Products: Abaqus/Standard Abaqus/Explicit
Abaqus/Standard and Abaqus/Explicit, the Abaqus analysis modules, are executed by running the Abaqus execution procedure. Several parameters can be set either on the command line or in the environment file (see “Using the Abaqus environment settings,” Section 3.3.1). 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,” Section 18.2 of the Abaqus/CAE User's Manual.
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.
abaqus | job=job-name |
| [analysis | datacheck | parametercheck | continue | convert={select | odb | state | all} | recover | syntaxcheck | information={environment | local | memory | release | support | system | all}] [input=input-file] [user={source-file | object-file}] [oldjob=oldjob-name] [fil={append | new}] [globalmodel={results file-name | output database file-name}] [cpus=number-of-cpus] [parallel={domain | loop}] [domains=number-of-domains] [mp_mode={mpi | threads}] [standard_parallel={all | solver}] [memory=memory-size] [interactive | background | queue=[queue-name][after=time]][scratch=scratch-dir] [output_precision={single | full} ] [madymo=MADYMO-input-file] [port=co-simulation port-number] [host=co-simulation hostname] [timeout=co-simulation timeout value in seconds] [unconnected_regions={yes | no}] |
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).
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.
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:
To run an analysis including a subsequent conversion of the results, use the convert option in conjunction with the job and analysis options.
To convert the results of a previously run analysis, use the convert option in conjunction with the job option.
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,” 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 “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.
Note: DIGITAL Visual FORTRAN on Windows platforms does not allow the @ symbol to be used in path names.
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 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 11.10.3, 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.
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).
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 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. The possible values are both and explicit. If double=both, both the Abaqus/Explicit packager and analysis will run in double 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. 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). For a discussion of when to use the double precision executable, see “Procedures: overview,” Section 6.1.1. 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 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 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 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 the Abaqus User's Guide for Crash Safety Simulation Using Abaqus/Explicit and MADYMO.
This option is used to specify the TCP/UDP port number for co-simulation between two Abaqus analyses or between Abaqus and AcuSolve (see “Preparing an Abaqus analysis for co-simulation,” Section 14.1.2). 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 to specify the host name for co-simulation between two Abaqus analyses or between Abaqus and AcuSolve (see “Preparing an Abaqus analysis for co-simulation,” Section 14.1.2). This option specifies the name of the machine that is hosting the connection. For co-simulation between two Abaqus analyses, you choose one analysis to host the connection; the other analysis must use the host option to refer to the machine for the hosting analysis. For co-simulation between Abaqus and AcuSolve, the host option is required if AcuSolve initiates communication; otherwise, do not specify the host name.
This option is used to specify a timeout value for co-simulation connection (see “Preparing an Abaqus analysis for co-simulation,” Section 14.1.2). This option specifies the timeout period in seconds. 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 (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.
The following examples illustrate the different functions and capabilities of the abaqus execution procedure.
Use the following command to run a heat transfer analysis called “c8” in the background:
abaqus analysis job=c8 backgroundThe 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 backgroundThe 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,” Section 1.2.1), 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=longThis 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
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 interactiveNote that the CPU-intensive analysis option is run in batch, while the other options are run interactively.
Use the following command to perform a parameter check run on an input file called “parmodel”:
abaqus job=parmodel parametercheckUse 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 datacheckThe following command will continue the previous datacheck job to execute the analysis:
abaqus job=parmodel continue
Use the following command for the first Abaqus analysis to initiate communication via port 55555:
abaqus job=explicit port=55555This Abaqus analysis acts as the server process and waits for the other Abaqus analysis to connect.
Assuming the first analysis is run on einstein.simulia.com, use the following command for the second Abaqus analysis to establish a connection with the first Abaqus analysis:
abaqus job=standard port=55555 host=einstein.simulia.com
Use the following command for Abaqus to initiate communication with AcuSolve via port 55555:
abaqus job=solid port=55555In this case Abaqus acts as the server process and waits for AcuSolve to connect.
Use the following command when AcuSolve initiates a connection on host einstein.simulia.com on port 55555:
abaqus job=solid port=55555 host=einstein.simulia.comIn this case Abaqus acts as the client process and will connect to AcuSolve, which is started on einstein.simulia.com.