Doubt regarding Multiphase simulation
 

Hi All

It might be a very basic question, but am not sure about this hence I want your suggestions.

Some people say for Multiphase simulation we need to have a CFL number less than 0.5 always. Is it true for all cases or is it something specific for some case ?

No, not true at all. It is a very common misconception than CFL (or Courant number for incompressible flows) is a fundamental parameter for implicit CFD codes like CFX.

For a start, CFL requires a compressible fluid. CFL is undefined for incompressible fluids. So you cannot use CFL as a criteria for incompressible multiphase models (which is the most common type of multiphase model).

With compressible multiphase models, some multiphase models have simple multiphase characteristics and can handle much bigger timesteps than results from CFL=0.5. Some are very challenging and will require smaller time steps than CFL=0.5.

You determine the time step size for your simulation in CFX by a time step sensitivity study.

So is it only for CFX or in general ? What about multiphase simulation of air bubbles in water channel using OpenFOAM ? There is it important to have CFL less than 0.5 since air bubbles are compressible ? (Sorry maybe I should ask this in OpenFOAM forum), but I thought you might be able to answer this as the physics is same.

There is Compressible and Compressible.

If you use compressible gas (ideal gas) to incorporate density differences as a result of hydrostatic pressure or varying temperature or composition, then consider this as Compressible version1. You can run this using Thermal energy in CFX. Your bubble size may change a little, depending on the static pressure and temperature, composition, etc. No need to limit yourself to CFL=0.5 in CFX.

If you have high velocities and significant gas volume fractions, then things become very complicated since the speed of sound of the mixture drops dramatically. This can result in choking flows with Mach around 1 and beyond. Then you also need to calculate compressible, but with Total Energy (in CFX). I call this Compressible version2. Required time steps will be low, CFL around 0.5.

I think this applies for both CFX and OpenFOAM when using a nice hex mesh. When applying an unstructered mesh, CFX tends to work fine, OpenFOAM is less foregiven and requires smaller steps. Then better use a poly mesh. However, this is based on my OpenFOAM experience some time ago. Possibly things have changed a lot. Better ask the OpenFOAM Forum.

CFX is an implicit solver. In fact most CFD codes are implicit solvers. There is no formal time step restriction on implicit solvers, you set the time step size based on discretisation accuracy and numerical stability considerations. So the way to set the time step size is by a time step size sensitivity study.

Explicit solvers have a hard limit of Courant number = 1 or CFL = 1, and usually they need a safety factor which brings it down to 0.5 to 0.75. This is from the numerical approach used and if you use CFL>1 it will immediately start to diverge. There are not many explicit solvers around, they tend to be mainly used for explosion and impact modelling (very fast transient events).

But a lot of people get the formal limit of explicit solvers confused and think it applies to implicit solvers as well.