Generating Substructures

The generated substructure is associated with a name. You can specify the substructure name, which is the preferred method for naming a substructure. By default, a substructure is named jobname_Zn, where jobname is the name of the substructure generation job, and n is the current step number of the job.

The substructure name must be unique in the substructure generation analysis. If several substructures are generated in the same substructure generation job, they must have different substructure names.

SUBSTRUCTURE GENERATE, NAME=name

Abaqus provides an alternative method to name a substructure. Instead of using the default name or specifying the substructure name, you can specify a prefix and an identifier. The identifier must begin with the capital letter Z followed by a positive integer that cannot exceed 9999. You can specify libname as the prefix and Zn as the identifier to construct the substructure name libname_Zn.

SUBSTRUCTURE GENERATE, TYPE=Zn, LIBRARY=libname

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

A substructure database is the set of files that describes the mechanical and geometric properties of a substructure. Abaqus writes all generated substructure data to the substructure database during the substructure generation analysis. The substructure database can include files with the following extensions: .sim, .prt, .mdl, .stt, and .odb.

The substructure database files are named using the substructure name. Therefore, if several substructures are generated in the same substructure generation job, they must have different substructure names. If a substructure with the same name already exists in the user directory, the analysis ends with an error message unless you specify to overwrite the existing substructure database files (see Overwriting the Substructure Database Files).

The substructure files are named as follows:

• name.sim
• name.prt
• name.mdl
• name.stt
• name_MODEL.odb
• name_MODEL.sim

The name.sim file is generated for every substructure. This file contains the condensed substructure operators, recovery matrices, and other generated substructure entities.

Files with the extensions .prt, .mdl, and .stt contain the internal Abaqus database for the finite element model from which a substructure is generated. These files are generated only if the solution within the substructure can be fully or partially recovered. Abaqus uses these files to recover element results within the substructure in the substructure usage analyses.

SUBSTRUCTURE GENERATE, MODEL DATA=ODB

SUBSTRUCTURE GENERATE, MODEL DATA=NONE

Controlling the generation of the model data file is not supported in Abaqus/CAE.

SUBSTRUCTURE GENERATE, OVERWRITE

By default, the solution at any degree of freedom in the substructure can be recovered. Abaqus must have access to the substructure's .mdl, .prt, and .stt files to perform a full recovery. These files all reside in the substructure database.

You can specify that a recovery of element or nodal information will not be required within this substructure. This reduces the size of the substructure database significantly for a large substructure because the information that is required to recover eliminated variables is not stored. However, this information cannot be recreated later except by regenerating the entire substructure with recovery enabled.

SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES (default)

SUBSTRUCTURE GENERATE, RECOVERY MATRIX=NO

Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Whole model

Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle off Evaluate recovery matrix for

SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES, NSET=Node set name

SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES, ELSET=Element set name

Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Region: Node set name

Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Region: Element set name

When frequency-dependent material properties are specified, Abaqus/Standard offers the option of choosing the frequency at which these properties are evaluated for use in substructure generation. If you do not choose the frequency, Abaqus/Standard evaluates the stiffness at zero frequency and does not consider the stiffness contributions from frequency-domain viscoelasticity. If you do specify a frequency, only the real part of the stiffness contributions from frequency-domain viscoelasticity is considered.

SUBSTRUCTURE GENERATE, PROPERTY EVALUATION=frequency

Step module: Step editor: Substructure generate: Options tabbed page: toggle on Evaluate frequency-dependent properties at frequency: frequency

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 might 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.

In a substructure generation analysis, you can specify a set of elements to define the coarse geometric representation of the substructure in the usage analysis. The nodes of these elements must have displacement degrees of freedom. This element set can include any 2-node elements (truss, beam, connector, etc.) and 3- or 4-node elements with two-dimensional geometry (surface, membrane, shell).

To define the substructure coarse geometric shape, you can specifically add elements that do not change the mechanical behavior of the model (for example, connector elements not associated with any connector behavior definition, surface elements, etc.). If these elements introduce new nodes rather than using nodes from existing elements, the new nodes must be connected to existing elements with significant mechanical properties. In this way, the new nodes used for defining the geometric shape also follow the model deformation.

*SUBSTRUCTURE GENERATE, DISPLAY ELSET=element_set_name

Specifying the display element set is not supported in Abaqus/CAE.

In a substructure generation analysis, you can specify a set of nodes for which to monitor the solution within the substructure in the usage analysis. The selected nodes can have any degrees of freedom (for example, translations, rotations, acoustic pressure, etc.).

*SUBSTRUCTURE GENERATE, MONITOR NSET=node_set_name

Abaqus limits the substructure size to 16,384 degrees of freedom (including retained nodal and generalized degrees of freedom) for substructures used in Abaqus and to 46,340 degrees of freedom for substructures generated in Abaqus and used outside of Abaqus, such as for flexible body dynamics workflows. Abaqus exits with an error message if you request generation of a substructure with more than 46,340 degrees of freedom.

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 might 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 nonphysical 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 stiffness matrix for a substructure. The default behavior is based on whether Abaqus/Standard uses the symmetric or unsymmetric solver for the current analysis step (see Matrix Storage and Solution Scheme in Abaqus/Standard). A symmetric instance of the substructure's reduced stiffness matrix is generated when Abaqus/Standard uses the symmetric solver. An unsymmetric instance of the substructure's reduced stiffness matrix is generated when Abaqus/Standard uses the unsymmetric solver.

You can modify this behavior to generate a symmetric instance, an unsymmetric instance, or both a symmetric and an unsymmetric instance of the reduced stiffness matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver. For acoustic-structural substructures, you can modify the default behavior only for those substructures generated using coupled modes.

If the global stiffness matrix of the model involves any unsymmetry, the symmetric instance of the reduced stiffness matrix generated in a step using the unsymmetric solver might not be equivalent to the symmetric instance of the reduced stiffness matrix generated in a step using the symmetric solver. The same is true about the unsymmetric instance of the reduced stiffness matrix generated in a step using the symmetric solver and the unsymmetric instance of the reduced stiffness matrix generated in a step using the unsymmetric solver.

For models with some sources of unsymmetry in stiffness (for example, models including sliding contact with friction), generating both the symmetric and unsymmetric instances of the reduced stiffness matrix can be beneficial at the usage level. Benefits at the usage level include the following:

• When a substructure generated with only an unsymmetric reduced stiffness matrix is used in an eigenfrequency analysis, Abaqus/Standard performs an averaging-based symmetrization of the unsymmetric stiffness matrix. The symmetric matrix is used for frequency extraction, and the eigenfrequencies that the procedure yields can be unphysical for some models. However, when a substructure generated with both the symmetric and unsymmetric instances of the stiffness matrix is used, appropriate instances of the stiffness matrix are chosen for the procedures in which you use the substructure. For example, an eigenfrequency procedure uses the symmetric instance of the stiffness matrix, and a static analysis using the unsymmetric solver uses the unsymmetric instance of the stiffness matrix.
• When a substructure generated with both the symmetric and unsymmetric instances of the stiffness matrix is used in a complex frequency extraction procedure, you can perform parametric studies by using a stiffness matrix obtained from a linear combination of the symmetric and unsymmetric instances of the substructure's stiffness matrix.

SUBSTRUCTURE GENERATE, STIFFNESS MATRIX=SYMMETRIC

SUBSTRUCTURE GENERATE,  STIFFNESS MATRIX=UNSYMMETRIC

SUBSTRUCTURE GENERATE,  STIFFNESS MATRIX=BOTH

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 might 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, 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.

A symmetric instance of the reduced structural damping matrix is generated when Abaqus/Standard uses the symmetric solver. An unsymmetric instance of the reduced structural damping matrix is generated when Abaqus/Standard uses the unsymmetric solver. For more information, see Matrix Storage and Solution Scheme in Abaqus/Standard).

You can generate a symmetric instance, an unsymmetric instance, or both a symmetric and an unsymmetric instance of the reduced structural damping matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver. For acoustic-structural substructures, you can generate these instances only for substructures generated using coupled modes.

If the global stiffness matrix of the model involves any unsymmetry, the symmetric instance of the reduced structural damping matrix generated in a step using the unsymmetric solver might not be equivalent to the symmetric instance of the reduced structural damping matrix generated in a step using the symmetric solver. The same is true about the unsymmetric instance of the reduced structural damping matrix generated in a step using the symmetric solver and the unsymmetric instance of the reduced structural damping matrix generated in a step using the unsymmetric solver.

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

SUBSTRUCTURE GENERATE, STRUCTURAL DAMPING MATRIX=SYMMETRIC

SUBSTRUCTURE GENERATE, STRUCTURAL DAMPING MATRIX=UNSYMMETRIC

SUBSTRUCTURE GENERATE, STRUCTURAL DAMPING MATRIX=BOTH

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. If the damping matrix is dependent on the stiffness matrix (for example, Rayleigh damping), the substructure damping matrix is unsymmetric.
• 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.

Unless requested explicitly in the substructure generation procedure, Abaqus/Standard generates a symmetric reduced viscous/structural damping matrix in a step using the symmetric solver and an unsymmetric reduced viscous/structural damping matrix in a step using the unsymmetric solver. To compute a substructure with unsymmetric viscous/structural damping matrices, you can do either of the following:

1. Generate the substructure using the unsymmetric solver. By default, Abaqus/Standard generates an unsymmetric instance of the reduced viscous/structural damping matrices.
2. Generate the substructure using the symmetric solver, and choose to generate a symmetric instance, an unsymmetric instance, or both a symmetric and an unsymmetric instance of the reduced viscous/structural damping matrices, as described in Generating a Reduced Viscous Damping Matrix for a Substructure and Generating a Reduced Structural Damping Matrix for a Substructure.

Option 2 allows you to take advantage of the performance of the symmetric solver while still being able to generate a substructure with unsymmetric viscous/structural damping matrices. The generated unsymmetric viscous/structural damping matrices can differ from those obtained using Option 1 if the model has any sources of unsymmetry in stiffness (for example, the presence of sliding contact with friction).

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 might 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 contains only the contributions due to thermal expansion (see Computing Thermal Strains in Linear Perturbation Steps). If temperature-dependent material 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), 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 

SUBSTRUCTURE LOAD CASE, NAME=name, GENERATE
DSLOAD

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 eigenfrequencies 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

You can add residual modes to the substructure basis to improve the high-frequency dynamic approximation capability of the substructure. The residual modes are computed in previous static perturbation analyses and as the load modes corresponding to the substructure load cases specified in the current substructure generation analysis.

SUBSTRUCTURE GENERATE, NAME=name, RESIDUAL MODES

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 × 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 × 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.

In a substructure generation analysis, the condition number of the substructure stiffness and mass matrices is also calculated. Outliers of the diagonal elements of the substructure stiffness and mass matrices are identified, together with their node and degree-of-freedom labels. This allows you to identify the retained degrees of freedom that can cause poor numerical quality of the substructure.

You can modify the tolerance values to use for the matrix check. If you request the matrix quality check, the check results are printed in the data (.dat) file.

You can decide whether problems reported by the matrix check are treated as errors. By default, problems reported by the matrix check are intended as warnings.

MATRIX CHECK

MATRIX CHECK, ERROR

MATRIX CHECK, REFERENCE NODE=node_id

MATRIX CHECK, TOLERANCE=ON

Abaqus/Standard can generate a flexible body from a substructure. Abaqus/Standard supports generation of several flexible body types for several external flexible body dynamics solvers. The generated flexible body entities are stored in the substructure .sim file, and the postprocessing programs (translators) are available to convert an Abaqus substructure into the conventional flexible body representation of a particular external flexible body dynamics solver.

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