## 4.2. ICEM CFD Replay Remeshing

ICEM CFD Replay remeshing provides a highly automated remeshing process that is ideally suited for users of the ANSYS ICEM CFD mesh generation software and cases that involve translational mesh motion only (that is, no rotation or general deformation). When this option is used, a master replay file is assembled from other task-oriented replay files and submitted to the ANSYS ICEM CFD mesh generator for batch execution. These replay files are illustrated in the figure below, along with the general process flow for this remeshing option. The dashed line in the figure highlights components of the master replay file and identifies files and steps that you can modify. Unless otherwise noted, files are contained in the `<CFXROOT>/etc/Remeshing` directory.

Figure 4.3: Schematic for ICEM CFD Replay remeshing

When this option is used, the following steps are automatically executed:

- Extract geometry and mesh control data and write them to the `cfx_params.rpl` replay file in the run directory. The data includes:

  - Centroid displacements for boundaries that are included in ANSYS ICEM CFD Part Maps

  - Mesh control parameters (for example, `ehgt` and `emax`)

  - Scalar parameters.

- Run (in batch) the ANSYS ICEM CFD mesh generation program using the master replay file. This master replay file executes the following tasks:

  - Read the `cfx_params.rpl` file.

  - Load the reference geometry from the Geometry File identified in the Remesh definition.

  - Apply displacements (including scaling and any offsets) corresponding to all ANSYS ICEM CFD Part Map definitions contained in the Remesh definition. This is done using the default geometry replay file provided, or using the user defined replay file if specified in the ICEM CFD Geometry Control setting.

  - Apply ICEM CFD Mesh Controls defined in the Remesh definition. This is done using the provided controls, or using the user-defined replay file if specified in the ICEM CFD Mesh Control setting.

  - Load your Mesh Replay File, specified in the Remesh definition.

  - Export a new mesh for ANSYS CFX.

- Insert the new mesh(es) into the analysis definition, and generate an updated CFX-Solver Input file.

- Interpolate the previously generated analysis results onto the new mesh, re-partition the mesh if a parallel run mode is selected, and continue the solution process.

You must create the reference Geometry File and the Mesh Replay File because these are specific to each case. However, the generic default replay files (`icemcfd_Remesh.rpl`, `icemcfd_GeomMod.rpl`, and `icemcfd_MeshMod.rpl`) used by this option are provided in the `<CFXROOT>/etc/Remeshing` directory. These files may be edited to provide installation-wide changes to the ICEM CFD Replay remeshing behavior. Alternatively, the geometry and mesh modification files may be copied and edited to provide case-specific changes.

Note: As indicated previously, only translational mesh motion is automatically handled by the ICEM CFD Replay remeshing option. This is accomplished by applying the displacements of centroids of boundaries in the ANSYS CFX analysis definition to parts in the ANSYS ICEM CFD geometry. All other mesh motion (such as rotation about the centroid or another point, or general deformation) will not be applied, and an inconsistency in the analysis geometry before and after remeshing will be introduced.

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