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.

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

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:

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:

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 14–42 in the Theory Guide.

(26–10)

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:

If the liquid’s free surface level lies above the origin, then the Free Surface Level is positive (see Figure 26.27: 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;
}

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 14–42 in the Theory Guide.

(26–11)

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:

If the channel’s bottom lies above the origin, then the Bottom Level is positive (see Figure 26.27: 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 26.27: 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.

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

(26–12)

where is the velocity magnitude and is the gravity magnitude.

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

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.

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:

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 26.28: Pressure Inlet for Open Channel Flow).

Figure 26.28: Pressure Inlet for Open Channel Flow

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.

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

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

Figure 26.29: Density Interpolation Method for Open Channel Flow

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 26.1: 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.

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

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

Open Channel + Translational Moving Reference Frame (MRF)

For high-speed moving hulls, it is generally recommended to ramp up the hull speed from zero to its actual speed for better stability. However, it has been observed that using pressure inlet or velocity inlet boundary conditions to mimic the hull speed causes many convergence issues. The alternative approach is to use a translational MRF with the following solution methodology:

A useful text command used to print out a summary of the open channel wave boundary condition settings is define/boundary-conditions/open-channel-wave-settings. The output will depend on whether you have chosen Wave Theories or Wave Spectrum.

Sample Output for Wave Theories

/define/boundary-conditions> open-channel-wave-settings

Wave Input Analysis for Velocity Inlet : Thread ID = 5
************************************************************

Wave-1 Analysis 
*****************************************

Current Settings :
------------------
Wave theory : 5th-order-Stokes , Wave regime = Shallow/Intermediate 
Wave Height (H) = 0.2160, Wave Length (L) = 1.9400
Liquid Depth (h) = 0.6000, Ursell Number (H*L*L/(h*h*h)) = 3.7636

Mandatory checks for full wave regime within wave breaking limit
-----------------------------------------------------------------
Relative Height: H/h = 0.3600 , Maximum theoretical limit = 0.7800 
Maximum numerical limit = 0.5500 
Relative height within wave breaking limit

Wave Steepness: H/L = 0.1113 , Maximum theoretical limit = 0.1420 
Stable numerical limit = 0.1000 , Maximum numerical limit = 0.1200 
Warning: Wave steepness exceeding the stable numerical limit.
Waves could be stable or unstable in this regime.

Checks for selected wave theory within wave breaking and stability limit
----------------------------------------------------------------------------
Relative height check
H/h = 0.3600 , Min : 0.0000 , Max : 0.5000
Relative height check : successful

Wave Steepness check
H/L = 0.1113 , Min : 0.0000 , Max : 0.1363
Wave steepness check : successful

Ursell Number check
Ur = 3.7636 , Min : 0.0000 , Max : 25.0000
Ursell number check : successful

Wave regime check
h/L = 0.3093 , Min : 0.0600 , Max : 10000.0000
Wave regime check : successful

Summary
----------------------
Checks : passed
Selected wave theory is appropriate for application.

Sample Output for Wave Spectrum

Wave Input Analysis for Velocity Inlet : Thread ID = 6
************************************************************

Wave Spectrum Analysis 
*****************************************

Current Settings :
------------------
Frequency Spectrum : Jonswap 
Direction Spreading Method : Unidirectional 

Significant Wave Height (Hs) = 5.0000
Peak Wave Frequency (wp) = 1.0000, Peak Time Period (Tp) = 6.2832
Minimum Frequency (wi) = 0.6600, Maximum Frequency (we) = 1.6600

Wave Lengths at Min/Peak/Max frequencies (Li, Lp, Le) = (141.5015, 61.6380, 22.3683)

Recommendation: Set the min and max wave frequencies so that most of the wave energy
  is concentrated in the selected regime of spectrum.
  - Min frequency = 0.5*Peak frequency
  - Max frequency = 2.5*Peak frequency


Wave Regime Check 
----------------------
Wave regime type = Short Gravity (Deep) 
Information: Validity of short gravity assumption : Liquid Depth > 0.5*Max Wave Length

Sea Steepness Check 
-----------------------
Peak Time Period (Tp) = 6.2832
Zero Upcrossing Time Period (Tz) = 4.7869

Sea Steepness based on Tp (Sp) = 0.0811, Steepness Limit = 0.0667
Sea Steepness based on Tz (Sz) = 0.1398, Steepness Limit = 0.1000

Warning: Sea Steepness based on peak time period exceeding limit.
Warning: Sea Steepness based on zero upcrossing time period exceeding limit.

Information: High wave steepness of any individual component too could affect the wave pattern,
  as superposition of wave components is based upon lienar wave theory.

Frequency Spectrum Check 
---------------------------
Peak Time Period to Wave Ht Sqrt Ratio (r = Tp/sqrt(Hs)) = 2.8099

Message: Selection of Jonswap spectrum is appropriate.

Recommended value of Peak Shape Parameter for r <= 3.6 :  5.0000 

Spectrum Resolution check
----------------------------
Number of frequency components = 50 
Number of angular components = 1 
Total number of wave components = 50 

Information: Higher number of wave components would have adverse effect on speed-up
  whereas smaller could affect the accuracy by not resolving the spectrum well.
  Following steps could assist to optimize the number of components
  1. Set number of frequency/angular components in boundary condition panel,
  2. Set TUI command solve> set> open-channel-wave-verbosity to 2 before initialization,
  3. Initialize (It would print Spectrum Energy for each frequency/angle.)
  4. Copy the information to plot Sw vs Omega and S_theta vs theta
  5. Optimize the number of components after repeating steps 1-4

Ansys Fluent supports transient profiles for all wave inputs using user-defined functions as seen by the example below:

/***********************************************************************
  UDF for defining transient profile wave inputs
 ************************************************************************/

#include "udf..h"

#define H 0.02 /* wave height for both waves : same */
#define LEN1 3. /* wave length for first wave */
#define LEN2 6. /* wave length for second wave*/
#define G 9.81
#define D 10. /* liquid depth */
#define U 1. /* wave current */
#define X 0. /* inlet point */

DEFINE_TRANSIENT_PROFILE(wave_ht, current_time)
{
	real k1 = 2.*M_PI/LEN1;
	real k2 = 2.*M_PI/LEN2;
	real w1 = sqrt(G*k1*tanh(k1*D)) + k1*U;
	real w2 = sqrt(G*k2*tanh(k2*D)) + k2*U;
	real dk = 0.5*(k1 - k2);
	real dw = 0.5*(w1 - w2);
	return (2.*H*cos(dk*X - dw*current_time));
}

Fluent uses Fenton’s formulation for Stokes theories by default. For additional information about the current Stokes theories formulation, see Stokes Wave Theories in the Fluent Theory Guide. To revert to the old formulation, provided by Skjebreia and Hendrickson, use the following text command:

/solve/set/open-channel-wave-options> 
set-buffer-layer-ht     set-verbosity           stokes-wave-variants

/solve/set/open-channel-wave-options> stokes-wave-variants
Use Fenton's formulation for Stokes wave theories [yes] no
Activating old formulation (Skjelbreia and Hendrickson) for Stokes wave theories.

For additional information on the old formulation, refer to Lin’s book [89].

To report values as wave speed, wave frequency, and time period for individual waves during initialization, you can set the following text command:

solve → set → open-channel-wave-options → set-verbosity

When prompted to set Verbosity for reporting of derived wave inputs during initialization, enter 1 as shown below:

/solve/set/open-channel-wave-options> set-verbosity

Verbosity for reporting of derived wave inputs during initialization
 [0] 1

A sample of the resulting output for wave groups after initializing is shown below:

Wave-1 : Wave Height = 0.0200, Wave Length = 3.0000
Wave Number = 2.0944, Wave Speed = 2.1642, Wave Frequency = 4.5328
Effective parameters: Wave Speed = 3.1642, Wave Frequency = 6.6272, Time Period = 0.9481

Wave-2 : Wave Height = 0.0200, Wave Length = 6.0000
Wave Number = 1.0472, Wave Speed = 3.0607, Wave Frequency = 3.2052
Effective parameters: Wave Speed = 4.0607, Wave Frequency = 4.2524, Time Period = 1.4776

Time Period based on average effective frequency: 1.1550

The resultant output for Shallow Waves option is shown below:

Wave-1 : Wave Height = 0.2400, Specified Wave Length = 16.0000
Wave Number = 0.5051, Estimated Wave Length = 12.4398
Elliptic Function Parameter (m) : Calculated = 0.9976, Used = 1.0000
Liquid Height = 0.8000, Trough Height = 0.800000
Wave Speed = 3.1868, Wave Frequency = 1.6096
Effective parameters: Wave Speed = 4.1868, Wave Frequency = 2.1147
Time Period based on effective frequency: 2.9712

Below are some helpful key points when using the Numerical Beach option:

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

The procedure for defining a secondary phase in a VOF calculation is similar to that for the primary phase:

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 14–32 in the Theory Guide), or the Weber number, We (defined by Equation 14–33 in the Theory Guide). Surface tension effects can be neglected if Ca  or We  .

You can 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, in the Phase Interaction > Forces tab of the Multiphase Model dialog box (Figure 26.38: The Multiphase Model Dialog Box (Forces Tab)).

 Setup → Models → Multiphase  Edit...

Figure 26.38: The Multiphase Model Dialog Box (Forces 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:

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:

When Surface Tension Force Modeling is enabled, the following additional variables become available for postprocessing under the Phases... category:

See Field Function Definitions for their definitions.

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:

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 26.39: The Multiphase Model Dialog Box for the VOF Model (Discretization Tab)

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

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

To use the VOF-to-DPM Model Transition capability, follow the steps below:

The Consider Diffuse Lumps option (see Setting up the VOF-to-DPM Model Transition) can be useful in the following scenario.

In industrial VOF-to-DPM calculations, some diffused VOF liquid structures may not be converted to Lagrangian parcels although they have obviously detached from the main liquid jet. If the automatic solution-adaptive mesh refinement has been set up such that it keeps every cell that contains any liquid (or is in close vicinity to such a cell) refined, then these liquid lumps can greatly increase computational time.

The following strategy helps to minimize the occurrence of such diffused liquid lumps.

In the Phase Interaction dialog box, under the Model Transition tab, define the following three vof-to-dpm mechanisms. The mechanisms will always be processed in the order in which they appear in the user interface.

If you use a different injection in each of these mechanisms, then in the future, you will be able to easily determine which particles were generated by which model transition mechanism.

Note that structures of cells with non-zero liquid volume fraction that do not detach completely from the initial jet (that is, they remain connected to the initial jet by a bridge of non-zero liquid volume fraction) will be regarded as part of the jet and will not receive any special treatment. Should such structures form and have an impact on the fidelity of the simulation, then that is an indication that either the VOF interface tracking algorithm or the discretization scheme cannot keep the gas-liquid interface sufficiently sharp. In such situations, you should double-check your case setup and make sure that the VOF Courant number remains around or below unity. If you really need to change the volume fraction cut-off for lump detection, you can use the define/phases/set-domain-properties/interaction-domain/model-transition/model-transition text command to modify the value for Lump Periphery Lower Liquid Volume Fraction Limit.

The following additional postprocessing variables will become available for postprocessing under the Lump Detection... category:

When the energy equation is enabled, the following additional variables are available for postprocessing under the Lump Detection... category:

The tracking of a DPM particle is stopped as soon as the transition criteria are met, and the particle is scheduled for the model transition. All such particles are then transitioned into equivalent amounts of the selected VOF phase before the transport equation solver for the continuous phase is started for the current timestep.

The DPM-to-VOF model transition mechanism conserves mass and momentum of the transitioning phase regardless of the sizes of the particles and the cells. Particles that are much smaller than the cell are usually transitioned into the same cell, while particles that are larger than the cell are transitioned by introducing VOF liquid and removing equal amounts of VOF gas in multiple cells that form a hemispherically-shaped phase boundary around the location of the particle at the time when the model transition mechanism is triggered.

The figures below show changes in the gas-liquid interface and in the mesh in the process of the DPM-to-VOF model transition and automatic mesh adaption.

Figure 26.42: DPM Particles at the Gas-Liquid Interface displays a planar gas-liquid surface and three large Lagrangian DPM particles. The center points of the particles have just reached the phase boundary and the particles are about to be converted.

Figure 26.42: DPM Particles at the Gas-Liquid Interface

Figure 26.43: Surface Mesh Before the Model Transition is Triggered shows the surface mesh of the surrounding box. The phase boundary has been resolved by the solution-adaptive mesh refinement using appropriate criteria.

Figure 26.43: Surface Mesh Before the Model Transition is Triggered

Figure 26.44: Gas-Liquid Interface after the Model Transition is Triggered shows the VOF phase interface right after the model transition has been triggered.

Figure 26.44: Gas-Liquid Interface after the Model Transition is Triggered

For the smallest particle, a hemisphere has been formed. Its volume is equal to that of the Lagrangian DPM particle. This includes the part of the particle that has already penetrated the VOF liquid.

The other two particles overlapped, which was neglected in the calculation of the particle trajectories. This has been taken into account by the DPM-to-VOF model transition mechanism to ensure total conservation of mass.

Figure 26.45: Surface Mesh After the Mesh Adaption and Phase Transition demonstrates the surface mesh of the same surrounding box as in Figure 26.43: Surface Mesh Before the Model Transition is Triggered after the DPM particles have been transitioned to VOF liquid. During the model transition, automatic adaption has been triggered as many times as necessary, so that the maximum mesh refinement has been reached, and the new gas-liquid boundary has been formed as a result. At the same time, the mesh coarsening has removed the mesh refinement in the location inside the large particle where an interface no longer exists after the model transition.

Figure 26.45: Surface Mesh After the Mesh Adaption and Phase Transition

In the current implementation of the DPM-to-VOF model transition, no splashing or any other kind of interaction between a droplet and a film or pool of liquid is considered. Whenever the center of a Lagrangian DPM particle reaches a cell that fulfills the applicable criteria, the amount of liquid represented by the particle is assumed to stick to the existing VOF liquid.

In addition to momentum and mass of the transitioning phase, heat and composition are also conserved. However, as explained above, in the Volume-Balancing Eulerian Phase, conservation of mass (or volume) and other quantities associated with the mass is not fulfilled.

The DPM-to-VOF model transition is not compatible with: