[harrislcy]

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

[jack1980]

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.

[harrislcy]

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

[jack1980]

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

[harrislcy]

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

[jack1980]

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...

[jack1980]

http://img222.imageshack.us/img222/4323/mesh.jpg

[jack1980]

http://img256.imageshack.us/img256/9554/gambit.jpg

[Chris D]

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.)

[makaero]

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!

[makaero]

see the attachments

[harrislcy]

Originally Posted by Chris D

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.)

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

[jack1980]

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

[Chris D]

Originally Posted by harrislcy

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

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!

[harrislcy]

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!

[Chris D]

Originally Posted by harrislcy

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.

[makaero]

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.

[harrislcy]

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.

[makaero]

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?

[harrislcy]

"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?