FLUENT  Guidance for accurately simulating unsteady, compressible flow problems with the coupled solver
I'm solving the unsteady supersonic jet flow impinging to deflected wall using coupled explicit solver. But the problem is scale of time marching is too big, and that results in unrealistic wave propagation time(time inaccurate). I didn't use any multigrid, Rsmoothing. I guess that time integration(multistage) scheme affects time marching. How do i tune the option of multistage parameter to get the time accurate solution? To model unsteady flows accuratley in the coupled solver the following should be adhered to: 1) if the explicit time marching scheme is used (Global time stepping ) then the Multigrid & Residual smoothing options should NOT be used. The user specifies the CFL value (typically lower than 1.0) The solver will then determine the appropriate time step to march the solution to the next time level. This method is the most accurate unsteady flow modeling available. The problem is the extereme small time steps taken by the solver to march the solution. another option 2) Use the 1stOrder dualtime stepping (Either in the Explicit or Implicit coupled solver... but it make more sense to use the Implicit solver here due to larger stability limits). In this method the user need sto input two values (1) time step for marching the solution (2) CFL value to be used in converging the solution at each time level (subiterations) It is very important to use a small enough time step so a max of 20 or less subitaration are needed for a converged solution at each time level. If the time step is not small enough then the solution will be diffused as use march in time. So the trick here is to find proper time step for acuurate unsteady flow modeling. (NOTE: the 2ndOrder time discretization should NOT be used for accurate unsteady flow modeling because the solution will be disspersive) (another NOTE: the 1stO and 2ndO I am talking about is for the time discretization and not the spatial discretization) 

