I wonder if someone can suggest or direct us. The problem we are about to simulate involve a large shallow channel where one half of the channel is filled with water (Rho = 1000 Kg/m3) and the other half is filled with salted (sea water Rho =1200 kg/m3) The algorithm we us is the collocated FV on 2D grids solving the continuity and the NS eqs and the the concentration transport with the well known Boussinesq approximation. At time t=0 the mixing process start from zero velocity. Our code is not able to predict the flow field we tried different methods to discretize the Boussinesq term and specifying the B.C Can any one help us by running it on Fluent or CFX as we don't have licence for them. It should be straight forward to assign. If you send me your e-mail we can discuss the problem details and maybe you can share us a publication. Thanks

The process is fairly straight forward. How do you update the species concentration (salt)?. The species concentration equation can be uncoupled from the N/E equations and then be solved prior to the solution of the N/E equations in each time-step. If you explain what approach you have chosen to simulate the stratification I might be able to help.

Thanks Mr Kourosh Hejazi for your response, Well, I would think after more testing I concluded that the correct physics may somehow be misplaced or simplified. If you think about the physical problem, we have a free surface on the top of the channel and as you know our channel is initially divided into two fluids sectors (on the left and the right sides). I would think the correct physics should be such that the free surface should moves up pushing the lighter fluid up like a hydraulic jump and a wave should develop on the free surface! That may be why the my solver never converages cause I have fixed grid.

About my recipe it is quite simple: a Finite volume discretization on a collocated 2D grid. I solve the U-V and P coupled and segregate the concentration equation. The Bousinesq term is added in the source term in the v-momentum. I start up from still (flow zero velocity) with the channel divided up into two fluids. I used the transport of density rather than the transport of concentration but this does not change anything since the density is linear function f the concentration. Now, if I put all the boundaries as walls the solution start to converge but when I put the upper boundary as fixed free surface it stalls and nver converge.

You mentioned something about solving the concentration first before the flow, Do you have any reason??

I would like to ask as well when should I expect turbulence to take place in such a problem? Can you highlight your own recipe and the capabilities of the code you have? and computer you use and the equation solver as well.

Do you really mean "collocated"?

"Collocation" is (I think) a method of approximation/interpolation.

"Colocation" is the practice of locating all of the flow variables at the same points on the grid - as opposed to "staggered grid" locations, pressure, etc. in control volume centers, velocities on the edges for example.

That is righ. The usual test for stratification is what you have assumed, a basin (or a channel) with two chambers. The physics you have described is almost what happens in the reality and of course in the numerical simulation, as we should have a free-surface flow. However, it is not like a hydraulic jump, but it is a very advective process which you have described. Therefore, the rigid-lid assumption, would not converge as the high pressure gardients would appear at surface. The simulation needs to be free surface. I see that you are using a coupled approach which is entirely fine. As for the question how my mdoel works: In my model I used a projection method by which a fractional-step approach is used. In this method the advection and diffusion are solved prior to solving the momentum equations. Then a Poisson equation is solved for computing the pressure values and then velocities are updated at the same time-step. The solution to the advection and diffusion can be uncoupled as well, so as solving advection and then diffusion sequentially, but this is not of any problem in your case. The reason for decoupling the concentration (density) from the the solution of N/E equationbs is that for updating the density you could use a higher-order explicit appraoch (I used a fifth-order-accurate upstream centred), and then use the updated density in the solution to the problem (i.e. the N/E equations) but this is not why your program does not converge, it only gives a little bit more accuracy than what you may have used in the coupled approach for the advection terms. As for the turbulence, I used a buoyant k-epsilon model. It is very sensitive to buoyancy terms, I would suggest you get the overal results with constant eddy viscosity distribution, and then deploy a stabdard k-e model and then add the buoyancy terms. About my code as I briefly mentioned it is a 3-D free-surface model with non-hydrostatic pressure in the arbitray Lagrangian-Eulerian (ALE) description, with the capability of solving the stratification. The turbulence model is a k-e model with buoynacy terms. The model is based on projection method. Good luck and if there is something that I could explain more, feel free.

Hi Kourosh Hejazi, I was wondering about the reason that one needs to solve the concentration trasport equation first? Could you suggest some paper that simulate the similar problem where KH vortices develops in the solution? If wonder if you can run this problem on your code and show me some prelimiary results or as you said if it is a standard test case can you send me some results for it if you already have them on shelf. Thanks

You do not have to solve the concentration equation first, but you probably solve it at a fractional-time-step which is probably not when you are solving N/E equations? From what I understand yo have used a coupled approach, which solves the N/E equations implicitly, but the density which appears in N/E equations and the source term in the z-direction momentum equation cannot be solved simultaneously and updated while you are solving the N/E equations? If this is the case then you may solve it prior or after solving the N/E equations at each complete time-step. I solve it prior to the whole solution as it is needed in the turbulence model process as well, but in a temporal-staggered computatioal domain this has very little influence. As for the papers, there are quite few papers about simulation the stratification, but those I have reviewed did not particularly reference the Kelvin-Helmoltz instability. Yes I have some results on few test cases, but I will only be able to forward them to you Tuesday afterwards, as they are on another computer.

Hi, I have some interesting results to share with you. You can download the animation from: http://storm.prohosting.com/tamer008...stratified.avi The animation is for 10 seconds of start from still of two fluids of Rho1=900 and Rho2=1000kg/m3 in 1 mt width x 0.3 m depth container. I just graped frames at 0.2 seconds that is animation does not look continuous. Any suggestions?

Can you give us the exact settings so that I can try it if possible. BTW, I could not run the animation you made. It says data invalid.

Tony

What kind of CFD are you using Tony? Well, the parameter I used are as follows: Initially the flow has zero velocity and one half(left half) of the domain has Rho_1=900 kg/m3 while the right half has Rho2-1000 I use the transport of density intead of the concentration but this should not matter if you are using a some CFD package as the transport equation is dimensionless for C already.

The Bossinesq term is added to the v-momentum in terms of the concentration which is the density in my case so my Beta =1, simply -Rho*9.81*Volume since i am using FVM. The diffusion coeffient in the concentration equation is 1.1e-9 m2/s. My code is double precision as well. I am all boundaries are walls so no slip and no concentration flux (dC/dn=0). My method is second order in time. I had to start with really small time step about 1e-3 sec to achieve convergence used that up to the first second (1000 time step) then I switched to 1e-2 second for the remaining of the simulation i only ran up to 10 seconds.

Hi Tamer,

Is it similar to the Rayleigh-Taylor instability problem (of cause, instead of up/down, you have left/right)? Could you repost your animation? I want to have a clear idea before trying the problem. I would like to test it with the two-phase flow solver (2d/3d) that I am formulating, but I am not sure if it is necessary to include the Bossinesq term.

Later,

Tony

Hi Tony, Ok, the problem is solved you should be able to get it from the same link now: http://storm.prohosting.com/tamer008...stratified.avi

Can you send me your e-mail and your affiliation?

Check your hotmail.

It looks like the website is prohibting the avi files for morality reasons I guess so try instead to download: http://storm.prohosting.com/tamer008...ratified.ravir then change the name to stratified.avi and play it

got it!

Hi,

What's the Reynolds number based on Rho2 = 1000?

Hi Tamer,

I made a similar computation. If you like to see the animation, please indicate where I should send it to you.

Tony, Please send it to my e-mail above, I am interested to see it. If you have large attachment to send you can upload to: http://www.fatfile.com/moreabout.php send me a message through them to download it of their server.