26.12.1 User Inputs for Time-Dependent Problems

To solve a transient problem, you will follow the procedure outlined below:

1.   Enable the Transient option in the General task page (Figure  26.12.3).

General

Figure 26.12.3: The General Task Page for a Transient Calculation

2.   Define all relevant models and boundary conditions. Note that any boundary conditions specified using user-defined functions can be made to vary in time. See the separate UDF Manual for details.

3.   Specify the desired parameters in the Solution Methods task page (Figure  26.12.4).

Solution Methods

Figure 26.12.4: The Solution Methods Task Page for a Transient Calculation

If you are using the pressure-based solver, select PISO from the Scheme drop-down list in the Pressure-Velocity Coupling group box. To increase the speed of the calculations, you may need to modify the parameters related to the PISO scheme from their default values. See Section  26.3.1 for more information about the optimal use of the PISO algorithm.

If you are using the LES turbulence model with small time steps, the PISO scheme may be too computationally expensive. It is therefore recommended that you select SIMPLE or SIMPLEC instead of PISO.

It is best to select the Coupled pressure-velocity coupling scheme if you are using large time steps to solve your transient flow, or if you have a poor quality mesh.

Next, specify the desired Transient Formulation. The First Order Implicit formulation is sufficient for most problems. If you need improved accuracy, you can use the Second Order Implicit formulation instead. The Explicit formulation (available only for the density-based solver) is used primarily to capture the transient behavior of moving waves, such as shocks. For details, see this section in the separate Theory Guide.

When using the pressure-based solver, you have the additional options of selecting Non-Iterative Time Advancement and Frozen Flux Formulation for your time-dependent flow calculations (see this section and this section in the separate Theory Guide , respectively). Note that the latter option is only available for single-phase transient problems that do not use a moving/deforming mesh model.

4.   (optional) If you are using the explicit transient formulation or if you are using the adaptive time stepping method (described in a later step and in Section  26.12.2) it is recommended that you enable the printing of the current time (for the explicit transient formulation) or the current time step size (for the adaptive time stepping method) at each iteration, using the Statistic Monitors dialog box.

Monitors Statistic Edit...

Make sure that the desired item is selected from the Statistics selection list ( time for the current time or delta_time for the current time step size) and enable the Print option. When ANSYS FLUENT prints the residuals to the console window at each iteration, it will include a column with the current time or the current time step size.

5.   (optional) Use the Drag Monitor dialog box, the Lift Monitor dialog box, the Momentum Monitor dialog box, or the Surface Monitor dialog box to monitor (and/or save to a file) time-varying force coefficient values or a report of a field variable or function on a surface as it changes with time. See Section  26.13 for details.

6.   Set the initial conditions (at time $t = 0$) using the Solution Initialization task page.

Solution Initialization

You can also read in a steady-state data file to set the initial conditions.

File $\rightarrow$ Read $\rightarrow$ Data...

7.   Use the Autosave dialog box to specify the file name and frequency with which case and data files should be saved during the solution process. To open the Autosave dialog box, click the Edit... button next to Autosave Every in the Calculation Activities task page.

Calculation Activities( Autosave Case/Data) Edit...

See Section  4.3.4 for details about automatic file saving.

The Calculation Activities task page also allows you to export solution and particle history data during the transient calculation. See Section  4.16 for details.

If you want to create a graphical animation of the solution over time, you can use the Solution Animation dialog box to set up the graphical displays that you want to use in the animation. See Section  26.16 for details.

You may also want to request automatic execution of other commands using the Execute Commands dialog box. See Section  26.14 for details.

8.   (optional) You can improve the convergence of the transient calculations by enabling the Extrapolate Variables option in the Run Calculation task page (Figure  26.12.5). This option instructs ANSYS FLUENT to predict the solution variable values for the next time step using a Taylor series expansion, and then inputs that predicted value as an initial guess for the inner iterations of the current time step. As a result, the absolute residual levels are lowered.

Note that the Extrapolate Variables option is not available if you are employing either the NITA scheme with the pressure-based solver or the explicit formulation with the density-based solver.

If you use the Extrapolate Variables option when modeling an incompressible flow with the density-based solver, it is recommended that you disable the extrapolation of pressure values. After you have enabled the Extrapolate Variables option, type the following text command in the console window:

> solve/set/extrapolate-eqn-vars/pressure

Extrapolate Pressure? [yes]  no

9.   (optional) If you want ANSYS FLUENT to gather data for time statistics (i.e., time-averaged and root-mean-square values for solution variables) during the calculation, follow these steps:

(a)   Enable the Data Sampling for Time Statistics option in the Run Calculation task page (Figure  26.12.5) and specify the Sampling Interval.

Run Calculation

Enabling this option will allow you to display and report both the mean and the root-mean-square (RMS) values, as described in Section  26.12.4.

To select the variables for which you want to collect statistics, click the sampling Options... button.

Run Calculation Sampling Options...

Note that gathering data for time statistics is not meaningful inside a moving cell zone (e.g., a sliding zone in a sliding mesh problem, a moving zone in a dynamic mesh problem).

(b)   Initialize the flow statistics.

Solution Initialization Reset Statistics

Note that you can also reset the flow statistics after you have gathered some data for time statistics. If you perform, say, 10 time steps with the Data Sampling for Time Statistics option enabled, check the results, and then continue the calculation for 10 more time steps, the time statistics will include the data gathered in the first 10 time steps unless you reinitialize the flow statistics.

10.   Specify time-dependent solution parameters and start the calculation as described below for the implicit and explicit transient formulations:

• If you have chosen the First Order Implicit or Second Order Implicit formulation, the procedure is as follows:

  (a)   Set the time-dependent solution parameters in the Run Calculation task page (Figure  26.12.5).

  Run Calculation

  Figure 26.12.5: The Run Calculation Task Page for Implicit Transient Calculations

  

  Solution parameters for the implicit transient formulations are as follows:

  • Max Iterations/Time Step: When ANSYS FLUENT solves the time-dependent equations using the implicit formulation, multiple iterations may be necessary at each time step. This parameter sets a maximum for the number of iterations per time step. If the convergence criteria are met before this number of iterations is performed, the solution will advance to the next time step.

  • Time Step Size: The time step size is the magnitude of $\Delta t$. Since the ANSYS FLUENT formulation is fully implicit, there is no stability criterion that needs to be met in determining $\Delta t$. However, to model transient phenomena properly, it is necessary to set $\Delta t$ at least one order of magnitude smaller than the smallest time constant in the system being modeled. A good way to judge the choice of $\Delta t$ is to observe the number of iterations ANSYS FLUENT needs to converge at each time step. The ideal number of iterations per time step is 5-10. If ANSYS FLUENT needs substantially more, the time step is too large. If ANSYS FLUENT needs only a few iterations per time step, $\Delta t$ should be increased. Frequently a time-dependent problem has a very fast "startup'' transient that decays rapidly. Therefore, it is often wise to choose a conservatively small $\Delta t$ for the first 5-10 time steps. $\Delta t$ may then be gradually increased as the calculation proceeds.

    For time-periodic calculations, you should choose the time step based on the time scale of the periodicity. For a rotor/stator model, for example, you might want 20 time steps between each blade passing. For vortex shedding, you might want 20 steps per period.

    To verify that your choice for $\Delta t$ was proper after the calculation is complete, you can plot contours of the Courant number within the domain. To do so, select Velocity... and Cell Courant Number from the Contours of drop-down lists in the Contours dialog box. For a stable, efficient calculation, the Courant number should not exceed a value of 20-40 in most sensitive transient regions of the domain.

  • Time Stepping Method: By default, the size of the time step is fixed (as indicated by the selection of Fixed).

    To have ANSYS FLUENT modify the size of the time step as the calculation proceeds, select Adaptive and click the Settings... button to specify the parameters in the Adaptive Time Step Settings dialog box. See Section  26.12.2 for details.

    For transient volume of fluid (VOF) calculations that use the explicit scheme of VOF, you can select the Variable time stepping method. The parameters set through the Parameters... button are in many ways the same as for the adaptive time stepping method, with the exception of specifying a global Courant number (see Section  26.12.3).

    Note that with the Adaptive or Variable time stepping method, the value you specify for the Time Step Size will be the initial size of the time step. As the calculation proceeds, the Time Step Size shown in the Run Calculation task page will be the size of the current time step.

  (b)   Specify the desired Number of Time Steps in the Run Calculation task page and click Calculate.

  As it calculates a solution, ANSYS FLUENT will print the current time at the end of each time step.

• If you have chosen the Explicit transient formulation, you will follow a different procedure:

  (a)   Use the default settings in the Solution Controls task page.

  Solution Controls

  If you have modified the parameters, you can click the Default button to retrieve the default settings.

  (b)   Specify the desired Number of Iterations and click Calculate.

  Run Calculation

  Remember that when the explicit transient formulation is used, each iteration is a time step. When ANSYS FLUENT prints the residuals to the console windows, it will include a column with the current time (if you requested this in step 4, above).

• You can access the information saved in a data file, which includes a standard set of quantities that were computed during the calculation, by clicking the Data File Quantities... button. More information about this feature is available in Section  4.22.

11.   Save the final data file (and case file, if you have modified it) so that you can continue the transient calculation later, if desired.

File $\rightarrow$ Write $\rightarrow$ Data...

Additional Inputs

The procedures for setting the reporting interval, updating UDF profiles, interrupting iterations, and resetting data are the same as those for steady-state calculations. See Section  26.11 for details.

If you are using a user-defined function in your time-dependent calculation, note that, in addition to being updated after every $n$ iterations (where $n$ is the value of the UDF Profile Update Interval), the function will also be updated at the first iteration of each time step.