Parametric modelling of control cable fittings geometric configuration with interpolation of FEA results

. Studying the behavior of control cable fittings (actually a pipe-type part) during radial crimping for fixation on the pipeline is a difficult task since it is necessary to control the presence of obvious plastic deformations: on the one hand, insufficient crimping can cause the fitting to break off from the cable conduit (axial loads over 100 kgf), and on other – the excessive crimping can block the operation of the cable (the core will jam). The selection of the optimal ratio of the fitting diameter and its wall thickness at different load values is the topic of a multi-parameter problem, and one of the ways of solving it will be presented in our research. To evaluate the nonlinear behavior of the Structural Steel NL Ansys material will be used Bilinear Isotropic Hardening stress-strain model with further interpolation of the Tangent Angle Coefficient (TAC) which is suggested as a new calculation parameter of pipe stress estimation.


Introduction
The steel fittings (caps, claps or hubs) are a typical part of many components and assemblies in the automotive industry and are used, for example, in push-pull remote-control cables that serve to transfer loads from the control body to the controlled one.The practical problem of the task is that being radially crimped, the fittings (detail in the form of pipe) must have a certain permissible range of stresses/strain in the area of the axial hole and on its outer cylinder surface to be rigid enough and avoid the transfer of unacceptable deformations inside of the cable.The strength analysis is simple at first glance, but in reality, it turns out to be filled with several possible problems and challenges so the fitting must: • press the conduit (red polymer in Fig. 1a) with sufficient force so as not to slip off it (normative tensile load not be less than 100 kgf for the cable); • should not cause internal conduit deformation that can limit the free movement of the core (the main transmission element in the remote-control cable).Otherwise, the cable has an increased risk of jamming, which is dangerous for the operation of the vehicle.

Literature review
The problem of calculating the plastic deformation of control cable fittings is related to the conditions of the cables exploitation and appropriate boundary conditions, thus the article [1] is recommended to get acquainted with possible push-pull cable-based actuation cases through experimental results and detailed analysis.The paper [2] introduces a novel pushpull cable-driven technology within the CORBYS rehabilitation system, enabling the creation of high-power-to-weight-ratio assistive devices.In [3], the authors describe the use of cables in UAVs, which is quite valuable for formulating specific boundary conditions for cable loading.Cable loading (as long as fittings are a part of the assembly) can overcome not just static loads but vibrations as well -vibration control of flexible manipulators by active cable tension is a topic of [4].Quite an actual topic that is close to our scope of research was raised in [5] -fastening characteristics of preformed helical fittings considering the surface effect of transmission lines.As long as the fittings provoke pressure on the conduit, it makes sense to investigate its structure and behavior: the paper [6] -full 3D finite element modeling of spiral strand cables and papers [7,8] -effect of interwire contact on the mechanical performance of wire rope strand (the part of cable conduit and core).Taking into account that cable fittings have a form of pipe [9], it's recommended to investigate the hoop stress nature [10].Bilinear Isotropic Hardening as a part of applied Ansys material characteristics is mentioned in [11].

Research results
The purpose of our research is to model the optimal configuration of the fitting (Fig. 1а) according to the criteria: outer diameter, inner diameter and plasticity of the material depending on the crimping load.An example of the radially crimped by 8 press elements fitting blank -a rod with a diameter of 20 mm without a hole is shown in Fig. 1b.It can serve as a valuable basis for forming an individual stress-strain characteristic that is quite important for the laboratories of the same push-pull cable manufacturers.Hoop stress, also known as circumferential stress, is the stress that develops in a cylindrical or spherical structure like a tube or pipe when radial loads are applied normally (perpendicular) to the outer surface of the structure.This type of stress is primarily due to the confinement of the material and results from the stretching or compression of the material in the circumferential direction.Let's calculate the Hoop stress for the thick-walled pipe using the next formula: where:   -Hoop Stress, MPa; applied radial pressure, MPa; inner radius, m; outer radius, m; radial position where stress is to be found, m; To calculate the   value, it's necessary to find the pressure  magnitude: considering we have 8 crimping press elements (Titanium Alloy in Ansys) with each element contact area of 5x20 mm and applied normally load of 40 kN (Fig. 1b), we will get  = 400 MPa.Other parameters are:  = 9 mm, which means that we seek to determine the stress on the already deformed surface of the pipe under the pressure of these crimping press elements.The fact is that the outer radius of the pipe in the places of crimping is subjected to plastic deformation and is reduced by the amount of penetration of the mentioned press elements (by approximately 1 mm), so the outer radius is reduced from 10 mm to 9 mm approximately.Thus the Hoop stress value according to equation ( 1) is   = 297.9MPa, that is higher than the Yield stress of Structural Steel NL used in Ansys modelling (250 MPa) and goes beyond the Hook's law.In this a case, it is necessary to take into account the plastic deformation of the pipe in order to establish the total stress: where: where:  the tangent modulus that represents the rate at which the stress-strain curve changes at each stress point, Pa;  deformation, m/m.In the context of the Ramberg-Osgood equation ( 4), it's the reciprocal of the first derivative with respect to strain: where:  the yield strength, usually the 0.2% proof stress, MPa; the elastic modulus, Pa; the strain hardening exponent (or Ramberg-Osgood parameter).
In the context of an idealized elastic-plastic material model, the tangent modulus is employed to characterize the gradient of the stress-strain curve once the material has surpassed its yield point.If the stress-strain graph is a non-linear curve that obeys a simple mathematical law (parabolic or logarithmic etc), then, the tangent modulus is calculated by taking the derivative (/) of the stress-strain curve at the specific point of interest beyond the yield point.The Bilinear Isotropic Hardening (Fig. 2a) consists of 2 linear regions, so it simplifies our further research.
Based on the   = 1,45•10 9 Pa applied in the Ansys graph (Fig. 2a) with the next intermediate points of the linear plastic hardening region (strain-stress dependence):  1 = 0.00125 mm/mm that matches  1 = 250 MPa and  2 = 0.0045 mm/mm that matches  2 = 255 MPa, we find the strain value   = 0.0324 that matches to   = 297.94MPa using interpolation according to (5): Thus, returning to (3), we can calculate the value   = 46.98MPa.Finally,   = 297.9+ 46.98 = 344.92MPa that should be compared with the Ansys FEA results (Fig. 3a) for the same boundary conditions (Fig. 2b): Average Stress value at the end of the experiment (t = 1 s) is 344.52 MPa (Fig. 3b), which is less than 1% error.
As part of our analytical FEA analysis, 3 types of fittings of the same outer diameter (20 mm) with the following wall thickness (  , mm) were additionally modeled (Table 1): 10 mm (rod), 4 mm (pipe) and 2.5 mm (pipe).Each model underwent 5 types of loads from F = 40 kN to 120 kN, resulting in the following Average Stress values.Besides we have suggested an original parameter TAC and TAC/  that will be described below.1, it can be seen that they have a close to linear character as the loads on the fitting increase (Fig. 4a).This is explained by the linear nature of the graph beyond the Yield point (Fig. 2a).A visual view of the stress-strain state of the models under characteristic selected loads is presented in Fig. 5.In the meantime, we can move on to a new stage -introduce the following evaluation indicator -TAC (Tangent Angle Coefficient):  = (  −   )/(  −   ), (6) where:   ,  maximum and minimum stress during the research (like 450.52 and 192.09MPa according to FEA);   ,  max and min force load (like 120 and 40 kN).The final results of  are presented on the graph (Fig. 4b)very interesting from a scientific point of view is its linear nature: the dependence of  on the thickness of the pipe wall (  ) is linear and this opens up wide prospects for modeling the required configurations of pipes without another FEA recalculation.Let's test our hypothesis of the linearity of the  indicator: Table 1 presents the actual values of the average stresses for all analyzed pipes, except for the fitting with a wall thickness of 5 mm (corresponding to a hole diameter of 10 mm). for this pipe with previously measured Average Stress in Ansys (  = 851.36MPa and   = 315.56MPa) according to ( 6) is:  The error is less than 1% between (7) and ( 8).An alternative test criterion for our theory сonfirmation is a calculation of  to   ratio and here we get quite an exciting results situation: 1.615, 1.694 and 1.709 for the   = 10, 4 and 2.5 mm accordingly.The closest of values forces us to judge the effectiveness of the proposed method of stress prediction in the case of Bilinear Isotropic Hardening stress-strain graph of material.An additional confirmation of the results convergence of the experiment with the calculation is the measurement of the deformations depth of the rodthe real depths measured with a caliper are 0.9-1.0mm (Fig. 1b), and the ones obtained as a result of FEA -0.96 mm (Fig. 6a).At the same time, the maximum values are recorded in the center of the rod and are 2.12 mm -the body bulges under pressure (tag "max" at Fig. 7a).The established trend of increasing deformations closer to the longitudinal axis is also observed in the analysis of pipe: under an external load of 120 kN of the fitting with the wall thickness tw = 4 mm has demonstrated the maximum deformations -6.33 mm that is observed along the axis (Fig. 6c).Being less thick (tw = 2.5 mm), the fitting, despite a significantly lower load (80 kN), gained even higher deformations -7.0 mm.This well demonstrates the influence of the wall thickness on the ability of the fitting to absorb the load and allows us to pre-calculate the magnitude of the load for crimping the fitting to obtain the required residual diameter of the inner hole.Recall that the last parameter determines the movement freedom of the core inside the conduit of the control cable on the one hand, and the strength of holding the fitting on the same conduit itself -on the other.A competent balance of these two indicators determines the final resource of the remote-control cable.

Conclusions
1.The task of finding the optimal crimping load of the fitting turns out to be quite difficult in the real conditions of the production of remote-control cables: excessive crimping can lead to the destruction of the cable conduit shell or even jamming of the travalling core due to an unacceptable reduction in the inner diameter of the fitting.On the other hand, not pressing the fitting leads to non-fulfillment of the condition of axial strength -the cable must withstand at least 100 kgf. 2. We performed FEA in Ansys with 4 types of fittings of the same outer diameter (20 mm) and different inner diameters (from 0 to 15 mm) in 5 load modes (from 40 to 120 kN).It can be clearly stated that below 40 kN the crimping is insufficient, and above 80 kN causes an unacceptable reduction in the diameter of the fitting hole.3.One of the key criteria for the formation of fitting plastic deformations is the zone beyond the Yield point of the stress-strain curve with the tangent modulus (in the case of Bilinear Isotropic Hardening used for Structural Steel NL in Ansys its magnitude is 1450 MPa).
The specified linearity allows obtaining almost linear stress-load graphs, which prompted the authors to create their own TAC evaluation criterion, which is perfectly amenable to interpolation for predicting results without FEA each time.Thus, for a pipe with an internal diameter of 10 mm, the error of the TAC value was less than 1% when comparing the FEA values and the analytical calculation.

Fig. 2 .
Fig. 2. Formulation of boundary conditions in Ansys: a) "Bilinear Isotropic Hardening" of Structural Steel NL stress-strain curve; b) application of fixed support and external loads.
let's compare the measured  (7) with the calculated one based on the interpolation method: