I am modeling flow over a cylinder. At what range of Re is the flow laminar, transition, and turbulent. Please provide a reference.

(1). It seems to me that you have not studied the basic book in boundary layer theory by Schlichting. (2).In Chapter-1, it has a sequence of photos taken by R. Homman in 1936, in terms of Re transition from laminar to vortex street. (3). Don't say that you have never seen the book by Schlichting.

I own Schlicting's Boundary Layer Theory and have referenced it quite often. The pictures on page 18 are those of formation of a vortex street for laminar flow.

I understand that when flow becomes turbulent the energy near the surface required to overcome a pressure gradient has increases and the boundary layer seperates at a later point. This leads to a decreased wake area and an associated decrease in drag. A sudden decrease in drag occurs at about a Re of 5x10^5. This leads me to believe that at this Re, flow has become fully turbulent. Tell me if I am correct or incorrect here.

I would like to know when the flow becomes transitionary. I see an almost steady decrease in Cd with increase in Re until about Re = 1000. Is this where flow becomes transitionary.

Tell me this, for flow over a relatively smooth cylinder at Re=900, is the flow still fully laminar or is it close enough to model with the laminar solution? If I add rotation and/or shear flow to this flow, will it be laminar?

(1). You can check the chapter for skin friction drag for flat plate at zero incidence. There is a cf vs Renolds number chart which will give you some information about the turbulent flow regime. (5x10^5 is about right) (2).Remember that flow around the front portion of a cylinder is basically "boundary layer under favorable pressure gradient". The boundary layer profile will be rather stable. (3). I would say Re=900 case is laminar and transient.

For this Re = 900 flow over a cylinder, would you use the laminar viscous model or would you use a turbulence model?

(1). It's better to treat the flow over a cylinder at Re=900 in a laminar flow fashion. (2). The wake would be transient based on the data, so a transient flow calculation would be more realistic. (3). But you can definitely treat it steady-state and get the solution first.(symmetric would be better) It is useful to serve as a reference solution for the transient flow. (4). If you trip the laminar boundary layer into the turbulent flow, then you can try to simulate it by using a turbulence model. (a low Reynolds number model will be required .)

Because I am studying the vortex shedding and frequencies of these vortices, I require unsteady calculations. I do find that after about 30 seconds I do get steady cycles with time periods, and calculate the Strouhal number to be about 0.21 (close agreement with Schlicting). I did use the laminar model here. My next step is to find vortex shedding in turbulent flow. Because the flow is fully turbulent at Re = 5x10^5, I am using Re = 10^6. I changed the velocity to modify my Reynolds number. Because of this velocity increase, and an increase in St to about 0.27, I find my time period to be about .0065 and I select a time step of about .0001. I am working on this solution at this time. Any suggestions or comments before I continue here? Perhaps someone has experience with this problem.

(1). We all know that to model the separated turbulent flow correctly, a low Reynolds number model has to be used (wall function is not appropriate here). (2). Then the high Reynolds number flow requires fine mesh near the wall to resolve the sublayer behavior. (3). These are two basic requirements for high Reynolds number turbulent, separated flows.

Not one completely clear on what you are saying. Could you provide some examples of what I might do as far as Fluent use is concerned.

(1). Can you check the user's guide and look for the low Reynolds number turbulence model, if any. (2). Or you can use a two-layer model which is half-way there. Most commercial codes have this model. (3). And make sure that your fine mesh satisfy the Y+=1 requirement at the first off-the-wall mesh. This has been discussed frequently here, so why not check the old messages related to this Y+ and low Re model requirement. (4). If you don't understand the high RE and low RE models, then you need to read some books on turbulence modeling first. Then there will be the issue of the mesh resolution problem in the transient wake region, and a lot of mesh points will be required there.

Not one completely clear on what you are saying. Could you provide some examples of what I might do as far as Fluent use is concerned.

Please ignore the repeat of my last message, it was added by mistake.

Hi there,

At up to around Re 5*10^5, the boundary layer is laminar prior to separation, i.e. laminar separation occurs.

At Re=900 the flow is completely laminar.

Somewhere in between turbulence starts to develop in the wake (only) due to entrainment from the freestream. I suggest that here you use the full NS equations (ie laminar) but with high grid resolution in the wake. You won't fully capture the turbulence in the wake but forces on the cylinder and the Stroul number should be predicted correctly.

At around 5*10^5 (where the drag suddenly drops) transition occurs upstream of separation and separation is delayed due to inctreased kinetic energy in the turbulent boundary layer. A turbulence model cannot model this as they typically predict transiton at a Reynolds number that is around an order of magnitude too low. You need a transiton model for the transition region. (Not in FLUENT)

At Reynolds numbers above where the drag levels off (and starts to increase) the flow is fully turbulent and your turbulence model should work fine. But use a low-reynolds number model (a model that integrates to the wall) I think FLUENT only has the zonal model for this which is not ideal. Moreover wall functions cannot capture separation.

Actually if FLUENT has the Spalart-Allmaras model for the eddy viscosity then this is probably the best as it integrates right down tot he wall and is designed for adverse-pressure gradients and separation.

I have done a full (Re) range of calculations for the cylinder with FLUENT once apon a time.

I got my drag plots from "Aerodynamic drag" (I can't remember who this is by but could find out if you can't find it).

All the Best Steve

For Re = 10^6 I'm trying it now with the k-epsilon RNG model with the differential viscosity equation activated for low Re. I am using the two layer zonal treatment for the near wall. From plotting y+ and y* I can see I am capturing the boundary layer all the way down to the laminar sublayer. I have refined my wake also (I am maxed out on memory for the computer I am using). As expected, I see seperation at about 140 degrees downstream. I get smaller vortices than I do for the laminar case (as I should expect because my wake is smaller). But i am not seeing obvious changes in the vortices shape. The changes I see in the laminar case are obvious. Does anyone know or have reference to what the vortex shedding is to look like when Re 10^6? How fine do I need to mesh my wake? Is there a way to calculate this?

What changes do you expect? If anything the onset of turbulence should stabilise the solution somewhat.

At Reynolds numbers over 1000 or so the wake should become quite chaotic, i.e. vortex shedding should be irregular.

You can't really expect a k-e model to resolve the wake or boundary layer of this flow accurately. The model is likely to unphysically delay separation due to two reasons: over-prediction of eddy-viscosity in the adverse pressure gradient upstream of the separation point; and also over-prediction of eddy-visocity due to inaacurate modelling of flow impingment at the stagnation point (can overcome this by refining the grid in the stagnation point region). These are the two major flaws of the k-e model. RNG can provide slight improvements for some flows but is known to degrade results for other flows.

Looking at my plots the drag drop off occurs between 1*10^5 and 5*10^5. During this region the flow is transitional and turbulence modelling is usuitable. At 10^6 the flow is fully turbulent so turbulence modelling is appropriate.

The reference I was thinking of was "Fluid Dynamic Drag" by S. F. Hoerner.

Try also: "Elements of Fluid Mechanics", by D. G. Shepherd.

I don't know if anyone has done any DNS, LES or DES for cylinder flows but this is really what you need for accurate wake modelling (your Re number is probably too high though).

I can try to run LES if someone can teach me how to perform parallel processing on an NT platform.

What is the approximate rule for DNS? The number of cells required = Re^9/4 (but is that the approximate for 2d solutions)? If I can parallel 20 computers at 200,000 cells per comp, thats about 4*10^6 cells. So I obviously cannot perform DNS, but I can see what I get with LES.

Again, can someone explain how to perform parallel processing on an NT (soon to be 2000) platform.

Much appreciate the help John, Steve, and everyone.

The Reynolds number is definately too high, and LES is not really suitable to wall bounded flows as even the large eddies are extremely small close to the wall.

The only realistic option is Dettached Eddy simulation (DES) where a RANS model is applied to the near-wall and LES is used outside. Even this approach would require millions of grid points.

If mean flow quantities like body forces and vortex shedding frequencies (stroul number) are all you need then a RANS model should be adequate. But those based on the epsilon equation will give poor results. Either a k-omega model or the Spalart-Allmaras model would be better.

Is the Spallart Allarmus model more accurate than LES, RSM and k-epsilon models? Does it work well with Vortex Shedding on the cylinder?

It is not in the same league as LES.

RSM can model the anisotropic stresses in wake, and the curvature in the boundary layer much better than the Spalart-Allmaras model. However unless it uses a formulation that resolves the near-wall, RSM will predict separation poorly. Same too with k-epsilon.

The Spalart-Allmaras model is probably better suited to your application, but this doesn't mean it is a better model.

Moreover the turbulent flow around a cylinder is very difficult probelem to model - all turbulence models will struggle in some aspect.

You see I obtain vortex shedding for the laminar case. When I try the turbulent case, i do get vortices but for the unsteady case, but i do not see much change in the vortex pattern. What all should I check?