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

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

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...

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.

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

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

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

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.

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

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

[maa]

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?

__________________________________________________ _____________

[thecfduser]

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

[Ekiguy]

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

[maa]

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?

[thecfduser]

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....

[maa]

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?

[thecfduser]

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???

[Ekiguy]

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

[thecfduser]

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

[Ekiguy]

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