Hi,

I am fluent beginner, trying to model a highly serpentine 3d duct using the coupled scheme and ke model. Experimental resuts verify highly turbulent patterns inside the duct, the duct is about 13 inches in length with and the flow enters at 64m/s. The residuals suddenly jump to a very large value of the order e5. I am initialing the flow at the first 10 milliseconds.I have also tried to keep the courant number low but its just not working. Please help me out with this.

Assuming standard sea level conditions, 64m/s is less than Mach .2, which is in the incompressible subsonic regime. Coupled solver is a density based solver (I know it has some techniques built in to deal with low speed flow, but I've still never had luck with the coupled solver at Mach numbers below .5), so it has a hard time dealing with low speed flows. Try the segregated solver. When switching to the segregated solver, set your control limits (Solve->Controls->Limits) so that you bound the pressure and temperature.

Also, turbulent flow means you need to pay careful attention to your wall mesh. For k-epsilon, make sure your y+ values are either all around 1 (.5 to 1.5) or they are all between 30 and 300. Make sure you have plenty of cells within the boundary layer (7 to 10 is usually recommended). Also, you shouldn't have any cell growth rate higher than 1.2.

Along with all of that, you have to be careful of your boundary condition choices. Pressure Inlet and Pressure Outlet are pretty reliable. Velocity Inlet shouldn't be combined with Pressure outlet when using the ideal gas law. Read through the manual on BCs for more information.

Hope this helps, and good luck, Jason