[ivanbuz]

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.

[jack1980]

@ 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.

[makaero]

@ jack1980

Thnx...

[harrislcy]

"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?

[jack1980]

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!

[harrislcy]

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

[AndyR]

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

[ferranpm]

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

[jack1980]

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!

[cfd seeker]

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

[LexMedina]

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.