If the incoming flow is uniform turbulence dies out. Turbulence needs a main flow velocity gradient to stay "alive". So my question is do you assume the main flow velocity to depend on the height (boundary layer profile)?

I kept the mean velocity at the inlet to be constant 10 m/s

Do you mean constant in time or uniform in space?

If you assumed a uniform profile (independent of the height) you should replace that by a typical atmospheric boundary layer profile U(z). The most simple model is a power (1/7) of the height (see http://en.wikipedia.org/wiki/Wind_profile_power_law).

Uniform in space. Actually this powerlaw can be used when I know the height from the ground right. In my case I just put a cylindircal domain around the blade. and I input velocity to be 10m/s at inlet and T.I 10%

It is much better if you have a good idea from measurements for your input turbulence intensity. 10% is usually used if there is no information about the inlet turbulent flow condition.you may also try the other option for the inlet turbulence condition, the turbulent viscosity.

Thanks Prof. Actually in the experiment conducted in NREL Phase VI turbine. Turbuelent Intensity maintained was 0.1%. I did the simulation for one turbine using it. Actually different atmopheric conditions have different turbulent intensity. These T.I has effect on Wake Recovery. So I'm trying to vary the T.I at inlet for a range from 0.1% to 10% to see the difference in wake recovery. But problem is whatever T.I (0.1% or 1% or 10%), it is damped to lower values around 0.0X(of order 1e-2). This is my concern is. why T.I I give at inlet is not maintained for free air

Typical rotor axis height will be 1.5 times the diameter. So you could try a power law (U/U0)=(h/h0)^(1/7) with U0=10 m/s and h0=1.5 D (D=diameter rotor). Just check whether your turbulence stays alive under these circumstances.

Which Turbulence model do you use and what starting conditions do you put inside the turbine? I ask this because it is usual (and correct) that as you vary TI this does not matter if the turbulence is generated or decays due to velocity gradients  within the main computational space . What is the geometry? 

I use SST K-omega model. I use hybrid initization in FLuENT.

My geometry is like attached.  

I suggest you define the velocity inlet in terms of height at the inlet and then define the intensity based on this velocity. Don’t go with the intensity defined in the Fluent. You can find the proper profile on the literature and for wind tunnel Also, the distance between inlet and blade is important to reach your desirable velocity and intensity just before blade.

For this geometry it is not justified.Please put a grid on the picture denoting inlet/outlet. Have you tried the standard k-e model? please do!

also see  a review by C.Argyropoulos and N.C.Markatos in Applied Mathematical Modelling June 2014  for SST and relevant

Hi Sir Thanks All But recently I got an idea. Might be tomorrow again I do my simulation with standard initialization with inlet.

I use Hybrid Initialization 

in which

Turbulence Settings

uses by default the domain averaged values for the turbulence parameters. If you want to use variable turbulence parameters you can deselect the Average Turbulent Parameters check box. When this option is disabled, then it calculates the turbulent parameters, such as kinetic energy, dissipation energy, etc., using local flow parameters. (http://www.arc.vt.edu/ansys_help/flu_ug/flu_ug_hi.html).

Since I have not disabled this option, it might not have taken local flow parameter, I set at the inlet

Good luck!

Ijaz,

I answered to you via LinkedIn too: this is not an error; It is the behaviour of k, Ti due to the turbulence-model/transport equation under a uniform inflow. There are some papers explaining why that happens and how to solve that (Spalart, P. R. and Rumsey, C. L., "Effective Inflow Conditions for Turbulence Models in Aerodynamic Calculations," AIAA Journal, Vol. 45, No. 10, 2007, pp. 2544 - 2553.). But perhaps the commercial codes do not have those options (www.refresco.org has it). K and Omega decrease/decay very fast with the distance while nu_t (EddyViscosity) not. And nu_t=cte K/Omega. You can play with Ti and EddyViscosity in order to get the correct K close to the turbine: decrease Ti and increase EddyVisc a lot and check K just 1c before the turbine and see the effect :-).

Good luck. 

Guilherme Vaz

hi all thank you so much. I got the issue of my problem solved. It is because of the viscosity ratio. I kept the ratio to be 10, which increased the omega, specific dissipation rate. When i reduced it, Intensity value is maintained

Hello Everyone,  I am also facing the same problem of TI decaying very fast. I am modeling the flow around 2D square cylinder and used k-e model. I made the model in ADINA and computed the values of k and e based on TI, length scale and mean flow velocity. I don't have the option of entering teh turbulent viscosity. So can you give some suggestions on how to solve this problem.

Hi I sort out of this issue by using UDF for creating atmospheric boundary layer.

Also pls once again have a look on Turbulent dissipation rate, if it is too high also it will lead to TI decay ......

Thank you for your answer Ijaz. I wanted to know if your user defined function for velocity was varying in only in space or also in time? Are the results also dependent on the turbulent model that we use. For example i tried the problem with spalart allamaras models also and found different results. 

Hi for my case I need to change velocity with altitude, I used K-Epsilon model as it is good for free stream

Pls have a look on TDR value at inlet, 

Thank you Ijaz. I will try to work out your suggestions.

For two-equation turbulence models, the turbulence related parameters set at the inlet will decay as it approaches the object. the decay rate is related to the Re, Tu, and eddy viscosity.

What this means is that turbulence intensity in your field depends of course on local conditions (air velocity, vicinity of solids ,irregularity of ground ,etc) and not on the inlet conditions. This is not an error. Indeed in most of my computations the turbulence generated/decaying inside the domain does not depend ,strongly at least, on its inlet value. However try and refine the grid, and ensure that the incoming parameters lead to 'eddy viscosity' say 1000*laminar viscosity.