of a real, experimental profile (with trailing egde thickness). I found out that the best turbulence model with this mesh was actually SST-kw (low-Re variant)! (I couldn't remember it anymore!!!). Experimental Cd at Re=500,000 is 0.06, and the result obtained with SST-kw is 0.07625. That's about 27 percent error. Not bad, but that was all I could get then.

Razvan

Hi Razvan: Thanks alot for your help. Do you think that because the Re=500,000 and there is a transition on the foil, the drag is over predicted? for higher Reynolds numbers, the problem persists? Thanks again,

Yasser

Naturally, as Re number increases, transition lenght should decrease and the flow over the airfoil come closer to "fully turbulent" assumption. So one guess would be that CFD drag prediction should improve at higher Re numbers.

Razvan

Hi,

It was very informative.

if you have a airfoil data for analysis can you share it.

It will be of very thankfull to you.

Could you be more specific? If you are asking me for experimental transition data for an airfoil, I'm afraid I cannot help you. Sorry.

Razvan

HI!

CFD almolst always overpredicts the drag of airfoils. It is very good at predicting lift (pressure forces) and bad predicting drag (viscous forces). Try RSM for modeling turbulence and Low Re approach for the boundary layer.

Reagrads MATEUS