Translating Abaqus output database files to Nastran Output2 results files

The toOutput2 translator can only be used to translate Abaqus output database of a STATIC or FREQUENCY procedure. 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.