Simulation Flow Around cylinder 3D
 

Hello people.. :)

After reading much in the forum and following some of the seen suggestions I have not been able to run one simulation of flow around a cylinder 3D.

The parameters with which I am trying to simulate are:
Re = 1000
d = 0.0164m
Model turbulence SST
to solver = CFX 12.0
Timestep 0.02

Until now I have not obtained a loosening of the vortices.
They suggest to obtain a value of Y+ for the wall of the cylinder < 1 (for this model of turbulence) questions:

1) When reviewing the value of Y+ this must be smaller to 1 of local form for the wall of the cylinder or global for all it mesh?

2) Serious good for using inflation layers in the cylinder or where?

3) In one of post referring to the subject they suggest to use to second to order spacial scheme (like hybrid differencing with the blend factor Seth to 1,0 or close to it) and to second to order temporary scheme. this talks about to advection scheme and transient scheme (second to order backward Euler)? because equal it does not give the awaited results.

4) The relative pressure in out (0 [Pa] my case) and reference pressure (1 [atm] my case) influence in vortex? I have understood that if. those values is OK or like configurarn pressures?

That another to take into account for the configuration of the simulation?

- Transitional turbulence.
- Turbulence numerics (high resolution my case).
- Convergence control >> min. coeff. loops 1
max coeff. loops 3 cause of the problem?increase max?

- Insert to expert parameter?

with respect to it mesh the walls that conform the volume of the fluid (external walls) need special meshing?

I believe that is everything or is what memory at this moment. please some suggestion of how forming the simulation or that I can change to obtain shedding vortex in 3D

excuse my english I do not dominate it perfectly :)

adjunt screen....

http://img190.imageshack.us/img190/2686/fluidflow.jpg


http://img512.imageshack.us/img512/904/filehty.jpg

Hi:

1) At this Re number there is no turbulence. Get rid of SST and use a laminar flow model.
2) Use maybe 10 max coeff loops.
3) Use adaptive timestepping, aiming for something like 3-5 coeff loops per iteration.
4) You will accurate discretisation in space and time. Use hybrid with a blend factor of 1.0 (ie pure 2nd order) and 2nd order transient discretisation.

thanks for the quick answer ghorrocks

At this moment I am simulating with the suggestions that are to me, now I have other questions:

when you say to 10 max coeff loops [2] and soon you suggest uses 3 - 5 per iteration, in timesteps adaptive forms target min and max loops, and in solver control >> convergence control forms min and max coeff loops then:

Target min. 3
Target max. 5

solver control >>> convergence control

min coeff loops: 1
max coeff loops: 10

thus it forms and of this form this realizing 10 iterations by timesteps and I believe that it is not what your you indicate to me.

in adaptive timesteps minimum asks me and maximun timestep that you limit is them of which timestep did not go, but I do not understand that values go there. if my timesteps is 0,02 serious minimum 0.02? and what serious max?

the factors of decrease and increase are by defect in 0.8 and 1.06 something far from original my timestep, tendria that to change them?

as time I do not dominate to much adaptive timestep, I thank for much to you if you oriented to me in this step or you facilitated additional information to me because with the CFX manual it is equal :confused:

thanks to respond and to help me again :)

adjunt my .cfx file out if I did not occur to understand (Ansys 12.0)

http://rapidshare.de/files/47936881/Fluid_Flow.cfx.html
http://www.megaupload.com/?d=1MW8O1JU

hi,

Sorry I did not understand your questions but I think I get the idea anyway. For simulations where you don't know what timestep size to use (and are too lazy to do a time step sensitivity analysis to find out) then use adaptive timestepping to get the simulation to fidn the correct timestep size for you. In my experience beginner CFD people always guess a time step which is far too big so to avoid this trap I recommend the following adaptive timestep settings (I am doing this from memory and don't have CFX in front of me so the names might not be quite right):

Minimum time step size: 1e-20s
Maximum time step size: 1e20s

Everything else you should leave at the default. The only parameter you need to set an appropriate value for is the initial timestep size. For a first go have a guess and try it. If it converges then let the adaptive timestepping run for a while and it should tell you what the time step size really should be. Then stop the simulation, set this timestep size as the initial guess and run the simulation again.

If it does not converge with your initial timestep size then decrease it by a factor of 10 and try again. Keep doing this until it converges!

Glenn Horrocks

Thanks ghorrocks. I believe that I have the idea. now of general form. somebody has some video or info on a simulation 3D of a cylinder and vortex shedding? until now I have only obtained info in 2D

Now Glenn. you suggested to me used to laminate flow model. by I number of Reynolds. and indeed you are right. but I have seen simulacines 2D with Reynolds numbers inferiors 100 and working with turbulence models. K-Omega... SST… LES... to that it must this?

Another question. it is possible that without I to have timestep correct can be able to visualize vortex shedding? of another form until I am not able timestep correct podre not to visualize vortex shedding?

Thanks Glenn and excuse again my english again..:rolleyes:

File LTCM_file00065.avi (6710 KB) uploaded!


Thank you for your upload. Remember that only those people are able to access your files knowing the exact link.
RapidShare is a file hoster and does not announce your files anywhere.
Your Download-Link #1:http://rapidshare.de/files/47954086/LTCM_file00065.avi.html


Source: http://www.ltcm.mecanica.ufu.br/defa...R&USR=aristeus

rogbrito what are you on about? :confused:

Sounds like you need to have a look at the definition of turbulence. True, vortex shedding at Re=1000 looks a bit like a turbulent flow and I guess that's why some people have tried to use turbulence models on it. But it is not a turbulent flow. A turbulent flow will have a turbulence spectrum with large eddies cascading energy down to smaller scales until it finally gets dissipated at the Kolmogorov length/time scales. If you draw a energy spectrum of this flow at Re=1000 you will find a cascade does not exist and the dissipation occurs at length/time scales of the order of the flow features.

To get accurate vortex shedding you will need accurate discretisation in space and time (use hybrid differencing with blend factor=1.0 and second order time stepping). If you use a turbulence model it will introduce additional dissipation and may well stop the vortex shedding.

Glenn Horrocks

Hello again

thanks rogbrito for the video but I suppose explains to me bad, videos since those there are several in you I had and I have obtained to others of diverse sources but until now all in 2D, now in 3D exists some or somebody has some?

Glenn already entendi what member state there are saying, and I create I have put it in practices, but sigosin to obtain results, associate screen

( no converg )

http://img33.imageshack.us/img33/7509/pruebawxd.jpg
http://img136.imageshack.us/img136/102/prueba2b.jpg

http://img33.imageshack.us/gal.php?g=nuevaimagen1t.png (screen solver manager)

As time follows without appearing vortex, that simulation was of around 18 hrs I stopped and it. (time of real simulation 10.382seg / 1000 timesteps) time of simulation is necessary but so that vortex takes place shedding, according to the sight by my after about 8 - 9 seg vortex tendrian that to be present. or increase I number maximum of timesteps?

In the graphic ones of solver to manager I observe variations, assumes that those variations grow in amplitude soon to stay fixed no?

they excuse my English again, apart from which I am not very good, to try to explain something as technical as this....

Hi,

Can you post your output file and a picture of your mesh?

Glenn Horrocks

Hello

Of mesh it places one above but in which a simulation finishes that this run now, adjunt what these asking to me.

now glenn, you dress the graphic RMS and MAX that behavior is correct?

http://img33.imageshack.us/gal.php?g=nuevaimagen1t.png (screen solver manager)

it excuses to as much insistence glenn, I am thankful for much your aid, without with himself run these simulations with your I appoint you aid in gratefulness of my thesis.


edit

Simulation transient
775 timesteps (stop)
Time real simulation 8.1523 s


http://www.megaupload.com/?d=C17CAE08 (Output file .txt)

http://img41.imageshack.us/gal.php?g=mesh1.jpg (galery mesh and solver manager graphic)

The element size jump from your inflation layers to your tri/tet mesh is too great. Try to make it so the volume of the outer inflation layer equals the volume of the adjacent tri/tet mesh.

Also I think your convergence is tighter than it needs to be, for now just converge to RMS residuals of 1e-4 and do a sensitivity analysis on it later to check whether you need tighter or not.

Glenn

thanks glenn, lets try what you say to me of output cases out some commentary?

you do not think that lowering my Reynolds it can improve chanc of shedding? or increasing it > 4000 and a turbulence model?

in fact the simulation typical are standard, I want to understand the configuration to establish a simulation with my data.

From memory you would expect vortex shedding from Re=100 and up. Low Re flows are easier to simulation so maybe Re=200 or 500 will be an easier starting point. I would go into the laminar flow regime, not turbulent as the CFD is much more precise and accurate in the laminar regime. But you should be able to get vortex shedding in both domains with careful analysis.

Ok glenn. now I am simulating with all the given suggestions.

but the behavior seems to me strange that takes the graphic ones from solver and to not even observe undulations in the flow after the cylinder since I have shown to you.

it observes graphic the present RMS (Simulation run)

http://img199.imageshack.us/img199/6083/laminari.png

strangely the passage of timestep has stopped advancing in the simulation or this of another form it advances to timestep really small, tomorrow post output file and mesh after the variation of the volume in inflation to layer.

the convergence criterion I have touched not yet it, I need to be varying a single parameter until seeing what affects the results to me, if changes several simultaneously I do not go that is to say in what it was failing.

all what has been said this in the following Link

http://img187.imageshack.us/gal.php?g=analysistype.png

This formed according to you say or is necessary to change something to me? in Time duration, I go away by Time total, maximun to number of timesteps or to number of tiemsteps for run?

thanks for the aid and excuse my insistence again

Hello, after trying much and forming, I obtained the results. thanks Glenn
indeed the refining of the meshed one is what but it influences in the results, is necessary very fine meshing in the wall of the cylinder.

thanks again for your time and your knowledge Glenn

This doesn't mean there aren't some really tiny time-scales. Re=1000 is in a very uncomfortable range, unfortunately.

I agree. But using a turbulence model in this Re range is not a good approach in general, so best try to model the small scale stuff directly with a laminar flow model.

For a full understanding of flow past a circular cylinder, see paper by CHK Williamson, published in 1996: "Vortex Dynamics in the Cylinder Wake".
The regime of laminar shedding is between Re = 50-190. Beyond Re = 190, some strange three-dimensional features occur: vortex deformations, then dislocations. In fact, small streamwise vortex structures form beyond Re = 260, indicating that there are eddies with varying frequency present in the cylinder wake at even these reynolds numbers. As the Reynolds number is increased and approaching 1000, there is increased three-dimensionality in the wake until finally transition to a fully turbulent flow (in the wake) occurs beyond Re = 1000.
This three dimensionality is generally not re-producible with U-RANS (unsteady-RANS) based numerical approaches regardless of the mesh density and time step size and must be done with either DES, LES, or DNS. The only known U-RANS approach that actually shows three-dimensional features in the wake is the SST-SAS model in CFX.
Dr. Menter, developed the SST model and the SST-SAS model and also has released many papers discussing the ability of these models to represent turbulent flow properly.