Hi

I am trying to simulate the flow past circular cylinder(s) at high Reynolds numbers (in the order of 10^4 to 10^5) using FLUENT 5 software. This regime is of interest in practical heat exchangers. The computational domain was discretized using hybrid mesh, i.e., quadrilateral cells around the cylinder and triangular cells in the rest of the domain using GAMBIT. The numerical simulation was made for unsteady, 2D case using LES as the turbulence model with Smagorinsky-Lilly subgrid model. The pressure coefficient recovered excessively at the rear of the cylinder. The experimental results show 10 to 15% recovery while the present analysis recovers almost to 45%. The separation point is also later than seen in experiments. I believe that this is because of inadequate accounting of turbulent viscosity in the model used.

Literature has references to simulation of flows at lower Re values. Predictions of Strouhal numbers seem to come out alright. However, the devil seems to be in the pressure distribution.

Have you worked on this problem? Do you have suggestions that I might find useful? Your contribution to my work will be gratefully acknowledged in my thesis and references and all the papers that will be published out of this work.

I can send the grid and pressure distribution results if you like. My email id is : jalaiah@hotmail.com

Thanks. Jalaiah.

(1). What is your role of running this case? (2). If the role is to document the results using this code and the grid you developed, then you should run several other grids and plot the results. (3). If your role is to find the flow field and the pressure field so that you can use the results later on, then you should try other approaches. This can include other turbulence models in the code or using other codes. (4). Since you are interested in the turbulence modeling, it is a good idea to look into this area and write your own code. It is really useless to ask questions about the results of Commercial code, because the only one who can answer your question is the one who has complete access to the source code and knows the logic of the code. It is a good idea to find out who wrote that section of the code, and whether he has checked out the code for the similar problems.

I am not sure what will happen if you use the LES model for a 2D simulation (see previous discussion on this topic). The derivation of the model assumes a normal 3D energy cascade. It may not cause a problem but you would have to check with FLUENT to see if the wall treatment, etc... is correctly handled in 2D. Even if it does not cause a problem, how the prediction relates to reality (if at all) will need careful consideration.

Your observations concerning Strouhal number and surface pressure distribution are typical. If you do not get the correct shedding frequency you have done something seriously wrong. The surface pressure distribution is much more of a challenge.

I would suggest:

- increase the resolution by a factor of 2 in all directions and look for observable changes.

- use a k-e model instead of the LES model since this may have a more reasonable wall treatment (note: the shedding is not turbulence)

- talk to FLUENT.

By performing a 2D simulation instead of a 3D simulation you are preventing the shed vortices from rolling up in three dimensions. You may have to perform a full 3D simulation if it is important to accuratley simulate the physical processes in the wake.

A late separation point is an indicator of too much diffusion. This may be numerical (too coarse a grid) or due to the turbulence model (turbulent transport is modelled by diffusive transport and this is a poor model in separations). The wall treatment would also bear scrutiny.

i agree with andy. i don't think LES is good in two dimensions (their was a discussion on this in this group a while back )so k-e or some other turbulence model is probably better. also you should refine your grid to ensure your result is grid independent and similarly shorten your timestep. also talking to FLUENT is a good idea

hi,

don't be disappointed, i'm not sure if a good les for the flow past a cylinder at reynolds numbers around 100000 exist, even with codes explicitly wrote for this problem. for these reynolds numbers you need more than 2 mio nodes for your calculation.

if you realy need this calculation, please contact me, i can help you with a code which is abel to handle the problem.

ulrich

Dear Dr.Chien,

Thank you for your detailed comments. Among other things I am also following up on your suggestions.

Jalaiah

Dear Andy,

Thanks for your help. I am implementing all that you suggested and shall contact you after making some progress.

Jalaiah

Dear Mr.Bradford,

I am in the process of trying your suggestions. You refer to an earlier discussion in the group on LES in 2-D. As I am a recent arrival in the group, how might I get to read this discussion?

Jalaiah

Dear Mr. Ulrich,

Thank you for your very useful and friendly comments. Even if I reach a Re. no. of 10,000 it will be new result as I have not seen such results in the literature.

Yes, I would very much like to try your code. My problem deals with flow in a duct(confined flow). The code I am using seems to behave a little better with unconfined flow. I look forward to your response.

Jalaiah

you can search using the search utility at the top of the page or just go through the posts (including the archived posts) til you find posts on LES