The Run Calculation task page allows you to start the solver iterations. See Performing Steady-State Calculations and Performing Time-Dependent Calculations for details about the items below.

Controls
opens the Case Check Dialog Box.
opens the Mesh Motion Dialog Box.
is available for fluid and solid zones and will only appear for steady-state cases, where the pressure-based coupled solver is used. Note that the Pseudo Transient option must be enabled in the Solution Methods Task Page. For details about the available options, see Performing Pseudo Transient Calculations.
(for steady flow calculations) sets the number of iterations to be performed. (For unsteady calculations using the explicit unsteady formulation, this will specify the number of time steps, since each iteration will be a time step.)
(for transient flow calculations) contains options for how the time step is determined.
selects a fixed time step, equal to the specified Time Step Size.
selects a time step that is initially equal to the specified Time Step Size, but gets modified by ANSYS Fluent as the calculation proceeds. See Adaptive Time Stepping for details.
enables variable time stepping method. The inputs are same as for the adaptive time stepping method, with the exception of specifying a global Courant number. Variable is selectable when the VOF multiphase model is enabled. See Variable Time Stepping for details.
opens either the Adaptive Time Step Settings Dialog Box when Adaptive is selected as the Time Stepping Method, or the Variable Time Step Settings Dialog Box when Variable is selected as the Time Stepping Method.
(for transient flow calculations) sets the magnitude
of the (physical) time step .
determines the highest frequency that the acoustic analysis reproduces. This is available when the FW-H acoustics model is enabled.
(for transient flow calculations) sets the number of time steps to be performed.
contains options related to unsteady calculations.
instructs ANSYS Fluent to predict the solution variable values for the next time step and then input that predicted value as an initial guess for the inner iterations of the current time step.
enables the sampling of data during an unsteady calculation. See User Inputs for Time-Dependent Problems and Postprocessing for Time-Dependent Problems for details.
allows you to specify the frequency of the Data Sampling for Time Statistics.
opens the Sampling Options Dialog Box for the Data Sampling for Time Statistics.
displays the time period over which data has been sampled for the postprocessing of the mean and RMS values.
enables a different time step to be specified for solid zones, either user specified or automatically calculated. See Specifying a Solid Time step for details.
for unsteady flow calculations using an implicit unsteady formulation) sets the maximum number of iterations to be performed 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. See User Inputs for Time-Dependent Problems for details.
sets the number of iterations that will pass before convergence monitors will be printed and plotted. The default is 1 (that is, reports will be updated after each iteration).
results in the automatic postprocessing of pollutants during a transient simulation. This option is available when one of the pollution models is enabled.
sets the maximum number of postprocessing iterations to be performed per time step. This field is available when the Postprocess Pollutants option is enabled.
sets the number of iterations that will pass before user-defined functions for boundary profiles will be updated.
allows you to set parameters that will help ANSYS Fluent guide the calculations to a converged solution (available only for steady-state flows in the density-based implicit solver). See Solution Steering for more information. When enabled, the following options are available:
allows you to select the flow type that best describes the flow in the solution domain. Five choices are available: incompressible, subsonic, transonic, supersonic, and hypersonic.
allows for full multigrid initialization.
allows you to reduce the desired solution accuracy by selecting a blending factor less than 100%. The default setting is 100%. See First-to-Higher Order Blending in the Theory Guide for more information. The blending factor will be grayed out if Second Order Upwind discretization for the Flow equations is not selected in the Solution Methods task page. The solution accuracy may be reduced (typical values are 75% or 50%) if it is not possible to obtain a converged solution with the maximum second-order accuracy (blending = 100%).
opens the Solution Steering Dialog Box.
is a non-adjustable field displaying the current CFL number, which allows you to view it during the calculation.
opens the Data File Quantities Dialog Box.
opens the Acoustic Signals Dialog Box. This button is only available when the acoustics model is enabled.
opens the Acoustic Sources FFT Dialog Box. This button is only available for three-dimensional transient simulations, when the Export Acoustic Source Data in ASD Format option is enabled in the Acoustics Model dialog box.
starts the calculations. While the calculation is in progress, a Working dialog box will appear. Clicking the Cancel button or typing Ctrl+c in the console window will interrupt the calculation at the earliest safe stopping point after the current iteration (in steady-state simulations) or the current time step (in transient simulations). The stopping point is chosen so that the field variables and solver state are updated and internally consistent. If you are running a transient simulation and want to stop the simulation immediately (before the completion of the current time step), you can type Ctrl+c a second time.
For additional information, see the following sections: