CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   square cavity? (http://www.cfd-online.com/Forums/main/1297-square-cavity.html)

 chaker September 16, 1999 05:45

square cavity?

Hello, I m working on natural convection in a 2-D square cavity. It s differientially heated by a hot left and cold right vertical wall. Horizontal walls are adiabatic (the problem is well known in literature). I m studying the turbulence case (Rayleigh=5.10^5) using k-epsilon model and wall fonction. I find a big problem in the two corners (up-left) and (down-right). In fact, at these places, a numerical viscosity appear, velocity is irregular, temperature is not stratified,whereas the flow in the other parts of the cavity is good (velocity, temperature, turbulent viscosity). convergence is very slow. if I allow a long iteration time, I find bad result in all the cavity !!

So please could you give me some advises???

my email is:

celamrani@student.ulg.ac.be

thanks a lot

 John C. Chien September 16, 1999 12:45

Re: square cavity?

(1). There is no way one can figure out who you approach the problem and how you solve the problem. (2). Apparently you are not getting good results. (3). I think, you must have generated a mesh and are using a code to solve the governing equations including k-epsilon equations with wall function. (4). There are some general questions you can try to answer first, in this way, you may be able to narrow down the problem area. (5). Is the mesh distribution adequate to handle the boundary layer flows? Here, you can improve the mesh density or arrangement to check the impact on the solution. (6). Is your solution procedure a steady-state approach? If the answer is yes, then you should be able to get a steady-state solution. You may have to use the lower-order accurate numerical scheme first to bring the solution to convergence first. Or, you need to used relaxation factors to control the rate of convergence. If you are writing your own code, you can apply the relaxation on the source terms and the final solution at each iteration. (7). Is your solution procedure transient approach? If the answer is yes, then you need to compute the proper time steps, and the final solution may not be steady-state. That is , it will oscillate all the time but it does not diverge. (8). If you are using someone's code, make sure that the code has been used to solve this type of problems. (9). I would say that over 90% of time, we are not getting good CFD solutions. ( oscillations, negative density, over-flow, ...you name it. CFD is not a fast-food restaurant. It will take years of experience to get reasonable answers.)

 Jin Wook LEE September 17, 1999 04:07

Re: square cavity?

As you said, your problem is very well known one. I myself have had some experience for the entirely same problem, about 14 years ago, but for laminar case. As far as I remember, your problem, for Ra=5.e05, should be laminar natural convection. I remember that natural convective flow in a square cavity is considered as laminar till Ra is order of 1.e06 and turbulent when Ra is greater than order of 1.e08.

My suggestion is, try your simulation with higher Rayleigh number, say, 1.e08. Be careful that thermal boundary layer is very narrow, so that enough grids should be located in the thermal boundary layer. As far as I remember, thermal boundary layer, del/H, is order of Ra^(-1/4).

If you need more information, please send e-mail me. I might have good reference in my old shelf which I guess I can find.

Sincerely, Jinwook

 chaker September 17, 1999 05:34

Re: square cavity?

Sorry, I make a mistake in my text, In fact I simulate a fully turbulent regime with Ra=5. 10^10 and not Ra=5. 10^5.

Mister C.Chien, would you like to explain me little more the relaxation technic ?? thanks a lot

 Mahesh Prakash September 19, 1999 18:10

Re: square cavity?

Dear Chaker,

I have studied your problem at the same Rayleigh number. Well as you might have understood by now, the problem is quite finicky numerically. Try using a very fine mesh close to the wall (not required if you are using the standard k-e model with wall functions. However for such flows it has already been shown that the wall functions used for forced convection flows cannot be applied) if you are using a low Re k-e model.

If you want a reliable converged solution go for a transient medthod eventhough the final solution is steady. Also use an underrelaxation factor of 0.2 for all variables to be on the safer side. Please do not use the central difference schemne. I would suggest you to use either the hybrid or the QUICK scheme.

All the best

 All times are GMT -4. The time now is 21:34.