To solve a time-dependent problem, you will follow the procedure outlined below:
Define Models Solver...
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.
Solve Controls 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.
| 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.
| 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.
Solve Monitors 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.
Solve Initialize Initialize...
You can also read in a steady-state data file to set the initial conditions.
File Read Data...
File Write 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.
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.
| 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).
Solve Initialize 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.
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 , 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).
As it calculates a solution, FLUENT will print the current time at the end of each time step.
Solve Controls Solution...
If you have modified the Solver Parameters, you can click the Default button to retrieve the default settings.
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).
File Write Data...
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.
| If you are using a user-defined function in your time-dependent calculation, note that, in addition to being updated after every
is the value of the
UDF Profile Update Interval), the function will also be updated at the first iteration of each time step.