Hello,everyone! what's the difference between the segerated solver and the coupled solver? i can use the coupled solver to compute. but when i use the the segerated solver to compute, there will be an error like this:"absolute pressure limited to 1.000000e+000 in 18 cells on zone 2 turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 81 cells" why? the material is idea-gas, thanks to every who can answer my question. my email is "xupengxian@gmail.com"

You check ur initilization condition Also u can increase the limit for turbulent viscosity ( It can be change from Solutuin control limit panel) i hope this will solve ur problem

thank you i have tried what you said ,but it does not work. maybe, it doesn't converge

Choice of solvers depends heavily on the model being solved. The segregated solver solves based on the pressure, while the coupled solver solves based on density. This makes the segregated solver better at low speed flows and the coupled solver better at solving transonic / supersonic cases. I wouldn't recommend the coupled solver at any flows below Mach .4 (until the pressure based coupled solver comes out in the next release of Fluent). I've used the Segregated solver up to Mach 1.5 with great results, but the higher speed, the more mesh dependent you become (because the segregated solver tends to "smooth out" shocks), so you have to pay a lot of attention to your meshing.

The coupled solver tends to be more stable with the defaults settings. The segregated solver tends to be very sensitive to the allowable limits. When trying to get a solution with the segregated solver, DO NOT increase the turbulent viscosity ratio limit (unless you have a great reason to based on past experience or the physics of your current model truly exceeding that limit, but I've never even heard of that being realistic). Instead limit the pressure and temperature limits to reasonable limits (i.e. Plimits = Pstatic +/- (2 * dynamic pressure), and calculate the appropriate temps). You need to give the solution "room to move" while it reaches a solution, but you don't want to give it enough room where it goes out to some totally impossible numbers, and the limits help prevent this.

The other thing to look at is to find the area that's giving the TVR warning (use the Plot->Contours, select the volume and then play with the limits so that you can just see the areas that have very high TVRs) and check the mesh in these areas. Is it refined enough? Is there highly skewed elements? High aspect ratios? Are the surfaces messed up for some reason? These kinds of things.

Hope this helps, and good luck, Jason