Using Substructures

Substructures

Substructures are collections of elements from which the internal degrees of freedom have been eliminated. Retained nodes and degrees of freedom are those that are recognized externally at the usage level (when the substructure is used in an analysis), and they are defined during generation of the substructure. Factors that determine how many and which nodes and degrees of freedom should be retained are discussed below and in Generating Substructures.

A substructure can be considered as a special type of element (and is sometimes referred to as a superelement). The retained nodes of a substructure form its connectivity. Multiple instances of a substructure (superelement) can appear in a model.

Why Use Substructures?

There are a number of good reasons to use substructures.

Computational Advantages

System matrices (stiffness, mass) are small as a result of substructuring. Subsequent to the creation of the substructure, only the retained degrees of freedom and the associated reduced stiffness (and mass) matrix are used in the analysis until it is necessary to recover the solution internal to the substructure.
Efficiency is improved when the same substructure is used multiple times. The stiffness calculation and substructure reduction are done only once; however, the substructure itself can be used many times, resulting in a significant savings in computational effort.
Substructuring can isolate possible changes outside substructures to save time during reanalysis. During the design process large portions of the structure will often remain unchanged; these portions can be isolated in a substructure to save the computational effort involved in forming the stiffness of that part of the structure.
In a problem with local nonlinearities, such as a model that includes interfaces with possible separation or contact, the iterations to resolve these local nonlinearities can be made on a very much reduced number of degrees of freedom if the substructure capability is used to condense the model down to just those degrees of freedom involved in the local nonlinearity.

Organizational Advantages

Substructuring provides a systematic approach to complex analyses. The design process often begins with independent analyses of naturally occurring substructures. Therefore, it is efficient to perform the final design analysis with the use of substructure data obtained during these independent analyses.
Substructures provide a clean and simple way of sharing structural information. In large design projects large groups of engineers must often conduct analyses using the same structures.
Many practical structures are so large and complex that a finite element model of the complete structure places excessive demands on available computational resources. Such a large linear problem can be solved by building the model, substructure by substructure, and stacking these level by level until the whole structure is complete and then recovering the displacements and stresses locally, as required.

Substructure Size

The retained nodal degrees of freedom and the generalized degrees of freedom associated with the substructure dynamic modes form a full set of the substructure degrees of freedom. The total number of substructure degrees of freedom is called the substructure size. 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 (see Generating a Flexible Body).

Valid Procedures

Substructures can be used without restriction in the following procedures:

Substructures can also be used in the following procedures, but recovery of eliminated degrees of freedom is not supported:

Using Substructures in Static Analysis

Substructuring introduces no additional approximation in linear static structural analysis: the substructure is an exact representation of the linear, static behavior of its members. The principal drawback to the use of substructures in stress/displacement analyses is that a substructure's stiffness matrix is fully populated (no zero terms) and, therefore, may be very large if the substructure has a large number of retained degrees of freedom. This, in turn, may mean that the wavefront of the model within which substructures are used may be large, thus leading to long computer times to solve the equations.

This difficulty can often be avoided by choosing the substructure's boundaries carefully or by reusing several smaller substructures rather than a single larger substructure. In some cases it is possible to take advantage of the fact that Abaqus/Standard allows individual degrees of freedom to be retained, rather than the whole set of degrees of freedom at a node. For example, in contact problems without friction only the displacement component normal to the surface need be retained for the contact solution. Nodal transformations can be helpful in orienting the displacement components at surface nodes for this purpose (see Transformed Coordinate Systems).

In a static analysis involving a substructure containing acoustic elements, the results will differ from the results obtained in an equivalent static analysis without substructures. The acoustic-structural coupling is taken into account in the substructure (leading to hydrostatic contributions of the acoustic fluid), while the coupling is ignored in a static analysis without substructures.

Using Substructures in Dynamic Analysis

Substructures introduce approximations in dynamic analysis. The default approach to the dynamic representation of a substructure is to reduce its mass and damping matrix with the same transformation as is used for its stiffness matrix, which is known as “Guyan reduction.” This approach assumes that the response between the eliminated and retained degrees of freedom is correctly represented by the static modes only. This representation may not be accurate if dynamic modes within the substructure are important. The dynamic representation may be improved for Guyan reduction by retaining additional physical degrees of freedom that are not required to connect the substructure to the rest of the model. For example, if the substructure is a plate or a beam, some transverse displacements (and, perhaps, in-surface rotation components) might be included as retained degrees of freedom for this purpose. For more details regarding Guyan reduction, see Substructuring and substructure analysis.

“Dynamic mode addition” can be used as an alternative to Guyan reduction. This approach involves adding generalized degrees of freedom associated with the eigenmodes extracted for the substructure. This improves dynamic behavior, but it introduces the additional cost of extracting the eigenmodes for the constrained substructure. For more details regarding dynamic mode addition, see Substructuring and substructure analysis.

The reduction methods can be applied simultaneously to different substructures within the same structure. Definition of the reduced mass matrix is discussed further in Generating Substructures.

Using Substructures in Geometrically Nonlinear Stress/Displacement Analysis

Substructures may undergo large motions if geometric nonlinearities are considered in a particular stress/displacement analysis (see About Static Stress Analysis Procedures). Abaqus/Standard will account for the large rigid body rotations and translations of the substructure. However, the substructure is assumed to undergo small (linear elastic) deformations at all times during the geometrically nonlinear analysis. An equivalent rigid body rotation for each substructure is computed during each equilibrium iteration using the retained nodes of the substructure. The substructure's mass, damping, stiffness matrix (including the retained eigenmodes), and force vectors are then rotated appropriately using the equivalent rigid body rotation. Appropriate (rotated) linear perturbation displacements (strain-inducing displacements relative to the rotating reference configuration) are used to compute the internal force associated with the substructure. Degrees of freedom at a node should not be retained selectively if the substructure is to be used in geometrically nonlinear analysis. Coupled acoustic-structural substructures should not be used in geometrically nonlinear analyses.

Comparison with Component Mode Synthesis

The component mode synthesis method has been developed to permit the structure to be subdivided into components (substructures), with most of the analysis being done on the smaller components to develop an approximate model for the entire structure.

The substructures in Abaqus/Standard are, in fact, a particular case of the component mode synthesis method extended to allow for large rotations and translations of the substructure (component) in the geometrically nonlinear analysis. The component mode synthesis method is based on the assumption that the small deformations of a substructure can be modeled using a collection of modes. The most frequently used modes in the literature are typically referred to as follows:

constraint modes, which are static shapes obtained by giving each retained degree of freedom in the substructure a unit displacement while holding all other retained degrees of freedom fixed;
fixed-interface normal modes, which are obtained by fixing the retained degrees of freedom and computing the eigenmodes of the substructure;
free-interface normal modes, which are obtained by computing the eigenmodes of the substructure with free (not fixed) retained degrees of freedom; and
mixed-interface normal modes, which are obtained by fixing a part of the retained degrees of freedom and computing the eigenmodes of the substructure.

The constraint modes are precisely the static modes (see Substructuring and substructure analysis) used by Abaqus/Standard. You include these modes in the substructure's representation by specifying the degrees of freedom that are to be retained (see Defining the Retained Nodal Degrees of Freedom). The fixed-interface, free-interface, or mixed-interface normal modes are the eigenmodes extracted in the eigenfrequency extraction step at the generation level, and these modes represent particular cases of substructure dynamic modes allowed in Abaqus (see Defining the Generalized Degrees of Freedom). You include the dynamic modes in the substructure's representation by selecting the eigenmodes to be used.

Including Substructures in a Model

When a substructure is used in a model, it is assigned an element number and defined by nodes just like any other element.

Use an element definition (Element Definition) with a substructure identifier to include substructures in the definition of another substructure (nested substructure) or in an analysis model.

In the element definition you define the substructure's element number at the usage level and assign node numbers to the substructure's retained nodes. You can define more than one substructure per element definition.

Once a substructure is introduced by an element definition, it is treated like any other element in the model, except that its response can be linear only (although it can be used as a part of a model that includes nonlinear effects, including large displacements).

Using substructures requires that the substructure database be available. All the files generated for the substructure (including the name.sim file and, optionally, the substructure model data file and the name.prt, name.stt, and name.mdl files) must be available if recovering substructure results is performed in the substructure usage analysis.

Abaqus distinguishes between different substructures by their unique substructure names. The substructure name is a significant part of the substructure element definition.

Two methods are available for including substructures in a model: use of the generic substructure element type SUBSTR and use of the Zn-type identifier. Although Abaqus supports both methods, the method using the generic substructure element type SUBSTR is preferred over the method using the Zn-type identification.

Preferred Method for Including Substructures in a Model

The preferred method for including substructures in a model is to associate all elements with the generic substructure element type SUBSTR.

If the substructure database files are located in the user directory, you can specify only the substructure name. If the substructure database files are located outside of the user directory, you must include the absolute or relative path to the file location.

Input File Usage

Use the following option to include one or more substructures in a model:

ELEMENT, TYPE=SUBSTR, FILE=name

Abaqus/CAE Usage

Specifying the generic substructure element type SUBSTR is not supported in Abaqus/CAE.

Alternative Method for Including Substructures in a Model

The alternative method for including substructures in a model is to associate all elements with the Zn type identification. In this method, the substructure name is formed from a prefix and a Zn-type identifier (for example, name_Zn).

Input File Usage

Use the following option to use the alternative method to include a substructure in a model:

ELEMENT, TYPE=Zn, FILE=name

Abaqus/CAE Usage

Use the following option to use the alternative method to include a substructure in a model:

All modules: FileImportPart: File Filter: Substructure

Repeat the import process for each substructure that you want to include in the model.

Ordering of the Substructure Nodes on the Usage Level

The node numbers that are used when a substructure is created and the node numbers that are associated with the substructure when it is used are entirely independent. The ordering of the retained nodes when the substructure is used can be defined in two different ways:

The nodes can be provided in the same order that they were listed in the substructure definition. In this case you must prevent the sorting of the retained nodes when you specify the retained degrees of freedom (see Preventing the Degrees of Freedom from Being Sorted). Duplicate nodes are not combined if the retained nodes are not sorted. Therefore, if the same nodes are specified more than once in the list of retained degrees of freedom to retain different degrees of freedom, the corresponding nodes at the usage level must appear the same number of times.
The substructure nodes must be specified in the same order as the retained nodes sorted into ascending numerical order according to their numbers used within the substructure. This approach is the default when you specify the retained degrees of freedom.

In either case you must ensure that the nodes match up properly whenever a substructure is used.

Interpreting the Model Output in the Data File

Substructures included in the model can have nested substructures; these nested substructure can also have nested substructures as well, up to 20 levels. All of these substructures constitute the substructure tree of the model, which is printed to the data file with the relevant indentation. For each substructure element, the tree shows the substructure element's label, the full name of the associated substructure, and the suffix for the recovery output database name.

If model definition data are written to the data file (Controlling the Amount of analysis input file processor Information Written to the Data File), substructure instances are identified in the data (.dat) file by the substructure identifier followed by an F and two digits that indicate the substructure database number. The full name of the substructure database associated with this number is also contained in the model output.

Defining the Substructure's Properties

You associate a property definition with each substructure in the model. The property definition serves the following purposes:

It defines any translation, rotation, and reflection of the substructure at the usage level.
It allows a tolerance to be set to ensure that the coordinates of the usage level nodes match the coordinates of the nodes used to generate the substructure.
It controls using various sources of substructure damping in the dynamic analysis at the usage level.
It controls the use of frequency-based substructures in direct steady-state dynamic analyses (see Direct-Solution Steady-State Dynamic Analysis).

Input File Usage

SUBSTRUCTURE PROPERTY, ELSET=name

Abaqus/CAE Usage

Use the following options to define translation and rotation of the substructure:

Assembly module: InstanceTranslate or InstanceRotate

Reflection of the substructure is not supported in Abaqus/CAE.

Use the following option to apply constraints that connect the retained nodes with the usage level nodes:

Interaction module: ConstraintCreate

Translating, Rotating, and Reflecting a Substructure

Translation, rotation, and/or reflection (in that order) of a substructure can be specified in a substructure property definition.

Specify a translation by giving a translation vector. Specify a rotation by giving two points, a and b, defining a rotation axis plus a right-handed angular rotation around that axis. Specify a reflection by giving three non-colinear points in the reflection plane.

A translation does not affect the substructure's stiffness or mass: the principal reason to apply a translation is to enable the tolerance check on nodal coordinates as discussed later. Rotation and/or reflection of a substructure affect the substructure's stiffness and mass. The substructure load case definitions are rotated and/or reflected in the same way as the substructure's stiffness and mass; therefore, all loads within substructure load cases are applied in the local directions associated with the substructure when it was created.

For distributed loads (for example, pressure loading of a surface) this application is precisely what is desired. However, distributed body forces in coordinate directions (BX, BY, BZ) are applied in the substructure's local directions instead of in the global directions, which may not be what is needed. Similarly, distributed loadings that depend on position (for example, hydrostatic pressure or centrifugal loads) are based on the substructure's local coordinates and not on the substructure position during usage. Be careful to ensure that loading of a rotated or shifted substructure is correct for its usage.

Whenever a substructure is translated, rotated, and/or reflected, the degrees of freedom at any retained nodes are with respect to the coordinate directions at the usage level. Therefore, if all of the degrees of freedom of a node are not retained or if a two-dimensional substructure is used in a three-dimensional model with rotation out of the x–y plane, additional degrees of freedom may be activated due to rotation and/or reflection. Be careful to check the validity of the substructure usage in such cases.

Setting a Tolerance on the Substructure Nodes

One difficulty with using large substructures is ensuring that the retained nodes in the substructure are connected to the correct nodes on the usage level (after substructure translation, rotation, and/or reflection, if applicable). Therefore, Abaqus/Standard checks that the coordinates of the retained nodes match the coordinates of the corresponding nodes on the usage level. A substructure does not require any coordinates on the usage level because it consists only of a stiffness matrix, a mass matrix, and a number of load cases. Nevertheless, it is usually a good check of a model's validity to verify that the substructure and the model into which it is introduced are geometrically consistent.

To check the coordinates, you can set a tolerance on the distance between usage level nodes and the corresponding substructure nodes. This tolerance indicates the largest deviation allowable before a warning is issued. If you do not specify this tolerance, the default is to use a tolerance of 10⁻⁴ times the largest overall dimension within the substructure. If you specify a tolerance of 0.0, the position of the retained nodes is not checked.

The geometric check is based on the coordinates of the retained nodes after translation, rotation, and/or reflection of the substructure at the usage level; motions of these nodes that occur as a result of geometrically nonlinear preloading during generation of the substructure are not considered in this check.

Input File Usage

SUBSTRUCTURE PROPERTY, ELSET=name, POSITION TOL=tolerance

Abaqus/CAE Usage

Assembly module: InstanceTranslate and InstanceRotate

Defining Substructure Damping

Defining substructure damping at the substructure usage level means defining viscous and structural damping matrices for the finite elements associated with the substructures. Abaqus allows you to choose a particular source of damping for a substructure, to add several sources, or to exclude the damping effects for a substructure at the usage level. All options defining the substructure damping belong to a substructure property definition and affect only the finite elements of the substructure type associated with the substructure property.

Sources of Substructure Damping

You can choose to model the damping of a substructure at the usage stage by using the reduced substructure damping matrices computed during the generation stage and stored on the substructure database. We denote the reduced viscous damping matrix of a substructure as ${\bar{C}}_{r e d u c e d}$ and the reduced structural damping matrix of a substructure as ${\bar{S}}_{r e d u c e d}$ . Alternatively, you can introduce the stiffness and mass proportional damping matrices by multiplying the reduced substructure stiffness and mass matrices, ${\bar{K}}_{r e d u c e d}$ and ${\bar{M}}_{r e d u c e d}$ , respectively, with the factors defined within the substructure property definition at the usage stage. You can also combine both damping sources or exclude the effects of damping altogether at the usage level. Finally, you can introduce viscous and structural modal damping matrices for a substructure specifying damping coefficients for the substructure eigenmodes calculated at the generation stage and stored on the substructure database.

The substructure modal damping contributes to the damping matrices for the finite elements associated with a substructure, and it can be used instead of or together with the other substructure damping sources. To define the substructure modal damping matrix, you specify the diagonal damping matrix on the substructure modal subspace. This matrix is transformed to the substructure degrees of freedom space to be added to the damping matrix of the finite element associated with the substructure.

Controlling the Sources of Substructure Viscous Damping

In the general case the substructure type element viscous damping matrix at the usage stage is defined by the following matrix equation:

$\bar{C} = {\bar{C}}_{r e d u c e d} + α \bar{M} + β \bar{K} + {\bar{C}}_{m o d a l} .$

You can specify substructure viscous damping using substructure damping controls and/or substructure viscous modal damping. If you specify substructure viscous modal damping, it is used in combination with all other activated viscous damping sources to form the viscous damping matrix of the finite element. Defining the substructure viscous modal damping is discussed in more detail in Defining Substructure Viscous Modal Damping below.

Input File Usage

To activate only the generated condensed viscous damping matrix of the substructure (the first term on the right-hand side), use the following option:

SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=ELEMENT

To activate only the stiffness and mass proportional substructure viscous damping, use the following option:

SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=FACTOR

To activate the combined generated and proportional substructure viscous damping matrix, use the following option:

SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=COMBINED

To exclude the effects of generated and proportional substructure viscous damping altogether at the usage level, use the following option:

SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=NONE

To specify the substructure viscous modal damping matrix (the last term on the right-hand side), use the following option:

SUBSTRUCTURE MODAL DAMPING

Abaqus/CAE Usage

Substructure damping controls and substructure modal damping are not supported in Abaqus/CAE.

Controlling the Sources of Substructure Structural Damping

In the general case the substructure type element structural damping matrix is defined by the following equation:

$\bar{S} = {\bar{S}}_{r e d u c e d} + γ {\bar{K}}_{r e d u c e d} + {\bar{S}}_{m o d a l} .$

You can specify substructure structural damping using substructure damping controls and/or substructure structural modal damping. If you specify substructure structural modal damping, it is used in combination with all other activated structural damping sources to form the structural damping matrix of the finite element. Defining the substructure structural modal damping is discussed in more detail in Defining Substructure Structural Modal Damping below.

Input File Usage

To activate only the generated reduced structural damping matrix of the substructure (the first term on the right-hand side), use the following option:

SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=ELEMENT

To activate only the stiffness proportional substructure structural damping matrix, use the following option:

SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=FACTOR

To activate the combined generated and stiffness proportional structural damping matrix, use the following option:

SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=COMBINED

To exclude the generated and stiffness proportional structural damping matrices, use the following option:

SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=NONE

To specify the substructure structural modal damping matrix (the last term on the right-hand side), use the following option:

SUBSTRUCTURE MODAL DAMPING

Abaqus/CAE Usage

Substructure damping controls and substructure modal damping are not supported in Abaqus/CAE.

Defining Substructure Damping Factors

By default, the damping factors, $α$ and $β$ , and the structural damping factor, $γ$ , used to define stiffness proportional and mass proportional damping for a substructure are zeros.

Input File Usage

Use the following options to define the values of the substructure damping factors at the usage level:

SUBSTRUCTURE DAMPING, ALPHA= $α$ , BETA= $β$ , STRUCTURAL= $γ$

Abaqus/CAE Usage

Defining substructure damping factors is not supported in Abaqus/CAE.

Defining Substructure Viscous Modal Damping

Substructure viscous modal damping is defined for the substructure eigenmodes extracted at the substructure generation level. The mode numbers and the eigenfrequencies used to define substructure viscous modal damping come from the solution of the substructure eigenvalue problem at the generation level.

Input File Usage

Use the following option to define the fraction of critical damping for a substructure by specifying mode numbers:

SUBSTRUCTURE MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=MODE NUMBERS

Use the following option to define the fraction of critical damping for a substructure by specifying a frequency range:

SUBSTRUCTURE MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=FREQUENCY RANGE

Use the following option to define substructure modal Rayleigh damping by specifying the substructure mode numbers:

SUBSTRUCTURE MODAL DAMPING, VISCOUS=RAYLEIGH, DEFINITION=MODE NUMBERS

Use the following option to define substructure modal Rayleigh damping by specifying a frequency range:

SUBSTRUCTURE MODAL DAMPING, VISCOUS=RAYLEIGH, DEFINITION=FREQUENCY RANGE

Abaqus/CAE Usage

Substructure modal damping is not supported in Abaqus/CAE.

Defining Substructure Structural Modal Damping

Substructure structural modal damping is defined for the substructure eigenmodes extracted at the substructure generation level. The mode numbers and the eigenfrequencies used to define substructure structural modal damping come from the solution of the substructure eigenvalue problem at the generation level.

Input File Usage

Use the following option to define substructure structural modal damping by specifying mode numbers:

SUBSTRUCTURE MODAL DAMPING, STRUCTURAL, DEFINITION=MODE NUMBERS

Use the following option to define substructure structural modal damping by specifying a frequency range:

SUBSTRUCTURE MODAL DAMPING, STRUCTURAL, DEFINITION=FREQUENCY RANGE

Abaqus/CAE Usage

Substructure modal damping is not supported in Abaqus/CAE.

Controlling the Use of Frequency-Based Substructures

Frequency-based substructures are supported only in direct steady-state dynamic analyses (see Direct-Solution Steady-State Dynamic Analysis). When used at the same frequencies as those used for generation, frequency-based substructures represent the substructure with dynamic exactness. This allows for large models to reduce to very small models without any loss of accuracy. By default, the frequency-based substructure is used only at those frequencies at which the frequency-based substructure is generated (see Generating Frequency-Based Substructures), and the conventional substructure is used at all the nonmatching frequencies. Therefore, the dynamic representation of the substructure is exact at the matching frequencies and is the same as that of the conventional substructure at nonmatching frequencies. The frequency-based substructure operators from the jobname_Zn.sim file obtained from the substructure generation procedure are used.

You can choose to use the frequency-based substructure at all frequencies of a direct steady-state dynamic analysis. However, the response at frequencies that do not match those used at generation is only an approximation. This approximation is based on the averaging of the frequency-based substructure operators corresponding to neighboring frequencies. If the frequency of interest is beyond the range of frequencies at which the frequency-based substructure is generated, this averaging is not possible, and Abaqus issues an error in the jobname.msg file. You can also disable the use of frequency-based substructures at any frequency, even if the frequency-based substructure operators are available in the jobname_Zn.sim file. In this case the conventional substructure is used instead at all frequencies.

Substructure modal damping is allowed only when the substructure does not contain frequency-based substructures or the use of frequency-based substructures is disabled; otherwise, substructure modal damping is ignored. Similarly, substructure loads are allowed in the direct steady-state dynamic analysis only when the substructure does not contain frequency-based substructures or the use of frequency-based substructures is disabled.

Input File Usage

Use the following option to use the frequency-based substructure when frequencies of interest match those frequencies at which the frequency-based substructure is generated and to use the conventional substructure at other frequencies:

SUBSTRUCTURE PROPERTY, ELSET=name, FREQUENCY BASED=MATCHED FREQUENCIES (default)

Use the following option to use the frequency-based substructure at all frequencies:

SUBSTRUCTURE PROPERTY, ELSET=name, FREQUENCY BASED=ALL FREQUENCIES

Use the following option to disable the use of the frequency-based substructure at all frequencies and to use the conventional substructure at all frequencies instead:

SUBSTRUCTURE PROPERTY, ELSET=name, FREQUENCY BASED=NO FREQUENCIES

Abaqus/CAE Usage

Frequency-based substructures are not supported in Abaqus/CAE.

Defining Kinematic Constraints and Transformations

All kinematic boundary conditions, MPCs, and transformations can be applied to retained degrees of freedom at the usage level. These specifications can be changed from step to step in the usual way. In this respect substructures and their retained nodes act in an identical manner to regular elements and their nodes.

Defining Transformations at Retained Nodes

If a nodal transformation (Transformed Coordinate Systems) is used during substructure generation at a retained node, the transformations are built into the substructure. This creates an inconsistency when the substructure node is attached to a standard Abaqus element since Abaqus/Standard uses the retained degrees of freedom directly without checking their directions. Therefore, it is suggested that this situation be avoided.

If a nodal transformation must be used, the resulting inconsistency can be resolved by retaining all degrees of freedom at the node and applying a linear constraint equation (Linear Constraint Equations) as follows. At any point where such a transformed substructure node is attached to a global model, define two coincident nodes on the usage level, P and Q, for example. Use node P for the substructure at the usage level (defined with an element definition); the local directions of the degrees of freedom are already built in at this node. Use node Q for all standard Abaqus elements attached to this point. Use a local transformation at node Q to transform the degrees of freedom to the same local directions that are built-in for node P. Now use a linear constraint equation to equate the individual degrees of freedom at nodes P and Q.

Performing Parametric Studies on the Substructure Stiffness Matrix

You can change the substructure properties to perform parametric studies by controlling the amount of unsymmetry in a substructure stiffness matrix. This feature is allowed only in complex frequency analyses using the unsymmetric solver. You control the unsymmetry by specifying a factor for the unsymmetric part of the substructure stiffness. This feature works only when both a symmetric and an unsymmetric instance of the substructure stiffness matrix are available (see Generating a Reduced Stiffness Matrix for a Substructure).

You specify an element set on which you want to perform parametric studies. Abaqus ignores any elements that are not substructures. You specify the factor of unsymmetry, $α$ , in the equation for the stiffness matrix:

$K = K_{s} + α (K_{u} - K_{s}),$

where

$K$ is the stiffness matrix computed by controlling the stiffness unsymmetry factor, and

$K_{s}$ and

$K_{u}$ are the symmetric and unsymmetric instances, respectively, of the available substructure stiffness matrix.

The default value of the unsymmetry factor is 1.0. You can perform parametric studies on different sets of elements, and the effect of the changes in the stiffness matrix is local to the current step.

Input File Usage

Use the following option to change the substructure properties:

SUBSTRUCTURE CHANGE, ELSET=name, STIFFNESS UNSYMMETRY FACTOR= $α$

Abaqus/CAE Usage

Changing the substructure properties is not supported in Abaqus/CAE.

Applying Loads to a Substructure

Loads that are to be applied to a substructure within an analysis (at the usage level) must be specified during the substructure generation step by defining a substructure load case or by requesting that the substructure's gravity load vectors be calculated (see Defining Substructure Load Cases for Subsequent Loading in an Analysis). A load case can be made up of any combination of loadings, and multiple load cases can be defined for any given substructure.

When you activate load cases created for a substructure, you specify the element number or element set name of the substructures, the associated substructure load case names, and the scaling multipliers for the specified substructure load case loads. To reproduce the loading conditions defined during substructure generation exactly, use a magnitude of 1.0.

Boundary conditions specified during a substructure's generation are always present. They are effectively built into the substructure and cannot be removed. Boundary conditions cannot be specified within the substructure load cases. See Generating Substructures for further information about defining boundary conditions in substructures.

Input File Usage

Use the following option to activate a substructure load case:

SLOAD

Abaqus/CAE Usage

Use the following option to activate a substructure load case:

Load module: load editor: Category: Mechanical: Types for Selected Step: Substructure load

Modifying or Removing Load Cases

By default, substructure loads are applied as modifications of existing loads or in addition to any loads previously defined. You can remove all previously defined loads and, optionally, specify new loads when you activate a load case. Boundary conditions cannot be removed.

Input File Usage

Use the following option to modify load cases:

SLOAD, OP=MOD

Use the following option to remove load cases:

SLOAD, OP=NEW

Abaqus/CAE Usage

Use the following option to modify load cases:

Load module: Load Case Manager: click Edit

Use the following option to remove load cases:

Load module: Load Case Manager: click Delete

Specifying Time-Dependent Load Cases

The magnitude of substructure loads can be varied with time by referring to an amplitude definition (Amplitude Curves).

Input File Usage

Use the following options to define time-dependent load cases:

AMPLITUDE, NAME=amplitude
SLOAD, AMPLITUDE=amplitude

Abaqus/CAE Usage

Use the following options to define time-dependent load cases:

Load module: amplitude editor: Create Amplitude: Amplitude: amplitude

Load module: load editor: Category: Mechanical: Types for Selected Step: Substructure load: Amplitude: amplitude

Load Cases in Geometrically Nonlinear Analyses

All substructure loads and boundary conditions are applied in a local system associated with the substructure. Since this local system rotates with the substructure when large motions are present, these loads and boundary conditions will rotate as well. As a consequence, you should be careful when using substructure loads 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 via a substructure property definition.

Gravity Loading

A distributed load definition can be used to apply gravity loading to a substructure with a user-defined magnitude, scaled by an amplitude definition, and acting in a specified direction. To enable gravity loading for a substructure, you must request the calculation of the substructure's gravity load vectors during the substructure generation step (see Gravity Loading). In this case gravity loading should not be defined as part of a substructure load case.

Input File Usage

Use the following option to define gravity loading:

DLOAD, AMPLITUDE=amplitude
element set or element number, GRAV, magnitude, direction

Abaqus/CAE Usage

Load module: Create Load: choose Mechanical for the Category and Gravity for the Types for Selected Step

Obtaining Output of the Solution for All of the Substructure Degrees of Freedom

The retained nodal degrees of freedom and the generalized degrees of freedom associated with the substructure dynamic modes form the full set of the substructure's degrees of freedom. You can output the solution at all of the substructure degrees of freedom. This feature is available only for Abaqus/Standard transient dynamic analysis; it is not supported for static and linear dynamic analyses. For more information, see Defining the Retained Nodal Degrees of Freedom and Defining the Generalized Degrees of Freedom.

Input File Usage

Use the following option to output the solution for all of the substructure degrees of freedom:

*SUBSTRUCTURE OUTPUT

Abaqus/CAE Usage

Obtaining output of the solution for all of the substructure degrees of freedom is not supported in Abaqus/CAE.

Obtaining Output for Selected Substructures

By default, the output is performed for all substructures in the model. You can output the solution for selected substructures by specifying the element set that contains all the substructure-type elements where you want to output the solution.

Input File Usage

Use the following option to obtain output for a selected subset of substructures in the model:

*SUBSTRUCTURE OUTPUT, ELSET=element set name

Abaqus/CAE Usage

Obtaining output of the solution for all of the substructure degrees of freedom is not supported in Abaqus/CAE.

Obtaining Output in Output4 Format

By default, the substructure solution is stored on SIM, which is a high-performance database available in Abaqus. The substructure output data are stored in files named jobname_STEPn_m.sim, where jobname is the name of the input file or analysis job, n is the number of the Abaqus step that generates the substructure output, and m is the substructure element label defined in the input file. The substructure output data written to SIM can later be converted to one of the conventional text or binary formats as a postprocessing operation.

You can also output the substructure solution in Output4 text format, which can be used, for example, by the MSC Nastran finite element solver from MSC.Software Corporation or by the AVL EXCITE™ flexible body dynamics solver from AVL LIST GmbH. The substructure output data in the OP4 text format are stored in files named jobname_STEPn_m.op4, where jobname is the name of the input file or analysis job, n is the number of the Abaqus step that generates the output, and m is the substructure element label defined in the input file.

Input File Usage

Use the following option to output the solution in Output4 text format:

*SUBSTRUCTURE OUTPUT, FORMAT=OP4

Abaqus/CAE Usage

Obtaining output of the solution for all the substructure degrees of freedom is not supported in Abaqus/CAE.

Obtaining Output of Results within a Substructure

You can obtain output within substructures used in static, dynamic, eigenfrequency extraction, and steady-state and transient modal dynamic analyses. The recovery of output is not possible for substructures used in response spectrum and random response analyses. Output within a substructure does not include the displacements, stresses, etc. resulting from the preload deformation of a substructure. Obtaining output for connector elements in a substructure is not supported in Abaqus/CAE.

Output within substructures is available in the data (.dat) file, in the results (.fil) file, and in output database (.odb) files. Separate output database files are created for each substructure using the naming convention inputfile-name_substructure-number.odb. If a substructure contains a nested substructure, a file called inputfile-name_substructure-number_nested-substructure-number.odb is created containing the output for the nested substructure. The abaqus substructurecombine execution procedure can combine model and results data from two substructure output databases into a single output database. For more information, see Combining Output from Substructures.

Recovery of the solution within substructures requires that the information for recovering the data within a substructure be available from the .sim, .prt, .stt, and .mdl files. Availability of the model data (.odb or .sim) file is not required but is strongly recommended: if this file is not provided, the element results for some element types cannot be displayed in the Visualization module of Abaqus/CAE.

Output is organized substructure by substructure: you direct Abaqus/Standard to go inside a particular substructure and then request output for that substructure. Results can be recovered within nested multilevel substructures only if the substructure databases for all substructures in the chain are available.

Substructure output requests are most easily pictured by thinking of substructures as “levels” of detailed modeling. At the global (top) level we have the analysis model (for example, an airplane). Dropping down from this level to the first substructure level, we have the main components of the model defined as substructures (wings, stabilizer, fuselage, etc.). Dropping down to the second substructure level, we have other substructures (flaps, tanks, floors, etc.), which, in turn, may contain third level substructures (spars, stringers, etc.), and so on. To obtain output, you move down and back up through these various levels using substructure paths, similar to the way you navigate a tree structure for file directories. Each substructure path definition consists of entering into a substructure at the next level down or leaving the current substructure and moving up one level in the tree.

At the start of the output requests, Abaqus/Standard is at the global model level. You must always enter and leave a substructure consistently, so that after a set of substructure output requests Abaqus/Standard is left at the global model level. You must return to the global level (outside all substructures) before the end of the step definition.

If you enter and leave in the same substructure path definition, the effect is to leave the substructure and enter another substructure at the same level.

Entering a Substructure for Output

To enter a particular substructure for output, you identify the substructure by the element number n chosen for it in the model. All subsequent output requests are for output within that substructure and must be given in terms of its internal node and element numbers (the node and element numbers used when the substructure was created).

Input File Usage

SUBSTRUCTURE PATH, ENTER ELEMENT=n

Abaqus/CAE Usage

Step module: field output request editor: Domain: Substructure: click the Edit button, and select substructure sets

Leaving a Substructure after Obtaining Output

After you have obtained output for a substructure, you must return to the level of the model of which the substructure forms a part, thus indicating the end of the output requests for variables within that substructure.

Input File Usage

SUBSTRUCTURE PATH, LEAVE

Abaqus/CAE Usage

Step module: field output request editor: Domain: Substructure: click the Edit button, and select substructure sets

Obtaining Output If Substructures Are Nested

You must enter several substructures if substructures are used at multiple levels and output is required several levels down. Nesting of substructures is not supported in Abaqus/CAE.

Example: Obtaining Output within Nested Substructures

For example, suppose that a model includes several substructures at two levels. Printed output of stress components is required in some elements within two substructures at the second level, as well as printed output of the displacements at some of the nodes of one of the first-level substructures. (Recall that “first-level” refers to substructures used directly in the analysis model; “second-level” substructures are used as components of first-level substructures.)

The data might be as follows:

SUBSTRUCTURE PATH, ENTER ELEMENT=N
** This option takes us into element number N, which must be a substructure.
SUBSTRUCTURE PATH, ENTER ELEMENT=M
** We now drop down into element number M of this substructure.
** M is the element number used for this substructure when N was created.
** M must refer to a substructure.
EL PRINT, ELSET=A1
S
** This option requests stress output in element set A1 of this substructure.
** This element set must have been defined during the creation of substructure M.
SUBSTRUCTURE PATH, LEAVE
** This option takes us back up into first-level substructure N.
SUBSTRUCTURE PATH, ENTER ELEMENT=P
** This option takes us down into element P, which must again be a substructure in element N.
EL PRINT, ELSET=A1
S
** This option requests the printing of stress output in element set A1. It is possible that
** this is the same set of elements in the same substructure as was used in the request above
** because substructures M and P may both be copies of the same substructure.
** However, the stresses will presumably be different because they represent the same
** component in different locations in the model.

SUBSTRUCTURE PATH, LEAVE
** Back to N.
SUBSTRUCTURE PATH, LEAVE
** We are now back at the global level.
SUBSTRUCTURE PATH, ENTER ELEMENT=R
** Enter element R at the global level: this element is the substructure in which we want
** to print the displacements.
NODE PRINT, NSET=FLANGE
U
** This option prints the displacements at all nodes in node set 
** FLANGE of the substructure.
** Again, FLANGE  must have been defined when the substructure was
** created.
SUBSTRUCTURE PATH, LEAVE
** Back to the global level.

Interpreting Nodal Variable Output

The nodal displacements within the substructure do not include the displacements resulting from the preload deformation if it exists.

If a substructure is rotated and/or reflected, nodal variables are output relative to the global coordinate system of the analysis. In a geometrically nonlinear analysis, the nodal displacements will include the large motions associated with the translation and rotation of the substructure in addition to the small-strain displacements. If a nodal transformation (Transformed Coordinate Systems) has been used, nodal output will be in either the local or the global directions, depending on the nodal output request (see Output to the Data and Results Files). If a nodal transformation has been used during substructure generation, the transformed directions are rotated with the substructure.

Interpreting Element Variable Output

Element output variables within a substructure do not include the values of the variable resulting from the preload deformation if it exists.

Element variables in continuum elements are output relative to the global coordinate system of the analysis model or in the local (material) coordinate system if one has been used (Orientations). Element output for structural elements is always given with respect to the element coordinate system used during substructure generation. Integration point coordinates and local material directions (see Output to the Data and Results Files) are given with respect to the global coordinate system.

Element quantities associated with nonlinear preload response (plastic strains, creep strains, etc.) can be output during a substructure recovery. Since the response in a substructure during its usage is entirely linear, these quantities, which are part of the base state, do not change from the values computed during the preload.

If a substructure was reflected, the element connectivities of continuum elements written to the substructure instance output database are adjusted so as not to violate the Abaqus convention for counterclockwise element numbering.

You cannot directly obtain the element output for the element centroidal values or the element output at the element nodes when you recover results within substructures. This output data can be calculated from the substructure-related data in the output database file using commands in the Abaqus Scripting Interface.

Interpreting Results Written to the Results File

Results within substructures can be written to the results file. Substructure path records are inserted in the results file to indicate the switch into a substructure: all records following such a record belong to the substructure defined on that record until the next substructure path record appears in the file.

Requests for output to the results file will cause Abaqus/Standard to write the definitions of elements and nodes at the global level and within all substructures in the model to the file. As with the results records themselves, these records for nodes and elements within substructures will be preceded and followed by substructure path records to indicate that they belong to that substructure.

Node and element numbers within each substructure are local to that substructure, so that the same node and element numbers may appear in several substructures and in the global level model. In such a case the substructure path records must be used to identify the location of a particular node or element within the model. If you can ensure that node and element numbers are unique throughout the entire model, including all substructures, the substructure path records in the results file can be ignored.

Visualizing Substructure Results

While Abaqus/CAE does not support substructures directly, you can view substructure results by combining all of the substructure instance output database (.odb) files into a single file. See Combining Output from Substructures for details.

You can also load and view each individual substructure instance output database (.odb) file separately in Abaqus/CAE.

Substructure Compatibility

Only the substructure SIM database (.sim) and the model data (.odb or .sim) files are backward compatible. If these files were generated from a previous general release or from a previous maintenance delivery of the same general release, they can be upgraded to the current release (see SIM Database Utilities and Output Database Upgrade Utility). Other substructure files (including the .stt, .prt, and .mdl files) are not compatible between maintenance deliveries of the same general release. These files are required only if recovering results within substructures is performed in the substructure usage analysis. When recovering results, you must regenerate your substructures in the current release.

Input File Template

The following template can be used to generate a substructure:

HEADING
…
NODE,NSET=N1
Data lines to define the nodes.
…
NSET,NSET=N3
Data lines to define the node set members.
…
ELEMENT, TYPE=CPE8, ELSET=E1
Data lines to define the elements that make up the substructure.
…
ELSET,ELSET=E3
Data lines to define the element set members.
…
SOLID SECTION, ELSET=E1, MATERIAL=M1
MATERIAL, NAME=M1
ELASTIC
30.E6, 0.3
DENSITY
0.0007324
STEP
FREQUENCY
Data line to specify the number of modes (  $\geq$  m). The FREQUENCY option
is required if modes are requested using the SELECT EIGENMODES option.
END STEP
STEP
STATIC
…
Options to define a linear or nonlinear static preload.
…
END STEP
STEP
SUBSTRUCTURE GENERATE, NAME=MY_SUBSTRUCTURE, OVERWRITE, MASS MATRIX=YES,
VISCOUS DAMPING MATRIX=YES, STRUCTURAL DAMPING MATRIX=YES,
RECOVERY MATRIX=YES, NSET=N3, ELSET=E3
RETAINED NODAL DOFS
Data lines to define the retained degrees of freedom.
SELECT EIGENMODES, GENERATE
1, m, 1
SUBSTRUCTURE LOAD CASE, NAME=LOADS
CLOAD
Data lines to define concentrated loading.
DLOAD
Data lines to define distributed loading.
END STEP

The following template can be used to define substructure instances:

HEADING
…
ELEMENT, TYPE=SUBSTR, FILE=MY_SUBSTRUCTURE, ELSET=E2
Data line to define the element.
SUBSTRUCTURE PROPERTY, ELSET=E2
BOUNDARY
…
RESTART, WRITE
STEP
STATIC
…
BOUNDARY
…
SLOAD
E2, LOADS, scale factor
SUBSTRUCTURE PATH, ENTER ELEMENT=n
EL PRINT
S,
NODE PRINT
U,
SUBSTRUCTURE PATH, LEAVE
END STEP
STEP
DYNAMIC
…
BOUNDARY
…
SUBSTRUCTURE PATH, ENTER ELEMENT=n
EL PRINT
S,
NODE PRINT
U, V
SUBSTRUCTURE PATH, LEAVE
END STEP