24.7.5 Eulerian Model

Calculating an Initial Solution

To improve convergence behavior, you may want to compute an initial solution before solving the complete Eulerian multiphase model. There are three 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 to obtain 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.

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.

Temporarily Ignoring Lift and Virtual Mass Forces

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.

Selecting the Solution Method

There are three options to solve the coupled system of equations arising in multiphase flows. These options that are available in the Solution Methods task page are:

Phase Coupled SIMPLE   

Multiphase Coupled   

Full Multiphase Coupled   

The Phase Coupled SIMPLE (PC-SIMPLE) is an extension of the SIMPLE algorithm [ 57] to multiphase flows. The velocities are solved coupled by phases in a segregated fashion. Fluxes are reconstructed at the faces of the control volume and then a pressure correction equation is built based on total continuity. The coefficients of the pressure correction equations come from the coupled per phase momentum equations. This method has proven to be robust and it is the only method available for all previous versions of ANSYS FLUENT.

The Multiphase Coupled solves all equations for phase velocity corrections and shared pressure correction simultaneously [ 24]. These methods incorporate the lift forces and the mass transfer terms implicitly into the the general matrix. This method works very efficiently in steady state situations, or for transient problems when larger time steps are required.

The Full Multiphase Coupled option couples velocity corrections, shared pressure corrections, and the correction for volume fraction simultaneously. Theoretically it should be more efficient, however it may have some drawbacks in robustness and CPU time usage. The robustness issue stems from the lack of control of the solution of the volume fraction equation. The continuity constraint (sum of all volume fractions equals 1, and individual values limited between zero and one) cannot be enforced exactly during inner solver iterations, and slight variations from the physical limits may lead to divergence. Research is undergoing in this area to improve the method. The method works well in dilute situations.

Discretization Scheme Selection for the Implicit and Explicit Formulations

When the implicit scheme is used, the available options for Volume Fraction Discretization are

• First Order Upwind

• QUICK

When the explicit scheme is used, the available options for Volume Fraction Discretization are

• First Order Upwind

• Geo-Reconstruct

• CICSAM

• Modified HRIC

• QUICK

When using the explicit scheme Second Order upwind, and Donor-Acceptor can be made available under Volume Fraction Discretization by using the following text command:

solve $\rightarrow$ set $\rightarrow$ expert

You will be asked a series of questions, one of which is

Allow selection of all applicable discretization schemes? [no]

to which you will respond yes.

Using W-Cycle Multigrid

For problems involving a packed-bed granular phase with very small particle sizes (on the order of 10 $\mu$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; i.e., to make sure that the pressure equation is solved to a desired level of convergence within the AMG solver during each global iteration. See Section  24.5.2 for more information about granular phases, and this section in the separate Theory Guide and Section  26.18.3 for details about multigrid cycles.

Including the Anisotropic Drag Law

When using the anisotropic drag law (Section  24.5.8), it is recommended that you start the solution with a lower anisotropy ratio. After you let your solution 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.