CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   flow over a cylinder, turbulent and laminar (https://www.cfd-online.com/Forums/fluent/28719-flow-over-cylinder-turbulent-laminar.html)

Chetan Kadakia July 13, 2001 02:01

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

John C. Chien July 13, 2001 02:38

Re: flow over a cylinder, turbulent and laminar
 
(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.

Chetan Kadakia July 13, 2001 04:18

Re: flow over a cylinder, turbulent and laminar
 
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?


John C. Chien July 13, 2001 12:56

Re: flow over a cylinder, turbulent and 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.

Chetan Kadakia July 13, 2001 15:05

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


John C. Chien July 13, 2001 20:25

Re: flow over a cylinder, turbulent and laminar
 
(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 .)

Chetan Kadakia July 13, 2001 21:22

Re: flow over a cylinder, turbulent and laminar
 
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.


John C. Chien July 15, 2001 13:25

Re: flow over a cylinder, turbulent and laminar
 
(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.

Chetan Kadakia July 15, 2001 17:50

Re: flow over a cylinder, turbulent and laminar
 
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.


John C. Chien July 15, 2001 19:19

Re: flow over a cylinder, turbulent and laminar
 
(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.

Chetan Kadakia July 16, 2001 00:43

Re: flow over a cylinder, turbulent and laminar
 
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.


Chetan Kadakia July 16, 2001 00:45

Re: flow over a cylinder, turbulent and laminar
 
Please ignore the repeat of my last message, it was added by mistake.

Steve Collie July 16, 2001 19:12

Re: flow over a cylinder, turbulent and laminar
 
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

Chetan Kadakia July 16, 2001 20:08

Re: flow over a cylinder, turbulent and laminar
 
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?


Steve Collie July 16, 2001 21:19

Re: flow over a cylinder, turbulent and laminar
 
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).

Chetan Kadakia July 16, 2001 22:56

Re: flow over a cylinder, turbulent and laminar
 
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.

Steve Collie July 16, 2001 23:59

Re: flow over a cylinder, turbulent and laminar
 
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.

Chetan Kadakia July 17, 2001 00:47

Re: flow over a cylinder, turbulent and laminar
 
Is the Spallart Allarmus model more accurate than LES, RSM and k-epsilon models? Does it work well with Vortex Shedding on the cylinder?


Steve Collie July 17, 2001 18:04

Re: flow over a cylinder, turbulent and laminar
 
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.


Chetan Kadakia July 25, 2001 03:56

Re: flow over a cylinder, turbulent and laminar
 
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?

Steve Collie July 26, 2001 21:00

Re: flow over a cylinder, turbulent and laminar
 
A low-order discretisation scheme may be stabilising the solution (nonphysically) somewhat. Try using a higher order scheme.

Chetan Kadakia July 26, 2001 21:04

Re: flow over a cylinder, turbulent and laminar
 
I use second order schemes.

After some reading and discussions, it seems that the vortex shedding will not be as obvious for a turbulent solution. And due to the added randomness, steady cycles may not be achieved. So my solution may be more accurate than i once thought, but I still need o understand the physics here.

cfdcfd123 April 4, 2010 23:24

Steve has given some valuable info about flow over cylinder. I have a question for all. When you say drag value at Re=10^6, what is it ? Is it average drag? Because the flow is turbulent the average value of drag can change with time(Correct me if I am wrong,please). How do you calculate this average drag. and how to we calculate the mean flow.

I have one more question. I am currently doing a Re=800 simulation without using any turbulence models. I have the flow solutions at different times. Can anybody tell me how to post process a turbulent flow (turbulence in wake in this case).

What do I need to do to calculate TKE and how do I get the E(k) vs k plot.
Thanks in advance . I think this is one of the best threads for flow over a cylinder

Ozgur_ December 5, 2010 19:16

Hello all,

I agree; this really is a good thread. I have a general question regarding the unsteady wake of the 3D circular cylinder in cross flow problem I'm interested in:

- The mesh I'm using is very fine, worked on it for quite a while. Also, the boundary conditions I set and the domain size is accurate and sufficient. My problem lies in the unsteady solution. I first iterate the case for 4000 steps using steady state, and make sure I reach convergence. Then I run it unsteady for 300 time steps using a time step about 1/50 the time step obtained from inverting the frequency obtained by using the definition of the Strouhal number (St = f*L/V). The problem is that the unsteady oscillations of the wake disappear and I get a symmetric wake once I get convergence. I wait until all the residuals level out and stay constant for a good while.

Any ideas why this is happening? Is it because of the turbulence model (k-omega SST) being diffusive and getting rid of the vortex shedding, or is it the time step that is too large? And one more thing, how many pseudo-time steps are required for each time step?

Cheers,

Ozgur

Ozgur_ December 5, 2010 19:17

To reply to some of your questions, cfdcfd123, here are my opinions:

- I haven't done calculations with Re magnitudes around a miliion, but I have worked on Re values around 10000 for quite a while.
- Fluent calculates TKE on its own; so you should be able to get TKE contour plots easily in post-processing.
- As for the plot (is it epsilon vs. k that you're looking for), you can take the average of any parameter you're interested in over the solutions obtained at different time steps. I take data at time steps placed really close to each other and take an arithmetic mean of the properties I'm looking at. Although, if you take an arithmetic mean with too large a time step between steps, this may be inaccurate.
- I am modeling 3D cross flow past a circular cylinder placed on a flat wall, but I'm not focused on drag that much; but I'll let you know if something comes to mind.

Best of luck,

Ozgur

Reynolds December 14, 2010 07:19

Ozgur_,

I am also currently running a similar problem at Re = 90,000. I am attempting to predict noise, and as such have based my time step on the max resolvable frequency that I desire to have. I picked 4000Hz (close to upper limit of human range) and then decided that for each wavelength I wanted to resolve it with 10 points.

So delta t = 1/(4000 x 10) = 2.5E-5 s

I am not sure this will help you, but could be of some use in the future maybe. TO reduce computational time I am currently only running 15-20 iterations per time step.

I am relatively new to CFD and have been using the K-omega SST model, however after reading this thread I am considering trying Spallart.

Matt

vmlxb6 April 18, 2011 03:37

I am trying to simulate a flow over a cylinder at Re= 10000 and using K-w SST as the turbulence model. I dont know how to select the BC for turbulence ???? Can anyone help me out.

Thank you

rishitosh December 8, 2012 06:08

flow over a circular cylinder.. @ Re=1000
 
hiii..

i m very new to in CFD area...
i have worked on flow over a single cylinder, two clinder in tandem and tow cylinder in side by side @ diff Re with diff ... i got good results....

but when i started working for Re=1000 .. for single cylinder...
i didnt get gud result.... :confused:
i have use used mesh wid y~min <1 to Y+max<5.. wid Kw-sst model...
Cd wich i m getting is 1.4 and as per journals and different thesis, i went through, Cd should be 1~ or < 1.

i hv tried 0.5% turbulence @inlet and hydraulic dia equal to dia of cylinder.... and @ outlet 0, 0.5 and 0.7 back flow turbulence and same hyd dia...

but still... :confused:


All times are GMT -4. The time now is 17:36.