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

abaqus analysis job=c8 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,” 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=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

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.

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

The following command will execute ABAQUS/CAE and load the model database file called “beam”:

abaqus cae database=beam

The following command will run the Python script in a file named “try.py” at application startup and pass “argument1” to the script:

abaqus cae script=try.py -- argument1

If “try.py” is defined as

import sys
print sys.argv[-1]

the above command will print argument1.

Use the following command to execute the Python script in a file named “parstudy.psf”:

abaqus script=parstudy

The following command will initiate a Python scripting session:

abaqus script

In a Python scripting session the following command will execute the Python script in a file named “scriptfile”:

script("scriptfile")

Use the following command to display the local installation notes:

abaqus information=local

The following command will write the local installation notes to the file support.log:

abaqus information=local job=support

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 “findkeyword” procedure will list the sample input files that use a specified keyword. For example, to list the sample problems that use the *RESTART option with the WRITE parameter, type the following command and data lines:

abaqus findkeyword
*RESTART,WRITE

To generate a list of sample problems that contain two keyword lines in the same file, both keywords are included as data lines. For example,

abaqus findkeyword
*RESTART,WRITE
*NGEN

To list all sample problems that use a keyword and parameter with a value, the value must be included on the data line. For example,

abaqus findkeyword job=beam
*BEAM SECTION,SECTION=ARBITRARY

The output is written to the file beam.dat.

User-specified parameter values (e.g., numeric data, set names, orientation names, etc.) are ignored. The following two examples are equivalent because the value MYSET is an element set name.

abaqus findkeyword
*ELSET,ELSET=MYSET

abaqus findkeyword
*ELSET,ELSET

The “fetch” procedure will extract an ABAQUS input file from the sample input file archive files. To fetch the example input file c2.inp from the archive files, use the following command:

abaqus fetch job=c2.inp

To fetch all files associated with job c8 from the archive files, use the command

abaqus fetch job=c8

In this case ABAQUS will extract both the input file (c8.inp) and the user subroutine file (c8.f).

To fetch the sample parametric study scripting file parstudy.psf from the archive files, use the following command:

abaqus fetch job=parstudy.psf

The “make” procedure will compile a user-provided FORTRAN source or object file and link it with the appropriate ABAQUS object libraries to create an executable postprocessing program. To create an executable called “pprocess” given a FORTRAN source file of the same name, use the following command:

abaqus make job=pprocess

This program can then be run using the command

abaqus pprocess

The “ascfil” procedure will convert a results file (.fil) from binary to ASCII format and vice versa. To convert the results file c4.fil from binary to ASCII format, use the following command:

abaqus ascfil job=c4

The translated file will have the name c4.fin.

The “append” procedure will append the history information of a second results file to the end of a first results file. The following command will append the history contents of the fjoin003.fil results file to the end of the fjoin002.fil results file and create the file fjoin001.fil:

abaqus append job=fjoin001 oldjob=fjoin002 input=fjoin003

The same command can be given with the alternative syntax

abaqus append -job fjoin001 -oldjob fjoin002 -input fjoin003