Johnson–Cook vs. Ductile Damage Material Models: A Comparative Study of Metal Fracture Prediction

Abstract

This study presents a comparative assessment of the Johnson–Cook (J-C) and Ductile Damage (DD) material models, evaluating their capability to replicate the tensile behavior and fracture development in ductile metals. Numerical models of AL6063-T4 aluminium and A36 steel dog-bone specimens with two different thicknesses were developed in ABAQUS to assess force–displacement response, stress–strain characteristics, and crack evolution under quasi-static loading. Results showed that specimen thickness directly doubled load capacity, while both models captured the overall elastic and plastic behavior of the materials. A key finding is that the DD model provided yield stresses closely matching the reference material values, whereas the J-C model exhibited higher apparent yields due to its intrinsic strain-rate sensitivity. Differences in damage behavior were also pronounced: the DD model better reproduced the gradual, inclined fracture path in aluminium, while the J-C model more accurately captured the strong necking-localization response characteristic of steel. Comparisons with experimentally tested specimens further supported these fracture tendencies. By analysing both materials under identical conditions, this work highlights the relative strengths and limitations of the two fracture formulations. The originality of the study lies in its systematic comparison across materials and thicknesses, providing clear guidance for selecting appropriate constitutive models in structural and computational mechanics research.

1. Introduction

Understanding material strength is crucial in engineering and science, particularly for materials commonly used in structural applications. In processes such as thin sheet metal forming, it is necessary to account for elastoplastic behavior, large deformations, and material anisotropy [1]. Tensile testing remains a fundamental method for characterising the elastic and plastic properties that define a material’s mechanical behavior [2]. Experimental observations suggest that matter exhibits a characteristic length scale, implying that a measurable quantity, such as strain, at a specific point reflects information from its surroundings [3].

Materials subjected to unusual loading conditions experience a wide range of strains, strain rates, temperatures, and pressures [4]. Under significant axial deformation, it becomes essential to modify the specimen’s geometry to account for the non-uniform stress and strain distribution in the necking region, ensuring an accurate description of the material’s response up to fracture.

Ductile fracture occurs in materials that undergo significant plastic deformation or necking before failure [5]. This behavior is typically governed by the nucleation, growth, and merging of voids, or through shear fracture arising from the formation of shear bands [6]. During a tensile test, a material initially undergoes elastic deformation and can return to its original shape upon unloading. As the applied load increases, the material undergoes permanent deformation and begins to thin or neck [7]. At this stage, micro-voids form at stress concentration areas, such as pores, inclusions, and grain boundaries, and eventually coalesce, leading to fracture [8,9].

Despite advancements in understanding the mechanical behavior of metals under various conditions [10,11,12,13,14], challenges remain in accurately predicting ductile fracture using numerical models. For instance, phenomenological formulations such as the Johnson–Cook model have been reported to exhibit limitations when applied outside their calibration regimes, including excessive damage localization and inaccurate fracture prediction under tensile loading and high stress triaxiality conditions [15]. Such discrepancies are particularly evident in the necking region, where strong coupling between plastic deformation and evolving stress states occurs.

To model the fracture mechanics of ductile metals, the literature has increasingly relied on advanced finite element formulations capable of handling large strain situations within a plasticity framework [15,16,17,18]. These formulations have been used to study ductile fracture under both isothermal and non-isothermal conditions [19,20,21,22]. However, only a few studies have systematically evaluated which type of material model is most effective in simulating fracture and deformation behavior in ductile metals.

Researchers [13] have compared the modified Lemaitre and Johnson–Cook (J-C) failure models to predict joint strength in the hot shear joining process. Their objective was to determine whether these models could be effectively applied in finite element (FE) simulations to compute shear joint strength and deformation behavior.

To improve materials’ fracture resistance, a comprehensive understanding of ductile fracture mechanisms is required. This necessitates an integrated approach that combines robust analytical description, advanced computational simulations and experimental observations. The Johnson–Cook and Ductile Damage models are widely used in engineering simulations involving large plastic deformation and material failure [23,24,25]. The Johnson–Cook model is commonly applied in impact, metal forming, machining, and crashworthiness analyses due to its robustness and straightforward calibration [26]. The Ductile Damage model is frequently employed in structural and fracture mechanics applications where progressive damage, void growth, and shear-dominated failure govern the response [27]. Their extensive use in practical engineering problems makes a direct comparison of their predictive capabilities both relevant and necessary. Hence, the aim of this study is to compare and evaluate numerically the effectiveness of commonly used material models, namely, the Johnson–Cook (J-C) and Ductile Damage (DD) models, in capturing tensile behavior of ductile metals.

2. Computational Simulations

As mentioned earlier, the aim of this study is to perform comparative analysis of the Johnson–Cook (J-C) and Ductile Damage (DD) material models using Abaqus Software (Version 2025, Dassault Systèmes, Vélizy-Villacoublay, France). The target is to find an optimum material model that can simulate uniaxial tensile behavior and predict fracture evolution in ductile metals.

2.1. Geometry and Testing Scheme

The geometry of the tested specimens used in this study was taken from studies involving tensile testing of ductile metals [21]. Figure 1 shows the standard dimensions of the dog-bone shaped specimen considered in this study. The geometry was modelled in ABAQUS/CAE with the same dimensions. Aluminium (6063-T4) and steel (A36) specimens were numerically modelled at two thicknesses, 1.5 mm and 3 mm, generating eight distinct simulation cases. Comparative analyses were conducted within each material type, evaluating the performance of the DD model against the J-C model at the specified thicknesses. To streamline the comparisons and for easier identification, each model has been assigned an abbreviation as highlighted in Figure 2 (e.g., AL-3.0-DD means: Aluminium, 3.0 mm thick, Ductile Damage model).

2.2. Numerical Model

The eight dog-bone specimens were modelled as deformable three-dimensional solid elements. This choice was favoured over shell elements, as solid elements more effectively capture complex behaviors such as necking and fracture. The use of solid elements allowed the model to better replicate a real tensile test scenario, thus improving the reliability and accuracy of the simulations. A homogeneous isotropic section was defined using the selected steel and aluminium alloys.

The 2 rectangular end plates with dimensions of 25 × 40 mm (Figure 1) were modelled as rigid bodies (Figure 3a). This was to ensure that the deformation is within the inner 80 mm (replicating lab testing where grip area is excluded). Moreover, such constraints can reduce the computational time. The specimen has a supporting end and a loading end (Figure 3b). Hence, in terms of boundary conditions, one end of the specimen was fixed (restraining all degrees of freedom), while the opposite end was allowed to displace through the tensile behavior. The reaction force at the fixed end point was recorded which is theoretically equivalent to the load required to cause such tensile behavior. The study also considered the stress, deformation and failure patterns of the computational model.

2.3. Loading

To replicate the experimental quasi-static loading, the computational analyses could not converge using Static/Abaqus-standard solver. This is related to the fact that the computational model contains large deformations and non-linear plasticity. Hence, the Abaqus-explicit solver was chosen. The use of Explicit dynamic solver for a quasi-static analysis is well-observed in the literature and approved by the software documentations. According to Abaqus documentations, “The explicit dynamics procedure is typically used to solve two classes of problems: transient dynamic response calculations and quasi-static simulations involving complex nonlinear effects” [28]. This explicit method calculates the response of the material at each increment explicitly, making it well-suited for capturing large deformations and fracture progression. To reduce the computational time required, the time for the explicit step was set as 0.04 s. In general, for quasi-static simulations incorporating rate-independent material behavior, the natural time scale is generally not important [29]. Uniaxial tensile load was applied using a pre-defined displacement with linear amplitude to simulate gradual elongation. The loading end point was displaced by 20 mm while the fixed end point remained constrained, ensuring realistic tensile behavior throughout the simulation. The displacement followed a linear gradual pattern from zero at time = 0 s till 20 mm at time = 0.04 s.

A loading-rate sensitivity analysis was additionally performed to verify the influence of the imposed explicit step time. Two tensile loading rates were considered: 0.5 m/s, corresponding to a forced displacement of 20 mm applied over 40 ms, and 0.25 m/s, corresponding to the same displacement applied over 80 ms. Figure 4 compares the resulting force-time responses for the numerical model of the 1.5 mm thick AL6063-T4 specimens predicted by the Ductile Damage (DD) model and the Johnson–Cook (J-C) model. For both constitutive formulations, the peak force values were essentially identical despite doubling the loading duration, reaching approximately 2.87 kN for the DD model and 3.1 kN for the J-C model. This indicates that the numerical response is insensitive to the applied loading rate within the investigated range. Consequently, the sensitivity analysis confirms that, for the present quasi-static simulations with rate-independent material behavior, the choice of time scale does not significantly affect the predicted mechanical response.

To ensure that the explicit analyses replicates the quasi-static regime, inertial effects were also monitored throughout the simulations. As shown in Figure 5, for both loading rates and constitutive models, peak kinetic energy (KE) remained significantly lower than peak internal energy (IE), confirming that the numerical response was dominated by material deformation rather than dynamic effects. Despite doubling loading duration, the nearly identical IE values (Figure 5) further confirms the insensitivity to loading rate.

2.4. Mesh Analysis

In terms of finite element type, hexahedral 3D elements were used. The C3D8I element type was selected, which is an eight-node linear brick element with incompatible modes. This element type is capable of modeling large deformations and complex behaviors associated with ductile fracture, making it well-suited for the simulation in this study. Mesh generation employed a sweep technique using the medial axis algorithm, which minimized transitions between elements and improved mesh smoothness.

A mesh sensitivity analysis was conducted using three element sizes (0.5 mm, 1 mm, and 2 mm) to assess the influence of spatial discretization on damage evolution (

Table 1. Influence of element size on the damage evolution in the numerical model of the tensile specimen.

Element Size	Numerical Model of the Tensile Specimen	Damage Evolution for AL6063-T4 Specimens
		DD	J-C
0.5 mm
1 mm
2 mm

) and global mechanical response (Figure 6). Table 1 illustrates the predicted damage patterns for the AL6063-T4 tensile specimen using the Ductile Damage (DD) and Johnson–Cook (J-C) models. For both constitutive formulations, mesh refinement led to improved localization of damage within the gauge section, with the 0.5 mm and 1 mm meshes producing more consistent and physically realistic fracture paths compared to the coarser 2 mm mesh, which exhibited more diffuse damage and reduced resolution of the fracture zone. Moreover, it is worth mentioning that the J-C model appeared to be less sensitive to mesh discretization compared to DD model.

Figure 6 compares the corresponding force–displacement responses. For both DD and J-C models, the elastic and plastic responses prior to damage initiation were largely mesh-independent, with all meshes predicting similar stiffness and peak force levels. Minor differences were observed in the post-peak softening and failure displacement, particularly for the coarsest mesh, which exhibited a slightly delayed or more abrupt loss of load-carrying capacity. The close agreement between the 0.5 mm and 1 mm meshes indicates numerical convergence, while the deviations observed for the 2 mm mesh reflect reduced accuracy in capturing damage localization. Overall, the results confirm that an element size of 1 mm provides an adequate balance between computational efficiency and accurate prediction of both damage evolution and global response for the DD and J-C models. Hence, the 1 mm mesh was selected as the optimal choice.

In all simulations, the out-of-plane direction of the tensile specimen was consistently discretized using three elements through the thickness to ensure adequate resolution of the stress and damage gradients while maintaining a reasonable computational cost. In Abaqus element controls, elements were deleted when the damage variable D reached 1.0 (complete failure), effectively removing elements that lost ~100% of stiffness. These settings ensured accurate modeling of material failure by removing elements that had significantly lost stiffness. This meshing approach was applied across all eight simulation scenarios ensuring consistent results for both materials under uniaxial tensile loading.

2.5. Johnson–Cook (J-C) Material Parameters

The Johnson–Cook (J-C) material model is a widely adopted phenomenological model that predicts material flow stress as a function of plastic strain, strain rate, and temperature. It is particularly valuable for simulating dynamic events such high-speed machining, impacts, and explosions where materials undergo complex loading conditions [4,11,30].

The strength model of the J-C material model describes how the flow stress ($\sigma$) of a material changes with plastic strain ($\epsilon$), strain rate ($\dot{\epsilon }$), and temperature (T). The model is represented by the following equation:

$$\sigma =\left(A+B{\epsilon }^n\right)\left(1+C\ln \left({\displaystyle \frac{\dot{\epsilon }}{{\dot{\epsilon }}_0}}\right)\right){\left(1-T^{\ast }\right)}^m$$

(1)

where A is the yield stress at the reference temperature, B is the hardening modulus, n is the strain hardening exponent, C is the strain rate sensitivity coefficient, m is the thermal softening exponent, $\epsilon$ is the equivalent plastic strain, $\dot{\epsilon }$ is the equivalent plastic strain rate, ${\dot{\epsilon }}_0$ is the reference strain rate, $T^{\ast }$ is the homologous temperature, defined as

$$T^{\ast }={\displaystyle \frac{T-T_{room}}{T_{melt}-T_{room}}}$$

(2)

where T is the current temperature, $T_{room}$ is the room temperature, and $T_{melt}$ is the melting temperature of the material. The material parameters must be measured at or below the transition temperature [4,31].

Within the constraints of large deflection, strain rate, and extreme heat, the J-C model may represent the material interactions between stress and strain [32]. Under conditions involving substantial deformation, high strain rates, and elevated temperatures, the stress–strain behavior of metallic materials can be effectively characterized by the J-C model. Researchers have used J-C model in different applications showing elastic, plastic and damage response [23,32,33,34]. The damage model in the J-C framework is used to predict the initiation and growth of damage leading to material failure [35]. It is described by cumulative damage parameter D:

$$D=\sum \left({\displaystyle \frac{\Delta \epsilon }{{\epsilon }_f}}\right)$$

(3)

where $\Delta \epsilon$ is regarded as the plastic strain increment and ${\epsilon }_f$ is the plastic strain at failure under the existing stress, temperature and strain rate [32]. The plastic strain at failure, ${\epsilon }_f$, is given by

$${\epsilon }_f=\left(d_1+d_2{e}^{d_3{\displaystyle \frac{p}{q}}}\right)\left(1+d_4\ln \left({\displaystyle \frac{\dot{\epsilon }}{{\dot{\epsilon }}_0}}\right)\right)\left(1+d_5{T}^{\ast }\right)$$

(4)

where ${\displaystyle \frac{\dot{\epsilon }}{\dot{{\epsilon }_0}}}$ is the non-dimensional plastic strain rate, ${\displaystyle \frac{p}{q}}$ is the pressure to Mises stress ratio and $d_1-d_5$ are the failure parameters.

In ABAQUS/Explicit, the J-C model supports progressive damage and failure modelling, allowing the implementation of initiation criteria and evolution laws. Material stiffness is reduced progressively until complete failure, at which the elements are deleted [36]. Utilizing the J-C dynamic failure model necessitates incorporating J-C hardening, but it does not require the inclusion of J-C strain rate dependency. Nonetheless, the rate-dependent term within the J-C dynamic failure criterion is only integrated when the J-C strain rate dependence has been explicitly defined [36].

The Johnson–Cook (J-C) material model requires accurate defined parameters to ensure reliable tensile behavior of the tested specimens.

Table 2. Johnson–Cook (J-C) material parameters of 6063-T4 Aluminum and A36 steel.

Category	Constant	Description	Units	Steel A36	AL6063-T4
Elastic constants	E	Young’s modulus	MPa	200,000	68,900
	ν	Poisson’s ratio	-	0.26	0.33
Density	ρ	Mass density	kg/m3	7850	2700
Yield stress and strain hardening	A	Yield strength	MPa	250	89.6
	B	Ultimate strength	MPa	525	172
	n	Work-hardening exponent	-	0.328	0.42
Reference strain rate	${\dot{\epsilon }}_0$	Typically for quasi-static loading	s−1	1.9 × 10−4	1 × 10−4
Strain rate sensitivity factor	C	For rate-independent material model	-	~zero, e.g., C = 1 × 10−10	~zero, e.g., C = 1 × 10−10
		For rate-dependent material model	-	0.0162	0.002
Adiabatic heating and temperature softening	$C_p$	Specific heat	J/kg-K	486	900
	χ	Inelastic heat fraction	-	0.9	0.9
	$T_m$	Melting temperature	K	1773	889.15
	$T_0$	Room temperature	K	293	293.2
	m	Thermal-softening exponent	-	0.917	1.34
Fracture strain constants	$d_1$	-	-	0.03	−0.77
	$d_2$	-	-	0.13	1.45
	$d_3$	-	-	−0.95	0.47
	$d_4$	-	-	0.036	0.00314
	$d_5$	-	-	0	1.6
Damage evolution		Displacement at failure (t = 1.5 mm)	mm	0.198	0.19
		Displacement at failure (t = 3 mm)	mm	0.25	0.24

provides the complete material properties of 6063-T4 Aluminum [37,38] and A36 steel [39,40].

As mentioned earlier, this study simulates a quasi-static analysis using Explicit dynamic solver. Hence, a rate-independent material should be defined where the stress should not change with the strain rate. This is achieved by setting the strain rate sensitivity factor C to zero. By setting C = 0, the term [1 + 0 × ln($\dot{\epsilon }$/$\dot{\epsilon }$₀)] becomes [1 + 0], which simplifies to 1, effectively making the flow stress dependent only on the plastic strain, A, B, and n, thereby making the model rate-independent. However, one can obtain an error when setting C to zero in Abaqus because the Johnson–Cook model is fundamentally a strain-rate-dependent model, and setting the strain rate sensitivity factor C to zero would essentially turn it into a rate-independent model. To tackle this problem, one can set the strain rate sensitivity factor C to a very small value close to zero, such as 1 × 10⁻¹⁰, as stated in Table 2. The underlined values in the table were not used in this study (added for reference). They can be helpful when rate-dependent material model is necessary, i.e., for simulations including dynamic loading.

It is important to mention that in Abaqus, the ‘reference strain rate’ in the J-C damage is the same as the reference plastic strain rate (epsilon dot zero) in the J-C plasticity rate-dependence. This rate, which typically corresponds to a quasi-static test is the baseline strain rate used in the model’s strain rate dependent term to normalize the effects of different strain rates.

The explicit analysis and the material model included adiabatic heating and temperature softening. In Abaqus, adiabatic heating refers to a material’s self-heating due to plastic deformation. This heat is generated by inelastic strain and may not have time to diffuse through the material, making it a critical factor in simulating processes with large strains and temperature-dependent material properties.

In the damage evolution, the ‘displacement at failure’ is the plastic displacement at which the damage variable D = 1. The value can be calculated as:

Displacement at failure = fracture strain × characteristic length

(5)

The characteristic length is a geometrical property of the element being used in the mesh, calculated as

• The cube root of the element’s volume (3D solid elements);
• The square root of the element’s area (2D shell elements);
• The element’s length (beams and trusses).

Table 3. The values of ‘displacement at failure’ calculated based on the fracture strain and the element characteristic length.

Specimen Thickness	A36 Steel	AL6063-T4
t = 1.5 mm	$0.25\times \sqrt[3]{0.5}=0.198$	$0.24\times \sqrt[3]{0.5}=0.19$
t = 3 mm	$0.25\times \sqrt[3]{1}=0.25$	$0.24\times \sqrt[3]{1}=0.24$

below shows how the given values of ‘displacement at failure’ were calculated. For future research, it is important to mention that ‘displacement at failure’ should be calculated for the studied model and should not be taken directly from Table 2 and Table 4.

In the current study, the fracture strain is 0.24 and 0.25 (for the aluminum and steel materials, respectively); the element volume is (1 × 1 × 0.5 = 0.5 mm³ for the 1.5 mm dog-bone specimen thick) and the element volume is (1 × 1 × 1 = 1 mm³ for the 3 mm dog-bone specimen thick). The element characteristic length is the cubic root of the element volume. Hence, Table 3 shows the values of ‘displacement at failure’ calculated based on the fracture strain and the element characteristic length.

2.6. Ductile Damage (DD) Material Parameters

Phenomenological fracture models are based on the fracture diagram that defines equivalent plastic strain at fracture ${\epsilon }_{eq}^{\ast \ast }$ as a function of the stress state, particularly stress triaxiality, η [6]. Accurate application of the Ductile Damage model depends on specifying the equivalent plastic strain at the point of damage initiation, along with the corresponding stress triaxiality, plastic strain rate, and the evolution of damage with respect to displacement [31]. For a linear fracture criterion, this relationship is straightforward. However, when a nonlinear behavior is involved, an integral formulation is necessary. This integral [6], that was developed by Kolmogorov, accounts for nonlinearity as follows:

$${\int }_0^{{\epsilon }_{eq}^{\ast \ast }}{\displaystyle \frac{d{\epsilon }_{eq}^{\ast \ast }}{{\epsilon }_{eq}^{\ast \ast }\left(\eta \right)}}=1$$

(6)

Hooputra et al. [6] proposed a modified equation that incorporates stress triaxiality, orthotropy, and boundary conditions of the equivalent fracture strain given by

$${\epsilon }_{eq}^{\ast \ast }={\displaystyle \frac{{\epsilon }_T^{+}\sinh \left[c\left({\eta }^{-}-\eta \right)+{\epsilon }_T^{-}\mathit{sinh}\left[c\left(\eta -{\eta }^{+}\right)\right]\right]}{\sinh \left[c\left({\eta }^{-}-{\eta }^{+}\right)\right]}}$$

(7)

where ${\epsilon }_{eq}^{\ast \ast }={\overline{\epsilon }}_D^{pl}\left(\eta ,\dot{{\overline{\epsilon }}^{pl}}\right)$ is the equivalent plastic strain as a function of stress triaxiality and ${\epsilon }_T^{+} \mathrm{and} {\epsilon }_T^{-}$ corresponds to the equivalent damage initiation for equibiaxial tensile and equibiaxial compressive deformations, respectively. If ${\eta }^{+}$ is the stress triaxiality for equibiaxial tension and ${\eta }^{-}$ indicates the stress triaxiality in equibiaxial compression, an isotropic material plasticity yields ${\eta }^{+}=2$ and ${\eta }^{-}=2.$ It is important to note that the values of stress triaxiality defined by Hooputra et al. [6] differ from those used in ABAQUS by a factor 1/3 [36]. The parameter $c$, or as defined in other studies as $k_0$, is introduced in the equation for the orthotropic case.

Once the damage initiation criterion is met, damage evolution plays an important role in describing the rate at which the material loses stiffness. In ABAQUS/Explicit, a plastic displacement-based linear damage evolution law is employed for each active failure mechanism. The stress tensor during the analysis is computed using the damage scalar equation [30,36]:

$$\sigma =\left(1-D\right)\overline{\sigma }$$

(8)

where $D$ is the overall damage variable and $\overline{\sigma }$ is the effective/undamaged stress tensor computed in the current increment.

A material is automatically removed from the mesh if all section points at any integration location have lost their load-carrying capacity, that is when $D=1$. The variable $D$ accounts for cumulative effect of all active damage mechanisms and is expressed in terms of individual damage variables [36].

For an elastic-plastic material, damage can manifest as either yield stress softening or elasticity degradation. Yield stress softening typically occurs post-necking, while elasticity degradation is observed during unloading [36]. The equivalent plastic strain at failure is dependent on the element’s characteristic length, making it unsuitable for defining damage evolution directly. Therefore, ABAQUS describes damage evolution in terms of equivalent plastic displacement or fracture energy [36]. The onset of damage ${\dot{\overline{\epsilon }}}_D^{pl}$, is governed by a critical equivalent plastic strain, which depends on both the stress triaxiality $\eta =-p/q$ where $p$ is pressure and $q$ is Mises equivalent stress and strain rate ${\dot{\overline{\epsilon }}}_D^{pl}\left(\eta ,\dot{{\overline{\epsilon }}^{pl}}\right)$ [36].

The Ductile Damage (DD) material model requires accurate defined parameters. Hence, Table 4 provides the complete material properties of 6063-T4 Aluminum [37,38] and A36 steel [39,40]. Elastic, density and adiabatic heating parameters were listed again to ensure that Ductile Damage (DD) material parameters are fully listed in one Table. The strain rate was set to zero to obtain a rate-independent material model that is necessary for quasi-static calculations. Regarding damage evolution, the ‘displacement at failure’ was calculated as mentioned earlier in Equation (5) and Table 3.

Table 4. Ductile Damage (DD) material parameters of 6063-T4 Aluminum and A36 steel.

Category	Description	Units	Steel A36	AL6063-T4
Elastic constants	Young’s modulus	MPa	200,000	68,900
	Poisson’s ratio	-	0.26	0.33
Density	Mass density	kg/m3	7850	2700
Plasticity	Yield strength	MPa	250	89.6
	Strain at yield	-	0.00125	0.0013
	Plastic strain at yield	-	0	0
	Ultimate strength	MPa	525	172
	Strain at ultimate strength	-	0.22	0.21
	Plastic strain at ultimate strength	-	0.219	0.209
Damage evolution	Fracture strain	-	0.25	0.24
	Stress triaxiality	-	0.33	0.33
	Disp. at failure (t = 1.5 mm)	mm	0.198	0.19
	Disp. at failure (t = 3 mm)	mm	0.25	0.24
Quasi-static	Strain rate	s−1	0	0
Adiabatic heating	Specific heat	J/kg-K	486	900
	Inelastic heat fraction	-	0.9	0.9

Table 4. Ductile Damage (DD) material parameters of 6063-T4 Aluminum and A36 steel.

Category	Description	Units	Steel A36	AL6063-T4
Elastic constants	Young’s modulus	MPa	200,000	68,900
	Poisson’s ratio	-	0.26	0.33
Density	Mass density	kg/m3	7850	2700
Plasticity	Yield strength	MPa	250	89.6
	Strain at yield	-	0.00125	0.0013
	Plastic strain at yield	-	0	0
	Ultimate strength	MPa	525	172
	Strain at ultimate strength	-	0.22	0.21
	Plastic strain at ultimate strength	-	0.219	0.209
Damage evolution	Fracture strain	-	0.25	0.24
	Stress triaxiality	-	0.33	0.33
	Disp. at failure (t = 1.5 mm)	mm	0.198	0.19
	Disp. at failure (t = 3 mm)	mm	0.25	0.24
Quasi-static	Strain rate	s−1	0	0
Adiabatic heating	Specific heat	J/kg-K	486	900
	Inelastic heat fraction	-	0.9	0.9

3. Results and Discussion

3.1. Force—Displacement Analysis

The force–displacement curves provide a direct assessment of the mechanical response of materials subjected to uniaxial loading. The results are illustrated in Figure 7a for AL6063-T4 specimens and Figure 7b for the A36 steel specimens, comparing the DD and J-C models.

The simulations revealed that specimen thickness plays a significant role in the force required to initiate fracture. Doubling the thickness of the dog-bone specimen from 1.5 to 3.0 mm doubled the maximum tensile load the specimen can reach before fracture initiation. The trend holds for the DD and J-C models. For example, the AL-3.0-DD (Figure 7a) reached a maximum load of 5.74 kN, twice the 2.87 kN required by the thinner model AL-1.5-DD (1.5 mm model). A similar pattern was observed for A36 steel specimens (Figure 7b). The findings indicate that increasing material thickness enhances not only the force-bearing capacity, but also the ductility of the specimen.

3.2. Stress–Strain Curves

From the force-displacement curves, the engineering stress–strain curves can be calculated. As is known, dividing the displacement values by the effective gauge length of 60 mm can give the strain. The engineering stress (in MPa) can be calculated by dividing the force (in N) by the cross-sectional area in mm². The cross-sectional area is 22.5 mm² (1.5 × 15 mm) or 45 mm² (3 × 15 mm), for the 1.5 mm thick specimens and the 3.0 mm specimens, respectively.

As shown in Figure 8, the stress–strain curves for the DD specimens reveal a linear elastic region followed by a clear yield point and subsequent strain hardening. In contrast, the J-C models start with linear elastic region followed by non-linear plasticity. For aluminum (Figure 8a), the yield points were approximately 88 MPa for DD models and 105 MPa for J-C models. Compared to the material yield strength (of 89.6 MPa) specified in Table 2 and Table 4, the DD models better estimate the yield strength than the value for J-C models. Such a higher yield point is expected in J-C models. This is because even though the material was defined as ‘rate-independent’, the J-C explicit dynamic formulation inherently involves inertia and strain-rate effects. In explicit dynamics, loads are applied as stress waves. The local stress can overshoot due to wave reflections and inertia before plastic deformation fully develops. This looks like a higher ‘apparent yield point’. For steel specimens (Figure 8b), the yield points were approximately 247 MPa for DD models and 300 MPa for J-C models. Compared to the material yield strength (of 250 MPa) specified in Table 2 and Table 4, the DD models better capture the yield strength than the higher value for J-C models. The reason for such difference is that the explicit dynamic solver inherently employs a central-difference time integration scheme, which may introduce small inertial effects during the early stages of loading. These effects can temporarily elevate local stresses before stable plastic flow develops. Owing to its stronger localization tendencies, the Johnson–Cook formulation makes this behavior more apparent, resulting in a slightly higher apparent yield point compared to the Ductile Damage model.

The ultimate strength values in the engineering stress–strain curves (Figure 8) cannot be directly compared to the material properties specified in Table 2 and Table 4. This is because Abaqus uses incremental large-strain plasticity. Each step updates stress based on the current configuration (not the original one). That means the stress integration is performed in the current (deformed) area and strain increments are logarithmic (true) increments. Therefore, if one provides engineering stress–strain, Abaqus will interpret it as true—and simulated material will look artificially softer because the code expects true data. In short, the simulated stress–strain curve will not match the experimental material properties (listed in Table 2 and Table 4) unless one converts simulation results to true stress–strain.

Analytically, the true stress–strain curves can be computed from the engineering stress–strain curves. The true strain = ln (1 + engineering strain) while the true stress = engineering stress × (1 + engineering strain). The results are presented in Figure 9 with closer mechanical properties to the ones specified in Table 2 and Table 4.

In the elastic region of J-C or DD models, the curves for both thicknesses are nearly identical, indicating consistent Young’s modulus values. The transition from elastic to plastic is smooth and well defined. A pronounced plateau is observed, representing the material’s capacity for significant plastic deformation without a substantial increase in stress. This plateau is well captured by the strain-hardening term in the J-C model. The sudden drop in stress following the plateau suggests abrupt failure.

In Figure 9a (aluminum specimens), the ultimate strength values of the DD and J-C models are 157 MPa and 164 MPa, respectively. Compared to the material ultimate strength (of 172 MPa) specified in Table 2 and Table 4, the difference is 8.7% and 4.7%, for the DD and J-C models, respectively. In Figure 9b (steel specimens), the ultimate strength values of the DD and J-C models are 500 MPa and 484 MPa, respectively. Compared to the material ultimate strength (of 525 MPa) specified in Table 2 and Table 4, the difference is 4.8% and 7.8%, for the DD and J-C models, respectively.

Table 5. The percentage error/difference between measured ultimate strength (Figure 9) and reference ultimate strength (Table 2 and Table 4) for the aluminum and steel specimens, comparing the DD and J-C models.

	Model	Ultimate Strength (from Figure 9)	Ultimate Strength (Table 2 and Table 4)	Error (%)
Aluminium (AL6063-T4)	DD	157	172	−8.7%
	J-C	164	172	−4.7%
Steel (A36)	DD	500	525	−4.8%
	J-C	484	525	−7.8%

shows the % error/difference between measured and tabulated ultimate strength values. This small difference (<9%) between defined and recorded material ultimate strength might be linked to the fact that the true curves in Figure 9 are computed analytically from the engineering stress–strain curves without taking into account element deletion or stress redistribution.

3.3. Damage Evolution

Figure 10 presents the crack patterns and damage evolution for AL6063-T4 Aluminum and A36 steel specimens simulated using two different constitutive models: the Ductile Damage model and the Johnson–Cook (J-C) damage model. The comparison highlights clear distinctions in how each material and model predict the onset, progression, and localization of failure.

In Figure 10, the damage initiation (D = 0) corresponds to the strain at which damage begins, often called the damage initiation strain or onset of softening. Damage evolution (0 < D < 1) is when material stiffness progressively decreases; the material is degrading but not broken yet. Damage completion (D = 1) represents loss of load-carrying capacity, i.e., the material is fully degraded and fracture occurs. The material fracture strain values are 0.25 (for aluminum) and 0.24 (for steel); Table 2 and Table 4 present the strain values where D = 1 (complete failure).

For AL6063-T4, the Ductile Damage model produces a more gradual and distributed damage evolution. The initiation of damage appears earlier in the deformation process, and the crack propagates in a smoother and more uniform manner along the expected ‘inclined’ failure path in aluminum. This behavior is consistent with the material’s relatively high ductility and the tendency of aluminum alloys to undergo significant plastic deformation before fracture. In contrast, the Johnson–Cook model predicts a more localized and abrupt damage zone. Damage tends to concentrate near the region of maximum plastic strain. This sharper localization is typical of the J-C model, which relies heavily on strain rate and stress triaxiality terms that can accelerate damage growth once initiated. Although necking is visible, the J-C prediction shows a comparatively more brittle-like failure mode, even for a naturally ductile material such as AL6063-T4.

For A36 steel, both models show higher strength and lower ductility of the steel specimen. The Ductile Damage model again exhibits a slightly more progressive damage evolution, with the crack initiating within the gauge region and propagating steadily as deformation increases. Conversely, the Johnson–Cook model predicts a more sudden collapse, with the damage concentrating sharply at the center of the specimen. The crack initiates later but grows rapidly once triggered, producing a failure pattern that is narrower and more localized. This behavior corresponds to the J-C model’s sensitivity to triaxiality, particularly in the presence of necking, where stress states promote rapid damage growth. The failure shape in J-C models is more consistent with experimental observations of mild steels, where necking and gradual loss of load-carrying capacity precede final fracture.

An additional qualitative comparison can be made by examining the experimentally fractured aluminium and steel specimens previously tested at the Structural Engineering Laboratory of Poznan University of Technology, as shown in Figure 11. Although these specimens were not tested specifically to validate the current numerical models, they offer useful insight into the realism of the simulated damage patterns. The aluminum specimens from earlier experiments consistently exhibited a pronounced inclined shear-type fracture surface, closely matching the failure orientation predicted by the Ductile Damage model. Conversely, the steel specimens showed a more localized necking zone followed by abrupt tensile rupture, a mode that aligns well with the concentrated damage band produced by the Johnson–Cook model. This qualitative agreement reinforces the interpretation that the DD model effectively captures gradual shear-dominated failure in more ductile alloys, while the J-C model is well suited to materials where fracture is driven by strong triaxiality and localized necking. In short, the DD model better reproduces the inclined, ductile fracture path in aluminum (as seen in experiments), while the J-C model better captures the necking-localization behavior of steel.

4. Conclusions

This study presents a comparative evaluation of the Johnson–Cook (J-C) and Ductile Damage (DD) material models in terms of their ability to simulate the tensile behavior and fracture evolution of ductile metals. Dog-bone specimens of AL6063-T4 Aluminum and A36 structural steel, modelled at two thicknesses, were analyzed to assess each model’s ability to capture force–displacement response, stress–strain characteristics, and crack progression under quasi-static loading.

The results demonstrated that specimen thickness has a dominant influence on the global tensile response, with load capacity scaling directly with cross-sectional area for both materials and models. While both constitutive models reproduced elastic stiffness and strain-hardening trends consistent with expected material behavior, the DD model provided more accurate predictions of yield strength. In contrast, the J-C model exhibited a slightly elevated apparent yield, attributed to its intrinsic strain-rate sensitivity. For aluminum, the predicted yield points were ~88 MPa (DD) and ~105 MPa (J-C), compared with the reference yield strength of 89.6 MPa. For steel, the predicted yields were ~247 MPa (DD) and ~300 MPa (J-C), versus a reference value of 250 MPa. True stress–strain curves generated from both models aligned with the reference material properties with an error/difference of less than 9%, confirming that both formulations can adequately represent overall plastic flow.

Clear distinctions emerged in the predicted damage evolution and failure mechanisms. The DD model produced a gradual, distributed softening response and an inclined shear-type fracture path in aluminum, closely matching typical experimental observations. The J-C model, however, displayed a stronger sensitivity to stress triaxiality, resulting in more localized necking and abrupt fracture, particularly in steel specimens- again consistent with commonly observed tensile failure in mild steels. Qualitative comparisons with previously tested specimens further supported these tendencies.

Overall, the findings provide practical guidance for selecting appropriate constitutive models in the design, assessment, and numerical simulation of ductile metallic components. Future work may extend the present comparison by considering computational cost, sensitivity to material parameters, and performance under different loading regimes, such as impact or cyclic loading.