To create a modal neutral file containing stress or strain, the Abaqus Interface for MSC.ADAMS must read data from two results files. You create the first results file according to the requirements described in “Setting up the Abaqus model to create a modal neutral file with stress or strain,” Section 2.3. Next, you use the adams command to create an input file for the second Abaqus analysis as described in “Creating the second input file,” Section 3.3.1. You then run the second Abaqus analysis, which writes the second results file. Finally, you use the adams command to create the modal neutral file as described in “Creating the modal neutral file from two results files,” Section 3.3.2.
To create the input file for the second Abaqus analysis, execute the Abaqus Interface for MSC.ADAMS using the following command:
abaqus adams | job=job-name |
[input=input-file] [make_se_recovery] [stress_modes={ON | OFF}] [strain_modes={ON | OFF}] [section_point=section_point_number] |
job
This option controls the name of the new input file that will be created. The job-name value is used to construct the new input file name, job-name_se_recovery.inp.
If this option is omitted from the command line, the user will be prompted for this value.
input
This option specifies the name of the results file from the first Abaqus analysis, if it is different from job-name.fil.
make_se_recovery
This option specifies that the translator is to create a new Abaqus input file. A modal neutral file will not be created.
stress_modes
This option specifies that the new Abaqus input file will contain commands to write stress to the results file. The possible values are ON and OFF. The default value is ON.
strain_modes
This option specifies that the new Abaqus input file will contain commands to write strain to the results file. The possible values are ON and OFF. The default value is OFF.
section_point
This option specifies the section point at which shell stresses and/or strains will be written to the results file. The default value is 1. This option will be ignored for three-dimensional continuum elements.
After running the two Abaqus analyses, as described above, you create a modal neutral file containing modal stress or strain by executing the Abaqus Interface for MSC.ADAMS using the following command:
abaqus adams | job=job-name |
[input=input-file] [se_recovery_job=se_recovery_job-name] [units=mmks | mks | cgs | ips] [length=length-units-name] [mass=mass-units-name] [time=time-units-name] [force=force-units-name] |
job
This option controls the name of the modal neutral file that will be created. The job-name value is used to construct the new modal neutral file name, job-name.mnf.
If this option is omitted from the command line, the user will be prompted for this value.
input
This option specifies the name of the results file from the first Abaqus analysis, if it is different from job-name.fil.
se_recovery_job
This option specifies the name of the results file from the second Abaqus analysis.
units
This option specifies the units system for the model. The possible values are mmks, mks, cgs, or ips, which correspond to the ADAMS/View options with the same names. The default value is mks.
length
This option specifies the length units for the model. If this option is specified, it overrides the length units of the specified units system.
mass
This option specifies the mass units for the model. If this option is specified, it overrides the mass units of the specified units system.
time
This option specifies the time units for the model. If this option is specified, it overrides the time units of the specified units system.
force
This option specifies the force units for the model. If this option is specified, it overrides the force units of the specified units system.