Hi,

I am a Fluent5.0 beginner. Could you help me with a problem ?

I am now running a laminar 3-D case with structured grid, segragated solver. It is very easy for me to get the converged results using 1st order momentum. But when I try the 2nd order momentum. It always spends a lot of time and cannot converge. I also try to change the Pressure-Velocity coupling from SIMPLE to SIMPLEC or reduce the under-relaxation factor that mentioned in the manual. But it still doesnot work at all. According to your experiences, Could you give me some other idea to get the 2nd order converged result ? ( Additionally, I find when I try a much lower entrance Re or a much coarse mesh, it can get a 2nd order convergence. )

Thanks a lot for your time.

Sangrar

1) It is very natural that 2nd order equation is difficult to converge. 2) Many of my junior engineer says that 'it was not converged because residual is higher than convergence criterion of the code'. Of course, residual is very good indicator to judge the convergency. However, please do not absolutely depend on the default criterion provided by your package. You can judge the convergene by yourself. How about to check 'physical reality of the result', 'degree of the change of the result, iteration by iteration' and/or 'comparison with the experimental data or previously published data'......

Sincerely, Jinwook

(1). I do not know what you are trying to achieve. (2). Your experience is fairly typical among CFD users. (3). I do have suggestion that you try something more systematic. (4). First, make the problem 2-D. Then run the code using the first-order method. But, make sure that you set all of the residuals to 1.0E-08. Try to see whether you can get converged solutions. At that point, you should see the the residuals drop to below 1.0E-06 and level-off (flat). (5). Once this is accomplished, increase the mesh density (total number of mesh points or cells) and run the code again. You should do this and plot the results vs the mesh density. You should do this until the result is independent of the mesh density ( increase in mesh density has no effect on the result). (6). The next thing to do is: use the converged solution and the final mesh , set the numerical method to the second-order method and run the code again. At this point, you have a very good initial solution (converged solution) and a fine mesh to begin with, the only change is the numerical method. (7). If you can't get the converged solution with this second-order method, then then it must be a post-doctor research topic. (8). If you can obtain a converged solution with the second-order method, then you can repeat the same processes to solve the 3-D problem. (9). By the way, when eating a hamburger at a fast food shop, you don't have to put everything in it. It is perfectly all right to have a simple hamburger, no cheese, no tomatos, no pickles, no onions. (actually, eating at all-you-can-eat place, you still have to watch your diet or weight. Otherwise, you will have upset stomach .)

Are you sure that the Re number is low enough to allow a laminar solution? Your description of the problems sounds as if the case is turbulent in reality - when you use a finer grid or a better scheme you get less artificial viscosity to stabilise your flow and you obtain a chaotic or turbulent solution which wont stabilize. That is how it should be if your Re number is high enough.

Thanks a lot,

it is interessting to see how experienced "cfd-people" raelize convergence. But I do not understand point 4.)

>But, make sure that you set all of the
>residuals to 1.0E-08.

scaled residuals ? normalized residuals ? absolut ? How can I scale them ?

>Try to see whether you can get converged solutions.
>At that point, you should see the the
>residuals drop to below 1.0E-06

scaled residuals ? normalized residuals ? absolut ?

>and level-off (flat).

Thank you

(1). It simply says that you should ignore the residual constraint, and set it to a very very small number. (2). If you can not reduce the residuals continuously, the flow is oscillating somewhere. It could be the boundary conditions or the mesh problem. (3). the easiest way to make sure that the flow field has converged is to compare the contour plots at two different times (or iterations). When the solution is converged, you will see only one contour plot instead of two. (4). I have been using FieldView to check the convergence based on this method. That is you look at the computed flow field variables directly using the contour plots from two different times (iterations). It is a practical approach.

Hy,

the idea with the contour-plots is really good. I'll try. But nevertheless: If you take the residuals, do you "scale" or "normalize" them or do you take the absolute values ? I have in the moment the problem that my continuity-res is about 1 whereas the others are about 1e-4 ("scaled"). So what can I do ? I hope it is converged (after 3000 iterations..). But I "feel" that there is something with the different "scaling-features" in fluent, because I never had such high conti-residuals and the solution is nevertheless good if you compare it with measurements.

chris

(1). Nobody has explained to me the definition of residuals in the code, so, it is very hard for me to say whether it should be "scaled" or not. I guess, it doesn't matter, as long as you used it consistently throughout the equations. That is, use the same definition for all equations. (2). I can tell you that this residual plots has a very bad effect on the users in industries, and it should be eliminated. When people run a code, the first thing they ask is related to the residuals and the convergence. And there is no answer to it. It is a very very bad problem. The users simply do not know when to stop the calculation based on the residual plots. (3). So, what I usually do is to push the residuals off the scale, that is to run the calculation until they are all below the bottom of the scale. And 1.0E-08 should do that. (4). The standard way (my standard) to monitor the convergence is to plot the variables at certain key locations , in term of the iterations or time. I think, the code you use had the option to do that, as I remember a couple of years ago. I tried the option, but since it required additional graphic resources in display, sometimes it did not work in the network environment I had. (5). The user of a code should be able to set the monitoring point and variable at the begining of the run, and watch the development of the monitored variables on the screen. I hope that commercial code vendor reading this message should change their code operation in this way. (it is a serious quality issue in the industries, if the users of the code do not know when the solution is converged or not. It is possible that even the vendor himself does not know the answer. ) (6). So, all I can say is every user hates to see the residual plots, because it does not tell him when the solution is converged and when to stop the calculation. (7). As for the global continuity, there is a place you can display the mass balance and heat balance around the various boundaries. It is very useful to use that window, because there you can determine the degree of mass balance. This is useful in internal flows, because everywhere in the flow field is different. And the mass conservation will give some indication about the convergence to the steady state. On the other hand, for external flows where there is a large portion of the uniform flow, it is not a good indicator. (8). So, check the global conservation display window to see whether the mass is conserved or not, or try to activate the monitoring of local flow variable or global variable in addition to this almost useless residual plots. ( I must say that I have not used the code for over six months now, so I don't have up-to-date information for you.)

Hi client,

Please keep in mind that laminar flow can become unstable at fairly low Re number. Examples are numerous, the most well-known one being symmetry-breaking and subsequent vortex shedding around a circular cylinder. The symmetry-breaking occurs around Re_D = 40. And solving the flow using steady option with full domain (without any imposed symmetry) at higher Reynolds number won't give converged solution.

Can you please turn on time-dependent option with time step of roughly 0.001 L/U ?