Hello! I am using Ansys/flotran and Star-cd to calculate lift and drag characteristics of NACA airfoil. I have experimental NACA results which are obtained in wind tunnel. My Clift coefficients are at a very good agreement with NACA's, but Cdrag are not. At the angle of attack (AOF) of 0, I have variance about 20-30% higher than NACA's. Increasing AOF leads to higher variance, so at AOF of 6 my Cdrag twice as much than NACA's. Maybe somebody could explain why does it happen? Why Cdrag increase? I try to use finer mesh, but sometimes it leads to increasing Cdrag. I try to relocate finer mesh areas over the domain and sometimes it leads to descrease Cdrag (which is good), but it's not close enough to NACA's result. I think there must be theoretical explanation of this fact. It's like an extra force, which increases aerodynamic resistance

what is your Reynolds number?. Can the codes you are using handle this flow regime appropriately?

What is the Reynolds number ? What turbulence model are you using ? What is the spatial accuracy of the scheme ?

Re=2,1*10^6. I don't use turbulence model. I initiate laminar flow, because at my angles of attack there is no turbulent flow (no stall). Moreover, turbulent model leads to worst results (no Clift or Cdrag coincidence). Codes I am using can handle this flow regime. Spatial accuracy: about 0.5 mm along the surface of 2D profile (I solve it in 2D), about 100 mm on domain wall

Try to find AIAA Drag Prediction Workshop material, they are available in the Internet

At that Re you will have turbulence along the airfoil. I guarantee that there was turbulence in the experiment. If your turbulent results don't agree with experiment, then you probably have errors in the implementation of the turbulence model. And turbulent flow is not the same thing as stall.

agree with ag. it's important that you first understand the physics. next understand capabilities and limitations of whatever code you are using. otherwise, just garbage in, garbage out.

Turbulence is located in boundary layer. There is no boundary layer separation => no stall (before approx. 16 degrees). In ansys/flotran I can't change turbulence options along airfoil, I can set only model for the whole domain (k-epsilon, for example). In star-cd results are in good agreement with standart NACA roughness plots, but not with smooth airfoil plots.

I understand psysics very good. I don't know what equations about boundary layer does flotan use . I couldn't find a word about boundary layer in flotran references. In star-cd I tried to vary almost all boundary layer characteristics, but didn't achieve coincidence with NACA's smooth airfoil.

You may understand the physics fine, but if you're trying to match drag of a flow that is going to be turbulent with a laminar simulation then you'll never get good agreement. The skin friction is entirely dependent on the turbulent nature of the bundary layer regardless of separation. A laminar simulation of a turbulent flow will never get you where you want to be.

There is a problem I can't understand. What does 'smooth airfoil' mean? I am sure, that there are small vortexes along airfoil caused by microscopic roughness on airfoil surface. Can I assume, that microscopic rougnness lead to turbulence in boundary layer??? If it is, then what's the difference between the turbulence I described above and turbulence caused by NACA's rougnness strip on 0.08 of chord? The purpose of this strip is to initiate turbulence in boundary layer, but as I described above, the surface of airfoils is not ideal and there already have to be turbulent flow. Another problem is that it's difficult to find proper method to describe one or another flow in finite-element soft. As I know, boundary layer model in star-cd can describe processes in boundary layer caused by microscopic roughness, but I don't know is this model suitable for above mentioned NACA roughness strip... therefore, I don't know what to match and with what

The roughness strip is designed to trip the BL and force transition from laminar to turbulent. It is used in wind tunnel testing to ensure a better match with flight, where the small tunnel scale makes it difficult to match Re. Using current CFD models the best approach is to assume fully turbulent flow over the entire airfoil unless the Re is low enough to guarantee true laminar flow (say 10000 to 100000). In real life at 2x10^6 the flow will be turbulent over most of the airfoil, and the assumption of turbulence over the entire airfoil will not introduce a lot of error. The bigger issue is how well the turbulence model your code can model the turbulent boundary layer and provide a good accounting of skin friction. One thing you can try is to separate the computation of drag into a pressure-based piece and a piece due to skin friction. See if you can find some data to compare the two pieces and see if that will give you some insight into how the code is performing. You can also look for data on the velocity profile in the turbulent boundary layer on the airfoil, or run a simulation over a flat plate to quantify how the turbulence model is performing.

In wind tunnel it is very easy to match with flight (take 60mm chord airfoil and 50m/s velocity and air - you'll get Re=2*10^6). Strip is used to improve stall characteristics of airfoils at low speed. It is a big question: what happens in boundary layer?. As I said earlier, there are microscopic roughness at the surface of airfoil and it generates small vortexes => we have turbulence in BL, the question is how big turbulence and how can it influence on drag and lift. If we increase sizes of roughness, we'll get bigger vortexes and at some point these vortexes will become so big, that it make great contribution to drag. The question is at what size of roughness we can assume that the BL is turbulent? Have you ever heard about laminar profiles? They are designed to be laminar at high Re (70-80% of along chord we have laminar BL).

I guess you have experienced that drag prediction is not that simple. You lift coefficient is quite accurate, because lift has very little to do with viscosity and turbulence (as long as the flow is attached). Even potential flow will give you a pretty good estimate on the lift, for a low enough angle of attack. The drag of an airfoil is much harder to predict, because it depends so much on the behavior of the boundary layer, which has to be partly "modeled" and those models are all prone to failure, unless wisely tuned. First of all you need to know (or model) the point of transition. Then you need an accurate turbulence model, which does not only predict the shear stress accurately, but also a possible separation! So these are the parameters you need to get right: Laminar shear stress before transition, location and extent of transition region, shear stress within the transition region, shear stress in the turbulent part, extent of the turbulent boundary layer until a possible separation point, shear stress in the separation region... possibly a reattachment point, and of course you need the correct pressure distribution. Why am I telling you this? To lower your expectations a bit. This is not at all simple, compared to the prediction of lift. I am also telling you this to point you toward the variety of issues that you have to address to find out what the problem is. What other information do you have from the experiments? Pressure distributions would be very helpful. Do you have them?

Now I understand why is it some difficult to predict drag. I have a lot of experiments in ansys/flotran and star-cd. Flotran is too easy - there are very simple tuning for boundary layer in flotran. Changing properties of BL leads to very big scatter of drag (2-3 times more and less from real value). I have pressure distributions over the whole domain and it's quite plausible expect for some instability in pressure on the top surface of the airfoil. Unfortunately I don't know how to get plot of pressure along the surface in flotran. I tried to change mesh sizes. Sometimes results are absurd - more cells for high pressure gradient zone, more difference in drag from real value. In star-cd I read theory reference for BL. There are a lot of models of BL and non of them lead to stable results. Change the size of BL from 5 to 5.1 mm and you'll get divergent solution. Pressure distributions in star-cd are quite well. My question is still unanswered: turbulent models of BL, such as k-epsilon, can model small turbulence, initiated by microscopic roughness. Can I compare results obtained with these turbulents models with NACA's results obtained with roughness strip. Strip initiates turbulence in BL, microscopic roughness initiates too, but in a less degree. How to correlate all this? What can I get from pressure distribution? I mean I can get something of course, maybe you will tell me something that I don't know

About the roughness strip: As you said, the purpose is to initiate transition to turbulent flow. The development of the turbulent boundary layer behind the strip, however, will depend more on the free stream and the pressure distribution than on the strip. We usually don't consider the actual roughness in the computation. Knowing the position of the roughness strip, you have an approximate location for transition, which you may use in your computation. Most turbulence models should be able to handle this unless you have strong separation (which you wouldn't expect at low angle of attack).

About the pressure distribution: If you have noticed a large change in drag depending on your boundary layer, this will most definitely be visible in the pressure distribution. In particular, you will be able to identify separated flow as a pressure "plateau" in the distribution. Compare your computed pressure distribution with the experimental one. A close match should be regarded as a necessary requirement (though not sufficient). Even if your pressure matches, you may still have errors in the shear stress (not visible as pressure), but check on the pressure first. If the pressure distribution doesn't match, you will certainly not get the right drag. You can then try to identify the problem (e.g. too much separation --> turbulence might be too weak).

You said that we usually don't consider the actual roughness in the computation. Does it mean, that I can computate airfoils at low angle of attack using laminar algorithms and forget about turbulent ones? Let's take smooth airfoil. On 30-40% of chord (doesn't really matter where) the BL becomes from laminar to turbulunt. What is the reason of this? Microscopic roughness? Or small separation caused by high Re with following turbulent reattachment? I don't know how to model the fact of existing laminar and turbulent BL along profile simultaneously. Should I point the location of BL transition to soft by myself? Or turbulent models can handle it theirselves?

Turbulence is a flow stability problem. Even over a perfectly smooth airfoil, the laminar flow will be unstable at high Reynolds numbers and become turbulent. You can think of the roughness strip as the "straw breaking the camel's back". It's not really the roughness strip that's responsible for the turbulence, and it's not the roughness that determines the level of turbulence. It just acts as a trip wire to trigger the flow instability that otherwise would take effect a little further downstream. The purpose of the strip is to control the position of the transition, so that you can use that information in your CFD analysis. Depending on the turbulence model, you may be able to specify laminar flow over the front part of the airfoil, and use the turbulence model only downstream of the transition point (the location of the roughness strip). How this is done (if possible at all) really depends on the model.

However, in your high Reynolds number case I would not worry about transition too much. You should be able to get reasonable results by assuming that the flow is fully turbulent, using the model over the entire airfoil. Do that first, and compare your pressure distribution with the experimental data, to identify any discrepancy. It is important that you use the correct Reynolds number in your computation and that you provide the necessary grid resolution in the boundary layer.

Your comment "The purpose of the strip is to control the position of the transition, so that you can use that information in your CFD analysis" is a bit misleading - the strip is there to stop the flow separating near to the leading edge (a by product of this is that you can use this information to fix the separation point in CFD). This is needed to reduce the drag and the possiblity of stall - without the strip you would have to contend with the problem of laminar separation and abrupt turbulent reattachment (not a very nice problem).

Very true, there are real practical reasons for roughness strips besides providing a predictable transition location to help code evaluation. I still suspect the latter purpose is dominant, here, because this 2D airfoil study is probably not for some real-world application, but an experimental survey with the purpose of providing a reproduceable database with clearly defined parameters such as transition location.

But let's stay focused on helping DAK565656 do his CFD, and for that purpose it's a matter of fixing the transition location.