6.13.1.3.13. Imported Rigid Bodies

When the source file contains rigid body definitions, Mechanical imports them as bodies with the Stiffness Behavior property of the Body object automatically set to Rigid (read-only). Currently this feature is only supported for ABAQUS files.

Supported Analysis Types

Imported Rigid Bodies are supported by the following analysis types:

  • Harmonic Response

  • Modal

  • Static Structural

  • Transient Structural

  • Response Spectrum

  • Random Vibration

Supported Source File Commands

The application imports the following source file data/commands as a rigid body:

CDB

Imported Rigid Bodies are not currently supported by CDB files.

ABAQUS

The ABAQUS command *RIGID BODY command is processed to import rigid bodies. The command supports the following arguments:

*RIGID BODY, ELSET=<elset_name>, REF NODE=<ref_node>

Where:

"<elset_name>" is the name of an element set (*ELSET). Supported elements are usual 2D and 3D continuum elements and rigid elements R3D3, R3D4.
"<ref_node>" is either a node number or a name of a nodal NSET that contains only one node number.
Note:

  • Once imported, the reference node (REF NODE) is available as a normal node and Mechanical automatically generates a node-based Name Selection for each REF NODE. You can use these system generated Name Selections to scope loads and boundary conditions.

  • The application supports contact between flexible and rigid bodies only when defined in the ABAQUS file. This means that manual contact definition (after import) is not supported as this requires to remesh your Model and will invalidate all your objects scoped on mesh entities.

  • Mechanical does not support multi body parts that have a mix of flexible and rigid bodies. In this instance, the application automatically sets the Stiffness Behavior to Flexible and issues a warning.

NASTRAN

Imported Rigid Bodies are not currently supported by NASTRAN files.

LS-DYNA

Imported Rigid Bodies are not currently supported by LS-DYNA files.