ANSYS Fluent supports the following options for volume fraction formulation:
The explicit formulation is non-iterative and is time-dependent. Thus it can only be used with the Transient solver. It exhibits better numerical accuracy compared to the implicit formulation. However the time step size is limited by a Courant-based stability criterion.
The implicit formulation is iterative and can be used with either the Steady or Transient solver. It is well-suited to steady-state applications as the solution information propagates much faster compared to the explicit formulation.
For steady-state flow applications, either a steady-state or a transient simulation may be required, depending on the characteristics of the flow:
Steady-state simulation: If the final steady-state solution is not affected by the initial flow conditions and there is a distinct inflow boundary for each phase.
Transient simulation: If the final steady-state solution is dependant on the initial flow conditions and/or you do not have a distinct inflow boundary for each phase.
For transient flow applications, the implicit formulation may allow you to use a much larger time step than the explicit formulation due to the implicit formulation’s unconditional stability. However, the implicit time-step size may be limited by truncation errors. The implicit formulation produces more numerical diffusion than the explicit formulation when using the First Order transient formulation. Therefore, the implicit formulation should be used along with higher-order transient formulations to achieve better numerical accuracy.
Both implicit and explicit volume fraction formulations are available for the VOF and Eulerian multiphase models. The mixture multiphase model supports only the implicit formulation.
To specify the volume fraction formulation to be used for the VOF and Eulerian multiphase models, select the appropriate Formulation under Volume Fraction Parameters in the Multiphase Model dialog box.
For the VOF model and for the Eulerian Multiphase model with Multi-Fluid VOF enabled, you must specify the interface regime that you will be modeling. This will determine the availability of the various volume fraction discretization schemes (Spatial Discretization Schemes for Volume Fraction). The following options are available for Interface Modeling Type:
for when a distinct interface is present between the phases
for when the phases are interpenetrating
a hybrid approach for flows consisting of both sharp and dispersed interfaces. This option can also be used to capture mildly sharp interfaces. Mildly sharp interfaces are those that are neither as sharp as would be captured by the schemes available with the Sharp option, nor as diffused as would be captured by the schemes available with the Dispersed option.
If you are using the Sharp interface modeling type, you can optionally enable the Interfacial Anti-Diffusion treatment. This treatment is applied only in interfacial cells and attempts to suppress the numerical diffusion that can arise from the volume fraction advection schemes.
The use of this treatment can have adverse effects on convergence, especially with aggressive settings and large time step size. Therefore, it should be used in cases that use a coarse mesh, that have high aspect-ratio cells, that have large cell-volume jumps in the vicinity of the fluid-fluid interface, or that suffer from excess numerical diffusion.
The strength of the anti-diffusion treatment can be specified
using the define/models/multiphase/interface-modeling-options text command. The strength can range between 0 (none) and 1 (maximum).
Selecting will make available some additional discretization options. To access these, click Interface Modeling Options... in the Multiphase Model dialog box.

These options allow you to adjust the discretization behavior on a per-zone and/or per-phase-pair basis for cases in which it is important to simultaneously model dispersed and sharp interfaces.
This option is appropriate for applications that require either sharp or dispersed interface modeling depending on the cell zone. After enabling Zonal Discretization you will need to specify the slope limiter value on the Multiphase tab of the Fluid dialog box for each cell zone. (See Defining Multiphase Cell Zone and Boundary Conditions)
This option is appropriate for applications that require either sharp or dispersed interface modeling depending on the phase-pair comprising the interface. After enabling Phase Localized Discretization you will need to specify the slope limiter values for each phase pair on the Discretization tab of the Phase Interaction dialog box.
You can choose from various spatial discretization schemes for volume fraction depending on the multiphase model in use, the interface regime type, and the volume fraction formulation chosen. The available discretization schemes for each combination off model, formulation, and interface regime are summarized in the following tables:
Table 24.1: Spatial Discretization Schemes for the VOF and Eulerian with Multi-Fluid VOF Models
| Interface Modeling Type | Implicit Formulation | Explicit Formulation |
|---|---|---|
| Sharp |
Compressive |
Geo-Reconstruct |
| Sharp/Dispersed |
Compressive | |
| Dispersed |
First Order Upwind |
First Order Upwind |
Table 24.2: Spatial Discretization Schemes for the Eulerian Model without Multi-Fluid VOF
| Implicit Formulation | Explicit Formulation |
|---|---|
|
First Order Upwind |
First Order Upwind |
Table 24.3: Spatial Discretization Schemes for the Mixture Model
| Implicit Formulation | Explicit Formulation |
|---|---|
|
First Order Upwind | Not Applicable |
The Geo-Reconstruct scheme is an interface tracking scheme based on geometrical information. It is the most accurate scheme, but is more computationally expensive than the other schemes. Geo-Reconstruct is the preferred scheme when solving on meshes of poor quality.
The CICSAM, Modified HRIC, and Compressive schemes are interface capturing schemes based on algebraic information.
The Donor-Acceptor discretization is a scheme applicable only to quad- and hex-meshes. As it is considered obsolete, it does not appear by default in the graphical user interface. However, it can be made available if required using the following text command:
/solve/set/expert<...>Allow selection of all applicable discretization schemes? [no]yes
This command can also be used to expose discretization schemes that may be applicable, but are hidden by default according to the tables above.
Important: For the geometric reconstruction and donor-acceptor schemes, if you are using a conformal mesh (that is, if the mesh node locations are identical at the boundaries where two subdomains meet), you must ensure that there are no two-sided (zero-thickness) walls within the domain. If there are, you will need to slit them, as described in Slitting Face Zones.
For more details about the implementations of the volume fraction discretization schemes, refer to Interpolation Near the Interface in the Fluent Theory Guide.
The Volume Fraction Cutoff allows you to specify a cutoff limit for the volume fraction values. The value that you provide is used as the lower cutoff for the volume fraction. All volume fraction values in the domain below this cutoff value are set to zero. The upper cutoff is calculated as (1.0 - lower cutoff). All volume fraction values above the upper cutoff value are set to 1.0. The default value is 1e-6, which is the recommended value. Using a higher value may lead to a higher volume imbalance.
Important: The Volume Fraction Cutoff value can be specified when using the VOF model, or when using the Eulerian Multiphase model with the Explicit formulation.
Note: For the Implicit formulation, the minimum value allowed is 0 and the maximum allowable value is 1e-6. For the Explicit formulation, the minimum value allowed is 0 and the maximum allowable value is 1e-4. A higher cutoff value is available with the Explicit formulation because it allows for the local redistribution procedure of partially filled cells, which accounts for volume loss. This treatment is not available with the Implicit formulation.
When using the Explicit formulation, there are several additional options that you can access by clicking Expert Options... in the Multiphase Model dialog box.

This setting controls how the time-scale is computed when determining the time step used for volume fraction.
This setting controls whether to solve the volume fraction equations once per iteration, or only once per time step.
For a more detailed discussion of how to use these options, refer to Setting Time-Dependent Parameters for the Explicit Volume Fraction Formulation.