I'm simulating steady vortex flow over circular cylinder. I'm using various Re start from 4 - 10^7. I think I can catch the vortex, but I have unsuitable Cd. For Re= 10^5 (rho=1.225, mu=1.789E-05, d=2m) I got Cd=1.6, while in Fundamentals of aerodynamics book (John anderson) it should be 1.2.

Anybody can give me answers for these questions? 1. what viscous model give the best result? 2. should I use different viscous model between the low and high Re? If yes, what should I use for each region?

thank you very much

Hi Sheila

The realizable k-epsilon model is quite good for flows with strong pressure gradients in boundary layers and also separated flows, which is what you have.

Although you see a separated region, this type of flow is best resolved using an unsteady solver. That way you can see the vortex shedding, and the temporal characteristics of the flow.

A Cd of 1.6 is not bad. This flow is quite challenging, even though it is two-dimensional, and a simple geometry.

Also, have you performed a grid study? Your grid might not be sufficiently refined which could increase dissipation.

Goncalo

hi Goncalo

first, thank you for your answer. it's really nice to have a help from you.

I have to perform both steady and unsteady flow. can I use the realizable k-epsilon model for both case? can you seggest a book for me to read about k-epsilon model in detail? I haven't performed a grid study intensively, I just read some books. Any suggestion to refine my grid?

thak you again

Hi Sheila

There are quite a few good books on CFD. A classic text on CFD is:

"Computational methods for fluid dynamics" by J.H. Ferziger and M. Peric, Springer

A book that specifically deals with turbulence is: "Turbulent Flows" by S.B. Pope, Cambridge University Press.

Both these texts present the basics of turbulence and include the k-epsilon model.

There are a lot of papers that deal specifically with cylinder flows. In the Reynolds number range you mentioned, there is:

"An experimental study of entrainment and transport in the turbulent near wake of a circular cylinder", B. Cantwell and D. Coles, Journal of Fluid Mechanics, Volume 136, pp. 321-374, 1983.

"A challenging test case for large eddy simulation: high Reynolds number circular cylinder flow", M. Breuer, International Journal of Heat and Fluid Flow, Volume 21, pp. 648-654, 2000.

Fluent allows for grid adaption, which is great for saving resources. Maybe look into that. How did you generate your mesh?

Goncalo

I just use the mesh options in Gambit.

I count the first cell height and interval of boundary layer near the cylinder using the formula from Fluent journal.

I mesh edges by trying to make a smooth and gradual transistion between one face to others. I use about 100000 grid Quad-Map.

the cylinder diameter is 2m, inlet is 15xR to the front, and outlet is 40 X R to the back.

what boundary layer should I use? I only use velocity inlet in front and both up and downside, and pressure outlet at back.

fluent give an example that use periodic in up and downside, but Fluent 5 don't have this type of boundary layer.

i don't have the latest version of fluent.

thank you

Hi Sheila

I think that you are on the right track. Your mesh sounds to be sufficient. Your domain is a good size.

You don't need periodic boundary conditions unless you are trying to simulate a cylinder array. So you boundary condition choice are sound.

For the cylinder wall, the conventional wall treatment available in Fluent does a pretty good job. Still, for flows with high pressure gradients and separation, it can still fall short.

You can try using the enhanced wall treatment, but this might increase your mesh requirements, and hence, computational cost.

Cheers

hi Goncalo,

i've done my steady simulation and the results is quite good compare to the fluent journal. thank you for your help.

now, i'm processing my unsteady flow and I have several questions:

- Which one is better: using the steady results and continue for the unsteady? start from the mesh file and run the unsteady?

-if using the steady result is better, how can I initialize the unsteady flow without eliminating the steady results?

- i have the new version of gambit, and I'm trying to open my old gambit file with the new one. I can open it but when I save some changes and try to export mesh file, it doesn't work. i use velocity inlet, periodic, and pressure outlet. can you tell me waht's the problem?

thank you

Hi Sheila

Using the steady state solution to start the unsteady simulation might save you some time, but probably not a whole lot.

There will still be a transient time, as the cylinder starts to shed vortices. You can monitor the drag signal, and wait for it to stabilize (into a periodic signal). Then take your data.

I think that you can just change the solver to unsteady and start the run. You don't need to "initialize" your data.

Are you still using the old version of fluent? I think that the new gambit will only export to the new version of fluent.

Cheers Goncalo