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 “Execution procedure for obtaining information,” Section 3.2.1, are used).

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 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.

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 the analysis is run in parallel with parallel=domain and multiple output file mode is set by setting parallel_odb=MULTIPLE in the environment file abaqus_v6.env, the separate output database files (job-name.odb.n) will be converted into a single output database file (job-name.odb) prior to conversion by the postprocessing calculator.

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.

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 “Execution procedure for 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 FORTRAN 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.

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.

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 specifies the name of the global model's results file or output 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 both a results file and an output database file exist for the global model and no extension is given, the results file will be used.

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 11.9.3, 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).

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 all platforms except Windows, which supports only thread-based parallel execution. The default setting on all other platforms can be changed in the environment file (see “Using the ABAQUS environment settings,” Section 3.3.1).

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 the maximum amount of memory that can be allocated by the analysis input file processor. The default is sufficient for most problems. If an analysis requires more memory than is currently in use by the analysis input file processor, it will issue an error message listing the current amount of memory in use. Incrementing the memory by 50% is the recommended approach to increasing memory. The default value for this parameter can be set with the pre_memory parameter in the environment file (see “Using the ABAQUS environment settings,” Section 3.3.1).

This option will cause the job to run interactively. For ABAQUS/Standard 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. This option is available only on machines where the default length of a single precision, floating point word is 32 bits. This option will run the executable for ABAQUS/Explicit that was built using double precision, floating point word lengths of 64 bits. This capability is also supported through the ABAQUS environment file with the environment variable explicit_precision (see “Using the ABAQUS environment settings,” Section 3.3.1). For a discussion of when to use the double precision executable, see “Procedures: overview,” Section 6.1.1.

This option is used to specify the name of the directory used for scratch files. On UNIX 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 output written to the output database file (job-name.odb). Using output_precision=full results in double precision output for ABAQUS/Standard analyses. To obtain double precision output for ABAQUS/Explicit analyses, use the double option in addition to using output_precision=full.

This option applies only to ABAQUS/Standard. It changes the default behavior for the handling of severe discontinuity iterations (see “Severe discontinuities in ABAQUS/Standard” in “Procedures: overview,” Section 6.1.1). The default behavior corresponds to convert_sdi=off, which forces a new iteration every time a severe discontinuity is encountered. Set convert_sdi=on to estimate residual forces associated with severe discontinuities. ABAQUS/Standard then checks whether the force equilibrium tolerances are satisfied to determine whether or not a new iteration is required. It is also possible to set this option on a step-by-step basis within an analysis. The value specified in the step overrides the value specified on the command line.

This option chooses between two internal ABAQUS/Standard algorithms that are associated with how the direct sparse solver accounts for changes in connectivity during an analysis. ABAQUS/Standard will choose a default setting that generally optimizes performance depending on characteristics of the model. Overriding the default setting may occasionally result in improved performance. You can directly choose between the algorithms by specifying active_topology=on or off. The default setting typically, but not always, corresponds to active_topology=on, in which case solver memory estimates and memory usage are based on the current list of nodal interactions rather than a conservative estimate of this list. ABAQUS/Standard requires one algorithm or the other for some models; if you specify the opposite algorithm in such cases, ABAQUS/Standard issues a warning message indicating which features cannot be used with the specified algorithm and the opposite algorithm is used. For more information, see “Efficiently accounting for changes in contact connectivity in the equation solver” in “Adjusting contact controls in ABAQUS/Standard,” Section 29.2.12.

This option is used to specify the MADYMO input file name for a co-simulation analysis that couples ABAQUS/Explicit and MADYMO. The MADYMO input file name must be given with the .saf extension. For more information, see “Running a co-simulation with MADYMO” in “Co-simulation with MADYMO,” Section 13.1.4.