I want to study the flow (of air) around (and inside) a football stadium. Can anyone tell me which turbulence model would feet better for this case? I know that the turbulence models affect the results, so I tried to figure out from POLIS the wright one but.....

I think its KEMODL but I'm not sure..... PLEASE HELP.

INFO ABOUT THE SIMULATION (maybe usefull)

-I use a big domain , and at the center I've put the stadium. At two opposite sides of domain I've put the Inlet (10m/sec X) and Outlet.

-I want to simulate the flow of air around and inside stadium, and to see if velocity (for the strongest wind) can exceed 2m/sec (which is the air-speed that below it the records are recognized in some Olympic games)....

It is best to start with the standard high-Re k-e model plus wall functions. If there are large regions of flow separation, then make further simulations using the Chen-Kim and RNG variants of the k-e model. The standard model tends to produce too high a turbulence level in separation and recirculation regions. For flow around buildings and other wind-engineering applications, the Kato-Launder and MMK variants of the k-e model are also popular. These models are expected to appear in the next release of PHOENICS. They are somewhat similar in performance to the Chen-Kim and RNG k-e models.

thanks for your reply...

I will test them and if I have a question I will post it here .....

thanks again

dear Mike,

Thank you for your suggestions. What are the recommended values of YPLUS for these models.i.e for which of those models , the first grid should be in the laminar sublayer and for which it should be in the log layer. If there were Blockages in the domain,how to ensure that all nearby nodes are consistent with the TM. Further, YPLUS is sometimes defined as a function of wall shear stress and in some literature is defined as a function of CMU and SQRT(K). What is its significance ?

RAMANI

Strictly, high-re closure models using wall functions should locate the first grid point in the range y+ = 30 to 150. However, this is not always possible due to the geometry and/or the nature of the flow. This criterion for the applicability of the wall functions is based on experimental data from classical attached boundary-layer flows, and serves only as a guideline.

For low-Re models, which do not use wall functions, the first grid point must be located around y+ equals unity and 4 or 5 points are needed in the laminar sub-layer (y+ < 11.5). More information can be found at the following web address:

http://www.cham.co.uk/phoenics/d_pol...d/enc_t344.htm

The use of friction velocity for the velocity scale in the y+ formula implies that the turbulence is in equilibrium, as in attached boundary-layer flows. For the case where the turbulence is removed from equilibrium, as in separating and reattaching flow, Spalding devised a so-called generalised, but I would call non-equilibrium, log law in which the friction velocity is replaced by a measure of the fluctuating velocity, i.e. SQRT(KE). When the turbulence is in equilibrium the form of the non-equilibrium wall-function formulae collapse to the equilibrium formulae.

Dear Mike,

Thanks for your clarifications.

Just one more point.

For high re KE (std KE) TM, how many nodes are needed to resolve the Boundary Layer and how to know the BL thickness (DELTA) in PHOENICS. Any Standard GROUND coding available for this ?

RAMANI

Strictly, I would say that for a reasonable solution at least 10 nodes are needed across the boundary layer with a streamwise cell size of about 30% of the boundary layer width. For grid-independent results you will need probably something like 30 nodes and 10% of width. If you are dealing with a classical flat-plate boundary layer, then the parabolic option with an expanding mesh is the best option. Otherwise, the elliptic method is used and depending on geometry you may need a much finer mesh to resolve the growing boundary layer all along the surface.

The calculation of the boundary layer thickness can be done in Group 19 Section 6 of GROUND. The formula used depends on how the boundary layer thickness is defined, which is somewhat arbitrary, e.g. a thickness based on 99% of the free stream velocity could be used as the criterion. The displacement and momentum thickness are more readily defined, as I guess you must know.

There is no standard GROUND coding, mainly I suppose because apart from the uncertainty about definition, the actual coding would depend on the solution method used (parabolic or elliptic), the geometry, and the alignment of the coordinate axes.

Dear Mike,

Thanks a lot.

RAMANI