Hi, I have a very simple simulation of transient flow over a flat plate. I want to capture the time-accurate development of the freestream starting from a zero-velocity initial condition. I specified an inlet boundary condition of uniform inflow at 3 m/s and outlet boundary condition of area-avg static pressure of 1 Pa. I set the simulation type to transient with timestep size of 0.00015 s. The grid resolution is such that the Courant number is approximately 1 everywhere in the domain. When I ran the simulation, I expected to see the inflow condition propagate downstream about one cell per timestep, since the Courant number is about 1. However, the transient files show that at Timestep 0, the results are at the initial condition (zero velocity everywhere), but at Timestep 1, the freestream flow in the whole domain suddenly jumped to 3 m/s--the inflow velocity. In other words, it appears that the initial condition is not being respected and the inlet boundary condition is applied across the whole domain after the first timestep. I want to see the flow propagate downstream in a time-accurate manner; am I doing something wrong? (By the way, when I turn off the multigrid solver, the boundary condition seems to propagate downstream properly but then the simulation won't converge.) Thanks, -- Joshua

Hi,

If the fluid is incompressible the speed of sound is infinite so transient pressure waves will not be seen. If you want to model the effects of the pressure wave starting the flow you will need to use a compressible fluid model.

Glenn Horrocks

Hi, thanks Glenn. I understand your argument. However, the question I have is this: if my Courant number is about 1, doesn't this imply that the inlet flow will be marched downstream at about one cell per timestep and the solution will develop incrementally in time? Thanks

Hi,

No. CFX is an implicit solver so signals can propagate across the domain instantaneously. It is only in explicit solvers that signals propagate per timestep.

Glenn Horrocks

Hi. In that case, which flow solver would be able to handle this sort of configuration--that is, where the flow propagates downstream in a time-accurate manner? Do you know of any?

Hi,

Please read my first post in this thread. CFX is correctly simulating the physics as you set it up. You need to implement compressibility to get pressure waves and CFX can do that type of simulations. No need to go to other codes.

Glenn Horrocks