14.7.2. Solving Reactor Networks

The steps and procedure for setting up and solving a Reactor Network model are outlined below.

  1. Enable the Reactor Network model.

     Setup → Models → Species → Reactor Network   Edit...


    Important:  Note that this model is only available when one of the reacting species models is enabled.


    When you select the Reactor Network Model option, the dialog box expands to show the relevant modeling controls (see Figure 14.27: Reactor Network Dialog Box (Steady-State Flow)).

    Figure 14.27:  Reactor Network Dialog Box (Steady-State Flow)

    Reactor Network Dialog Box (Steady-State Flow)


  2. If a detailed chemical mechanism has already been imported, select the mixture material from the Detailed Mechanism Material Name drop-down list. Otherwise import a mechanism in CHEMKIN format by clicking Import CHEMKIN Mechanism.... The mechanism files are imported into your case using the CHEMKIN Mechanism Import dialog box as described in Specifying a Chemical Mechanism File for Flamelet Generation.

  3. Set the Number of Reactors in the reactor network. The default value of 50 is a good starting value, but it can be increased for greater accuracy.

  4. Specify whether or not the temperature is calculated from the equation of state by selecting or clearing the Solve Temperature check box. By default, this option is selected, and ANSYS Fluent will determine the temperatures in the reactor network.

  5. Once cells are agglomerated and a reactor-network solution is calculated, you can select the Use Current Reactor Network option to perform further reactor network simulations with the existing network of connected reactors. This option can be used to continue iterations from the previous reactor- network solution if additional convergence is desired. The option also allows you to change the chemical mechanism or species boundary conditions to generate a new solution on the current reactor network.

  6. (for transient analysis with the Data Sampling For Time Statistics option selected in the Run Calculation task page only) Specify whether or not you want to use the time-averaged composition fields to agglomerate the reactors and time-averaged velocity fields to calculate the reactor mass flux matrix (instead of the instantaneous fields) by selecting or clearing the Use Time Averaged Fields option.


    Note:  The Use Time Averaged Fields option should be used for unsteady simulations (for example, LES) of statistically stationary combustors.


  7. If necessary, specify custom-field functions and adjust the default solver settings using the Expert Options control. When Expert Options is selected, the Reactor Network dialog box expands to reveal the following advanced options:

    Figure 14.28:  Reactor Network Dialog Box - Expert Options

    Reactor Network Dialog Box - Expert Options

    ODE Relative Error Tolerance, ODE Absolute Error Tolerance

    The default values for the ODE relative and absolute error tolerances are 1e-05 and 1e-12, respectively. If the ODE solver fails to converge, it is often helpful to lower the ODE Relative Error Tolerance and the ODE Absolute Error Tolerance.

    Reactor Network Convergence Tolerance

    The default value for the reactor network convergence tolerance is 1e-08. Residuals should be well converged at the default tolerance. Higher tolerances may be acceptable for engineering accuracy.

    Solver

    The default segregated solver typically converges faster than the coupled solver. However, when using the segregated solver, residuals may stall above an acceptable tolerance. In this case, the coupled solver should be used.

    Maximum Number of Iterations (segregated solver)

    If residuals are still decreasing and better convergence is desired, increase the maximum number of iterations. If residuals are stalled and a quicker exit from the solver is desired, decrease the maximum number of iterations.

    Maximum Integration Time (coupled solver)

    The ODE solver terminates the calculation at this time if residuals fail to converge.

    Use Custom Field Functions to Define Reactor Zones

    When selected, this option allows you to use custom field functions (Custom Field Functions) as composition variables to create the reactor volumes. ANSYS Fluent clusters CFD cells that have similar compositions using the following default composition variables:

    • temperature and mixture fraction for Non-Premixed and Partially-Premixed cases

    • temperature and mass fractions of and for Species Transport cases

    You can override these default composition variables by selecting Use Custom Field Functions to Define Reactor Zones and then selecting up to four custom field functions from the Custom Field Functions selection list. ANSYS Fluent will group CFD cells that are close in these custom field function composition variables. In the example shown in Figure 14.28: Reactor Network Dialog Box - Expert Options, cells with similar turbulent kinetic energy, x coordinate, and y coordinate will be agglomerated to form the reactor network.

  8. Click Calculate Reactor Network to obtain a flow solution.

    As the calculation is progressing, ANSYS Fluent prints the reactor network residuals for each iteration in the console.


    Note:  The reactor network solution should converge with the default settings. However, if the model fails to converge with sufficient accuracy, you can adjust the default reactor network solver settings by using the Expert Options control.



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