Hi,

I am now doing an unsteady stay modelling of 2 identical bluff objects of 7m x 7m rectangular with round conner of R=2.0m, one in front of another by 40m in a 10 m/s flow using k-e model. The turbulent intensity of the flow is 0.05%.

The time step was 0.2s and the drag coefficient obtain was quite close to estimation. What make me feel strange is the lift force (which expected to be 0 or move up and down due to shedding around zero axis) appears to go down very far at t=5.8s.

Any suggestion why this imbalancing happened? The grid is symmetrical, the shape is symmetrical, the domain is also symmetrical.

A steady state analysis has also been carried out before these one but found that the lift coefficent was always positive and is almost 40% of the drag (which is inconsistance with physical observation) anyone got a suggestion why?

Yours, Desmond

(1). The only quetion I have at this moment is " are your solutions mesh independent?" (2). What is the mesh size (total number of grid points or cells) and the turbulence model used?

Hi John,

My solution empolyed a 50k cells mesh and it yield the same result with a 140k cells model, I have tried several mesh configuration but yielding the same answer. (except some time the lift is positive and some time the lift is negative with the same order of magnitude)

(1). I can only say that it is difficult to compute the separated flow accurately, especially you have two body interaction. (2). You could vary the spacing between the two bodies, to see how the solution behaves. (3). Do you get the same trend if the body has sharp corners? I mean is it code related or the geometry related?

Hi John,

It is so unfortunate that the spacing is an essential criteria of the model cause it is the separation of 2 buildings which we have to investigate.

I have not tried a sharp coner one, what is the significant of trying that?

yours, Desmond

(1). Flow separation from the sharp corner tends to fix the separation point at the corner. This will stabilize the flow, although the flow field in the separated region is still oscillating. This principle has been used in the sports car rear end design. So the flow can separate from the body in a rather clean fashion. (2). If you have smooth curved surface, and the flow has to separate from it, then the separation point will move on the smooth surface, which will make the downstream separation region more unstable. (3). So, on the tall buildings, like the tall chimney, it is a good idea to induce the flow separation at some fixed locations, instead of letting the flow to separate freely on the smooth surface. (4). So, based on this principle, you would rather design a building with many beams sticking out on the surface of the building. In other words, flow separation on a smooth surface is going to be very unstable because you can not keep the separation point or lines at the same place. So, a building with round corners is not a good design related to the induced flow separation behavior. (5). Symmetric geometry and arrangement is rather weak to keep the flow symmetric, unless the Reynolds number is very low (unlikely for building cases). So, the nature is on the asymmetric side. But I was interested in the source of this asymmetry, whether it is from the solution itself, or because of the numerical procedure of the code.

Bluff bodies in tandem - In problems like this one, summetry-breaking occurs first and it eventually leads to alternate vortex shedding. The k-epsilon model (I suppose you're using the standard k-epsilon model, the default model in FLUENT) is likely overly diffusive as is well known, suppressing the alternate shedding of votices. I suggest you to try the RNG model or the RSM model instead of the standard k-epsilon model.

No matter what turbulence model you choose, you should wait long enough until the transient solution settles down and exhibit a periodic shedding.

Hi Kim,

The model I am using now is RNG k-e with standard wall function, after 200 stanard time step, Fluent shows me that the solution become a steady one... insteady of the unstable shedding behaviour predicted by the steady slover...

At a Re= 5e6, I do expected that there would not be much shedding to be occure. But it is strange that the steady solver give me that prediction..

Also, the unsteady slover give me an Cd of around 0.8 and Cl at 1.7e-3, which is reasonable and agree with the books values for similar objects.

So, my focus is now on when to use an unsteady slover and when could a model being simulated by a steady slover. That is essential to the efficient of the software in commerical application.

yours. Desmond

At the Reynolds number you quoted (5 million), experimental data seem to suggest that the flow in the wake begind a isolated circular cylinder tends to get completely chaotic (no regular alternate shedding). What you witness in your steady solution is likely nothing more than what non-converging flowfield typically exhibits. Having said that, I also know from my experience that"limit cycle" behavior exhibited by a steady solution is sometimes a token that the flow is subjected to some sorts of instability. The discretized steady NS equations based on implicit under-relaxation factors "resemble" those for unsteady NS equations, and the steady solution may still exhibit some psuedo-transient behavior when the flow is subjected to strong inherent instability. But it's not a time-accurate solution.

Regarding your question about when to use ...:

When a transient phenomenon is suspected and it's critical to capture it, wouldn't it be safe to pursue transient solution ? If you're absolutely sure that you'll be modeling, using RANS models, a circular cylinder in freestream at 5 million all the time, why bother to purse time-accurate soluton ? If you're going to do LES to study the chaotically looking wake, you can't avoid transient simulation. So, I guess my answer is it's all upto the purpose of your computation.