MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide2/AbaqusAnalysisUserGuide2_013.md

Controlling the incrementation during the cyclic time period

To ensure an accurate solution, the material history as well as the residual vector must be evaluated at a sufficient number of time points during the cycle. The number of time points, n _ { T } , at which the response is computed must be larger than the number of Fourier coefficients; i.e., n _ { T } > 2 n + 1 . Abaqus/Standard will automatically adjust the number of Fourier coefficients if such a condition is not satisfied. You can specify the time incrementation over the cycle directly, or it can be determined automatically by Abaqus/Standard.

You should specify the maximum number of increments allowed in the time period as part of the step definition. The default is 100.

Automatic incrementation

There are several ways to choose the automatic incrementation scheme. If you specify only the maximum allowable nodal temperature change in an increment, the time increments are selected automatically based on this value. Abaqus/Standard will restrict the time increments to ensure that the maximum temperature change is not exceeded at any node during any increment of the analysis.

For rate-dependent constitutive equations you can limit the size of the time increment by the accuracy of the integration. The user-specified accuracy tolerance parameter limits the maximum inelastic strain rate change allowed over an increment:

t o l e r a n c e \geq (\dot {\bar {\varepsilon}} ^ {c r} | _ {t + \Delta t} - \dot {\bar {\varepsilon}} ^ {c r} | _ {t}) \Delta t,

where t is the time at the beginning of the increment, \Delta t is the time increment (so that t + \Delta t is the time at the end of the increment), and \dot { \bar { \varepsilon } } ^ { c \bar { r } } is the equivalent creep strain rate. To achieve sufficient accuracy, the value chosen for the accuracy tolerance parameter should be on the order of \sigma _ { e r r } / E for creep problems, where \sigma _ { e r r } is an acceptable level of error in the stress and E is a typical elastic modulus, or on the order of the elastic strains for viscoelasticity problems.

If rate-dependent constitutive equations are used in combination with a varying temperature, both controls can be used simultaneously. Abaqus/Standard will then choose the increments that satisfy both criteria.

If the time integration accuracy measure specified by either or both of the above controls is satisfied after I _ { T } consecutive increments without cutbacks, the next time increment will be increased by a factor of D _ { M } . Both I _ { T } and D _ { M } are user-defined parameters (see “Increasing the time increment size” in “Time integration accuracy in transient problems,” Section 7.2.4). The defaults are I _ { T } = 3 and D _ { M } = 1 . 5 .

Input File Usage: Use the following option to specify the maximum allowable nodal temperature change:

*DIRECT CYCLIC, DELTMX=

Use the following option to specify the accuracy tolerance parameter:

*DIRECT CYCLIC, CETOL=tolerance

Abaqus/CAE Usage: Use the following option to specify the maximum allowable nodal temperature change:

Step module: Create Step: General: Direct cyclic; Incrementation:

Max. allowable temperature change per increment: \Delta \theta _ { m a x }

Use the following option to specify the accuracy tolerance parameter:

Step module: Create Step: General: Direct cyclic; Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance

Fixed time incrementation

If neither the accuracy tolerance parameter nor the maximum allowable nodal temperature change is specified, the size of the time increment is fixed. You must specify the time increment and the time period T.

Input File Usage: *DIRECT CYCLIC , T

Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Basic: Cycle time period: T; Incrementation: Type: Fixed, Increment size:

Defining the time points at which the response must be evaluated

The user-defined time incrementation for a direct cyclic step can be augmented or superseded by specifying particular time points in the loading history at which the response of the structure should be evaluated. This feature is particularly useful if you know prior to the analysis at which time points in the analysis the load reaches a maximum and/or minimum value or when the response will change rapidly. An example is the analysis of the heating/cooling thermal cycle of an engine component where you typically know when the temperature reaches a maximum value.

When time points are used with fixed time incrementation, the time incrementation specified for the direct cyclic step is ignored and instead the time incrementation precisely follows the specified time points. If time points are used with automatic incrementation, the time incrementation is variable; but the response of the structure will be evaluated at the specified time points.

The time points can be listed individually, or they can be generated automatically by specifying the starting time point, ending time point, and increment in time between the two specified time points.

Input File Usage: Use the following options to list time points individually:

*TIME POINTS, NAME=time points name *DIRECT CYCLIC, TIME POINTS=time points name

Use the following options to generate time points automatically:

*TIME POINTS, NAME=time points name, GENERATE *DIRECT CYCLIC, TIME POINTS=time points name

Abaqus/CAE Usage: Use the following options to list time points individually:

Step module: Create Step: General: Direct cyclic; Incrementation: Evaluate structure response at time points: time points name

Use the following options to generate time points automatically:

Step module: Create Step: General: Direct cyclic; Incrementation: Evaluate structure response at time points: Create; Edit Time Points: Specify using delimiters: Start, End, Increment

Controlling the application of periodicity conditions

By default, Abaqus/Standard imposes periodic conditions during the iterative solution process by using the state obtained at the end of the previous iteration as the starting state for the current iteration; i.e., s _ { t = 0 } ^ { i + 1 } = s _ { t = T } ^ { i } st=0 , where s is a solution variable such as plastic strain.

In cases where the periodic solution is not easily found (for example, when the loading is close to causing ratchetting), the state around which the periodic solution is obtained may show considerably more “drift” than would be obtained in a transient analysis. In such cases you may wish to delay the application of periodic conditions as an artificial method to reduce this drift. Figure 6.2.6–3 compares the response of two identical structures subjected to the same set of cyclic loads and boundary conditions, where each structure experienced a different loading history prior to the application of the cyclic loads. Figure 6.2.6–3 shows that the prior loading history only affects the mean value of stress and strain; it does not affect the shape of the stress-strain curves or the amount of energy dissipated during the cycle.

line

Plastic strain [x10⁻³]	Stress (periodicity condition imposed from iteration 1)	Stress (periodicity condition imposed from iteration 5)
-10.00	-80.00	-80.00
-5.00	-60.00	40.00
0.00	-40.00	60.00
5.00	-20.00	80.00

Figure 6.2.6–3 Influence of periodicity condition on mean value of the strains over a stabilized cycle.

By delaying the application of periodicity conditions, you can influence the mean stress and strain level. However, this is rarely necessary since the average stress and strain levels are usually not needed for low-cycle fatigue life predictions.

You can control when the periodicity conditions are applied by defining direct cyclic controls to specify the variable I _ { P I } . This variable defines from which iteration onward the application of periodic conditions will be activated. For example, setting I _ { P I } = 6 means that the periodicity conditions are applied from iteration 6 onwards. The default is I _ { P I } = 1 , which is appropriate for most analyses.

Input File Usage: *CONTROLS, TYPE=DIRECT CYCLIC IP1

Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit; Direct Cyclic:

Initial conditions

Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified (see “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. During the analysis, prescribed boundary conditions must have an amplitude definition that is cyclic over the step: the start value must be equal to the end value (see “Amplitude curves,” Section 34.1.2). If the analysis consists of several steps, the usual rules apply (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1). At each new step the boundary condition can either be modified or completely defined. All boundary conditions defined in previous steps remain unchanged unless they are redefined.

Loads

The following loads can be prescribed in a direct cyclic 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.”

During the analysis each load must have an amplitude definition that is cyclic over the step where the start value must be equal to the end value (see “Amplitude curves,” Section 34.1.2). If the analysis consists of several steps, the usual rules apply (see “Applying loads: overview,” Section 34.4.1). At each new step the loading can either be modified or completely defined. All loads defined in previous steps remain unchanged unless they are redefined.

Predefined fields

The following predefined fields can be specified in a direct cyclic analysis, as described in “Predefined fields,” Section 34.6.1:

• Temperature is not a degree of freedom in a direct cyclic analysis, but nodal temperatures can be specified as a predefined field. The temperature values specified must be cyclic over the step: the start value must be equal to the end value (see “Amplitude curves,” Section 34.1.2). If the temperatures are read from the results file, you should specify initial temperature conditions equal to the temperature values at the end of the step (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). Alternatively, you can ramp the temperatures back to their initial

condition values, as described in “Predefined fields,” Section 34.6.1. 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. The field variable values specified must be cyclic over the step.

Material options

Most material models, including user-defined materials (defined using user subroutine UMAT), that describe mechanical behavior are available for use in a direct cyclic analysis.

The following material properties are not active during a direct cyclic analysis: acoustic properties, thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity properties, piezoelectric properties, and pore fluid flow properties.

Rate-dependent yield (“Rate-dependent yield,” Section 23.2.3), rate-dependent creep (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4), and two-layer viscoplasticity (“Two-layer viscoplasticity,” Section 23.2.11) can also be used during a direct cyclic analysis.

Elements

Any of the stress/displacement elements in Abaqus/Standard can be used in a direct cyclic analysis (see “Choosing the appropriate element for an analysis type,” Section 27.1.3).

Output

Different types of output are available for postprocessing and for monitoring a direct cyclic analysis.

Message file information

Abaqus/Standard prints the residual force, time average force, and a flag to indicate if equilibrium was satisfied in the message (.msg) file at different time increments for each iteration. You can control the frequency in increments at which information is printed to the message file, and you can suppress the output; the default is to print output every 10 increments (see “The Abaqus/Standard message file” in “Output,” Section 4.1.1, for more information).

Abaqus/Standard also prints the number of Fourier terms used, the maximum residual coefficient, the maximum correction to displacement coefficients, and the maximum displacement coefficient in the Fourier series in the message file at the end of each iteration. An example of the output is shown below:

		ITERATION	26 STARTS
INC	TIME	STEP	LARG. RESI.	TIME AVG.	FORCE
	INC	TIME	FORCE	FORCE	Equiv.
10	0.250	2.50	1.008E+01	50.9	N

20	0.250	5.00	1.622E+01	76.8	N
30	0.250	7.50	4.622E-02	99.8	Y

	ITERATION	26 SUMMARY
NUMBER OF FOURIER	TERMS USED 40,	TOTAL NUMBER OF INCREMENTS	120
CYCLE/STEP TIME	30.0,	TOTAL TIME COMPLETED	31.0
AVERAGE FORCE	21.2	TIME AVG. FORCE	25.7

MAX. COEFFICIENT OF DISP.	0.142	AT NODE 24	DOF 2
MAX. COEFF. OF RESI. FORCE ON CONST. TERM	31.7	AT NODE 44	DOF 1
MAX. COEFF. OF RESI. FORCE ON PERI. TERMS	0.82	AT NODE 6	DOF 3
MAX. CORR. TO COEFF. OF DISP. ON CONST. TERM	0.002	AT NODE 50	DOF 3
MAX. CORR. TO COEFF. OF DISP. ON PERI. TERMS	0.015	AT NODE 50	DOF 3

Results output

Element and nodal output are written only when the stabilized cycle is reached. If a stabilized cycle has not been reached at the end of an analysis, output is written for the last iteration of the step. The element output available for a direct cyclic analysis includes stress; strain; energies; and the values of state, field, and user-defined variables. All the energies are set equal to zero at the beginning of each iteration since energies dissipated over an entire stabilized cycle are of interest in making fatigue life predictions in direct cyclic analysis. The nodal output available includes displacements, reaction forces, and coordinates. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1.

Recovering additional results for an iteration

You may want to recover additional results for an iteration rather than for the 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). This feature is particularly useful if you want to evaluate the shift of the strain from one iteration to another iteration when plastic ratchetting occurs.

Input File Usage: *POST OUTPUT, ITERATION=n

Abaqus/CAE Usage: Recovering additional results for an iteration is not supported in Abaqus/CAE.

Specifying output at exact times

Output at exact times is not supported for direct cyclic 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 direct cyclic analysis is subject to the following limitations:

• Contact conditions cannot change during a direct cyclic analysis; they remain as they were defined at the beginning of the analysis or at the end of any general step prior to the direct cyclic step. Frictional slipping is not allowed during direct cyclic analyses; all points in contact are assumed to be sticking if friction is present.
• A direct cyclic step is always performed using the original coordinates of a model, even when the direct cyclic step follows a geometrically nonlinear step. To perform a direct cyclic analysis on the updated coordinates, you can use the import capability to import both the current state as well as the current configuration from the end of the desired geometrically nonlinear step.

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 (, INC=)
Set INC equal to the maximum number of increments in a single loading cycle
*DIRECT CYCLIC
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
*TIME POINTS
Data lines to list time points
*BOUNDARY, AMPLITUDE=
Data lines to prescribe zero-valued or nonzero boundary conditions
*CLOAD and/or *DLOAD, AMPLITUDE=
Data lines to specify loads
*TEMPERATURE and/or *FIELD, AMPLITUDE=
Data lines to specify values of predefined fields
*END STEP
**
*STEP (, INC=)
*DIRECT CYCLIC, DELTMX
Data line to control automatic time incrementation and Fourier representations
*BOUNDARY, OP=MOD, AMPLITUDE=
Data lines to modify or add zero-valued or nonzero boundary conditions
*CLOAD, OP=NEW, AMPLITUDE= 

Data lines to specify new concentrated loads; all previous concentrated loads will be removed

*DLOAD, OP=MOD, AMPLITUDE=

Data lines to specify additional or modified distributed loads

*TEMPERATURE and/or *FIELD, AMPLITUDE=

Data lines to specify additional or modified values of predefined fields

*END STEP

6.2.7 LOW-CYCLE FATIGUE ANALYSIS USING THE DIRECT CYCLIC APPROACH

Products: Abaqus/Standard Abaqus/CAE

References

• “Defining an analysis,” Section 6.1.2
• “Static stress analysis procedures: overview,” Section 6.2.1
• “Direct cyclic analysis,” Section 6.2.6
• “Crack propagation analysis,” Section 11.4.3
• “Damage and failure for ductile materials in low-cycle fatigue analysis,” Section 24.4
• “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1
• *DAMAGE EVOLUTION
• *DAMAGE INITIATION
• *DEBOND
• *DIRECT CYCLIC
• *FRACTURE CRITERION
• *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 low-cycle fatigue analysis:

• is characterized by states of stress high enough for inelastic deformation to occur in most cases;
• is a quasi-static analysis on a structure subjected to sub-critical cyclic loading;
• can be associated with thermal as well as mechanical loading;
• uses the direct cyclic approach to obtain the stabilized cyclic response of the structure directly;
• models progressive damage and failure in bulk ductile material based on a continuum damage mechanics approach, in which case damage initiation and evolution are characterized by the accumulated inelastic hysteresis strain energy per stabilized cycle;
• models propagation of a discrete crack along an arbitrary, solution-dependent path without remeshing in the bulk material based on the principles of linear elastic fracture mechanics (LEFM) with the extended finite element method, in which case the onset and growth of fatigue crack are characterized by the relative fracture energy release rate;

• models progressive delamination growth along a predefined path at the interfaces in laminated composites, in which case the onset and growth of fatigue delamination at the interfaces are characterized by the relative fracture energy release rate;
• uses the damage extrapolation technique to accelerate the low-cycle fatigue analysis; and
• assumes geometrically linear behavior and fixed contact conditions within each loading cycle.

Approaches to low-cycle fatigue analysis

The traditional approach for determining the fatigue limit for a structure is to establish the curves (load versus number of cycles to failure) for the materials in the structure. Such an approach is still used as a design tool in many cases to predict fatigue resistance of engineering structures. However, this technique is generally conservative, and it does not define a relationship between the cycle number and the degree of damage or crack length.

One alternative approach is to predict the fatigue life by using a crack/damage evolution law based on the inelastic strain/energy when the structure’s response is stabilized after many cycles. Because the computational cost to simulate the slow progressive damage in a material over many load cycles is prohibitively expensive for all but the simplest models, numerical fatigue life studies usually involve modeling the response of the structure subjected to a small fraction of the actual loading history. This response is then extrapolated over many load cycles using empirical formulae such as the Coffin-Manson relationship (see Coffin, 1954, and Manson, 1953) to predict the likelihood of crack initiation and propagation. Since this approach is based on a constant crack/damage growth rate, it may not realistically predict the evolution of the crack or damage.

Low-cycle fatigue analysis in Abaqus/Standard

The direct cyclic analysis capability in Abaqus/Standard provides a computationally effective modeling technique to obtain the stabilized response of a structure subjected to periodic loading and is ideally suited to perform low-cycle fatigue calculations on a large structure. The capability uses a combination of Fourier series and time integration of the nonlinear material behavior to obtain the stabilized response of the structure directly. The theory and algorithm to obtain a stabilized response using the direct cyclic approach are described in detail in “Direct cyclic algorithm,” Section 2.2.3 of the Abaqus Theory Guide.

The direct cyclic low-cycle fatigue procedure models the progressive damage and failure both in bulk materials (such as in solder joints in an electronic chip packaging or intra-laminar crack growth in laminated composites) and at material interfaces (such as delamination in laminated composites). The former can be based on either a continuum damage mechanics approach or the principles of linear elastic fracture mechanics with the extended finite element method. The response is obtained by evaluating the behavior of the structure at discrete points along the loading history (see Figure 6.2.7–1). The solution at each of these points is used to predict the degradation and evolution of material properties that will take place during the next increment, which spans a number of load cycles, . The degraded material properties are then used to compute the solution at the next increment in the load history. Therefore, the crack/damage growth rate is updated continually throughout the analysis.

The elastic material stiffness at a material point remains constant and contact conditions remain unchanged when the stabilized solution is computed at a given point in the loading history. Each of the