The ability to play session files is missing in Ansys Workbench for Ansys CFX applications.

The undo stack is cleared in CFX-Pre/CFD-Post after the application receives commands from Ansys Workbench.

You cannot launch Ansys CFX products from one another in Ansys Workbench; you must use the system cells.

Ansys Workbench "remembers" previous locations of imported files / projects. Ansys CFX, however, displays different behavior for loading or saving any files, always using the directory specified in the Tools > Options > Default Folder for Permanent Files in Ansys Workbench.

Duplicate node removal for importing Fluent meshes into CFX-Pre is always ON in Ansys Workbench, regardless of any settings in the Ansys CFX preferences file. CFX-Pre does not read this file when run in Ansys Workbench.

If you have a Fluid Flow (CFX) system, and you want to duplicate the system in such a way that the duplicate shares Geometry and Mesh with the original system, then right-click the Setup cell of the original Fluid Flow system (not the system header) and choose Duplicate. The CFX data associated with the original Setup cell is copied to the duplicated Setup cell, ready for you to modify it.

If you create a set up by duplicating an existing one, the run files associated with the first schematic are named according to the name of the schematic; in this release it is not possible to control the name of the run files in the duplicate schematics.

Duplication normally involves only user files (files for which you have specified settings). For Ansys CFX, these are the .cfx and .cst files. Other files, which are considered to be "generated" (for instance, the .def, .res, and .out files), are not duplicated.

Rename all your CFX and Fluid Flow (CFX) systems to something unique and meaningful that reflects the contents of the system, especially if there are multiple systems. The names of the files associated with the system cells will incorporate this system name when the files are first created, making it easier for you to identify the files in the Files pane. Furthermore, CFD-Post will take the system name (by default "Fluid Flow" for a Fluid Flow system) as the case name of the results in CFD-Post. Note that it is best to rename the systems as soon as they are placed on the Project Schematic, as the generated file names and/or the CFD-Post case names will not necessarily be updated if a system is renamed after the appropriate cells already have associated data (for example, a .cfx file with the Setup cell). It may be useful to reset the Results cell to update the CFD-Post case name if the system is renamed, but you will lose any existing CFD-Post settings and objects by doing this.

When you connect an up-to-date Mesh cell to the Setup cell of a CFX or a Fluid Flow (CFX) system, the Mesh cell becomes out-of-date because the relevant data must be created. You must update the Mesh cell.

If a second identical component system is added (CFX+CFX or Fluent+Fluent), there is no need to update the project again. An update of the project is required if a different system component is added (CFX+Fluent or Fluent+CFX).

Changing the Mesh Import options (for example, relating to Names Selections or Contact settings) for importing a mesh from a Mesh cell into a Setup cell (CFX-Pre) is not straightforward. The Setup cell will use whatever options are stored in your preferences file at the time when the mesh is imported. You can change these settings by using Tools > Options or by using the Mesh Import form in stand-alone CFX-Pre (choosing Use settings next time). The next time you refresh the Setup cell with a new Mesh, CFX-Pre will use the new mesh import settings. In some circumstances this could lead to unexpected results, for example if you were relying on a specific set of Named Selection options to identify your regions but changed these settings when working on another project.

If you make changes to the execution control in CFX-Pre while you have CFX-Solver Manager open, you need to click the Refresh button on the Define Run dialog box in order to make sure that the CFX-Solver Manager re-reads the new information from the CFX-Solver Input file.

When you edit the Solution cell, the Define Run dialog box of the CFX-Solver Manager has a Save Settings button. Clicking this button associates the settings on the dialog box with the Solution cell and closes the dialog box. You must now update the Solution cell to run the CFX-Solver.

Always check that the Initialization Option property is set correctly for each Solution cell in any CFX-related system. This can be viewed and set using:

The default value for the Initialization Option property is Update from current solution data if possible unless you change the Workbench preference for this property. Details of the Initialization Option property are given in Properties Pane.

After running the CFX solver multiple times within the same system, for example when updating the solution or continuing the calculation, you may accumulate unwanted results files from the previous runs. Consider using Reset or Clear Generated Data on the Solution cell before re-running the CFX-Solver on this cell. These delete all the files from any previous run on that cell (for example, all CFX-Solver Results and CFX-Solver Output files), and prevent the project from getting too large. If you do not want to clear all the files, but want to clear some of them, consider using Clear Old Solution Data or Clear Cached Solution Data on the Solution cell. If you want to delete specific files:

After doing this, you may want to remove the obsolete file references from the list in the Files pane. Multi-select all the red files (sort by ascending size to get them all together) and choose to Remove <file> from List to get Ansys Workbench to remove them from the Files pane completely.

If you set the CFX-Solver to Background mode and shut down Ansys Workbench, upon restarting Ansys Workbench and reopening the project, if the solver run has not completed, you will need to use the Reconnect button to continue monitoring the solver run.

The information at end of a CFX-Solver Output file shows only the temporary location for the CFX-Solver Results file, not the final location. The correct locations can be found in the Files pane.

CFX-Solver Results files (in particular the .res files) are associated with the Solution cell, not the Results cell. This means that a CFX-Solver Results file cannot be imported onto a Results cell; it can be imported onto a Solution cell of a Fluid Flow or CFX system. Similarly, resetting the Results cell will not remove the CFX-Solver Results file.

Ansys Workbench permits you to import data from a Polyflow Solution cell into the Solution cell of a CFX system; however, the CFX-Solver execution will fail when the Solution cell of the CFX system is updated.

For simulations involving multiple configurations, initializing a Solution cell of either a Fluid Flow (CFX) analysis system or a CFX component system from another Solution cell is not supported. Attempts to update the downstream Solution cell will result in an error. You must define initialization conditions for each configuration manually.

In Ansys Workbench, the state of CFD-Post is associated with the Results cell. To maintain multiple states, you must generate multiple Results systems. For your convenience, you can provide a unique name for each system.

To perform a file comparison in CFD-Post, drag a Solution cell from another system to the Results cell.

You can have CFD-Post generate report output at every update (by setting Generate Reports in Results cell Properties pane). The .html file is visible in the Files pane: right-click it, select Open containing folder, and double-click the file in the explorer to see the report in a browser.

When updating existing Results cell data (with CFD-Post open) where a turbo chart with an averaged variable was used (for example, turbo reports), a warning dialog box may appear reporting that "No data exists for variable …" This warning can be ignored.

You can change the CFD-Post multi-configuration load options (available on the Load Results panel of CFD-Post when in stand-alone mode) by editing the Properties of the Solution cell. This is a property of the Solution cell, rather than the Results cell.

If you accidentally delete the current .def, .res or .out files for a CFX system and the Solution cell status is up-to-date, you may get errors when trying to display the solution monitor or edit the Results cell. In this case you will need to replace the files in the File Manager, or Reset the Solution cell, and update the system. If the .def file is missing, you may also need to Clear Generated Data for the Setup cell before updating the system.

When importing a .wbdb file (that contains .agdb, .cmdb, .cfx, and .res files), only a Mesh system is imported instead of a "Fluid Flow (CFX)" analysis system. You need to drag a CFX system and associate the files with this system.

Pointers to the original CFX files are present in the Files pane. Using the right-click option Import Onto Schematic, a copy of the file is taken and an associated system is generated with the copy - however the Files pane now seems to have two versions of the same file.

You can drag a CFX system and associate the files with this system, manually importing the file into the correct cell.

Ansys Workbench does not support directly importing legacy FSI cases, so you have to create a CFX system from the legacy CFX-Solver Results file, manually link it to the Static Structural system, suppress the old load in Static Structural, and update it to import the load in the proper format from the CFX system.

Files that are moved or deleted and that were previously associated with a cell in the Project Schematic will be highlighted in red in the Files pane. There are right-click options to Remove or Repair the files. You should be aware that Ansys Workbench will ensure that the file is repaired using a file of a similar type but not necessarily the same name (or contents). If the contents of the repaired file do not match those of the original file, unexpected results may be produced or the case will fail.

If you are using license sharing in Ansys Workbench, you can use only one license for CFX-Pre/CFD-Post even if you have more available. This has implications if, for example, you want to run a long animation in CFD-Post and use CFX-Pre at the same time. If you know you are going to be working with CFX-Pre and CFD-Post at the same time, you need to change the license-sharing setting before starting your project.