The difficulties associated with solving compressible flows are a result of the high degree of coupling between the flow velocity, density, pressure, and energy. This coupling may lead to instabilities in the solution process and, therefore, may require special solution techniques in order to obtain a converged solution. In addition, the presence of shocks (discontinuities) in the flow introduces an additional stability problem during the calculation. Solution techniques that may be beneficial in compressible flow calculations include the following:
(Pressure-based solver only) Initialize the flow to be near stagnation (i.e. velocity small but not zero, pressure to inlet total pressure, temperature to inlet total temperature). Turn off the energy equation for the first 50 iterations. Leave the energy under-relaxation at 1. Set the pressure under-relaxation to 0.4, and the momentum under-relaxation to 0.3. After the solution stabilizes and the energy equation has been turned on, increase the pressure under-relaxation to 0.7.
Set reasonable limits
for the temperature and pressure (in the
Solution Limits dialog box) to avoid solution divergence, especially at the start of the calculation. If
ANSYS FLUENT prints messages about temperature or pressure being limited as the solution nears convergence, the high or low computed values may be physical, and you will need to change the limits to allow these values.
If required, begin the calculations using a reduced pressure ratio at the boundaries, increasing the pressure ratio gradually in order to reach the final desired operating condition. If the Mach number is low, you can also consider starting the compressible flow calculation from an incompressible flow solution (although the incompressible flow solution can in some cases be a rather poor initial guess for the compressible calculation).
In some cases, computing an inviscid solution as a starting point may be helpful.
See Chapter
26 for details on the procedures used to make these changes to the solution parameters.
![[ANSYS, Inc. Logo]](fluentlogo.gif)
