The Abaqus to OptiStruct conversion tool uses an open conversion scheme; you can specify different mappings in the configuration file. 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.

 

Contact and Pretension Groups

---

The table below shows the supported contact group mapping between Abaqus and OptiStruct.

 

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 OptiStruct element type, or vice versa. For example, for an Abaqus to OptiStruct 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 OptiStruct 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 OptiStruct direction below:

Abaqus CONN3D2 connector C3D20R elements are converted to OptiStruct CBUSH, PBUSH using the following guidelines:

 

It is possible to use a simplified conversion of Abaqus connectors (CONN3D2) to rbe2 elements when modifying ConfigurationFile.txt in the following way (change the entry for rod element type configuration:

 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.

All SPRING and DASHPOT related conversions (including JOINTC) map to CELAS1, CDAMP1, or CBUSH/PBUSH using the following guidelines:

 

Sectional Properties

---

The table below shows supported sectional property mapping between Abaqus and OptiStruct. Some of the properties in one solver can be converted to two different sections in the other solver. For an Abaqus to OptiStruct 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.

The property conversion scheme and corresponding element conversion scheme must be consistent. For example, if you define *CONNECTOR SECTION to PBUSH at the property mapping scheme, the corresponding element CONN3D2 must map to CBUSH in the element mapping scheme.

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

For BEAM (GENERAL) SECTION the algorithm automatically decides which property to convert to depending on the element type chosen in the ElementTypeConversion section of the ConfigurationFile.txt. For example, if you want to convert B31 elements to CBAR, the beam property will get converted to a PBAR or PBARL property. If you choose to convert B31 elements to CBEAM, then the converter creates PBEAM or PBEAML properties accordingly. The same logic applies to B32 elements; the difference is that they are changed to first order beam elements first on conversion.

 

Materials

---

The table below shows supported material mapping between Abaqus and OptiStruct.  The material mapping scheme can be edited under *PropertyConversion block in the ConfigurationFile.txt file.

 

Loads

---

HM 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 OptiStruct 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).

Temperature with *INTIAL condition is converted to TEMP(INTIAL) and mapped to Global Case Control.

FILM loads are converted to CHBDYE elements, sink temperatures are converted to SPC and heat transfer coefficient(H) with PCONV.

SFILM loads are converted to CHBDYE elements, sink temperatures are converted to SPC and heat transfer coefficient(H) with PCONV.

For a specific configuration, you can map any supported Abaqus load type to any supported OptiStruct load type. The conversion tool does not support conversion across load configurations. The load mapping scheme can be edited under the *BCsTypeConversion block in the ConfigurationFile.txt file. You need to provide both configuration and type information to specify the mapping scheme as shown below:

 

Sets

 

Systems

 

Load Steps and Analysis Type

---

The conversion tool maps between Abaqus steps and OptiStruct 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, an SPCADD card is created automatically. The same happens in case of loads in separate load collectors; a new LOAD card is created on conversion.

For models containing contacts, NLPARM card is automatically created and assigned to a nonlinear quasi-static subcase.

Abaqus models that contain both conductivity and temperature defined under *CONDUCTIVITY in *MATERIAL is converted to a non-linear Heat transfer (NLHEAT) analysis type in OptiStruct.

*FREQUENCY (analysis type) is converted to normal modes with the EIGRL card (load collector) mapped in the loadstep on conversion.

 

 

See Also:

Abaqus Conversion Tools