In CFX-10, it can help to set the various numerics options under SOLVER CONTROL:

* VELOCITY PRESSURE COUPLING/Rhie Chow Option = High Resolution . This
reduces wiggle size adjacent to shocks and can also improve stability
* ADVECTION SCHEME/Gradient Relaxation = 0.1 (steady state only) . This
can improve convergence behaviour.
* ADVECTION SCHEME/Blend Factor Relaxation = 0.1

In CFX-11, there is an option to set under SOLVER CONTROL/COMPRESSIBILITY CONTROL the parameters:
* Carbuncle Fix = t . This improves 2D stability adjacent to shocks with high
aspect ratio meshes. For a reason yet to be understood, it can also improve
the path to convergence for steady state calculations. The carbuncle fix
implementation essentially prevents the development of the so called
'carbuncle instability' by 1. reducing the order of the advection scheme in the
area of the shock and 2. by adding some additional dissipation. For more
information on this fix and when it is relevant, please take a look at the
attached powerpoints.
* High Speed Numerics = t. This enables the numerics options listed above
(Carbuncle Fix , as well as SOLVER CONTROL options for CFX-10)

Note also that, for high speed flows, a large timestep can sometimes give better convergence behaviour than a small timestep. This is because in a steady state run a small timestep starts to track the true transient, but not perfectly because we aren't converging each time step. But the transient effects it tries to resolve are complex and can be nasty. A large timestep does not try to track these and can therefore be better behaved. Use a small timestep (CFL~1) only if you want to resolve the true transient; else use a timestep based on L/V for the domain.

Another general recommendation would be to run double precision.

Also sometimes when the flow goes supersonic. setting the expert parameter 'max continuity loops = 2' can help stabilise the run.