김경종
18 KiB
10. Modeling Abstractions
Substructuring 10.1
Submodeling 10.2
Generating matrices 10.3
Symmetric model generation, results transfer, and analysis of cyclic symmetry models 10.4
Periodic media analysis 10.5
Meshed beam cross-sections 10.6
Modeling discontinuties as an enriched figure using extended finite element method 10.7
10.1 Substructuring
• “Using substructures,” Section 10.1.1
• “Defining substructures,” Section 10.1.2
10.1.1 USING SUBSTRUCTURES
Products: Abaqus/Standard Abaqus/CAE
References
• “Defining substructures,” Section 10.1.2
• *SLOAD
• *SUBSTRUCTURE PATH
• *SUBSTRUCTURE PROPERTY
• *SUBSTRUCTURE DAMPING
• *SUBSTRUCTURE DAMPING CONTROLS
• *SUBSTRUCTURE MODAL DAMPING
Overview
Substructures:
• allow a collection of elements to be grouped together and all but the retained degrees of freedom eliminated on the basis of linear response within the group;
• are used in the same manner as any of the standard element types in the Abaqus element library once created as described in “Defining substructures,” Section 10.1.2;
• can be used in stress/displacement and in coupled acoustic-structural analyses;
• have linear response but allow for large translations and large rotations;
• are particularly useful in cases where identical pieces appear several times in a structure (such as the teeth of a gear) since a single substructure can be used repeatedly;
• can be translated, rotated with respect to the global system, and reflected in a plane when they are used;
• are connected to the rest of the model by the retained degrees of freedom at the retained nodes;
• may contain a set of internal load cases and boundary conditions that can be activated and scaled;
• can include dynamic effects by including retained eigenmodes; and
• appear to the rest of the model as a stiffness, optional mass, damping, and a set of scalable load vectors.
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 will be 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 “Defining substructures,” Section 10.1.2.
Substructures versus superelements
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.
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.
• Substructure libraries allow analysts to share substructures. In large design projects large groups of engineers must often conduct analyses using the same structures. Substructure libraries provide a clean and simple way of sharing structural information.
• 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.
Valid procedures
Substructures can be used without restriction in the following procedures:
• “Static stress analysis,” Section 6.2.2
• “Implicit dynamic analysis using direct integration,” Section 6.3.2
• “Direct-solution steady-state dynamic analysis,” Section 6.3.4
• “Natural frequency extraction,” Section 6.3.5
• “Complex eigenvalue extraction,” Section 6.3.6
• “Mode-based steady-state dynamic analysis,” Section 6.3.8
• “Transient modal dynamic analysis,” Section 6.3.7
Substructures can also be used in the following procedures, but recovery of eliminated degrees of freedom is not supported:
• “Response spectrum analysis,” Section 6.3.10
• “Random response analysis,” Section 6.3.11
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,” Section 2.1.5).
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,” Section 2.14.1 of the Abaqus Theory Guide.
“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, with all of the physical retained degrees of freedom automatically constrained. 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,” Section 2.14.1 of the Abaqus Theory Guide.
The reduction methods can be applied simultaneously to different substructures within the same structure. Definition of the reduced mass matrix is discussed further in “Defining substructures,” Section 10.1.2.
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 “Static stress analysis procedures: overview,” Section 6.2.1). 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,” Section 2.14.1 of the Abaqus Theory Guide) 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” in “Defining substructures,” Section 10.1.2). 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” in “Defining substructures,” Section 10.1.2). 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,” Section 2.2.1) with a substructure identifier to include substructures in the definition of another substructure (nested substructure) or in an analysis model. The substructure can be read from a substructure library. A maximum of 500 libraries can be accessed to read substructure data within a given analysis.
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. More than one substructure can be defined per element definition.
Once a substructure has been 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 a substructure including the .sup and .sim files and/or the .prt, .stt, and .mdl files must be available.
Input File Usage: Use the following option to include one or more substructures in a model:
*ELEMENT, TYPE=Zn
Abaqus/CAE Usage: Use the following option to include one substructure in a model:
All modules: File→Import→Part: 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” in “Defining substructures,” Section 10.1.2). 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.
Reading the substructure definition from a substructure library
You can read the substructure definition from a substructure library.
Input File Usage: *ELEMENT, TYPE=Zn, FILE=substructure_library_name
Abaqus/CAE Usage: Substructure libraries are not supported in Abaqus/CAE.
Interpreting the model output in the data file
If model definition data are written to the data file (“Controlling the amount of analysis input file processor information written to the data file” in “Output,” Section 4.1.1), 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.
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.
Input File Usage: *SUBSTRUCTURE PROPERTY, ELSET=name