I'm working with FLUENT 5.4, and find that the iteration rate with Segregated solver is much higher than that with Coupled solver. Now I have obtained a converged solution using the Segregated one. How ever, I am not clear whether it is accurate or not. Is the Coupled solver is more accurate than the Segregated one?

thanks. sean.

If you have converged solutions, they should be equally accurate. The iteration rate with the segregate solver may be higher, but you need many more iteration to reach a converged solution. The coupled solver is more efficient. With a coupled solver, you might get a converged solution in a few dozen iterations where with the segregate solver it may take a few hundred or even thousands.

Just a few comments - if you have shocks the coupled solver resolves them much better. Only use the segregated solver for incompressible and subsonic cases.

I don't agree that the coupled solver is faster in general. For most low-speed pressure driven cases the segregated solver is much faster. The coupled solver can be more robust if you have, for example, strong system rotation, or other things which make the problem more stiff. I used to use the coupled solver much more than I do now. I come from the "compressible" world of CFD and hence that was my first choice. With time the segregated solver has become my favoutite though. It is really a very robust and fast solver for being a commercial code. The coupled solver needs some further work from Fluent to come close to the numerics of other good coupled solvers IMHO.

I must say I don't have experience with Fluent's coupled solver. My experience has been with CFX TascFlow's solver which is fantastic. So I agree that how they implement it is important.

I've also heard that TascFlow's coupled solver is very good. I haven't had the chance to test it myself though. Anyone who have experence from both Fluent's coupled solver and TascFlow's coupled solver?

(1). I have used Fluent codes and CFX-TASCflow codes extensively in the last several years. (2). I think, the Fluent/coupled used to be called Fluent/Rampant which is "density-based". This is the main-stream approach for compressible flows and is always a transient approach. It tries to capture the waves, sound waves, Mach waves, or shock waves. It is not suitable for low subsonic flows, in general. Therefore, it is not suitable for internal flows, which is mostly subsonic. (3). The CFX-TASCflow code is "pressure-based". I called this the "Imperial College approach", suitable for subsonic flows. It is incompressible-flow based with upwind schemes. In the turbomachinery applications, if you use the wall function (which is not a good choice anyway) with corase mesh, the convergence speed is faster than the "density-based appraoch" (this is well-known fact in general, that's why you need super-computers) (4). The problem is: when you are looking for accurate solution, say using Low Renolds number turbulence model (Tascflow has a 2-layer model)instead of using wall function treatment, you will need fine mesh near the wall. In this case, it is very hard to get the code started. It diverged right away. And the only way to get it started was to use extremely small time step (it is a transient formulation), and ramp up the time step gradually. It required a lot of effort to do so. Well, when you can put it under the control, it will converge faster. (5). So, when someone says he is getting fast convergence, you have to guess that he is getting not-so accurate solutions. (relative to my requirement) (6). So, one should not make the direct comparison between the two. They are two different things, meant for different flow problems. But TASCflow by formulation is suitable for internal flows. (this does not mean that the solution is accurate. The loss predicted for turbomachinery flow were several times off.)

Dear Alex, I agree with your opion. I found that when I run the coupled solver, then hard-disk shakes and the machine becomes so slow in responsing me. One iteration may cost scores of hours. On the other hand, the segerated one convergences much faster. Though it may cost more iterations, I do get a solution. Of course, I am computing a incompressible and subsonic gas flow.