## Abstract

The article presents an example of a structural solution of a mesh facade installed on a public building. The types of loads that can affect the structure of such a mesh have been characterized. The course of the wire shaping process used to produce the described mesh was reported. A finite element method (FEM) model was developed to simulate mechanical phenomena occurring during the technological process of crimping stainless-steel wire. Material model parameters have been defined. The developed model was verified in production conditions. Relations between wire-forming loads and tensile limit loads, as well as the distribution of equivalent tensile stress forced by the crimping process and internal stresses after crimping, were determined. The description of the technological process was presented in a form of a graph. The work contains the results of strength tests of wire materials and shaping tools.

## Introduction

Steel wire is one of the basic metallurgical semi-finished products. By default, it is used to manufacture machine parts such as coil springs [1], transport ropes [2], conveyor belts, sieves, and power line cables [3]. In construction, which is another area of steel wire application, it is used to fabricate reinforced concrete elements [4], gabion meshes [5], rock curtains, as well as mesh facades introduced to the market a few years ago.

Thanks to the manufacturing technology of wire drawing, the wires obtain good strength properties at tensile loads. For example, concrete has high compressive strength but low tensile strength, so introducing a reinforcing wire system or mesh into the tensile stress area provides compensation for the weaker structure [4]. Elements made of wire, which in addition to tensile loads are subjected to torsional loads, include, among others, coil springs, transport ropes, braided power line cables, and gabion mesh. These elements are obtained from the plastic shaping process. Plastic forming introduces stresses in the shaped element, which are called internal stresses. These stresses affect the permissible range of external loads of the shaped element. Residual stresses can be reduced, e.g., by heat treatment.

Residual stresses have a particular impact on fatigue strength parameters. Load-bearing parts can be deliberately preloaded to reduce stress amplitude. The paper [6] presents the positive effects of introducing stresses in a plastically shaped stent segment. Residual stresses also arise in the machining process, which has been described, for example, in Ref. [7]. In publications [6,7], the finite element method (FEM) was used to determine the residual stresses.

The subject of the tests described below is a corrugated wire made of stainless steel and used to make a mesh facade mounted on the Lodz University of Technology building (Fig. 1).

In contrast to the hot-rolled reinforcing wire [8], the wire used in our research is cold-formed and is not subject to an annealing treatment due to the need to maintain gloss. Therefore, when analyzing the load capacity of such an element, it is necessary to take into account the residual stress arising during crimping.

The structure of the mesh facade (Fig. 2) consists of alternately interwoven corrugated vertical (1) and horizontal wires (2). The outer vertical edges of the mesh are curved and pressed into clamps (3) made of sheet metal. Holes, made in the clamps, and screws (5) are used to mount the mesh using the bracket (4) to the beams (7). These beams are combined to the building walls. The mesh tension force is imposed by springs (6) coupled with the bracket (4).

Mesh facades are an increasingly frequent subject of research, especially when it comes to their impact on construction elements of buildings. For example, in Ref. [9], an analysis of the aerodynamic effects of a mesh facade installed on the buildings of the Bocconi University (Milano) campus is presented. Laboratory tests were carried out using an aerodynamic tunnel in which rigid models of buildings constructed on a scale of 1:50 were placed. The authors identified the profile of dynamic pressure changes in front of and behind the mesh. These data make it possible to determine the aerodynamic drag forces acting on the mesh structure depending on the building location conditions. Knowledge of these interactions is useful when performing strength analyzes and selecting grid shapes and dimensions. It also shows the share of wind energy absorbed by the mesh facade and by other elements of the building.

An extreme case of strength analysis of the support structure of building facades is described in a work [10], where pyrotechnic effects were taken into account.

Another case of research indirectly related to mesh facades is the assessment of the impact of vines adjacent to facade grids on the functioning of passive energy-saving systems in buildings, as presented in a study [11]. Periodically, other factors may occur that cause loads on the mesh facades, such as icing of the structure, where the weight of the ice mesh adjacent to the wires can cause a significant increase in structural effort and, consequently, dangerous damage.

Works by Refs. [12,13] describe the results of fatigue tests on smooth wire subjected to axial loads and transverse contact loads. The tests were carried out for three high-strength steel, including stainless steel. It was found that if the transverse load does not exceed 50% of the longitudinal load capacity, the assumed fatigue limit for the longitudinal loads would not be reduced [12]. The fatigue criterion was developed along with a description of the destruction mechanism; however, no stress distribution analysis was conducted [12].

The authors of this publication took part in the development of the technological process of the corrugated wire for the mesh facade presented in Figs. 1 and 2. During the cooperation, it was found that a simulation model should be developed that would allow for the analysis of internal loads that arise during the production process and in the conditions of using corrugated wire. From a practical point of view, mapping the state of an internal load of the wire has become important, because it allows analyzing the load on production tools and thus controlling the parameters of the manufacturing process. Since the main load acting on the facade grid wires is the axial load, and it applies in particular to vertical wires (Fig. 2), this paper focuses on the strength analysis of such wires. The novelty of the presented publication is the practical (engineering) use of the finite element method to develop a universal model that can also be used for:

determination and analysis of the parameters of the wire crimping technological process (unit pressure of the tool depending on the set tool displacement range—tool stroke, tool internal load condition, etc.)

determination and analysis of strength parameters (distribution of equivalent tensile stress, destructive stresses) resulting from producing the crimped wire and from loads that may affect the product under conditions of use.

The task of the model presented below was a sound reproduction (in simulations) of the strength properties of the wire made of 316L stainless steel. An essential aspect of modeling was selecting a constitutive model (material model) of the tested system. It should also be considered that stainless steels are not typical material subjected to plastic forming treatments. The design of plastic forming processes for these steels is associated with many difficulties. The biggest problems arise from the small difference between the tensile strength and the yield point (yield point compared to typical plastic working materials).

## Description of the Wire Crimping Process

The wire crimping system is shown in Fig. 3. Crimping is a cyclical process. In the first step, the straightened (smooth) wire (1) is inserted between the jaws (2) via the feed rollers (3). In the second step, the jaws (2) embedded in the press warhead are steadily closed up (4). As a result of this operation, the wire undergoes permanent deformations. In the third step, the jaws and warhead move apart. During the fourth step, the shaped wire is taken over by the splines of the rotating rollers (5) while the simultaneous rotation of feed rolls (3). These rolls (3) have an independent synchronous drive realized by using a chain transmission and a stepper motor. The roller drive system works similarly (5). During one reciprocating cycle of the jaws (2), the shaped wire is displaced by the pitch value *P* (Fig. 4(a)). The replaceable jaws (2) are seated in the press warhead (4) and are fixed with screws (7). Vertical guides (6) have been placed in the warheads to ensure symmetry of the bends of the wire.

A wire made of 316L steel, in accordance with the standard [14], was used for wire crimping. The chemical composition of 316L steel is shown in Table 1. Despite the high tensile strength of the wires described in papers [12,13], they were not chosen for the grid production because they had almost twice the yield strength. Thus, the shaping process would require more energy input and more durable tools.

Material/chemical composition | C | Mn | Si | P | S | Cr | Ni | Mo |
---|---|---|---|---|---|---|---|---|

316L (%) | 0.021 | 0.66 | 0.31 | 0.035 | 0.002 | 16.28 | 10.07 | 2.04 |

42CrMo4 (%) | 0.38 | 0.4 | 0.17 | 0.035 | 0.3 | 0.9 | 0.3 | 0.15 |

Material/chemical composition | C | Mn | Si | P | S | Cr | Ni | Mo |
---|---|---|---|---|---|---|---|---|

316L (%) | 0.021 | 0.66 | 0.31 | 0.035 | 0.002 | 16.28 | 10.07 | 2.04 |

42CrMo4 (%) | 0.38 | 0.4 | 0.17 | 0.035 | 0.3 | 0.9 | 0.3 | 0.15 |

The basic outline and geometrical parameters of the vertical corrugated wire are shown in Fig. 4(a). These include plain wire diameter *d _{w}* = 2 mm, crimping pitch

*P*= 11 mm, bending radius

*R*= 1.8 mm, and embossing

_{w}*h*= 3.6 mm. Based on the assumed geometry of the corrugated wire, the basic geometrical dimensions of the working part of the jaw were defined (Fig. 4(b)):

*R*= 1.8 mm,

_{t}*b*= 2 mm,

*c*= 4 mm, and

*a*= 2 mm. The jaws are made of thermally improved 42CrMo4 material. When selecting the material model, a static tensile test of a smooth wire and a standard sample made of jaw material were carried out.

## Finite Element Method Model of the Wire Crimping Process

Considering the complexity of the phenomena that accompany cold forming processes, the FEM was used to model wire deformation. The finite element mesh of the FEM model is presented in Fig. 5.

In order to map different material properties, two groups of finite elements were identified in the model, which defined the jaw structure (EG1) and wire structure (EG2), respectively. Both groups were discretized with eight-node three-dimensional (3D)-solid finite elements [15]. Between the nodes of both groups of finite elements that define the outer surfaces of modeled objects, the conditions of surface contact were defined taking into account penetration and friction [15,16] with the value of the friction coefficient *μ* = 0.1. In order to reduce the size of the numerical task and reduce the calculation time, symmetry conditions were used. Half of the modeled structures’ volume was discretized with a mesh of both finite elements’ groups. Nodes contained in the model's symmetry plane (*YZ* plane) were deprived of the translations in the *x*-axis direction. In order to identify the technological parameters of the crimping process, N1 and N2 nodes were given stepwise values of *T* displacements simulating the reciprocating movement of the press head. N1 node displacements were associated with constraints [15] with nodes describing the upper surface of the working part of the jaws. In the same way, displacements of the N2 node were associated with the nodes describing the lower surface of the working part of the jaw.

In order to correctly select the material model, a static tensile test of smooth wire and a standard sample made of jaw material were carried out. Based on the obtained *σ*–*ɛ* plot, the modulus of longitudinal elasticity *E*, Poisson's ratio *ν*, strain hardening modulus *E _{1}*, yield strength

*σ*

_{p}_{l}, and tensile strength

*σ*were determined. These data are summarized in Table 2.

_{m}Materiał/parameter | E (MPa) | E_{1} (MPa) | ν | σ (MPa)_{pl} | σ (MPa)_{m} |
---|---|---|---|---|---|

316L | 200,000 | 1995 | 0.3 | 760 | 989 |

42CrMo4 | 200,000 | 20,000 | 0.3 | 1500 | 2050 |

Materiał/parameter | E (MPa) | E_{1} (MPa) | ν | σ (MPa)_{pl} | σ (MPa)_{m} |
---|---|---|---|---|---|

316L | 200,000 | 1995 | 0.3 | 760 | 989 |

42CrMo4 | 200,000 | 20,000 | 0.3 | 1500 | 2050 |

The wire outline is made during the drawing process. According to the guidelines contained in Ref. [17], the primary parameter identifying the homogeneity of the wire structure in the cross section is the distribution of microhardness. Optimally selected angles of the die cones can ensure a satisfactory homogeneity of the material [17]. The paper [18] presents the distribution of microhardness in the cross-sectional area of a steel wire with a diameter of 5.5 mm. The research shows that steel wires with diameters in the presented range achieve a homogeneous microhardness distribution. Based on the aforementioned parameters, it was assumed that the modeled wire (EG2) structure is homogeneous. Thus, in the second group of finite elements of the model (EG2), no zones with separate material properties were distinguished (unlike the FEM bearing model presented in the publication [19]).

For both groups of finite elements, an elastic–plastic material model was defined; the graph of which is presented in Fig. 6. The group EG1 assumed the isotropic nature of material hardening [16]. In the EG2 group, however, the modeled hardening was of a kinematic type [15]. A similar model of material strengthening resulting from the consideration of contact issues in modeling residual stresses was presented in the publication [20].

The process simulation was carried out in three steps. In the first step, the sign of the given displacement *T* of the nodes with the N1 node was negative, and the sign of displacement of the nodes with the N2 node was positive. After obtaining permanent deformation of the EG2 group elements, the signs of the given displacements changed (second step). The third step was related to the task of loading the resultant force *F* distributed into nodes describing the frontal surfaces of the wire.

Static linear equilibrium equations for the model's finite elements, taking into account the constitutive laws, implemented in the matrix form in the ADINA [15] system, were solved using a sparse matrix solver. This solver is based on the Gaussian elimination method. Nonlinear equations resulting from the necessity to solve the contact problem between the nodes of groups EG1 and EG2 were solved iteratively based on the Full Newton method. The defined tolerance value determined the convergence of solutions between successive steps (iterations) of calculations for the strain energy and the contact force tolerance. The deformation energy tolerance was ETOL = 0.001 (ETOL – energy convergence tolerance [15]) and the contact force tolerance RCTOL = 0.05 (RCTOL – contact force convergence tolerance [15]). It means that the strain energy quotient between the two consecutive steps must be lower than the ETOL value. The same is true for the quotient of contact forces [15,16].

Since the work's primary goal is to assess the wire's strength properties under the conditions of shaping and application, a finite element mesh's sensitivity was tested before carrying out the strength analysis in the FEM model. The influence of mesh density on the calculations of equivalent tensile stress located in the longitudinal section of the crimped wire was considered. The description of the mesh size selection criterion and the metric data of the FEM model is presented in the Appendix. The calculation results presented in the paper were obtained using the model with the maximum mesh density ( Appendix).

## Verification of the Finite Element Method Model of the Wire Crimping Process—Stress Analysis

As part of the numerical tests, four simulations were carried out in which the values of the maximum displacement *T*_{max} were changed successively (Fig. 5). These values in subsequent simulations were respectively 0.6, 0.8, 1.0, and 1.2 mm. On the other hand, the tensile force *F*'s value was applied iteratively until the equivalent tensile stress in the crimped wire was equal to the tensile strength *σ _{m}*. Based on the determined values of deformation of the wire structure, it was found that achieving the desired embossing (

*h*= 3.6 mm) can be achieved with a given jaw displacement

*T*

_{max}= 1 mm. For this value, a section of crimped wire was made, and the model validation started.

To this end, contact measurements (Fig. 7(a)) of the characteristic dimensions of corrugated wire, according to Fig. 4(a), were made using the ROMER measuring arm head (HEXAGON company). These parameters were also identified based on the distance of the respective nodes in the FEM model covered by the group finite elements EG2 (Fig. 5).

A visualization of the position of these nodes assigned to permanent deformations in the dimension range equal to one pitch *P* is shown in Fig. 7(c). However, the orthogonal form of wire deformation resulting from crimping is shown in Fig. 7(b). The values of the corrugated wire geometrical parameters measured and determined based on the FEM model are summarized in Table 3. Due to the discretization errors of geometric structures, the distance values between the characteristic nodes were averaged.

Dimension according to Fig. 4(a) | d (mm)_{s} | P (mm) | h (mm) |
---|---|---|---|

Measurement | 1.860 | 11.040 | 3.600 |

FEM model | (1.867 + 1.870)/2 = 1.869 | (10.985 + 11.171)/2 = 11.078 | (3.606 + 3.605)/2 = 3.606 |

Dimension according to Fig. 4(a) | d (mm)_{s} | P (mm) | h (mm) |
---|---|---|---|

Measurement | 1.860 | 11.040 | 3.600 |

FEM model | (1.867 + 1.870)/2 = 1.869 | (10.985 + 11.171)/2 = 11.078 | (3.606 + 3.605)/2 = 3.606 |

In the next stage of model validation, the crimped wire sample was subjected to a static tensile test. Then, measurements of the same geometrical parameters of the crimped wire were made under the ultimate tensile force conditions. These results were compared with the results of the third step of the simulation for the given limit force *F _{m}*

_{max}. The values measured and calculated based on the FEM simulation results are summarized in Table 4.

Dimension, according to Fig. 4(a) | d (mm)_{s} | P (mm) | h (mm) |
---|---|---|---|

Measurement | 1.760 | 12.230 | 2.600 |

FEM model | (1.793 + 1.789)/2 = 1.791 | (12.219 + 12.227)/2 = 12.223 | (2.577 + 2.574)/2 = 2.576 |

Dimension, according to Fig. 4(a) | d (mm)_{s} | P (mm) | h (mm) |
---|---|---|---|

Measurement | 1.760 | 12.230 | 2.600 |

FEM model | (1.793 + 1.789)/2 = 1.791 | (12.219 + 12.227)/2 = 12.223 | (2.577 + 2.574)/2 = 2.576 |

As a result of the tested crimped wire's tensile test, the maximum tensile force *F*_{max} = 2970 N was obtained. However, based on the FEM simulation, this value was set at the level of *F _{m}*

_{max}= 2947 N. Taking into account the satisfactory compliance of the parameters obtained by simulation with the actual parameters, the following relationships were developed.

Table 5 summarizes the essential results of the diameter *d _{s}* calculations and the embossing

*h*obtained for the maximum jaw displacement

*T*

_{max}values.

T_{max} (mm) | d (mm)_{s} | P (mm) | h (mm) |
---|---|---|---|

0.6 | (1.881 + 1.888)/2 = 1.885 | (11.001 + 11.000)/2 = 11.001 | (2.901 + 2.903)/2 = 2.902 |

0.8 | (1.872 + 1.878)/2 = 1.875 | (10.997 + 10.995)/2 = 10.996 | (3.271 + 3.274)/2 = 3.273 |

1.0 | (1.867 + 1.870)/2 = 1.869 | (10.985 + 10.988)/2 = 10.987 | (3.606 + 3.605)/2 = 3.606 |

1.2 | (1.864 + 1.869)/2 = 1.867 | (10.979 + 10.975)/2 = 10.977 | (4.053 + 4.046)/2 = 4.050 |

T_{max} (mm) | d (mm)_{s} | P (mm) | h (mm) |
---|---|---|---|

0.6 | (1.881 + 1.888)/2 = 1.885 | (11.001 + 11.000)/2 = 11.001 | (2.901 + 2.903)/2 = 2.902 |

0.8 | (1.872 + 1.878)/2 = 1.875 | (10.997 + 10.995)/2 = 10.996 | (3.271 + 3.274)/2 = 3.273 |

1.0 | (1.867 + 1.870)/2 = 1.869 | (10.985 + 10.988)/2 = 10.987 | (3.606 + 3.605)/2 = 3.606 |

1.2 | (1.864 + 1.869)/2 = 1.867 | (10.979 + 10.975)/2 = 10.977 | (4.053 + 4.046)/2 = 4.050 |

In the conducted analysis, it can be stated that the dimensions *d _{s}* and

*h*depend on the set value of the maximum jaw displacement

*T*

_{max}. The technological parameter

*T*

_{max}is associated with the value of the maximum force

*F*

_{T}_{max}that must be used to make a single bend of wire (force permanent wire deformations). The

*F*

_{T}_{max}force was determined based on the N1 node reaction (Fig. 5) at the set maximum displacement

*T*

_{max}(measured from the beginning of the contact zone of groups EG1 and EG2). The value of the maximum displacement of the jaws

*T*

_{max}also affects the value of the force

*F*

_{m}_{max}, breaking the crimped wire. The set values of

*T*

_{max}in the third step of the simulation were determined based on the stress distribution obtained, the

*F*

_{m}_{max}force values. Both dependencies, together with approximation formulas, are placed on the graph (Fig. 8).

Due to the satisfactory compatibility of dimensions and form between the developed model and the manufactured element, the analysis of stress distribution caused during the technological process of wire crimping was started. Figure 9 shows the distribution of equivalent tensile stress *σ*_{o} that arose during wire shaping using the maximum force *F _{T}*

_{max}in the displacement range

*T*

_{max}= 1 mm. Visible bands of equivalent tensile stress exceeding the yield strength

*σ*

_{p}_{l}= 760 MPa identify the places of the most significant effort of the material. The presented image confirms that despite the occurrence of the crumple zone, the tensile strength

*σ*= 989 MPa, and thus, the loss of material continuity has not been exceeded.

_{m}On the other hand, Fig. 10 presents the distribution of internal stresses generated after the crimping process. Visible elastic recovery due to the phenomenon of material hardening ensures that the load limit is maintained at a level similar to the load destroying the smooth wire (in the considered case, it is the value of the force *F* = 3105 N).

The distribution of stresses in the limit state under tension is shown in Fig. 11. Visible stress propagation zones with values exceeding the value of *σ _{m}* indicate the mechanism of material delamination.

This phenomenon was also noticed during a static test of stretching a fragment of the facade mesh (Fig. 12). As a result of a significant difference in stress in specific plasticizing areas, the phenomenon of material flow and loss of structure continuity occurs. This fact confirms the advisability of using a material model with kinematic strengthening.

## Conclusion

The developed FEM model of wire crimping satisfies the assumed goals and can be used in the selection of technological parameters for the crimping of facade wires. The use of elastic–plastic material models with material hardening enabled a satisfactory representation of the form of wire deformation in the crimping process. Using the presented model, it is also possible to analyze the tool's geometry and strength (jaws). Based on the distribution of equivalent tensile stress arising in the process of wire crimping, it was found that the used pitch *P* was correctly selected in terms of structural strength. Consequently, there is no continuity of the state of permanent plasticization along with the wire structure, especially in terms of internal stress. Adopting a smaller pitch could lead to the concentration of permanent stress and, consequently, to a violation of the structure continuity at the crimping stage. It should be noted that no strength analyzes were carried out in order to select the pitch, and the adopted value resulted only from the aesthetical values of the crossing of the horizontal wires with the vertical wires of the facade mesh. The difference between the values of the measured geometrical parameters of the wire and the values obtained from the simulation (Tables 3 and 4) may be an imperfection of mapping the smooth wire structure in the FEM model.

It has been shown that as the wire shaping forces increase, its tensile strength slightly decreases. In this case, this phenomenon was described by a parabolic function. In the experimentally tested case, it was found that the tensile strength of the wire after crimping decreased by about 5%. The values of equivalent tensile stress preserved in the material due to notching constitute a maximum of 80% of the yield point. As mentioned in the Introduction, the facade mesh is pre-tensioned by a system of parallel arranged springs. In the analyzed object, the mesh's tension force for a single vertical crimped wire, taking into account the weight, is 260 N. This value is a small percentage of the crimped wire's strength. Nevertheless, in combination with other loads related to, e.g., wind aerodynamics, ice retention should be taken into account when designing the facade's supporting structure.

The presented model can also be used to simulate external loads acting on the mesh in different directions. Fatigue analysis, including aerodynamic effects, will be subject to further research.

Similarly, further research will focus on the durability of the tool shaping the contour of the crimped wire, taking into account the research results presented in Ref. [21]. The mesh segments will also be stress-tested under the triaxial load condition.

## Acknowledgment

The work was realized in cooperation with the DAWID Ltd.—producer of facade gratings (address: ul. Gronowa 23, 42-271 Częstochowa, Poland, e-mail: dawid@dawid.pl, www.dawid.pl)

## Conflict of Interest

There are no conflicts of interest.

## Data Availability Statement

The data sets generated and supporting the findings of this article are obtainable from the corresponding author upon reasonable request. The authors attest that all data for this study are included in the paper.

### Appendix

In order to reduce the discretization errors of the geometric structure with finite elements of the tool (EG1) and wire (EG2) and to ensure a satisfactory validation of the developed FEM model, test calculations were carried out for three variants of mesh density (minimum, average, and maximum). The geometric structure of a smooth wire sample with a length of 50 mm and the jaws’ geometric structure was divided into eight-node finite elements while defining the maximum distance between nodes in the same finite element. The metric data for the tested mesh density variants are summarized in Table 6.

A model with the minimum density of the finite element mesh of the model | A model with the average density of the finite element mesh of the model | A model with the maximum density of the finite element mesh of the model | |
---|---|---|---|

The maximum distance between nodes in a finite element of group EG1 (mm) | 0.65 | 0.36 | 0.27 |

The maximum distance between nodes in a finite element of group EG2 (mm) | 0.71 | 0.34 | 0.27 |

The number of finite elements in group EG1 | 810 | 3280 | 6090 |

The number of finite elements in group EG2 | 1600 | 9600 | 20000 |

Number of model contact equations | 1530 | 3510 | 5445 |

Number of general (remaining) equations of the model | 10072 | 47110 | 92221 |

A model with the minimum density of the finite element mesh of the model | A model with the average density of the finite element mesh of the model | A model with the maximum density of the finite element mesh of the model | |
---|---|---|---|

The maximum distance between nodes in a finite element of group EG1 (mm) | 0.65 | 0.36 | 0.27 |

The maximum distance between nodes in a finite element of group EG2 (mm) | 0.71 | 0.34 | 0.27 |

The number of finite elements in group EG1 | 810 | 3280 | 6090 |

The number of finite elements in group EG2 | 1600 | 9600 | 20000 |

Number of model contact equations | 1530 | 3510 | 5445 |

Number of general (remaining) equations of the model | 10072 | 47110 | 92221 |

The calculations of reduced stresses for the tested models under the conditions of the given maximum displacement *T*_{max} = 1 mm are presented in Fig. 13. Based on the results, it can be concluded that in the case of models with minimum and average mesh density, the tensile strength limit would be exceeded in the process of crimping the wire in zone A (Fig. 13). It could prove that the outer structure of the wire would delaminate during shaping. This phenomenon was not noticed during production. Thus, it was found that the model with the maximum density of the finite element mesh should be used to model the wire crimping process and strength tests.