### 2.6.6. Processing the ANSYS Input File

The processing of an ANSYS input file is a procedure that takes a solid physics setup in the form of an ANSYS input file and a multi-field setup from a CFX-Solver input file, and combines them into a new ANSYS input file that contains both the solid physics setup and the multi-field setup. The new ANSYS input file has a name of the form `jobname`.mf and can be used to start the ANSYS Solver as part of an ANSYS Multi-field run.

The following topics are discussed in this section:

- When the ANSYS Input File Needs Processing

- The Processing Step

#### 2.6.6.1. When the ANSYS Input File Needs Processing

The preprocessing steps for an ANSYS Multi-field run result in the fluid physics set-up (contained in a CFX-Solver input file), the solid physics set-up (contained in an ANSYS input file) and the ANSYS Multi-field settings (contained in either the CFX-Solver input file or the ANSYS input file). When the multi-field settings are only contained in the CFX-Solver input file, then the ANSYS input file must be processed before the run begins to create a new "multi-field" file with the extension `.mf`, which contains both the solid physics from the supplied ANSYS input file and the multi-field settings from the CFX-Solver input file, and this is then used as input for the ANSYS Solver, instead of the supplied ANSYS input file.

A CFX-Solver input file will contain multi-field settings if it was created in `ANSYS MultiField` mode, but not if it was created in `ANSYS MultiField via Prep7` mode.

An ANSYS input file will only contain multi-field settings if these were explicitly added (by hand or in the ANSYS Prep7 user interface); there will be no multi-field settings in an ANSYS input file created by Simulation. A "multi-field" file created from one run can be used as the ANSYS input file for another run, and this will contain multi-field settings.

#### 2.6.6.2. The Processing Step

When CFX-Pre writes a CFX-Solver input file in `ANSYS MultiField` mode, the CCL in the CFX-Solver input file contains various MFX settings, which are translated to commands for the ANSYS solver when the ANSYS input file is processed. This section contains a few notes on how the MFX settings in the CFX-Solver input file are converted to ANSYS commands.

- Every quantity set in a CFX-Solver input file has units; a timestep has a unit of time, most commonly seconds. For example, timesteps may appear in the CCL as `Timesteps = 0.1 [s]`. You can use any unit of the appropriate dimension to specify any physical quantity, and CFX handles the conversion to a consistent set of units (CFX Solution Units) as part of setting up the solver run. However, ANSYS commands appear without units (for example, `MFDT,0.1,0.1,0.1`) and it is assumed that you have entered the value in units that are consistent with the rest of the ANSYS set-up. When an MFX run is performed, it is a requirement that the units used for the ANSYS set-up match the CFX Solution Units. Therefore, when quantities with units in the CFX CCL are translated to ANSYS commands, the values used are always written in the CFX Solution Unit of the appropriate dimension. For example, if you specify a coupling time duration of `30.0 [s]`, and the CFX Solution Units of time are set to minutes, then the ANSYS command that corresponds to this CCL (MFTI) will be written with the value 0.5 in implicit units of minutes: `MFTI,0.5`.

- The CFX CCL records the name of an ANSYS Interface, not its number, where possible. For details, see Boundary Conditions in ANSYS Multi-field Mode in the CFX-Solver Modeling Guide. When the CFX-Solver input file is processed, this is automatically converted to the required interface number, as required by the MFLC command.

- The processing always adds a `KBC,1` command to the input file, as this is required for any multi-field case.

- The processing always adds the `/GST` command to ensure output for monitoring the run is available, and the `CMWRITE` command to ensure that any named selections or components in the ANSYS input file are available for CFD-Post to use. For details, see ANSYS Files in the CFD-Post User's Guide.

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