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, , , 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

NASTRAN shell elements may have their orientations and offsets defined on the element connectivity. By default, all elements that reference a single PSHELL translate to a single *SHELL SECTION or *SHELL GENERAL SECTION in ABAQUS and the variation in their properties will be defined using the *ELEMENT PROPERTIES and *DISTRIBUTION keywords. If distribution=OFF, a separate *SHELL SECTION or *SHELL GENERAL SECTION is created for each element set that has a unique combination of orientation, offset, and/or thickness.

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

fromnastran_distribution={OFF | 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}

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 S4. 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