To improve convergence behavior, you may want to compute an initial solution before solving the complete Eulerian multiphase model. There are multiple methods you can use to obtain an initial solution for an Eulerian multiphase calculation:
Set up and solve the problem using the mixture model (with slip velocities) instead of the Eulerian model. You can then enable the Eulerian model, complete the setup, and continue the calculation using the mixture-model solution as a starting point.
Set up the Eulerian multiphase calculation as usual, but compute the flow for only the primary phase. To do this, deselect Volume Fraction in the Equations list in the Equations Dialog Box. Once you have obtained an initial solution for the primary phase, turn the volume fraction equations back on and continue the calculation for all phases.
Use the mass-flow inlet boundary condition to initialize the flow conditions. It is recommended that you set the value of the volume fraction close to the value of the volume fraction at the inlet.
At the beginning of the solution, a lower time step is recommended in order to reach convergence.
If using the volume fraction explicit scheme, do not start with a large Courant number at the beginning of your run.
If using the volume fraction explicit scheme, start a run with a lower time step and then increase the time step size. Alternatively, this could be done by using variable time stepping, which would increase the time step size based on the input parameters.
For problems involving a free surface or sharp interfaces between the phases, it is recommended that you use the symmetric drag law, available in the Phase Interaction Dialog Box.
Variable time stepping is not recommended for compressible flows.
Important: You should not try to use a single-phase solution obtained without the mixture or Eulerian model as a starting point for an Eulerian multiphase calculation. Doing so will not improve convergence, and may make it even more difficult for the flow to converge.
If you are planning to include the effects of lift and/or virtual mass forces in a steady-state Eulerian multiphase simulation, you can often reduce stability problems that sometimes occur in the early stages of the calculation by temporarily ignoring the action of the lift and the virtual mass forces. Once the solution without these forces starts to converge, you can interrupt the calculation, define these forces appropriately, and continue the calculation.
For problems involving a packed-bed granular phase with very
small particle sizes (on the order of 10 m), convergence can be obtained
by using the W-cycle multigrid for the pressure. In the Multigrid tab, under Fixed Cycle Parameters in the Advanced Solution Controls Dialog Box, you
may need to use higher values for Pre-Sweeps, Post-Sweeps, and Max Cycles. When
you are choosing the values for these parameters, you should also
increase the Verbosity to
1 in order to monitor the AMG performance; that is, to make sure that
the pressure equation is solved to a desired level of convergence
within the AMG solver during each global iteration. See Defining the Phases for the Eulerian Model for more information about
granular phases, and The V and W Cycles in the Theory Guide and Modifying Algebraic Multigrid Parameters for details about multigrid
cycles.
When using the anisotropic drag law (Including the Multi-Fluid VOF Model), it is recommended that you start the solution with a lower anisotropy ratio. After your solution has run for some time, you can then increase the ratio by reducing the friction factor in the tangential direction. Note that You can also start the solution with the symmetric drag law, then change to the anisotropic drag law.
Using a smaller under-relaxation for pressure and momentum may also help in convergence for cases with a higher anisotropy ratio.
If the flow for a particular phase is important in both directions
(normal and tangential to the interface), use a lower anisotropy ratio,
between 100-1000. A higher anisotropy ratio might cause an unstable
solution for such cases. For a higher anisotropy ratio of more than
1000, a smaller under-relaxation for pressure and momentum is recommended.
When using the coupled multiphase solver, if the solution is unstable
with a higher anisotropy ratio, then reducing the courant number may
be beneficial. Anisotropic Drag Method [1],
with Viscosity option [2] is recommended
for a higher viscosity ratio.
For the Eulerian multiphase model, the Non-Iterative Time Advancement (NITA) scheme uses PISO as a pressure velocity coupling method, where the pressure correction equation is solved in two steps named predictor and corrector.
For the face pressure calculation, the Eulerian multiphase model uses PRESTO as a default method for both the predictor and corrector steps. You can change it to the Second Order method using the following text command:
solve/set/multiphase-numerics/nita-controls/face-pressure-options
If you selected PRESTO for the predictor step, then you can select either the PRESTO or Second Order method for the corrector step. If, however, you selected the Second Order method for the predictor step, then ANSYS Fluent will use the Second Order method for the corrector step also.
Note that when PRESTO is used for the face pressure calculation, the impact of fluxes on the face pressure is inversely proportional to the time step size, which may lead to numerical problems as the time step size decreases. Therefore, the exclusion of transient terms is recommended for very small time steps when using PRESTO:
exclude transient terms in face pressure calculation? [no]
yes