Tips for successfully modeling cavitation flows in rotating equipment
Cavitation in rotating equipment (e.g. pumps) is an important industrial problem. Fluent 6.1 has a cavitation modes that can be used with rotating reference frames to model cavitation in pumps. However, converging these problems for cases with significant cavitation can be challenging. This solution outlines a procedure that has been found to be successful in a wide range of pump calculations. Additional information can found in the following Technical Note, available from Fluent Inc.:
Kelecy, F.J. (2003)
"Numerical Prediction of Cavitation in a Centrifugal Pump"
TN 211, Fluent Inc.
Consider a pump with a velocity or pressure inlet and a pressure outlet. For simplicity we'll assume that the pump is being modeled as a single blade passage with periodic boundaries using a single moving reference frame (SRF). The working fluid is assumed to be incompressible, and the cavitation model is to be applied to this system. It should be noted that the mixture model version of the cavitation model is used with the Slip Velocity option disabled (that is, we assume the vapor and liquid move with nearly the same velocities though the blade passage). This option could be enabled if desired.
The key to converging the problem is to initialize the solution with a *** single phase solution *** wherein the minimum pressure in the system is above the prescirbed vapor pressure (set in the Define->Models->Multiphase panel). One of the best ways to control this is through the exit pressure - simply set the exit pressure to a high enough value such that the minimum pressure is safely above the vapor pressure. Since the absolute pressure value is not important for an incompressible fluid (only pressure differences are), setting the pressure level in this manner will not affect the single phase solution.
Once the single phase solution has been established, you can then enable the cavitation model. However, it is useful to begin the calculation by *** not changing the exit pressure *** and simply running the model with cavitation turned on. You should not observe any vapor being formed, or if it does (due to fluctuations in pressure), it should rapidly disappear.
When the foregoing solution has converged, you may then reduce the exit pressure to the desired value. If the final exit pressure is significantly different than your initial exit pressure, you should gradually reduce the exit pressure to prevent convergence problems. For example, if your initial back pressure were 500 kPa and your target value was 100 kPa, you can reduce the exit pressure to 400 kPa, converge the solution, reduce it to 300 kPa, converge the solution, and so on until the desired level is reached.
If you encounter convergence difficulties, here are some things you can try to enhance stability:
(1) Reduce the under-relaxation factor for pressure correction equation with the command :
(rpsetvar 'pressure-correction/relax 0.6) or even smaller. The default value is 0.7.
(2) Reduce the relaxation factor for momentum equations. You may try to use the values as small as 0.02 in some cases. The cavitating flow sometimes is similar to swirling flows, and thus it can take a while for the vapor bubbles to stabilize.
(3) Reduce the under-relaxation factors for density & vaporization mass.
(4) Modifying the Multigrid settings in Solve->Controls->Multigrid can sometimes help. I have found that setting the Pressure equation termination criterion to 0.001 (rather than 0.1) and setting the post-sweeps to 3 can make the solution of the pressure equation more robust.