Abaqus/Standard and Abaqus/Explicit execution

Abaqus/Standard and Abaqus/Explicit are executed by running the Abaqus execution procedure. Several parameters can be set either on the command line or in the environment file (see Environment File Settings). Alternatively, you can use the convenient Abaqus/CAE user interface to submit an Abaqus analysis from an input file and set the analysis parameters; see Understanding analysis jobs.

Abaqus enforces a character limit on file names. For any command line reference to a file, the total length of the file name, including the path description, cannot exceed 256 characters.

The following topics are discussed:

Related Topics
About Execution Procedures

ProductsAbaqus/StandardAbaqus/Explicit

Command summary

abaqus jobjob-name analysisdatacheckparametercheckcontinueconvert{selectodbstateall}recoversyntaxcheckinformation{environmentlocalmemoryreleasesupportsystemall} inputinput-file user{source-fileobject-file} oldjoboldjob-name fil{appendnew} globalmodel{results file-nameODB output database file-name SIM database file-name } cpusnumber-of-cpus parallel{domainloop} domainsnumber-of-domains dynamic_load_balancing mp_mode{mpithreads} standard_parallel{allsolver} gpusnumber-of-gpgpus memorymemory-size interactivebackgroundqueue queue-name aftertime double{explicitbothoffconstraint} scratchscratch-dir output_precision{singlefull} resultsformat{odbsimboth} portco-simulation port-number hostco-simulation hostname csedirectorCo-Simulation Engine director host:port-number timeoutco-simulation timeout value in seconds unconnected_regions{yesno}

Command line options

Required option

job

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 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.

Mutually exclusive options that determine which phases of an analysis are performed

All options are order independent. If none of these options is present, the analysis option is assumed. The convert option is an exception to the mutual exclusion rule: convert can appear with any option except datacheck, parametercheck, syntaxcheck, and information.

analysis

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

datacheck

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.

parametercheck

This option indicates that the run is for input parameter checking only (parameter definitions must have been used; see Parametric Modeling). No analysis or data checking will be performed.

continue

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

convert

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:

  1. To run an analysis including a subsequent conversion of the results, use the convert option in conjunction with the job and analysis options.

  2. To convert the results of a previously run analysis, use the convert option in conjunction with the job option.

  3. To convert results from a job that is currently running, use the convert option in conjunction with the oldjob option (to name the running job) and the job option (to supply a new name for the files generated by the convert option).

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). This conversion is necessary only if the types of output listed in The Postprocessing Calculator 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.

recover

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). If the original analysis was run in parallel with parallel=domain, it must be restarted with parallel=domain and the same number of processors.

syntaxcheck

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.

information

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. 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.

Additional options available for the analysis module

input

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.

user

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 and Abaqus/Explicit 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.

oldjob

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) run is to be started or from which results are to be imported. A path or file extension is not allowed. The oldjob-name must be different from the current job-name.

This option is required when a restart, postprocessing, or symmetric model generation analysis reads data from the restart or the results file.

For import analysis, this option can be used when importing from a single previous analysis. This option should not be used when importing from multiple previous analyses.

fil

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.

globalmodel

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.

cpus

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 Environment File Settings).

parallel

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 for more information on these methods. The default value is domain, which can be changed in the environment file (see Environment File Settings).

domains

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 (seeEnvironment File Settings). A restart analysis uses the same number of parallel domains as the original analysis, and the value specified with this option will be ignored.

dynamic_load_balancing

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).

mp_mode

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 Environment File Settings).

standard_parallel

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 Environment File Settings).

gpus

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 Environment File Settings).

memory

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 Resources). The default values can be changed in the environment file (see Environment File Settings).

interactive

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 Environment File Settings).

background

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 Environment File Settings).

queue

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 Environment File Settings).

after

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 Configuration Guide for details.)

double

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 Environment File Settings).

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.

scratch

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 Environment File Settings).

output_precision

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

resultsformat

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.

port

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 Environment File Settings). This option is used in conjunction with the host option. For more information, see Selecting TCP/UDP port numbers.

host

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.

csedirector

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.

timeout

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 Environment File Settings).

Additional option available for the datacheck module

unconnected_regions

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.

Examples

The following examples illustrate the different functions and capabilities of the abaqus execution procedure.

Running analyses in Abaqus/Standard

Use the following command to run a heat transfer analysis called “c8” in the background: 

abaqus analysis job=c8 background

The following command will run the job c8 in the background and output the current environment settings to the log file: 

abaqus analysis job=c8 information=environment background

The follow-up analysis to the heat transfer analysis c8 is “c10,” which is a static analysis that uses temperature data from c8 as input. The temperature data are read in from the c8 results file as predefined fields. The execution procedure scans the Abaqus/Standard input file for file dependencies of this sort. In this example the procedure will look for the c8 results file in the current directory with the extension .fil. The results file identifier can include a path name (see Input Syntax Rules), and the execution procedure will then look in the directory specified. In either case an error message will be issued if the file does not exist. The following command is used to run the job c10 in the “long” queue: 

abaqus analysis job=c10 queue=long

This job is next restarted as “c11,” using the final results from c10 as the starting point for a creep analysis. The following command is used to run this job in the default queue: 

abaqus analysis job=c11 oldjob=c10 queue=

The following command is used to run an Abaqus/Standard analysis called “draw_imp” that imports the results from a previously run Abaqus/Explicit analysis called “draw_exp”: 

abaqus analysis job=draw_imp oldjob=draw_exp

Running analyses in Abaqus/Explicit

Use the following command to submit an Abaqus/Explicit analysis called “beam” to the default queue: 

abaqus analysis job=beam convert=all queue=

Equivalent results would be obtained from the following series of commands: 

abaqus datacheck job=beam interactive
abaqus continue job=beam queue=
abaqus convert=all job=beam interactive

Note that the CPU-intensive analysis option is run in batch, while the other options are run interactively.

Running different phases of an analysis

Use the following command to perform a parameter check run on an input file called “parmodel”: 

abaqus job=parmodel parametercheck

Use the following command to perform a data check run on an input file called “parmodel” (the parameter check is done again if this job is run after the previous one): 

abaqus job=parmodel datacheck

The following command will continue the previous datacheck job to execute the analysis: 

abaqus job=parmodel
continue