I am in the ventilation business and usually deal with air flow in room-like enclosures. For time-independent boundaries I was expecting steady flow. But running steady CFD I often observe fluctuating, non-decaying residuals. Recently I learned that flow can be unsteady even for time-independent boundaries. Running unsteady CFD then leads to smoothly decaying residuals. Can I conclude that my case is (physically) unsteady and that treating it with a steady CFD-code will produce "garbage"? Is there a way to tell from the case definition (length scales, velocities, temperature differences, densities, viscosities, etc.) whether it will produce unsteady flow? I am thinking of something like the Reynolds-Number to tell whether a flow will be turbulent.

With respect to interpretting results of a steady simulation that is undergoing limit cycles (i.e., the residual fluctuates about some floor that is higher than the expected converged floor), you need to be careful. You certainly cannot extract frequency data from the simulation. However, the mean solution (i.e. the solution averaged over the limit cycles) may be reasonable. It depends on the case and what you are trying to extract. I believe trying to extract an RMS value would be futile in any case.

In general, unless your numerical method is overly dissipative, you will have problems converging solutions that contain large separation regions. In these cases, you are better off performing an unsteady simulation. In any event, limit cycling is usually a good indicator for the presence of large regions of unsteadiness.

Thanks, Jake. Are there other comments/opinions/advice?

Maybe some more information: the cases I have to deal with frequently contain buoyant plumes. From the Re-Number, I am expecting turbulent flow, so I employ a turbulence model (RNG k-e). The unsteady turbulent fluctuations of the problem definition are handeled by the k-e turbulence model. But on top of that there could possibly be unsteady behaviour of the mean flow. This is the point where I am asking you for help. How can I determine whether the mean flow will be unsteady? Or how does the CFD model distinguish between these two types of unsteadiness (turbulent fluctuations vs. mean flow)? Thanks.

Felix,

From my experience, CFD modelling of an environment containing bouyant plumes must be done using an unsteady solver. This is because of the inherent phenomenon of "meandering" or "looping". These phenomena result in unsteadiness with too low a frequency for the turbulence model to average out (just look at the plume from a cigarette in a still env). If you badly need a steady-state simulation you can suppress the unsteadiness via numerical schemes, or use a plane of symmetry, or find the period of fluctuation and then average over that.

In any case the resulting sim. will be less accurate than a full unsteady sim.; the degree of inaccuracy will need to be determined by running and validating an unsteady case anyways!

I don't think the issue here is the type of RANS model you use; that will come into play when you are tweaking at a later stage. Best of luck

T

Tom, thanks for sharing your experience.

Do you (or anybody else) happen to know the frequency up to which the RANS model averages the turbulent fluctuations? [Obviously I only have an understaning of RANS at the level of introductory texts.]

I still have the problem of understanding the difference between turbulent unsteadiness (which is averaged in any RANS model) and "mean flow unsteadiness".

Thanks.

Just like it becomes fuzzy which spatial scales are resolved and which ones are modeled in an LES, which temporal scales are resolved by an unsteady RANS simulation becomes fuzzy. I.e., since the numerical methods smoothly vary from accurate to inaccurate as the signal resolution decays, you cannot define a sharp cut-off. There is definately some hand waving going on (at least with conventional methods).

Typically, you have some idea of the frequency range of importance in your problem. You must then estimate the spatial size of the flow structures responsible for these frequencies (for instance, by considering the speed at which you expect these structures to be moving.) Your grid needs to accurately resolve these structures. Then, you must choose a timestep that accurately resolves the frequency range of interest.

A more interesting question might be, which scales are modeled and which are simulated if the grid is infinitely fine and the timestep is infinitely small. RANS does not revert to DNS in this limit, so I would expect a steady RANS solution for a turbulent flat plate boundary layer, for example. I would guess that it depends on the turbulence model being used and the empiricism that is fed into it.

Felix,

If you run your solver in a steady mode, ie local time stepping, and you get non-decaying residuals and an unsteady flow field, it does not necessarily mean your flow is unsteady. If then you run the case in an unsteady manner, ie. global time stepping and the residuals decay nicely, then what you had was a numerical instability based on the fact that your solution was not advancing uniformly everywhere. If this is the case you then need to check the unsteady solution to see if it is really unsteady. Save the solution at a regular frequency and see if there is a time varying component to it. In my experience the solution usually becomes steady - the only unsteadyness was numerical.