Abaqus Execution (Part 1)¶
Abaqus/Standard and Abaqus/Explicit Execution¶
Products: Abaqus/Standard Abaqus/Explicit
References¶
- About Execution Procedures
Overview¶
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.
Command Summary¶
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}]
[uniquelibs]
[oldjob = oldjob-name]
[fil = {append | new}]
[globalmodel = {results file-name | ODB output database file-name | SIM database file-name}]
[cpus = total number-of-cpus]
[parallel = {domain | loop}]
[domains = number-of-domains]
[dynamic_load_balancing = {on | off}]
[threads_per_mpi_process = number of threads per mpi process]
[standard_parallel = {all | solver}]
[gpus = total number-of-gpgpus]
[memory = memory-size]
[interactive] | [background] | [queue [ = queue-name ][after = time]]
[double = {explicit | both | off | constraint}]
[scratch = scratch-dir]
[output_precision = {single | full}]
[resultsformat = {odb | sim | both}]
[port = co-simulation port-number]
[host = co-simulation hostname]
[csedirector = Co-Simulation Engine director host:port-number]
[timeout = co-simulation timeout value in seconds]
[unconnected_regions = {yes | no}]
[noFlexBody]
[license_type = {token | credit}]
[ssd_split = number-of-frequency-partitions]
[ssd_partition = frequency-partition-number]
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:
- 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"). This conversion is necessary only if the types of output listed in "The Postprocessing Calculator" are requested.
If convert=state, if the analysis is run in parallel with parallel=domain, the separate Abaqus/Explicit state files (job-name.abq.n) will be converted into a single Abaqus/Explicit state file (job-name.abq).
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.
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.
uniquelibs: This option indicates that input file execution is to use libraries created with the uniquelibs option in the abaqus make execution procedure.
oldjob: This option identifies the files from a previous run from which an import, restart, or postprocessing run (Abaqus/Standard only; see "Recovering Additional Results Output from Restart Data in Abaqus/Standard") is to start or from which to import results. You specify the oldjob-name (without a file extension). For an import or restart analysis, you can include a full or a relative path. 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.
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 SIM output database file. If both the results file and the SIM output database file do not exist, Abaqus uses the ODB database file.
cpus: This option specifies the total 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. The default value is domain, which can be changed in the environment file (see "Environment File Settings").
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.
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.
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/deactivates the dynamic load balancing scheme. The default value is on. Abaqus/Explicit will attempt to improve computational efficiency by periodically reassigning domains to processors in a way that minimizes load imbalance.
threads_per_mpi_process: This parameter is used to select the parallel execution mode from the following options: pure MPI mode, pure thread mode, or a hybrid mode. The thread mode of execution requires that all cores be limited to a single compute node, whereas the cores may span multiple compute nodes for the other two modes.
A value of 1 results in pure MPI mode. Pure MPI mode is active by default for Abaqus/Explicit (see "Parallel Execution in Abaqus/Explicit"). A value equal to the cpus parameter results in pure thread mode. A value in between 1 and the cpus parameter, divisible into the cpus parameter value, results in hybrid mode. Hybrid mode is active by default for Abaqus/Standard with the threads_per_mpi_process value selected automatically (see "Parallel Execution in Abaqus/Standard").
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.
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 total number of GPGPUs to be used in an Abaqus/Standard analysis. In an MPI-based analysis, this parameter is the number of GPGPUs across all hosts.
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.
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.
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.
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. Available queues are site specific.
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.
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.
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.
scratch: This option is used to specify the name of the directory used for scratch files.
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.
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.
port: This option is used to specify the TCP/UDP port number for co-simulation between solvers using the direct coupling interface. The default value is 48000.
host: 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.
timeout: This option is used to specify a timeout value in seconds for establishing the co-simulation connection. The default value is 3600 seconds.
noFlexBody: This option is used to indicate that no translation to generate a flexible body should be done.
license_type: This option is used to control the type of license Abaqus uses for the SimUnit license model. The possible values are token and credit. The default value is token.
ssd_split: This option specifies a value for splitting the frequencies into partitions to execute a steady-state dynamic analysis by running multiple Abaqus jobs.
ssd_partition: This option specifies a particular frequency partition number in conjunction with the frequency split specified by the ssd_split option.
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.
Examples¶
Running Analyses in Abaqus/Standard¶
Use the following command to run a heat transfer analysis called "c8" in the background:
The following command runs the job c8 in the background and outputs the current environment settings to the log file:
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.
Use the following command to run the job c10 in the "long" queue:
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:
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":
Running Analyses in Abaqus/Explicit¶
Use the following command to submit an Abaqus/Explicit analysis called "beam" to the default 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
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":
Use the following command to perform a data check run on an input file called "parmodel":
The following command continues the previous datacheck job to execute the analysis:
Source: Abaqus 2025 FD02 Execution Guide