The Write ICEM CFD Files control determines whether Ansys ICEM CFD files are written, and includes options for running Ansys ICEM CFD interactively or in batch mode from an Ansys ICEM CFD Replay file.
Note: The Write ICEM CFD Files control is available when you use any Ansys ICEM CFD mesh method that is available in the Meshing application (Patch Independent Tetra, MultiZone, or MultiZone Quad/Tri). However, the Interactive and Batch options are available only if Ansys ICEM CFD is installed. A warning is issued if you try to use one of these options and Ansys ICEM CFD cannot be found.
Note: Another method for writing meshing data to ICEM CFD files is to select the Mesh cell in Workbench and select Transfer Data to New>ICEM CFD. While the Write ICEM CFD control writes the geometry of a part, using the Ansys ICEM CFD Add-in component links to the entire Geometry assembly. For more information, see Component Systems in the Ansys Workbench User's Guide.
Options for Write ICEM CFD Files include:
No
No files are written. This is the default.
Yes
Writes Ansys ICEM CFD files. Useful when you are working in Ansys Workbench but you want to export your project files for further mesh editing in Ansys ICEM CFD. If this control is set to Yes, your Ansys ICEM CFD project (.prj), geometry (.tin), unstructured domain (.uns), and blocking (.blk) files will be saved during mesh generation.
If your Ansys Workbench project file has been saved, your Ansys ICEM CFD files will be written to the Ansys Workbench project directory. Ansys Workbench creates a project folder as the top level folder for each project, at the same level as the project file. The project folder will be named <
filename>_files, where <filename> is a name you provide. The project file will be named <filename>.wbpj. Under the project folder is a design point subdirectory for each design point in the project. The active design point is always design point 0 (dp0) and corresponds to the design point labeled Current in the Ansys Workbench GUI. Under each design point folder are system folders for each system type in the project ( Mechanical, Fluent, etc.). Each system folder contains solver-specific files and folders, such as input files, model directories, engineering data, resources, etc. Following this structure, the Ansys ICEM CFD files will be written to <filename>_files\dp0\global\MECH\SYS.If your Ansys Workbench project file has not been saved, your Ansys ICEM CFD files will be written to the temporary Ansys Workbench folder, as follows: %TEMP%\WB_<
computer>\unsaved_project_files\dp0\global\MECH\SYS.
Note:
Only appropriate files are written, based on the selected mesh method.
Refer to the Ansys Workbench help for more information about project file management in Ansys Workbench.
Interactive
Applicable only when Ansys ICEM CFD is installed.
When the Interactive option is set and you select Generate Mesh, the Meshing application launches Ansys ICEM CFD in interactive mode. When you specify the Interactive option, you must also select an option for ICEM CFD Behavior to determine whether the geometry and/or mesh is transferred to Ansys ICEM CFD.
Typically, you run in interactive mode to set up an Ansys ICEM CFD Replay script file (*.rpl) that can be run later in either batch or interactive mode. You can begin by loading a generic Replay file. It is important to use this default Replay file because the batch process requires the pre and post steps that are defined within it. To load the default Replay file:
From within Ansys ICEM CFD, select > > and the Replay Control window appears.
Click on the Replay Control window and the Open Script File window appears.
Click on the Open Script File window to load the default Replay file.
You can incorporate your custom commands into the Replay file by using the Replay Control feature or a text editor. The Replay file will be associated with your Ansys ICEM CFD project when you save the project and exit Ansys ICEM CFD.
After the mesh is returned to the Meshing application and the Ansys Workbench project is saved, the Replay file will be written to the Ansys Workbench project directory. Later you can set Write ICEM CFD Files to Batch and the mesh will be updated automatically in batch. You can change parameters on the Ansys Workbench project page and Update the mesh in batch from either the project page or from within the Meshing application.
Refer to Rules for Interactive Editing and Limitations of Ansys ICEM CFD Interactive for related information.
For more information about Replay Control, refer to the documentation available under the Help menu within Ansys ICEM CFD.
Batch
Applicable only when Ansys ICEM CFD is installed.
Runs Ansys ICEM CFD in batch mode from an existing Replay file. If you specify the Batch option, you must also select an option for ICEM CFD Behavior to determine whether the geometry and/or mesh is transferred to Ansys ICEM CFD.
ICEM CFD Behavior
Determines Ansys ICEM CFD behavior when running Ansys ICEM CFD in Interactive or Batch mode.
For Patch Independent Tetra, the available options under are:
Generate Mesh - After the meshing operation completes, transfers both the geometry and mesh to Ansys ICEM CFD for editing.
Skip Meshing - Bypasses the meshing operation and transfers only the geometry to Ansys ICEM CFD for meshing and editing.
For MultiZone and MultiZone 2D, the available options under are:
Generate Blocking and Mesh - After the meshing operation completes, transfers the geometry, blocking, and mesh to Ansys ICEM CFD for editing.
Generate Blocking - Bypasses the meshing operation and transfers only the geometry and blocking to Ansys ICEM CFD for meshing and editing.
Update pre-existing Blocking - Bypasses the blocking operation, updates pre-existing blocking and meshes, and transfers the geometry and mesh to ANSYS ICEM CFD for meshing and editing. When you select Update pre-existing Blocking, the Update Sizes is set to Yes by default and updates the bunching with the given Workbench parameters while meshing. When the Update Sizes is set to No, protects the bunching in ICEM CFD files.
Named Selection Treatment: Provides named selection transfer for Interactive and Batch. The available options are Parts and Subsets.