The coupled with volume fractions option has the following limitations:

Recommended uses of the coupled with volume fractions option:

For a multiphase flow, the sum of the phase volume fractions must always equal 1. By default, Fluent enforces this constraint by solving the volume fraction equations for each of the secondary phases and then setting the volume fraction of the primary phase to the complement.

In certain cases, where poor convergence and/or mass imbalance are observed, enabling Solve N-Phase Volume Fraction Equations may improve solutions, although in practice the results obtained from using this option are case dependent. If selected, this option will solve all volume fraction equations, including both primary and secondary phases. The resulting phase volume fractions are then scaled in order to satisfy the requirement of summing to 1. This approach is more computationally expensive than the default approach and, in general, should not be necessary for the simulation.

Ansys Fluent provides you with the tools to manage the version-specific defaults.

Starting from version 2020-R1, for newly created cases, the new multiphase defaults will be applied automatically. If you read in an old case file saved in any version prior to Ansys Fluent 2020 R1, the existing settings will be respected.

If you want to apply the new multiphase defaults to the pre 2020-R1 case, you can issue the text user interface (TUI) command as shown in the example below. The information about the new settings will be printed in the Ansys Fluent console. You can review these settings prior to executing the changes.

solve/set/multiphase-numerics/default-controls/
recommended-defaults-for-existing-cases

The multiphase flow default changes integrated in Fluent version 2020-R1 are 
as follows: 
 Operating Conditions :
  - In case of gravity, the operating density method is changed to minimum 
    of phase averaged densities.
 Surface Tension :
 - For surface tension force modeling, the number of smoothings for volume 
   fraction is changed to 2. 
 Initialization :
 - The Patch Reconstructed Interface and Volumetric Smoothing options are 
   enabled. 
 - The Volumetric Smooting Relaxation Factor is changed to 0.5. 
 - These settings are applied when executing the Patch and Smooth commands.
 Solver Methods :
 - The unstructured variant of PRESTO is enforced irrespective of a mesh type.

Do you want to execute these default changes? [no] yes

To revert some of the new defaults to the pre-R20.1 default settings, you can use the text commands shown in the example below:

Revert to the old default of operating density method? [no] yes
  - the operating density method has changed to mixture-averaged.
Revert to the old default of volume fraction smoothings for surface tension? [no] 
yes
  - the number of volume fraction smoothings has changed to 1.
Revert to the old variant of PRESTO for cases using structured mesh? [no] yes
  - the structured variant of PRESTO has been enabled for structured mesh.

The VOF model is numerically more challenging compared to other models due to resolution of sharp discontinuities in the flow system. Body force and pressure gradient imbalances near free surface may lead to unphysical acceleration of the lighter phase. Diffusing these discontinuities adversely affects the interface accuracy; therefore, it may not be an efficient approach.

Complex VOF applications may also suffer from solution instabilities due to several other reasons:

Ansys Fluent offers the following options for controlling the solution process:

To access the stabilization methods:

To access the velocity limiting treatment:

The solution stabilization controls can be also set in the Text User Interface (TUI). The TUI also provides additional options.

The site of the reference pressure can be moved to a location that will result in less round-off in the pressure calculation. By default, the reference pressure location is the center of the cell at or closest to the point (0,0,0). You can move this location by specifying a new Reference Pressure Location in the Operating Conditions Dialog Box.

 Setup →   Cell Zone Conditions → Operating Conditions...

The position that you choose should be in a region that will always contain the least dense of the fluids (for example, the gas phase, if you have a gas phase and one or more liquid phases). This is because variations in the static pressure are larger in a more dense fluid than in a less dense fluid, given the same velocity distribution. If the zero of the relative pressure field is in a region where the pressure variations are small, less round-off will occur than if the variations occur in a field of large nonzero values. Thus in systems containing air and water, for example, it is important that the reference pressure location be in the portion of the domain filled with air rather than that filled with water.

For all VOF calculations, you should use the body-force-weighted pressure interpolation scheme or the PRESTO! scheme.

 Solution →   Controls

By default, Ansys Fluent uses an unstructured variant of the PRESTO pressure scheme for all types of meshes. For cases created in versions prior to Ansys Fluent 2020 R1, the structured variant of the PRESTO scheme will be used for structured meshes.

To enable the unstructured variant of the PRESTO scheme, use the following text command:

solve/set/vof-numerics

When prompted with

Use unstructured variant of PRESTO pressure scheme? [no]

Answer yes.

The availability of discretization schemes for volume fraction is summarized in Spatial Discretization Schemes for Volume Fraction.

If you are modeling a sharp interface regime on meshes that have high aspect ratio cells, large jumps in cell size, or high skewness, interface capturing schemes such as Compressive and CICSAM will not produce very sharp results. For such cases, you should use the Geo-Reconstruct scheme.

For meshes of good quality, it is recommended that you use the Compressive scheme, which is available in both explicit and implicit formulations and is applicable to both sharp and dispersed flow regimes. The Compressive scheme also provides better accuracy compared with CICSAM and Modified HRIC for most cases. When used with the implicit formulation and the second order time scheme, the Compressive scheme produces quite a sharp interface.

When using the Compressive spatial discretization scheme, it is recommended that you use step-wise sharpening after the flow transitions from the diffused zone to the sharpening zone. In other words, you would want to transition from first order to second order, followed by a transition from second order to compressive. You would want to take this approach if the flow has a smooth transition from a sharp interfacial zone to a diffused interfacial zone. However, if the flow has a nonuniform transition from a diffused interfacial zone to a sharp interfacial zone, this might create unphysical sharpening of the interface if not handled properly, especially for transient cases. For example, transitioning from a slope limiter of 2 (compressive) to a slope limiter of 0 or 1 (first order or second order) might be acceptable, but a first order to compressive transition might create unphysical sharpening of the interface.

If you are solving a problem with the evaporation-condensation mass transfer mechanism enabled (Including Mass Transfer Effects) it is recommended that you use one of the diffusive interface capturing schemes such as QUICK, HRIC, or Phase Localized Compressive (Discretizing Using the Phase Localized Compressive Scheme).

In VOF modeling, using a high-order discretization scheme for the momentum transport equations may reduce the stability of the solution compared to cases using first-order discretization. In such situations, there are a couple of recommendations:

For cases using Moving Mesh/Dynamic Mesh/Multiple Reference Frame models, Ansys Fluent does not consider the unsteady terms for Rhie-Chow face flux interpolation by default. Accounting for the unsteady terms helps to achieve better solution stability, especially when using a lower time step size with the PRESTO scheme.

To enable forced treatment of unsteady terms in Rhie-Chow face flux interpolation, use the following text command:

solve → set → vof-numerics

You will be asked

 Use forced treatment of unsteady terms in Rhie-Chow flux? [no]

to which you will respond yes.

Another change that you should make to the solver settings is in the pressure-velocity coupling scheme and under-relaxation factors that you use. The PISO scheme is recommended for transient calculations in general. Using PISO allows for increased values on all under-relaxation factors, without a loss of solution stability. You can generally increase the under-relaxation factors for all variables to 1 and expect stability and a rapid rate of convergence (in the form of few iterations required per time step). For calculations on tetrahedral or triangular meshes, an under-relaxation factor of 0.7–0.8 for pressure is recommended for improved stability with the PISO scheme.

 Solution →   Controls

As with any Ansys Fluent simulation, the under-relaxation factors will need to be decreased if the solution exhibits unstable, divergent behavior with the under-relaxation factors set to 1. Reducing the time step size is another way to improve the stability.

If you are using the steady-state implicit VOF scheme, the under-relaxation factors for all variables should be set to values between 0.2 and 0.5 for improved stability.

You should begin the mixture calculation with a low under-relaxation factor for the slip velocity. A value of 0.2 or less is recommended. If the solution shows good convergence behavior, you can increase this value gradually.

For some cases (for example, cyclone separation), you may be able to obtain a solution more quickly if you compute an initial solution without solving the volume fraction and slip velocity equations. Once you have set up the mixture model, you can temporarily disable these equations and compute an initial solution.

 Solution →   Controls

In the Equations Dialog Box, deselect Volume Fraction and Slip Velocity in the Equations list. You can then compute the initial flow field. Once a converged flow field is obtained, turn the Volume Fraction and Slip Velocity equations back on again, and compute the mixture solution.

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:

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.

In the Eulerian multiphase model, the volume fraction and continuity equations (see Equation 14–203 in the Fluent Theory Guide) can be represented either in the mass or volumetric form by choosing a reference density method using the following text command:

solve/set/mp-reference-density

The available reference methods are listed in the below table.

There is not much difference between Methods 0 and 1 for incompressible flows. Method 2, in general, may not be very stable at larger time steps and, therefore, is not recommended. Method 3 is similar to the Mixture multiphase model and may provide better stability in certain cases.

Note that both the volume fraction and continuity equations remain mass conservative regardless of their representation. Different representations affect only the solution stability and convergence behavior.

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 the face pressure interpolation method using the following text command:

solve/set/multiphase-numerics/nita-controls/face-pressure-options

To select Body Force Weighted as a face pressure interpolation method for both predictor and corrector steps, enter yes at the enable body-force-weighted for face pressure calculation? prompt.

To select the Second Order method as a face pressure interpolation method for both predictor and corrector steps:

To select the Second Order method as a face pressure interpolation method for the corrector step only:

When PRESTO is used for the face pressure calculation, you will be asked whether you want to exclude transient terms. Because 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, the exclusion of transient terms is recommended for very small time steps when using PRESTO:

exclude transient terms in face pressure calculation? [no] yes

When you use the wet steam model (described in Wet Steam Model Theory in the Theory Guide, and Setting Up the Wet Steam Model), the following two field variables will show up in the inflow, outflow boundary dialog boxes, and in the Solution Initialization task page and Patch dialog boxes.

When you select the wet steam model for the first time, a message is displayed indicating that the Minimum Static Temperature should be adjusted to 273 K since the accuracy of the built-in steam data is not guaranteed below a value of 273 K. If you use your own steam property functions, you can adjust this limit to whatever is permissible for your data.

To adjust the temperature limits, go to the Solution Limits dialog box.

 Solution → Controls Limits...

The default maximum wetness factor or liquid mass fraction () is set to 0.1. In general, during the convergence process, it is common that this limit will be reached, but eventually the wetness factor will drop below the value of 0.1. However, in cases where the limit must be adjusted, you can do so using the text user interface.

define → models → multiphase → wet-steam → set → max-liquid-mass-fraction

If you face convergence difficulties while solving wet steam flow, try the following solver settings:

If you are still unable to obtain a converged solution, try lowering the flow Courant number when using the density-based solver or the coupled pressure-based solver with the pseudo time method turned off. For the segregated pressure-based solver, try lowering the under-relaxation factor for the momentum equations. These parameters also can be found in the Solution Controls task page. For the coupled pressure-based solver with the pseudo time method turned off, try lowering the value for the Time Scale Factor available in the Run Calculation task page:

 Solution → Run Calculation

Lastly, you can try to use the first-order discretization schemes for the solution, available on the Solution Methods task page.

 Solution → Solution → Methods

If you have convergence difficulties for a turbomachinery case using a Mixing Plane (MP) interface, it is recommend that you first obtain a solution using the No Pitch-Scale (NPS) interface type. Once you have a converged flow field, switch the MP interface back on again and then attempt to compute the solution. Details of different GTI types are described in Blade Row Interaction Modeling.