[lint]

Hi, this is another post with another problem that i've been trying to resolve since i've started the modelling process.

The domain size is about 3x3km and the base size is 20m. I am using a roughness length value for grass as given in literature of 0.03m, which according to the Star help files is translated using E*z/C (8.75*0.03/0.25) to a roughness height of r=1.05. I then limit my first cell centroid height by using another relationship provided in Star: y >10z or y > 0.2r giving me a minimum value of 0.6m. Now i import a velocity profile using a xyz Table for a height of 1 to any number of meters and run the simulation. I have tried refining the mesh further as well as using different turbulence models with different wall treatments but every single time i exceed the turbulent viscosity limit. Visualizing the results I can see that the problem is occurring in the turbulent boundary layer (or maybe it is the inner boundary layer due to the roughness).

I have also tried manually calculating the initial boundary k-e values but that only leads to the whole region suffering from the problem rather than just the boundary layer. I have searched the forums and there are some solutions proposed, but most of them suggest mesh refinement which has not worked for me. Additionally my wall y+ values are around 2500 at a minimum!

I'm at a complete loss as i don't understand the nature of the problem so have no means of finding a solution. Am I missing something? Should I be setting other parts of the boundary in relation to the custom velocity profile rather than let it develop on its own. If so are could you list some sensible values for reference as I'm not sure where the ballpark is.

Any help would be forever appreciated, thank you!

[ggulgulia]

hey lint

Atmospheric boundary layer problems are best solved with LES turbulence models since atmospheric phenomena involves large and in principal anisotropic eddies, which are not taken into consideration by K-e turbulence models. The larger eddies, apart from being a isotropic in nature, also interact and extract energy from the mean flow and their behavior is dictated by the geometry of the problem and the boundary conditions as well.
The k-e models (RANS Model to be more general) the collective behavior of all eddies by so called averaging the effects of Reynolds stresses for the flow field.

I would suggest you to thoroughly go through the LES turbulence modeling in STAR CCM+ manual to understand the suitable meshing strategy for your case

[yannaos]

Hi lint,

If we exclude typical modelling errors, you may be surprised to discover that your problems could come from the value of the limiter. Such value---I think 1e5---should be Reynolds-number-dependent. In other words, there are physical flows where the turbulent viscosity ratio could be over those limits. You can find a nice explanation in the Spalart, Rumsey article, link below, page 6 of the article.
Practically, you can do the following test: multiply the limiting value by 100 and continue to run the calculation. Check if the limiter warning appears again or disappears.
If it dissapears then this is a strong indication that your limiter was too low. If, on the other side, the warnings, never end, then recheck your model again.
In both cases, use a threshold to look for the cells with highest turbulent viscosity ratio for checking cell geometry and inspecting physical fields.

http://arc.aiaa.org/doi/pdf/10.2514/1.29373

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.

Hope it helps,

Yannaos

[lint]

ggulgulia -

Thanks for your advice, I have considered using the LES model but the goal of my project is to achieve a low cost model of a "known error" as it has to be automated and run through many input wind conditions. At this stage i just want the solution to converge with results that are at an acceptable level, i've seen many papers that manage to do this but unfortunately they don't explain how they did it.

yannaos-

I did find that the limiter is far too low. Using flat plate boundary layer theory as reference my Reynolds numbers are in the 2*10^9 region. Increasing the limit by one order initially solves this error. I have thought to obtain the correct boundary conditions by running the simulation several times and parsing the output to the input. However the region initial conditions(which i don't believe i have set correctly) limit the efficiency of convergence and eventually the turbulent viscosity grows out of control again.

I tried another way. I scaled the mesh down by a factor of 100. I also scaled the velocity and roughness length by the same factor. The solution converges very slowly but some of the results don't appear to be of the right order. For example the y+ value is now 0.004 instead of 2500, since it is a non-dimensional value i would expect the result to remain constant.

[Muzz]

I had the same problem when modeling environmental flow in an urban environment. Apart from refining your mesh size, you also have to increase the viscosity ratio limit to about ~1x10^9.

I had the most success using the boundary conditions outlined in this paper:

"Validation of CFD Simulations of Wind-Driven Rain on a Low-Rise Building Facade" B. Blocken, J. Carmeliet (2007).