24.3.6. Recommendations for Open Channel Initialization

Once you have selected either the Open Channel Flow or the Open Channel Wave BC option in the Multiphase Model dialog box, then the Open Channel Initialization Method drop-down list appears in the Solution Initialization task page.

 Solution →   Initialization

Figure 24.24:  The Solution Initialization Task Page

The Solution Initialization Task Page

Select an inlet zone from the Compute from drop-down list. You can now make your selection from the Open Channel Initialization Method drop-down list. If only the Open Channel Flow option was enabled, then you only have a choice of None or Flat. If you enabled Open Channel Wave BC, then your choices are None, Flat, or Wavy. The default initialization method is None.

If you initialize the solution using None, it has no effect as it does not use any open channel information from the selected zone. The Open Channel Initialization Method comes into effect when you select either Flat or Wavy.


Important:  This initialization is only valid for pressure-inlets, pressure outlets, and mass-flow inlets for open channel flow and velocity inlets for open channel wave boundary conditions. If the selected inlet zone does not have either open channel flow or open channel wave boundary conditions, ANSYS Fluent will report an error message after you initialize the flow with open channel initialization method of Flat or Wavy.


For open channel initialization from the pressure outlet boundary, the hydrostatic pressure profile based on the Free Surface Level is patched in the domain. The volume fraction in the domain is patched based on Free Surface Level provided at the pressure outlet boundary. To patch velocity and other variables, the values in the Solution Initialization task page will be used.


Important:  The pressure specification methods, with the exception of Free Surface Level, are not supported for open channel initialization from the pressure outlet boundary.


Initialization will result in the volume fraction, X, Y, and Z velocities, and pressure being patched in the domain. The volume fraction will be patched in the domain based on the free surface level of the selected zone from the Compute from list. The velocities in the domain will be patched assuming the constant value provided for the velocity magnitude in the selected zone.


Important:  If you specify a profile for the velocity magnitude or direction vectors, the initialization will select the value for the velocity magnitude and direction vectors from only one face. Therefore the initialization may be inaccurate. However, generally, open channel inputs for velocity magnitude and direction vectors are constant.


The pressure that is patched is the hydrostatic pressure based on the free surface level specified in the selected zone.

You can use the following text command for open channel automatic initialization:

solve → initialize → open-channel-auto-init

When prompted, set up the following parameters:

boundary thread id

Enter the thread id for the boundary to be selected for open channel automatic initialization.

flat free surface initialization

This option is available for both open channel flow and open channel wave boundary conditions.

wavy free surface initialization

This option appears only for open channel wave boundary conditions, when flat free surface initialization is not selected.

The steps to be followed for open channel automatic initialization are

  1. Compute defaults based on valid open channel boundary thread. This step is required for better initialization of turbulence parameters based on uniform velocity magnitude.

    solve → initialize → compute defaults

  2. This would provide information about the selected boundary and type of initialization.

    solve → initialize → open-channel-auto-init

  3. Initialize

    solve → initialize → initialize

24.3.6.1. Reporting Parameters for Open Channel Wave BC Option

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:


Note:  You can enter values of 0, 1, or 2. Entering a higher number provides more information.


/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

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