Ha guys! I am a man doing CFD works in Hong Kong. As you may know, there are a lot of high-rise building in Hong Kong. The influence of buildings on wind or the flow pattern around a group of building becomes a very important problem to our (I mean Hong Kong people) daily life. As a result, I was assigned (of course by my boss) to use CFD techniques to study the wind amplifaction factors in the vicinity of some buildings. This is really a mission impossible. But I still have to use the limited resources that is available to me to finish the task. Anyway, I want to know if there is anyone who has done similar things before and if you have such a experience. Please let me know 1) how many cells that you have used , 2) what is the running time to get a steady state solution. 3)What is the turbulence model? (Standard k-epsilon, RNG, RSM ..etc?) 4)Which commercial code that you are using? 5) Is there any good literature that you think is useful for reference? 6) How many buildings that have simulated? 7) How to set the inlet boundary condition, what turbulence intensity and viscous ratio should be chosen?

I hope there is someone out there who has the expertise in assisting me to short out all these questions. Thanks !

There are lots of studies published in journals on flow over buildings - which is basically a bluff body flow case.

First you need to decide what it is that you are looking for. Do you want to study the wind effect on the ground level or its effect on the building itself (and its occupants). If the latter, then you may have to look into unsteady simulation of flow over the entire building, because unsteady vortex shedding leads to noise/vibration problems.

If you are interested in the ground level, then I think you may not have to look at the whole building. As far as people are concerned high rises are infinitely tall. So, you can get a first order understanding of the problem by simulating a 2-D flow over a bunch of squares. This will also let you do unsteady flow if you wish.

Having learned something about the flow, you can then move on to 3-D, but not full-scale. I don't think it's necessary. You can chop off your buildings at fairly close levels to the ground, say 3-4 floor levels. You can use some modeling for the top boundary condition (for example periodic BC). The only reason you need 3-D is to simulate 3-D reciurcation near the ground level (if it is signifant - look at basic fluids books for a reference)

As for the other issues, sorry can't help

Adrin Gharakhani

Thank you, Mr Gharakhani.

Yes, we are interested in the wind effect near the ground level. Our intention is to study how the buildings will amplify the wind in the pedestrian level. We have already done some 2-D CFD flow analysis on the site, but the agreement between the 2-D results with our Wind tunnel test results (based on the erosion test mehtod) is not very satisfactory. So, we are trying to do a 3-D full model simulation of the buildings.

What you have suggested is quite interesting, but since the high and geometry of the buildings are not uniform and complicated. So, it seems not possible to apply the periodic boundary condtion in this case. Anyway, I have already created a unstructural mesh with about 500,000 cells for this problem. And I am running it on my Sun Ultra 6.0 microsystem. The cell size is about 2 meters.

For those CFD experts who has done a similar CFD simulation, please drop a few lines for me to learn something from you. Many thanks!

You may want to check out ARIA Technologies of Paris. We have done a good deal of wind simulation work with them for the U. S. government for hazard dispersal. They have a Navier-Stokes code called MERCURE which may be just what you need.

Their web site is http://www.aria.fr . Their contact information is also there. Give it a look, hope this helps. Best wishes with a challenging problem.

(1). Your problem is well-defined. Basically, you are computing a boundary layer flow over complex objects in the form of groups of buildings. (2). I think, you are concerned about the accuracy of cfd simulations relative to the wind tunnel measurement. (3). The main feature of the problem is the behavior of the building when exposed to the wake of another building. So, you have to make sure that your results can capture this behavior first. (4). Although the flow separation from a sharp corner of a building is easier to compute relative to that from a smooth cylinder, you still need to make sure that you have the ability to compute the wake flow over a building. In this case, flow over two buildings is a good starting point. And you can use this case to estimate the accuracy vs the total cell numbers and the computing time. You can also validate the results using the wind tunnel testing quite easily. (5). After that, you can systematically add additional buildings to the group, and recompute the flow field. In this way, you will be able to make the mission impossible a reality. (6). So, somewhere along the line, you will be able to present the results of flow over two buildings in a conference, and at the same time, have enough time to convince your boss for more funding. (7). If it turns out that the two building problem results can not match the wind tunnel test data, you can still try to convince your boss that this mission is indeed impossible.

Hi! Tomb, I have some experience regarding this problem. There are some information for you just for reference.
>1) how many cells that you have used, I used about 500,000~750,000 cells.
>2) what is the running time to get a steady state solution. Using DEC-alpha(500/MHz), one week.
>3)What is the turbulence model? (Standard k-epsilon, RNG, RSM ..etc?) K-epsilon model is not good for this problem, RNG may be much better. RSM is hard to running.
>4)Which commercial code that you are using? STREAM.
>5) Is there any good literature that you think is useful for reference? Please take look this journal. "J. of Wind Engineering and Industrial Aerodynamics"
>6) How many buildings that have simulated? Over 10. 7) How to set the inlet boundary condition, what turbulence intensity and viscous ratio should be chosen? The inlet boundary was set by a power law function for velocity. U/U0=(Z/Z0)**alpha where, alpha=1/4,or 1/7 etc. alpha =1/4 may reasonable for Hong Kong. Turbulence k, experimental data was used. epsilon: Ep=Cmu*K**1.5/lm where Cmu=0.09, I hope this information will be useful for you. Good luck. Wei

Dear fellows, Adrin, Doug, John and Wei

Thank you all very much for your useful suggestions and discussions. I think there is still a long way to go in order to make it possible to replace wind tunnel test by CFD simulation completely. But, we still have to try before it really come true, right? Luckily, at least, I found that I am not alone in this long long road.

Thanks!

Anyone have an idea what the range of Strouhal numbers might be for building shaped objects? I have found some data for rectangular prisms with Re~10^4 giving Sr~.13. However, this is a low Reynolds number for a building.

Thanks,

Carey