Defining Substructure Generation Steps

You can use a substructure generation step to create a reduced-order model that can be used in other models.

See Also
About Substructure Generation Steps
  1. From the Procedures section of the action bar, click Substructure Generation Step .
  2. Optional: Enter a descriptive Name.
  3. Enter an integer value for the Substructure Identifier, which (prefixed by the letter Z) is used when including the substructure in another FEM.

    This value must be between 1 and 9999, and it must be unique to the current substructure model.

  4. Optional: Enter the Substructure FEM Name.

    The default is <analysis case name>_Substructure_ZID.

  5. Select nodes for the Interface, which is the portion of the substructure that is exposed in the usage model.

    These nodes are available for loads and restraints when the substructure is imported into another model.

  6. Optional: From the Calculation Options, select one or more of the following:
    1. Select Gravity load vectors to generate gravity vectors that can be used to define gravity loading that acts in a fixed global direction during usage.
    2. Select Reduced mass matrix to generate a reduced mass matrix.
    3. Select Reduced structural damping matrix to generate a reduced structural damping matrix.
    4. Select Reduced viscous damping matrix to generate a reduced viscous damping matrix.
    5. In the Evaluate dependent properties at frequency field, enter the frequency at which the solver evaluates frequency-dependent material properties.
  7. Optional: Specify the Retained Eigenmodes. The selected modes must be calculated in a previous frequency extraction step. To select the eigenmodes, see Selecting Eigenmodes for Mode-Based Procedures.

    Retained eigenmodes can be used when a more accurate dynamic response is required; for example, in a coupled acoustic-structural substructure.

  8. From the Global damping options, select one of the following:
    OptionDescription
    None Does not include global damping.
    Structural and acoustic Includes structural and acoustic damping.
    Structural only Includes structural damping.
    Acoustic only Includes acoustic damping.
  9. If you selected global damping, specify the following
    1. In the Mass Proportional field, enter the alpha factor to create global Rayleigh mass-proportional damping.
    2. In the Stiffness proportional field, enter the beta factor to create global Rayleigh stiffness-proportional damping.
    3. In the Stiffness proportional structural field, enter the s-global factor to create frequency-independent, stiffness-proportional, structural damping.
  10. From the Motion Analysis Options select one or more of the following:
    1. Select Recovery domain to recover displacements at eliminated nodes in the multibody dynamic analysis.
    2. Select Motion analysis data to generate reduced Coriolis, centrifugal forces, and further inertia matrices for use in subsequent multibody dynamic analyses.

The substructure is generated as a mesh part feature consisting of a single substructure element with one or more groups of nodes. A substructure property is also created.

You can select nodes from the substructure to create orphan node groups. You can also create features that use these node groups; for example, ties, connectors, point forces, and clamps.

Note: From the Calculation Options you must select the Reduced mass matrix when the substructure is used as a linear flexible body in subsequent multibody dynamic analyses. Otherwise, the inertia properties of the linear flexible body cannot be calculated.