Using substructures

In the finite element literature substructures are also referred to as superelements. In earlier releases of Abaqus a distinction was made between substructures and superelements. The term “substructure” was used when it was needed to make clear that results were recovered within the substructure. Otherwise, both terms were used interchangeably. To avoid confusion, the term “superelement” will no longer be used.

There are a number of good reasons to use substructures.

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.

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.

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.

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 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.

You can read the substructure definition from a substructure library.

ELEMENT, TYPE=Zn, FILE=substructure_library_name

Substructure libraries are not supported in Abaqus/CAE.

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 library number. The full name of the substructure library associated with this number is also contained in the model output.

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.

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.

SUBSTRUCTURE PROPERTY, ELSET=name, POSITION TOL=tolerance

Assembly module: InstanceTranslate and InstanceRotate

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.

SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=ELEMENT

SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=FACTOR

SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=COMBINED

SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=NONE

SUBSTRUCTURE MODAL DAMPING

SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=ELEMENT

SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=FACTOR

SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=COMBINED

SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=NONE

SUBSTRUCTURE MODAL DAMPING

SUBSTRUCTURE DAMPING, ALPHA=$\alpha$, BETA=$\beta$, STRUCTURAL=$\gamma$

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

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

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

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

SUBSTRUCTURE MODAL DAMPING, STRUCTURAL, DEFINITION=MODE NUMBERS

SUBSTRUCTURE MODAL DAMPING, STRUCTURAL, DEFINITION=FREQUENCY RANGE

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.

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.

SLOAD, OP=MOD

SLOAD, OP=NEW

Load module: Load Case Manager: click Edit

Load module: Load Case Manager: click Delete

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

AMPLITUDE, NAME=amplitude
SLOAD, AMPLITUDE=amplitude

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

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

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.

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 specifed 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.

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

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

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).

SUBSTRUCTURE PATH, ENTER ELEMENT=n

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

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.

SUBSTRUCTURE PATH, LEAVE

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

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.

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.

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.

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.

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.