August 13, 2013, 00:11
Join Date: Jul 2013
Rep Power: 4
according to the http://www.sharcnet.ca/Software/Flue...me_inputs.html
- 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 . Since the ANSYS FLUENT formulation is fully implicit, there is no stability criterion that needs to be met in determining . However, to model transient phenomena properly, it is necessary to set 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 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, 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 for the first 5–10 time steps. 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 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 Adaptive Time Stepping 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 Variable Time Stepping).
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.
- 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.