Comparison the airfoil 0012 experimental result and simulation result
 

Dear Fluent user,

Great to found this forum.
I have some doubt here, i have done the simulation for the NACA 0012 and NACA 4415 different AoA by using Fluent. With the airfoil chord length 1m, Re = 3e6, SA.

I tried to compare the simulation result with the airfoil NACA0012 and NACA 4415 wind tunnel test experimental data which found from a book "Theory of Wing Section" wrote by Ira H. Abbott.

For the lift coefficient, the comparison between two data are quite close and error no more than 10% for all AoA. However, drag coefficient no seem good, the difference of the experimental result and simulation are more than 50% or even more when in higher AoA.

Meshing quality is around 100k and meshing method used is O grid method 2d.

Any users here ever have this experience before?Kindly share with me what is the reason to have such a divergence between both data.

Thanks

CY

Solve > Controls > Solution
Are you calculating 1st upwind? Setting to 2nd upwind is likely to reduce cd by some 50%

2nd upwind already?:

Model > Viscous
Using k-epsilon turbulence model, you could check wall y+. Under Plot XY, plot wall y+ along your profile. If y+ < 5 use Enhanced Wall Treatment. If 30 < y+ < 300 use Standard Wall Treatment. For 5 < y+ < 30 or y+ > 300 you might try redoing your mesh.

For 5 < y+ < 30 or y+ > 300 you might try redoing your mesh.May i know why?

Sure. Wall y+ is a dimensionless indicator of the position of your first cell in the boundary layer. See:
http://www.fluent.com/software/unive.../turbulent.pdf

Hope that will help. Also, your boundary layer might improve by using a structured mesh around your foil. Gambit has a boundary layer tool for this. For example have a look at the top part of:
http://www.cfd-online.com/Wiki/Image...eshdetails.jpg
(This has Re 2e6, chord 1.2 m, boundary cell width 1.7 mm, wall y+ 52+17, standard wall function.)

It appears you're not the first finding same lift but higher drag, for example (p. 11):
http://www.ecs.syr.edu/Faculty/elhad...%20Airfoil.pdf

I'm only learning about this subject myself, so there might be other options. Still it is an interesting and 'wanted' validation case for the cfd-online wiki. Please let know if your results improve!

Good luck

Same result
 

Hi jack1980

I had did the way you told me, however i found that wall y+ for both simulations are in range 450 - 10. Is that acceptable range?

Even i used 2nd order up wind, the result is no change much, some of them even worse.

i try to refine the meshing to higher cell but it seems no helping much.

even k-epsilon turbulence model have a poor drag coefficient result.

May i know how you build the mesh on your airfoil? do you have any sample? what i did is similar to the fluent tutorial, i ever try other meshing method like tri pave, around 200k cells created, but same poor result.

And how you set up the simulation?

Thanks

Hi,

Friday I ran in to a friend of the aerospace faculty, he told me he uses the Spalart-Allmares viscous model.

I have set up a quick model in Gambit/Fluent for the NACA 0012, 0 deg, Re=3e6:

- The experimental cd is some 0.0060 to 0.0064, depending on the experiment.

- The mesh is shown below. It is a structured C-type mesh. Since the 0 deg problem is symmetric I only modelled the upper half. I took 100 cells along the foil (from other models I would estimate the drag to have converged to an order of 1% for this number of cells). The mesh is a first try and could certainly be inproved. The length of the foil is 1 m, the width of the first cell at the foil boundary is 2e-5 m (this is 'a' in the 'Create Boundary Layer' dialogue). To get a nice boundary layer I have created a 'blow up' foil around the actual foil, shown in blue in the last picture. In retrospect this might not be necessary.

- The main Fluent settings:
Define > Materials: density = 1, visc = 1e-6
Define > Boundary Conditions > Inflow: v = 3 m/s
Define > Boundary Conditions > Side: Specified Shear = 0 Pa
Define > Models > Energy: on
Define > Models > Viscous: Laminar
Solve > Controls > Solution: Pressure standard, others 2nd upwind
Iterate some 50 times
Define > Models > Viscous: Spalart-Allmaras
Solve > Initialize > Patch: Turb Visc = 0.001 m^2/s
Iterate some 100 times

Here I have kept all other Spalart-Allmaras settings to default. Note that the drag is especially sensitive to the inflow conditions.

- The resulting average wall y+ = 1.3 (min = 0.3, max = 1.9). This should be small enough for the Spalart-Allmares model to resolve the laminar sub layer.

- The resulting cd = 0.009. Which is indeed still to high...

Will add pics later, sorry...

Since you're using a turbulence model, you assuming that the flow is turbulent everywhere. In the experiment, however, there is both laminar and turbulent flow, unless the boundary layer is tripped at the leading edge. Could this explain why you're overpredicting drag with the simulation? (I.e., you are overpredicting drag because you are simulating laminar flow regions as being turbulent.)

Cp plot
 

Good job guys....Jack1980 and harrislcy

The interesting news is im on the same track, as in my case geometry is wing with Naca2412 section, Ctype Structured mesh, 200K cells (Gambit)

Fluent: Inviscid model, Pre-farfiled BC, Re-5.7e6
trying to validate my wrk with the values given in plots of Cl, Cd and Cm frm theory of wing sections book.

I got thee corect Cl value, but very less drag coeff. for zero deg AOA, I need to run case for diff AoA.

How to solve the prob with corect Drag coeff. and do u guyz no how to plot Cp on airfoil Crs-secn?
As in my case i created a plane intersecting wit wing, i need cp dist only on top and bottom surfaces of airfoil, im unable to draw a ployline like wing and airfoil intersecn.

and if u guyz progress wit ur wrk let me know, thnx.
Good luck! :)

see the attachments

Ya, may be you are right, but how are we going to do with this situation? just using the laminar flow in the simulation? How about when deal with the high AoA, which model are we suppose to used? That's good to try tripping a boundary layer at the leading edge, see how the output is, thanks

That makes sense! The laminar cd = 0.003, the k-epsilon cd = 0.009. The experimental is in between. Assumed Enhanced Wall Treatment would resolve this, wrong assumption.

Why not compare calculated cd to experimental results with a 'trip wire'? Then you're sure that the experiment is fully turbulent, such that turbulence model is ok. For example:
[img=http://img217.imageshack.us/img217/945/tripwire.th.jpg]

Shows that at Re=3e6, although the 'regular' fit is around 0.007, the 'trip wire' fit is around 0.009.

http://ntrs.nasa.gov/archive/nasa/ca...1988002254.pdf

Since FLUENT can't predict transition, you can divide the airfoil into a laminar zone and a turbulent zone at the point where the Reynolds number, based on distance from the leading edge, is around 5e5. (Unless you experimentally know the transition point. Then, use that instead.) Under the boundary conditions panel for the laminar fluid zone, click the "Laminar Zone" checkbox.

I've never actually tried this, so I'm not sure if it will work. So good luck!

No good Result
 

Every suggestions for getting a better drag coefficient has been tried but regret to said that unable to get the better result for a greater aoa then 0 degree. Zero aoa are able to get the value close to error 10%, but other aoa still seem no good, any professionals are able share your methodology to getting a correct Drag Coefficient by using Fluent?

I exhausted with trying Fluent to get the closer Drag Coefficient.....help!

Is your y+ in the correct range? For the S-A model, I think it should be from 1-5 or 30-300.

Is your y+ in the correct range? For the S-A model, I think it should be from 1-5 or 30-300.............


yes most of the y+ values are >= 30, in my case
AoA= 4deg
SA model
but fluent over predicts Cd by 80% and Cl is close by 5%

Plz see the Y+ plot.

Thnx a lot.

ya, most of my simulation's wall Y+ are in range 30-300.but still no able to get the good drag coefficient, 80% i think is to much, 10% is just acceptable.

im annoyed by trying all the combinations to get corect Cd.

It is closer for 0deg, but as AoA increases Cd is much far away from wht it is.

In BC's>wall>momentum>Roughness contant-->by default this value is 0.5
it is mentioned in fluent tht this value is given for smooth walls and it shud not be zero, wht if we give it as 0<K<0.5

does it reduce drag?

"absolute pressure limited to 1.000000e+000 in 24668 cells on zone 2 "

When i simulate my model with k-epsilon, this sentence pop up, what is that meaning?how do i solve this so that i can use k-epsilon for my simulation?

try LES
 

you guys may want to try LES. I did some airfoil flow simulation. though Cl and Cd are not important in my cases, I did simple comparison and they match experimental data pretty well. I guess the reason is that LES deals with the transition from leminar to turbulence pretty well.

But surely the computation cost is much much higher. parallel computation is needed for LES.

@ Makaero: roughness constant 0.5 is fine for flat plate, would expect to be ok for airfoil. However, it only takes effect when your roughness height is sufficiently large. So just converge your solution for smooth foil (ie rougness height = 0) and then try, say, roughness height of 0.0001 m. Roughness height is the diameter of the roughness grains on your surface.

@ harrislcy: Maybe the following will work? First converge your solution with 1st upwind laminar model. Then (do not initialize) for 1st upwind k-e. Finally (again do not initialize) for 2nd upwind k-e.

@ jack1980

Thnx...

What is this?
 

"turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 2 cells "

What make this happen? Is it the meshing problem? How to solve it?

Sorry, should have told, that happens oftenly.

Before running k-e calcs, do the following:

Solve -> Initialize -> Initialize ...
Do not press Init! Scroll to the box containing Turbulent Kinetic Energy and write down the value. Press Close.

Solve -> Initialize -> Patch ...
Variable = Turbulent Kinetic Energy
Value = value you've written down
Zones to patch = fluid
Press patch

This should help, good luck!

error...
 

Error: divergence detected in AMG solver: temperature

Again, another error opup again when in the K-ep silmulation. This happen after 200 iterations. How to avoid this?Thanks

Inflow Boundary
 

Check your inflow condition.
Make sure that the inflow is a close to laminar conditions as possible. Core flow of wind tunnels is generally turbulent, but at a very small intensity and length scale. This depends on the tunnel of course. Look at what the viscosity ratio is just downstream from the inlet. Except at tunnel walls (if you modeled them). It should be less than 1. A good quiet tunnel might have a turbulent viscosity ration of less than .1

Learned this the hard way myself
- Andy

Hello people!

I want to test the profile NACA 0012 for differents alfa and compare the results with experimental and XFoil graphics. It should be simple, but my results are not satisfactory:

ro= 1,225 Kg/m^3
Mu_air=1,75*10^5 Kg/(m*s)
D=1

with these Data, i obtain the differents velocities (in m/s):

Re=200K -> vs= 2,8
Re=500k -> vs= 7,102
Re=3M -> vs=42,612
Re=6M -> vs=85,224

For alpha= 0°and different viscosity theories:

RE=6M
Spall. Alm. /// K-E Stndrd /// K-w SST Trans.flow /// X-Foil(=Exper.)
cd 3.31*10^(-2) /// 6.2*10^(-2) /// 3.32*10^(-2) /// 5.08*10^(-3)


RE=1M
K-E RNG /// K-E Stand (Ehn. W.T.) /// K-w SST Trs.fl /// X-Foil(=Exper.)
cd 2.1*10^(-3) /// 3.24*10^(-3) /// 1.73*10^(-3) /// 5.4*10^(-3)
RE=200k
Spall. Alm. /// K-E RNG /// K-w SST/// Trs.flow /// X-Foil(=Exper.)
cd 6.4*10^(-5) /// 1.5*10^(-4)/// 3.14*10^(-4) /// 1.02*10^(-2)



For Low-Re I thought that K-omega sst could be better than K-Epsylon, but I don't see a good result...anywhere :( (the mesh is good, from the profes.)


Thank you for your help!




Ferran

Hi, you might be having trouble with the transition point. I think there are two approaches:

- Move from xfoil to experimental data with a ' trip wire '. This should fix the transition point near the leading edge. Now you can really use a turbulence model in you entire domain.

- If you want to stick with the xfoil data: try running viscous as well. If the exp. data is somewhere between your viscous and turbulent (for examp. rke) results, you might want to look into fixing the transition point manually. This can be done by splitting your grid in a viscous and a turbulent part.

Good luck!

hey all of you try k-w turbulence model. This works best for airfoils

Hey guys,

I am having the same problem with Fluent here. I am an aeronautical engineering bachelor's student and as part of a research project I am first simulating the flow around a NACA0012 with 0 AoA.

My Reynolds is about 1.0 e4, and my Cd should be around 0.037.
First I tried to use a K-Omega SST, but after reaching 1.0e-7 residuals, my cd is still 0.13. I tried also S-A, and the cd drops to 0.05, but my continuity can't converge to less than 1.0e-4.
Since it is a symmetric airfoil, the Cl should be zero, but now is around 1.0e-5 for S-A and 1.0e-3 for k-W SST.

I used all the standart settings. Also, my Y+ is in the range 1.0 to 1.4.