lift, drag and moment coefficient of airfoil
 

Hi guys,
I'm trying to plot my data to agree with experiment one. Cl plot follows the trend but I think values are not close enough to experiment, so is Cd plot. How do I adjust? And I'm not sure how to calculate Cm. Can't figure this out, please help me, thanks.

I use SC/Tetra. Re=1e006, no. of elements=150,000. Have tried k-eps and SST for turbulent model.

Hi mate, I am new in this forum... So, can you be more specific? Which airfoil is it?
I am doing several airfoils in typical Reynolds numbers (3*10^6), of course in incompressible flow.
I may have very similar problems, my lift coefficient is ridiculously small as the angle of attack increases. Conversely, the drag coefficient increases dramatically off the experimental data as the α increases.
In fact my project deals only with symmetrical foils so I shouldn't worry that much, but I can not present so shitty results...
I compare my results to those from Xfoil and to the experimental results from Abbott's & von Doenhoff's book. Fluent gives cm as well (monitor - residuals), what exactly is your problem with cm?? You can also try Aerofoil version 2.2, the free version.
See if you can help me to get somewhat better cl without destroying my zero angle of attack results which are pretty cool.
The wall y+ for me just doesn't work, I've tried to get it as small as possible, only deteriorating my results. I use Spalart-Allmaras model, reference area based on the wetted surface area.
Try to be more specific, I might be able to help you (if you are still stuck there) If you can't help me, it's ok, cheers!

Pano,

what airfoil are you using and what Mach number ? Are you using the pressure based solver of the density based solver of Fluent ?

Do

Hi again, thanks for reply.
I am testing NACA0012, NACA0010-34, NACA64-012 and other similar foils.
My Mach number (for the verification process at least) is 0.1277.
Yes, I'm using pressure-based solver. This shouldn't matter me thinks. I've done verification for 4 original naca foils and in all of them the lift coefficient obviously has the trend line (to increase with α) but is so unbelievably small... I've tried different settings in Solutions - Controls and I have also tried other viscous models (k-ε and k-ω): almost the same shit...
i just need to do something to get higher lift coefficient without much changing my results at α=0.
Thanks in advance, hope you don't have to spend ur weekend in Fluent like me :-)

1. I suppose you know that for each alpha you must change the reference vectors in the force panels, otherwise (for alpha different of 0) you will not obtain the Cl and Cd but the A and N forces (axial and normal).

2. What value has your y+ ? You must keep this larger then 100 or lower then 1, intermediary values will give you a wrong solution.

3. For alpha=0 your Cl is zero for a symmetric airfoil (like NACA0012).

3. For such a low speed Mach=0.12.. you will have a large part of your airfoil in laminar flow, using a turbulence model for the entire flow domain will give you a wrong Cd. I suggest to use one of the turbulence model that account for transition (available only in Fluent 12).

Do

Hi Do, that was pretty helpful!
1. I sure change the vectors for the lift/drag directions.

2. My y+ is from 0 to 35. Originally it was from 0 to 250. After twto times adapting the y+ I reduced it. I saw no improvements in results. Should I just continue to adapting?? How many times do you usually have to adapt? Of course it depends on the grid, but I can;t afford adapting so many times each foil, I've got 30 of them in the project...
Or maybe do u think I should raise it instead of reducing it? Cos I tried but didn;t make it; I thought that if you only coarsen (and not refine), I would increase it, but again it was reduced.... Is there any quick approach to get it down or up???
I saw the derivation of this parameter by Nikuradse when he was establishing his semi-empirical formulae for velocity gradients in Boundary Layers, but I can't see any clear method on how to obtain optimum values for this Y+. Is it just by experience or is there any physical meaning relatively easy to grasp?

3. All my foils are symmetrical and yes (thank god) the Cl at α=0 is always zero, this is the only right result I get fro lift coeff.

4. Crap! I didn't know that. I actually didn't even know there is Fluent V12... my dept has only Fluent 6.3... Anyways I guess there is not much I can do about it then apart from some comments... Indeed I have large parts of laminar flow ... I innocently believed that those viscous models like S-A would somehow predict the transition point and would hence treat the laminar part as such.... In this case is there any method to estimate the error for not properly accounting the part of laminar zone??

Cheers,
Pano

2. You don't need to adapt for y+, you can make your grid from the start to keep a y+ of about 100. Use a y+ calculator for that (there are 2 here on cfd-online), you input Re, Mach, the desired y+ and you get dy which is the height of the first row of cells at the wall.

4. Yes you can account for the laminar part of the flow even in Fluent 6.3, you need to split the mesh in two regions: turbulent and laminar. See this article for an example:

Silisteanu, P., Botez, R - Transition-Flow-Occurrence Estimation: A New Method, Journal of Aircraft, Vol. 47, No. 2, March–April 2010

For determining the transition "point" you can use the method from the article or you can use as a first approximation Xfoil to get the transition point.

Do

Hi Do, thanks for sharing knowledge! you have really contributed effectively here.

1. So, I see my grid is simply redundant... It is very annoying though to see others getting cool results with the same settings and mesh. The grid basic spacing calculator gave a result of the order of 1e-06m which is extremely small, me thinks. I have a relatively dense mesh, (at least according to other experienced friends who have seen it) and it has 1e-03. This is a huge difference!! I don't think I can make a grid that dense, gambit is definitely going to crash and even if it doesn't, I don't think Fluent will ever converge!! I actually have some decent results now at least up to 2 degrees angle of attack. I remind you that in my project, I actually deal with zero angle of attack!!
But it’s a dissapointment, I never expected a simple case like a fucking foil to be so hard in fluent, with so much time i have already spent, I could have actually solved Navier-Stokes in matlab or Visual basic or something

2. Yeah the article you suggested is very interesting. I found one more; just in case it has slipped off your attention:
Greer D., Hamory Ph., Krake K., Drela M., 1999. Design and predictions for a High Altitude (Low-Reynolds-Number) Aerodynamic Flight Experiment, USA: National Aeronautics & Space Administration (NASA) & Dryden Flight Research Centre, Edwards, California.
I think block-structured grid is the way to define a laminar region up to the estimated point of separation!! haven't made it to work yet though.

Now apart from all these, I have one more question for you, I hope I'm not causing you much inconvenience: How do you define the reference area. because I only get meaningful results when A is based on the wetted surface i.e. the perimeter of the section times the depth which is one as the simulation is 2-d. this cd1 I used throughout all the verification process.
By doing so, however, it seems that the smaller the thickness-to-chord ratio the smaller the drag coefficient. This as you understand cannot be realistic as you would end up with very slim bodies which indeed have small viscous pressure drag but huge friction drag.
So, I decided to define a second drag coefficient cd2 which I would only use for the comparison and not for the verification process (i hope this thinking is not ridiculously stupid), then I get a meaningful results in terms of a drag coefficient which supposedly resembles the trendline of the drag force itself (which is essentially of interest to the designer). I find that for each family of wing sections if you keep reducing the t/c beyond a certain point the drag increases again in a roughly parabolic pattern, which is reasonable!
cd1 = D (per unit span) / (0.5ρ(V^2)P)
cd2 = D (per unit span) / (0.5ρ(V^2)sqrt(A))
Hence cd2 = cd1*P/sqrt(A).
P is the perimeter; P=2qc, c:chord length, q: factor to show how longer is the perimeter when developed relative to the chord length. A: the sectional area.
Note: All foils I have designed (some of them are original naca sections (from 4-digit, 4-digit improved and 6-digit series) some others are custom designs have the same section area A) I put it in square root, just to be consistent with units.
Is the thinking correct?????? How can I adequately justify that the drag coefficient that is matching the experimental data, Xfoil, Aerofoil and so on, fails to predict the actual drag force behaviour??
Please tell me if I am not describing things very well here or If you need more information on my case to give an opinion.
cheers,

Pano

Hi guys!

I am sorry for disrupting your discussing.

I would like to say something, hope this helps a little you guys.

The comparison between the experimental data and computational data for airfoil (wing) can be difference in magnitudes of Cd, Cl, especially in the post-stall region. However, the important thing is, in my opinion, the trends of Cd, Cl curves.

The magnitude of Cd, Cl can be difference because of the conditions of EXPERIMENT and COMPUTATION are difference, such as, the effect of the tunnel walls -- farfield in computation, the flow transition in the experiment --- fully developed turbulent in computation . . . Those can effect on your results of magnitudes.

So I think you should check the trends firstly and carefully, and then the magnitude of Cl, Cd.

The reference area for a 2D airfoil is chord*span, where the span is always 1! This is the definition, you can check a classical book like Milne - Theoretical Aerodynamics or Anderson - Fundamentals of Aerodynamics. For a 3D simulation you will use the actual wing span.

You can also obtain quantitatively good results (at least for Cl) on a coarse mesh if you impose a y+ of 100 (using Spalart-Allmaras). I suppose this was the approach used by your friends. Also you need to be sure that your Re from the simulation is the same as the one from the experimental data (keeping the same Re and M will ensure the flows similarity).

About using Matlab of VB to integrate the full NS equation good luck (you have no chance using these 2 languages). For DNS the mesh requirements are much worse then a dy of 1e-06. Your best bet if you want to implement a serious CFD code is Fortran 95, you can also use C++ but with a serious lose in accuracy.

You can successfully use Xfoil for this kind of calculation, however in order to get a better Cd estimate you need to know the turbulence intensity of your wind tunnel, from this you can estimate the Ncrit used by Xfoil to trip transition.

Do

Hi you all,

@ tanphong: I am happy to agree with you that the trendlines should dictate whether results are satisfactory or not, rather than the absolute quantities. Thanks for hints. I have fairly good trendlines for all coefficients:
- the cl increases according to a linear-like model and at 7 degrees it starts to get flat which is pretty much what i'm after even though the absolute numbers are for example 5 times smaller at 8 degrees (!!),
- the cm coefficient is very accurately predicted (I am saying very accurately given the values from Xfoil and Aerofoil, because in the experimnetal data you can't read much detail anyways)
- the cd is fairly accurate at 0 and 2 degrees of α and then it increases faster than experimental and Xfoil results. I do not worry very much about it though since I focus on the α=0.

@Do: ok mate, I was not speaking very seriously saying that I could program it, I know it's painful, but at least, in programming you know beforehand how it is going to be. In CFD you're kind of deceived; that following steps that have worked for others is going to be fine for you as well but... Don't get me wrong here, I don't mean I wanna escape the hard job, it's just that I can't really feel getting any benefit from employing CFD so far. Anyways this is not the point to discuss :-)

I agree that for the verification process, the area can be defined as c*span. This is how I started as well, then I noticed that the cd results were a bit more than two times the experimental ones, so as I was told I could define the area as two times the chord times a factor to account for the actual wetted length which essentially is the perimeter of the section.
BUT still when it comes to comparison, how can you account for the thickness, i.e. the thickness-to-chord ratio??? Because as i said if you use the cd based on the area as you suggest (c*span), you get misleading comparison, in that the less the t/c the less the cd until t/c tends to zero (flat plate). This is not true, the total drag force (viscous pressure drag + skin friction drag, free surface is assumed to be far away) does not behave like that!! Don't you agree that for comparison purposes and only one has to define a different drag coefficient?? something like the one I suggested previously??
I am dealing with a special case as I demand the profile area to remain contant for all foils, meaning that the slim sections for the same area and the same maximum thickness (same with those of bulky - full sections) but different chordwise distribution in the mean lines (a part of the comparison deals with such foils) have vary large "reference area'' because of their very long chord hence small cd. Up to a point this totally makes sense, but after that the skin friction drag increases dramatically and eventually dominates the viscous pressure drag, hence the drag force actually increases again... How could I capture this with the original cd you (and others) suggest???
have a nice day,
pano