ProductsAbaqus/StandardAbaqus/CAE ## Generating a substructureWhen 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. Input File Usage SUBSTRUCTURE GENERATE, TYPE=Zn Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Substructure generation: n ## Substructure databaseA substructure database is the set of files that describe the mechanical and geometrical properties of a substructure, and Abaqus writes all substructure data to the substructure database during the substructure generation analysis. The substructure database can include files with the following extensions: .sup, .sim, .prt, .mdl, .stt, and .odb; the .sup file is called the substructure library. By default, substructure data are written to a substructure database named jobname (which is the name of the substructure generation job), and the substructure files named jobname.sup, jobname_Zn.sim, jobname_Zn.prt, jobname_Zn.mdl, jobname_Zn.stt, and jobname_Zn.odb. Files with the extensions .sup and .sim are generated for all substructures. Files with the extensions .prt, .mdl, and .stt contain the internal Abaqus database for the finite element model from which a substructure is generated, and they are generated only if the solution within the substructure can be fully or partially recovered. The file with the extension .odb is called the model data file, and it is generated by default if the solution within the substructure can be fully or partially recovered. This file contains the finite element model data required for visualization of results recovered within the substructure. You can control the generation of this file. If the .odb file is not generated, the solution within the substructure can still be visualized in the Visualization module of Abaqus/CAE; however, the element results (for example, stresses) cannot be displayed for some groups of elements (for example, beam and shell elements). A file with the extension .odb cannot be generated for substructures that are generated from two-dimensional finite element models. Several substructures can share a substructure library (.sup) file; however, this practice is not recommended. All other files are individual for each substructure. You can choose to write the data to a user-specified substructure database. If you specify the substructure library name, the files will be named library_name_Zn.sim, library_name_Zn.prt, library_name_Zn.mdl, library_name_Zn.stt, and library_name_Zn.odb. Input File Usage Use the following option to define a substructure library: SUBSTRUCTURE GENERATE, TYPE=Zn, LIBRARY=library_name Use the following option to force generation of the model data file: SUBSTRUCTURE GENERATE, MODEL DATA=ODB Use the following option to suppress generation of the model data file: SUBSTRUCTURE GENERATE, MODEL DATA=NONE Abaqus/CAE Usage `Defining substructure libraries and controlling generation of the model data file are not supported in Abaqus/CAE.` ## Overwriting the substructure data in a libraryIf a substructure generation analysis is rerun using the same jobname without deleting the substructure library and one substructure or more will be regenerated, you must specify that the existing substructures can be overwritten. This requirement also holds true if the jobname is different for the second analysis but the same library_name is specified. Input File Usage SUBSTRUCTURE GENERATE, TYPE=Zn, LIBRARY=library_name, OVERWRITE Abaqus/CAE Usage `Defining substructure libraries is not supported in Abaqus/CAE.` ## Recovery within a substructureBy 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 needed to recover eliminated variables is not stored. However, this information cannot be recreated at a later time except by regenerating the entire substructure with recovery enabled. Input File Usage Use the following option to enable recovery for a substructure: SUBSTRUCTURE GENERATE, TYPE=Zn, RECOVERY MATRIX=YES (default) Use the following option to disable recovery for a substructure: SUBSTRUCTURE GENERATE, TYPE=Zn, RECOVERY MATRIX=NO Abaqus/CAE Usage Use the following option to enable recovery for a substructure: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Whole model Use the following option to disable recovery for a substructure: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle off Evaluate recovery matrix for ## Using the selective recovery methodIf results recovery is desired only at a subset of the internal degrees of freedom, disk usage can be reduced substantially by using the selective recovery method. To enable selective recovery, the region where recovery is desired can be specified directly. Input File Usage Use the following option to define the node set for selective recovery: SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES, NSET=Node set name Use the following option to define the element set for selective recovery: SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES, ELSET=Element set name Abaqus/CAE Usage Use the following option to define the node set for selective recovery: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Region: Node set name Use the following option to define the element set for selective recovery: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Region: Element set name ## Evaluating frequency-dependent material propertiesWhen 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. Input File Usage SUBSTRUCTURE GENERATE, PROPERTY EVALUATION=frequency Abaqus/CAE Usage Step module: Step editor: Substructure generate: Options tabbed page: toggle on Evaluate frequency-dependent properties at frequency: frequency ## Defining the retained degrees of freedomThe 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. Input File Usage RETAINED NODAL DOFS Abaqus/CAE Usage Load module: boundary condition editor: Category: Mechanical: Types for Selected Step: Retained nodal dofs ## Preventing the degrees of freedom from being sortedYou can prevent the degrees of freedom from being sorted. The ordering of the nodes when using a substructure is then the same as the ordering used when specifying the retained nodes. Input File Usage RETAINED NODAL DOFS, SORTED=NO Abaqus/CAE Usage `You cannot prevent retained nodes from being sorted in Abaqus/CAE.` ## Retaining degrees of freedom when the substructure is intended for geometrically nonlinear analysis at the usage levelWhen the substructure is intended for use in geometrically nonlinear analyses, it is recommended to retain all translational and/or all rotational degrees of freedom from a particular node. Even in the case when only a single translational/rotational degree of freedom of a particular node is deemed as needed at the usage level, you should retain all translational/rotational degrees of freedom associated with that node. Otherwise, as the substructure rotates during a geometrically nonlinear analysis, local numerical instabilities (negative eigenvalues) may occur since the rotated substructure may have no stiffness in particular degrees of freedom. You must choose an appropriate number of nodes that will allow for the computation of an equivalent rigid body motion of the substructure. In two-dimensional or axisymmetric analyses, retaining two nodes with all translational degrees of freedom or one node with all translational and rotational degrees of freedom is sufficient to compute an equivalent rigid body motion of the substructure at the usage level. In three-dimensional analysis, three non-colinear nodes with all translational degrees of freedom retained or one node with all translations and rotations are needed. If the retained nodes are colinear or fewer than three nodes are retained, you must retain at least one node with all rotational degrees of freedom. When Abaqus/Standard cannot compute an equivalent rigid body motion for the substructure during the analysis at the usage level because the number of retained degrees of freedom is not appropriate, a warning message is issued and any geometrically nonlinear effects associated with the substructure are ignored. ## Defining kinematic constraintsKinematic constraints are defined as described in About Kinematic Constraints. The following rules apply: -
All kinematic boundary conditions associated with degrees of freedom that are not retained must be specified when the substructure is generated. The conditions are built into the substructure and remain imposed any time that it is used. Once the substructure is generated, kinematic constraints on internal variables cannot be respecified; they can be modified or removed only by erasing and recreating the substructure in the library. The magnitude of a prescribed boundary condition applied to an internal degree of freedom can be associated with a substructure load case and can be changed at the usage level. The restraint itself is built into the substructure and cannot be removed by omitting a reference to the load case. -
During substructure generation, multi-point constraints in which some of the substructure's retained degrees of freedom are eliminated in favor of internal degrees of freedom must be avoided. If it is desirable to retain certain degrees of freedom that are eliminated by the multi-point constraints, you must reassign all of the variables appearing in the multi-point constraints as retained degrees of freedom and impose the constraints at the usage level.
## Defining the generalized degrees of freedomAn 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. ## Selecting the modes to be used in a substructure generation analysis by their mode numbersYou can directly specify the eigenmodes to be used in a substructure generation analysis by their mode numbers. Input File Usage SELECT EIGENMODES eigenmode 1, eigenmode 2, etc. Abaqus/CAE Usage Use the following option to generate the list of eigenmodes by mode range, with each row in the data table specifying a single mode number. The starting mode number and ending mode number in each row should be equal, and the increment value should be zero. Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Specify retained eigenmodes by: Mode range: Start Mode: eigenmode 1: End Mode: eigenmode 1: Increment: 0Start Mode: eigenmode 2: End Mode: eigenmode 2: Increment: 0etc. ## Generating a list of the eigenmodes by mode rangeInstead of listing all the retained eigenmode numbers, you can generate the list of eigenmodes. Input File Usage Use the following option to generate the list of eigenmodes by mode range, with each data line specifying the start mode number, the end mode number, and the increment in mode numbers between these two values: SELECT EIGENMODES, GENERATE first mode number, last mode number, increment Abaqus/CAE Usage Use the following option to generate the list of eigenmodes by mode range, with each row in the data table specifying the start mode number, the end mode number, and the increment in mode numbers between these two values: Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Specify retained eigenmodes by: Mode range: Start Mode: first mode number: End Mode: last mode number: Increment: increment ## Generating a list of the eigenmodes by frequency rangeYou can select all the modes from the specified frequency range including frequency boundaries. Input File Usage Use the following option to generate the list of eigenmodes by frequency range, with each data line specifying the lower boundary of the frequency range and the upper boundary of the frequency range: SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE lower boundary of the frequency range, upper boundary of the frequency range Abaqus/CAE Usage Use the following option to generate the list of eigenmodes by frequency range, with each row in the data table specifying the lower boundary of the frequency range and the upper boundary of the frequency range: Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Specify retained eigenmodes by: Frequency range: Lower Frequency: lower boundary of the frequency range: Upper Frequency: upper boundary of the frequency range ## Preloading a substructureSubstructures 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. ## Computation of the total response of a variableAny recovered response variable within a substructure (such as stress or displacement) is defined to be a perturbation (with some exceptions for geometrically nonlinear analyses) from the preloaded base state. For geometrically nonlinear analyses, the displacement output includes both the equivalent rigid body rotation and translation associated with the substructure and the strain-inducing small-displacement perturbation. If the total response of a variable is desired, it can be computed by adding the perturbation result to the final result computed during the substructure preload. ## Computation of the tangent stiffness of a preloaded substructureThe rules for calculating the stiffness matrix of a preloaded substructure are the same as those for a static linear perturbation step. See General and perturbation procedures for a detailed description of the rules. ## Defining a preloading historySpecify the loading history that defines the preload state for a substructure. Input File Usage Use the following options: STEP Options to define the preloading history. END STEP Any number of steps can be defined. STEP SUBSTRUCTURE GENERATE Options to define the substructure. END STEP Abaqus/CAE Usage The Substructure generation step must be defined after the preloading steps in an Abaqus/CAE analysis. ## Prescribing boundary conditions at retained degrees of freedom during preloading stepsDuring substructure preloading, boundary conditions can be prescribed at retained degrees of freedom. When the preloaded substructure is subsequently created in a substructure generation step, you must release all the retained degrees of freedom (see Removing boundary conditions). An error message will be issued if some of the retained degrees of freedom are not released. The reaction forces at the released degrees of freedom become concentrated loads that are in equilibrium with the stresses within the substructure. These concentrated loads cannot be removed without changing the preload. The preloaded substructure is, thus, in equilibrium. If the preload in a substructure must effectively apply loading to other parts of the structure, a substructure load case corresponding to the loads applied in the preload history must be created. The technique is demonstrated in Analysis of a rotating fan using substructures and cyclic symmetry. ## Generating a reduced mass matrix for a substructureYou 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. Input File Usage SUBSTRUCTURE GENERATE, TYPE=Zn, MASS MATRIX=YES Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced mass matrix ## Generating a reduced viscous damping matrix for a substructureYou can generate a reduced viscous damping matrix for a substructure. The reduced viscous damping matrix is calculated in a manner similar to that used for the reduced mass matrix. Input File Usage SUBSTRUCTURE GENERATE, TYPE=Zn, VISCOUS DAMPING MATRIX=YES Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced viscous damping matrix ## Generating a reduced structural damping matrix for a substructureYou 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. Input File Usage SUBSTRUCTURE GENERATE, TYPE=Zn, STRUCTURAL DAMPING MATRIX=YES Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced structural damping matrix ## Generating substructures with unsymmetric damping matricesWhen 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 viscous damping matrix will be unsymmetric if a substructure is generated from the rolling tire. 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 damping matrices with unsymmetric contributions. ## Defining substructure load cases for subsequent loading in an analysisThe 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. Input File Usage Use the following options: SUBSTRUCTURE LOAD CASE, NAME=name CLOAD and/or DLOAD and/or DSLOAD and/or TEMPERATURE The load case defined via the SUBSTRUCTURE LOAD CASE option ends when an option other than CLOAD, DLOAD, DSLOAD, or TEMPERATURE is encountered. The load definitions can be specified in any order. Abaqus/CAE Usage Use the following option to define a substructure load case and the loads included in it: Load module: Create Load Case: click the Add button: select loads ## Defining boundary conditionsAll boundary conditions to be built into the substructure matrices must be specified using a boundary condition definition. These cannot be part of a substructure load case specification. Once a kinematic boundary condition is specified on a particular nodal degree of freedom, it is built into the substructure matrices, is in effect for all load cases, and cannot be removed (or redefined at the usage level). The boundary conditions specified as part of the preloading history are built into the substructure matrices. If there is any doubt whether a restraint is permanent or not, it is better to make the degree of freedom a retained degree of freedom and not specify any restraint in the substructure definition. The restraint can then be included as needed in each analysis step. ## Load cases when the substructure is used in geometrically nonlinear analysesAll loads included in a substructure load case at the generation level and applied as a substructure load at the usage level are applied in a local system associated with the substructure. Since this system rotates with the substructure when large motions are present, these loads will rotate as well. As a consequence, you should be careful when using substructure load cases in geometrically nonlinear analyses to ensure that the loading is in the appropriate direction at the usage level. This situation is similar to rotating the substructure using a substructure property definition. ## Gravity loadingTo apply gravity loading, density must be defined for at least some of the elements included in the substructure. A gravity load can be applied to a substructure in two different ways with two different interpretations. If a distributed load definition is used as a part of a substructure load case during substructure generation (as described in Defining substructure load cases for subsequent loading in an analysis above), the gravity loading becomes part of the substructure load case and, hence, rotates to follow the substructure's local system during usage (the local system may rotate by rotating the substructure via a substructure property definition or due to geometrically nonlinear response). To define gravity loading that acts in a fixed global direction during usage, you can request that the substructure's gravity load vectors be calculated during substructure generation. In this case gravity loading should not be defined as part of a substructure load case. When the gravity load vectors are calculated, Abaqus/Standard generates a gravity load vector for each global direction (three for three-dimensional analyses and two for two-dimensional/axisymmetric analyses). At the usage level, a distributed load definition can be used (see Gravity loading) to specify gravity loading on the substructure that acts in a fixed global direction with the specified magnitude. Input File Usage Use the following option to calculate the substructure's gravity load vectors during substructure generation: SUBSTRUCTURE GENERATE, GRAVITY LOAD=YES Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute gravity load vectors ## Substructure eigenvalue problemWe 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. Input File Usage Use the following option to enable solving of the substructure eigenvalue problem: SUBSTRUCTURE GENERATE, EIGENPROBLEM=YES (default) Use the following option to disable solving of the substructure eigenvalue problem: SUBSTRUCTURE GENERATE, EIGENPROBLEM=NO Abaqus/CAE Usage Disabling the substructure eigenvalue problem solution is not supported in Abaqus/CAE. When it is possible, the substructure eigenvalue problem is solved. ## Checking generated substructure matricesIn 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. Input File Usage Use the following option to request the matrix check: MATRIX CHECK Use the following option to specify the center of rotation of the coordinate frame to be used for the matrix check: MATRIX CHECK, REFERENCE NODE=node_label Abaqus/CAE Usage Checking generated substructure matrices is not supported in Abaqus/CAE. ## Generating a flexible bodyAbaqus/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. Input File Usage Use the following option to generate flexible body entities for the ADAMS™ flexible body dynamics solver from MSC.Software Corporation: FLEXIBLE BODY, TYPE=ADAMS Use the following option to generate the CON6 flexible body entities for the AVL EXCITE™ flexible body dynamics solver from AVL LIST GmbH: FLEXIBLE BODY, TYPE=EXCITE Use the following option to generate a generic flexible body (default): FLEXIBLE BODY, TYPE=GENERIC Use the following option to generate the Standard Input Data representation of the flexible body: FLEXIBLE BODY, TYPE=SID Use the following option to generate flexible body entities for the Simpack flexible body dynamics solver: FLEXIBLE BODY, TYPE=SIMPACK Abaqus/CAE Usage Generating a flexible body from a substructure is not supported in Abaqus/CAE. ## Writing the recovery matrix, reduced stiffness matrix, mass matrix, load case vectors, and gravity vectors to a fileYou 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 output to write out: 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. Input File Usage SUBSTRUCTURE MATRIX OUTPUT, MASS=YES, RECOVERY MATRIX=YES, SLOAD=YES, STIFFNESS=YES, GRAVITY LOAD=YES Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Whole model or Region ## Writing the records to the Abaqus/Standard results fileBy default, the requested matrices are written to the Abaqus/Standard results file corresponding to the substructure generation input file name. The record formats for the results file are described in Results file output format. The file can be written in either binary or ASCII format (About Output). Input File Usage SUBSTRUCTURE MATRIX OUTPUT, OUTPUT FILE=RESULTS FILE Abaqus/CAE Usage Abaqus/CAE automatically writes the requested matrices to the Abaqus results file when you run an analysis with a Substructure generation step. ## Writing the records to a user-defined fileYou can specify the name of the file (without an extension) to which the data will be written. The records are written to be compatible with a linear user-defined element. The record formats are described in User-defined elements. An .mtx extension will be added to the file name specified. Input File Usage SUBSTRUCTURE MATRIX OUTPUT, OUTPUT FILE=USER DEFINED, FILE NAME=file_name Abaqus/CAE Usage Job module: job editor: Name ## Managing substructures inside librariesSubstructures 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. Input File Usage Use any of the following options (described in detail below) to perform housekeeping functions on substructure libraries: SUBSTRUCTURE COPY SUBSTRUCTURE DELETE SUBSTRUCTURE DIRECTORY The housekeeping options can appear anywhere within the model portion of the input file (Abaqus Model Definition). An input file can consist of merely the HEADING option and one or more of the housekeeping options. In this case the files and substructures to which the housekeeping options refer must exist at the start of the analysis. Abaqus/CAE Usage `Substructure libraries are not supported in Abaqus/CAE.` ## Listing the substructures stored in a substructure libraryYou can obtain a summary of information about the substructures stored in a substructure library. If necessary, you can identify a nondefault name for the library (the default name is jobname). Input File Usage SUBSTRUCTURE DIRECTORY, LIBRARY=substructure_library_name Abaqus/CAE Usage `Substructure libraries are not supported in Abaqus/CAE.` ## Removing a substructure from a substructure libraryYou can remove a specified substructure from a substructure library. If necessary, you can identify the name of the library. Input File Usage SUBSTRUCTURE DELETE, TYPE=Zn, LIBRARY=substructure_library_name Abaqus/CAE Usage `Substructure libraries are not supported in Abaqus/CAE.` ## Copying or moving a substructure definitionYou can copy a substructure definition from one library to another or from one substructure to another within the same library. You must identify the substructure being copied and assign a name to the substructure being created. When copying substructures from library to library, you can identify the name of the library containing the substructure being copied. Similarly, you can identify the name of the new library to which the substructure will be copied. This new library need not exist prior to the substructure being copied; it will be created in this case. If the original substructure is to be deleted, you can follow the copy with a delete (see above). Input File Usage SUBSTRUCTURE COPY, OLD TYPE=Zn, NEW TYPE=Zn, OLD LIBRARY=substructure_library_name, NEW LIBRARY=substructure_library_name Abaqus/CAE Usage `Substructure libraries are not supported in Abaqus/CAE.` ## Renaming substructure librariesOnce a substructure library has been generated, the disk file should not be renamed manually. To rename a substructure library, copy the existing substructures to a new library. The new library need not exist prior to the first substructure being copied. You can then delete the original disk file manually if you do not need it anymore. |