Hi all, I am simulating flows within a naturally ventilated building driven by thermal buoyancy. The plume emitted from the outlet of the building (roof apex) starts to meander during the solution process and this stalls convergence. If I force symmetry by placing a symettrical plane down the centre of the plume then the solution converges fine, but am I actually simulating real conditions by doing this? Could anyone give me some advice on this? thanks. and very much appreciated

The meander is often physical. Think of the wake behind a boat at certain speeds, or the vortices shed behind a truck (lorry, etc) in a certain speed range.

Does the meander propogate itself back into the interior of the building?

I don't think you're simulating a real condition with the symmetry plane. Try pushing the physical effect that's driving your flow (raise the temperatures in the building)to see if the meander disappears at higher velocities.

Interesting problem - and complex. Good luck.

I think this is called 'looping'. It's a natural transient phenomena. Try solving transient, forcing steady state might be the cause of your problems.

I am assuming you are trying to solve for a steady state? You may want to test if an unsteady computation converges. You could then take your unsteady data an perform a time-average over one period of the oscillation. As was pointed out before, the plume may well exhibit a physical instability that leads to this behavior. In that case there is no such thing as a "steady state", and that might explain the numerical problems when trying to solve the steady equations.

However, that doesn't mean you cannot "enforce" some steady solution, like the one you get with the symmetry plane. You are basically forcing a steady state that does not really exist in nature. Likewise, you could apply different numerical integration methods (maybe more diffusive ones) to suppress the instability. Sometimes choosing a coarser grid will lead to enough numerical diffusion to get a (nonphysical) steady state.

I am not saying, this is what you should do. If this is appropriate or not depends on your accuracy requirements and the purpose of your study. Just understand that any solution of the steady-state equations is only an approximation of "time-averaged" flow. And in cases like yours it can be a pretty bad approximation. Just think of the Karman vortex street behind a bluff body in crossflow as another example. A regular steady-state computation will severely underpredict the drag because the unsteady generation of vorticity is suppressed. The more accurate solution (but also more expensive) is to solve the unsteady problem first and then average it.