Translating Nastran bulk data files to Abaqus input files

This option is used to specify the name of the Abaqus input file to be output by the translator. It is also the default name of the file containing the Nastran data. Diagnostics created by the translator will be written to a file named job-name.log.

This option is used to specify the name of the file containing the Nastran data if it is different from job-name.

If wtmass_fixup=ON, the value on the Nastran data line PARAM, WTMASS, value is used as a multiplier for all density, mass, and rotary inertia values created in the Abaqus input file.

This option can be defined in the Abaqus environment file as follows:

fromnastran_wtmass_fixup={OFF | ON}

By default, each SUBCASE is translated to a STEP option in Abaqus. If loadcases=ON, this behavior is altered for linear static analyses: each SUBCASE is translated to a LOAD CASE option, and all such LOAD CASE options are grouped in a single STEP option.

This option can be defined in the Abaqus environment file as follows:

fromnastran_loadcases={OFF | ON}

Nastran allows beams to have zero values for cross-sectional area or moments of inertia; Abaqus does not. Set this option equal to a small real number to reset any zero values for A, $I_1$, $I_2$, or J to the specified small real number. If this option is omitted or present without a value, the default value of 1.0 × 10⁻²⁰ is used in place of the zeros. To retain the zeros in the translated Abaqus input file, set pbar_zero_reset=0.

This option can be defined in the Abaqus environment file as follows:

fromnastran_pbar_zero_reset=small-real-number

This option determines how shell and membrane sections in Nastran data are translated to Abaqus. If distribution=OFF, a separate section is created for each combination of orientation, material offset, and/or thickness. If distribution=preservePID or ON, element orientations and offsets are written using the DISTRIBUTION option. If distribution=preservePID, an Abaqus section is created corresponding to each PSHELL or PCOMP property ID. If distribution=ON, a single Abaqus section is created for all homogeneous elements referencing the same material.

This option can be defined in the Abaqus environment file as follows:

fromnastran_distribution={OFF | preservePID | ON}

Certain Nastran rigid elements have more than one equivalent in Abaqus. If surface_based_coupling=ON, RBE2 and RBE3 elements translate to COUPLING with the appropriate parameters. Otherwise, RBE2 elements translate to KINEMATIC COUPLING and RBE3 elements translate to DISTRIBUTING COUPLING. This translation behavior also applies to implied RBE2-type rigid elements used for offsets on CBAR, CBEAM, and CONM2 elements.

For input files created with surface_based_coupling=ON, the translated elements can be visualized and manipulated in Abaqus/CAE. However, large numbers of these elements may cause slower performance.

This option can be defined in the Abaqus environment file as follows:

fromnastran_surface_based_coupling={OFF | ON}

If beam_offset_coupling=ON, beam element offsets are translated by creating new nodes at the offset locations, changing the beam connectivity to the new nodes, and rigidly coupling the new and original nodes.

If beam_offset_coupling=OFF, beam element offsets are translated to the CENTROID and SHEAR CENTER options, which are suboptions of the BEAM GENERAL SECTION option.

The setting for this parameter is ignored if the beam element references a PBARL or PBEAML property or if the beam offset has a significant component in the direction of the beam axis. In these situations the beam offsets are always translated as if beam_offset_coupling=ON.

This option can be defined in the Abaqus environment file as follows:

fromnastran_beam_offset_coupling={OFF | ON}

If beam_orientation_vector=OFF, beam cross-section orientations are translated by creating new nodes at the tips of vectors defining the first principal direction of the cross-section and changing the beam connectivity to the new nodes.

If beam_orientation_vector=ON, beam cross-sections are translated by defining vectors on the BEAM SECTION and BEAM GENERAL SECTION options.

This option can be defined in the Abaqus environment file as follows:

fromnastran_beam_orientation_vector={OFF | ON}

This option is used to define the 2-node beam that is created from CBAR and CBEAM elements. The default is B31.

This option can be defined in the Abaqus environment file as follows:

fromnastran_cbar=2-node-beam-element

This option is used to define the 4-node shell that is created from CQUAD4 elements. The default is S4R. If a reduced-integration element is chosen, the enhanced hourglass formulation is applied automatically.

This option can be defined in the Abaqus environment file as follows:

fromnastran_cquad4=4-node-shell-element

This option is used to define the 8-node brick that is created from CHEXA elements. The default is C3D8I. If a reduced-integration element is chosen, the enhanced hourglass formulation is applied automatically.

This option can be defined in the Abaqus environment file as follows:

fromnastran_chexa=8-node-brick-element

This option is used to define the 10-node tetrahedron that is created from CTETRA elements. The default is C3D10.

This option can be defined in the Abaqus environment file as follows:

fromnastran_ctetra=10-node-tetrahedron-element

By default, PLOTEL elements are not translated. If plotel=ON, PLOTEL elements are translated to T3D2 truss elements in an element set named PLOTEL_TRUSSES. The cross-sectional area of the trusses is 1.0 × 10⁻²⁰, and the material has a Young's modulus, E, equal to 1.0.

By default, CHEXA elements with RBE3 elements at all eight corner nodes are translated to the type of 8-node element specified in the chexa parameter. If cdh_weld=RIGID, CHEXA elements with RBE3 elements at all eight corner nodes are translated to rigid fasteners in Abaqus. If cdh_weld=COMPLIANT, CHEXA elements with RBE3 elements at all eight corner nodes are translated to compliant fasteners in Abaqus.