김경종
20 KiB
SDEG Scalar stiffness degradation, D.
CYCLEINI Number of cycles to initialize the damage at the material point.
The following variables are available for discrete crack propagation along an arbitrary path based on the principles of linear elastic fracture mechanics with the extended finite element method:
STATUSXFEM Status of the enriched element. (The status of an enriched element is 1.0 if the element is completely cracked, 0.0 if the element is not. If the element is partially cracked, the value lies between 1.0 and 0.0.)
CYCLEINIXFEM Number of cycles to initialize the crack at the enriched element.
ENRRTXFEM All components of strain energy release rate range; i.e., the difference between the energy release rate at the maximum loading and at the minimum loading.
Recovering additional results for a stabilized cycle
You may want to recover additional results for a stabilized cycle. You can extract these results from the restart data (see “Recovering additional results output from restart data in Abaqus/Standard” in “Output,” Section 4.1.1).
Input File Usage: *POST OUTPUT, CYCLE=n
Abaqus/CAE Usage: Recovering additional results for a stabilized cycle is not supported in Abaqus/CAE.
Specifying output at exact times
Output at exact times is not supported for low-cycle fatigue analysis. If output at exact times is requested, Abaqus will issue a warning message and change the output to an output at approximate times.
Limitations
A low-cycle fatigue analysis using the direct cyclic approach is subject to the following limitations:
• Contact conditions cannot change during a given cycle when direct cyclic analysis is used iteratively to obtain a stabilized solution.
• The analysis may not perform well when there is compressive load on the crack surface during a loading cycle because the global stiffness is formed only one time at the beginning of each given loading cycle.
• Geometric nonlinearity can be included only in any general step prior to a direct cyclic step; however, only small displacements and strains will be considered during the cyclic step.
The following is an example of modeling progressive damage and failure in the bulk material based on the continuum damage mechanics approach and progressive delamination growth at the interface:
*HEADING
...
*BOUNDARY
Data lines to specify zero-valued boundary conditions
*INITIAL CONDITIONS
Data lines to specify initial conditions
*AMPLITUDE
Data lines to define amplitude variations
**
*MATERIAL
Options to define material properties
* DAMAGE INITIATION, CRITERION=HYSTERESIS ENERGY
Data lines to define material constants for bulk ductile material damage initiation
* DAMAGE EVOLUTION, TYPE=HYSTERESIS ENERGY
Data lines to define material constants for bulk ductile material damage evolution
**
*SURFACE, NAME=slave
Data lines to define slave surface at delamination interface
*SURFACE, NAME=master
Data lines to define master surface at delamination interface
*CONTACT PAIR
slave, master
**
*STEP (, INC=)
Set INC equal to the maximum number of increments in a single loading cycle
*DIRECT CYCLIC, FATIGUE
Data line to define time increment, cycle time, initial number of Fourier terms, maximum number of Fourier terms, increment in number of Fourier terms, and maximum number of iterations
Data line to define minimum increment in number of cycles, maximum increment in number of cycles, total number of cycles, and damage extrapolation tolerance
*DEBOND, SLAVE=slave, MASTER=master
*FRACTURE CRITERION, TYPE=FATIGUE
Data lines to define material constants used in Paris law and fracture criterion
**
*BOUNDARY, AMPLITITUDE=
Data lines to prescribe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD, AMPLITITUDE= Data lines to specify loads *TEMPERATURE and/or *FIELD, AMPLITITUDE= Data lines to specify values of predefined fields ** *END STEP
The following is an example of modeling discrete crack growth in the bulk material based on the principles of linear elastic fracture mechanics with the extended finite element method and progressive delamination growth at the interface:
*HEADING ... *ENRICHMENT, TYPE=PROPAGATION CRACK, INTERACTION=INTERACTION, ELSET=ENRICHED *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions *AMPLITUDE Data lines to define amplitude variations ** *MATERIAL Options to define material properties *SURFACE, INTERACTION=INTERACTION *SURFACE BEHAVIOR *FRACTURE CRITERION, TYPE=FATIGUE Data lines to define material constants used in the Paris law and fracture criterion in the bulk material for enriched elements ** *SURFACE, NAME=slave Data lines to define slave surface at delamination interface *SURFACE, NAME=master Data lines to define master surface at delamination interface *CONTACT PAIR slave, master ** *STEP (, INC=) Set INC equal to the maximum number of increments in a single loading cycle *DIRECT CYCLIC, FATIGUE Data line to define time increment, cycle time, initial number of Fourier terms, maximum number of Fourier terms, increment in number of Fourier terms,
and maximum number of iterations
Data line to define minimum increment in number of cycles,
maximum increment in number of cycles, total number of cycles,
and damage extrapolation tolerance
*DEBOND, SLAVE=slave, MASTER=master
*FRACTURE CRITERION, TYPE=FATIGUE
Data lines to define material constants used in the Paris law and fracture criterion at the interface
**
*BOUNDARY, AMPLITITUDE=
Data lines to prescribe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD, AMPLITITUDE=
Data lines to specify loads
*TEMPERATURE and/or *FIELD, AMPLITITUDE=
Data lines to specify values of predefined fields
**
*END STEP
Additional references
• Coffin, L., “A Study of the Effects of Cyclic Thermal Stresses on a Ductile Metal,” Transactions of the American Society of Mechanical Engineering, vol. 76, pp. 931–951, 1954.
• Manson, S., “Behavior of Materials under Condition of Thermal Stress,” Heat Transfer Symposium, University of Michigan Engineering Research Institute, Ann Arbor, MI, pp. 9–75, 1953.
• Paris, P., M. Gomaz, and W. Anderson, “A Rational Analytic Theory of Fatigue,” The Trend in Engineering, vol. 15, 1961.
6.3 Dynamic stress/displacement analysis
• “Dynamic analysis procedures: overview,” Section 6.3.1
• “Implicit dynamic analysis using direct integration,” Section 6.3.2
• “Explicit dynamic analysis,” Section 6.3.3
• “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
6.3.1 DYNAMIC ANALYSIS PROCEDURES: OVERVIEW
Overview
Abaqus offers several methods for performing dynamic analysis of problems in which inertia effects are considered. Direct integration of the system must be used when nonlinear dynamic response is being studied. Implicit direct integration is provided in Abaqus/Standard; explicit direct integration is provided in Abaqus/Explicit. Modal methods are usually chosen for linear analyses because in direct-integration dynamics the global equations of motion of the system must be integrated through time, which makes direct-integration methods significantly more expensive than modal methods. Subspace-based methods are provided in Abaqus/Standard and offer cost-effective approaches to the analysis of systems that are mildly nonlinear.
In Abaqus/Standard dynamic studies of linear problems are generally performed by using the eigenmodes of the system as a basis for calculating the response. In such cases the necessary modes and frequencies are calculated first in a frequency extraction step. The mode-based procedures are generally simple to use; and the dynamic response analysis itself is usually not expensive computationally, although the eigenmode extraction can become computationally intensive if many modes are required for a large model. The eigenvalues can be extracted in a prestressed system with the “stress stiffening” effect included (the initial stress matrix is included if the base state step definition included nonlinear geometric effects), which may be necessary in the dynamic study of preloaded systems. It is not possible to prescribe nonzero displacements and rotations directly in mode-based procedures. The method for prescribing motion in mode-based procedures is explained in “Base motions in modal-based procedures,” Section 2.5.9 of the Abaqus Theory Guide.
Density must be defined for all materials used in any dynamic analysis, and damping (both viscous and structural) can be specified either at the material or step level, as described below in “Damping in dynamic analysis.”
Implicit versus explicit dynamics
The direct-integration dynamic procedure provided in Abaqus/Standard offers a choice of implicit operators for integration of the equations of motion, while Abaqus/Explicit uses the central-difference operator. In an implicit dynamic analysis the integration operator matrix must be inverted and a set of nonlinear equilibrium equations must be solved at each time increment. In an explicit dynamic analysis displacements and velocities are calculated in terms of quantities that are known at the beginning of an increment; therefore, the global mass and stiffness matrices need not be formed and inverted, which means that each increment is relatively inexpensive compared to the increments in an implicit integration scheme. The size of the time increment in an explicit dynamic analysis is limited, however, because the central-difference operator is only conditionally stable; whereas the implicit operator options available in Abaqus/Standard are unconditionally stable and, thus, there is no such limit on the size of the time increment that can be used for most analyses in Abaqus/Standard (accuracy governs the time increment in Abaqus/Standard).
The stability limit for the central-difference method (the largest time increment that can be taken without the method generating large, rapidly growing errors) is closely related to the time required for a
stress wave to cross the smallest element dimension in the model; thus, the time increment in an explicit dynamic analysis can be very short if the mesh contains small elements or if the stress wave speed in the material is very high. The method is, therefore, computationally attractive for problems in which the total dynamic response time that must be modeled is only a few orders of magnitude longer than this stability limit; for example, wave propagation studies or some “event and response” applications. Many of the advantages of the explicit procedure also apply to slower (quasi-static) processes for cases in which it is appropriate to use mass scaling to reduce the wave speed (see “Mass scaling,” Section 11.6.1).
Abaqus/Explicit offers fewer element types than Abaqus/Standard. For example, only first-order, displacement method elements (4-node quadrilaterals, 8-node bricks, etc.) and modified second-order elements are used, and each degree of freedom in the model must have mass or rotary inertia associated with it. However, the method provided in Abaqus/Explicit has some important advantages:
- The analysis cost rises only linearly with problem size, whereas the cost of solving the nonlinear equations associated with implicit integration rises more rapidly than linearly with problem size. Therefore, Abaqus/Explicit is attractive for very large problems.
- The explicit integration method is often more efficient than the implicit integration method for solving extremely discontinuous short-term events or processes.
- Problems involving stress wave propagation can be far more efficient computationally in Abaqus/Explicit than in Abaqus/Standard.
In choosing an approach to a nonlinear dynamic problem you must consider the length of time for which the response is sought compared to the stability limit of the explicit method; the size of the problem; and the restriction of the explicit method to first-order, pure displacement method or modified second-order elements. In some cases the choice is obvious, but in many problems of practical interest the choice depends on details of the specific case. Experience is then the only useful guide.
Direct-solution versus modal superposition procedures
Direct solution procedures must be used for dynamic analyses that involve a nonlinear response. Modal superposition procedures are a cost-effective option for performing linear or mildly nonlinear dynamic analyses.
Direct-solution dynamic analysis procedures
The following direct-solution dynamic analyses procedures are available in Abaqus:
• Implicit dynamic analysis: Implicit direct-integration dynamic analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2) is used to study (strongly) nonlinear transient dynamic response in Abaqus/Standard.
• Subspace-based explicit dynamic analysis: The subspace projection method in Abaqus/Standard uses direct, explicit integration of the dynamic equations of equilibrium written in terms of a vector space spanned by a number of eigenvectors (“Implicit dynamic analysis using direct integration,” Section 6.3.2). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. This method can be very effective for systems
with mild nonlinearities that do not substantially change the mode shapes. It cannot be used in contact analyses.
• Explicit dynamic analysis: Explicit direct-integration dynamic analysis (“Explicit dynamic analysis,” Section 6.3.3) is available in Abaqus/Explicit.
• Direct-solution steady-state harmonic response analysis: The steady-state harmonic response of a system can be calculated in Abaqus/Standard directly in terms of the physical degrees of freedom of the model (“Direct-solution steady-state dynamic analysis,” Section 6.3.4). The solution is given as in-phase (real) and out-of-phase (imaginary) components of the solution variables (displacement, stress, etc.) as functions of frequency. The main advantage of this method is that frequency-dependent effects (such as frequency-dependent damping) can be modeled. The direct method is the most accurate but also the most expensive steady-state harmonic response procedure. The direct method can also be used if nonsymmetric terms in the stiffness are important or if model parameters depend on frequency.
Modal superposition procedures
Abaqus includes a full range of modal superposition procedures. Modal superposition procedures can be run using a high-performance linear dynamics software architecture called SIM. The SIM architecture offers advantages over the traditional linear dynamics architecture for some large-scale analyses, as discussed below in “Using the SIM architecture for modal superposition dynamic analyses.”
Prior to any modal superposition procedure, the natural frequencies of a system must be extracted using the eigenvalue analysis procedure (“Natural frequency extraction,” Section 6.3.5). Frequency extraction can be performed using the SIM architecture.
The following modal superposition procedures are available in Abaqus:
• Mode-based steady-state harmonic response analysis: A steady-state dynamic analysis based on the natural modes of the system can be used to calculate a system’s linearized response to harmonic excitation (“Mode-based steady-state dynamic analysis,” Section 6.3.8). This mode-based method is typically less expensive than the direct method. The solution is given as in-phase (real) and out-of-phase (imaginary) components of the solution variables (displacement, stress, etc.) as functions of frequency. Mode-based steady-state harmonic analysis can be performed using the SIM architecture.
• Subspace-based steady-state harmonic response analysis: In this type of Abaqus/Standard analysis the steady-state dynamic equations are written in terms of a vector space spanned by a number of eigenvectors (“Subspace-based steady-state dynamic analysis,” Section 6.3.9). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. The method is attractive because it allows frequency-dependent effects to be modeled and is much cheaper than the direct analysis method (“Direct-solution steady-state dynamic analysis,” Section 6.3.4). Subspace-based steady-state harmonic response analysis can be used if the stiffness is nonsymmetric and can be performed using the SIM architecture.
• Mode-based transient response analysis: The modal dynamic procedure (“Transient modal dynamic analysis,” Section 6.3.7) provides transient response for linear problems using modal superposition. Mode-based transient analysis can be performed using the SIM architecture.
• Response spectrum analysis: A linear response spectrum analysis (“Response spectrum analysis,” Section 6.3.10) is often used to obtain an approximate upper bound of the peak significant response of a system to a user-supplied input spectrum (such as earthquake data) as a function of frequency. The method has a very low computational cost and provides useful information about the spectral behavior of a system. Response spectrum analysis can be performed using the SIM architecture.
• Random response analysis: The linearized response of a model to random excitation can be calculated based on the natural modes of the system (“Random response analysis,” Section 6.3.11). This procedure is used when the structure is excited continuously and the loading can be expressed statistically in terms of a “Power Spectral Density” (PSD) function. The response is calculated in terms of statistical quantities such as the mean value and the standard deviation of nodal and element variables. Random response analysis can be performed using the SIM architecture.
• Complex eigenvalue extraction: The complex eigenvalue extraction procedure performs eigenvalue extraction to calculate the complex eigenvalues and the corresponding complex mode shapes of a system (“Complex eigenvalue extraction,” Section 6.3.6). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. The complex eigenvalue extraction can be performed using the SIM architecture.
Using the SIM architecture for modal superposition dynamic analyses
SIM is a high-performance software architecture available in Abaqus that can be used to perform modal superposition dynamic analyses. The SIM architecture is much more efficient than the traditional architecture for large-scale linear dynamic analyses (both model size and number of modes) with minimal output requests.
SIM-based analyses can be used to efficiently handle nondiagonal damping generated from element or material contributions, as discussed below in “Damping in a mode-based steady-state and transient linear dynamic analysis using the SIM architecture.” Therefore, SIM-based procedures are an efficient alternative to subspace-based linear dynamic procedures for models with element damping or frequencyindependent materials.
Activating the SIM architecture
To use the SIM architecture for a modal superposition dynamic analysis, activate SIM for the initial frequency extraction procedure. SIM-based frequency extraction procedures write the mode shapes and other modal system information to a special linear dynamics data (.sim) file. By default, this data file is written to the scratch directory and deleted upon job completion; however, if restart is requested, the file is saved in the user directory. All subsequent mode-based steady-state or transient dynamic steps in an analysis automatically use this linear dynamics data file (and by extension the SIM architecture). If you restart an analysis that uses the SIM architecture, you must include the linear dynamics data file.
For more information about frequency extraction procedures, see “Natural frequency extraction,” Section 6.3.5.
Input File Usage: *FREQUENCY, SIM