Can you give me some recommendations on how I can effectively model transient free surface flows such as in ink jets with FLUENT?

Use the Volume of Fluid (VOF) model in FLUENT to model free surface flows. Some recommendations for the mesh and solver settings are given below:

Although the VOF model will work with any mesh type, quad cells in 2D and hex cells in 3D are recommended for free surface flows. Also, try to make the mesh as uniform as possible.

Use the PRESTO! Pressure interpolation scheme for Pressure under "Discretization" in the Solution Controls GUI panel (SolveControls Solution...). Make sure that the "Implicit Body Force" formulation (in Define  Models  Multiphase) is NOT activated. If your model contains Tri/Tet cells, use "Body Force Weighted" for Pressure discretization in the Solution Controls GUI panel and activate the "Implicit Body Force" formulation in the Multiphase Model GUI panel (Define Models  Multiphase).

Use "PISO" for Pressure-Velocity Coupling in the Solution Controls GUI panel (Solve  Controls Solution...).

Set all the Under-Relaxation Factors in the Solution Controls GUI panel to 1 and run the calculation for a few time steps to observe convergence behavior. If the convergence behavior is poor, reduce the under-relaxation factor for Momentum to 0.7 and run the calculation again for a few time steps. If convergence is still hard to achieve, lower the under-relaxation factors for Pressure to 0.5 and Volume Fraction to 0.5.

Select a time step size (when you start iterating) such that the solution converges within 20 to 30 iterations at each time step. To determine this, set the maximum iterations per time step to a large number initially (say, 100) and experiment with the time step size to determine how many iterations the solution converges in.

As for convergence criteria (Solve MonitorsResidual), use 1.0e-04 for all variables if your model has inlet/outlet boundary conditions. Otherwise, use the default 1.0e-03 value.

You may also want to use the double precision version of FLUENT if your model involves very small length scales.

Show Form
No comments yet. Be the first to add a comment!