Keywords

1 Introduction

Friction Stir Spot Welding (FSSW) is an advanced joining technique for lightweight materials such as aluminum alloys. The FSSW process is a variant of friction stir welding (FSW), proposed to make spot welding. Like friction stir welding (FSW), this process creates a softened region near the tool by heat generated from friction between the rotating tool and the sheets. Instead of moving the tool in FSW, the tool is fixed in the longitudinal direction of the workpiece while rotating. FSSW can make joints without melting the base metal, which is an advantage compared with the other spot welding processes (resistance spot welding) [1, 2]. In FSSW, the voids and defects from rapid solidification of fused aluminum alloy can be easily avoided.

As shown in Fig. 1, the FSSW process consists of three stages: plunging, stirring, and retracting [3]. During the plunging step, the tool with a probe pin penetrates the workpieces with high rotational speed and constant indentation rate. An anvil beneath the lower sheet is used to support the tool’s downward force. At stirring, after an indentation depth, the tool is stopped but continuously rotating. The materials adjacent to the tool are softened and mixed to form a solid-state joint [4]. Finally, the tool is drawn out of the sheets as shown in Fig. 1c. The quality of weld joint depends on the tool parameters, the rotation speed, the stirring time, and the characteristics of material being joined.

Fig. 1
figure 1

Illustration of the FSSW process: a plunging, b stirring, and c retracting [5]

Full size image

In [6, 7], Sundaram et al. performed FSSW experiments to optimize welding joints of similar and dissimilar material sheets. Because experiments are expensive and time-consuming, numerical simulation needs to be performed. Many studies were conducted to investigate various aspects of the FSSW process and the effects of the parameters on the weld geometries [8, 9]. However, it remains challenging to understand the complex FSSW process, Finite Element Analysis (FEA) is the most powerful to understand the complexities of thermal–mechanical problem during FSSW. The FEA of FSSW involves many complex problems such as thermal–mechanical coupling, boundary contact, and large deformation. Among the challenges, large deformation is the most difficult to deal with conventional FEM.

In [10], Awang and Mucino used a conventional Lagrangian approach to analyze energy generation of FSSW. The result showed a good agreement of the peak temperature and energy dissipation with the experiment [11]. However, the simulation only reached the beginning plugging stage of the process. Using the Lagrangian approach, due to extreme material deformation, severe mesh distortions are observed, and the calculation cannot run until the end [12].

In order to deal with large deformation problem, the coupled Eulerian–Lagrangian (CEL) method is one of the most advanced technologies [13,14,15]. This analysis technique combines two mesh approaches—Lagrangian and Eulerian—in the same analysis. The purpose of this technique is to avoid non-converging problems when performing simulations that involve high/extreme deformations. In contrast to the Lagrangian formulation, in Eulerian mesh, the node is fixed while the material can flow in the mesh. In [16], the CEL technique is used for FSSW simulation for one metal sheet to study the temperature evolution, mainly to investigate the feasibility of the method.

In this paper, we use the CEL approach to simulate the complex FSSW process of two overlap AL6061-T6 aluminum sheets. In Sect. 2, the modeling CEL technique will be introduced. The material model, friction contact treatment, heat transfer, and mass scaling problems are discussed. In Sect. 3, the numerical results are presented in comparison with experiment. Conclusion and future work are presented in Sect. 4.

2 Numerical Simulation

2.1 Experimental Setup

Su et al. [17] performed FSSW to produce joints on similar aluminum AL6061-T6 sheets (101.6 × 25.4 × 2 mm) with (25.4 × 25.4 mm) overlap area. The sheets were welded using a 5 horsepower milling machine under displacement-controlled conditions. The plunge motion was produced at a constant rate of 2 mm/s. The welding temperatures were measured by K-type thermocouples (having a response time of 0.5 s) at locations A, B, C, and D of 0.4 mm underneath the bottom surface of the lower sheet. Location A is at the center and B, C, and D are located at 4, 5, and 6 mm in the radial direction from A, respectively, as indicated in Fig. 2.

Fig. 2
figure 2

Position of thermocouples

Full size image

Three welding tools, named T1, T2, and T3, are used to perform the FSSW with tool radii of 4, 5, and 6 mm, respectively, see Fig. 4. These tools are made of high-speed steel SKD 11 thermal-treated. We consider tool geometry with a flat shoulder and flat pin. The tool rotation speed is set from 400 to 2000 rpm.

A weld joint made by FSSW in a lap-shear specimen is shown in Fig. 3a and a cross section of the weld is presented in Fig. 3b. To optimize the welded joint, welding process parameters (tool pin radius, shoulder radius, stirring time, indentation depth, and rotation speed) have been changed. Due to the limit of material and equipment, several configurations have been considered as in Fig. 4. Welding parameters are summarized in the Table 1.

Fig. 3
figure 3

a A weld joint with a 6061-T6 FSSW in a lap-shear specimen and b a cross section of the weld

Full size image
Fig. 4
figure 4

Geometry and material assignment in the Eulerian domain

Full size image
Table 1 Welding parameters and values
Full size table

To consider a larger number of sets of parameters, numerical simulations are needed. In the next section, we will reproduce these experiments by numerical simulations. CEL analysis developed in Abaqus/Explicit has been employed to study this problem. The model consists of one Eulerian domain for workpiece and Lagrangian domains for the tool and the anvil. The material temperature can be very high and significantly influences the mechanical response. Therefore, fully coupled thermal stress analysis is chosen in this study to account for heat generation by tool–workpiece friction and plastic deformation.

2.2 Geometry Configuration

To reduce the computational cost, only the overlap part of the two sheets is considered in simulation. We consider a Eulerian domain of 25.4 mm × 25.4 mm × 3.2 mm which is divided into three parts vertically as in Fig. 4. Two aluminum sheets of 1 mm each in the lower part and 1.5 mm of air in the upper part so that the material can flow in the domain. We assume that the material is not allowed to enter or leave the Eulerian domain.

The tool (Fig. 5) and the anvil (Fig. 6) have been modeled using the Lagrangian formulation with thermally coupled elements. The tool is modeled as a rigid body. The anvil is fixed at the bottom.

Fig. 5
figure 5

Tool configuration

Full size image
Fig. 6
figure 6

Model boundary conditions

Full size image

2.3 Material Model

In this study, it is assumed that the workpiece material is isotropic, plastic hardening as a function of strain and strain rate. FSSW induces high strain rate deformationand temperature softening. We employed strain, temperature-dependent viscoplastic Johnson–Cook model for aluminum workpiece. The flow stress is expressed as [18, 19]

$$\overline{\sigma }=\left[A+B{\overline{\varepsilon }}^{n}\right]\left[1+Cln\left(\frac{\dot{\overline{\varepsilon }}}{\dot{\overline{{\varepsilon }_{0}}}}\right)\right]\left[1-{\left(\frac{T-{T}_{room}}{{T}_{melt}-{T}_{room}}\right)}^{m}\right]$$
(1)

where \(\overline{\sigma },\overline{\varepsilon },\dot{\overline{\varepsilon }},\dot{\overline{{\varepsilon }_{0}}},{T}_{room},{T}_{melt}\) are flow stress, plastic strain, effective strain rate, reference strain rate, room temperature, and melting temperature, respectively.

In the Johnson–Cook damage model, the damage parameter is defined as

$$w=\Sigma \left(\frac{\Delta {\overline{\varepsilon }}^{pl}}{{\overline{\varepsilon }}_{f}^{pl}}\right)$$
(2)

where \(\Delta {\overline{\varepsilon }}^{pl}\) is a variation of equivalent strain rate, and \({\overline{\varepsilon }}_{f}^{pl}\) is the strain rate at failure and determined by

$${\overline{\varepsilon }}_{f}^{pl}=\left[{d}_{1}+{d}_{2}exp\left(\frac{{d}_{3}p}{q}\right)\right]\left[1+{d}_{4}ln\left(\frac{\dot{\overline{\varepsilon }}}{\dot{\overline{{\varepsilon }_{0}}}}\right)\right]\left(1+{d}_{5}\widehat{\theta }\right)$$
(3)

where \({d}_{1}-{d}_{5}\), are failure parameters, \(\widehat{\theta },p,q\) are transition temperature, pressure stress, and von Mises stress, respectively.

The AL6061-T6 parameters are chosen as below by Lesuer et al. [20] (Tables 2 and 3).

Table 2 Material parameter for AL6061-T6
Full size table
Table 3 Johnson–Cook parameter for AL6061-T6
Full size table

2.4 Contact and Boundary Conditions

In the models, the bottom surface of the anvil is fixed in all directions, and material is not allowed to enter or exit the domain as described in Fig. 4. The displacement of the tool is described by applying the boundary conditions at the reference points (center of top surface of the tool). During the plunging stage, the tool penetrates at a velocity of 2 mm/s and a rotation speed of 70 rad/s. During stirring, the tool is stopped at indentation depth, while continuously rotating; therefore, the displacement is removed while the rotation speed is maintained.

The contact interactions between the tool and the workpiece are included as general contact. Heat sources are from friction at tool–workpiece interface and plastic deformations. The general contact algorithm implements the penalty method with a friction coefficient. Following Backar et al. [21], the friction coefficient depends on the temperature. For simplification, we consider a constant value of 0.5 which corresponds to the friction coefficient at ambient temperature. It is assumed that the energy generated by friction is converted to heat and 90% of energy in plastic deformation is dissipated as heat [22].

The heat dissipation to the ambient should be also considered. For simplification, the heat removal from the bottom surface is modeled to be due to heat convection with a film coefficient of 3 W/m2 (air convection). The heat transfer from the side face and tool surface is simplified to be due to the convection heat transfer with a coefficient of 3000 W/m2 (replacing heat conduction in the anvil and specimen). Heat transfers between material layers are considered as thermal heat conductance with pressure dependence as derived from [23].

3 Results and Discussions

The history output is extracted for nodal temperature of 2 points at 0.4 mm from the anvil top surface (Point A and B as in Fig. 2).

3.1 Temperature Evolution

The temperature evolution is plotted in Fig. 7 for two points A and B. Experimental data is available in [17] and used as a reference in this paper. Three tool configurations have been considered as follows (Table 4).

Fig. 7
figure 7

Comparison of temperature history between numerical result and experiment a T1, b T2, and c T3

Full size image
Table 4 Welding parameters and values
Full size table

As can be observed from Fig. 7, the temperature increases when the tool pin contact with the workpiece. It is the result of heat generation from the friction between pin surface and aluminum surface. At 0.8 s, when the tool shoulder meets the surface, contact area is larger, more heat is generated, and temperature rises faster. At stirring, the temperature gradually increases to the maximum value and is then stable. For T1, the average errors at points A and B are 4.7% and 3.6%, respectively. For T2, the average errors are higher, 9.1% at point A and 7.8% at point B. For T3, we get 8.7% and 6.0% of average errors at points A and B, respectively. The temperature evolution at points A and B are in good agreement with the experiment.

3.2 Thermal Heat-Affected Zone

Figure 8 displays the plots of temperature at the 1 s stirring stage for three tools. The softening zone with the a close to 925 K, as well as TMAZ and HAZ, can be observed by visualization module. For the welds made by the three weld tools under identical processing conditions, the TMAZ sizes are generally proportional to tool size and the TMAZ profiles are quite similar. The TMAZ sizes are calculated equal to 4.4 mm, 6.2 mm, and 9.1 mm for simulation results of T1, T2, and T3, respectively. To compare, the TMAZ sizes estimated for experiments of T1, T2, and T3 are about 4 mm, 5.8 mm, and 8.2 mm, respectively. The computational results of the heat-affected zones are in relatively good agreement with the experiments.

Fig. 8
figure 8

Comparison of TMAZ between experimental and numerical results of T1, T2, and T3

Full size image

4 Conclusion

In this paper, a novel 3D thermal–mechanical coupling finite element analysis based on the CEL method has been used to simulate the friction stir spot welding process for joining two aluminum sheets. Details on material model, boundary conditions, and contacts have been presented. The computational results are in relatively good agreement with the experiments. Some conclusions are as follows: the CEL approach shows no mesh distortion and can be applied for extreme deformation problem; temperature diffusion, material flows, and mixture zone results can be obtained to evaluate the quality of the joint; CEL approach is computation cost where the mesh need to be refined. In the future work, this model can be used to investigate the influence of friction coefficient, heat convection and combined with machine learning to find the best parameters for the FSSW process.