-
input
-
This option is used to specify the input file name, which might be given with or
without the .inp extension (if the extension is not supplied,
Abaqus appends 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 might contain a
path name and might 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 required 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 required. 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.
The user subroutines must be written to consider the implications of parallel
execution, particularly thread-safety (see Ensuring Thread Safety). In
addition, they must be written to consider any coordination required on account of
parallelism, particularly in user subroutines such as VEXTERNALDB and UEXTERNALDB.
-
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.
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 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. For more information
on these methods, see Parallel Execution in Abaqus/Explicit.
-
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 (see Environment 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/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 (see Parallel Execution in Abaqus/Explicit).
-
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 might span multiple compute nodes for the
other two modes.
A value of 1 results in pure
MPI mode. The 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. The 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
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 and Abaqus/Explicit dynamic explicit 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 or Abaqus/Explicit analysis. In an MPI-based analysis, this
parameter is the number of GPGPUs across all hosts.
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 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 using the
run_mode parameter (see Environment File Settings).
-
after
-
This option is used with the queue option to
specify the time when the job starts 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. You can set the default value for this parameter 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 Services director process when performing a co-simulation using the SIMULIA Co-Simulation Services. The csedirector entry identifies the host
name and the TCP/UDP port number for the listening
port of the SIMULIA Co-Simulation Services 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 Services. 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).
-
noFlexBody
- This option is used to indicate that no translation to generate a
flexible body should be done. By default, the
abaqus execution procedure executes the
tosimpack or
toexcite translators with default arguments on
completion of an Abaqus/Standard flexible body generation analysis set to generate a flexible body in the Simpack or
AVL EXCITE™ format, respectively.
-
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. This capability is also supported through the Abaqus environment file with the environment variable
license_type. For more information, see License management parameters.
-
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.