I would like to solve turbulent problem with Re =6000 with DNS. I have gone through the discussion using Fluent for solving DNS in laminar. My question is does fluent have capability of solving DNS in turbulent? if it does how to implement the DNS in fluent. There was one discussion mentioning to choose LES model but building the mesh small enough. Can anyone tell me which one is correct using laminar unsteady or LES for solving DNS in fluent for turbulent flow? I need some enlightenment in this area. Thank you in advance

i think Fluent can't solve DNS,because it hasn't the DNS model that you can choose, but you can choose LES model to compute Re=6000 turbulence. and in general Re=6000 flow isn't laminar flow, so you can't choose the laminar unsteady model.

What is a DNS model ??? Just curious.

Does refining the mesh using LES model mean the same as using DNS?

DNS is for turbulence modeling only. When the Re=6000, the flow regim is a turbulence flow.DNS= RANS close to boundary+ LES in fluid.

Sorry,my DNS should be DES (Detached Eddy Simulation).Since there is not DNS model in Fluent, I assumed that Hengky meant DES.

Hengky,

DNS means: solving the equations of motion without using turbulent models! As a result the equations of motion for DNS model is the same as laminar flow.

The question is why we can not use DNS for every kind of flow? The answer is we need a high CPU capability. I do not know what complexities your case has but if it is very complicated and you can not mesh it as fine as needed for DNS then you won't get the result expected.

For more information about the smallest scales of time frame and displacement needed for DNS refer to advanced texts describing turbulency.

Mohammad

Thank you so much for the insightful thought Mohammad. I know the kolmogorov length scale equation to determine how fine the meshes shoud be based upon the Re number. I just want to ask you again do you think Fluent has a capability of doing DNS? Many believes there is no DNS option in FLuent so that we can not simulate the turbulent flow using DNS by Fluent. I believe there are two options to approach the DNS in FLuent firstly is selecting laminar although the flow is turbulent second is selecting LES model and refining the mesh in such a way that less than the minimum length scale. That way, the whole mesh will be resolved by the large scale eddy (filtered navier stokes) without getting into subgrid scale model. I am not sure which one is correct. Could you please give me your opinion as soon as you can. Thank you in advance.

Hengky,

I believe that fluent can do DNS. You should just set it to laminar flow and mesh as fine as needed for DNS.

Best Wishes,

Mohammad

The equations of DNS are same as those of laminar flows. In fact, I don't think Fluent or any other commericial software (cfx,pheonix, starcd,etc) could do DNS. This is due to the insensitivity of turbluent flows to small perturbance in bc or initial conditions. While most of commerical softwares are robust, they are not accurate enough for DNS of turbulent flows. Cost and effectiveness are another issues. Sure you can use laminar model in Fluent to solve your turbulent flows, howvever, grid refinement will tell you that your grids need to be refined and refined until your computer fail to do this. Just my opinion.

sarah

Sarah may be true. You may have some other problems with accuracy. You may generate your mesh as fine as possible may be going to kolmogorov length scales to omit perturbance!

I don't see why a commercial code would be unable to run a DNS case - I certainly don't agree with the statement that all commercial codes are "robust but not accurate".

Anyway, in answer to the original question, should you run laminar or LES: it depends.

The "correct" approach is to run laminar - as has already been said, DNS = no turbulence model = laminar. NB: a laminar setting means no turbulence model, it does not mean that whatever scenario you apply it to will/must be laminar. Obviously, the problem being that if your flow really is turbulent and you run true-DNS/laminar, you'd better have a very large computer!

Alternatively, you could run LES. Because the subgrid scale contributions from LES's turbulence model are dependant on the cell size (filter length), if you refine your mesh enough, you should end with a DNS solution. The advantages of this approach being: 1. if your mesh is too coarse you'll get a better answer, as the subgrid scale model will do its job; 2. it's likely to be more stable - one significant benefit of using a turbulence model is that they tend to stabalise the calculation.

I have used STAR-CD with the second approach and obtained excellent results as compared with experiment.