Prediction of Bolted Joint Dynamics Based on the Thin-Layer Element of Nonlinear Material

2.1 The TLE method

The TLE method is an approach to model the joint surface. It was initially developed to model the rock interface, which features thin elements and a large width-to-thickness ratio. The constitutive model of the thin elements can be expressed as the matrix below:

$\left\{ \begin{matrix}   {{\sigma }_{1}}  \\   {{\sigma }_{2}}  \\   {{\sigma }_{3}}  \\   {{\tau }_{12}}  \\   {{\tau }_{23}}  \\   {{\tau }_{31}}  \\\end{matrix} \right\}=\left[ \begin{matrix}   {{c}_{11}} & {{c}_{12}} & {{c}_{13}} & {{c}_{14}} & {{c}_{15}} & {{c}_{16}}  \\   {} & {{c}_{22}} & {{c}_{23}} & {{c}_{24}} & {{c}_{25}} & {{c}_{26}}  \\   {} & {} & {{c}_{33}} & {{c}_{34}} & {{c}_{35}} & {{c}_{36}}  \\   {} & {} & {} & {{c}_{44}} & {{c}_{45}} & {{c}_{46}}  \\   {} & {} & {} & {} & {{c}_{55}} & {{c}_{56}}  \\   Sym. & {} & {} & {} & {} & {{c}_{66}}  \\\end{matrix} \right]\left\{ \begin{matrix}   {{\varepsilon }_{1}}  \\   {{\varepsilon }_{2}}  \\   {{\varepsilon }_{3}}  \\   {{\gamma }_{12}}  \\   {{\gamma }_{23}}  \\   {{\gamma }_{31}}  \\\end{matrix} \right\}$        (1)

where, c_ij are unknown parameters. The number of unknown parameters can be reduced based on reasonable physical assumptions. Mayer and Gaul put forward four assumptions for these parameters: (1) The nondiagonal elements are zeros, because the joint surface does not shrink in the transverse direction.

(2) The parameters c₁₁ and c₂₂ are negligible, due to the lack of stiffness along the interface parallel to the joint surface.

(3) The normal stiffness of the joint is reflected by c₃₃, while the shear stiffness of the joint is defined by c₅₅＝c₆₆.

(4) The parameter c₄₄ is zero, due to the absence of in-plane shear stiffness.

According to the above assumptions, the constitutive model only contains the physical quantities that are perpendicular to the normal direction and parallel to the tangential direction of the joint surface.

2.2 Constitutive relation of shear stiffness

For a jointed structure, the increase in the excitation amplitude will push up the nonlinearity of the mechanical joint, which brings about two phenomena: the weakening stiffness and growing friction damping. To characterize the two phenomena, a nonlinear Richard-Abbot model was introduced to describe the stress-strain relationship in the tangential direction of the elements on the joint surface [12-14]:

$\sigma=\frac{\left(E_{e}-E_{p}\right) \varepsilon}{\left(1+\left|\frac{\left(E_{e}-E_{p}\right) \varepsilon}{S_{Y}}\right|^{n}\right)^{1 / n}}+E_{p} \varepsilon$            (2)

where, E_e and E_p are stick elastic stiffness and slip plastic stiffness, respectively; S_y is the yield point; n is the shape factor that controls the smoothness of the transition portion of the curve.

1.jpg

Figure 1. Stress-strain curves of different shape factors

Figure 1 shows the stress-strain curves of different shape factors. It can be seen that, when n=0, the curve takes the traditional linear form; with the increase of the shape factor, the stress-strain curve gradually approaches the smooth nonlinear form, which is suitable to describe the transition from stick state to micro-slip state or macro-slip state; as the shape factor further increases (n→∞), the curve approximates the bilinear elastoplastic shape (n=100). Therefore, the nonlinear Richard-Abbot model can describe the load-displacement backbone curves about the stick and micro-slip on the surface of a mechanical joint under external loads. With four unknown parameters (E_e , E_p, S_y and n), this parameterized constitutive model can be integrated into the main program of Abaqus, using the user-defined material function (VUMAT).

The model parameters in Table 2 are essentially function of the preload, roughness and material of the joint surface. These functions determine the stick and micro-slip of the joint surface. The parameters of the TLM in the finite-element model can be corrected effectively by minimizing the difference between the numerical and experimental load-displacement curves. The tangential load F_i^num obtained by numerical calculation can be described as:

$F_{i}^{\mathrm{num}}=f\left(x_{i}, E_{n}, E_{e}, E_{p}, S_{Y}, n\right)$      (3)

where, x_i are the discrete displacements. Then, the objective function can be optimized as:

Objective function$=\sum_{i=1}^{10}\left(F_{i}^{\operatorname{num}}-F_{i}^{\mathrm{exp}}\right)^{2}$       (4)

where, F_i^exp is the tangential load at displacement x_i. In addition to the origin, there are 10 pairs of load-displacement values. Considering its nonlinear material features, the finite-element model is time-consuming and costly to solve directly by an optimization algorithm. Here, the response surface methodology (RSM) and genetic algorithm (GA) are integrated to complete the parameter identification.

4.1 RSM and GA

The RSM is a statistical modelling tool that obtains the relationship between several explanatory variables and one or more response variable through regression analysis. Since its birth in 1951, the RSM has been widely applied in engineering [17-20]. Its creators, Box and Wilson, suggested approximating the relationship by a quadratic polynomial function:

$R \simeq a_{0}+\sum_{i=1}^{N} b_{i} v_{i}+\sum_{i=1}^{N} c_{i i} v_{i}^{2}+\sum_{i j(i<j)} c_{i j} v_{i} v_{j}$       (5)

where, R is the response, i.e. the load F_i^num; N is the number of input parameters; v_i is the encoded values of E_n, E_e, E_p, S_Y and n; a, b and c are regression coefficients.

The main idea of the RSM is to approximate the response model of the design of experiments (DOE) through a seires of experiments. Here, the DOE adopts the optimized Latin hypercube design [12, 13].

In the optimization process, the GA was employed to obtain the required parameters. Mimicking the natural selection process, the GA is detailed in the works of Mohan et al. [21-20].

In this paper, the RSM and the GA are integrated in the global leading optimization software, Isight.

4.2 Parameter identification based on Abaqus and Isight

As shown in Figure 5, Abaqus and Isight were combined to establish the response surface function and optimize model parameters. First, the finite-element model of the bolted joint was set up on Abaqus, together with a script file of Python. Being the input for Abaqus solver, the script file contains the entire finite-element model, the boundary and loading conditions, as well as the meshing and model parameters. Through the solving process, the load-displacement relationship was outputted to a destination file. The Python script and Abaqus solver were driven by Isight DOE components to automatically perform the numerical experiments. Table 3 shows the design intervals for the parameters at the time of the DOE. The optimized Latin hypercube technique was used to select 100 sampling points.

5.jpg

Figure 5. The integrated process of parameter identification

Table 3. Design intervals for parameters

The response surface function was defined with the linear least squares (LS) method. The objective function was created with Isight script components, and minimized with the GA. The resulting updated parameters are shown in Table 4.

Table 4. Updated parameters

6.jpg

Figure 6. Comparison between load-displacement curves obtained through numerical simulation and experiment

As shown in Figure 6, the load-displacement curve obtained through numerical calculation based on the updated parameters only differed slightly from that obtained by the experiment. In other words, the identified data can accurately reflect the response of the isolated bolted joint under external loads.