## 12.2. Command-Line Options and Keywords for cfx5solve

The command-line options for `cfx5solve` are described below. To see command-line help, from a CFX command line run:

    cfx5solve -help | more

Note: When running the solver from the command line using a CFX-Solver input file or CFX-Solver results file, any execution control CCL contained in the file takes precedence over the command-line options.

If an option is specified multiple times within the context of a specific configuration, then the last specification of the option takes precedence.

Command-Line Options | Alternative form | Usage
--- | --- | ---

`-affinity <option>`

Applying process affinity restricts execution of a solver process to a processing element (for example, a CPU core) so that the process is not free to migrate between processing elements. This can improve performance by increasing the use of cached data. MPI implementations are usually able to apply process affinity; this is typically enabled by default, although the behavior may vary depending on the hardware and operating system configuration.

The CFX-Solver accepts the following values for `<option>` to control process affinity:

`implicit`: This is the default option. Affinity settings are not changed by the solver. Any pre-existing affinity settings (for example, from an MPI implementation) are used unchanged. Note that processes are not necessarily free to migrate to any processing element because a preexisting affinity setting may prevent this.

`explicit`: The solver applies process affinity to its processes at runtime; any pre-existing affinity setting is superseded by the solver’s own affinity setting. A summary is shown in the solver output file giving the topology of each host and the result of the attempt to apply process affinity. If there are fewer solver processes than processing elements (that is, the hosts are not fully loaded), the solver attempts to distribute the processes as uniformly as possible among the processing elements.

Note that Windows HPC systems may report the host topology as being unavailable; this is expected. In this case, the job scheduling system usually sets the process affinity, hence setting the affinity in the solver is unnecessary.

In all cases, the solver checks if any other CFX-Solver processes are running on the hosts used. If other running processes are detected, affinity is not applied by the solver in order to avoid overloading a given processing element, which can strongly degrade performance.

`-ansys-arguments <arguments>` |  | For an ANSYS Multi-field run, enables you to specify any additional options when starting the Mechanical application solver. The specified options are passed to the Mechanical application solver as command-line arguments. For details, see MultiField Tab.
`-ansys-input <file>` |  | For an ANSYS Multi-field run, specifies the Mechanical application input file to use. For details, see MultiField Tab.
`-ansys-input-is-complete` |  | For an ANSYS Multi-field run, this turns off the Processing Mechanical input file option. For details, see MultiField Tab.
`-ansys-installation <directory>` |  | For an ANSYS Multi-field run, sets the ANSYS installation directory. This option is needed only if ANSYS is installed in a non-standard location. For details, see MultiField Tab.
`-ansys-jobname <name>` |  | For an ANSYS Multi-field run, sets the jobname for the Mechanical application component of the simulation. The CFX-Solver Manager defaults this to `ANSYS`. On a restart, the jobname must be the same as for an initial run.
`-ansys-license <licensekey>` |  | For an ANSYS Multi-field run, sets the license that the Mechanical application solver should use.
`-ansys-restart <file>` |  | For an ANSYS Multi-field run, tells CFX that the Mechanical application component of the simulation is a restart, and gives the database (*.db or *.rdb) from the previous Mechanical application run to be used for the restart. For details, see MultiField Tab.
`-bak-elapsed-time <elapsed time frequency>` | `-baket <elapsed time frequency>` | Causes the flow solver to write a backup file every <`elapsed time frequency`> hours, minutes, seconds, et cetera. Elapsed time must be in quotes and have units in square brackets. For example: `-baket “10 [min]”` or `-baket “5 [hr]”`.
`-batch` |  | Starts CFX-Solver in batch mode (that is, without starting the CFX-Solver Manager interface).
`-bg-ccl <file>` |  | Reads Command Language from the named file, and uses it to provide defaults for the current run. If the file specifies a CFX-Solver input file for the run, the command language contained in that CFX-Solver input file will take precedence over that supplied. Also see the `-ccl` option.
`-ccl <file>` |  | Reads additional Command Language from the named file. Overrides most CFX Command Language specified in the CFX-Solver input file. If `<file>` is the single character '`-`', the Command Language is read from the standard input (usually the terminal). If any settings are made in the Command Language file that also occur on the command line to the left of the `-ccl` option, the settings in the file will take precedence, as stated above. This option may be repeated to include Command Language from more than one file.[a]
`-ccl2flow <executable>` |  | Starts <executable> instead of the standard ANSYS CFX `ccl2flow`.
`-cclsetup <executable>` |  | Starts <executable> instead of the standard ANSYS CFX `cclsetup`.
`-chdir <directory>` |  | Sets the working directory as specified.
`-check-only` |  | When running in batch mode, this will cause `cfx5solve` to verify its options, but exit before starting any processes, and is mostly for use by CFX-Solver Manager.
`-config <configuration name>` |  | Applies subsequent options to the specified configuration.
`-continue-from-file <file>` | `-cont-from-file <file>` | Uses initial values and continues the run from the specified CFX-Solver results file. The mesh from the CFX-Solver input file is used unless the `-use-mesh-from-iv` option is also specified. Only one -continue-from-file argument can be supplied. See Continuing the History in the CFX-Solver Modeling Guide for more details.
`-continue-from-configuration <configuration name>` | `-cont-from-config <configuration name>` | Uses initial values and continues the run from the most recent results for the named configuration. The mesh from the configuration (.cfg) file is used unless the `-use-mesh-from-iv` option is also specified. Only one -continue-from-configuration argument can be supplied. See Continuing the History in the CFX-Solver Modeling Guide for more details.
`-cplg-host <port@host>` |  | For an ANSYS Multi-field run, specifies to the CFX-Solver which Port Number and Host Name to use to communicate with the Mechanical application solver. For details, see MultiField Tab.
`-definition <file>` | `-def <file>` | Uses `<file>` as the solver input file for a single configuration simulation. This may be a CFX-Solver input file or a CFX-Solver results file for a restart. The file specified is used in the same way as the input file on the Define Run dialog box. For details, see Define Run Command. Also see the `-mdef` option.
`-display <display>` |  | (UNIX only) Uses the X11 server `<display>` instead of the X11 server defined by the DISPLAY environment variable.
`-double` |  | Starts the double-precision version of ANSYS CFX Partitioner, Interpolator and Solver. Also see the `-single` option.
`-example <file>` | `-eg <file>` | Starts the CFX-Solver using one of the example CFX-Solver input files provided with the product. The example `StaticMixer` is currently available.
`-fullname <name>` |  | Specifies the basename for the CFX-Solver output file, CFX-Solver results file, and the temporary directory based on <name> instead of the CFX-Solver input file name. No numerical suffix (such as `_001`) is added to the specified name.
`-help` | `-h` | Displays the help information for command-line options.
`-initial <file>` | `-ini <file>` | Uses the initial values in the CFX-Solver results file `<file>`. The mesh from this results file is used unless the `-interpolate-iv` option is also specified. This option has been deprecated and should be replaced by `-initial-file` or `-continue-from-file` as appropriate.
`-initial-configuration <configuration name>` | `-ini-conf <configuration name>` | Uses initial values from the most recent results for the named configuration as a basic initial guess for the run. The run history from this file is discarded. The mesh from this results file is used unless the `-interpolate-iv` option is also specified. See Continuing the History in the CFX-Solver Modeling Guide for more details.
`-initial-file <file>` | `-ini-file <file>` | Uses initial values from the specified CFX-Solver Results file as a basic initial guess for the run. The run history from this file is discarded. The mesh from the configuration (.cfg) file or the CFX-Solver input file is used unless the `-use-mesh-from-iv` option is also specified. See Continuing the History in the CFX-Solver Modeling Guide for more details.
`-interactive` | `-int` `-manager` | Starts CFX-Solver Manager in graphic user interface (GUI) mode. The CFX-Solver Manager interface enables starting a new run or managing or monitoring an existing run.
`-interpolate-iv` | `-interp-iv` | Interpolates the solution from the initial values file, if one is supplied (using the `-initial` option), onto the mesh from the CFX-Solver input file, rather than using the mesh from the initial values file. This option has been deprecated and should be replaced by the `-initial-file` or `-continue-from-file` option, as appropriate.
`-interp-double` |  | When running with the solver-based interpolator (`-interp-iv` option), this option will select the double-precision version of the interpolator. It will not override the `-interpolator` option if both are used.
`-interp-single` |  | Uses the single precision ANSYS CFX Interpolator executable.
`-interp-large` |  | Uses the large problem ANSYS CFX Interpolator executable.
`-interpolator <executable>` |  | When running with the interpolator (`-interp-iv` option), this option will start `<executable>` instead of the default interpolator.
`-job` |  | Keeps the .job file after an ANSYS CFX Solver run. This file contains a brief summary of various solution values, and is most useful for regression purposes.
`-job-part` | `-jobp` | Keeps job file after an ANSYS CFX Partitioner run. This file contains a brief summary of various solution values, and is most useful for regression purposes.
`-large` |  | Default to the large problem version of the ANSYS CFX Partitioner, Interpolator and Solver.
`-max-elapsed-time <elapsed time>` | `-maxet <elapsed time>` | Sets the maximum elapsed time (wall clock time) that CFX-Solver will run. Elapsed time must be in quotes and have correct units in square brackets. For example: `-maxet “10 [min]”` or `-maxet “5 [hr]”`.
`-mdefinition <file>` | `-mdef <file>` | Uses `<file>` as the solver input file. This may be a multi-configuration definition file or results file for a restart (that is, .mdef or .mres, respectively). The file specified is used in the same way as the input file on the Define Run dialog box. For details, see Define Run Command.

`-mfx-run-mode <mode>`

Use this option to specify one of the following MFX run modes for an ANSYS Multi-field run:

`"Start ANSYS and CFX"`

`"Start ANSYS only"`

`"Start CFX only"`

`"Process Input File only"`

For details, see MultiField Tab.

`-monitor <file>` |  | When starting ANSYS CFX-Solver Manager, use this option to monitor the run represented by `<file>`, which may be a CFX-Solver results file or CFX-Solver output file.
`-multiconfig` |  | Treats the CFX-Solver input file as a multi-configuration input file.
`-name <name>` |  | Specifies the basename for exported files and the temporary directory based on the problem name `<name>` instead of the CFX-Solver input file name, unless other names are explicitly defined. This name cannot be set when using the CFX-Solver Manager to start the CFX-Solver.
`-norun` |  | Use this option to preprocess the CFX-Solver input file only, without running the CFX-Solver executable. When used with a multi-configuration CFX-Solver input file, this option produces complete solver input files for the individual configuration (.cfg) files. When used with the "`-config`" option, only the specified configuration is preprocessed.

`-numa <option>`

Non-Uniform Memory Access (NUMA) is a hardware feature that associates regions of memory with specific groups of CPU cores. Although all memory is generally accessible from any CPU core, the fastest access is to local memory.

NUMA memory containment can improve performance by restricting memory access for a solver process to its local memory.

If a solver process requires more memory than a single NUMA node can provide, NUMA containment can cause a failure because memory outside the local NUMA node is inaccessible. Parallel runs using relatively few CPU cores, having memory requirements close to the system limit, or widely differing between partitions, may be susceptible to this problem. NUMA memory containment is disabled by default and is not available for the partitioner or interpolator because these run as serial processes that often have a high memory requirement. Failures of this type are likely to be abrupt; as in the event of an ‘out of memory’ condition, the operating system terminates the offending process. Therefore if NUMA containment has been enabled and the solver fails without giving any diagnostics, a repeat run without NUMA containment should be considered.

`<option>` can be set to:

`none`: (default)

`auto`

`-output-summary-option <option>` |  | Use this option to specify the job summary format in the CFX-Solver output file. `<option>` may be set to: 0: minimal 1: terse format (default, no information per partition) 2: compact format (one line per partition) 3: verbose format (the default prior to ANSYS CFX Release 15.0)

`-par-dist <host-list>`

Use this option to set the comma-separated `<host-list>` in the same form as is used in the Command Language definition. This option does not require the `-partition` option, as one partition is run on each host mentioned in the list. To run multiple partitions on the same host, it may be listed multiple times, or an asterisk may be used with the count, as in `"wallaby*3,kangaroo*4"` for a 7-partition run.

Host details are taken from the hostinfo.ccl file, if they are there; otherwise, if possible, the required information will be automatically detected. `<host>` may be specified as `[<user>@]<hostname>[:<CFX_ROOT>]`, if the user name or the ANSYS CFX installation root directory differs from the local host.

`-par-host-list <host1> [,<host2> [,...]]` |  | When running in parallel, uses the specified host list. See the `-par-dist` option for details of the host list. This option defaults to Intel MPI Local Parallel on UNIX/Linux platforms and Windows.
`-par-local` |  | When running in parallel, uses only the local host. This will override the `-par-dist` or `-par-host-list` options.
`-parallel` | `-par` | Starts the solver in parallel mode. This option can be combined with `-partition` for a partitioning run. If the `-part` option is not specified, then the `-parfile-read` option must be used to specify a valid partitioning information file.
`-parfile-read <parfile>` |  | Specifies the name of an input partition file used to set up a partitioning or parallel run. Note: Only *.par files that are generated in ANSYS CFX 12.0 (or later) are supported. For details, see CFX Partition File.
`-parfile-save` |  | When used with a parallel run, saves the partitioning information to a file with the same basename as the results file, and the extension .par.
`-parfile-write <parfile>` |  | Specifies the name of a partition file to which to write the information from a partitioning run.
`-partition <number of partitions>` | `-part <number of partitions>` | Starts the solver in partitioning mode. This option should not be used if an existing partition file is also specified.
`-partitioner <executable>` |  | Starts `<executable>` instead of the standard partitioner.
`-part-coupled` |  | Activates coupled partitioning mode for multidomain problems. This is not activated by default.
`-part-independent` |  | Activates independent partitioning mode for multidomain problems. This is the default.
`-part-large` |  | Starts the large problem partitioner, which can partition problems up to 2^31-1 elements. This partitioner uses 64-bit integer and logical variables so it will allocate more memory than the default partitioning executable.

`-part-mode <mode>`

Sets the partitioning mode to use when running the partitioner. Valid options are `metis-kway` (MeTiS k-way), `metis-rec` (MeTiS Recursive Bisection), `simple` (Simple Assignment), `drcb` (Directional Recursive Coordinate Bisection), `orcb` (Optimized Recursive Coordinate Bisection), `rcb` (Recursive Coordinate Bisection)

Finer control over the partitioning method is available through the Command Language.

`-part-only <number of partitions>` |  | Starts the solver in partitioning mode only. This is normally equivalent to `-part`, but may be necessary if partitioning a results file from a previous run.
`-part-single` |  | Uses the single precision ANSYS CFX Partitioner. This is the default, but is provided for overriding any information that might be stored in the CFX Command Language dataset in a file from previous runs. Also see the `-double` option.
`-preferred-license <license name>` | `-P <license name>` | Sets the first license used by solver, given the availability of multiple usable licenses.
`-priority <level>` | `-pri <level>` | Enables the specification of a job priority to a solver run; the allowed values are `Idle` (`0`), `Low` (`1`), `Standard` (`2`), and `High` (`3`). The default value is `Standard`, which corresponds to a nice increment of 0 on UNIX platforms or a priority level of Normal on Windows platforms. Note that on UNIX platforms, Standard and High job priorities both yield a nice increment of 0.
`-respect-suffix-history` |  | In addition to the files in the working directory, this option also considers results files referenced by initial values files when choosing the numerical suffix (such as _001) added to the run name.
`-save` |  | Use this option to avoid deleting any temporary files after the run. Normally the standard temporary files created by CFX-Solver are deleted automatically after each run.
`-scid` value |  | Specifies the licensing ID of the System Coupling analysis. CFX System Coupling is described in Coupling CFX to an External Solver: System Coupling Simulations in the CFX-Solver Modeling Guide.
`-sclic` port`@`host |  | Specifies the licensing port@host to use for the System Coupling analysis. CFX System Coupling is described in Coupling CFX to an External Solver: System Coupling Simulations in the CFX-Solver Modeling Guide.
`-serial` |  | Use this option to explicitly specify that a serial run is required. This is useful when restarting a run from a results file produced by a parallel run, where this option forces a serial run instead.
`-single` |  | Starts the single-precision version of the CFX-Solver, Partitioner, and Interpolator. This is the default, but is provided for overriding any information that might be stored in the CFX Command Language dataset in a file from a previous run. Also see the `-double` option.

`-size <factor>`

`-S <factor>`

`-s <factor>`

Changes memory estimates used by the CFX-Solver by a factor of `<factor>`. Memory estimates are sometimes inaccurate and this option must to be used to increase the memory allocated. For example, using `-size 1.05` increases memory allocated by 5%. This option provides the same functionality as set in Solver Memory. For details, see Solver Tab.

Further options for controlling the CFX-Solver memory allocation are available. Execute `cfx5solve -help` for full details.

`-size-cat <size>`

`-size-nr <size>`

`-size-ni <size>`

`-size-nd <size>`

`-size-nc <size>`

`-size-nl <size>`

`-scat <size>`

`-nr <size>`

`-ni <size>`

`-nd <size>`

`-nc <size>`

`-nl <size>`

These flags are for advanced users to change the memory allocation parameters for the solver. Usually, you should use the `-size` option instead. `<size>` is the desired memory allocation in words, and may have K or M appended for kilo or mega. If the suffix is 'x', then the number is treated as a multiplier.

`-size-cclsetup <factor>` | `-sizeccl <factor>` | Changes the memory estimates used by the ANSYS CFX cclsetup executable by a factor of <factor>.

`-size-cclsetup-cat <size>`

`-size-cclsetup-nr <size>`

`-size-cclsetup-ni <size>`

`-size-cclsetup-nd <size>`

`-size-cclsetup-nc <size>`

`-size-cclsetup-nl <size>`

`-scatccl <size>`

`-nrccl <size>`

`-niccl <size>`

`-ndccl <size>`

`-ncccl <size>`

`-nlccl <size>`

These options are the same as the `-size-*` options above, but provide sizes needed for the ANSYS CFX CCL Setup executable.

`-size-interp <factor>` | `-sizeint <factor>` | Changes the memory estimates used by the solver-based interpolator by a factor of `<factor>`. Also see the `-size` option.

`-size-interp-cat <size>`

`-size-interp-nr <size>`

`-size-interp-ni <size>`

`-size-interp-nd <size>`

`-size-interp-nc <size>`

`-size-interp-nl <size>`

`-scatint <size>`

`-nrint <size>`

`-niint <size>`

`-ndint <size>`

`-ncint <size>`

`-nlint <size>`

These options are the same as the `-size-*` options above, but provide sizes needed for the ANSYS CFX Interpolator.

`-size-mms <factor>` | `-smms <factor>` | Changes the initial MMS catalogue size estimate used by the CFX-Solver by a factor of `<factor>`. This option has been deprecated and should be replaced by `-size-cat`.
`-size-part-mms <factor>` | `-smmspar <factor>` | Changes the initial MMS catalogue size estimate used by the partitioner by a factor of `<factor>`. This option has been deprecated and should be replaced by `-size-part-cat`.
`-size-part <factor>` `-size-par <factor>` | `-sizepart <factor>` `-sizepar <factor>` | Changes the memory estimates used by the ANSYS CFX Partitioner by a factor of `<factor>`. Also see the `-size` option. Further options for controlling the partitioner memory allocation are available. Execute `cfx5solve -help` for full details.

`-size-part-cat <size>`

`-size-part-nr <size>`

`-size-part-ni <size>`

`-size-part-nd <size>`

`-size-part-nc <size>`

`-size-part-nl <size>`

`-scatpar <size>`

`-nrpar <size>`

`-nipar <size>`

`-ndpar <size>`

`-ncpar <size>`

`-nlpar <size>`

These options are the same as the `-size-*` options, but provide sizes needed for `partitioner` rather than `solver`.

`-solver [<os>=]<executable>, <os>=<executable>[...]]`

`-exec [<os>=]<executable> [,<os>=<executable>[, ...]]`

Starts `<executable>` instead of the standard ANSYS CFX solver on `<os>`, where `<os>` is the short architecture string for the desired operating system. If `<os>` is omitted, then the current operating system is assumed.

For example: the command-line option `-solver "linux-amd64/mysolver.exe,linux=linux/mysolver.exe"` uses the executable "linux-amd64/mysolver.exe" for the current operating system and the executable "linux/mysolver.exe" for the "linux" operating system. Full paths or paths relative to the working directory may be used when specifying solver executables. In this example, it is worth noting that the current operating system is presumed to be "linux-amd64", and that the "linux-amd64/mysolver.exe" and "linux/mysolver.exe" will be used for all solvers running on "linux-amd64" and "linux" operating systems, respectively.

The string value for `<os>` can be determined by running the following command:

- On Unix-like systems, execute `<CFXROOT>/bin/cfx5info -os`.

- On a Windows system, execute `<CFXROOT>\bin\cfx5info -os`.

where `<CFXROOT>` is the path to your installation of ANSYS CFX.

`-solver-double` |  | Uses the double precision ANSYS CFX Solver.
`-solver-single` |  | Uses the single precision ANSYS CFX Solver.
`-solver-large` |  | Uses the large problem ANSYS CFX Solver.
`-start-method <name>` |  | Uses the named start method to start the solver. This option enables you to use different parallel methods, as listed in the CFX-Solver Manager user interface, instead of the defaults. For parallel runs, you also need to provide the `-part` or `-par-dist` options.
`-use-mesh-from-iv` |  | Uses the mesh from the source initial values (that is, from a file or configuration) rather than from the solver input file. This is only valid if a single initial-values source is specified.
`-verbose` | `-v` | Specifying this option may result in additional output being sent to the standard output file (normally the screen).
[a] Changes that affect the way that the mesh is defined, or that affect the way that the physics CCL relates to the topology of the mesh that is stored in the solver input file, cannot be made using the `-ccl` argument. For example, locators for applying physics cannot be modified using the `-ccl` option. Such changes can, however, be made in CFX-Pre. For details, see Solver Tab.

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