24.3.8. Defining the Phases for the VOF Model

Instructions for specifying the necessary information for the primary and secondary phases and their interaction in a VOF calculation are provided below.


Important:  In general, you can specify the primary and secondary phases whichever way you prefer. It is a good idea, especially in more complicated problems, to consider how your choice will affect the ease of problem setup. For example, if you are planning to patch an initial volume fraction of 1 for one phase in a portion of the domain, it may be more convenient to make that phase a secondary phase. Also, if one of the phases is a compressible ideal gas, it is recommended that you specify it as the primary phase to improve solution stability.


24.3.8.1. Defining the Primary Phase

To define the primary phase in a VOF calculation, perform the following steps:

  1. Select phase-1 in the Phases list.

  2. Click Edit... to open the Primary Phase dialog box (Figure 24.27: The Primary Phase Dialog Box).

    Figure 24.27:  The Primary Phase Dialog Box

    The Primary Phase Dialog Box

  3. In the Primary Phase dialog box, enter a Name for the phase.

  4. Specify which material the phase contains by choosing the appropriate material in the Phase Material drop-down list.

  5. Define the material properties for the Phase Material.

    1. Click Edit..., and the Edit Material dialog box will open.

    2. In the Edit Material dialog box, check the properties, and modify them if necessary. (See Physical Properties for general information about setting material properties, Modeling Compressible Flows for specific information related to compressible VOF calculations, and Modeling Solidification/Melting for specific information related to melting/solidification VOF calculations.)


      Important:  If you make changes to the properties, remember to click Change before closing the Edit Material dialog box.


  6. Click OK in the Primary Phase dialog box.

24.3.8.2. Defining a Secondary Phase

To define a secondary phase in a VOF calculation, perform the following steps:

  1. Select the phase (for example, phase-2) in the Phases list.

  2. Click Edit... to open the Secondary Phase dialog box (Figure 24.28: The Secondary Phase Dialog Box for the VOF Model).

    Figure 24.28:  The Secondary Phase Dialog Box for the VOF Model

    The Secondary Phase Dialog Box for the VOF Model

  3. In the Secondary Phase dialog box, enter a Name for the phase.

  4. Specify which material the phase contains by choosing the appropriate material in the Phase Material drop-down list.

  5. Define the material properties for the Phase Material, following the procedure outlined above for setting the material properties for the primary phase.

  6. Click OK in the Secondary Phase dialog box.

24.3.8.3. Including Surface Tension and Adhesion Effects

As discussed in When Surface Tension Effects Are Important in the Theory Guide, the importance of surface tension effects depends on the value of the capillary number, Ca (defined by Equation 17–31 in the Theory Guide), or the Weber number, We (defined by Equation 17–32 in the Theory Guide). Surface tension effects can be neglected if Ca  or We  .

Several surface tension options are provided through the text user interface (TUI) using the solve/set/surface-tension command :

solve → set → surface-tension

The surface-tension command prompts you for the following information:

  • whether you require node-based smoothing

    The default value is yes, indicating that node-based smoothing will be used. Note that if you are reading in a case that was created in versions prior to ANSYS Fluent 13, then cell-based smoothing will be used by default for the VOF calculations.

  • the number of smoothings

    The default value is 1. A higher value can be used in case of tetrahedral and triangular meshes in order to reduce any spurious velocities.

  • the smoothing relaxation factor

    The default is 1. This is useful in the cases where VOF smoothing causes a problem (for example, liquid enters through the inlet with wall adhesion on).

  • whether you want to use VOF gradients at the nodes for curvature calculations

    With this option, ANSYS Fluent uses VOF gradients directly from the nodes to calculate the curvature for surface tension forces. The default is yes which produces better results with surface tension compared to gradients that are calculated at the cell centers.


Important:  Note that the calculation of surface tension effects will be more accurate if you use a quadrilateral or hexahedral mesh in the area(s) of the computational domain where surface tension is significant. If you cannot use a quadrilateral or hexahedral mesh for the entire domain, then you should use a hybrid mesh, with quadrilaterals or hexahedra in the affected areas.

ANSYS Fluent uses node based smoothing for smoothed volume fraction and node based gradients for smoothed curvature calculation to provide better accuracy and robustness.



Important:  Pressure jump caused by the surface tension is discontinuous in nature, and also it acts locally at the interface. These numerical difficulties are overcome in an approximate manner by considering the smoothed distribution of the volume fraction field within the finite interfacial width. Smoothing procedures, in general, are mesh dependent. Therefore, the amount and nature of the smoothing procedure could have a significant effect on the results for surface tension cases.


If you want to include the effects of surface tension along the interface between one or more pairs of phases, as described in Surface Tension and Adhesion in the Theory Guide, click Interaction... to open the Phase Interaction Dialog Box (Figure 24.29: The Phase Interaction Dialog Box for the VOF Model (Surface Tension Tab)).

Figure 24.29:  The Phase Interaction Dialog Box for the VOF Model (Surface Tension Tab)

The Phase Interaction Dialog Box for the VOF Model (Surface Tension Tab)

Perform the following steps to model surface tension (and, if appropriate, include adhesion) effects along the interface between one or more pairs of phases:

  1. Click the Surface Tension tab.

  2. Enable the Surface Tension Force Modeling option to include the surface tension method.


    Note:  Make sure you specify the Surface Tension Coefficients as constant or user-defined. If none is selected, then Surface Tension Force Modeling will automatically be disabled.


  3. Select the surface tension method that is most applicable to your case. You can choose between Continuum Surface Force and Continuum Surface Stress. Information about each of the methods is described in Surface Tension in the Theory Guide.

  4. For each pair of phases between which you want to include the effects of surface tension, specify an input for the surface tension coefficients using one of the following options:

    • Constant Value

    • Temperature-dependent polynomial, piecewise polynomial, or piecewise linear


      Note:  These options are available while modeling energy.


    • User-defined surface tension coefficient


      Note:  This can be defined as a function of any space variable or time.


    See Surface Tension and Adhesion in the Theory Guide for more information on surface tension, and the Fluent Customization Manual for more information on user-defined functions. All surface tension coefficients are equal to 0 by default, representing no surface tension effects along the interface between the two phases.


    Important:  For calculations involving surface tension, it is recommended that you also turn on the Implicit Body Force treatment for the Body Force Formulation in the Multiphase Model dialog box. This treatment improves solution convergence by accounting for the partial equilibrium of the pressure gradient and surface tension forces in the momentum equations. See Including Body Forces for details.


  5. If you want to include wall adhesion, enable the Wall Adhesion option. When Wall Adhesion is enabled, you will need to specify the contact angle at each wall as a boundary condition (as described in Defining Multiphase Cell Zone and Boundary Conditions).

    The contact angle is the angle between the wall and the tangent to the interface at the wall, measured inside the phase listed in the left column under Wall Adhesion in the Momentum tab of the Wall dialog box. For example, if you are setting the contact angle between the oil and air phases in the Wall dialog box shown in Figure 24.30: The Wall Dialog Box for a Mixture in a VOF Calculation with Wall Adhesion, is measured inside the oil phase, as seen in Figure 24.31: Measuring the Contact Angle. For more information, refer to Wall Adhesion in the Theory Guide.

    Figure 24.30:  The Wall Dialog Box for a Mixture in a VOF Calculation with Wall Adhesion

    The Wall Dialog Box for a Mixture in a VOF Calculation with Wall Adhesion

    Figure 24.31:  Measuring the Contact Angle

    Measuring the Contact Angle

  6. If you want to include jump adhesion, enable the Jump Adhesion option. When Jump Adhesion is enabled, you will need to specify the contact angle at the porous jump in the Porous Jump dialog box (as described in Defining Multiphase Cell Zone and Boundary Conditions). The contact angle specification and measurement for jump adhesion is similar to that of wall adhesion (as explained in step 3 above).


    Important:  Jump adhesion only supports the cell based smoothing option for surface tension. When the Jump Adhesion option is enabled in the Phase Interaction dialog box, the correct settings are automatically set for surface tension. To view the surface tension settings, use the solve/set/surface-tension text command.



Note:  The following limitations exist:

  • When the Wall Adhesion and Jump Adhesion options are enabled, you must specify a nonzero surface tension coefficient.

  • Jump Adhesion is not available with the Continuum Surface Stress model.

  • The Continuum Surface Stress model and the Jump Adhesion option are not available with the Level Set option.


24.3.8.4. Discretizing Using the Phase Localized Compressive Scheme

Most of the interface capturing or tracking schemes, which are common in literature, can simulate either diffused interface modeling or sharp interface modeling. There are a number of applications where you may be interested in modeling diffused and sharp interfaces in different regimes, which results in the need for a unique discretization procedure to handle such applications.

Below are some examples of such applications:

  • Air bubble rise in water-solid slurry: Diffused interface modeling is required for the water and solid, and sharp interface modeling for the air bubble is desirable. A sharpening scheme would cause undesirable effects for the modeling of the diffused interface between water and solids and a diffusive scheme would not be able to maintain the sharp interface for bubble rising in the slurry.

  • Evaporation/condensation in a tank partially filled with water and being heated at the bottom: Diffused interface modeling is required for the liquid-vapor and sharp interface modeling for the water-air regime is desirable. A sharpening scheme, would not be able to simulate the diffused phenomena of evaporation/condensation for the liquid- vapor phase and a diffusive scheme would not be able to maintain the sharp interface between water and air.

  • Air jet penetrating through layer of liquids: You may be interested in diffused jet modeling and sharp interface modeling between the liquid layers. A sharpening scheme would not be able to maintain the continuous air stream and a diffusive scheme would not be able to maintain the sharp interfaces between the layers of liquids.

Using the Modified HRIC and Compressive schemes for such applications would result in the HRIC scheme producing undesirable sharpening of the dispersed phases and undesirable diffusion of the continuous phases, whereas the Compressive scheme would produce undesirable sharpening of the dispersed phases.

Therefore, the phase localized compressive scheme is particularly useful in cases where the desirable behavior is such that you have diffused modeling of dispersed phases and sharp modeling of continuous phases. In ANSYS Fluent, diffusive and anti-diffusive discretization procedures can be used across the distinct interfaces, which share a pair of phases. This functionality is provided through the compressive discretization scheme, where the degree of diffusion or sharpness is controlled through the value of the slope limiters. The theory used is described in The Compressive Scheme and Interface-Model-based Variants.

Figure 24.32:  The Phase Interaction Dialog Box for the VOF Model (Discretization Tab)

The Phase Interaction Dialog Box for the VOF Model (Discretization Tab)

To use the phase localized compressive scheme, perform the following steps:

  1. Click the Discretization tab.


    Note:  The Discretization tab is available if the VOF model or the Eulerian multiphase model with Mulit-Fluid VOF is enabled, and the Phase Localized Discretization option is enabled in the Interface Modeling Options dialog box. (Interface Modeling Type).


  2. Enable Phase Localized Compressive Scheme.


    Important:  When this option is enabled, the Compressive spatial discretization scheme is automatically selected for the Volume Fraction in the Solution Methods dialog box.


  3. For each pair of phases, specify the value of the slope limiter. You can enter a value of 0, 1, or 2, or any value between 0 and 2. Refer to Table 24.11: Slope Limiter Discretization Scheme to equate each value of the slope limiter with a discretization scheme.

    Table 24.11:  Slope Limiter Discretization Scheme

    Slope Limiter Value Scheme
    0first order upwind
    1second order reconstruction bounded by the global minimum/maximum of the volume fraction
    2compressive
    and blended: where a value between 0 and 1 means blending of the first order and second order and a value between 1 and 2 means blending of the second order and compressive scheme


When using the Phase Localized Compressive Scheme, note the following:

  • The minimum limit for the slope limiter is 0, whereas the maximum is 2.

  • The slope limiter can be interpreted as the degree of compression/anti-diffusion, where 0 demonstrates the minimum compression and 2 demonstrates the maximum compression.

  • For interfaces sharing the diffused phases, a slope limiter value of 2 should not be used. A value between 0 and 1 is recommended.

  • For interfaces sharing the continuous phases, any value between 0 and 2 can be used depending on the application.

  • For interfaces sharing the continuous and diffused phases, any value between 0 and 2 can be used based on the application.

  • If you want variable discretization behavior for an interface between two phases, you can do so via the DEFINE_PROPERTY user-defined function.


    Note:
    • If the interface has a transition from sharp to diffused modeling, you should not experience any problems.

    • If the interface has a transition from diffused to sharp modeling, this transition should be smooth by gradually varying the value of the slope limiter within some transition zone.



Release 18.2 - © ANSYS, Inc. All rights reserved.