Advances in Materials Science and Engineering

Volume 2016, Article ID 2193684, 7 pages

http://dx.doi.org/10.1155/2016/2193684

## A Modified Fatigue Damage Model for High-Cycle Fatigue Life Prediction

^{1}Department of Engineering Mechanics, Southeast University, Nanjing 210096, China^{2}Jiangsu Key Laboratory of Engineering Mechanics, Nanjing 210096, China

Received 15 November 2015; Revised 17 January 2016; Accepted 20 January 2016

Academic Editor: Konstantinos G. Anthymidis

Copyright © 2016 Meng Wang et al. This is an open access article distributed under the Creative Commons Attribution License, which permits unrestricted use, distribution, and reproduction in any medium, provided the original work is properly cited.

#### Abstract

Based on the assumption of quasibrittle failure under high-cycle fatigue for the metal material, the damage constitutive equation and the modified damage evolution equation are obtained with continuum damage mechanics. Then, finite element method (FEM) is used to describe the failure process of metal material. The increment of specimen’s life and damage state can be researched using damage mechanics-FEM. Finally, the lifetime of the specimen is got at the given stress level. The damage mechanics-FEM is inserted into ABAQUS with subroutine USDFLD and the Python language is used to simulate the fatigue process of titanium alloy specimens. The simulation results have a good agreement with the testing results under constant amplitude loading, which proves the accuracy of the method.

#### 1. Introduction

Fatigue failure, as one of the major causes of damage for the mechanical components, relates to alternative loads subjected on engineering structures, which drew increasingly researching work focusing on the fatigue life prediction. There are two methods to forecast the structure fatigue life: one is fatigue safe life prediction based on fatigue cumulative damage theories and the other is damage tolerance method based on fracture mechanics [1]. In general, the fatigue life of material is estimated based on the damage tolerance method. However, a high proportion of the overall lifetime for the metal high-cycle fatigue is the fatigue initiation life [2].

Damage mechanics is the theory studying the mechanisms and rules of solid material degradation performance by changing mechanical variables under the external loads. As an important branch of damage mechanics, the continuum damage mechanics [3–5] is a theory based on continuum mechanics and irreversible thermodynamics. Therefore, the process of fatigue crack initiation and development can be analyzed by the fatigue life prediction model based on continuum damage mechanics. And the model of fatigue damage can be classified briefly into ductile fatigue damage model [6] and brittle fatigue damage model [7, 8]. Considering that the metal subjected to high-cycle fatigue could be regarded as quasibrittle material, the brittle damage mechanism is often employed to build a damage propagation model on the basis of irreversible thermodynamics [8], which is broadly accepted in engineering practices on account of less parameters of evolution equations. Moreover, the damage numerical analysis method is another core element of damage mechanics. The determination of damage field and the forecast of fatigue life have been achieved by the damage mechanics-finite element method [9–11], which can be utilized to obtain the lifetime of damage initiation and damage propagation path.

In this study, a brittle fatigue damage model is modified and combined with a damage constitutive model to predict the fatigue life of the metal material in Section 2. The method to estimate fatigue lifetime of titanium alloy components is accomplished by the commercial software ABAQUS which is developed by programming in Python and Fortran in Section 3. Then, the correctness of the fatigue damage model, the finite element model, and the simulation method is validated through comparing the analytical results with experimental results under constant amplitude loading in Section 4.

#### 2. Modified Fatigue Damage Model

The degeneration of material mechanical properties results from nucleation, growth, and integration of microcracks and voids within metal material. Thus, for one-dimensional structure, damage variable [3, 12] can be defined aswhere is the total area of the cross section and is the total area of microcracks and cavities.

Since Lemaitre [4] has obtained the true stress of material by the strain equivalence theory after damage initiation, the constitutive relation of material can be defined, under the state of one-dimensional stress, aswhere , , and are, respectively, the true stress of damaged material, the initial elasticity modulus of material, and the elastic strain.

The constitutive relation of three-dimensional isotropic damage material can be written aswhere means the material is undamaged and means the material has completely failed.

Here, a damage evolution model [8, 13] is introduced aswhere and are both material constants, is the maximum equivalent stress of loading (MISES), and is the minimum equivalent stress.

To obtain the stress and damage field of the model numerically, the nonlinear equations above are solved with the damage parameter as the increment variable. According to (3), is a constant matrix in the increment step of damage parameter. So, the damaged material can be considered as a “new” kind of undamaged material. For the linear elastic materials,where is the stress ratio of fatigue loads and a constant during the damage process.

Rewrite (4) intowhere and are the material constants in this study. Equation (6) is modified as follows:

Since the stress ratio is constant during the modeling cycle, is a constant too. The modified model has less fitting parameters and is accommodative to be integrated into finite element programs.

Combined with geometric equation, constitutive relation, equilibrium equation, and boundary conditions, the damage evolution model modified above can be applied to compute the lifetime based on known conditions of stress and damage. The lifetime estimation of damage initiation and propagation is accomplished by the damage mechanics-finite element method.

#### 3. Numerical Methods of Fatigue Life Prediction

Damage mechanics-finite element method [10, 13] is employed for the fatigue life prediction and damage field simulation. The main feature of the method is that the damage increment of dangerous point is kept constant in the analytical process. The steps could be described as follows:(1)Finite element model considering damage is developed. At the first loading step, the values of damage of the elements are assumed to be zero.(2)Damage evolution is calculated according to the stress field, and the element with a maximum damage value is selected as the dangerous point of the structure. Furthermore, the damage status of the dangerous point needs to be checked during every loading step, and if it has failed, the dangerous point of the structure should be reestimated.(3)Life increment of the th modeling cycle () is calculated according to (7): The value of total life is updated as(4)The damage increment of gauss points of other elements is obtained on the basis of life increment: The damage values of gauss integral points of each element are(5)With the new damage field, the stress field is updated until the components lose efficacy or is infinitesimally smaller than .

The damage mechanics-finite element method is implemented in ABAQUS, coding with Python and Fortran to use the built-in functions, such as finite element modeling, postprocess of stress, and damage field analysis results. The implementation flow chart of damage mechanics-finite element method is shown in Figure 1.(1)Firstly, finite element model is built using the Python language in ABAQUS and at the same time the initial value of damage field is set to zero.(2)Secondly, the damage field is imported by a subroutine named SDVINI and passed to another subroutine named USDFLD. After that, the structural stress will be analyzed.(3)Thirdly, after the stress distributions of the inner structure are obtained, Python language is used to read the results, confirm the dangerous points of structure, obtain the life increment and damage values of other gauss integral points considering the damage increment, and output the file containing damage status of the model.(4)Fourthly, the dangerous point needs to be reselected if the damage value of dangerous element reaches a critical state, and step is conducted until the component loses efficacy.