### 4.2.1. Steps to Set Up a Simulation Using ICEM CFD Replay Remeshing

The following discussion presents the three general steps required to set up a simulation using the ICEM CFD Replay remeshing option.

The first step involves creating the reference Geometry File within the ANSYS ICEM CFD environment. If the geometry was not created within that environment, use one of the File > Import Geometry options in the ANSYS ICEM CFD environment. At this point, ensure that all required Parts (or Families) are defined and named so that they can be referenced when completing the ICEM CFD Replay remeshing definition later in CFX-Pre. Finally, store the geometry in the ICEM CFD native geometry file format (namely, a `.tin` file).

The second step involves generating the Mesh Replay File, again, from within the ANSYS ICEM CFD environment. Start with the previously created geometry loaded, and work sequentially through the mesh generation process until acceptable mesh controls have been specified. This may require fine tuning, which will involve the regeneration of your mesh after moving the geometry through its expected range of motion. Once you are satisfied with the mesh control settings, purge the last mesh using File > Mesh > Close Mesh, and reload the original reference geometry. Complete the following tasks to generate the required Mesh Replay File:

1. Use File > Replay Scripts > Replay Control to begin recording the commands for the Mesh Replay File. The Replay Control dialog box is displayed.

2. Revisit all of the mesh related tabs and settings used to generate the mesh, clicking either the Apply or OK to commit the settings into the Replay Control panel.

3. Generate the mesh.

4. In the Replay Control panel, clear the Record (after current) toggle and select Save to write the settings to replay file.

You may also want to export the mesh that was (re)generated for use in the simulation definition (as in the next step).

The third step involves defining the simulation within CFX-Pre. Complete the following tasks to prepare the simulation:

1. Start a new simulation and import the (previously generated) mesh.

2. Define expressions for the motion of the geometry.

   Note: See also the discussion in Mesh Re-Initialization During Remeshing.

3. Define the flow analysis including the definition of one or more solver interrupt controls, as described in Interrupt Control in the CFX-Pre User's Guide, to identify the condition(s) under which solver execution will be interrupted.

4. Define a configuration and complete the ICEM CFD Replay remeshing setup as described in ANSYS ICEM CFD Replay Remeshing in the CFX-Pre User's Guide. The Geometry File and Mesh Replay File created above are referenced here. Note also, that references to one or more of the previously defined solver interrupt control conditions are required to activate remeshing.

5. Complete any execution controls for the simulation and either start the solver or write the CFX-Solver Input file for later use.

Release 18.2 - © ANSYS, Inc. All rights reserved.