ABAQUS Analysis User's Manual  


3.2.22 Execution procedure for translating ABAQUS output database files to NASTRAN Output2 results files

Products: ABAQUS/Standard  ABAQUS/Explicit  

Reference

Overview

The translator converts certain results from an ABAQUS output database (.odb) file to the NASTRAN Output2 file format.

Using the translator

Results from an ABAQUS analysis are written to the ABAQUS output database by using the *OUTPUT option. The following options should be included in the ABAQUS input file to ensure that the results to be translated are available in the ABAQUS output database:

*OUTPUT, FIELD
*NODE OUTPUT
U,
RF,
CF,
*ELEMENT OUTPUT
S,
E,
SF,
NFORC,
Results in the ABAQUS output database other than those specified above are skipped during translation. Only results from spring elements and three-dimensional continuum, shell, membrane, beam, and truss elements are translated.

For shell elements, the translator treats stresses and strains at the lowest numbered section point as being at the bottom surface and stresses and strains at the highest numbered section point as being at the top surface. Midsurface stresses and strains translated to the Output2 file are computed as the averages of the stresses and strains at the bottom and top surfaces.

Nodal results are always in global coordinates. Element tensor results are in the ABAQUS element coordinate system.

Model data from the output database (nodal coordinates, element topology, material properties, and element properties) are written to the Output2 file when applicable records exist.

Command summary

abaqus toOutput2
job=job-name
 
[odb=odb-name]
[step=step-number]
[increment=increment-number]

Command line options

job

This option specifies the name of the NASTRAN Output2 file to be created by the translator. It is also the default name for the ABAQUS output database.

odb

This option specifies the name of the ABAQUS output database if it is different from job-name.

step

This option specifies the step number of the ABAQUS output database for the translator to translate. If the specified step contains multiple load cases, all of the load cases are translated. The default value is the last step of the analysis.

increment

This option is valid only when used in conjunction with the step option. It is used to specify the increment number of the step in the ABAQUS output database for the translator to translate. The default value is the last increment of the specified step.

slim

This option is used to include data blocks required for postprocessing in the SLIM/VISION software (available from Third Millennium Productions, Inc.) in the Output2 file.

quad4corner

This option is used to request shell output at corner nodes instead of at the centroid. This option is relevant for stress, strain, and section force output.