You will begin the sliding mesh calculation by initializing the solution (as described in Initializing the Entire Flow Field Using Standard Initialization) and then specifying the time step size and number of time steps in the Run Calculation Task Page, as for any other transient calculation. (See Performing Time-Dependent Calculations for details about time-dependent solutions.) Note that the time step size in the initial case file is saved without clicking . ANSYS Fluent will iterate on the current time step solution until satisfactory residual reduction is achieved, or the maximum number of iterations per time step is reached. When it advances to the next time step, the cell and wall zones will automatically be moved according to the specified translational or rotational velocities (as discussed in the previous section). The new interface-zone intersections will be computed automatically, and resultant interior/periodic/external boundary zones will be updated.
Note that you can run the MRF case using mesh interfaces with an appreciable loss of accuracy, doing so makes it easier to later on convert to a sliding mesh.
Note: The sliding mesh can be initialized with an MRF solution (rather using Standard or Hybrid initializations).
It is recommended that you preview the sliding mesh motion (as described in Previewing the Dynamic Mesh) before beginning your calculation. This can catch problems with the motion specification(s) before you begin the CFD calculation. Remember to save the case and initial data files before doing a mesh preview since the mesh position is altered once you do the preview. You can reread the initial condition case/data files to get back to the original mesh position.
ANSYS Fluent’s automatic saving of case and data files (see Automatic Saving of Case and Data Files) can be used with the sliding mesh model. This provides a convenient way for you to save results at successive time steps for later postprocessing.
Important: You must save a case file each time you save a data file because the mesh position is stored in the case file. Since the mesh position changes with each time step, reading data for a given time step will require the case file at that time step so that the mesh will be in the proper position. You should also save your initial case file so that you can easily return to the mesh’s original position to restart the solution if desired.
For some problems (for example, rotor-stator interactions),
you may be interested in a time-periodic solution. That is, the startup
transient behavior may not be of interest to you. Once this startup
phase has passed, the flow will start to exhibit time-periodic behavior.
If is the period of unsteadiness, then for some flow
property
at a given point in the flow field:
(10–1) |
For rotating problems, the period (in seconds) can be calculated
by dividing the sector angle of the domain (in radians) by the rotor
speed (in radians/sec): . For 2D rotor-stator problems,
, where
is the pitch and
is the blade speed. The number of time steps in
a period can be determined by dividing the time period by the time
step size. When the solution field does not change from one period
to the next (for example, if the change is less than 5%), a time-periodic
solution has been reached.
To determine how the solution changes from one period to the next, you must compare the solution at some point in the flow field over two periods. For example, if the time period is 10 seconds, you can compare the solution at a given point after 22 seconds with the solution after 32 seconds to see if a time-periodic solution has been reached. If not, you can continue the calculation for another period and compare the solutions after 32 and 42 seconds, and so on until you see little or no change from one period to the next. You can also track global quantities, such as lift and drag coefficients and mass flow, in the same manner. Figure 10.11: Lift Coefficient Plot for a Time-Periodic Solution shows a lift coefficient plot for a time-periodic solution.
The final time-periodic solution is independent of the time steps taken during the initial stages of the solution procedure. You can therefore define “large” time steps in the initial stages of the calculation, since you are not interested in a time-accurate solution for the startup phase of the flow. Starting out with large time steps will allow the solution to become time-periodic more quickly. As the solution becomes time-periodic, however, you should reduce the time step in order to achieve a time-accurate result.
Important: If you are solving with second-order time accuracy, the temporal accuracy of the solution will be affected if you change the time step during the calculation. You may start out with larger time steps, but you should not change the time step by more than 20% during the solution process. You should not change the time step at all during the last several periods to ensure that the solution has approached a time-periodic state.