CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   Under-Relaxation Factors: how to change them (

Chetan Kadakia November 1, 2000 03:57

Under-Relaxation Factors: how to change them
Hi everybody,

I have a general question which will require some detailed answers and perhaps some specific examples.

For accuracy, we are always trying to minimize our residuals and we often change the under-relaxation factors throughout our solution to do so.

But how do we know when to start changing them, which factors to change, and by how much.

I am hoping someone who understands the mathematics involved and/or has much experience with CFD codes is ready to give me a detailed lecture on the use of the Under-relaxation factor.

The Fluent Manual's explanation is to simple and vague.

Harry November 1, 2000 07:37

Re: Under-Relaxation Factors: how to change them
Hello Chetan.. in my experience you must watch your residual, if it's going up that you predict it can't be going down, then you must try to reduce your residual, for example by factor 0.1. For example viscosity is too high (there's a message viscosity limited to viscosity ratio of ....), then reduce the viscosity under relaxation. I think that's trial and error. About the mathematical detail, maybe others can answer it.


Chetan Kadakia November 1, 2000 08:01

Re: Under-Relaxation Factors: how to change them
That is more or less the approach I have taken, but I do not always find it fruitful. When you have a limiting message, it is because your values are beyond your limits for a certain number of cells. But i do not see how that would necessarily make one conclude that under-relaxation factor reductions will improve that calc (unless you re-initialized your solution with new relaxation factor(s). And I sometimes have trouble decifering which factors to change, and by how much. Thanks Harry. Anybody else have any more thoughts..

Sugen Chetty November 1, 2000 11:56

Re: Under-Relaxation Factors: how to change them
Well I've just been doing something with the relaxation factors. Problem was mainly between pressure and dissipation residual.(I hope it's not caused by an error on my part but I checked my model.) Well, the solution diverges after behaving itself for a while. Fluent gives certain guides in the manual. eg. pressure and dissipation relaxation factors must not be greater than 0.2. Adjustment did get rid of the divergence but convergence was slower. I specified different relaxation factors for pressure and dissipation depending on which was converging slower. Pressure was the problem so I set a higher relaxation factor (0.3). That did improve things. I generally don't mess with the minimum residual sum since that may not affect the values since the solution will kick out of a time step loop due to easier tolerance. Also try solving for a few parameters at a time. Residuals for parameters may be interdependant, hence try leaving some trouble one sout until the other ones are lower. This did not always work for me, but it worth a crack.


John C. Chien November 5, 2000 11:36

Re: Under-Relaxation Factors: how to change them
(1). I would say that most people using a commercial code did not really obtained the converged solution, for various reasons. (2). I have used Fluent extensively for two years, using un-structured meshes automatically generated by Tgrid. This was pre-version5 two years ago. (3). I think, the users were frustrated that they just stopped the iteration after so many iterations. And I did the same in the begining. (4). But in the process of checking out the code using simple problems and good quality meshes, I realized that it is possible to reduce the residuals to below 0.000001. So, in most calculations, I simply set the residual limits for every equations to 0.00000001 right from the begining. (5). My suggestion is: try a coarse mesh with high mesh quality first. Run the calculation long enough to reach the residual value below 0.000001 If you can not succeed in doing so, it is hopeless. Once you have done so, then, refine the mesh and run the calculation again, until you reached the same residual limit. (6). The automatically generated mesh, especially in 3-D, in most cases, can not provide uniformly high quality in un-structured mesh for complex geometry. On the surface, the unstructured mesh does have advantages to cover large areas of complex geometry, but, in reality, a high quality mesh is always hard to obtain. So, I was forced to go back to the blocking of the geometry. That is, to divide the geometry into smaller pieces and re-create the surface geometry so that I can avoid the highly skewed cells. (7). In the last two years, I have been using another commercial cfd code strictly in structured blocked meshes. Even though the mesh quality is still an important issue, in most cases, I was able to drive the residuals to well below 0.000001 for 99% of the cases. ( I have been using the code almost day and night for 3-D problems) (8). So, there is a huge difference in the convergence characteristics between the two codes and two kind of meshes (structured vs unstructured mesh). (9). Another suggestion is: if the high accuracy converged solution is important to you, it is very important to use multi-blocked structured mesh which can provide the needed mesh quality and also the good convergence. (10). As for the under-relaxation factors or the time steps, it is a function of your initial flow field guess. you will have to adjust these parameters slowly through the initial phase of iteration process. If you can use the coarse mesh as the initial guess by interpolation, you should have no big trouble to get the converged solution. But the initial guess and the converged solution is highly problem dependent, there is no general guideline to adjust the parameters for the initial phase of iteration. (in this phase, the solution will diverge, regardless of the mesh type, structured or un-structured.) (11). If it is possible, write your own code, using a commercial code generally will take a lot of extra time to deal with issues like mesh quality, and convergence.

All times are GMT -4. The time now is 08:47.