CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Phoenics (https://www.cfd-online.com/Forums/phoenics/)
-   -   divergent (https://www.cfd-online.com/Forums/phoenics/51109-divergent.html)

 ryo September 24, 2000 05:00

divergent

hi,everone i want to know how can i do if the result is divergent after computed by PHOENICS.someone can help me please

 John C. Chien September 25, 2000 00:28

Re: divergent

(1). It is a complex issue, and is a function of mesh quality (non-smooth, or highly stretched or skewed), the initial flow field guess, the geometry of the problem, the boundary conditions, and the relaxation factors, not to mention the turbulence model used. (2). It is a good idea to run some simple cases (tutorial samples) to gain the experience related to these factors. (3). As a rule, try a more uniform and smooth mesh first. Use the first order upwind algorithm, because it is usually more stable than the higher-order methods. Use wall functions. Use smaller relaxation values.( there may be some rules in selecting the relaxation factors for particular algorithm. So, be sure to check the user's guide in this area.)

 Mike Malin September 25, 2000 05:08

Re: divergent

It would be helpful if you could provide some description of precisely what flow situation you are trying to simulate and with what solver option (parabolic or elliptic?, single or two-phase? etc) and what physical models (turbulent or laminar? isothermal or not? etc) and what boundary conditions. Is the problem 1d, 2d or 3d? Is it steady or unsteady? and so on.

Is the divergence immediate? Or does it occur after many iterations or time steps? If the model been convergent, does it suddenly or gradually diverge? Have the solution residuals been oscillating prior to the onset of divergence? and so on.

I don't know if the following is applicable to your situation as I have no idea what you are doing. The advice is that, in addition to what John Chien wrote, the golden rule is to build a cfd model step-by-step on a coarse mesh rather that introduce all the necessary geometrical and physical features all at once on a fine mesh. The temptation to do the latter is always present because 'the client or management wants it now, but preferably yesterday'. However, in my experience a step-by-step approach is usually quicker. The reason is that in the event of convergence problems, the origin of the problems can be detected relatively easily or even identified immediately as the result of the introduction of a new feature. In the event that the model is already built, then check the mesh is reasonable and even if it is, coarsen the mesh if it is too fine to permit quick computer turnaround. Otherwise, unless divergence is very rapid, you will be waiting forever to see the effects of any changes you make. Next, experiment with the numerous relaxation features to try and secure convergence. If this fails, then look at the solution after a few sweeps and examine the flow field very carefully. Sometimes you can identify the growth of the instability from a particular region of the flow. If all this gets you no where, then you have to start simplifying further, e.g. use a uniform density if it is variable, use a fixed eddy viscosity rather than the k-e model, eliminate buoyancy in mixed-convection problems, use very high interphase friction when doing a two-phase Eulerian simulation, and so on. The idea is to get something that converges, and then go on from there.

 All times are GMT -4. The time now is 12:45.