Help on cavity flow
 

hi,there,

when simulating the driven flow in a square cavity,I met a problem,that is,I cannot get the streamline pattern as GHIA(1982,J.COMP.PHYSICS),my primary vortics are always away from the center of the cavity,and a little close to the driven top,no matter what Re num. for my simulation,I donot know why,i use:

1.FVM,Hybrid scheme,nodimensional NSe.

2.Projection-1 method,with pressure omited in the momentum equation for the temperal velocity

3.uniform girds

anyone with experience on cavity flow,please give me some advices,thanks for your time

Re: Help on cavity flow
 

(1). Set your mesh size to 100x100 uniform, and Re=10. And run the case to converge. (2). Use the same mesh and set Re=400, and run another case. (3). Set the mesh size to 200x200, and Re=400, and tun another case. (4). make comparison with published results. (5). Make sure that your solution is mesh independent. And plot the velocity gradient at the center of the moving plate vs the mesh size, until the value is independent of the mesh size. (6). If you are not using the same method as that used by Prof. Ghia, then you are not likely to get the same results. (7). The handling of the boundary will also affect the results.

Re: Help on cavity flow
 

hi,there,

at this time,i meet another question,i am not sure how to get a suitable time step length dt for a given case,on other words,the final converge results seems more dependent on the time step length(dt).because i use projection method,which means,using unsteady NSe for this steady driven flow.the converged results just as following: 1.for Re=10,100x100 mesh,i can use dt=1,the case converges quickly 2.for Re=10,100x100 mesh,if dt=1000,the case also converges quickly.but the results is different from the first case,the difference for streamline maybe large. 3.if the nodimensional time step dt=0.001,the case converges ,but even i stop the code after a lot of time step(i.g.20),i cannot get a good results,or a bad results.the vortice is close the driven top. so,the time step length is more important for me,i want some one to help me. thanks in advance

Re: Help on cavity flow
 

(1). For Re=10 case, keep the mesh size = 100x100, keep the dt=1, and study the convergence of the solution. (2). compare the converged solution with the published results. (3). For this low Re case, study the mesh independent solution. This could be done by using meshes 25x25, 50x50, 100x100, and so forth. (4). I don't know why you are changing the time step from dt=1 to 1000, and 0.001 My feeling is: if your time step is very small, then it will take a long time to converge (like slow motion play back). Large time step is also not a good idea, because it will promote oscillation.

Re: Help on cavity flow
 

Pendy; Have you tried the power law scheme instead of the three straight lines or hybrid scheme?( see Patankar " Numerical heat transfer and fluid flow book. Also if your time step is small enough, you might use the Crank-Niclson scheme for the time discretization. Otherwis, the fully implicit scheme is recommended. Good luck.

Re: Help on cavity flow
 

hi,there,

thanks for help,for cavity flow,if both of small time step and large time step are not suitable,maybe,I can only try again and again and compare the converged solutinos with the published papers,in order to find a suitable time step,but how can I choose a suitable time step for other simulations which cannot be compared with published paper,is there any rule to choose the time step when using unsteady NSe.to get a steady flow?

Re: Help on cavity flow
 

(1). Usually, the method you are using should give you some hints on the time step and the stability. (2). so, it is in the method you are using. In general, the explicit method is quite limited in time step, and small time steps must be used to avoid divergence. (3). For Implicit method, sometimes there is no such limit. So, You will have to check out the method's stability properties first. And in most cases, it is problem dependent (geometry), and is a function of the initial guess of the flow field. (4). All I can say is, you can do more research in this area (as you have been doing, but I don't have the answer.)

Re: Help on cavity flow
 

1. Ghia's solution is based on classical Taylor's series discretisation. It should not matter much, in practicality, if you are using the integral approach (cv fdm - Patankar). Mathematical problem lies in tackling the points of singularities - with coarse grids it gets pronounced. 2. Ghia's formulation excluded the body force terms - the rho*grav - ensure if you are following the same. 3. To arrive at Ghia's results (or very close to it), you have to use 128/129 cvs either direction. Marginal differences in the numerical values in the results will primarily depend on factors like your scheme error, computer precision, etc. 4. Time step : Most important role is played by dt. Arrive at it thru CFL (Courant-Fredrich-Lewy) criteria and grid Fourier No.[consult the book by Anderson, Tannehill and Pletcher]. 5. First try with Re=10 or 100 (128x128 cvs), then with Re=10000 (256x256 cvs). Please remember that with increasing Re, the problem is that one has to get the reduced diffusion flux at the top (if the driving lid is at the top) transmitted inside. For Re>10000, you are likely to experience oscillation [consult archives in this forum).

Wish you the best of luck.

Re: Help on cavity flow
 

> Mathematical problem lies in tackling the points of singularities - with coarse grids it gets pronounced.

Interesting comment/observation!

If there is a singularity (and not inconsistency of BC at the corners), I would think that the coarser the grid is, the more "smoothed" the singularity in the solution will become. As you get the grids finer and finer near the singularity, the solution will have to become more and more singular! After all, the idea is to "capture" the singularity that exists, right?

The "sloppy" handling of inconsistent BC's so that you will get "a" solution (no matter what) has been one of the "blessings" of traditional finite volume formulations (I say traditional because there are BC correction schemes in the literature that don't seem to have permeated in the mainstream - unfortunately)

Adrin Gharakhani

Re: Help on cavity flow
 

(1). Well, for a cancer patient with a few months to live, "a solution" is better than "no solution". (2). So the story is repeated over and over again. (3). The FVM , I think, is well suited for poor people who is interested in instant solution and can't afford the extra effort to make it right.

Re: Help on cavity flow
 

Can we have some more contributions? I focus on the lid driven cavity problem going for a Patankar approach with staggerred grids, etc. What happens to the u-cv adjacent to the singularity especially when the grid is coarse. Let us remember that we solve the continuity not for the same cv (as for u) but for the coresponding main grid point only. Do the u-coefficients required for the continuity (p') not get affected?

Re: Help on cavity flow
 

(1). I don't like the staggered grid approach of Patankar, because, u,v,w,and p are all defined at different locations of a cell. (2). If you have only one control volume (or cell) in the computational domain, then you are going to be very confused. You may want to try out this one cell domain in the moving lid cavity problem.

Re: Help on cavity flow
 

I worked on this problem using FEM recently, both 2D and 3D and got similar results with Dr.Ghia, the mesh size I used is 20X20, and 40X40, Re=100, using coupled solver w/ penalty approach.

However, there is not many references in the literature on segregated solver with collocated nodal properties (correct me if I am wrong). I had a hard time getting it work, but the primary vortex was similar to what Pendy has said...

Any suggestions?

Re: Help on cavity flow
 

The question again is why you are getting a more "singular" solution for the coarse grid! Can you point exactly to the source of the problem? Of course there is the issue of the multiplicity of the velocity at the lid-cavity junction (which is really a modelling issue), but how do you handle that? Also, in a staggered grid system you have to make sure that you account for the "extra/ghost" volumes that go outside the physical domain - make sure there are no leaks (you have to account for them somehow) Other than this I don't exactly understand your statements

Adrin Gharakhani

Re: Help on cavity flow
 

Can I guess that you intended to say "colocated" (all variables defined at the same nodal point)

and not "collocated", which is some sort of interpolation or superposition technique?

Re: Help on cavity flow
 

sorry, my mistake. you are right, co-located, instead of staggered like in FVM.

Re: Help on cavity flow
 

I have the same idea and feeling as Adrin Gharakhani,this is a public place where we can discuss problems,of course,for people who have no experience and meet problem on some simulations,what he or she expect most is to get the answers,and point exactly to the source of the problem.for the above help,I still donot know how to sovle the problem I have met.what's meaning "singular" for this cavity flow?and how to determinate the time-step?

thanks

Re: Help on cavity flow
 

(1). As you can see that even for this seemingly simple square cavity/lid driven problem, the answer to it can be somewhat difficult. This is the reason why it was used as a test case. (2). And think, the problem could be the method you are using, this includes the method, the boundary condition and the implementation (code). (3). I had studied this problem many years ago, using my own method and code. I did not find any big problems. (4). So, my suggestion is: if you are using your own code, then first check it out on simple problems with known analytical solutions first. In this way, you can get the code debugged thoroughly, then apply it to the cavity flow problem. (5). And even in this case, it still depends on the method you used in the code. (6). In most cases, the corner problem is not a critical problem, unless you are the professional. So, you can safely ignore it for the moment. For higher Reynolds number solutions, it is known that you will have to use fine mesh near the wall with non-uniform mesh. Otherwise, solutions for Reynolds number several hundreds have been studied quite often and I think, the solution published in this range should be fairly good. (7). So, keep your Reynolds number in this range first, until you have a good handle of your code.