Flow over a Circular Cylinder
 

Hi,

Can anyone suggest me how to simulate 2-d flow over a circular cylinder using FLUENT. The simulation should be able to show the vortex shredding too.

Thank you

Sanjay

Re: Flow over a Circular Cylinder
 

Try LES turbulence model. How to setup, i guess you know.

Re: Flow over a Circular Cylinder
 

Hi US,

I don't think LES is an appropriate way to solve this problem, because I should get the vortices behind the cylinder even with laminar model. Vortex shredding has also been reported with k-e and other turbulence models. Moreover, LES requires large amount of grids and hence computation time.Why should not FLUENT work with laminar and other turbulent models ?

Thanks anyway...

Re: Flow over a Circular Cylinder
 

Hello Sanjay,

I am currently working on the same project as yours but mind is more into analysing Cd and Cl of a piggyback pipeline. I use ske model and so far it gives me reasonable results. I'd be happy to cooperate with you.

Thanks.

Sham.

Re: Flow over a Circular Cylinder
 

Hi all!

I think you should start with Laminar flow over 2D cylinder first, and then go to Turbulent flow with some models as you can. It is my opinion. In 2D Cylinder, you can make grid in Gambit and then export to Fluent to set up the Laminar flow. This problem has a lot of paper, you can see them to compare the results.

Pah

Re: Flow over a Circular Cylinder
 

Hi Sham,

Thanks for your mail. I would like to know how you have modeled your flow in FLUENT. I have generated the grid in Gambit and given the boundary conditions. If you can comprehend the steps you followed in FLUENT it would help me a lot.

Thanks anyway...

Sanjay

Re: Flow over a Circular Cylinder
 

Definitely, it always depends on what you have in terms of resources and what amount of details you want. On top of everything, it depends on what is the flow specification and its expected behavior. In the choice of spallart-allmarah, k-eps, k-w, LES or DNS, each has its advantages over the other. But should be kept in mind the limitations each model offers with underlying assumptions, which can affect final results. To keep in mind, it is well known fact that, k-eps model assumes isotropic turbulent visocity. Also, using that near the stagnant body, a special near wall treatment becomes very important. I assumed your flow is very turbulent and LES is definitely superior than k-eps in a larger Re range. But ofcourse, finally it is what you are interested in and the resources you have. -US

Re: Flow over a Circular Cylinder
 

A note: Not the LES but i was intending to write RSM in the place where i wrote LES. Sorry for all trouble it may hv caused to yr minds.

Re: Flow over a Circular Cylinder
 

dear sir use the follwing steps 1-solve laminar flow 2-construct c-grid type:5D upstream(velocity inlet) and above (velocity inlet)and lower(velocity inlet);20D downstream(outflow) 3-solve at Re=100 for example 4- U=1,chang nu according to Re 5-after solving the flow for steady case and obtain the solution 6-convert to unsteady by i-define new custom field function as (y+|y|) /2y(perterpation to cause unsteady) ii-patch all the fluid to have this x velocity after initilazion iii-iterate to t=42 or after with dt=0.02

Have a good Luck

Khairy-Egypt

Re: Flow over a Circular Cylinder
 

Dear Sanjay,

I am using the RSM model to simulate the vortex shedding in a flow past a cylinder. I managed to get twin vortices as well as von karman vortices in unsteady simulations with this turbulence model. Just be sure to have a sufficiently small time step. If you don't want to calculate it, you could easy estimate it by trials watching the vorticity magnitude contours. Just make sure that in the contour panel, the auto range is not enabled for the vorticity and lower the top limit. Then you will be able to watch the vortices. Otherwise, with auto range, The vorticity magnitude near the walls is too high, and the shedding is invisible!

Regards, Ilias

Dear Ilias,

I´m using the RSM model to simulate the vortex shedding in a flow past a cylinder, us you.

The value of drag coefficient is less and the angle of flow separation is higher than the literature values. I try change the y plus for higher value when I do the mesh on Gambit and I changed the intensity of turbulence (1% to 10%) but the results are the same.
Why I´m not getting the same result if the method is the same ? Can yuo help me?

__________________________________________________ _____________

Hi
to simulate vortex schedding, use a DNS (laminar model of Fluent), with of course an unsteady solver. Rans models are bad when the gerometry is symmetric.
Use a fine mesh on the cylinders wall.
If ure cylinder is enough long, u can use 2D. Von karman's instability is a 2D instability.
If ure mesh is fine, u will get the real solution
Regards

This is one classical fluid flow problem. You can find many online tutorials on this, try:

http://www.et.byu.edu/~maynesrd/clas...20Cylinder.pdf

-E

Flow over a circular cylinder
 

Hi,

The problem is that I´m working in turbulent flow (Re= 27 000) using the fluent.

The k-e standard, the k-e RNG and the realizable with the 3 wall function (standard, non-equilibrium, enhanced wall treatment), PRESTO for the discretization of the pressure and PISO for the Pressure-velocity coupling and I don´t have the vortex shedding. The Cl goes to a constant and I don’t have fluctuations.

When I do the mesh I imposed different distance to the wall of the cylinder (y= 0.0005, 0.001, 0.002), however the result is the same. After the simulation I get 7< y+< 37 when I impose y=0.002.
The Cd =0.3 (literature Cd=1.17) and the separation angle is 140 (literature is 120).
What should I do? :confused:

Are u using steady or unsteady solver????

When Re=27 000, it is not a vortex schedding that u are simulating. It is a turbulent flow. U must use turbulence models of course.

For y+, remmeber that it is not a linear function of y.

U must do simulatin, hoping that y+ will be good. If not, u refine ure y, as u was doing....

Flow over a circular cylinder
 

I´m using unsteady and pressure based in solver.

I´m simulate the flow over a circular cylinder.
I need to have the same Cd that I fine in literature because the model used is the same (RNG) but I don´t know what change in my simulation in order to get the same value.
I do the same simulations for a square cylinder and I have good results (equal to the literature).

You could see the x-velocity in the next file.

Should I change the under-relaxation factors pre-define by the Fluent?

It is bizzare to do simulations that are alerady done :)

1-are u verifying that ure simulation is converging at every time step???
2- RNG is a diffusif model. If u use steady simulation u will get the same or better results i think. I see that ure simulation is not capting at all any unsteady motion.
3-In litterature, they was in 2D aslo?
4-Are u using low-Re modification? (differential viscosity)
did u get the good range of y+ yhis time???

From my experience, using a turbulence model diffuses the fluctuations so you wont get any... if you are at a high Re, then you need to really refine your mesh and this will cost you of course... but try not using the turbulence model and refine your mesh...

hope this helps

-E

dont use a turbulence model for a Re=27 000 ?????????????????????????????????????????????????? ?????????????????????????????????????????????????? ?????????

Thecfduser, I know, it doesnt make sense,thats why one needs to greatly refine the mesh...
have you tried it with turbulence model and it worked?

-E

If u are looking for the mean values, u must of course use a turbulence model.
Anyway, it is why we invented turbulence models.

U does not need to refine the mech very much....Only near the solid boundaries if u want to use a low-Re model, or a 2 layer model....

I dont know if a URANS model will be able to capture a non-stationnary flow....but i think no.
We cannot use a DNS for such a flow, unleast u can wait a mont to get a solution

Remember that for such a Re, even in experiences u will not see a vortex schedding (u have it, but u have a lot of other scale eddies...)

Flow over a circular cylinder
 

I need to repeat the simulations because I ´ll work for another Reynolds and I need to know if the results are or not correct.

1- I think that the simulation is converged because I have 20 time step and during the simulation the fluent use only 11 time step to converge.
2- I have done one simulation for RNG steady and the result has the same of the unsteady.
3- In literature they used 2D.
4- I don´t have low-Re modification because I´m using the FLUENT 6.3 and I don´t have that option.

Why shouldn´t I use a turbulence model for Re = 27 000? :confused:

1-Monitor variables. Residuals are not sufficent to judge convergence. Anyway, in my life, i never used more than 2 iterations per time step.... Refine ure time step instead of using 11 iterations by step. if ure time step is dt, u will only resolve correctly the scales wich lifetime is higher than dt/2.
2-Yes because RNG as k-epsilon model is a bit...lets say robust.
In fact, RANS models are models that take average.
In average, u have 50% probability that the first big eddie comes from the top, and 50% that it comes from the down of the cyclinder. So a RANS model wil not give u a vortex schedding because it is doing averages (unleast the model is not highly diffusive, so it will be the NUMERICAL residuals that makes ure vortex schedding start).
3-OK. They are supposing a very long cylinder and uses RANS models (DNS or LES will need 3D, even if the average mean flow is 2D)
4-U have it, but it is for professional so it can only be activated by typing a command line. Anyway, for RNG u still have it in the interface: differentiel viscosity option. U must year a very fine near wall mesh.
U can use an intermediate near wall resolution, wich is the enhanced treatement in FLUENT.

So, to know wich model using, compare with litterature. Find the best model, that u can use it for the rest of ure simulations.
Verify that solution is independant of the grid.
Use steady RANS if the simulation still converging (monitor variables and not only residuals)
An important thing, do a good grid quality. Gambit does not handle body fitted grid and this is a big limitation....

flow over cylinder
 

I modeled 2-D flow over cylinder .ICEMCFD used for grid generation with O-grid.Computational domain like 10d upstream,20d top and bottom,20d downstream.Used BC such that inlet-velocity inlet,oulet-outflow,Top,bottom-symmetry.Firstly for Re=100 with dt=0.01,t=20.compared this Cd=1.31+-0.02 value with research paper data

Vortex Shedding
 

Hi Sanjay

I think the accuracy of capturing vortex shedding is more fundamentally based on the grid that you use.Use a very fine grid in the wake region.Try and control the y+ value also.

I think if you can do this you ca capture vortex shedding with any turbulence model.

Rishikesh

Something odd in inviscid simulation
 

Hi all,
I have done the simulation of inviscid flow in circular cylinder (i just follow the step of http://www.et.byu.edu/~maynesrd/clas...20Cylinder.pdf). I think some thing odd there. I find wake behind the cylinder. How it can be?? In my mind, inviscid flow will not give wake. Is any body can explain the reason??
Thank you
Teguh Hady Ariwibowo