24.3.4. Modeling Open Channel Flows

Using the VOF formulation, open channel flows can be modeled in ANSYS Fluent. To start using the open channel flow boundary condition, perform the following:

  1. Enable Gravity and set the gravitational acceleration fields.

     Setup → General Gravity → On

  2. Enable the volume of fluid model.

    1. Open the Multiphase Model dialog box.

       Setup →   Models →   Multiphase → Edit...

    2. Under Model, enable Volume of Fluid.

    3. Under Formulation, select either Implicit or Explicit.

  3. Under VOF Sub-Models, select Open Channel Flow.


    Note:  The default VOF formulation is set to Implicit after enabling the Open Channel Flow option. This is done to allow the use of larger time step sizes for such applications.


In order to set specific parameters for a particular boundary for open channel flows, enable the Open Channel option in the Multiphase tab of the corresponding boundary condition dialog box. Table 24.10: Open Channel Boundary Parameters for the VOF Model summarizes the types of boundaries available to the open channel flow boundary condition, and the additional parameters needed to model open channel flow. For more information on setting boundary condition parameters, see Cell Zone and Boundary Conditions.

Table 24.10:  Open Channel Boundary Parameters for the VOF Model

Boundary TypeParameter
pressure inletInlet Group ID; Secondary Phase for Inlet; Flow Specification Method; Free Surface Level, Bottom Level; Velocity Magnitude
pressure outletOutlet Group ID; Pressure Specification Method; Free Surface Level; Bottom Level
mass-flow inletInlet Group ID; Secondary Phase for Inlet; Free Surface Level; Bottom Level; Mass Flow Rates for the Phases
velocity inletSecondary Phase for Inlet; Free Surface Level, Averaged Velocity Inputs/Segregated Velocity Inputs (Available with Open Channel Wave Boundary Condition)
outflowFlow Rate Weighting

Further details are provided in the following sections:

24.3.4.1. Defining Inlet Groups

Open channel systems involve the flowing fluid (the secondary phase) and the fluid above it (the primary phase).

If both phases enter through the separate inlets (for example, inlet-phase2 and inlet-phase1), these two inlets form an inlet group. This inlet group is recognized by the parameter Inlet Group ID, which will be same for both the inlets that make up the inlet group. On the other hand, if both the phases enter through the same inlet (for example, inlet-combined), then the inlet itself represents the inlet group.


Important:  In three-phase flows, only one secondary phase is allowed to pass through one inlet group.


24.3.4.2. Defining Outlet Groups

Outlet-groups can be defined in the same manner as the inlet groups.


Important:  In three-phase flows, the outlet should represent the outlet group, that is, separate outlets for each phase are not recommended in three-phase flows.


24.3.4.3. Setting the Inlet Group

For pressure inlets and mass-flow inlets, the Inlet Group ID is used to identify the different inlets that are part of the same inlet group. For instance, when both phases enter through the same inlet (single face zone), then those phases are part of one inlet group and you would set the Inlet Group ID to 1 for that inlet (or inlet group).

In the case where the same inlet group has separate inlets (different face zones) for each phase, then the Inlet Group ID will be the same for each inlet of that group.

When specifying the inlet group, use the following guidelines:

  • Since the Inlet Group ID is used to identify the inlets of the same inlet group, general information such as Free Surface Level, Bottom Level, or the mass flow rate for each phase should be the same for each inlet of the same inlet group.

  • You should specify a different Inlet Group ID for each distinct inlet group.

    For example, consider the case of two inlet groups for a particular problem. The first inlet group consists of water and air entering through the same inlet (a single face zone). In this case, you would specify an inlet group ID of 1 for that inlet (or inlet group). The second inlet group consists of oil and air entering through the same inlet group, but each uses a different inlet (oil-inlet and air-inlet) for each phase. In this case, you would specify the same Inlet Group ID of 2 for both of the inlets that belong to the inlet group.

24.3.4.4. Setting the Outlet Group

For pressure outlet boundaries, the Outlet Group ID is used to identify the different outlets that are part of the same outlet group. For instance, when both phases enter through the same outlet (single face zone), then those phases are part of one outlet group and you would set the Outlet Group ID to 1 for that outlet (or outlet group).

In the case where the same outlet group has separate outlets (different face zones) for each phase, then the Outlet Group ID will be the same for each outlet of that group.

When specifying the outlet group, use the following guidelines:

  • Since the Outlet Group ID is used to identify the outlets of the same outlet group, general information such as Free Surface Level or Bottom Level should be the same for each outlet of the same outlet group.

  • You should specify a different Outlet Group ID for each distinct outlet group.

    For example, consider the case of two outlet groups for a particular problem. The first outlet group consists of water and air exiting from the same outlet (a single face zone). In this case, you would specify an outlet number of 1 for that outlet (or outlet group). The second outlet group consists of oil and air exiting through the same outlet group, but each uses a different outlet (oil-outlet and air-outlet) for each phase. In this case, you would specify the same Outlet Group ID of 2 for both of the outlets that belong to the outlet group.


Important:  For three-phase flows, when all the phases are leaving through the same outlet, the outlet should consist only of a single face zone.


24.3.4.5. Determining the Free Surface Level

For the appropriate boundary, you need to specify the Free Surface Level value. This parameter is available for all relevant boundaries, including pressure outlet, mass-flow inlet, and pressure inlet. The Free Surface Level, is represented by in Equation 17–41 in the Theory Guide.

(24–2)

where is the position vector of any point on the free surface, and is the unit vector in the direction of the force of gravity. Here a horizontal free surface that is normal to the direction of gravity is assumed.

We can simply calculate the free surface level in two steps:

  1. Determine the absolute value of height from the free surface to the origin in the direction of gravity.

  2. Apply the correct sign based on whether the free surface level is above or below the origin.

If the liquid’s free surface level lies above the origin, then the Free Surface Level is positive (see Figure 24.18: Determining the Free Surface Level and the Bottom Level). Likewise, if the liquid’s free surface level lies below the origin, then the Free Surface Level is negative.

You can also specify a transient profiles for a Free Surface Level for the relevant open channel boundaries as shown in the example below:

/*********************************************************************
Example UDF that demonstrates transient profile for free surface level
**********************************************************************/

#include "udf.h"

#define H 1.5   /* Original Free surface level */ 
#define T0 0.2  /* Time */

DEFINE_TRANSIENT_PROFILE(fs_level, current_time)
{
    real level;
    if (current_time <= T0)
      level = H - current_time;
    else
      level = H - T0; 

    return level;
}

24.3.4.6. Determining the Bottom Level

For the appropriate boundary, you need to specify the Bottom Level value. This parameter is available for all relevant boundaries, including pressure outlet, mass-flow inlet, and pressure inlet. The Bottom Level, is represented by a relation similar to Equation 17–41 in the Theory Guide.

(24–3)

where is the position vector of any point on the bottom of the channel, and is the unit vector of gravity. Here we assume a horizontal free surface that is normal to the direction of gravity.

We can simply calculate the bottom level in two steps:

  1. Determine the absolute value of depth from the bottom level to the origin in the direction of gravity.

  2. Apply the correct sign based on whether the bottom level is above or below the origin.

If the channel’s bottom lies above the origin, then the Bottom Level is positive (see Figure 24.18: Determining the Free Surface Level and the Bottom Level). Likewise, if the channel’s bottom lies below the origin, then the Bottom Level is negative.

Figure 24.18:  Determining the Free Surface Level and the Bottom Level

Determining the Free Surface Level and the Bottom Level

You can also specify a transient profiles for a Bottom Level for the relevant open channel boundaries.

24.3.4.7. Specifying the Total Height

The total height, along with the velocity, is used as an option for describing the flow. The total height is given as

(24–4)

where is the velocity magnitude and is the gravity magnitude.

24.3.4.8. Determining the Velocity Magnitude

For pressure inlet boundaries, input for Velocity Magnitude is required to calculate the dynamic pressure being used in the total pressure calculation.


Note:  The provided Velocity Magnitude is not applied to the boundary.


24.3.4.9. Determining the Secondary Phase for the Inlet

In the case of a flow with more than two phases, for pressure inlets and mass-flow inlets, you can select the desired secondary phase from the Secondary Phase for Inlet drop-down box.


Important:  Note that only one secondary phase is allowed to pass through one inlet group.


Consider a problem involving a three-phase flow consisting of air as the primary phase, and oil and water as the secondary phases. Consider also that there are two inlet groups:

  • water and air

  • oil and air

For the former inlet group, you would choose water as the secondary phase. For the latter inlet group, you would choose oil as the secondary phase (as shown in Figure 24.19: Pressure Inlet for Open Channel Flow).

Figure 24.19:  Pressure Inlet for Open Channel Flow

Pressure Inlet for Open Channel Flow


24.3.4.10. Determining the Secondary Phase for the Outlet

For a flow application with more than two phases, if you select Free Surface Level for the Pressure Specification Method (in the Pressure Outlet dialog box, Multiphase tab), you must also select the appropriate Secondary Phase for Level Specification and specify the Free Surface Level and Bottom Level. See Determining the Free Surface Level and Determining the Bottom Level for details about these parameters. For more information about the available pressure specification methods, refer to Pressure Outlet in the Fluent Theory Guide.

The hydrostatic pressure profile is imposed in the selected secondary phase that shares the interface with the primary phase. It is assumed that other secondary phases will not disturb the imposed pressure distribution.

For example, in a three-phase cavitating flow consisting of air, water, and vapor, the vapor is generated in the localized region adjacent to moving bodies. If the pressure outlet boundary is sufficiently far away from the cavitating region, then the hydrostatic assumption in the water phase that shares the interface with air can be safely imposed.

24.3.4.11. Choosing the Pressure Specification Method

For a pressure outlet boundary, the outlet pressure can be specified in one of three ways:

  • by prescribing the free surface level, such as a hydrostatic pressure profile (available for two-phase flow only)

  • by specifying the constant pressure

  • by specifying the neighboring cell pressure


Note:  You can also specify a hydrostatic pressure profile at the pressure outlet for axisymmetric open channel flow. However, there are certain limitations as noted in Limitations.



Important:  This option is not available in the case of three-phase flows since the pressure on the boundary is taken from the neighboring cell.


24.3.4.12. Choosing the Density Interpolation Method

For problems involving sub-critical flow, the following options exist for the Density Interpolation Method:

  • From Neighboring Cell is the default option, where the mixture density used in the hydrostatic profile is interpolated using the volume fraction calculated from the neighboring cell.


    Note:  In some cases, this method may cause free surface oscillation near the upstream boundaries. These oscillations are particularly visible in cases where boundaries are close to the object; or if the boundary has unstructured mesh near the free surface level. For such cases, it is recommended that you use the From Free Surface Level option under Density Interpolation Method.


  • From Free Surface Level where the mixture density used in the hydrostatic profile is interpolated from the volume fraction calculated from the free surface level.

  • Hybrid where the mixture density used in the hydrostatic profile is calculated either from the From Neighboring Cell or From Free Surface Level options, depending on the direction of flux. This method is only available at a pressure outlet.

Figure 24.20:  Density Interpolation Method for Open Channel Flow

Density Interpolation Method for Open Channel Flow

24.3.4.13. Open Channel Flow Compatibility with Velocity Inlet

Open channel flow compatibility with velocity inlet is provided in the framework of the open channel wave boundary condition, therefore, the Open Channel Wave BC option in the Figure 24.1: Multiphase Model Dialog Box for the VOF Model must be enabled first.

Velocity inlet compatibility allows you to use either averaged or segregated velocity inputs to moving obstacles, water and air, which is not possible using either the pressure inlet or mass-flow inlet boundary conditions.

Select the Open Channel Wave BC option in the Velocity Inlet dialog box. For detailed information about the velocity inputs, see Inputs at Velocity Inlet Boundaries.

24.3.4.13.1. Velocity Inlet, Open Channel Flow, Steady-State

you must specify (in the Multiphase tab of the Velocity Inlet dialog box):

  • Secondary phase for the inlet

  • Free surface level

24.3.4.13.2. Velocity Inlet, Open Channel Flow, Transient

You must set the Wave BC Option to None (in the Multiphase tab of the Velocity Inlet dialog box).

24.3.4.14. Limitations

The following list summarizes some issues and limitations associated with the open channel boundary condition.

  • The conservation of the Bernoulli integral does not provide the conservation of mass flow rate for the pressure boundary. In the case of a coarser mesh, there can be a significant difference in mass flow rate from the actual mass flow rate. For finer meshes, the mass flow rate comes closer to the actual value. So, for problems having constant mass flow rate, the mass flow rate boundary condition is a better option. The pressure boundary should be selected when steady and non-oscillating drag is the main objective.

  • Specifying the top boundary as the pressure outlet can sometimes lead to a divergent solution. This may be due to the corner singularity at the pressure boundary in the air region or due to the inability to specify local flow direction correctly if the air enters through the top locally.

  • Only the heavier phase should be selected as the secondary phase.

  • In the case of flows with more than two phases, only one secondary phase is allowed to enter through one inlet group (that is, the mixed inflow of different secondary phases is not allowed).

  • For axisymmetric flow, pressure and mass-flow inlets do not support open channel boundary conditions.

  • Open channel wave boundary conditions for velocity inlets do not support cases with axisymmetric flow.

  • Axisymmetric open channel flow is available for two phase flow and the pressure outlet boundary.

  • For axisymmetric open channel flow, the direction of gravity must be aligned with the direction of the axis.

24.3.4.15. Recommendations for Setting Up an Open Channel Flow Problem

The following list represents a list of recommendations for solving problems using the open channel flow boundary condition:

  • In the cases where the inlet group has a different inlet for each phase of fluid, then the parameter values (such as Free Surface Level, Bottom Level, and Mass Flow Rate) for each inlet should correspond to all other inlets that belong to the inlet group.

  • The solution begins with an estimated pressure profile at the outlet boundary.

    In general, you can start the solution by assuming that the level of liquid at the outlet corresponds to the level of liquid at the inlet. The convergence and solution time is very dependent on the initial conditions. When the flow is completely subcritical (upstream and downstream), in marine applications for instance, the above approach is recommended.

    If the final conditions of the flow can be predicted by other means, the solution time can be significantly reduced by using the proper boundary condition.

  • In the case of super-critical flow at the outlet, you can use the From Neighboring Cell option at the outlet, as it may provide better convergence.

  • The initialization procedure is very critical in the open channel analysis. Refer to Recommendations for Open Channel Initialization.

  • For the initial stability of the solution, a smaller time step is recommended. You can increase the time step once the solution becomes more stable.

  • For flows that do not make a transition from sub-critical to super-critical, or vice-versa, you can speed-up the solution calculation by specifying the frequency of Froude number updates during run time by setting the following text command: solve → set → open-channel-controls.

    When prompted, set up the following parameter for steady-state flows:

    /solve/set> open-channel-controls
    Iteration interval for Froude number update [10]

    When prompted, set up the following parameter for transient flows:

    /solve/set> open-channel-controls
    Time step interval for Froude number update [1]

  • For pure open channel flow applications, the inlet and outlet boundary conditions are controlled by the Froude number. In certain cases, it is possible to impose a hydrostatic profile at the outlet without any Froude number dependency. You can use the following text command: solve → set → open-channel-controls.

    When prompted, set up the following parameter as shown below:

    /solve/set> open-channel-controls
    Use Froude number independent boundary condition at outlet? [no] yes
  • Relevant open channel inputs, along with the Froude number, can be reported using the following text command: define → boundary-conditions → openchannel-threads.

  • In the case of reverse flow, the pressure outlet boundary behaves as a pressure inlet, and the boundary-specific static pressure is taken as the Total Pressure. In this case, the static pressure is calculated from the total pressure. You can use the following text command to fix the boundary-specified static pressure, which helps to suppress reflections from the pressure boundary for certain cases: solve → set → open-channel-controls

    When prompted, set up the following parameter as shown below:

    /solve/set> open-channel-controls
    Use boundary specified static pressure for backflow? [no] yes

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