CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Calculation of a cube (bluff body) (http://www.cfd-online.com/Forums/fluent/28501-calculation-cube-bluff-body.html)

Sepp May 3, 2001 11:27

Calculation of a cube (bluff body)
 
Hi everybody,

I try to calculate the flow around a cube (building) sited in a atmospheric boundary layer (ABL). Additional I carried out measurements in our atmospheric windtunnel. The experiments are similar to those of Castro & Robins (1977). My results agree with the values in the literature. My problem is that my numerical simulation can't reproduce die pressure distribution at the surface of the cube. Especially my pressure coefficient cp=(p-p_ref)/(rho*u_ref^2/2) at the front side is greater then 1!

Is there anybody who had the same problem??

Hope to hear from someone

Sepp

Regert May 12, 2001 09:20

Re: Calculation of a cube (bluff body)
 
Hello Sepp,

Unfortunately I don't know the solution for this problem but I have met it. I think, that the applied boundary conditions can cause the problem. How do You model the buliding? Have You made a half building using a Symmetry in the vertical middle plane? In my case two symmetry (top closing face and vertical mirror plane) and one wall surfaces are intersecting eachother in the same point at the front face (the result is a large region with Cp>1 values on it). I'm sorry for being not able to solve this problem. Regards, Regert

Sepp May 14, 2001 02:26

Re: Calculation of a cube (bluff body)
 
Hello Regert,

thank you for your remarks. I haven't tryed it using a half building but I calculate the problem using a RSM instead of a k-e-model with the same net. It works! But why is the k-e-model not able to reproduce the pressure distribution on the front face? I am working on it. Best Regards, Sepp

Regert May 15, 2001 09:20

Re: Calculation of a cube (bluff body)
 
Hello Sepp,

I heard what the source of the problem with Cp is. The turbulence model k-epsilon is based on energy production and dissipation. This feature causes the problem, because if a large stagnation area builds up somwhere the turbulent kinetic energy increases and it means an energy production for this place into the flow, that direct means the increase of the stagnation pressure, i.e. the value of Cp will grow above 1. For the Reynolds Stress modell in Fluent the k and epsilon equations are also solved but only for boundary conditions at walls are used and in some terms for modelling. But in general, the RSM does not work with energy, so it makes no energy production anywhere in the domain. I hope that satisfies your question, for details there are some literature in the field of k-eps turbulence models.

Regards, Tamas Regert


All times are GMT -4. The time now is 22:32.