11.2.3 Solution Strategies for Sliding Meshes

You will begin the sliding mesh calculation by initializing the solution (as described in Section  26.9.1) 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 Section  26.12 for details about time-dependent solutions.) Note that the time step size in the initial case file, is saved without clicking Calculate. 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 ( this section in the separate Theory Guide).

Saving Case and Data Files

ANSYS FLUENT's automatic saving of case and data files (see Section  4.3.4) 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.

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.

If you are planning to solve your sliding mesh model in several stages, whereby you run the calculation for some period of time, save case and data files, exit ANSYS FLUENT, start a new ANSYS FLUENT session, read the case and data files, continue the calculation for some time, save case and data files, exit ANSYS FLUENT, and so on, there may be some distortion in the mesh with each subsequent continuation of the calculation. To avoid this problem, you can delete the mesh interface before saving the case file, and then create it again after you read the case file into a new ANSYS FLUENT session.

Time-Periodic Solutions

For some problems (e.g., 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 $T$ is the period of unsteadiness, then for some flow property $\phi$ at a given point in the flow field:

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): $T = \theta/\Omega$. For 2D rotor-stator problems, $T = P/v_b$, where $P$ is the pitch and $v_b$ 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 will need to 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  11.2.2 shows a lift coefficient plot for a time-periodic solution.

Figure 11.2.2: 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.

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.