Abaqus to Nastran Conversion Mapping

Care has to be taken so that the element and property mappings are consistent. A valid mapping scheme is provided in the ConfigurationFile.txt file. This document explains the scope and limitations of the mapping scheme.

Elements

HyperMesh 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 Abaqus element type to any supported Nastran element type, or vice versa. For example, for an Abaqus to Nastran direction, 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 Nastran 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 as shown for the Abaqus to Nastran direction below:

It is also possible to use a simplified conversion of Abaqus connectors (CONN3D2) to rbe2 elements when modifying the ConfigurationFile.txt file. Change the entry for rod element type configuration to: rod,CONN3D2 rigid,rbe2

CONN3D2 elements will now be converted to RBE2 elements. Depending on the connection type set in the CONNECTOR SECTION, such as AXIAL or HINGE, degrees of freedom will be set for the RBE2 element. If systems are associated to the connector elemental nodes they will be assigned to the nodes of the RBE2 as well. Not all connection types are supported. If a system is ignored by a particular CONNECTOR SECTION, it will not be assigned to the nodes of the RBE2 either.

These connector types are currently considered in conversion: AXIAL, JOIN, LINK, SLIDE-PLANE, SLOT, ALIGN, REVOLUTE, BEAM, CYLINDRICAL, HINGE, PLANAR, TRANSLATOR, WELD.

*COUPLING/*KINEMATIC constraints with element based surfaces, currently mapped to groups in HyperMesh, are converted into RBE2 rigid elements. *COUPLING/*DISTRIBUTING constraints are converted to RBE3 elements.

Sectional Properties

Some of the properties in one solver can be converted to two different sections in the other solver. For an Abaqus to Nastran conversion, for example, *DASHPOT can be converted to *PELAS or PDAMP. The property mapping scheme can be edited under the *PropertyConversion block in the ConfigurationFile.txt file.

For SOLID SECTION the converter will always convert to PSOLID unless the property has a data line indicating a cross-sectional area for a truss element. In this case, conversion results in a PROD property.

Materials

Loads

HyperMesh loads have two basic attributes – configuration (or config) and type. The supported load "configs" 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 Nastran types: PLOAD, PLOAD2 or PLOAD4. 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).

Sets

Systems

Load Steps and Analysis Type

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

The converter converts *STEP into SUBCASE. Load collector references are maintained upon conversion. If multiple load collectors of a particular step contain constraints, a SPCADD card is created automatically. The same happens in case of loads in separate load collectors; a new LOAD card is created on conversion.