Next: Interface Elements Up: Model Definition Previous: Model Definition

Model Geometry

The model geometry section of the ABAQUS input file is preceded by the following comments:

**
*******************
** MODEL GEOMETRY *
*******************
**

FEMGEN will generate a finite element mesh of nodes and geometric element types. These geometric element types are related to the ABAQUS element names via an element variant number. The element variant mappings for ABAQUS may be displayed by using the FEMGEN command 'UTILITY TABULATE FE ABAQUS', and these mappings are shown in tables 2.1 to 2.5. In addition, the user can now set their own default ABAQUS element variants by defining them in a FEMGV resource file (see the FEMGV Users Manual for more details).

Element variants are assigned using the command 'MESHING TYPES part ELTYPE variantno'. The variant number is optional and the default is 1. It is also possible to specify an element variant by using its name directly, i.e. 'MESHING TYPES part CPS8R'.

'*NODE' cards are generated for all nodes in the model. Nodal coordinates are output in the global cartesian system, regardless of the system in which the model was defined in FEMGEN.

'*ELEMENT' cards are generated for all elements in the model. Elements are grouped into sets, one set per FEMGEN part, where the set name is equal to the part name. The automatic generation of ABAQUS element sets for every FEMGEN geometric part can be switched off by setting the resource *.model.element_set : NO (see Table 1.1).

The jacobian (or sense) of all elements is checked by the interface and corrected where necessary. The interface also re-numbers the elements according to the ABAQUS conventions. For models where one or more nodes lie outside the X-Y plane, the interface will not perform a jacobian check on TR3, TR6, QU4, QU8 and QU9 elements.

All nodes in the model or the whole geometry (i.e. all nodes and elements) can be written to a separate ABAQUS input file. This can be done by setting the resource *.model.include to the required option (NONE/NODES/GEOM) or by selecting this option in the dialogue session (see Sections 1.3 and 1.4). The name of this additional file will take the name of the main ABAQUS input file ('.inp') but with the extension '.nod' for the nodes (NODES) or the extension '.geo' for the geometry (GEOM). In the default case (option NONE), only one ABAQUS input file is created.