Increasing instability for flow around as cylinder.
 

I am currently attempting to model flow around a stationary cylinder at a Re=200,000 using Fluent 14. However, after running my simulation it appears my solution is too steady as no vortex shedding occurs.
I am currently using the URANS solver coupled with the K-e turbulance model and have tried running the simulation.
I originally used a 1st order upwind scheme and left the Pressure - Velocity coupling as SIMPLE. I then changed this to a 2nd order upwind scheme and used the PISO to do the pressure - velocity coupling.
I have found my wall y+ value and applied the appropriate wall function to my simulation but in doing so i coarsened my mesh.

Does anybody have any suggestions on how to create instability in the flow and hence produce vortex shedding?

How long have you been waiting? My experience is that you have to wait quite a long time until von Karman shows up...
Is your timestep small enough?

My time step was originally 0.1s but I then changed this to 0.05s.

What is the radius of your cylinder and the velocity of your fluid?

what about your grid resolution? have you used second order accuracy in time?
check also the value in time of the vertcal component in some points at the rear of the cylinder, along the longitudinal direction, and see if it is really steady for several non-dimensional time unit.

My radius is 0.5m and my flow velocity is 2.364 m/s.

Ok, that sounds ok for the time step. Now, could you post a picture of your mesh?

How many timesteps have you been waiting before you stopped?

Sorry for the slow reply I have been out of the office for a while. I am currently running 600 time steps.

The mesh i am using is posted below, along the axis it has 96 elements with a bias factor of 10. The average element size was 0.328125m which gives a CFL=0.3602.

The time step accuracy is second order, I have been assuming it is steady as on my Cl vs time plot (otherwise known as convergence history) I have an oscillating graph which quickly dampens wafter 20% of the time has been ran.

Is there any good fluent literature or troubleshooting websites that either of you could recommend.

I dont find it...

Sorry it is in the attachment of this post

What is your y+ currently?

I do not have a exact value for the y+ around the cylinder, but the values range between 50 - 850. I have attached the plot below.

That means you are using wall functions. Maybe these wall functions restrain eddy shedding? Did you try to resolve the sheath (y+<=1)?

BTW: I don't think you need a turbulent inlet flow to get a von Kármán street. As I understand it, it is an instability that has in the first instance nothing to do with turbulence.

Are you using air? I quickly rebuild your case and I am getting a nice vortex street right from the start... Maybe you should post your settings...

You can try giving it just a little kick of angle of attack so the problem is not completely symmetric.

That being said, the instability should develop on it's own even if things were "symmetric" but it will take a while. The time to instability is dependent on how accurate the numerical method is. If it was "perfectly" accurate, the problem will theoretically remain symmetric. In other words, it is statically stable but dynamically unstable. However, I'm not sure what your turbulence model will do. It may dampen out the dynamic instability. This is a reason DES is used.

Oh, one thing to watch is lift. If it starts to oscillate from machine zero you're on your way. But, it sounds like this was zero for you? And, just to be clear, you do have two big vortices (symmetric about x axis) behind your cylinder?

i had this issue for long time with lattice boltzmann, every time i tried i got exactly like this. No vortex shedding, untill i put the outer boundaries far away.

But do you think his domain looks like it is too small compared to the radius?

In my opinion, the grid is extended enough from the cylinder, perhaps I don't understand the requirement to use an O-grid ...
First, the instability should appear also for laminar flows, therefore I would try the solver without any tubrulence modelling, then I see only 600 time-steps that can be not sufficient to develop instability. An acceleration of the onset of the instability can be obtained by prescribing small fluctuations in the initial condition.
Finally, owing to the particular shape of the grid, I would take attention to the outflow conditions

can't really say. Because with iNavier and old versions of fluent like fluent 6.3 i could get vortex shedding even when boundaries were close.

I was just sharing my experience with such problem how it went away. So it is worth trying. Personally I do think with finite volume codes like fluent starccm he should have got this vortex shedding without much of hassle.

that may very well be the issue here. It usually requires much larger number of steps to get.