Hi, all

I have a question about unsteady 3d flow in an ventilated enclosure and the use of a two equations models. The enclosure is 9m x 3m x 5m (x,y,z) and have a slot inlet just below the ceiling and in the full width of the enclosure. Outlet is in the floor below the inlet, also full width.Inlet velocity is 4 m/s and the slot height is 0.02 m. From experiments we know that the flow will either go to the right wall (standing under the inlet and looking into the enclosure). But sometimes the flow will shift to the other wall (left) for some time and then back again.

When doing simulation of the same enclosue with approx. 100.000 to 400.000 grid points using either k-eps, low Re k-eps, and two-layer wall function with k-eps shows, that k-eps and the low-Re model will always predict that the flow goes to the right wall. With the two-layer k-eps the flow also goes to the left a few times. Unsteady simulation shows then same results.

Should the two-equations turbulence models always predict the same solution ?

Or is this just a non-converged solution, although more that 70.000 iteration has been performed. (I know that the two-layer k-eps model are more expensive than it counterpart)

Or will only LES be able to simulate the true unsteady flow in this case ?????

Thanks in advance.

Regards

J. Roued

If I understand your case right the geometry and the boundary conditions are fully symmetric, but the flow field is not symmetric and sometimes shifts mode from the left wall to the right wall or the opposite. If this is the case then which mode you obtain is dependent on the numerical details of how you solve your equations - grid assymetries, which direction you iterate in etc. Small round-off errors can also make the solver go in one direction. If you use the same solver you will then often obtain the same mode all the time unless you introduce pertubations in the flow field or "switch solution direction".

This is really not a turbulence modeling issue, although the turbulence model might stabilize the problem so that the shifting between modes becomes impossible. It could also perhaps be so that one turblence model gives one mode and another model gives another mode due to the combination of numerics-turbulence model - sounds a bit unlikely in my opinion though. All turbulence models are symmetric of course and do not in themselve introduce any assymetry.

I would guess that it is very difficult to obtain the unsteady mode-shift with a k-epsilon model. LES should have a better chance in theory. Interesting case!

Very good case: I believe a situation like this (with switching between quasi-stable modes) actually happens in reality. I suspect John has just given you the answer, but if you want to be quite sure, you can play a little game: if you take the mesh and renumber it in the reverse cell order (I presume you're using something like Incomplete Cholesky preconditioned solvers), the opposite solution will become more likely. Please tell us what happened... My guess is that the dependence of the preconditioner on cell ordering is enough to make the solution "switch".

Hi..

check this page : www.tfd.chalmers.se/~lada Prof. Davidson has been working on this problem of ventilated enclosures for a while... you may find a lot of other interesting stuff...

take care

mayank

Buoyancy often leads to transient jet/plume behaviour in environemtns such as this (more in a 'vertical' sense though). As your BCs seem symmetric it may well be a numerical issue. Funnily enough it is cases such as this that are used to test/ensure exact symmetric behviour of the solver used by FLOVENT from FLOMERICS. If you are using a structured cartesian grid then you may want to try having both an even number and odd number of cells in the spanwise direction......

Robin.

Hi,

just some question about the experiment. Isn't it possible that the preferred right way of the fluid is due to any micro asimmetry in the model, such as any little difference in the height of the inlet or outlet, or in rugosity and that the switch to the left side id due to any little asimmetry in the inflow? Otherwise, isn't it possible that the asimmetry is due to any external force such as the Coriolis one which are not implemented in the numerical model (I know they are very very little, but in some particular condition they can make the difference)? Thank you for any clarification

Marco

Hi, again

Thanks for the quick reply.

I am pretty sure that the are no buoyancy involved. The experiments are in full scale and any temperatur difference are most certainly below 0.05 C.(the best we could do) The boundary condition are fully symmetric and has be check and recheck due to the unsteady flow. Most research papers about ventilation only concider data in the midt plan of the enclosure and hence does not study (or find) asymmetric 3d flowes.

The grid is structured. But I do not think shifting from even to odd number of cells would resolve the problem. Because the problem has been studied with both a two commecial CFD code and my research code. And with many different grid sizes. (66x32x32 - 98x66x66 and just now I have tested 98x98x98).

More I think that maybe the problem has to do with how well the grid is spaced close to the wall, especially in the spanwise direction. Maybe hyperbolic fucntion is not good when generating the grid spacings ? And that maybe the two-layer k-eps model , which is known for that it requires much more cpu_time to converged to the final solution than k-eps with log-law wall function still has not fully converged ???

regards

Roued

Hi, I do not think that the small asymmetrices will make the big difference. But perhaps rugosity, but why does the simulation for only a few times shift to this other side and not always choose the right side ?? And only when uisng the two-layer k-eps model. The flow solver has been extensively validated for both laminar and turbulence cases. And I am using QUCIK for velocities and Hybrid for all other variables.

The external force such as the Coriolis, maybe, We have talked about it, but as you said not implemented it, yet !

Regards

Roued

In the experiment, is the mode-shift (ie when the flow switches from left to right) a periodic phenomena or does it occur seemingly at random?

If the mode-shift is seemingly random I'd guess that it is very difficult to predict with CFD because that means that it occurs either due to external disturbances or due to growth of coherent structures (in themself caused by small disturbances) - very diffucult to model and predict!

Has anyone heard of someone predicting these type of seemingly random mode-shifts with an unsteady RANS or LES code? Vortex sheddding and similar periodic phenomena must be much easier.

I wouldn't worry too much if my code always gave one of the modes, as long as that mode matches one of the modes in the experiments.

Hi,

The mode-shift is seemingly random, and correlation in time could not be established.

Furthermore, due to the unsteadiness of the flow, it seems like the residuals in the simulation are difficult to bring down when I compare standart k-eps and two-layer k-eps.

Regards

Roued

There is one article on flow attachement due to Coanda effect:

D J Burt, J Stairmand, "Transient Flow in a Load switched fluidic pulser", IMechE, 1993 (C461/041)

I am not sure if it is what you are looking for.

I also think it could be so called "Coanda effect" (attachement of flow to the wall). I know it from fluidic devices (which is not your case), where the side to which the flow is going to attach is given by transverse pressure gradient.

You have almost the same problem in a simpler system. Assuming you have a carnot diffusor, you get experimently three flow cases: The first has a bigger recyrculation domain at the bottom that at the top, the second vice versa and the third has two recirculation domains of the same size. You can get experimenty all three cases if you are patient enough. The CFD-experiment would give you usually only the symmetric solution ( case three ) exept if you use a Gaus Seidel algorithm AND you don't change the solution direction. ( tried as student). Well the real boundary contitions can not always be implemented or some sort of assymetry may occur. You should have the same problem, if you have a cube with a different Temperatur at the top and the bottom of it. Several symmetric solutions do exist but only one occurs in reallity. Anyway don't forget: The simulation is always right but the nature doesn't care about it.

regards I.Dotsikas

(1). I agree. (2). The last sentense should be the only words printed in every CFD books, codes, and forum. (3). I am very happy to know that there is still a real expert among the readers. (4). How do you get the last sentense printed many times here? " The simulation is always right, but the nature doesn't care about it." posted by I. Dotsikas. Is it original? (just kidding) It is really good !!!