The first step in substructure definition is the addition of a Substructure generate step in your analysis. The substructure generation step enables you to create a substructure in your model database and, if desired, specify substructure-related options such as the writing of the recovery matrix, stiffness matrix, mass matrix, and load case vectors to a file. These options are described later in this section.
A single analysis can include multiple substructure generate steps, and Abaqus/CAE creates corresponding output database files for each step. Multiple preloading steps can precede every substructure generation step in your analysis. If you want to specify retained eigenmodes for substructure generation, you must also include a frequency extraction step in the analysis.
Substructure identifier
You must specify a unique identifier for each substructure you create. Substructure identifiers must begin with the letter Z followed by a number that cannot exceed 9999.
Recovery options
You can recover the field output data for a substructure during the usage-level analysis, but you must specify the recovery region during substructure generation. Substructure recovery can be performed only on the sets included in the recovery region. You can specify that recovery be performed on the whole model or for an individual node set or element set. While performing the substructure recovery in the usage model, Abaqus/CAE must have access to the substructure's .mdl, .prt, .stt, and .sup files. For more information about these file types, see “Defining substructures,” Section 10.1.2 of the Abaqus Analysis User's Guide.
Generation options
You can control several aspects of the substructure generation process, including calculation of gravity load vectors, evaluation of frequency-dependent material properties, and generation of a reduced mass matrix, reduced structural damping matrix, and viscous damping matrix.
Retained eigenmodes
You can specify retained eigenmodes for generation of a coupled acoustic-structural substructure. When you choose to specify retained eigenmodes, Abaqus/CAE enables you to specify eigenmodes by mode range or by frequency range.
Damping
You can specify several global damping controls and substructure damping controls. For global damping you can choose to apply damping settings to acoustic or mechanical options; for substructure damping you can specify separate controls for viscous and structural damping.
