The Nastran To Abaqus 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. Altair provides a valid mapping scheme in the ConfigurationFile.txt. This document explains the scope and limitations of the mapping scheme.

Use the Conversion tool to convert a Nastran file to an Abaqus file.

Any rigid element with one of the degree of freedom left free during conversion will be converted as a hinge element when this option in enabled.

 

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 as shown below:

Notes:

 

Sectional Properties

---

The table below shows supported sectional property mapping between Nastran and Abaqus. 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.

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.

Notes:

 

Materials

---

The table below shows supported material mapping between Nastran and Abaqus. The material mapping scheme must be defined under *PropertyConversion block in the ConfigurationFile.txt file.

 

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 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).

The SPC load collectors referenced in SPCADD will have INITIAL_CONDITION as its card image on conversion.

The LOAD cards referenced in LOADADD will be attached to all of the load steps in the model on conversion.

For a specific configuration, you can map any supported Nastran 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 as shown below:

In addition to the above load types, the conversion tool also converts Nastran 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.

All loads in a load collector with the LOAD card image assigned, are converted to respective loads, with scaling applied to loads as defined in the LOAD card.

 

Load Steps and Analysis Type

---

The conversion tool maps between Nastran subcases and Abaqus steps. It does not convert the solution types to/from any Abaqus analysis type. You must define them manually using the Abaqus Step Manager or the Load Step browser.

 

Systems and Mass

---

The conversion tool converts Nastran 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. The mapping can be summarized as:

 

WTMASS

---

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

 

 

See Also:

Nastran Conversion Tools