I am looking at the flow around a circular cylinder at a range of Reynolds numbers (re=26 to re=2e5)using Fluent V4. At Re up to around 1000 the result seem to correlate well with the experimental, however, at Reynolds numbers higher than around 2000 the flow starts to go back to what seems to be the invisid flow and the static pressure values etc are very inaccurate, CAN ANYBODY TELL ME WHY THIS HAPPENS? (as this is pre-critical flow I am not using any of the turbulence models). I really need to model at around Re=1e5 accurately can anybody tell me how I can do this?

I do not what Fluent can/can't do. For flow past a circular cylinder, in the Reynolds number range of 150-300 the vortex street transforms to turbulent. However, the boundary layer still remains laminar upto 2e5 or so. Hence, you need to adequately account for the turbulent vortex street of the wake region.

At Re=2000 do you think you have the proper grid density near the cylinder? Are you picking up the proper separation characteristics in the lower Reynolds number range? You are not specifying what property of your simulation "correlates well" with the experiment - if it is just drag coefficient, that is not much info to take comfort in the accuracy of the results.

I would recommend that you check the paper by C.R. Anderson and M. Reider, "A High order explicit method for the computation of flow about a circular cylinder," J. Comp. Phys, vol 125, 207-224 (1996) and if I'm not mistaken in this particular paper you'll see that you will need quite a large number of grid-points to get accurate solutions for flow over cylinders.

If external flow is what you're interested in (and espcially if you need solutions of flow over cylinders only) then the best solution methodology would be based on the vortex element technology.

Adrin Gharakhani

1. First, you should be aware of that it is impossible to simulate accurately a pure laminar folw around circular cylinder at Re as high as 1e5. Current numerical scheme is not so accurate, especially for commercial codes. (Although you can find some papers reported it, their results are suspect.) 2. As Re becomes larger, the boundary layer is very thin. For computation starting as a potential flow, it is really more like inviscid one at the early iterations. The boundary layer developes rather slow. 3. At Re smaller than 1e4, you need not to consider any turbulence effect if your are only interested in the boundary layer around the circular cylinder and near wake flow. Turbulence is far away from the obstacle, it hardly influence the boundary layer because of convective property of the wake flow. When Re is as large as 1e5, I think turbulence effect should be included as least in the wake.

I think the problems you met in the computation are most probably dut to two reasons: 1. you did not make the spatial size of your grids as fine enough. or 2. you havenot take enough iterations. You may tyr to use a large time step to see if there is any change in the flow. For the description of circular cylinder at different states, you may refer Triton's book.

I do not know if FLUENT can solve steady N.-S. equations, and anyway you are probably interested in unsteady solutions which can be expected to correlate with experiments. If so, the following is irrelevant. However, your reference to inviscid flow (do you mean potential?) implies to a certain degree steady solutions. In this case I recommend any one of two papers by B.Fornberg: Steady viscous flow past a circular cylinder up to Reybnolds number 600. J.Comput.Phys., 1985, v.61, 297-320. and Steady incompressible flow past a row of circular cylinders. J.Fluid Mech., 1991, v.225, 655-671. If you wish to know more about high-Re steady solutions please feel free to contact me, I'll be happy to help.

Yours Sergei

Hi Paul,

I'd like to remind you of a couple of things that occur as the Reynolds number is increased.

1) In the Reynolds number range you referred to, the boundary layer thickness becomes smaller as the Reynolds number increases. 2) The vortex shedding frequency changes very rapidly in the Reynolds number range of you mentioned. In fact, the Strouhal number (non-dimensional shedding frequency) increases from 0.16 at Re_D = 40 to 0.3 at Re_D = 1000 to 0.8 at Re_D = 2,000.

With these in mind, you may want to question first whether the mesh near the circular cylinder is fine enough to resolve the boundary layer. The drag prediction is largely determined by how well the boundary layer and its separation can be predicted. Next, considering that the shedding frequency rapidly increases in the Reynolds number range, especially in the neighborhood of 1000, you may want to make sure that the size of the time step you're using is small enough to resolve the shedding and the vortex street evolving in the wake.

And finally it's always beneficial to use high-order discretization schemes (second-order or third-order) which are available in FLUENT.

The drag coefficient for a cylinder varies very little between Re=1000 and Re=150000, to drop sharply when the separation mode converts from laminar separation to turbulent separation. In this flow range separation should occur at about 80 deg from forward stagnation point.

I would (if Fluent allows that) have a look at the calculated integral boundary layer parameters (such as formfactor H = displacement thickness / momentum loss thickness) and check whether they show the correct values especially close to where the separation should occur.

Thank you everybody that has contributed, your suggestions are greatly appreciated.

Thanks!

Dear Mr. Chernyshenko,

In response to your email posting on Feb. 16, 1999, I am interesting to know more about High Reynold-number (Re > 1.e+5) flow past around a circular cylinder. Could you kindly direct me some references or steady solution regarding to this issue? Thank you so much.

Yung-Ming