김경종
27 KiB
solving the nonsymmetric tangent matrix at each iteration. Therefore, for example, Abaqus/Standard invokes the symmetric matrix storage and solution scheme automatically in problems with Coulomb friction where every friction coefficient is less than or equal to 0.2, even though the resulting tangent matrix will have some nonsymmetric terms. However, if any friction coefficient is greater than 0.2, Abaqus/Standard will use the unsymmetric matrix storage and solution scheme automatically since it may significantly improve the convergence history. This choice of the unsymmetric matrix storage and solution scheme will consider changes to the friction model. Thus, if you modify the friction definition during the analysis to introduce a friction coefficient greater than 0.2, Abaqus/Standard will activate the unsymmetric matrix storage and solution scheme automatically. In cases in which the unsymmetric matrix storage and solution scheme is selected automatically, you must explicitly turn it off if so desired; it is recommended to do so if friction prevents any sliding motions.
Input File Usage: *STEP, UNSYMM=YES or NO
Abaqus/CAE Usage: Step module: step editor: Other: Storage: Use solver default or Unsymmetric or Symmetric
Rules for using the unsymmetric matrix storage and solution scheme
The following rules apply to matrix storage and solution schemes in Abaqus/Standard:
-
Since Abaqus/Standard provides eigenvalue extraction only for symmetric matrices, steps with eigenfrequency extraction or eigenvalue buckling prediction procedures always use the symmetric matrix storage and solution scheme. You cannot change this setting. In such steps Abaqus/Standard will symmetrize all contributions to the stiffness matrix.
-
In all steps except those with eigenfrequency extraction or eigenvalue buckling procedures, Abaqus/Standard uses the unsymmetric matrix storage and solution scheme when any of the following features are included in the model. You cannot change this setting.
a. Heat transfer convection/diffusion elements (element types DCCxxx)
b. General shell sections with unsymmetric section stiffness matrices (“Three-dimensional conventional shell element library,” Section 29.6.7)
c. User-defined elements with unsymmetric element matrices (“User-defined elements,” Section 32.17.1)
d. User-defined material models with unsymmetric material stiffness matrices (“User-defined mechanical material behavior,” Section 26.7.1, or “User-defined thermal material behavior,” Section 26.7.2)
e. User-defined surface interaction models with unsymmetric interface stiffness matrices (“Userdefined interfacial constitutive behavior,” Section 37.1.6) -
The following features all trigger the unsymmetric matrix storage and solution scheme for the step. You cannot change this setting.
a. Fully coupled thermal-stress analysis, except when a separated solution scheme is specified for the step (“Fully coupled thermal-stress analysis,” Section 6.5.3)
b. Coupled thermal-electrical analysis, except when a separated solution scheme is specified for the step (“Coupled thermal-electrical analysis,” Section 6.7.3)
c. Fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electricalstructural analysis,” Section 6.7.4)
d. Coupled pore fluid diffusion/stress analysis with absorption or exsorption behavior (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1)
e. Coupled pore fluid diffusion/stress analysis (steady-state)
f. Coupled pore fluid diffusion/stress analysis (transient with gravity loading)
g. Mass diffusion analysis (“Mass diffusion analysis,” Section 6.9.1)
h. Radiation view factor calculation controls (“Cavity radiation,” Section 41.1.1)
-
By default, the unsymmetric matrix storage and solution scheme is used for the complex eigenvalue extraction procedure. You can change this setting.
-
In all other cases you can control whether a symmetric or a full matrix storage and arithmetic solution is chosen. If you do not specify the matrix storage and solution scheme, Abaqus/Standard utilizes the value used in the previous general analysis step.
-
If you do not specify the matrix storage and solution scheme in the first step of an analysis, Abaqus/Standard will choose the unsymmetric scheme when any of the following are used:
a. Any Abaqus/Aqua load type
b. The concrete damaged plasticity material model
c. Friction with a friction coefficient greater than 0.2
The default value in the first step is the symmetric scheme for all other cases, except those covered by rules 2 and 3 above and for cases in which a friction coefficient is increased above 0.2 after the first step.
-
For radiative heat transfer surface interactions (“Thermal contact properties,” Section 37.2.1), certain follower forces (such as concentrated follower forces or moments), three-dimensional finite-sliding analyses, any finite sliding in coupled pore fluid diffusion/stress analyses, and certain material models (particularly nonassociated flow plasticity models and concrete) introduce unsymmetric terms in the model’s stiffness matrix. However, Abaqus/Standard does not automatically use the unsymmetric matrix storage and solution scheme when radiative heat transfer surface interactions are used. Specifying that the unsymmetric scheme should be used can sometimes improve convergence in such cases.
-
Coupled structural-acoustic and uncoupled acoustic analysis procedures in Abaqus/Standard generally use symmetric matrix storage and solution. Exceptions are the subspace-based steady-state dynamics or complex frequency procedures used for coupled structural-acoustic problems, where unsymmetric matrices are a consequence of the coupling procedure used in these cases. Using acoustic infinite elements or the acoustic flow velocity option triggers the unsymmetric matrix storage and solution scheme in Abaqus/Standard, except for natural frequency extraction using the Lanczos eigensolver, which uses symmetric matrix operations.
You can choose a double-precision executable (with 64-bit word lengths) for Abaqus/Explicit on machines with a default, single-precision word length of 32 bits (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2). Most new computers have 32-bit default word lengths even though they may have 64-bit memory addressing. The single-precision executable typically results in a CPU savings of 20% to 30% compared to the double-precision executable, and single precision provides accurate results in most cases. Exceptions in which single precision tends to be inadequate include analyses that require greater than approximately 300,000 increments, have typical nodal displacement increments less than 10−6 times the corresponding nodal coordinate values, include hyperelastic materials, or involve multiple revolutions of deformable parts; the double-precision executable is recommended in these cases (for example, see “Simulation of propeller rotation,” Section 2.3.15 of the Abaqus Benchmarks Guide).
You can also run only a part of Abaqus/Explicit using double precision, while using single precision for the rest (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2). These options are described below.
• If double=explicit is used or the double option is specified without a value, the Abaqus/Explicit analysis will run in double precision, while the packager will run in single precision. While this choice would satisfy higher precision needs in most analyses, the data are written to the state (.abq) file in single precision. Moreover, analysis-related computations performed in the packager will still be executed in single precision. Thus, new steps, restart, and import analyses will commence from data that are stored/computed in single precision despite the fact that calculations during the step are performed in double precision. Thus, in general, one can expect somewhat noisy solutions at the beginning of the first step, at step transitions, upon restart, and after import.
• If double=both is used, both the Abaqus/Explicit packager and analysis will run in double precision. This is the most expensive option but will ensure the highest overall execution precision. Analysis database floating point data will be written to the state (.abq) file at the end of packager or of a given step in double precision, thus ensuring in most cases the smoothest transition at step boundaries, upon restart, and after an import.
• There may be cases where the default single precision analysis is inadequate, while the double=both option is too expensive. These are typically models that have complex links of constraints (such as a complex mechanism with connector elements, complex combinations of distributed/kinematic couplings, tie constraints and multi-point constraints, or interactions of such constraints with boundary conditions). For such models it is desirable to solve only the constraints in the model in double precision while the rest of the model is solved in single precision. This combination gives the desired accuracy of the solution while increasing performance compared to a full double precision analysis.
• If double=constraint is used, the constraint packager and constraint solver are executed in double precision, while the remainder of the Abaqus/Explicit packager and analysis are executed in single precision.
• If double=off is used or the double option is omitted (default), both the Abaqus/Explicit packager and the analysis will run in single precision. The double=off option is useful when you want to override the setting in the environment file.
The significance of the precision level is indicated by comparing the solutions obtained with single and double precision. If no significant difference is found between single- and double-precision solutions for a particular model, the single-precision executable can be deemed adequate.
6.1.3 GENERAL AND LINEAR PERTURBATION PROCEDURES
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Defining an analysis,” Section 6.1.2
• “Linear and nonlinear procedures,” Section 14.3.2 of the Abaqus/CAE User’s Guide
Overview
An analysis step during which the response can be either linear or nonlinear is called a general analysis step. An analysis step during which the response can be linear only is called a linear perturbation analysis step. General analysis steps can be included in an Abaqus/Standard or Abaqus/Explicit analysis; linear perturbation analysis steps are available only in Abaqus/Standard.
A clear distinction is made in Abaqus/Standard between general analysis and linear perturbation analysis procedures. Loading conditions are defined differently for the two cases, time measures are different, and the results should be interpreted differently. These distinctions are defined in this section.
Abaqus/Standard treats a linear perturbation analysis as a linear perturbation about a preloaded, predeformed state. Abaqus/Foundation, a subset of Abaqus/Standard, is limited entirely to linear perturbation analysis but does not allow preloading or predeformed states.
General analysis steps
A general analysis step is one in which the effects of any nonlinearities present in the model can be included. The starting condition for each general step is the ending condition from the last general step, with the state of the model evolving throughout the history of general analysis steps as it responds to the history of loading. If the first step of the analysis is a general step, the initial conditions for the step can be specified directly (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1).
Abaqus always considers total time to increase throughout a general analysis. Each step also has its own step time, which begins at zero in each step. If the analysis procedure for the step has a physical time scale, as in a dynamic analysis, step time must correspond to that physical time. Otherwise, step time is any convenient time scale—for example, 0.0 to 1.0—for the step. The step times of all general analysis steps accumulate into total time. Therefore, if an option such as creep (available only in Abaqus/Standard) whose formulation depends on total time is used in a multistep analysis, any steps that do not have a physical time scale should have a negligibly small step time compared to the steps in which a physical time scale does exist.
Sources of nonlinearity
Nonlinear stress analysis problems can contain up to three sources of nonlinearity: material nonlinearity, geometric nonlinearity, and boundary nonlinearity.
Material nonlinearity
Abaqus offers models for a wide range of nonlinear material behaviors (see “Combining material behaviors,” Section 21.1.3). Many of the materials are history dependent: the material’s response at any time depends on what has happened to it at previous times. Thus, the solution must be obtained by following the actual loading sequence. The general analysis procedures are designed with this in view.
Geometric nonlinearity
It is possible in Abaqus to define a problem as a “small-displacement” analysis, which means that geometric nonlinearity is ignored in the element calculations—the kinematic relationships are linearized. By default, large displacements and rotations are accounted for in contact constraints even if the small-displacement element formulations are used for the analysis; i.e., a large-sliding contact tracking algorithm is used (see “Contact formulations in Abaqus/Standard,” Section 38.1.1, and “Contact formulations for contact pairs in Abaqus/Explicit,” Section 38.2.2). The elements in a small-displacement analysis are formulated in the reference (original) configuration, using original nodal coordinates. The errors in such an approximation are of the order of the strains and rotations compared to unity. The approximation also eliminates any possibility of capturing bifurcation buckling, which is sometimes a critical aspect of a structure’s response (see “Unstable collapse and postbuckling analysis,” Section 6.2.4). You must consider these issues when interpreting the results of such an analysis.
The alternative to a “small-displacement” analysis in Abaqus is to include large-displacement effects. In this case most elements are formulated in the current configuration using current nodal positions. Elements therefore distort from their original shapes as the deformation increases. With sufficiently large deformations, the elements may become so distorted that they are no longer suitable for use; for example, the volume of the element at an integration point may become negative. In this situation Abaqus will issue a warning message indicating the problem. In addition, Abaqus/Standard will cut back the time increment before making further attempts to continue the solution. Abaqus/Explicit also offers element failure models to allow elements that reach high strains to be removed from a model; see “Dynamic failure models,” Section 23.2.8, for details.
For each step of an analysis you specify whether a small- or large-displacement formulation should be used (i.e., whether geometric nonlinearity should be ignored or included). By default, Abaqus/Standard uses a small-displacement formulation and Abaqus/Explicit uses a large-displacement formulation. The default value for the formulation in an import analysis is the same as the value at the time of import. If a large-displacement formulation is used during any step of an analysis, it will be used in all following steps in the analysis; there is no way to turn it off.
Almost all of the elements in Abaqus use a fully nonlinear formulation. The exceptions are the cubic beam elements in Abaqus/Standard and the small-strain shell elements (those shell elements other than S3/S3R, S4, S4R, and the axisymmetric shells) in which the cross-sectional thickness change is ignored so that these elements are appropriate only for large rotations and small strains. Except for these elements, the strains and rotations can be arbitrarily large.
The calculated stress is the “true” (Cauchy) stress. For beam, pipe, and shell elements the stress components are given in local directions that rotate with the material. For all other elements the stress
components are given in the global directions unless a local orientation (“Orientations,” Section 2.2.5) is used at a point. For small-displacement analysis the infinitesimal strain measure is used, which is output with the strain output variable E; strain output specified with output variables LE and NE is the same as with E.
Input File Usage: Use the following option to specify that a large-displacement formulation should be used for the step:
*STEP, NLGEOM=YES (default in Abaqus/Explicit)
Use the following option to specify that a small-displacement formulation should be used for the step:
*STEP, NLGEOM=NO (default in Abaqus/Standard)
Omitting the NLGEOM parameter is equivalent to using the default value.
Abaqus/CAE Usage: Step module: Create Step: select any step type: Basic: Nlgeom: Off (for a small-displacement formulation) or On (for a large-displacement formulation)
Boundary nonlinearity
Contact problems are a common source of nonlinearity in stress analysis—see “Contact interaction analysis: overview,” Section 36.1.1. Other sources of boundary nonlinearity are nonlinear elastic springs, films, radiation, multi-point constraints, etc.
Loading
In a general analysis step the loads must be defined as total values. The rules for applying loads in a general, multistep analysis are defined in “Applying loads: overview,” Section 34.4.1.
Incrementation
The general analysis procedures in Abaqus offer two approaches for controlling incrementation. Automatic control is one choice: you define the step and, in some procedures, specify certain tolerances or error measures. Abaqus then automatically selects the increment size as it develops the response in the step. Direct user control of increment size is the alternative approach, whereby you specify the incrementation scheme. The direct approach is sometimes useful in repetitive analyses with Abaqus/Standard, where you have a good “feel” for the convergence behavior of the problem. The methods for selecting automatic or direct incrementation are discussed in the individual procedure sections.
In nonlinear problems in Abaqus/Standard the challenge is always to obtain a convergent solution in the least possible computational time. In these cases automatic control of the time increment is usually more efficient because Abaqus/Standard can react to nonlinear response that you cannot predict ahead of time. Automatic control is particularly valuable in cases where the response or load varies widely through the step, as is often the case in diffusion-type problems such as creep, heat transfer, and consolidation. Ultimately, automatic control allows nonlinear problems to be run with confidence in Abaqus/Standard without extensive experience with the problem.
Strong nonlinearities typically do not present difficulties in Abaqus/Explicit because of the small time increments that are characteristic of an explicit dynamic analysis product.
Stabilization of unstable problems in Abaqus/Standard
Some static problems can be naturally unstable, for a variety of reasons.
Unconstrained rigid body motions
Instability may occur because unconstrained rigid body motions exist. Abaqus/Standard may be able to handle this type of problem with automatic viscous damping (see “Adjusting contact controls in Abaqus/Standard,” Section 36.3.6) when rigid body motions exist during the approach of two bodies that will eventually come into contact.
Input File Usage: Use one of the following options:
*CONTACT STABILIZATION
*CONTACT CONTROLS, STABILIZE
Abaqus/CAE Usage: Automatic viscous damping is not supported in Abaqus/CAE.
Localized buckling behavior or material instability
Instability may also be caused by localized buckling behavior or by material instability; such instabilities are especially significant when no time-dependent behavior exists in the material modeling. The static, general analysis procedures in Abaqus/Standard can stabilize this type of problem if you request it (see “Static stress analysis,” Section 6.2.2; “Quasi-static analysis,” Section 6.2.5; “Steady-state transport analysis,” Section 6.4.1; “Fully coupled thermal-stress analysis,” Section 6.5.3; “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4; or “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1).
Input File Usage: Use one of the following options:
*STATIC, STABILIZE
*VISCO, STABILIZE
*STEADY STATE TRANSPORT, STABILIZE
*COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE
*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, STABILIZE
*SOILS, CONSOLIDATION, STABILIZE
Abaqus/CAE Usage: Step module: Create Step: General: any valid step type: Basic: Use stabilization with dissipated energy fraction
Linear perturbation analysis steps
Linear perturbation analysis steps are available only in Abaqus/Standard (Abaqus/Foundation is essentially the linear perturbation functionality in Abaqus/Standard). The response in a linear analysis step is the linear perturbation response about the base state. The base state is the current state of the model at the end of the last general analysis step prior to the linear perturbation step. If the first step of an analysis is a perturbation step, the base state is determined from the initial conditions (“Initial
conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). In Abaqus/Foundation the base state is always determined from the initial state of the model.
Linear perturbation analyses can be performed from time to time during a fully nonlinear analysis by including the linear perturbation steps between the general response steps. The linear perturbation response has no effect as the general analysis is continued. The step time of linear perturbation steps, which is taken arbitrarily to be a very small number, is never accumulated into the total time. A simple example of this method is the determination of the natural frequencies of a violin string under increasing tension (see “Vibration of a cable under tension,” Section 1.4.3 of the Abaqus Benchmarks Guide). The tension of the string is increased in several geometrically nonlinear analysis steps. After each of these steps, the frequencies can be extracted in a linear perturbation analysis step.
If geometric nonlinearity is included in the general analysis upon which a linear perturbation study is based, stress stiffening or softening effects and load stiffness effects (from pressure and other follower forces) are included in the linear perturbation analysis.
Load stiffness contributions are also generated for centrifugal and Coriolis loading. In direct steadystate dynamic analysis Coriolis loading generates an imaginary antisymmetric matrix. This contribution is accounted for currently in solid and truss elements only and is activated by using the unsymmetric matrix storage and solution scheme in the step.
Linear perturbation procedures
The following purely linear perturbation procedures are available in Abaqus/Standard:
• “Eigenvalue buckling prediction,” Section 6.2.3
• “Direct-solution steady-state dynamic analysis,” Section 6.3.4
• “Natural frequency extraction,” Section 6.3.5
• “Complex eigenvalue extraction,” Section 6.3.6
• “Transient modal dynamic analysis,” Section 6.3.7
• “Mode-based steady-state dynamic analysis,” Section 6.3.8
• “Subspace-based steady-state dynamic analysis,” Section 6.3.9
• “Response spectrum analysis,” Section 6.3.10
• “Random response analysis,” Section 6.3.11
• “Time-harmonic analysis” in “Eddy current analysis,” Section 6.7.5
In addition, the following analysis techniques are treated as linear perturbation steps in an analysis:
• “Defining substructures,” Section 10.1.2
• “Generating matrices,” Section 10.3.1
Except for these procedures and the static procedure (explained below), all other procedures can be used only in general analysis steps (in other words, they are not available with Abaqus/Foundation). All linear perturbation procedures except for the complex eigenvalue extraction procedure are available with Abaqus/Foundation.
Linear static perturbation analysis
A linear static stress analysis (“Static stress analysis,” Section 6.2.2) can be conducted in Abaqus/Standard.
Input File Usage: Use both of the following options to conduct a linear static perturbation analysis:
*STEP, PERTURBATION
*STATIC
Omitting the PERTURBATION parameter on the *STEP option implies that a general static analysis is required.
Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Static, Linear perturbation
Loading
Load magnitudes (including the magnitudes of prescribed boundary conditions) during a linear perturbation analysis step are defined as the magnitudes of the load perturbations only. Likewise, the value of any solution variable is output as the perturbation value only—the value of the variable in the base state is not included.
Multiple load case analysis
Multiple load cases can be analyzed simultaneously for static, direct-solution steady-state dynamic and SIM-based steady-state dynamic (including subspace projection) linear perturbation steps. See “Multiple load case analysis,” Section 6.1.4, for a description of this capability.
Restrictions
A linear perturbation analysis is subject to the following restrictions:
• Since a linear perturbation analysis has no time period, amplitude references (“Amplitude curves,” Section 34.1.2) can be used meaningfully only to specify loads or boundary conditions as functions of frequency (in a steady-state dynamics analysis) or to define base motion (in mode-based dynamics procedures). If loads or boundary conditions are specified as functions of time, the amplitude value corresponding to time=0 will be used.
• A general implicit dynamic analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2) cannot be interrupted to perform perturbation analyses: before performing the perturbation analysis, Abaqus/Standard requires that the structure be brought into static equilibrium.
• During a linear perturbation analysis step, the model’s response is defined by its linear elastic stiffness at the base state. For viscoelastic materials the elastic moduli at the base state is evaluated as described in “Materials options” in “Static stress analysis,” Section 6.2.2, for static procedures, and in “Evaluating frequency-dependent material properties” in “Natural frequency extraction,” Section 6.3.5, for frequency-based procedures. Plasticity and other inelastic effects are ignored