### 2.2.3. MultiField Tab

The MultiField tab is used for launching ANSYS Multi-field runs and only appears if the specified CFX-Solver input file has External Solver Coupling set to `ANSYS MultiField` or `ANSYS Multifield via Prep7`. When this setting is enabled, the CFX-Solver Manager can be used to launch a complete ANSYS Multi-field run, including processing the multi-field commands (where appropriate) and launching CFX and ANSYS solvers. For details, see Preprocessing in the CFX-Solver Modeling Guide. A description of the different run modes and settings can be found in ANSYS Multi-field Run in the CFX-Solver Manager User's Guide.

The following table outlines various settings available on MultiField tab. The settings are marked as required or optional based on the MFX run mode chosen for the ANSYS Multi-field run.

Settings for MultiField Tab | MFX Run Mode [a]
--- | ---
Start ANSYS and CFX (default) | Start ANSYS only | Start CFX only [b] | Process Input File only
Input File | Mechanical application input file [c] | Required | Required |  | Required
Process ANSYS Input File [d] | Optional | Optional |  |
Restart ANSYS Run [e] Previous Run DB | Optional | Optional |  | Optional
MultiField Solver Settings [f] ANSYS Install Directory | Required | Required |  |
MultiField Remote Solver Settings Host Name Host Port |  |  | Required |

[a] The default setting for MFX Run Mode is `Start ANSYS and CFX` that launches the complete MFX run, including starting the ANSYS Solver. The other modes enable you to start just one or other solver, or to process the multi-field commands only using the specified ANSYS Input File. The latter option is available only if the specified CFX-Solver input file has External Solver Coupling set to `ANSYS MultiField`.

[b] Start CFX only: If the MFX Run Mode setting is `Start CFX only`, then no further ANSYS settings are required. However, when the CFX-Solver is started, it needs to know how to communicate with the ANSYS Solver that must have already been started elsewhere (that is, on another machine), and so Host Name and Host Port must be provided. The host name is the machine on which the ANSYS Solver was started. The host port number is determined by the ANSYS Solver when it starts, and can be read from the file `<jobname>.port` in the ANSYS working directory once the ANSYS Solver has started.

[c] Mechanical Input File: For all MFX run modes other than `Start CFX only`, the ANSYS input file must be provided. This will be read from the CFX-Solver input file specified on the Run Definition tab; however, you may choose to change this if the file is now in a different location, or if you want to use a different input file.

[d] Process ANSYS Input File: For the MFX run modes that will start the ANSYS Solver (`Start ANSYS and CFX` and `Start ANSYS only`), it is necessary to select Process ANSYS Input File if the specified ANSYS input file does not already contain the multi-field set-up (the MF commands required for the run), and if you want the multi-field set-up to be read from the CFX-Solver input file. This option will not be available if the specified CFX-Solver input file has External Solver Coupling set to `ANSYS MultiField via Prep7`, as in this case the CFX-Solver input file will not contain any multi-field set-up. For details, see Processing the ANSYS Input File in the CFX-Solver Manager User's Guide.

[e] Restart ANSYS Run: If the run is a restart from a previous ANSYS Multi-field run, then you need to select Restart ANSYS Run and supply the name of the database (`*.db` or `*.rdb`) from the previous run. This is not necessary if you are starting the CFX part of the ANSYS Multi-field run from an existing results file (for example, to provide initial conditions).

[f] MultiField Solver Settings: If the ANSYS Solver is to be started, you will need to specify the following settings:

- ANSYS Install Directory: On UNIX systems, you may need to manually specify where the ANSYS installation is if it is not in the default location. In this case, you must provide the path to the `v182/ansys` directory.

- Additional Arguments: You can use this setting if you want to pass the ANSYS Solver additional arguments. Whatever you specify here will be added to the command that starts the ANSYS Solver.

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