OptiStruct to Abaqus Conversion Mapping

The OptiStruct to Abaqus conversion 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. 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.

OptiStruct Abaqus
tria3, CTRIA3 tria3, S3
tria3, CTRIAR tria3, S3R
quad4, CQUAD4 quad4, S4
quad4, CQUADR quad4, S4R
quad4, CSHEAR quad4, M3D4
tetra4, CTETRA tetra4, C3D4
penta6, CPENTA penta6, C3D6
hex8, CHEXA hex8, C3D8
tria6, CTRIA6 tria6, STRI65
quad8, CQUAD8 quad8, S8R
tetra10, CTETRA tetra10, C3D10
penta15, CPENTA penta15, C3D15
hex20, CHEXA hex20, C3D20
mass, CONM2 mass, MASS
mass, CELAS1 mass, SPRING1
mass, CELAS2 mass, SPRING1
rigid, RBE2 rigid, COUP_KIN
rigidlink, RBE2 rigidlink, COUP_KIN
rbe3, RBE3 rbe3, DCOUP3D
spring, CELAS1 spring, SPRING2
spring, CELAS2 spring, SPRING2
spring, CDAMP1 spring, DASHPOT2
spring, CDAMP2 spring, DASHPOT2
spring, CBUSH rod, CONN3D2
bar2, CBEAM bar2, B31
bar2, CBAR bar2, B31
rod, CROD rod, T3D2
rod, CONROD rod, T3D2
gap, CGAP gap, GAPUNI
weld, RBAR rigid, KINCOUP
Note:
  • The CELAS1 or CELAS2 elements in OptiStruct have both spring stiffness and damping attributes. If both spring and damping values are present and the mapping scheme is CELAS1 to SPRING1, the conversion tool will automatically create an extra DASHPOT element.
  • Similarly, the CONM2 elements in OptiStruct have both translational and rotational mass values. If both translational and rotational values are present and the mapping scheme is CONM2 to MASS, the conversion tool will automatically create an extra ROTARY1 element.
  • *COUPLING/*KINEMATIC constraints with element based surfaces (currently mapped to groups in Engineering Solutions) are converted into rigid elements. Currently conversion of *COUPLING/*DISTRIBUTING with element based surfaces is not supported.

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.

Composite sections PCOMP and PCOMPG can be converted to Abaqus as well. From ConfigurationFile.txt a user can select to convert to SHELL SECTION or SHELL GENERAL SECTION properties. Besides individual layers, the conversion takes care of system assignments, offsets, SYM, BEND and other similar parameters. In PCOMPG a global ply id (GPLYID) number is honored in the ply name in Abaqus user profile after conversion.
OptiStruct Abaqus Beam axis/property option
PSOLID *SOLID SECTION  
PSHELL *SHELL SECTION or *SHELL GENERAL SECTION  
PCOMP(G) *SHELL SECTION or *SHELL GENERAL SECTION (COMPOSITE)  
PBEAM *BEAM GENERAL SECTION 1 or 0
PBEAML *BEAM SECTION 1 or 0
PBAR *BEAM GENERAL SECTION 1 or 0
PBARL *BEAM SECTION 1 or 0
PROD *SOLID SECTION  
PBUSH *CONNECTOR SECTION  
PELAS (*SPRING + *DASHPOT) or *CONNECTOR SECTION 1 or 0
PDAMP *DASHPOT or *CONNECTOR SECTION  
CELAS2 (*SPRING + *DASHPOT) or *CONNECTOR SECTION  
CDAMP2 *DASHPOT or *CONNECTOR SECTION  
CONM2 (*MASS + *ROTARY INERTIA)  
Note:
  • CELAS2, CDAMP2 and CONM2 are elements in OptiStruct but they are sectional properties in Abaqus. Therefore, the mapping for them must also be defined under *PropertyConversion
  • The PELAS or CELAS2 in OptiStruct both spring stiffness and damping attributes. If both spring and damping values are present and they are mapped to *SPRING, the conversion tool will automatically create an extra *DASHPOT property. The elements will both be kept in the same component and the property will be directly assigned to the *SPRING or *DASHPOT element.
  • Similarly, the CONM2 in OptiStruct has both translational and rotational mass values. If both translational and rotational values are present and it is mapped to *MASS, the conversion tool will automatically create an extra *ROTARY INERTIA component.
  • The property conversion scheme and corresponding element conversion scheme must be consistent. For example, if you define PBUSH to *CONNECTOR SECTION at the property mapping scheme, the corresponding element CBUSH must map to CONN3D2 in the element mapping scheme.

Materials

The material mapping scheme must be defined under *PropertyConversion block in the ConfigurationFile.txt file.
OptiStruct Abaqus Notes
MAT1 *MATERIAL *ELASTIC, TYPE=ISO; *EXPANSION, TYPE=ISO; and *DENSITY (G is used only for *BEAM GENERAL SECTION)
MAT2 *MATERIAL When used alone in a PSHELL, MAT2 is translated to *ELASTIC, TYPE=LAMINA or *ELASTIC, TYPE=ANISOTROPIC
MAT8 *MATERIAL ELASTIC, TYPE=LAMINA; *EXPANSION, TYPE=ORTHO; and *DENSITY
MAT9 *MATERIAL *ELASTIC, TYPE=ANISOTROPIC unless the data are found to be orthotropic, in which case the data are analyzed to create *ELASTIC, TYPE=ENGINEERING CONSTANTS. Also *DENSITY; and *EXPANSION, TYPE=ANISO or ORTHO.
Note: If a PBEAM or PBAR is mapped to a *BEAM GENERAL SECTION, the material properties defined in the corresponding OptiStruct material are mapped to the *BEAM GENERAL SECTION card. No *MATERIAL is created in this case.

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).

For a specific configuration, you can map any supported OptiStruct load type to any supported Abaqus load type. The conversion tool does not support conversion across load configurations. The load mapping scheme is valid for either direction and must be under the *BCsTypeConversion block in the ConfigurationFile.txt file. You need to provide both configuration and type information to specify the mapping scheme.
OptiStruct Abaqus
force, FORCE force, CLOAD
moment, MOMENT moment, CLOAD
const, SPC const, BOUNDARY
const, SPCD const, VELOCITY
const, SUPORT const, BOUNDARY
pressure, PLOAD pressure, DLOAD
pressure, PLOAD2 pressure, DLOAD
pressure, PLOAD4 pressure, DLOAD
temp, TEMP temp, TEMPERATURE
equation, MPC equation, EQUATION

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

The conversion tool converts OptiStruct system types into the corresponding Abaqus system (*SYSTEM, *TRANSFORM or *ORIENTATION). It also converts the NSM into *NONSTRUCTURAL MASS and assigns them to the relevant properties.
OptiStruct Abaqus
NSM *NONSTRUCTURAL MASS
NSM1
NSML
NSML1
NSMADD
GRID *NODE AND *SYSTEM
CORD1R *SYSTEM for nodes

*TRANSFORM if referred to on GRID

*ORIENTATION for elements

CORD1C
CORD1S
CORD2R
CORD2C
CORD2S

WTMASS

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