Generating substructures

When you generate a substructure, you specify an identifier that will be assigned to this substructure in a substructure library. The identifier must begin with the letter Z followed by a number that cannot exceed 9999.

Substructure identifiers must be unique within a library. If a substructure with this same identifier already exists in the library, the analysis will terminate with an error message unless you have specified that the existing substructure should be overwritten, as described below.

Abaqus limits the substructure size to 16,384 for substructures used in Abaqus and to 46,340 for substructures generated in Abaqus and used outside of Abaqus, such as for flexible body dynamics workflows. The analysis preprocessor exits with an error message if generation of a substructure with more than 46,340 degrees of freedom is requested.

SUBSTRUCTURE GENERATE, TYPE=Zn

Step module: Create Step: Linear perturbation: Substructure generation: n

The degrees of freedom at a node can be divided into retained degrees of freedom (for use at the usage level of the substructure) and eliminated degrees of freedom (internal to the substructure). Abaqus/Standard allows any of the degrees of freedom at any of the nodes of a substructure to be retained with one exception: if an acoustic-structural substructure is generated, based on coupled or uncoupled modes, only structural degrees of freedom can be retained. You must make sure that the choice of retained degrees of freedom is reasonable so that the substructure can be connected correctly to the rest of the model.

Any degrees of freedom where kinematic constraints may have to be respecified during usage of the substructure should be kept as retained degrees of freedom.

If any degrees of freedom of nodes used to define distributing coupling elements are retained, the degrees of freedom of an internal node associated with the Lagrange multipliers are added automatically to the list of the retained degrees of freedom of the substructure.

To define the retained degrees of freedom, specify the node number or node set label and, optionally, the first and the last degree of freedom to be retained.

By default, the nodes associated with the retained degrees of freedom will be sorted into ascending numerical order.

RETAINED NODAL DOFS

Load module: boundary condition editor: Category: Mechanical: Types for Selected Step: Retained nodal dofs

An effective technique for modeling the dynamic behavior of a substructure is to augment the response within the substructure by including some generalized degrees of freedom associated with the dynamic modes. You can select the modes to retain, which must be calculated in a previous frequency extraction step (Natural frequency extraction). For some cases of the substructure generation, the dynamic modes have to be fully recovered; if they were computed with the AMS eigensolver and only partially recovered, an error message is issued in such cases. For example, if a substructure includes the substructure load cases or structural-acoustic coupling (or it will be used for flexible body generation) the eigenmodes have to be fully recovered. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. If all retained degrees of freedom of the substructure are constrained in the frequency extraction step, this technique is commonly referred to as the Craig-Bampton method. If all retained degrees of freedom of the substructure are not constrained in the frequency extraction step, this technique is commonly referred to as the Craig-Chang method. The substructure dynamic modes in the Craig-Bampton method are commonly referred to as the fixed-interface modes, and the substructure dynamic modes in the Craig-Chang method are commonly referred to as the free-interface modes. If some retained degrees of freedom of the substructure are constrained and other retained degrees of freedom are not constrained in the frequency extraction step, the dynamic modes are called mixed-interface modes. If the free-interface or mixed-interface dynamic modes are selected, the substructure generation time can increase substantially compared to the case when the same number of fixed-interface dynamic modes is used. Abaqus issues a warning message in this case. However, better solution accuracy can sometimes be achieved with a significantly smaller number of free- or mixed-interface dynamic modes than by using fixed-interface modes.

A sufficient number of the dynamic modes should be selected to provide adequate dynamic representation of the substructure. You should examine loading frequencies and frequency content of the structure to determine this range. Specify a shift point and/or a cutoff frequency in the eigenfrequency extraction step definition to obtain modes in the desired frequency range only. Inclusion of generalized degrees of freedom adds the cost of the frequency extraction to the substructure generation step but greatly improves the accuracy of the solution if the substructure is used in a subsequent dynamic (Implicit dynamic analysis using direct integration), steady-state dynamic (Direct-solution steady-state dynamic analysis), or frequency extraction (Natural frequency extraction) analysis.

In the case of the displacement normalization of the eigenvectors in a frequency extraction analysis, a substructure must have at least one physical degree of freedom active on the usage level; otherwise, the modes cannot be normalized properly. See Substructuring and substructure analysis for additional details.

The retained eigenmodes must be selected when an acoustic-structural substructure is generated.

The effect of acoustic-structural coupling can be included in the retained eigenmodes during the natural frequency extraction procedure. To calculate the coupled structural-acoustic eigenmodes, use a frequency extraction analysis with the default Lanczos eigensolver and include the effect of acoustic-structural coupling during the natural frequency extraction procedure (Natural frequency extraction).

Abaqus can also use uncoupled eigenmodes, generated from either SIM-based Lanczos or AMS eigensolver, to generate a coupled acoustic-structural substructure. In this case the effect of acoustic-structural coupling is included during the substructure generation. Both structural and acoustic eigenmodes have to be retained for the substructure generation, and the selection of the acoustic zero-frequency modes, if such modes are present, is required to get an accurate substructure.

Substructures can be used in models that exhibit nonlinear response (associated with standard Abaqus elements or with contact definitions), but the response within a substructure assumes linear small deformations. However, a substructure's response may be a linear perturbation about a predeformed (possibly rotating and translating) base state, defined on the basis of nonlinear response within the substructure during its preload history.

When the substructure is intended for use in geometrically nonlinear analyses, the substructure preloading should be limited to loads that generate self-equilibrating stresses only (such as thermal stresses or interference fits). In most cases, preload stresses are not self-equilibrating (such as stresses from specified boundary conditions or applied loads). If non-self-equilibrating prestress exists and the substructure undergoes a rigid body motion at the usage level, additional stress is generated in the substructure. Such usage level stresses are non-physical and will lead to convergence problems and results that are difficult to interpret. Therefore, you should use extreme care when preloading a substructure intended for use in geometrically nonlinear analyses.

This preloading concept allows such effects as stress stiffening to be included in a substructure. Preloading is a part of the state of the substructure: the preload is self-equilibrating and so does not generate a load vector when the substructure is used. Any loading of the substructure during its use in a model is in addition to the preload.

It is important to distinguish the difference between a preload and a load case. Both are allowed during a substructure generation analysis, but only the preloads are actually applied to the substructure during generation. Load cases, defined during substructure generation, can only be applied at the usage level (see Applying loads to a substructure). Load cases are discussed in more detail later.

You can generate a reduced mass matrix for a substructure.

A reduced mass matrix is calculated by projecting the global mass matrix to the subspace of the substructure modes. This technique is known as Guyan reduction if only the static modes associated with the nodal retained degrees of freedom are used. Using only the static modes may not be sufficient to define the dynamic response of the substructure accurately. Additional dynamic modes must be used to improve the response inside the substructure.

SUBSTRUCTURE GENERATE, TYPE=Zn, MASS MATRIX=YES

Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced mass matrix 

Viscous damping in the Abaqus model can be defined by "Rayleigh-type" damping associated with materials (see Material damping), by dashpots (see Dashpots), by connector elements, by user-defined elements, by direct matrix input (see Using matrices), and by some other modeling features. You can generate a reduced structural damping matrix for a substructure that will represent all sources of the viscous damping in the model.

The reduced viscous damping matrix is calculated in a manner similar to that used for the reduced mass matrix.

SUBSTRUCTURE GENERATE, VISCOUS DAMPING MATRIX=YES

Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced viscous damping matrix 

Structural damping in the Abaqus model can include contributions from the material structural damping defined as a scaling factor for the stiffness (the imaginary stiffness), damping contributions from frequency-domain viscoelasticity, structural damping contributions from connectors and spring elements, and from user-defined elements. It can also be defined by direct matrix input (see Using matrices). You can generate a reduced structural damping matrix for a substructure.

The reduced structural damping matrix is calculated in a manner similar to that used for the reduced mass matrix.

SUBSTRUCTURE GENERATE, TYPE=Zn, STRUCTURAL DAMPING MATRIX=YES

Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced structural damping matrix 

Usually, the reduced substructure operators (matrices) are symmetric, but the substructure stiffness and damping matrices can be unsymmetric for a number of special modeling cases. For example:

• When a coupled acoustic-structural substructure, generated from coupled or uncoupled modes, is generated from a model with damping specified on the acoustic domain, the substructure damping matrices are unsymmetric.
• The substructure stiffness matrix is unsymmetric if the substructure is generated from a model including sliding contact with friction.
• The substructure viscous damping matrix is unsymmetric if the substructure is generated from a rolling tire.
• The substructure viscous damping matrix is unsymmetric if the friction-induced contributions are included.

Abaqus does not automatically generate an unsymmetric substructure in these cases. You must explicitly select the unsymmetric solver (see Defining an analysis) for the substructure generation step to obtain correct substructure matrices with unsymmetric contributions.

The load cases defined during the generation of a substructure and activated at the usage level are the equivalent of the elemental loading types available for the regular elements in Abaqus. They can be made up of any combination of loadings (distributed loads, concentrated nodal loads, thermal expansion, and load cases defined for any substructures that may be used as part of the definition of this substructure).

The load cases are needed so that, when the substructure is subsequently used in a model, the consistent loads on the retained degrees of freedom need be scaled only by the appropriate magnitudes of the particular loads applied: it is not necessary to go inside the substructure and repeat the basic element calculations to distribute the loads.

Each such load case can be applied when the substructure is used by associating it with an amplitude/time curve and a magnitude (Amplitude Curves). When a substructure is used, the substructure load case loadings that were created when the substructure was generated are the only loads that can be used in that substructure. Except for gravity loading, when using the substructure, you cannot apply distributed loads, temperature loads, etc. to the elements that make up any substructure. These loads must be built into the substructure during its creation.

You can define multiple substructure load cases during the substructure generation to define different loadings for the substructure. Each load case is assigned a name that will be used when the load case is applied on the usage level.

You can use any combination of concentrated load, distributed load, substructure load, and temperature fields (Concentrated loads and Distributed loads) to define each load case.

You assign each basic loading a reference magnitude, which will then be scaled by the actual magnitude specified when the substructure load is applied. The reference magnitude assigned to each basic loading must be defined as the change in load or boundary condition from the base state, not the total of the base state plus the perturbation value. Initial conditions applied within the substructure generation are not included as part of a load case definition.

For temperature loads, the load vector for the substructure load case will contain only the contributions due to thermal expansion. If temperature-dependent properties are present, they are evaluated at the temperatures specified in the preloaded state. Consequently, to take into account nonzero initial temperature fields prescribed as initial conditions (Initial conditions in Abaqus/Standard and Abaqus/Explicit), it is necessary to preload the structure before creating the substructure. When using temperature loading in a substructure load case, the data cannot be read from a results file. The temperatures specified must be defined as the change in the temperatures from the base state.

Abaqus/Standard currently has a limitation when a substructure load case definition includes acoustic loading during a substructure generation procedure in which retained modes are specified: the contribution of the singular (constant pressure) acoustic modes (Acoustic, shock, and coupled acoustic-structural analysis) is not taken into account in the generated load case. Since the contribution of this mode is significant for low frequency response, the generated load case will inadequately represent the specified acoustic load in these cases. If there are no singular acoustic regions in the coupled acoustic-structure substructure, the acoustic loads are represented accurately.

It is important to distinguish the difference between a load case and a preload. Both are defined during substructure generation, but only the preloads are actually applied to the substructure on the generation level; load cases, defined on the generation level, can only be applied on the usage level, and they act on a preloaded base state if one has been specified. (Preloads were discussed earlier.)

In general analysis steps and perturbation steps substructure loads are treated in the same way as other loads, such as concentrated loads and distributed loads (Concentrated loads and Distributed loads). For example, if a general analysis step is followed by another general analysis step, the substructure loads will be retained in the second step with their magnitude equal to that at the end of the previous general analysis step, unless the substructure load is modified or removed. In a linear perturbation step the substructure load represents an incremental load.

If a substructure load is used to apply Coriolis loading in a direct-solution steady-state dynamic analysis, the unsymmetric load stiffness contribution is not taken into account.

SUBSTRUCTURE LOAD CASE, NAME=name
CLOAD and/or
DLOAD and/or
DSLOAD and/or
TEMPERATURE 

Load module: Create Load Case: click the Add button: select loads

We define the substructure eigenvalue problem as the generalized eigenvalue problem for reduced substructure stiffness and mass matrices. The reduced stiffness matrix is always generated for Abaqus substructures. If a generated substructure has the reduced mass matrix, the substructure eigenvalue problem can be solved and the substructure eigenmodes can be extracted. The substructure eigenfrequencies provide useful information about the substructure dynamic properties. The substructure eigenmodes can be used to define the substructure modal damping at the substructure usage stage, and they are required for the flexible body generation. By default, the substructure eigenvalue problem is solved when it is possible (when the reduced mass matrix is available). If generation of the reduced mass matrix is not requested but generation of a flexible body from a substructure is performed, we solve the substructure eigenvalue problem; but instead of the conventional reduced mass matrix, we use a projection of the lumped mass matrix on the substructure modal subspace. The lumped mass matrix is created from the global mass matrix of the finite element model by the commonly used heuristic algorithm. If the substructure eigenvalue problem is solved, the obtained substructure eigenvalues and eigenfrequences are printed in the data (.dat) file. If desired, you can disable the solve of the substructure eigenvalue problem.

SUBSTRUCTURE GENERATE, EIGENPROBLEM=YES (default)

SUBSTRUCTURE GENERATE, EIGENPROBLEM=NO

In a substructure generation analysis, you can check the quality of the generated substructure stiffness and mass matrices. The matrix check generates six “artificial” rigid body modes and projects the substructure matrices onto the rigid body modal subspace. It is expected that the projected 6 $\times$ 6 stiffness matrix (also known as the rigid body energy matrix) is close to zero in the absence of the boundary conditions and constraints. The total inertia statistics for the model are extracted from the projected 6 $\times$ 6 rigid body mass matrix. You can specify the center of rotation for creating the artificial rotational rigid body modes and calculating the global inertia tensor. If the matrix quality check is requested, the check results are printed in the data (.dat) file.

MATRIX CHECK

MATRIX CHECK, REFERENCE NODE=node_label

Abaqus/Standard can generate a flexible body from a substructure. The generated flexible body can be used in flexible body dynamic simulations using external solvers. Abaqus/Standard supports generation of several flexible body types that can be used by external flexible body dynamics solvers. The generated flexible body entities are stored in the substructure .sim file and can be converted to conventional flexible body representations by postprocessing programs.

FLEXIBLE BODY, TYPE=ADAMS

FLEXIBLE BODY, TYPE=EXCITE

FLEXIBLE BODY, TYPE=GENERIC

FLEXIBLE BODY, TYPE=SID

FLEXIBLE BODY, TYPE=SIMPACK

You can write a substructure's recovery matrix, reduced stiffness matrix, mass matrix, and load case vectors to a file. This output is useful when the substructure is to be used in another program.

The output records can be written either to the Abaqus/Standard results file, to a user-defined file, or to the output database file (see below). In each case you must specify which matrices/vectors to output: the mass matrix, the recovery matrix, the load case vectors, the stiffness matrix, and/or the gravity load vectors. By default, no output will be generated.

Repeat the substructure matrix output request in the substructure generation file of each substructure for which the substructure matrix output is required.

If substructure load case vector output is requested for a preloaded substructure, the output will contain a record with a load case number that is equal to zero. This load vector contains the forces that were necessary to equilibrate any stresses that were generated during the previous steps.

SUBSTRUCTURE MATRIX OUTPUT, MASS=YES, RECOVERY MATRIX=YES, SLOAD=YES, STIFFNESS=YES, GRAVITY LOAD=YES

Substructures are stored in a collection of libraries. Housekeeping functions are provided to help maintain extensive libraries; for example, substructures can be deleted from a library or moved to a different library.

Once a substructure library has been generated, the disk files can be made read-only to protect the library from accidental deletion or modification. A substructure library must be write-accessible during a substructure's generation and when substructures are added or deleted from a library using the substructure housekeeping functions.

When multiple analyses are used to generate a substructure library, these analyses must be run one after another; they cannot be run simultaneously. Abaqus may not be able to provide any indication that the substructure library being written may already be in use by another Abaqus analysis. If several analyses write to the same library simultaneously, the library may get corrupted. If this occurs and the library is used in a subsequent analysis, the result may be a large preprocessor memory demand.

SUBSTRUCTURE COPY
SUBSTRUCTURE DELETE
SUBSTRUCTURE DIRECTORY

Substructure libraries are not supported in Abaqus/CAE.