Three-Dimensional Finite Element Modeling of Double-Twisted Hexagonal Mesh

doi:10.21203/rs.3.rs-3118725/v1

Download PDF

Research Article

Three-Dimensional Finite Element Modeling of Double-Twisted Hexagonal Mesh

https://doi.org/10.21203/rs.3.rs-3118725/v1

This work is licensed under a CC BY 4.0 License

Journal Publication

published 23 Jan, 2024

Read the published version in Journal of the Brazilian Society of Mechanical Sciences and Engineering →

You are reading this latest preprint version

The mesh structure based on double-twisted hexagonal grids is an important part of reinforced gabion structures. Due to challenges in sensor placement during physical experimentation on complex gabion mesh mechanical properties, numerical simulation serves as a valuable means of study, with accurate numerical grids being integral to obtaining reasonable results. This article proposes a novel approach for constructing a numerical model that incorporates unique geometric features. The approach categorizes mesh wire types into three groups based on their geometric structure and presents a relational equation governing the motion of a single wire axis during manufacturing. Secondly, A three-dimensional finite element model of a double-twisted hexagonal mesh was constructed using ABAQUS software to simulate a quasi-static uniaxial tensile experiment. Finally, the proposed approach was validated by comparing its numerical and experimental results, supporting its rationality. Additionally, it addresses the limited availability of three-dimensional numerical models for gabion meshes, thereby offering potential for further research on the mechanical properties of gabion structures under complex working conditions.

Double-twisted hexagonal mesh

3D model

Geometric parameters

Finite element method (FEM)

Mechanical analysis

Double-twisted hexagonal meshes are made of aluminum-plated low carbon steel wire, which is used extensively in various protection systems as a key component, for example, against rock fall (Duffy et al. 2005) and reinforced gabion walls (Quang et al. 2009; Zhang et al. 2007). Gabion walls are a proven construction solution with established results in slope and hydraulic applications (Cho et al. 2021; Srineash and Murali 2015). The meshes are the main components of gabion walls (Fig. 1(a)) and reinforced gabion embankment (Fig. 1(b)). At present, the research on double-twisted hexagonal meshes is primarily focused on its mechanical property with numerical simulations and physical experiments.

Physical experiments are often employed to provide the necessary material properties and to calibrate the numerical model. Thoeni et al. (2014) and Sasiharan et al. (2006) concluded that the mesh physical experiments can obtain the necessary mechanical characteristics. Bergado et al. (2001) and Wei (2017) studied the parameters of the interface friction characteristics between the meshes and the backfill by pull-out experiments. Yang et al. (2016), Zhang et al. (2007) and Hsieh et al. (2013) found that the key factors affecting the tensile strength are hexagonal mesh size, wire diameter, and wire winding method from the quasi-static tensile experiments. Meanwhile, the phenomenon of out-of-plane deformation characteristics of the mesh outside the tension device was also observed in the quasi-static tensile experiments of mesh. Mazzon et al. (2016) described the modalities to define a comprehensive experimental campaign of mesh. Physical experiments can provide a macroscopic understanding of the mesh’s mechanical properties. But physical experiments can only acquire fewer mechanical indicators, and a large number of sensors need to be deployed for more detailed research. There are many difficulties in sensor deployment for such complex models. Therefore, it is important to study the mechanical properties using numerical simulation, which is helpful to study the influence of different parameters and employed to optimize mesh designs or experimental schemes (Volkwein et al. 2011).

The discrete elements method (DEM) typically uses rigid spherical particles to assemble into arbitrary shapes with the intrinsic relationship of the material defined by the remote interaction forces between each particle. DEM had been applied in the design optimization of double-twisted hexagonal meshes (Bertrand et al. 2005; Pol and Gabrieli 2021; Previtali et al. 2021; Thoeni et al. 2013), of which the hexagonal mesh is represented by spherical particles located at the physical nodes of the mesh, and the interaction force of the wires is expressed by the force-displacement relationship obtained from physical experiments. Meanwhile, the geogrid element (Wei 2017) and the solid element (Su et al. 2021) are often used to simulate the simplified mesh models. The latter has been used to simulate the damage caused by impact blocks on rock-filled gabions. However, for discrete element models, the constitutive models for each type of wire overreliance on experimental calibration, and it is impractical to perform physical experiments on every type of mesh.

It is well known that the finite element method (FEM) is suitable for dealing with continuum problems such as nonlinear geometry, complex mechanical behavior, and various contact conditions. Nowadays, the FEM is used to simulate the mesh protection system as well as its parts, and some simplified models have been proposed based on the truss element (Cazzani et al. 2002; Gentilini et al. 2012; Tran et al. 2013), shell element (Sasiharan et al. 2006), and some special purpose elements (Priour 2003; Volkwein 2005). These models can simulate specific mechanical responses under a variety of loads at a low computational cost. However, these simplified models are lacking an accurately describing the mechanical properties of the wires, and the 3D deformation and the progressive failure characteristics of the mesh under external force are difficult to be acquired. Consequently, a detailed 3D model is an essential tool for the accurate prediction of mesh mechanical response under any given condition (Govoni et al. 2011), but only a few 3D models of the mesh have been achieved (Gentilini et al. 2012). These models are not simple enough for practical projects. Therefore, it is an urgent issue to establish a credible and efficient 3D finite element model.

In this article, the authors propose a detailed numerical modeling approach for 3D double-twisted hexagonal mesh based on the combination of SolidWorks software and ABAQUS software, with which the spatial complexity of the mesh adequately is considered, and the complex mesh modeling is implemented by capturing the trajectory of wire movement. The approximate modeling procedure is shown in Fig. 2. With the approach, the mesh structures of different sizes can be rapidly modeled by modifying the parameters, which introduces a new perspective to investigate double-twisted hexagonal meshes using numerical simulation. Subsequently, a detailed 3D mesh model is established for the experimental works of Thoeni et al. (2013), and the values of model parameters are discussed. To improve the efficiency of numerical simulation, the explicit algorithms and some skills are utilized in the study. Finally, the correctness and applicability of the model are confirmed by physical experimental results.

2.1 Overview of Double-Twisted Hexagonal Mesh

As shown in Fig. 3(a), the components of the double-twisted hexagonal mesh can be divided into the hexagonal mesh, the selvage wire, and the terminal wire according to the distribution position. The wires are wrapped around the terminal wire to form the winding wire. The main geometric dimensions of the mesh include the panel length L, the panel width W, the wire diameter d, and the hexagonal dimensions M×N. As shown in Fig. 3(b), the hexagonal mesh consists of the single wire and the double-twist, the angle between the single wire and the horizontal plane is α and the length of the double-twist is s.

Wires are twisted into each other by special machinery following certain geometric rules in production as shown in Fig. 4(a). The movement of the wires is geometrically regular, with multiple sets of identical hexagonal wires interwoven to form the mesh. Therefore, all of the wires can be considered as a trajectory of a cross-sectional circle perpendicular to and centered on its central axis. The central axis of the double-twist can be represented as the cylindrical spiral shown in Fig. 4(b).

The three basic factors that determine a cylindrical spiral are the direction, the pitch H, and the diameter D. The double-twisted spiral is characterized by linear motion along the braiding direction and rotation around the contact point of the two wires. The spiral of the two wires has the same direction, while the starting angle on the projection circle differs by 180° as shown in Fig. 5(a). The pitch H is determined by ascending turns r of the double-twist and the windings n as shown in Fig. 5(b). The obvious one is that r = n/2. The pitch H of the central spiral can then be obtained from Eq. (1).

$$H=\raisebox{1ex}{$s$}\!\left/ \!\raisebox{-1ex}{$r$}\right.=\raisebox{1ex}{$2s$}\!\left/ \!\raisebox{-1ex}{$n$}\right.$$

The proximity of the double-twist makes the cross-sectional circles at the same height as the central spiral tangent to each other and the diameter of the central spiral equal to the wire diameter D = d. Thus, there are five independent parameters required to model the double-twisted hexagonal mesh, which are the wire diameter d, the hexagonal dimensions M × N, the double-twisted length s, and the windings n.

It is important to note that the trajectory of the two points furthest apart on the same horizontal section during the movement of the double-twist is a cylindrical spiral, which is described as an enveloping spiral, as shown in Fig. 6. The spiral direction and pitch of the enveloping spiral are the same as the central spiral but the diameter D′ is twice as large as the central spiral, i.e., D′ = 2d. The lift angle ${\theta }^{{\prime }}$ of the envelope spiral can be obtained from Eq. (2).

$${\theta }^{{\prime }}=\text{arctan}\left(\frac{H}{\pi {D}^{{\prime }}}\right)=\text{arctan}\left(\frac{s}{n\pi d}\right)$$

The oblique angle α can be obtained from Eq. (3).

$$\alpha =\text{arctan}\left(\frac{N-s}{M}\right)$$

2.2 Modelling of the Wire Parts

SolidWorks® 2016 is a 3D CAD software that can change mechanical characteristics by modifying the parameters of models. In this section, the modeling process of double-twisted hexagonal mesh is introduced, based on the tensile experiments of Thoeni et al. (2013). In Thoeni’s work, the panel size of experiment meshes are L×W = 360×950 mm², and the detailed dimensional characteristics are listed in Table 1. Figure 7 shows the connection system, in which the black dots indicate the connection points between the clamp of the metallic plate and the mesh.

Table 1

The mesh characteristics and dimensions (Thoeni et al. 2013)
Mesh characteristics	Dimension
Length of the panel (L)	360 mm
Width of the panel (W)	950 mm
Mesh opening	80×100
Wire diameter (d)	2.7 mm
The windings (n)	3

The five parameters required for modelling are obtained once the double-twisted hexagonal mesh model has been determined. According to Eq. (1) and Eq. (3) the pitch H = 10 mm and the oblique angle α = 41° can be found. Similarly, the enveloping spiral lift angle ${\theta }^{{\prime }}=49.7^\circ$ is obtained from Eq. (2). The detailed parameters are listed in Table 2.

Table 2

Dimensional parameters of the mesh model
Geometrical parameters	Dimension	Geometrical parameters	Dimension
Mesh opening size (M)	80 mm	Pitch (H)	10 mm
Mesh opening size (N)	100 mm	Oblique angle (α)	41°
Length of double-twist (s)	30 mm	Spiral diameter (D)	2.7 mm
Selvage wire diameter	2.7 mm	Enveloping spiral lift angle (${\theta }^{{\prime }}$)	49.7°
Terminal wire diameter	2.7 mm

The mesh model is composed of three types of wires (i.e., the hexagonal mesh, the selvage wire, and the terminal wire as shown in Fig. 3(a)). The hexagonal mesh and the selvage wire are mainly composed of two parts, which would be called part A and part B. The terminal wire model is relatively simple and is a straight line. The flow chart of the mesh modeling is shown in Fig. 8, and the modeling process is described in the following.

The central axis of part A (Fig. 9(a)) is created in SolidWorks based on the mesh dimensional feature parameters (H, r, M, and N). As indicated by the red oval in Fig. 9(a), the central axis is misaligned with the single wire axis because of the oblique angle α is not equal to the enveloping spiral lift angle ${\theta }^{{\prime }}$, a transition is required for the connection of the double-twist to the single wire axis. In this article, the transition is smoothed using the chamfer which bevels a selected edge or vertex. After chamfering of α'=48°, the absolute error from the calculated angle α is 7°.

For part B, the tangent of the starting point in Fig. 9(b) is perpendicular to the mesh plane, it is necessary to change the tangent direction to match the physical model. After increasing the ascending turns r by 0.25 turns as shown in black cycle in Fig. 9(b), the central axis of the winding wire is adjusted by the chamfer function, and then is connected to another axis on the mesh plane.

Finally, the cross-sectional circle perpendicular to the axis is stretched along the central axis to obtain the 3D models of part A and part B, as shown in Fig. 10.

2.3 Modelling of 3D FE Mesh

After importing the model parts into the FEM software ABAQUS® 6.14, the mesh model will be built. The hexagonal mesh, the selvedge wire, and the terminal wire models are obtained by merging parts A&B through Boolean operations, and then the mesh model assembly is completed. The mesh for simulating the tensile experiment of Thoeni et al. (2013) is shown in Fig. 11.

According to the works of Thoeni et al. (2013), a numerical simulation of a uniaxial tensile experiment is performed for the assembled model in Fig. 11. The model adopts highly-detailed 3D 8-node reduced integration hexahedral solid elements (C3D8R). The friction coefficient is 0.3 (Buzzi et al. 2011), and normal contact is hard contact in general contact. The constraint and coupling points are marked in Fig. 11. Cylindrical and cubic rigid bodies are established at the model tension point and the boundary constraint. All behaviors of the rigid bodies are controlled by a single coupling point. The tensile rigid bodies are coupled to the reference point RP-1, which moves 65 mm along the Y-axis in 100 seconds. The bottom rigid bodies are coupled to the reference point RP-2, of which the displacement and rotation are frozen.

The stress-strain relation of the 2.7 mm wire is referenced, and Thoeni et al. (2013) summarized the stress-strain curve by physical experiment, as shown in Fig. 12.

Figure 12 shows that the wire is a typical elastic-plastic material with a long plastic phase, and the elastic modulus is E = 20000MPa. However, the curves obtained from wire tensile experiments represent the relationship between the characteristic stress and the characteristic strain, which are expressed as the nominal strain $\epsilon$_n and the nominal stress $\sigma$_n shown in Eq. (4) and Eq. (5).

$${\epsilon }_{\text{n}}=Δ l/{l}_{0}$$

$${\sigma }_{\text{n}}=F/{A}_{0}$$

in which, $Δ l$ is the amount of change in wire length, ${l}_{0}$ is the initial length, F is the load, and ${A}_{0}$ is the initial cross-sectional area.

It is well known that the elastic-plastic parameters of material should be independent from the section and size of the test sample and applicable in the numerical simulation of different mesh types to avoid the repetitive wire tensile experiments. Thus, a true strain $\epsilon$_t and a true stress $\sigma$_t are defined, as shown in Eq. (6) and Eq. (7).

$${\epsilon }_{\text{t}}={\int }_{{l}_{0}}^{l}\frac{dl}{l}=\text{ln}\left(\frac{l}{{l}_{0}}\right)=\text{ln}(1+{\epsilon }_{\text{n}})$$

$${\sigma }_{\text{t}}=\frac{F}{A}=\frac{F}{{A}_{0}\frac{{l}_{0}}{l}}={\sigma }_{\text{n}}(1+{\epsilon }_{\text{n}})$$

in which, l is the true length of the wires and A is the true cross-sectional area.

The plastic strain ${\epsilon }_{p}$ can be obtained from Eq. (8).

$${\epsilon }_{\text{p}}=\left|{\epsilon }_{\text{t}}\right|-\left|{\epsilon }_{\text{e}}\right|=\left|{\epsilon }_{\text{t}}\right|-\frac{\left|{\sigma }_{\text{t}}\right|}{E}$$

where ${\epsilon }_{e}$ is the elastic strain.

According to Eq. (4) to Eq. (8), the material plasticity obtained by inversion from the tensile data are listed in Table 3. Assign material properties using ${\sigma }_{\text{t}}$ and ${\epsilon }_{\text{p}}$ in Table 3, the tensile simulation of a single wire was performed and the nominal stress-strain curve was obtained, as shown in Fig. 12. The simulation result almost matches the tensile experimental data, which indicates that the elastic-plastic parameters are set correctly.

Table 3

The material parameters of wire
Material parameters
True stress (${\sigma }_{t}$)/MPa	301.577		476.837		532.967		600.300		626.750
Plastic strain (${\epsilon }_{p}$)		0.000		0.015		0.041		0.110		0.152

3.1 Reliability of Numerical Calculations

It is a typical quasi-static issue to stretch the mesh at a low loading rate. In general, the static and quasi-static analysis can be solved with ABAQUS/Standard. However, by using Standard, it frequently takes a long calculation time to handle the nonlinear issues (such as geometric nonlinearity, material nonlinearity, and nonlinear boundary conditions) and even fails to converge to the final solution. Explicit is suitable for solving nonlinear dynamic problems and quasi-static problems as well as highly nonlinear problems with varying contact conditions, by which the convergence of the nonlinear issues is resolved to a great extent. However, the detailed FE models are computationally expensive (Escallón et al. 2014). The mass scaling method refers to the technique of obtaining large explicit time steps by adding nonphysical mass to the structure, which is available for static or quasi-static simulations. Thus, the mass scaling method is adopted in order to improve the computational efficiency.

The stabilization time increments in ABAQUS/Explicit can be obtained from Eq. (9).

$$Δ t={L}_{e}/\sqrt{E/\rho }$$

where ${L}_{\text{e}}$ and ρ are the minimum characteristic element length and density of the element.

The initial time increment $Δ t$ of this model is 3.7 × 10^− 8s. Furthermore, during the simulation experiment, the elements extremely deform under the load, and the minimum characteristic size shortens rapidly. Deformed elements will consume more computing resources. By changing the mass scaling of elements to increase the time step, convergence and computational efficiency can be improved. However, mass increases lead to changes in the kinetic energy of the system, which may affect the dynamic behavior and the reliability of the results. Therefore, balancing the relationship between computational cost and model reliability becomes particularly important. Figure 13 shows the change curves of energy with the elongation of the mesh system, including the kinetic energy E_K, the total strain energy E_I, the artificial strain energy E_A, and the total energy balance E_T. As shown in Fig. 13(a), the E_K slowly increases to 7.0 J before the elongation reaches 14% and then decreases to 5.0 J when the elongation reaches 17%. At the elongation of 17%, the wire failure causes the kinetic energy to surge and then fall back rapidly. The E_K is almost negligible compared to the E_I, which means that the computational cost savings of using mass scaling without changing the quasi-static behavior of model.

The statement in the previous section shows that the reduced integration elements (C3D8R) are used in the simulation to reduce the computational cost. These elements have a small number of integration points in each direction. In some cases, the node displacement is not zero, but the strain obtained by interpolation is zero. This phenomenon is called hourglass, also known as non-physical zero energy deformation. The E_A is used to control the hourglass. Numerically, E_I is the sum of the E_A, the energy dissipated by plastic deformation, the energy dissipated by damage, and the recoverable strain energy (ABAQUS 2014). E_I and E_A are the outputs during the simulation experiment. As shown in Fig. 13, the E_I and the E_A exhibit a similar growth. In addition, the ratio of the E_A to E_I is an important indicator to judge whether the calculation results are reliable. The ratio of the E_A to E_I generated by the system is defined from Eq. (10).

$$\mu =\raisebox{1ex}{${E}_{A}$}\!\left/ \!\raisebox{-1ex}{${E}_{I}$}\right.$$

µ is highly correlated with the accuracy of calculation results. The larger the µ, the lower the reliability of the calculation results. Some scholars recommend that the value of µ must be controlled below 10% and preferably not exceed 5% (ABAQUS 2014; Cao and Shi 2009; Sun et al. 2019). As shown in Fig. 13(b), µ suddenly leaps to 7% and then drops to 3% at the beginning of the experiment, which is a normal phenomenon caused by the loading. Then, after a small fluctuation, µ decreases to 2.4% and the corresponding elongation is 3%. As the mesh elongation grows, the distortion of the elements becomes more and more serious, the value of µ gradually increases due to the E_A increases faster than the E_I until the elongation reaches 8%, at which µ equals 3%. After the elongation is greater than 8%, the growth rate of the E_A is slower than the E_I, resulting in µ continues to drop to 1.8% when the elongation is 17% and some wire break. In conclusion, µ is controlled below 3% and does not exceed the 5% limit during the whole simulation process.

The E_T is the total energy balance (ABAQUS 2014) during the simulation experiment on the whole mesh system. The closer the E_T is to 0, the better the convergence of all the energies in the simulation, and the better the reliability of the numerical simulation results. As shown in Fig. 13(a), the E_T is almost 0 until the elongation is 14%. The E_T rises progressively after the elongation is greater than 14%, but its maximum is only 0.6 J. The ratio of E_T to E_I is negligible, which means the convergence of all energies in the simulation is excellent.

From the analysis above, this simulation experiment is reliable.

3.2 Deformation Characteristics

Figure 14 presents the deformation characteristics of mesh under quasi-static uniaxial tension obtained by numerical simulation. During the mesh tensile process, a phenomenon similar to "necking" occurs in the X-axis direction. The hexagonal mesh near the tension boundary becomes longer and thinner, while the mesh inside maintains a better hexagonal shape.

As shown in Fig. 14(a), the final deformed mesh panel length is 353.0 mm, while the initial is 330.0 mm, thus, the mesh’s absolute displacement is only 23.0 mm, which is less than the displacement of the tension device (56.0 m). This phenomenon indicates that the double-twists would be compressed by the device to produce mechanical deformation during tension. In view of the fact that the displacement of the tension device is usually taken as the mesh extension in physical experiments, the recorded displacement in physical experiments is not the real mesh displacement.

Figure 14(b) shows the mesh displacement in the Z-direction, indicating that the mesh within the tension device has almost no deformation in the Z-direction, but the right selvage wire has an obvious bulge toward the Z-axis. The hexagonal meshes near the tension device are squeezed by it resulting in out-of-plane deformation. The bulging of the right selvage wire is caused by the terminal wire beyond the tension device bending inward, resulting in a column-like eccentric pressure instability, as shown in Fig. 14(c). This is consistent with the physical experimental phenomena and indicates that the mesh model can effectively demonstrate the 3D deformation characteristics under a specific load.

3.3 Stress Distribution

As the French standard requires, the stress at the failure of the mesh material must be between 350 and 550 MPa with a minimum elongation of 10% (Bertrand et al. 2008). The Mises stress cloud at the moment of wire failure is shown in Fig. 15, with the black circle being part of the most serious stress concentration, and the red circle being part of the more serious stress concentration. As shown in Fig. 15, the stress concentration is most serious at the hexagonal mesh opening around the tension device, and the maximum stress is 644 MPa. Simultaneously, some hexagonal mesh openings within the tension device also have a more serious stress concentration, with a stress magnitude of 590 MPa. The stress distribution of the mesh corresponds well to the macroscopic phenomena of the physical experiment of (Thoeni et al. 2013) shown in Fig. 16. In the physical experiments, most of the wires failed at the extremely deformed hexagonal mesh openings around the boundary of the tension device, where the most severe stress concentration occurred. Furthermore, failure locations in physical experiments are common at the tension device and the hexagonal mesh opening, which may be caused by the variability in the material properties of the wires as the stress magnitude at hexagonal openings is only 8% less than at the maximum. As far as the numerical model is concerned, compared with the DE model which can only obtain the wire where the break occurs, the FE model obtains the point on the failure wire.

There is no stress concentration in selvage wires and terminal wires, and the stress is 50 MPa on average. The terminal wires only provide a winding position for wires to maintain a specific shape of the mesh, and fail to improve the tensile mechanical properties. The tensile properties provided by the selvage wires are limited by the boundary constraint of the stretching device. To investigate the effect clearly, the stretching device needs to be improved, and the possibilities are to remove the boundary constraint and extend the stretching device in the panel width direction so that it stretches the entire mesh or apply tension along the horizontal direction.

3.4 Axial Force-Elongation Result

Figure 17 shows the force-elongation curves for the uniaxial stretching of the mesh obtained from physical experiments and numerical simulation respectively and it can be seen that the two have a good coincidence. The tensile failure process can be divided into two typical stages. The first stage is the tensile deformation of hexagonal mesh, and the second stage is the deformation of the wires. But the critical elongation of the two stages in numerical simulation is slightly different to that in physical experiment. It can be observed from the numerical simulation results that the axial force increases smoothly in the first stage, and the critical elongation is 8% which is larger than the 5% in physical experiment. After the elongation is greater than 8%, the slope of the curve remains constant until the wire fails.

The average force curve of the physical experiments has the same growth trend as the numerical experimental curve at the first stage. However, the error of the two curves increases obviously after entering the second stage, when the wire starts plastic deformation. It is different from the increase of the physical experiments, the curve slope of the numerical simulation shows a decreasing and then increasing trend. The slope of the second stage in the physical experiment increased obviously until failure, with a maximum axial force of 31.4 kN. But, the maximum axial force at wire failure in the numerical simulation is 30.5 kN. The error is about (31.4–30.5)/30.5 = 3%. In addition, in the physical experiment, the slope of the axial force curves decreases before the second stage ends, and the mesh shows a clear plastic flow, while the numerical experiment is more inclined to brittle failure. There are many possible reasons for the discrepancy. Firstly, the boundary conditions are different, the ideal rigid body in the numerical simulation makes the constraint conditions stronger, while the force causing the tension device deformation in the physical experiment may make the constraint weaker. Secondly, the explicit method will inevitably accumulate errors. In addition, all aspects are more desirable in the numerical simulations than in the physical experiments, where the mesh size and material properties would differ. But such errors are acceptable, particularly since they save a lot of computational costs. Compared with physical experiments, FE simulations are more convenient and economical. It can reveal the mechanical properties of the mesh to a certain extent.

A new 3D modeling approach was proposed in this article for the double-twisted hexagonal mesh, utilizing computer-aided design and implemented through the use of SolidWorks and ABAQUS software. This approach aims to more accurately replicate the mechanical tests of gabion structures and facilitate further research. Based on this approach, numerical simulation of the tensile test of a mesh (Thoeni et al. 2013) was conducted, leading to several notable conclusions:

There are five main geometric parameters affecting the mesh modeling, which are the windings n, the Length of double-twist s, the wire diameter d, and the hexagonal dimensions M×N. Based on these parameters, the numerical modeling of a double-twisted hexagonal mesh can be realized by using the proposed method.

The material parameters of wires in the numerical model are the elastic modulus$E$, the true stress $\sigma$_t and the plastic strain ${\epsilon }_{\text{p}}$, and the methods to get the values of these parameters have been given in the article.

The numerical simulations fit well with the physical experiments and provide a basic reproduction of the three-dimensional deformation characteristics and mechanical response of the mesh under a load.

In summary, the newly proposed numerical model in this paper has high accuracy and can accurately reflect the mechanical response of complex mesh structures. If the mass scaling is turned off, it can be tentatively considered that the model has a very strong potential for dynamic analysis and has a greater possibility of being applied to against rockfall simulation.

The following symbols are used in this paper:

A = true cross-sectional area;

${A}_{0}$ =initial cross-sectional area;

D = Spiral diameter;

$D{\prime }$ =Wire diameter of the spiral diameter;

d = Wire diameter;

$E$ =modulus of elasticity;

E _A=artificial strain energy;

E _I=total strain energy;

E _K =kinetic energy;

E _T=total energy balance.;

F = load;

H = pitch;

L = panel length of the mesh;

l = true length of the wires;

${L}_{e}$ =smallest characteristic element length;

${l}_{0}$ =initial length;

M = hexagonal mesh opening size of length;

N = hexagonal mesh opening size of width;

n = windings;

r = ascending turns of double-twist;

s = length of double-twist;

W = panel width of the mesh;

α = oblique angle;

$\alpha {\prime }$ =oblique angle after chamfering;

$Δ l$ =the amount of change in wire length;

$Δ t$ =Stabilization time increments;

${\epsilon }_{e}$ =elastic strain;

${\epsilon }_{n}$ =nominal strain;

${\epsilon }_{p}$ =plastic strain;

${\epsilon }_{t}$ =true strain;

θ = spiral lift angle;

${\theta }^{{\prime }}$ =enveloping spiral lift angle;

$\mu$ =ratio of the artificial strain energy to the total strain energy;

$\rho$ =density;

${\sigma }_{n}$ =nominal stress;

${\sigma }_{t}$ =true stress.

Acknowledgments

These writers wish to acknowledge the National Key R&D Program of China (Grant No. 2018YFF0300205) for the financial assistance that made this investigation possible.

Data Availability Statements

All data, models, and code generated or used during the study appear in the submitted article.

Conflicts of interests/Competing interests

The authors declare that they have no known competing financial interests or personal relationships that could have appeared to influence the work reported in this paper.

ABAQUS. 2014. User's Manual, Version 6.14. Providence: Dassault Systemes Simulia Corp.
Bergado, D. T., P. Voottipruex, A. Srikongsri, and C. Teerawattanasuk. 2001. "Analytical model of interaction between hexagonal wire mesh and silty sand backfill." Can. Geotech. J., 38 (4), 782–795. https://doi.org/10.1139/t01-019.
Bertrand, D., F. Nicot, P. Gotteland, and S. Lambert. 2005. "Modelling a geo-composite cell using discrete analysis." Comput. Geotech., 32 (8), 564–577. https://doi.org/10.1016/j.compgeo.2005.11.004.
Bertrand, D., F. Nicot, P. Gotteland, and S. Lambert. 2008. "Discrete element method (DEM) numerical modeling of double-twisted hexagonal mesh." Can. Geotech. J., 45 (8), 1104–1117. https://doi.org/10.1139/t08-036.
Buzzi, O., A. Giacomini, M. Spadari, and S. Fityus. "Numerical modeling of a rock fall mesh perforation upon impact."In Vol. 2 of Proc., 13th Int. Conf. Computer Methods for Geomechanics: Frontiers And New Application, IACMAG 2011. Centre for Infrastructure Engineering and Safety, edited by N. Khalili, and M. Oeser, 1141–1146. University of New South Wales (UNSW), Centre for Infrastructure Engineering and Safety (CIES).
Cao, J. F., and Y. P. Shi. 2009. ABAQUS finite element analysis frequently asked questions, first ed. [In Chinese.] Beijing: China Machine Press.
Cazzani, A., L. Mongiovı̀, and T. Frenez. 2002. "Dynamic finite element analysis of interceptive devices for falling rocks." Int. J. Rock Mech. Min. Sci., 39 (3), 303–321. https://doi.org/10.1016/s1365-1609(02)00037-0.
Cho, M. T. T., A. Chueasamat, T. Hori, H. Saito, and Y. Kohgo. 2021. "Effectiveness of filter gabions against slope failure due to heavy rainfall." Soils Found., 61 (2), 480–495. https://doi.org/10.1016/j.sandf.2021.01.010.
Duffy, J. D., S. M. Lowell, T. C. Badger, O. A. hattamleh, N. Sasiharan, S. Shu, and B. Muhunthan. 2005. "Analysis and design of wire mesh/cable net slope protection. Guidelines." https://www.semanticscholar.org/paper/Analysis-and-Design-of-Wire-Mesh%2FCable-Net-Slope-Duffy-Lowell/2434c41d536dfef95282c425ef0995a5a0d918d8#citing-papers
Escallón, J. P., C. Wendeler, E. Chatzi, and P. Bartelt. 2014. "Parameter identification of rockfall protection barrier components through an inverse formulation." Eng. Struct., 77, 1–16. https://doi.org/10.1016/j.engstruct.2014.07.019.
Gentilini, C., L. Govoni, S. de Miranda, G. Gottardi, and F. Ubertini. 2012. "Three-dimensional numerical modelling of falling rock protection barriers." Comput. Geotech., 44, 58–72. https://doi.org/10.1016/j.compgeo.2012.03.011.
Govoni, L., S. de Miranda, C. Gentilini, G. Gottardi, and F. Ubertini. 2011. "Modelling of falling rock protection barriers." Int. J. Phys. Model. Geotech., 11 (4), 126–137. https://doi.org/10.1680/ijpmg.2011.11.4.126.
Hsieh, C. W., C. W. Chang, I. W. Liu, and R. S. Liu. 2013. "Structural pattern effects on engineering behavior of hexagonal wire mesh gabion panels." Transp. Res. Rec., 2349 (1), 3–8. https://doi.org/10.3141/2349-01.
Mazzon, N., F. Ferraiolo, and M. Vicari. 2016. "Experimental study of the mechanical behaviour of double twisted steel mesh gabions." Procedia Eng., 158, 422–427. https://doi.org/10.1016/j.proeng.2016.08.466.
Pol, A., and F. Gabrieli. 2021. "Discrete element simulation of wire-mesh retaining systems: An insight into the mechanical behaviour." Comput. Geotech., 134, 104076. https://doi.org/10.1016/j.compgeo.2021.104076.
Previtali, M., M. O. Ciantia, S. Spadea, R. Castellanza, and G. Crosta. "Discrete element modeling of compound rockfall fence nets."In Vol. 26 of Proc., Challenges and Innovations in Geomechanics. IACMAG 2021. Lecture Notes in Civil Engineering, edited by M. Barla, A. Di Donna, and D. Sterpi, 560–567. Springer.
Priour, D. 2003. "Analysis of nets with hexagonal mesh using triangular elements." Int. J. Numer. Methods Eng., 56 (12), 1721–1733. https://doi.org/10.1002/nme.635.
Quang, T. S., H. Ghazi, and B. de Patrick. 2009. "A multiphase approach to the stability analysis of reinforced earth structures accounting for a soil–strip failure condition." Comput. Geotech., 36 (3), 454–462. https://doi.org/10.1016/j.compgeo.2008.06.003.
Sasiharan, N., B. Muhunthan, T. C. Badger, S. Shu, and D. M. Carradine. 2006. "Numerical analysis of the performance of wire mesh and cable net rockfall protection systems." Eng. Geol., 88 (1-2), 121–132. https://doi.org/10.1016/j.enggeo.2006.09.005.
Srineash, V. K., and K. Murali. 2015. "Pressures on gabion boxes as artificial reef units." Procedia Eng., 116, 552–559. https://doi.org/10.1016/j.proeng.2015.08.325.
Su, Y., C. E. Choi, Y. R. Lv, Y. Wang, and X. Li. 2021. "Towards realistic simulations of the impact dynamics of boulders on rock-filled gabion: Combined effects of rock shapes and their crushing strength." Eng. Geol., 283, 106026. https://doi.org/10.1016/j.enggeo.2021.106026.
Sun, L., C. Li, Y. Tie, Y. Hou, and Y. Duan. 2019. "Experimental and numerical investigations of adhesively bonded CFRP single-lap joints subjected to tensile loads." Int. J. Adhes. Adhes., 95, 102402. https://doi.org/10.1016/j.ijadhadh.2019.102402.
Thoeni, K., A. Giacomini, C. Lambert, S. W. Sloan, and J. P. Carter. 2014. "A 3D discrete element modelling approach for rockfall analysis with drapery systems." Int. J. Rock Mech. Min. Sci., 68, 107–119. https://doi.org/10.1016/j.ijrmms.2014.02.008.
Thoeni, K., C. Lambert, A. Giacomini, and S. W. Sloan. 2013. "Discrete modelling of hexagonal wire meshes with a stochastically distorted contact model." Comput. Geotech., 49, 158–169. https://doi.org/10.1016/j.compgeo.2012.10.014.
Tran, P. V., K. Maegawa, and S. Fukada. 2013. "Experiments and dynamic finite element analysis of a wire-rope rockfall protective fence." Rock Mech. Rock Eng., 46 (5), 1183–1198. https://doi.org/10.1007/s00603-012-0340-0.
Volkwein, A. 2005. "Numerical simulation of flexible rockfall protection systems." Computing in Civil Engineering, 1–11.
Volkwein, A., K. Schellenberg, V. Labiouse, F. Agliardi, F. Berger, F. Bourrier, L. K. A. Dorren, W. Gerber, and M. Jaboyedoff. 2011. "Rockfall characterisation and structural protection – a review." Nat. Hazards Earth Syst. Sci., 11 (9), 2617–2651. https://doi.org/10.5194/nhess-11-2617-2011.
Wei, F. 2017. "Pullout characteristics and conceptual model of gabion reinforcement." [In Chinese.] Chin. J. Rock Mech. Eng., 36 (7), 1670–1679. https://doi.org/10.13722/j.cnki.jrme.2016.0603.
Yang, G. L., J. Y. Duan, and Y. Zhang. 2016. "Experimental study on selvage strength characteristics of gabion mesh." [In Chinese.] J. Hunan Univ. Nat. Sci., 43 (7), 132–138. https://doi.org/10.3969/j.issn.1674-2974.2016.07.018.
Zhang, L., M.-h. Zhao, and W. He. 2007. "Working mechanism of two-direction reinforced composite foundation." J. Cent. South Univ. Technol., 14 (4), 589–594. https://doi.org/10.1007/s11771-007-0113-1.

Download PDF

Journal Publication

published 23 Jan, 2024

Read the published version in Journal of the Brazilian Society of Mechanical Sciences and Engineering →

Reviewers agreed at journal
29 Aug, 2023
Reviewers invited by journal
11 Aug, 2023
Editor assigned by journal
01 Jul, 2023
First submitted to journal
28 Jun, 2023

You are reading this latest preprint version

Three-Dimensional Finite Element Modeling of Double-Twisted Hexagonal Mesh

Status:

Journal Publication

Version 1

Abstract

Figures

1. Introduction

2. Methodology

2.1 Overview of Double-Twisted Hexagonal Mesh

2.2 Modelling of the Wire Parts

2.3 Modelling of 3D FE Mesh

3. Results and Discussion

3.1 Reliability of Numerical Calculations

3.2 Deformation Characteristics

3.3 Stress Distribution

3.4 Axial Force-Elongation Result

4. Conclusions

Notation

Declarations

References

Status:

Journal Publication

Version 1

Material parameters
True stress (\({\sigma }_{t}\))/MPa	301.577		476.837		532.967		600.300		626.750
Plastic strain (\({\epsilon }_{p}\))		0.000		0.015		0.041		0.110		0.152