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, R-smoothing. I guess that time integration(multi-stage) 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.
2) Use the 1st-Order dual-time 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 2nd-Order time discretization should NOT be used for accurate
unsteady flow modeling because the solution will be disspersive)
(another NOTE: the 1st-O and 2nd-O I am talking about is for the time discretization
and not the spatial discretization)