24.3.5 Setting Time-Dependent Parameters for the VOF Model

If you are using the time-dependent volume fraction formulation in ANSYS FLUENT, an explicit solution for the volume fraction is obtained either once each time step or once each iteration, depending upon your inputs to the model. You also have control over the time step used for the volume fraction calculation.

To compute a time-dependent VOF solution, you will need to enable the Transient option in the General task page (and choose the appropriate Transient Formulation in the Solution Methods task page, as discussed in Section  26.12.1).

There are two inputs for the time-dependent calculation for the VOF model:

• By default, ANSYS FLUENT will solve the volume fraction equation(s) once for each time step. This means that the convective flux coefficients appearing in the other transport equations will not be completely updated each iteration, since the volume fraction fields will not change from iteration to iteration.

  If you want ANSYS FLUENT to solve the volume fraction equation(s) at every iteration within a time step, first make sure that you have selected Volume of Fluid from the Model list in the Multiphase Model dialog box, and then enter the following text command in the console:

  define $\rightarrow$ models $\rightarrow$ multiphase $\rightarrow$ volume-fraction-parameters

  When prompted to solve vof every iteration?, enter yes.

  When ANSYS FLUENT solves these equations every iteration, the convective flux coefficients in the other transport equations will be updated based on the updated volume fractions at each iteration. This choice is the less stable of the two, and requires more computational effort per time step than the default choice.

  If you are using sliding meshes, or dynamic meshes with layering and/or remeshing, using the solve vof every iteration? option will yield more accurate results, although at a greater computational cost.

• When ANSYS FLUENT performs a time-dependent VOF calculation, the time step used for the volume fraction calculation will not be the same as the time step used for the rest of the transport equations. ANSYS FLUENT will refine the time step for VOF automatically, based on your input for the maximum Courant Number allowed near the free surface. The Courant number is a dimensionless number that compares the time step in a calculation to the characteristic time of transit of a fluid element across a control volume:

  
  

  
  

  In the region near the fluid interface, ANSYS FLUENT divides the volume of each cell by the sum of the outgoing fluxes. The resulting time represents the time it would take for the fluid to empty out of the cell. The smallest such time is used as the characteristic time of transit for a fluid element across a control volume, as described above. Based upon this time and your input for the maximum allowed Courant Number in the Multiphase Models dialog box, a time step is computed for use in the VOF calculation. For example, if the maximum allowed Courant number is 0.25 (the default), the time step will be chosen to be at most one-fourth the minimum transit time for any cell near the interface.

  Note that these inputs are not required when the implicit scheme is used.