The value of this option specifies the name of all files generated during the run and the name of files that are read in the continue, convert, and recover phases.

If this option is omitted from the command line, you will be prompted for its value (except when only the informational options described in “Obtaining information,” Section 3.2.1, are used). If the input option is not supplied, the procedure will look for an input file called job-name.inp in the current directory.

This option indicates that a complete Abaqus analysis (or a restart of an Abaqus analysis) is to be performed.

This option indicates that the run is for data checking only. No analysis will be performed. If this option is used, all files necessary to continue the analysis are saved.

This option indicates that the run is for input parameter checking only (parameter definitions must have been used; see “Parametric input,” Section 1.4.1). No analysis or data checking will be performed. This option is not applicable for Abaqus/CFD.

This option indicates that the run is to begin at the point at which a previous data check run ended.

The value of this parameter indicates which files will be postprocessed. This option is not applicable for Abaqus/CFD.

Results can be converted either immediately following an analysis run, as a separate run subsequent to an analysis run, or while an analysis is running as follows:

If convert=select, the Abaqus/Explicit selected results file (job-name.sel) will be converted into a standard Abaqus results file (job-name.fil). If the analysis is run in parallel with parallel=domain, the separate selected results files (job-name.sel.n) will be converted into a single selected results file (job-name.sel) prior to being converted into a standard Abaqus results file.

If convert=odb, the output database (job-name.odb) will be converted using the postprocessing calculator (see “The postprocessing calculator,” Section 4.3.1). This conversion is necessary only if the types of output listed in “The postprocessing calculator,” Section 4.3.1, are requested.

If convert=state, the separate Abaqus/Explicit state files (job-name.abq.n) will be converted into a single Abaqus/Explicit state file (job-name.abq) if the analysis is run in parallel with parallel=domain.

If convert=all, all of the applicable convert options will be executed.

This option applies only to Abaqus/Explicit. It indicates that an analysis is to be restarted at the last available step and increment in the state file. This capability is available to restart after a catastrophic failure, such as exceeding a CPU limit or a disk quota (see “Restarting an analysis,” Section 9.1.1). If the original analysis was run in parallel with parallel=domain, it must be restarted with parallel=domain and the same number of processors.

This option indicates that the run is for checking the syntax of the input file only. This option does not use any license tokens. No analysis will be performed, and the continue option cannot be used to continue with an analysis. Only the data (.dat) and output database (.odb) files are generated for viewing. In an Abaqus/Explicit analysis, the model data in the output database may not be complete.

This option writes information about the installation and the environment that is in effect to the screen or to the file job-name.log. For output information for each value of this option, see “Obtaining information,” Section 3.2.1. If the information option is used in conjunction with the analysis option, the job must be run in the background to write the information text to the log file.

This option is used to specify the input file name, which may be given with or without the .inp extension (if the extension is not supplied, Abaqus will append it automatically). If this option is not supplied, the procedure will look for an input file called job-name.inp in the current directory. If job-name.inp cannot be found, the procedure will prompt for the input file name.

This option specifies the name of a source or object file that contains any user subroutines to be used in the analysis. The name of the user routine may contain a path name and may be given with or without a file extension. Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD accept user subroutines written in C, C++, or Fortran.

If an extension is given, the program will take the appropriate action based on the file type. If the file name has no extension, the program will search for a C, C++, or Fortran source file. If the source file does not exist, an object file will be searched for instead. The execution procedure creates a shared library using the user subroutine file that is used by the analysis during execution.

If the same user subroutine will be needed often, consider setting the usub_lib_dir environment file parameter and using the abaqus make execution procedure to create a shared library containing the user subroutine. This will avoid the need to recompile and/or relink the user subroutine each time it is needed. The user option is not required if the user subroutine called by the analysis is contained in the user library. User libraries contained in the directory given by the usub_lib_dir environment file parameter will not be used if the user option is specified.

The user option cannot be used to specify an object file when the double option is used to run an Abaqus/Explicit analysis because Abaqus/Explicit double precision runs need both single precision and double precision objects. In this case you must set the usub_lib_dir environment file parameter and place the single and double precision object files in the specified directory; alternatively, you can supply the user subroutine source.

This option specifies the name of the files from a previous run from which a restart or postprocessing (Abaqus/Standard only; see “Recovering additional results output from restart data in Abaqus/Standard” in “Output,” Section 4.1.1) run is to be started or from which results are to be imported. A path or file extension is not allowed. This option is required when a restart, postprocessing, symmetric model generation, or import analysis reads data from the restart or the results file. The oldjob-name must be different from the current job-name.

This option specifies whether the data from the old results file specified in a restart run are included at the beginning of the new results file (default). If fil=new is used, the new results file will contain only the data from the point in the analysis where the restart occurred. This feature is used for Abaqus/Standard runs to join the output from restarted analyses into a single, continuous results file. Non-restart jobs cannot use this feature to append results file output to an old results file; the abaqus append execution procedure must be used for this purpose. Setting fil=new is not allowed for Abaqus/Explicit runs. This option is not applicable for Abaqus/CFD.

This option specifies the name of the global model's results file, ODB output database file, or SIM database file from which the results are to be interpolated to drive a submodel analysis. This option is required whenever a submodel analysis or submodel boundary condition reads data from the global model's results.

The file extension is optional. If you omit the file extension, Abaqus uses the results file. If the results file does not exist, Abaqus uses the ODB output database file. If both the results file and the ODB output database file do not exist, Abaqus uses the SIM database file.

This option is not applicable for Abaqus/CFD.

This option specifies the number of processors to use during an analysis run if parallel processing is available. The default value for this parameter is 1 and can be changed in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1).

This option specifies the method to use for thread-based parallel processing in Abaqus/Explicit. The possible values are domain and loop. If parallel=domain, the domain-level method is used to break the model into geometric domains. If parallel=loop, the loop-level method is used to parallelize low-level loops. See “Parallel execution in Abaqus/Explicit,” Section 3.5.3, for more information on these methods. The default value is domain, which can be changed in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1).

This option specifies the number of parallel domains in Abaqus/Explicit. If the value is greater than 1, the domain decomposition will be performed regardless of the values of the parallel and cpus options. However, if parallel=domain, the value of cpus must be evenly divisible into the value of domains. The default value is set equal to the number of processors used during the analysis run if parallel=domain and 1 if parallel=loop. The default value can be changed in the environment file (see“Using the Abaqus environment settings,” Section 3.3.1). A restart analysis uses the same number of parallel domains as the original analysis, and the value specified with this option will be ignored.

For domain-parallel execution in Abaqus/Explicit (parallel=domain) where the number of domains is larger than the number of cpus, this option activates the dynamic load balancing scheme. Abaqus/Explicit will attempt to improve computational efficiency by periodically reassigning domains to processors in a way that minimizes load imbalance (see “Parallel execution in Abaqus/Explicit,” Section 3.5.3).

If this option is set equal to mpi, the MPI-based parallelization method will be used when applicable. Set mp_mode=threads to use the thread-based parallelization method. The default value is mpi on Windows platforms if MPI components are installed; otherwise, thread-based parallel execution is the default behavior. On all other platforms, the default value is mpi. The default setting can be changed in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1). For Abaqus/CFD only mp_mode=mpi can be used.

This option specifies the parallel execution mode in Abaqus/Standard. The possible values are all and solver. If standard_parallel=all, both the element operations and the solver will run in parallel. If standard_parallel=solver, only the solver will run in parallel. The default value is standard_parallel=all on platforms where MPI-based parallelization is supported.

The parallel execution mode can also be set in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1).

This option specifies acceleration of the Abaqus/Standard direct solver. This option is meaningful only on computers equipped with appropriate GPGPU hardware. By default, GPGPU solver acceleration is not activated. The value of this parameter is the number of GPGPUs to be used in an Abaqus/Standard analysis. In an MPI-based analysis, this is the number of GPGPUs to be used on each host.

GPGPU-based solver acceleration can also be set in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1).

Maximum amount of memory or maximum percentage of the physical memory that can be allocated during the input file preprocessing and during the Abaqus/Standard analysis phase (see “Managing memory and disk use in Abaqus,” Section 3.4.1). The default values can be changed in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1). This option is not applicable for Abaqus/CFD.

This option will cause the job to run interactively. For Abaqus/Standard and Abaqus/CFD the log file will be output to the screen; for Abaqus/Explicit the status file and the log file will be output to the screen. The default run_mode can be set in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1).

This option will submit the job to run in the background, which is the default. Log file output will be saved in the file job-name.log in the current directory. The default method for submitting the job can be set in the environment file by using the run_mode parameter (see “Using the Abaqus environment settings,” Section 3.3.1).

This option will submit the job to a batch queue. If the option appears with no value, the job will be submitted to the system default queue. Quoted strings are allowed. The available queues are site specific. Contact your site administrator to find out more about local queuing capabilities. Use information=local to see what local queuing capabilities have been installed. The default method for submitting the job can be set in the environment file by using the run_mode parameter (see “Using the Abaqus environment settings,” Section 3.3.1).

This option is used in conjunction with the queue option to specify the time at which the job will start in the selected batch queue. This capability is supported for each individual site through the Abaqus environment file. (See the Abaqus Installation and Licensing Guide for details.)

This option is used to specify that the double precision executable is to be used for Abaqus/Explicit. The possible values are both, constraint, explicit, and off. This capability is also supported through the Abaqus environment file with the environment variable double_precision (see “Using the Abaqus environment settings,” Section 3.3.1).

If double=both, both the Abaqus/Explicit packager and analysis will run in double precision.

If double=constraint, the constraint packaging and constraint solver in Abaqus/Explicit will run in double precision, while the Abaqus/Explicit packager and Abaqus/Explicit analysis continue to run in single precision.

If double=explicit, the Abaqus/Explicit analysis will run in double precision, while the packager will still run in single precision. The default value is explicit.

If double=off, the environment file setting is overridden if necessary to invoke both the Abaqus/Explicit packager and Abaqus/Explicit analysis in single precision. For a discussion of when to use the double precision executable, see “Defining an analysis,” Section 6.1.2.

This option is used to specify the name of the directory used for scratch files. On Linux platforms the default value is the value of the $TMPDIR environment variable or /tmp if $TMPDIR is not defined. On Windows platforms the default value is the value of the %TEMP% environment variable or \TEMP if this variable is not defined. During the analysis a subdirectory will be created under this directory to hold the analysis scratch files. The default value for this parameter can be set in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1).

This option specifies the precision of the nodal field output written to the output database file (job-name.odb). Using output_precision=full results in double precision field output for Abaqus/Standard analyses. To obtain double precision field output for Abaqus/Explicit analyses, use the double option in addition to using output_precision=full. Nodal history output is available only in single precision. This option cannot be used with the recover option.

This option specifies the output format of the results. If resultsformat=odb, the output is written in ODB format only. If resultsformat=sim, the output is written in SIM format only. If resultsformat=both, the output is written in both ODB and SIM formats. The default value is odb. For more information, see “The output database” in “Output,” Section 4.1.1. This option is not applicable for Abaqus/CFD.

This option specifies the format of field output for Abaqus/CFD. If field=odb, field output is written in ODB format. If field=sim, field output is written in SIM format. The default value is odb. For more information, see “Alternate output formats in Abaqus/CFD” in “Output,” Section 4.1.1.

This option specifies the format of history output for Abaqus/CFD. If history=odb, history output is written in ODB format. If history=sim, history output is written in SIM format. If history=csv, history output is written to a file in comma-separated values format.

The default value depends on the setting for the field option. When field=odb, the default is history=odb. When field=sim, the default is history=sim. For more information, see “Alternate output formats in Abaqus/CFD” in “Output,” Section 4.1.1.

This option is used to specify the TCP/UDP port number for co-simulation between solvers using the direct coupling interface, which includes co-simulation between Abaqus and certain third-party analysis programs. Set port equal to the port number used for the connection. The default value is 48000. The default port number that Abaqus uses to initiate communication can be set with the cosimulation_port parameter in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1). This option is used in conjunction with the host option. For more information, see “Selecting TCP/UDP port numbers” in “Execution procedure for Abaqus: overview,” Section 3.1.1.

This option is used to specify the host name for co-simulation between solvers using the direct coupling interface, which includes co-simulation between Abaqus and certain third-party analysis programs. This option specifies the name of the machine that is hosting the connection. Refer to the third-party program documentation to determine if the host option is required. This option is used in conjunction with the port option.

This option is used to specify the connection (e.g., host:port) for the SIMULIA Co-Simulation Engine director process when performing a co-simulation using the SIMULIA Co-Simulation Engine. The csedirector entry identifies the host name and the TCP/UDP port number for the listening port of the SIMULIA Co-Simulation Engine director process.

This option is used to specify a timeout value in seconds for establishing the co-simulation connection using the direct coupling interface or the SIMULIA Co-Simulation Engine. Abaqus terminates if it does not receive any communication from the coupled analysis program during the time specified. The default value is 3600 seconds. The default timeout value that Abaqus uses can be set with the cosimulation_timeout parameter in the environment file when using the direct coupling interface (see “Using the Abaqus environment settings,” Section 3.3.1).

This option is used to request that Abaqus/Standard create element and node sets for unconnected regions in the analysis output database. Set unconnected_regions=yes to create element and node sets that are named MESH COMPONENT N, where N is the component number.