김경종
22 KiB
Unstable problems
Some types of analyses may develop local instabilities, such as surface wrinkling, material instability, or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid of automatic incrementation. Abaqus/Standard offers the ability to stabilize this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1.
Initial conditions
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified, as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1.
Boundary conditions
Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6); to warping degree of freedom 7 in open-section beam elements; or, if hydrostatic fluid elements are included in the model, to fluid pressure degree of freedom 8. If boundary conditions are applied to rotation degrees of freedom, you must understand how Abaqus handles finite rotations. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1.
Loads
The following types of loading can be prescribed in a quasi-static analysis:
• Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 34.4.2.
• Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 34.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.”
Predefined fields
The following predefined fields can be specified in a quasi-static analysis, as described in “Predefined fields,” Section 34.6.1:
• Although temperature is not a degree of freedom in quasi-static analysis, nodal temperatures can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any.
• The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any.
Material options
The quasi-static procedure in Abaqus/Standard is generally used to analyze quasi-static creep and swelling problems, which occur over fairly long time periods (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4). This procedure can also be used to analyze viscoelastic materials (“Time domain viscoelasticity,” Section 22.7.1, and “Parallel rheological framework,” Section 22.8.2) and two-layer viscoplastic materials (“Two-layer viscoplasticity,” Section 23.2.11). In addition, all material models that are valid in a static analysis procedure can be used.
Elements
Any of the stress/displacement elements in Abaqus/Standard (including those with temperature or pressure degrees of freedom) can be used in a quasi-static stress analysis—see “Choosing the appropriate element for an analysis type,” Section 27.1.3.
Output
In addition to the usual output variables available in Abaqus/Standard (see “Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables are provided specifically for creep problems:
Element integration point variables:
CEEQ Equivalent creep strain, \int_0^t\dot{\varepsilon}^{cr}dt .
CESW Magnitude of the swelling strain.
CEMAG Magnitude of the creep strain, \sqrt{\frac{2}{3}\varepsilon^{cr}:\varepsilon^{cr}} .
CEP Principal creep strains.
CE Output of all of the creep strain components and CEEQ, CESW, and CEMAG.
Input file template
*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
**
*STEP (, NLGEOM)
*VISCO, CETOL=tolerance
Data line to define time incrementation and a “real” time scale
*BOUNDARY
Data lines to describe nonzero boundary conditions
*CLOAD and/or *DLOAD and/or *TEMPERATURE and/or *FIELD
Data lines to specify loading
*END STEP
6.2.6 DIRECT CYCLIC ANALYSIS
Products: Abaqus/Standard Abaqus/CAE
References
• “Defining an analysis,” Section 6.1.2
• *DIRECT CYCLIC
• *TIME POINTS
• *CONTROLS
• “Configuring a direct cyclic procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
A direct cyclic analysis:
• is a quasi-static analysis;
• uses a combination of Fourier series and time integration of the nonlinear material behavior to obtain the stabilized cyclic response of the structure iteratively;
• avoids the considerable numerical expense associated with a transient analysis;
• is ideally suited for very large problems in which many load cycles must be applied to obtain the stabilized response if transient analysis is performed;
• can be performed with linear or nonlinear material with localized plastic deformation;
• can be used to predict the likelihood of plastic ratchetting;
• assumes geometrically linear behavior and fixed contact conditions;
• uses the elastic stiffness, so the equation system is inverted only once; and
• can also be used to predict progressive damage and failure for ductile bulk materials and/or to predict delamination/debonding growth at the interfaces in laminated composites in a low-cycle fatigue analysis.
Introduction
It is well known that after a number of repetitive loading cycles, the response of an elastic-plastic structure, such as an automobile exhaust manifold subjected to large temperature fluctuations and clamping loads, may lead to a stabilized state in which the stress-strain relationship in each successive cycle is the same as in the previous one. The classical approach to obtain the response of such a structure is to apply the periodic loading repetitively to the structure until a stabilized state is obtained. This approach can be quite expensive, since it may require the application of many loading cycles before the stabilized response is obtained. To avoid the considerable numerical expense associated with a transient analysis, a direct cyclic analysis can be used to calculate the cyclic response of the structure directly.
The basis of this method is to construct a displacement function \overline { { u } } ( t ) that describes the response of the structure at all times t during a load cycle with period T as shown in Figure 6.2.6–1.
line
| t | stabilized solution | solution at iteration n+1 | solution at iteration n |
|---|---|---|---|
| Δt₁ | ~0.5 | ~0.3 | ~0.2 |
| tₙ₋₁ | ~0.8 | ~0.6 | ~0.4 |
| tₙ₊₁ | ~0.7 | ~0.5 | ~0.3 |
| T | ~0.6 | ~0.4 | ~0.2 |
Figure 6.2.6–1 A displacement function at all times t during a load cycle with period T at different iterations.
A truncated Fourier series is used for this purpose,
\overline {{u}} (t) = u _ {0} + \sum_ {k = 1} ^ {n} \left[ u _ {k} ^ {s} \sin k \omega t + u _ {k} ^ {c} \cos k \omega t \right],
where n stands for the number of terms in the Fourier series, \omega ~ = ~ 2 \pi / T is the angular frequency, and u _ { 0 } , u _ { k } ^ { s } , and u _ { k } ^ { \mathrm { c } } are unknown displacement coefficients associated with each degree of freedom in the problem. Abaqus/Standard solves for the unknown displacement coefficients by using a modified Newton method, with the elastic stiffness matrix at the beginning of the analysis step serving as the Jacobian in the scheme. We expand the residual vector in the modified Newton method using a Fourier series of the same form as the displacement solution:
\overline {{R}} (t) = R _ {0} + \sum_ {k = 1} ^ {n} \left[ R _ {k} ^ {s} \sin k \omega t + R _ {k} ^ {c} \cos k \omega t \right],
where each residual vector coefficient R _ { 0 } , R _ { k } ^ { s } , and R _ { k } ^ { c } in the Fourier series corresponds to a displacement coefficient u _ { 0 } , u _ { k } ^ { s } , and u _ { k } ^ { c } . , respectively. The residual coefficients are obtained by tracking through the entire load cycle. At each instant in time in the cycle Abaqus/Standard obtains the residual vector R ( t ) by
using standard element-by-element calculations, which—when integrated over the entire cycle—provide the Fourier coefficients
\begin{array}{l} R _ {0} = \frac {1}{T} \int_ {0} ^ {T} R (t) d t, \\ R _ {k} ^ {s} = \frac {2}{T} \int_ {0} ^ {T} R (t) \sin k \omega t d t, \\ R _ {k} ^ {c} = \frac {2}{T} \int_ {0} ^ {T} R (t) \cos k \omega t d t. \\ \end{array}
The displacement solution is obtained by solving for corrections to the displacement Fourier coefficients corresponding to each residual coefficient. The updated displacement solution is used in the next iteration to obtain the displacements at each instant in time. This process is repeated until convergence is obtained. Each pass through the complete load cycle can, therefore, be thought of as a single iteration of the solution to the nonlinear problem. Convergence is measured by ensuring that all entries of the residual coefficients are small.
The algorithm to obtain a stabilized cycle is described in detail in “Direct cyclic algorithm,” Section 2.2.3 of the Abaqus Theory Guide.
Direct cyclic analysis
A direct cyclic step can be the only step in an analysis, can follow a general or linear perturbation step, or can be followed by a general or linear perturbation step. If a direct cyclic step is followed by a general step, the solution at the end of the direct cyclic step will be the initial state of the general step. If a direct cyclic step follows a general or linear perturbation step, the elastic stiffness matrix at the end of the last general analysis step prior to the direct cyclic step will serve as the Jacobian in the direct cyclic procedure. Any prior (non-cyclic) loads are simply included in the constant part of the Fourier expansion of the residual vectors, and the plastic strains at the end of the preloading step are used as initial conditions for the direct cyclic step.
Multiple direct cyclic analysis steps can be included in a single analysis. In such a case the Fourier series coefficients obtained in the previous step can be used as starting values in the current step. By default, the Fourier coefficients are reset to zero, thus allowing application of cyclic loading conditions that are very different from those defined in the previous direct cyclic step.
You can specify that a direct cyclic step in a restart analysis should use the Fourier coefficients from the previous step, thus allowing continuation of an analysis that has not reached a stabilized cycle. In a direct cyclic analysis a restart file is written at the end of the cycle or time period. Consequently, a restart analysis that is a continuation of a previous direct cyclic analysis will start with a new iteration at (see “Restarting an analysis,” Section 9.1.1).
Input File Usage:
Use the following option to reset the Fourier series coefficients to zero:
*DIRECT CYCLIC, CONTINUE=NO (default)
Use the following option to specify that the current step is a continuation of the previous direct cyclic step:
*DIRECT CYCLIC, CONTINUE=YES
Abaqus/CAE Usage: Use the following option to reset the Fourier series coefficients to zero (default):
Step module: Create Step: General: Direct cyclic
Use the following option to specify that the current step is a continuation of the previous direct cyclic step:
Step module: Create Step: General: Direct cyclic; Basic: Use displacement Fourier coefficients from previous direct cyclic step
Using the direct cyclic approach to perform low-cycle fatigue analysis
The direct cyclic procedure can also be used in conjunction with the damage extrapolation technique to predict progressive damage and failure for ductile bulk materials and/or to predict delamination/debonding at the interfaces in laminated composites in a low-cycle fatigue analysis. In this case multiple cycles can be included in a single direct cyclic analysis, as described in “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7.
Input File Usage: *DIRECT CYCLIC, FATIGUE
Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Fatigue: Include low-cycle fatigue analysis
Controlling the solution accuracy
Direct cyclic analysis combines a Fourier series approximation with time integration of the nonlinear material behavior to obtain the stabilized cyclic solution iteratively using a modified Newton method. The accuracy of the algorithm depends on the number of Fourier terms used, the number of iterations taken to obtain the stabilized solution, and the number of time points within the load period at which the material response and residual vector are evaluated. Abaqus/Standard allows you to control the solution in several ways, as described below.
Controlling the iterations in the modified Newton method
In the direct cyclic method global Newton iterations are performed to determine corrections to the displacement Fourier coefficients. During each global iteration Abaqus/Standard tracks through the entire time cycle to compute the residual vector at a suitable number of time points. This involves standard element-by-element finite element calculations in which history-dependent material variables are integrated. The residual vector is integrated over the period to obtain the Fourier residual coefficients, which in turn yield corrections in displacement coefficients when the system of equations is solved. Abaqus/Standard will continue with the iterative process until convergence is obtained or until the maximum number of iterations allowed has been reached. You can specify the maximum number of iterations when you define the direct cyclic step; the default is 200 iterations.
Input File Usage: *DIRECT CYCLIC , , , , , , , max number of iterations
Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Incrementation: Maximum number of iterations: max number of iterations
Specifying convergence criteria
Convergence is best measured by ensuring that all the residual coefficients are sufficiently small compared to the time averaged force and that all the corrections to displacement Fourier coefficients are sufficiently small compared to the displacement Fourier coefficients. The time averaged force is defined in “Convergence criteria for nonlinear problems,” Section 7.2.3. Abaqus/Standard requires that the ratio of the maximum residual coefficient to the time averaged force, C R _ { n } ^ { \alpha } , and the ratio of the maximum correction to the displacement coefficients to the largest displacement coefficient, C U _ { n } ^ { \alpha } , are less than the tolerances. The default values are C R _ { n } ^ { \alpha } = 0 . 0 0 5 and C U _ { n } ^ { \alpha } = 0 . 0 0 5 . To change these values, you must define direct cyclic controls.
When a stabilized cyclic response does not exist, the method will not converge. In the case where plastic ratchetting occurs, the displacement and residual coefficients of all the periodic terms ( \boldsymbol { u } _ { k } ^ { s } , \boldsymbol { u } _ { k } ^ { c } , and R _ { k } ^ { c } , R _ { k } ^ { c } ) in the Fourier series converge. However, the displacement and the residual coefficients of the constant term ( u _ { 0 } and R _ { 0 } ) in the Fourier series continue to grow from one iteration to another iteration. The user-specified tolerances C R _ { 0 } ^ { \alpha } and C U _ { 0 } ^ { \alpha } are used to detect the plastic ratchetting. The default values are C R _ { 0 } ^ { \alpha } = 0 . 0 0 5 and C U _ { 0 } ^ { \alpha } = 0 . 0 0 5 . For more information, see “Controlling the solution accuracy in direct cyclic analysis” in “Commonly used control parameters,” Section 7.2.2.
Input File Usage: *CONTROLS, TYPE=DIRECT CYCLIC
Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit; Specify: Direct Cyclic
Controlling the Fourier representations
The number of Fourier terms required to obtain an accurate solution depends on the variation of the load as well as the variation of the structural response over the period. In determining the number of terms, keep in mind that the objective of this kind of analysis is to make low-cycle fatigue predictions. Hence, the goal is to obtain good approximation of the plastic strain cycle at each point; local inaccuracies in the stresses are less important. More Fourier terms usually provide a more accurate solution but at the expense of additional data storage and computational time. In addition, an accurate integration of the Fourier residual coefficients requires that the residual vector be evaluated at an adequate number of time points during the cycle. Abaqus/Standard uses a trapezoidal rule, which assumes a linear variation of the residual over a time increment, to integrate the residual coefficients. For accurate integration the number of time points must be larger than the number of Fourier coefficients (which is equal to 2 n + 1 , where n represents the number of Fourier terms). Abaqus/Standard will automatically reduce the number of Fourier coefficients used for the next iteration if it is found to be greater than the number of increments taken to complete an iteration.
Abaqus/Standard uses an adaptive algorithm to determine the number of Fourier terms. By default, Abaqus/Standard starts with 11 terms and determines the response of the structure by using the iterative method described before. Once convergence is obtained (which is measured by ensuring that all the residual vector coefficients and all the corrections to displacement coefficients in the Fourier series are sufficiently small), Abaqus/Standard evaluates if a sufficient number of Fourier terms are used by determining if equilibrium was satisfied at all the time points during the cycle. If equilibrium is satisfied at all time points, the solution is accepted. Otherwise, Abaqus/Standard increases the number of Fourier
terms (by default, 5 terms are added) and continues with the iterative scheme until convergence with the new number of Fourier terms is obtained. This process is repeated until equilibrium is reached or until the maximum number of Fourier terms has been used. This scheme is best illustrated in Figure 6.2.6–2, where both local equilibrium and overall convergence are obtained when the number of Fourier terms is equal to 21. A maximum number of 25 Fourier terms is used by default. You can specify the initial and maximum number of Fourier terms and the increment in the number of terms when you define the direct cyclic step.
line
| t | equilibrium tolerance | stabilized iteration with 11 terms | stabilized iteration with 16 terms | stabilized iteration with 21 terms |
|---|---|---|---|---|
| 0 | 0 | 0 | 0 | 0 |
| 1 | ~0.5 | ~0.8 | ~0.6 | ~0.4 |
| 2 | ~0.3 | ~0.6 | ~0.5 | ~0.3 |
| 3 | ~0.1 | ~0.4 | ~0.3 | ~0.2 |
| 4 | ~0.0 | ~0.2 | ~0.1 | ~0.1 |
| 5 | ~0.0 | ~0.0 | ~0.0 | ~0.0 |
Figure 6.2.6–2 Stabilized iterations with different Fourier terms.
You can also define the convergence criteria for determining convergence and for determining whether equilibrium is achieved at all time points through the period (see “Commonly used control parameters,” Section 7.2.2), with suitable defaults set by Abaqus/Standard.
In a direct cyclic analysis that has not reached a stabilized cycle, you can increase the number of iterations or Fourier terms upon restart, thus allowing continuation of an analysis.
Abaqus/Standard provides detailed output of the maximum residual at each time point, the maximum residual coefficient, the maximum displacement coefficient, the maximum correction to displacement coefficients, and the number of Fourier terms at the end of each iteration in the message (.msg) file. This output is described in more detail below.
Input File Usage: *DIRECT CYCLIC , \ldots , initial number of terms, max number of terms, increment in number of terms
Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Incrementation: Number of Fourier terms: Initial: initial number of terms, Maximum: max number of terms, Increment: increment in number of terms