vortex shedding
Hi I am using FLUENT to simulate a jet oscillation, which has a strong feedback in practice. I want to get the steady flow field first. Then a disturbance is added at one time. And the model is changed to timedependent to simulate the oscillation. However I even cannot get the steady solution. The flow field is oscillating at the first step. I wonder why? May this be caused by the feedbak effect?

Re: vortex shedding
(1). I think, I know why. There is a name for it. It is called "backyard mechanics". It's fun, but I don't think you are going anywhere. (2). My suggestion is: talk to the support engineer of the software about your idea and problem first to determine the feasibility, then, determine how to set up the problem and whether some training is necessary. (3). I don't think it is a good idea to state explicitly the software name in this way. (4). You must state clearly what you did in setting up the problem in order for others to have an opportunity to answer it.

Re: vortex shedding
Dear FLUENT user,
It's my experience that many inherently unsteady flows (e.g. vortex shedding, precession of vortex core in cyclones, TaylorGoetler instability) won't converge to a steadystate when they are modeled using steady formulation. Instead, under certain conditions, the solutions show oscillatory behaviors that resemble the genuine unsteady phenomena. So, it appears that you have company, at least. In my opinion, the reason perhaps has to do with that the steady formulation, often used in conjunction with underrelaxation as in FLUENT, still allows the salient timedependent nature of the flow to partly embody itself through the NS or RANS equations. I know that people often apply initial perturbation to break symmetry and to subsequently trigger unsteadiness, like an asymmetric disturbance to trigger vortexshedding. You can do that, but then you'll have to make sure that you wait long enough for the effects of artificial disturbance to die out, especially if the magnitude of the disturbance is not small. I'd like to suggest you go ahead and click on "unsteady" botton and see if the vortex shedding you set out to predict comes along. I strongly suspect the vortex shedding will be spontaneous in FLUENT. 
Re: vortex shedding
Thanks for all your advices. In my project, I'm dealing with the fluidic flowmeter, which is similar to vortex meter. But the latter is more familiar to all. And the jet oscillation is inherent just like vortex shedding. The inherent unstable is strong due to the feedback effect. When I first tried, I set the converge limit to be 0.001(default) for steady situation. I got the solution. But when I changed to 0.0001, the oscillation began. So if I try the unsteady botton, how about the converge limit for each time step? How can this value be improved?
Thanks. 
Re: vortex shedding
All that you saw indicates that steadystate solution does not exist for this problem.
I suggest you now move on to timedependent calculation. You can set the convergence criteria (in terms of scaled residual) to 0.0001 for all solution variables. If your time step is small enough accurately to resolve the timescale of the jet oscillation (40  50 time steps in one period of oscillation), the residuals for all solution variables will drop below the convergence criteria in a few or 5 6 iterations per each time step. And I would recommend at least the secondorder spatial and temporal discretization schemes. 
Re: vortex shedding
sir, one of intriguing problems in C.F.D analysis is finding the equation of the twister.this may sound a bit trivial to you but in my respect it's a serious problem i.e if we can find out the equation of the twister and simulate the same thing on the computer then the nature of the cyclone can be predetermined and its area of influence.

Re: vortex shedding
When you are not sure whether the solution has converged or not, it is a good idea to set all the limits (convergence criteria) to 0.00000001 and watch the residual history profile. When the steady state solution does exist, the residual history profile will become flat, and drop below 0.000001. This was based on my experience with Fluent/UNS code in steady state calculations. For Fluent/Rampant ( in Fluent5 the names have been changed), this number (0.000001) is hard to reach. The best way to make sure that the solution has reached a steady state is to plot the flow field contour plots at two different iterations on the top of each other. In this way, you can easily see the difference and the location if the flow field is still changing. In most CFD applications, steady state solutions were not obtained in steady state calculations for different reasons. By the way, residual oscillation or unsteady behavior are in many cases related to the poor mesh used in the computation ( or some poor local cells ). So, before you run any calculation, know your Reynolds number and your mesh. ( make sure that you can obtain a steady state low Reynolds number solution first with a good mesh in using a CFD code.)

All times are GMT 4. The time now is 08:54. 