[Fluent Inc. Logo] return to home search
next up previous contents index

25.17.1 User Inputs for Time-Dependent Problems

To solve a time-dependent problem, you will follow the procedure outlined below:

1.   Enable the Unsteady option in the Solver panel (Figure  25.17.3), and specify the desired Unsteady Formulation.

Define $\rightarrow$ Models $\rightarrow$ Solver...

Figure 25.17.3: The Solver Panel for an Unsteady Calculation
figure

The 1st-Order Implicit formulation is sufficient for most problems. If you need improved accuracy, you can use the 2nd-Order Implicit formulation instead. The Explicit formulation (available only if the density-based explicit formulation is selected under Solver and Formulation at the top of the panel) is used primarily to capture the transient behavior of moving waves, such as shocks. See Section  25.3.2 for details.

You can also use the Non-iterative Time Advancement option, under Transient Controls, when using the pressure-based segregated algorithm for your time dependent flow calculations (see Section  25.4.5).

When using the pressure-based solver, you can also select Frozen Flux Formulation under Transient Controls in your time dependent flow calculations (see Section  25.4.4). Note that this option is only available for single-phase transient problems that use the pressure-based solver and do not use a moving/deforming mesh model.

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.   If you are using the pressure-based solver, choose PISO as the Pressure-Velocity Coupling scheme under Discretization in the Solution Controls panel.

Solve $\rightarrow$ Controls $\rightarrow$ Solution...

In general, to increase the speed of the calculations, you will need to modify the PISO Parameters from their default values. See Section  25.9.1 for more information about the optimal use of the PISO algorithm.

figure   

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 use SIMPLE or SIMPLEC instead of PISO.

figure   

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

4.   (optional) If you are using the explicit unsteady formulation or if you are using the adaptive time stepping method (described below and in Section  25.17.2) it is recommended that you enable the printing of the current time (for the explicit unsteady formulation) or the current time step size (for the adaptive time stepping method) at each iteration, using the Statistic Monitors panel.

Solve $\rightarrow$ Monitors $\rightarrow$ Statistic...

Select time (for the current time) or delta_time (for the current time step size) in the Statistics list and turn on the Print option. When FLUENT prints the residuals to the console at each iteration, it will include a column with the current time or the current time step size.

5.   (optional) Use the Force Monitors panel or the Surface Monitors panel to monitor (and/or save to a file) time-varying force coefficient values or the average, mass average, integral, or flux of a field variable or function on a surface as it changes with time. See Section  25.18 for details.

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

Solve $\rightarrow$ Initialize $\rightarrow$ Initialize...

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

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

7.   Use the automatic saving feature to specify the file name and frequency with which case and data files should be saved during the solution process.

File $\rightarrow$ Write $\rightarrow$ Autosave...

See Section  4.3.4 for details about the use of this feature.

You may also want to request automatic execution of other commands using the Execute Commands panel. See Section  25.19 for details.

8.   (optional) If you want to create a graphical animation of the solution over time, you can use the Solution Animation panel to set up the graphical displays that you want to use in the animation. See Section  25.20.1 for details.

9.   (optional) If you want 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)   Turn on the Data Sampling for Time Statistics option in the Iterate panel.

Solve $\rightarrow$ Iterate...

Enabling this option will allow you to display and report both the mean and the root-mean-square (RMS) values, as described in Section  25.17.4.

figure   

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

(b)   Initialize the flow statistics.

Solve $\rightarrow$ Initialize $\rightarrow$ Reset Statistics

Note that you can also use this menu item to 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 unsteady formulations:

  • If you have chosen the 1st-Order or 2nd-Order Implicit formulation, the procedure is as follows:

    (a)   Set the time-dependent solution parameters in the Iterate panel (Figure  25.17.4).

    Solve $\rightarrow$ Iterate...

    Figure 25.17.4: The Iterate Panel for Implicit Unsteady Calculations
    figure

    Solution parameters for the implicit unsteady formulations are as follows:

    • Max Iterations per Time Step: When FLUENT solves the time-dependent equations using the implicit formulation, an iteration is 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 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 FLUENT needs to converge at each time step. The ideal number of iterations per time step is 5-10. If FLUENT needs substantially more, the time step is too large. If FLUENT needs only a few iterations per time step, $\Delta t$ may 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 determine a proper choice of $\Delta t$, 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 panel. For a stable, efficient calculation, the Courant number should not exceed a value of 20-40 in most sensitive transient regions of the domain.

    By default, the size of the time step is fixed (as indicated by the selection of Fixed under Time Stepping Method). To have FLUENT modify the size of the time step as the calculation proceeds, select Adaptive and specify the parameters under Adaptive Time Stepping in the expanded Iterate panel. See Section  25.17.2 for details.

    With the Adaptive time stepping method (Figure  25.17.5), 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 Iterate panel will be the size of the current time step (see Section  25.17.2).

    For transient VOF calculations, the inputs that are used in the Variable time stepping method (Figure  25.17.6) are in many ways the same as for the adaptive time stepping method, with the exception of specifying a global Courant number (see Section  25.17.3).

    (b)   Specify the desired Number of Time Steps in the Iterate panel and click Iterate.

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

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

    (a)   Use the default settings for the Solver Parameters in the Solution Controls panel.

    Solve $\rightarrow$ Controls $\rightarrow$ Solution...

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

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

    Solve $\rightarrow$ Iterate...

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

11.   Save the final data file (and case file, if you have modified it) so that you can continue the unsteady 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  25.16 for details.

figure   

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.


next up previous contents index Previous: 25.17 Performing Time-Dependent Calculations
Up: 25.17 Performing Time-Dependent Calculations
Next: 25.17.2 Adaptive Time Stepping
© Fluent Inc. 2006-09-20