OptiStruct to Abaqus Conversion Mapping

Care has to be taken so that the element and property mappings are consistent. Altair provides a valid mapping scheme in the ConfigurationFile.txt. This document explains the scope and limitations of the mapping scheme.

Elements

Engineering Solutions elements have two basic attributes – configuration (or config) and type. The "config" defines the basic geometrical shape of an element. For example, tria3 configuration is a 3 node triangular element and hexa8 is an 8-node hexahedral element. The "type" defines the solver specific element type of a particular configuration. For example, the 4-node quadrilateral (quad4) element in Abaqus can be any of the following types: S4, S4R, M3D4, R3D4, and so on. The Element Types panel shows all supported element configurations and their types for a user profile.

For a specific configuration, you can map any supported Nastran element type to any supported Abaqus element type. For example, for an OptiStruct to Abaqus conversion, several 2-noded element configurations such as spring, rigid, bar2, rid, and so on are supported. Because all of them are 2-noded elements, conversion across these configurations is also allowed for some element types. For example, CBUSH is of "spring" configuration in the Engineering Solutions user profile and CONN3D2 is of ‘rod" configuration in the Abaqus user profile. It is possible to map a CBUSH to CONN3D2 even though their configurations are different. The element mapping scheme must be under the *ElemTypeConversion block in the ConfigurationFile.txt file. You need to provide both configuration and type information to specify the element mapping scheme.

Sectional Properties

Some of the properties in one solver can be converted to two different Abaqus sections in the other solver. For a OptiStruct to Abaqus conversion, for example, PSHELL can be converted to *SHELL SECTION or *SHELL GENERAL SECTION. In the mapping scheme, you must select one of them. The property mapping scheme must be under the *PropertyConversion block in the ConfigurationFile.txt file.

Abaqus beam section axes are defined at element level in OptiStruct. They are in the sectional property level in Abaqus unless the beam axis is defined by a third node in element connectivity. This means that several elements with different beam axis direction can point to the same PBEAM, PBEAML, PBAR or PBARL property in OptiStruct. But in Abaqus, all elements under a *BEAM SECTION or *BEAM GENERAL SECTION property have one beam axis orientation. If a third node is used to define the beam axis, even Abaqus beams with a different axis can belong to a single *BEAM SECTION property. Use the conversion tool to select an extra (1 or 0) argument to define the beam axis conversion mechanism.

If the argument is 0 (or not defined), the conversion tool will take the beam axis direction of the first element corresponding to a PBEAM, PBEAML, PBAR or PBARL property and map that to the corresponding *BEAM SECTION or *BEAM GENERAL SECTION card. The beam axis vectors of other elements with the same property will be ignored.

If the argument is 1, the conversion tool will create a third node for each element to define the equivalent beam axis vector. As a result, the axis direction for each element will be maintained after the conversion. Because this option updates each element, the conversion process might take a considerable amount of time for models with a large number of beams.

The system for CELAS1 or CELAS2 elements is sitting on the grid nodes. Thus, every element can have a different system. Ideally, on conversion one *SPRING (and *DASHPOT) or *CONNECTOR SECTION per element needs to be created. For large models this can be time-consuming.

Therefore for CELAS1 two options can be set in the ConfigurationFile.txt (1 or 0). If the option is 1, one property per element will be created (default). If the flag is set to 0, one property per PELAS card will be created. In this case, the settings of the first element found on this property will be translated. From CELAS2 elements you always create a *SPRING and *DASHPOT or *CONNECTOR SECTION property per element.

Materials

Loads

Engineering Solutions loads have two basic attributes – configuration (or config) and type. The supported load "config" are: force, moment, constraint, pressure, temperature, flux, velocity, acceleration and equation. The load "type" defines the solver specific type of a particular configuration. For example, pressure load can be any of the following Abaqus types: DLOAD, FILM, DFLUX, and so on. The Load Types panel shows all supported load configurations and their types for a user profile.

The converter also converts distributed surfaces loads (*DLSOAD) applied on faces of shell or solid elements into pressure loads (PLOAD4).

In addition to the above load types, the conversion tool also converts OptiStruct Dload, with corresponding Rload1, Rload2, DAREA, TABLED1, TABLED2, TABLED3, to Abaqus *BOUNDARY or *CLOAD (with corresponding *AMPLITUDE curve). No mapping scheme needs to be specified for this conversion; the conversion is done automatically if present in the model.

Load Steps and Analysis Type

The conversion tool maps between OptiStruct subcases and Abaqus steps. It does not convert the solution type from/to any Abaqus analysis type. You must define it manually using the Abaqus Step Manager or the OptiStruct Load Step Browser.

Systems and Masses

WTMASS

If the WTMASS parameter is defined in the OptiStruct model, it is used to modify density, mass, and inertia values during conversion.