Nastran to Abaqus Conversion Mapping

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 Elem Types panel shows all supported element configs 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. 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" config in the Nastran user profile and CONN3D2 is of ‘rod" config in the Abaqus user profile. It is possible to map a CBUSH to CONN3D2 even though their configs are different. The element mapping scheme must be under the *ElemTypeConversion block in the ConfigurationFile.txt file. You need to provide both config and type information to specify the element mapping scheme.

Table 1. Supported Element Mappings
Nastran 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, COUP_DIS
spring, CELAS1 spring, SPRING2
spring, CELAS2 spring, SPRING2
spring, CDAMP1 spring, DASHPOT1
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 Nastran 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 Nastran 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 HM, are converted into rigid elements. Currently conversion of *COUPLING/*DISTRIBUTING with element based surfaces is not supported.
  • The configuration file can be updated such that config can be changed to DCOUP3D for Rbe3 with COUP_DIS as the default conversion.
  • In the Nastran to Abaqus Conversion browser, the conversion option Define Direction Cosines in Property after conversion for PBar, PBeam, PBarL, and PBeamL is selected by default. If your provided direction cosines for beams in Nastran then this option will transfer this information to *Beam Section in Abaqus.

Contacts

BSURF is converted to *SURFACE ELEMENT

BCBODY in BCTABLE is mapped to CONTACT PAIR

Friction in BCTABLE is mapped to *SURFACE INTERACTION

Sectional Properties

Some of the properties in one solver can be converted to two different Abaqus sections in the other solver. For a Nastran 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 the element level in Nastran. 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 directions can point to the same PBEAM, PBEAML, PBAR or PBARL property in Nastran. 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.

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.

Table 2. Supported Section Property Mappings
Nastran Abaqus Beam axis option
PSOLID *SOLID SECTION  
PSHELL *SHELL SECTION or *SHELL GENERAL SECTION  
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  
PBUSHT(KN) *CONNECTOR PLASTICITY  
PELAS (*SPRING + *DASHPOT) or *CONNECTOR SECTION 1 or 0
PDAMP *DASHPOT or *CONNECTOR SECTION  
PGAP *GAP PROPERTY  
CELAS2 (*SPRING + *DASHPOT) or *CONNECTOR SECTION  
CDAMP2 *DASHPOT or *CONNECTOR SECTION  
CONM2 (*MASS +*ROTARY INERTIA)  
Note:
  • CELAS2, CDAMP2 and CONM2 are elements in Nastran, but they are sectional properties in Abaqus. Therefore, the mapping for them must also be defined under *PropertyConversion.
  • The PELAS or CELAS2 in Nastran have 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 Nastran 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.
  • A Nastran model with PBUSHT KN referencing TABLED1 is converted to CONNECTORSECTION & CONNECTOR_BEHAVIOR ,and TABLED1 is mapped to CONNECTOR PLASTICITY.

Materials

The material mapping scheme must be defined under *PropertyConversion block in the ConfigurationFile.txt file.
Table 3. Supported Material Mappings
Nastran Abaqus  
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.
MAT9ORT *MATERIAL *ELASTIC,TYPE=ENGINEERING CONSTANTS
Note: If a PBEAM or PBAR is mapped to a *BEAM GENERAL SECTION, the material properties defined in the corresponding Nastran material are mapped to the *BEAM GENERAL SECTION card. No *MATERIAL is created in this case.