The ability of any material to carry mechanical, thermal, or electrical loads is limited. Permanent damage occurs to the material when it is loaded beyond its capacity to recover. When the material is subjected to external loading, the atoms and/or molecules move and rearrange causing strain. If the strain is within elastic limit, the material will recover its original shape upon unloading.
However, if the applied external loads exceed yield stress, permanent deformation occurs, and the material will not be able to recover its original shapes upon unloading. In a ductile metal for example, if the plastic deformation exceeds the ultimate tensile strength of the material, the dislocations become concentrated in a localized region. Any additional plastic deformation leads to reduction in cross sectional area and further stress concentration in that region, ultimately leading to breaking of the material as shown in the image below.
Damage is a highly dynamic process and needs to be considered while simulating the behavior of components under high strains. There are many examples (including this fun one that we made) of finite element simulations that use damage material models to predict the behavior of materials and structures under different loading conditions. Here are some examples:
Crashworthiness Analysis: In automotive engineering, crashworthiness analysis is used to predict the behavior of a vehicle under crash conditions. Modeling damage with the FEA allows us to predict the extent and location of damage in the vehicle structure, as well as the occupant injury potential.
Metal Forming Simulation: In metal forming processes, such as forging or stamping, damage material models can be used to predict the onset and progression of damage, such as cracking or necking, in the material. This information can be used to optimize the forming process and prevent component failure.
Composite Material Analysis: Composite materials, such as carbon fiber reinforced plastics (CFRPs), have complex failure modes due to their anisotropic and heterogeneous nature. Finite element simulations with damage material models can be used to predict the onset and progression of damage, such as delamination or fiber fracture, in composite materials under different loading conditions.
Concrete Structure Analysis: Concrete structures, such as buildings or bridges, can experience damage due to various factors, such as weathering, seismic events, or overloading. Finite element simulations with damage material models can be used to predict the onset and progression of damage, such as cracking or spalling, in concrete structures under different loading conditions.
Biomechanical Analysis: In biomedical engineering, finite element simulations with damage material models can be used to predict the behavior of biological tissues, such as bone or cartilage, under different loading conditions. This information can be used to design and optimize medical implants or prostheses.
If damage is not defined in a material model, Abaqus continues to evaluate stress strain behavior indefinitely. Instead, the material behavior can be accurately represented by multiple damage initiation and evolution criteria. Let’s briefly discuss damage initiation and evolution for ductile materials in this article.
Incorporating Damage In An Abaqus Material Model
The figure below shows stress-strain behavior of a material undergoing damage. The solid line shows the damaged behavior of the material whereas the dashed line shows the material response when the damage is not present. The progressive degradation of material occurs due to damage after the stress exceeds ultimate tensile stress (UTS) of material. In the figure, σy0 and εpl0 are the UTS and equivalent plastic strain at the onset of damage, and εplf is the equivalent plastic strain at failure. At the failure point, the overall damage variable reaches the value D = 1. This overall damage variable D encompasses the combined effect of all the active damage mechanisms occurring within the material. The value of D at initiation of damage is zero and it progressively increases to 1 at the complete failure of material.
Two aspects must be considered in the damage model to implement it into a finite element simulation. One is defining when the damage is initiated in the element and the other is how the stresses in the elements evolve once the damage is initiated. These two aspects for ductile damage model are explained elaborately here.
Ductile Damage Criterion
This is a basic damage model used to define the fracture of metals using uniaxial test data. Fracture in ductile metals occurs due to nucleation, growth, and coalescence of voids. This damage criterion can be used along with equation of state and different plastic models such as Mises, Johnson-Cook, Drucker-Prager and Hill in Abaqus.
Damage Initiation
This model assumes that the equivalent plastic strain at the onset of damage εplD is a function of stress triaxiality and strain rate. The damage initiation occurs when the following condition is satisfied at the material integration point.
Here, ωD is the state variable that increases monotonically with plastic deformation in the material, η is the stress triaxiality and ε.pl is the equivalent plastic strain rate. Stress triaxiality is calculated as,
Here, p is the hydrostatic pressure from the stress tensor and q is the von Mises equivalent stress. The values of stress triaxiality for different loading modes are given in the table below.
At each step time increment of the analysis, the increment in damage variable ΔωD is calculated as,
The increment is added to the state variable at previous time increment and damage is initiated when this state variable reaches 1. If the damage is independent of equivalent strain rate ε.pl, its value can be prescribed as 0. The effect of temperature and other field variables can also be incorporated into this initiation criterion in Abaqus.
Damage Evolution
Once the damage is initiated in the material, the progression of stresses at integration point are highly effected. The material fails due to progressive degradation of material stiffness. Evolution defines how the material degrades after the damage initiation criteria is met. The equivalent plastic strain at failure depends on the element dimensions, it cannot be used as a material parameter. The parameters selected to define evolution should be independent of the element dimensions in the model.
Based on effective plastic displacement - In this criterion, the damage is defined as a function of plastic displacement after the damage initiation. This displacement is independent of the element size.
Based on energy dissipation - In this evolution method, fracture energy required for failure of the material is defined. This is the area under stress train curve after the initiation of damage.
Final Thoughts
Damage is a highly dynamic process and needs to be considered while simulating components subjected to very high strains. There are many damage initiation and evolution models available for finite element implementations in Abaqus. Hopefully, this article has provided some insights on the ductile damage criterion, which is very well suited to model fracture of metals.
We are always here to help, so if you have questions about damage in your models, or just FEA in general, don’t hesitate to reach out!