Abaqus to OptiStruct 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.

Contact and Pretension Groups

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.

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.

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

Nodal thickness is mapped to respective grid post conversions.

HTML report supported for Joints.

Configuration file paths are selected in batch mode conversion. Conversion options can be used in batch mode conversion by editing the configuration file.

Sectional Properties

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 cross-sectional 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

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.

Distributed surfaces loads (*DLSOAD) applied on faces of shell or solid elements into pressure loads (PLOAD4).

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.

Abaqus *connector behavior STOP/LOCK with Elastic/Non-linear/RIGID convert to PJOINTG with STOP/LOCK with ELAS/NLELAS/RIGID.

Sets

Control Cards

Systems

Control Cards

Displacement, Stress and Contact pressure output card is created on conversion and is mapped to respective loadstep.

Node set and element set from output block for displacement and stress are mapped if mapped to step.

PARAM,INREL,-2 is created if there is *INERTIA RELIEF in the Abaqus deck.

PARAM,RBE3COL is created if there are rbe3 elements in the Abaqus deck.

*PREPRINT,CONTACT=YES to OptiStruct CONTPRM,PREPRT,YES.

If OUTPUTBLOCK is not mapped to any loadstep these are updated in GLOBAL CASE CONTROL.

*RESTART,WRITE,OVRELAY is converted to OS RESTARTW= 1 ,COVER

Load Steps and Analysis Type

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

The converter converts *STEP into respective supported SUBCASE. Load collector references are maintained upon conversion. If multiple load collectors of a particular step have constraints, an SPCADD card is created automatically. Similarly, a LOAD card is created for homogeneous loads and mapped to step.

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.

NLGEOM is set to YES in a loadstep with id 'i', CNTNLSUB will be set checked on, OPTION set to YES and SCID points to the previous loadstep in loadstep with id 'i+1'. The chain continues for the loadsteps.

*PERTURBUTION steps are converted to linear static.

*FREQUENCY RESIDUAL=YES is converted to RESVEC=YES on conversion.

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

*SELECTEIGENMODES converted OptiStruct MODESELECT.

SUBCASE (MONITOR) converted to MONITOR and updated in the Loadstep.

*STATIC load step wuth Int_INC is mapped to NLPARM load collector with NINC=1/Int_INC.

*STATIC load step with MinIcr is mapped to NLADAPT,DTMIN load collector.

*STATIC load step with MaxIncr is mapped to NLADAPT,DTMAX load collector.

*STEP with unsymm=yes is converted to PARAM, UNSYMSLV.

*ENDLOADCASE conversion supported.

Dynamic NLGEOM=yes to Transient Nonlinear analysis.