Design Parameter Identification and Verification for Thermoplastic Inserts

(1)

Linköping University | Department of Management and Engineering Master’s thesis, 30 credits| Master’s Programme Autumn 2020| LIU-IEI-TEK-A--20/03904—SE

Design Parameter

Identification and

Verification for

Thermoplastic Inserts

Malhar Shrikrishna Ozarkar

Supervisor: Lars Johansson Examiner: Jonas Stålhand

Linköping University SE-581 83 Linköping, Sweden +46 013 28 10 00, www.liu.se

(2)

ii

Abstract

Inserts are a crucial part of household and industrial furniture. These small plastic parts which often go unnoticed to the naked eye perform crucial functions like providing a base for the furniture, leveling the furniture, safeguarding the user from edges of the tubes used and providing an aesthetic finish. The inserts have a wing like structure on the exterior which enables them to be inserted and securely held in the tubes. The inserts are assembled into the pipes manually or through machines. The force required to install these inserts in the tube is called a push-in force whereas a pull-out force is the force required for removal of the is called a pull-out force. These forces are experienced by someone who assembles the furniture together. Thus, these forces directly define the ease with which the furniture can be assembled. In the first part of the present thesis, these push-in and pull-out forces are predicted using finite element simulations. These finite element simulations were validated by performing physical assembly and disassembly experiments on these inserts. It was found that the finite element simulations of the insert are useful tool in predicting the push-in forces with a high accuracy.

These push-in and pull-out forces for a single insert vary by 2-5 times when the dimensional variations in the tube are considered. The dimensional variations can be a result of the manufacturing processes from which these tubes are produced. The maximum and minimum dimensions that the tube can have are defined by the maximum material condition (MMC) and the least material condition (LMC). To reduce the variation in push-in and pull out forces, a stricter tolerance control can be applied to the manufacturing process. To avoid this cost while having a lower variation in the push-in and pull out forces, the design of the insert was modified. To achieve this enhanced design of the insert, a metamodel based optimization technique was used in the second part of the thesis. For this optimization, the geometrical parameters - wing height, wing diameter and stem thickness the of the insert were identified as the crucial factors which govern the assembly/disassembly forces. The identification of these parameters was done through a design of experiments. These parameters were then varied simultaneously in a metamodel based optimization which had an objective to minimize the variation in forces observed for an insert when the maximum material condition and the least material conditions are considered. The result for the enhanced design of the insert was then stated in terms of the ratio of these identified parameters. The modified design of the insert not only enables the manufacturer to have better performance, but also reduces the amount of plastic material required for manufacturing of the insert.

Keywords: Contact modelling, experimental validation, thermoplastic material, metamodel based design optimization.

(3)

(4)

iv

Acknowledgement

Firstly, I would like to sincerely thank Gustav Holstein at Ikea Components AB who has been a motivation and was extremely supportive throughout the duration of the project. His guidance and mentorship in the project have been crucial in achieving the results for the thesis. I would like to thank him for being directly involved in major discussions decisions regarding the project and giving me the opportunity to apply my learnings to the simulations done in the industry.

In addition, I would like to thank Björn Stoltz for leading many fruitful and interesting discussions regarding the project. His inputs and experience regarding contact simulations and material behaviour were valuable and crucial while carrying out the experimentation. I would also like to express sincere gratitude to Jenny Gurell and Marko Kokkonen at Ikea Test Lab for their insights and support in the experimentation phase. I would also like to thank Carolina Kroon and Carina Skov Pedersen for their prompt arrangement of the resources required for the project. I would also like to extend my gratitude towards the entire design team for the valuable knowledge on the design and the materials of the insert.

I would also like to thank my supervisor, Lars Johansson and my examiner, Jonas Stålhand at Linköping University for their advice and guidance. Their constructive feedback on the theoretical framework have been valuable contributions to the project. I would also like to thank my opponent Puneeth Ballakkuraya for his thorough opposition and valuable insights on the project.

Last but not the least, I would like to thank my family and friends for their continuous motivation during the project.

(5)

List of Figures

Figure 1: Examples of applications of inserts in household furniture ... 1

Figure 2: Parameters needed to be investigated for their effect on the push-in and pull-out Forces ... 3

Figure 3: Flowchart of the methodology used for the thesis ... 4

Figure 4: Conventional design optimization process ... 8

Figure 5: Illustration of contact detection zone ... 9

Figure 6: Simplified illustration of a contact detection algorithm ... 10

Figure 7: Simplified version of a penalty-based contact ... 12

Figure 8: Geometries of the inserts used for verifying push-in and pull-out forces ... 17

Figure 9: Classification of models based on mesh properties (* indicates applicable to Insert-1 only) ... 18

Figure 10: Overview of boundary conditions used in the simulations ... 19

Figure 11: Example of displacement applied to the pipe in the simulations ... 20

Figure 12: Example of difference between stress-strain curves for dry and conditioned PA6 material... 21

Figure 13: Comparison in geometries of the designed and manufactured insert ... 22

Figure 14: Experimental setup for mapping the push-in forces ... 23

Figure 15: Example of set of curves obtained from the experiments for push-in force. ... 23

Figure 16: Experimental setup for mapping the pull-out forces ... 24

Figure 17: Example of set of curves obtained from the experiments for pull-out force ... 24

Figure 18: Comparison of simulated and experimental push-in forces for Insert-1 ... 25

Figure 21: Comparison of simulated and experimental pull-out forces for Insert-1 ... 27

Figure 24: Effect of coefficient of static friction on contact force ... 29

Figure 25: Effect of change in coefficient of kinetic friction on contact force ... 30

Figure 26: An example of weld-line present on the inner surface of the pipe ... 31

Figure 27: Effect of variation in pipe diameter on contact force ... 32

Figure 28: Example of a forces acting on a single wing of the insert ... 32

Figure 29: Dimensions of the insert used as design variables ... 33

Figure 30: Effect of variation in wing diameter (DVAR1) on contact force ... 35

Figure 31: Effect of variation in stem thickness (DVAR2) on contact force ... 36

Figure 32: Effect of variation in wing height (DVAR3) on contact force ... 36

Figure 33: Example of difference in forces for MMC and LMC for pipe ... 37

Figure 34: Flowchart of the approach used for optimization of the insert ... 38

Figure 35: Illustration of peaks and differences in peaks (Diff) for MMC and LMC conditions. ... .40

Figure 36: Comparison of forces observed in MMC and LMC conditions for baseline and optimized designs by difference method ... 41

(7)

vii

Figure 37: Comparison of cross-sections of original and optimized design by difference method

... 42

Figure 38: Comparison of cross-sections of original and optimized design by division method ... 43

Figure 39: Comparison of forces observed in MMC and LMC conditions for baseline and optimized designs by division method ... 44

List of Tables

Table 1: Summary of number of nodes and elements used in different types of models ... 18

Table 2: Tolerances specified by the manufacturer for different components ... 31

Table 3: Summary of Design Variables and their limits ... 34

(8)

1

1 Introduction

1.1 Background

Tube inserts have a wide range of application in furniture, especially as bottoms of legs for chairs as shown in Figure 1. During assembly of furniture components, these inserts are press-fitted in a hollow tube. The inserts are designed to be assembled using an interference-fit method and require a certain amount of force for their insertion and removal, depending upon the design and application of the insert. The forces during the assembly and disassembly of these products are crucial as they directly address the effectiveness of the design and their ability to be customer friendly. Traditionally, these inserts are physically tested to map the forces involved. The simulation of this assembly-disassembly process is necessary to reduce the costs incurred during repetitive physical testing of the components. This also enables the manufacturer to provide a better performance to the customers. Due to the wide range of designs of these inserts, it is desired to identify the effect of the design parameters on the forces.

Figure 1: Examples of applications of inserts in household furniture (Picture Courtesy: www.ikea.com)

The inserts commonly used in industry are usually manufactured by injection molding and are made up of thermoplastic materials namely Poly Amide 6 (or PA6, for short) or Polyethylene (PE, for short) or Acrylonitrile Butadiene Styrene (ABS, for short). The composition of the insert’s material depends on the application and the intended use of the insert. In cases where a stiffer insert is needed, fibers are added to the matrix of the above-mentioned materials. These fibers are made of glass, nylon, cotton, or other materials. By altering the amount of fibers added, the stiffness of the insert can be altered. In furniture applications, usually glass fibers are added which typically constitute up to 30% of the volume.

The pipes in which the inserts are inserted are usually made from sheet metal like steel and then bent and welded to form a hollow pipe. The surface properties of these pipes are often altered by applying a coating or by painting. This is for aesthetic purposes as well as to provide protection from corrosive environments.

(9)

2

1.2 Problem Description

During the assembly of furniture components, the inserts are assembled with the hollow pipes. This is done manually by the customer or by assembly technicians at the factory. The two parts – insert and the pipe – are designed using interference fit where the dimensions of the parts have some overlap between them. This is necessary to secure the insert inside the pipe while in use and in idle conditions. Due to the interference fit, these parts require a force to be applied for proper assembly. These forces for installation of the insert and for its removal are called push-in and pull-out forces respectively, and they vary for different designs of the insert and the application. The forces during the assembly and disassembly of these products are crucial as they directly determine the effectiveness of the design and its ability to be customer friendly.

Traditionally, the inserts are physically tested to map the forces involved. The design of the insert allows a small of amount of deviation in the dimensions. This deviation, also called the tolerance, affects the dimensions of the insert as well as the tube, which leads to variation in the push-in and pull-out forces. To avoid repetitive physical testing, finite element (FEM) simulations are explored. These simulations not only help reduce the costs incurred during testing, but they also help the designers of these inserts to achieve better performance by simulating the behavior of the insert under various loading conditions. As the parts consists of plastic materials, these simulations have a high degree of non-linearity in terms of deformation behavior and the contact conditions. Thus, to replicate the behavior of the insert during the assembly-disassembly, it is important that the contact between the insert and the tube is simulated correctly.

1.3 Contact Between the Insert and the Pipe

The interaction between the insert and the pipe during the assembly/disassembly operations results in a contact between the interacting surfaces. This contact or interaction of the parts results in a force which is required to be overcome for continuous sliding of the insert inside the pipe. The contact forces are made of normal pressure exerted by the insert and tangential components known as frictional components. As the material of the insert (plastic) is significantly softer than that of the pipe (steel), the contact results in deformation of the inserts and a change the area of the contact. Thus, to simulate the assembly/disassembly operation, it is important that these forces are determined accurately to replicate this process through finite element methods.

1.4 Project Objectives

The objectives of the present thesis are:

i. Verification of push-in and pull-out forces: Corelating the forces from the finite element simulations to the forces observed during physical experiments or testing. ii. Geometrical parameter identification and optimization: The effect of the geometrical

dimension (parameters) of the insert will be investigated and the design of the insert will be optimized to reduce the difference in recorded forces for the maximum material condition and least material conditions of the pipe.

Through these stages, the thesis will address the following questions:

• What parameters and contact properties of the FE-model are needed to obtain pull-out and push-in forces which agrees with the experimentally obtained values?

(10)

3

The parameters in this phase of simulation consist of different contact conditions, mesh densities and method of load applications. These factors are major influencers on results of the simulation. The conditions needed to replicate the physical experiments through the FE-model will be determined largely on these parameters. The contact properties as stated in the problem statement depend on the static and dynamic friction coefficients of the interacting materials. The thesis intends to find the correct parameters needed for such an optimization.

• Which geometrical parameters of the design of the insert have a profound effect the forces experienced during the installation and removal of the insert? What causes the variation of these forces and how can this variation be reduced?

Figure 2: Parameters to be investigated for their effect on the push-in and pull-out forces The geometry of the inserts varies on the type of application where it is used. The important features of the geometry of the insert in contact with the pipe are firstly, the wing tip diameter(∅𝐷_𝑤), the rib height (h) as shown in Figure 2 and secondly the assembly tolerance. These parameters alter the contact area of the insert with the pipe and in-turn the force required for assembly/dis-assembly. Also, the stem diameter (∅𝐷_𝑠) and the wing base diameter (∅𝐷_𝑏) which contribute to the wall thickness of the insert stem which provides the radial stiffness to the insert. Thus, it is crucial to examine the effect of these parameters on the push-in and pull-out forces to optimize the insert.

1.5 Environmental and Sustainability Considerations

As mentioned earlier, the thesis deals with finding out the correct way of simulating the actual tests carried out on the inserts and finding the correct geometrical dimensions in order to enhance the performance of the insert. Thus, no direct impact on the environment are expected. In turn, having an optimum design of the insert may result in a reduced rejection of these plastic parts as the performance is improved.

(11)

4

2 Methdology

To achieve the desired outcomes of the thesis, the work is divided into several phases. These phases are defined in such a way that through each of them, a desired outcome is stated and the outcomes from each phase are needed as in input for the subsequent phases. An overview of this approach is shown in Figure 3

Figure 3: Flowchart of the methodology used for the thesis

2.1 Literature Review

Due to the complex nature of the problem and due to company policies regarding privacy of research, the material available is limited. Nevertheless, the material available for similar problems in the different phases of this thesis will be reviewed to reach an understanding of theory and the approach behind the problem. This phase helps in laying a foundation for the thesis.

2.2 Model Building and Preliminary Simulations

This phase mainly consists of discretizing the geometry of the insert (meshing) to setup the constraints and boundary conditions required to simulate the load cases. For the simulation results to be accurate, the mesh of the insert needs to be sufficiently converged, i.e. further refinement of the mesh should not significantly affect the results. Also, during this phase, various forms of elements will be tested to observe their response to the contact conditions required for the problem. As the contact between the insert and the pipe is dependent on the mesh, a robust method that handles the variation in the number of elements and the element formulation is needed. This phase aims at finding a way to develop a robust model which meets these requirements. In these simulations, a perfect geometry was considered which did not consider the differences in dimensions due to tolerances. These conditions are simulated for preliminary results prior to physical experiments.

2.3 Experimentation

To map the forces that occur during the actual assembly/disassembly of the insert in the pipe, an experimental phase is included. The process of recording the forces will be done using a universal testing machine on which a force transducer is set up. From the experiments, a force-displacement curve will be obtained for each insert design. Moreover, to reduce the error in measurements and to obtain an average curve for each of the insert designs, a sample set consisting of multiple

(12)

5

samples of each design was tested. This phase provided real life force values which could be compared to the preliminary simulation results. In this phase, the deviation in dimensions from a perfect geometry are also measured. In case of a water absorbing material like PolyAmide-6, the samples were tested for dry and conditioned states of the inserts. Due to machine limitations, it was not possible to measure the coefficients of friction (static or dynamic).

2.4 Simulations to Obtain Push-In and Pull-Out Forces

After the experimental phase, some of the sources of errors that were observed during the testing, like the actual dimensions of the components and the rate of loading were included into the simulation models. As the friction properties of the interacting surfaces is not known, the exact contact conditions could not be simulated through the preliminary simulations and due to the limitations in measuring the actual friction coefficients, the coefficients were obtained from a literature review of similar interacting materials. Through these simulations, force vs displacement curves were obtained for different mesh densities and element types which were compared with the experimental curves

2.5 Geometrical Parameter Identification and Enhancement

In this phase, the geometrical parameters that affect the push-in and pull-out forces in the simulation and experimentation phase are identified. The effect of these identified parameters on the contact forces is then investigated. These geometrical parameters are later modified in such a way that for Maximum Material Conditions (MMC) and Least Material Conditions (LMC) of the tube, the difference in the assembly forcers observed is minimized. Thus, the outcome of this stage will be a modified design of the insert, the assembly forces for which have a reduced dependency on the tube dimensions.

(13)

6

3 Literature Review

This section discusses previous research carried out for similar problems as well as their limitations and the things that can be learned from previous research.

3.1 Finite Element Modelling

In the area of finite element modelling, there are several different elements which differ in their configuration and the mathematical model from which the stresses and strains are calculated. The elements can be divided into 1-D, 2-D and 3-D elements based on the number of dimensions the element has. As the insert geometries have solid sections, they are commonly modelled using hexahedrons and tetrahedrons. The elements can be further classified based on the order of the shape function they have as linear, quadratic, or cubic. Linear solid elements are comparatively simple elements and are often an extension of linear plane elements like a linear quadrilateral or linear triangular elements. Tetrahedron elements are commonly used for meshing of complex geometries like foam parts, cast components etc. In case of large bending, the linear tetrahedral elements have poor performance and often exhibit shear locking. In such cases, quadratic elements which have a higher degree of the shape function and can be used to simulate such problems with better accuracy (Cook et al. 2001).

However in cases where the geometry is modelled using smaller elements, the use of quadratic elements leads to increased computational costs as the number of nodes doubles and because of the computation of second derivatives of element in order to simulate their behavior (Jansen 1999). In case of modelling, contradictory research exists. Some research suggests that the use of hexahedral elements provides more accuracy compared to the use of tetrahedral elements if the order of elements used is the same (Bussler and Ramesh 1993), whereas some suggest that the use of bi-linear hexahedral elements provide similar results when compared to quadratic tetrahedral elements in terms of accuracy and cost (Cifuentes and Kalbag 1992). When small deformations are expected, the use of both linear hexahedral and linear tetrahedral elements are sufficient to capture the behavior (Benzley et al. 1995). In some insert designs, the cross section of the insert has cyclic symmetry. In such cases, the geometry can be modelled using axi-symmetric elements, which reduces the computational costs significantly (Hüyük et al. 2014).

Apart from their configurations, elements can be classified based on the numerical integration methods used to calculate the element stiffness matrix as fully integrated or under integrated elements. When fully integrated elements are used, the computation costs can be high (Livermore Software Technology Corporation 2006). In order to save computational costs, under-integrated elements are used. This also helps in reducing the volumetric locking which is observed in fully integrated elements. However, this reduced integration technique can induce zero-energy modes in the elements or ‘hour-glassing’ and to overcome this modes, hourglass control is needed (Schultz 1985).

Thus, from the above research, it could be concluded that in cases of large deformation, where the behavior of the element is relatively unknown, the type of element to be used along with the formulation and integration technique needs to be carefully reviewed in order to tailor it to the specific model requirements.

(14)

7

3.2 Contact Modelling

As the deformation of the insert and the force observed during its installation is dependent on its interaction with the pipe, the contact area for undeformed and deformed shape needs to be modelled correctly in FEM to obtain accurate results. The field of contact modelling has gained increased focus over the last few years as more and more industries demand robust contact algorithms which are stable and capable of handling material and geometrical non-linearity (Rodriguez-Tembleque and Aliabadi 2018). Contact friction models based on adhesion theory of friction have been developed and are supported by the experimental measurement of static and dynamic friction coefficients (Manninen et al. 2007). In FEM, there are two major types of contact algorithms - constraint-based contact and penalty-based contact. In constraint-based contact, a kinematic set of constraints is created between the two interacting surfaces and these constraints are checked at every time step in the simulation. If the constraints are being violated, a reaction force is applied at the nodes to the elements to satisfy the constraint requirement. The more widely used method, the penalty method, allows for minute penetrations observed in the contacting elements. This makes the penalty method economical and useful for solving problems pertaining to contact friction (Stefancu et al. 2011). The main difficulties in modelling a penalty based contacts are that parameter tuning is required and it does not treat simultaneous contact well (Rengifo 2009). If a large penetration is observed, the contact area will be altered and will also have an effect on the contact forces observed (Bay and Wanheim 1976). Moreover, due to the way the penalty method works, there will always be small penetrations between the pipe and the insert which will minutely alter the real dimensions of the tube and the contact area between them. Thus, it is necessary to limit the penetrations in the simulation.

In finite element methods the implementation of the contact algorithms can be classified be broadly classified into two stages:

i. Contact detection: Here the finite element program establishes if the interacting surfaces are considered as ‘in contact’ or ‘not in contact’

ii. Contact treatment: Here, if the interacting surfaces are in contact, a method or algorithm is specified by the program which defines how the contacting surfaces will be handled in the simulation.

The area of contact mechanics will be discussed in detail in Section 4

3.3 Optimization

A traditional approach for optimizing a design shown in Figure 4. The design of a component is modified based on the results of the simulation by the designers and the new designs are simulated again to learn more about their behaviour. This iterative process incurs recurring costs to the manufacturer. However, this process can be reduced by carrying out continuous simulation through optimization techniques. In recent times, due to advancements in computational capacities, the finite element simulations are coupled with mathematical optimization algorithms. Through these optimization algorithms, it is possible to tailor the design of the insert to the required response. In such optimization calculations, one or more sets of design parameters are varied to either minimize or maximize an objective function. The objective function is most often expressed in terms of a response which is obtained from the finite element simulations. When several parameters in the design are varied, it is essential to identify the effect of each parameter varied and

(15)

8

then achieve optimal design for given conditions. To explore multiple design parameters simultaneously, a parameter optimization is used. One technique for such multi-parameter optimization is called a metamodel based design optimization (MBDO). This technique allows numerical optimization to be applied even to compute complex problems and thus reduce the computationally intensive conventional process of design re-iteration (Wang and Shan 2007). The metamodels or surrogate models are created using the response obtained from a robust simulation and input datasets for the varied parameters. The process of placing the design points in space is called design of experiments. The surrogate models created compute the response for variation in datasets (Ryberg et al. 2012). A detailed description of the working of such an optimization is given in Section 5.

(16)

9

4 Contact Mechanics

This section describes the typical implementation of contact mechanics in a finite element program. The section is divided into two sub-sections - Contact Detection and Contact Treatment. Under the treatment of contacts, the various methods that are used in handling contact phenomena are described along with different discretization techniques for the contact.

4.1 Contact Detection

To understand how contacts are treated in a finite element code, it is essential to understand the conditions that define a contact phenomenon. These conditions are needed to invoke the part of the program which specifies the treatment of the contact. Consider two arbitrary bodies Ω1 and Ω2

in space as shown in Figure 5. The position of the bodies in space is known from their co-ordinates with respect to a global co-ordinate system. This position of the body in a simulation is generally defined using a design tool. In continuum mechanics, it is assumed that two distinct points cannot occupy the same position in space simultaneously (Gonzalez and Stuart 2008). In case of distinct bodies in space, no bodies can penetrate each other (Heinstein et al. 1993). If there are two or more elements from two different bodies are intersecting each other at the start of a finite element simulation, an initial penetration is said to occur. In such conditions, the contact algorithm may not work.

Figure 5: Illustration of contact detection zone

The bodies Ω1 and Ω2 obtained from a design software (CAD) are discretized using a pre-processor

into elements which are connected by nodes. To detect the contact, each of these points or nodes on body Ω1 is projected on to body Ω2 and the normal distance to the body form the point is

(17)

10

said to occur. The conditions for maximum distance and the normal traction force acting on a body are written as inequality constraints (Kloosterman 2002):

𝑛_𝑑 ≤ ⅆ_max (1)

𝑡𝑛 ≤ 0 (2)

𝑡𝑛 𝑛𝑑 = 0; (3)

where 𝑡_𝑛 is the traction component in the outward normal direction.

Along with the constraints in Equations 1, 2 and 3, frictional constraints are also applicable in simulations where friction is considered. Different finite element solvers use different friction laws which are governed by the displacements or velocities of the contacting bodies. In this thesis, the friction law used in the LS-DYNA solver is:

𝜇 = 𝜇𝑠 + (𝜇𝑠 − 𝜇𝑘)𝑒−𝐷𝐶 ∣𝑣𝑟𝑒𝑙∣; (4)

where, 𝜇_𝑠 is the coefficient of static friction, 𝜇_𝑘is the coefficient of kinetic friction, DC is the damping coefficient and 𝑣𝑟𝑒𝑙 is the relative tangential velocity between the contacting surfaces.

Equation 1 creates a constraint for the contact to be initiated. This specified distance dmax, creates

an envelope of a detection area in the vicinity of the body. Equation 2 states that the normal traction acting on the body should be compressive whereas Equation 3 states a complementary condition for impenetrability. A simplified version of such an envelope and example of contact detection is shown in Figure 6. It should be noted that the distance of this envelope is negligible compared to the size of the contacting bodies and its discretized parts. If the nodes of one such body are in this envelope, a contact is established between these two bodies. In this example, the detection of the nodes of is considered through one arbitrarily chosen body. However, in contact algorithms, the detection of these nodes is based on the contact discretization selected.

(18)

11

4.2 Contact Discretization and Types

When contact is detected between two bodies, the contact algorithm kicks in. In the LS-DYNA, contact algorithm, the contacting surfaces are termed as a master surface and a slave surface. In most common contact algorithms, for the detection of contact, the penetration of the nodes on the slave side are checked at the master side. That is, only the master body will have an envelope around it to detect this contact, and if the slave body is inside this envelope, contact is said to occur. The contact algorithms can be classified based on how the master and slave sides are defined. This discretization of the contact is based on the elementary units which transmit the stresses from one contacting surface to the other. Typically, these elementary units can be:

a. Nodes, b. Edges

c. Segments (Face of the element)

Based on these units, the contacts between the master and slave sides are classified as: i. Nodes to segment

ii. Nodes to node iii. Edge to segment iv. Edge to edge

v. Segment to segment or surface to surface

The node to node discretization passes Taylor’s patch test, which is a used to assess the robustness of the contact condition (Taylor and Papadopoulos). Due to this robustness, the node to node discretization is comparatively simple to implement. However, this method requires the mesh on both the contacting bodies to be approximately of the same size and the simulation is limited to small slip and deformation conditions (Kikuchi and Oden 1988). To handle large deformations and slip, the node to segment contact was developed which is independent of the mesh density used in the contacting bodies (Bathe and Chaudhary 1985). These contact algorithms work well with simple geometries, but a drawback is that they do not pass Taylor’s patch test. A segment to segment based contact is typically used for modelling contact behavior of soft materials (Mayer and Gaul 2007). Any of the above contact algorithms can be optimized by inclusion of treatment of segments in the contacting bodies, for example, a node to surface contact algorithm can be improved by including an algorithm for the contacting segments. The segment-to-segment contact provides a robust solution for most of the contacting conditions. In this type of contact, the contacting surfaces are discretized using the faces of the elements modelling these bodies. As a result, this method has a better ability to handle the mesh differences in the bodies.

As mentioned earlier, the contact formulations can also be divided into kinematic constraint-based contact and penalty-based contacts. In the penalty-based formulation, the penetration between the two interacting surfaces is detected and then this penetration is minimized by applying a force to remove the penetration between the interacting elements. This force is applied by placing virtual springs which are normal to the interacting surfaces. A simplified diagram of this type of contact algorithm is shown in Figure 7, where the force required to minimize the penetration is provided by an imaginary spring with stiffness 𝑘_{𝑐𝑜𝑛𝑡𝑎𝑐𝑡}. The contact forces are then calculated using:

(19)

12

where, 𝑥 is the penetration depth. If solid elements are used for modelling the contacting interfaces, the contact stiffness used in LS-DYNA is given by (Livermore Software Technology Corporation 2005):

𝑘_{𝑐𝑜𝑛𝑡𝑎𝑐𝑡}𝑠𝑜𝑙𝑖𝑑 = (Sf𝐾𝐴2)

𝑉

⁄ , (6)

where, Sf is the stiffness scale factor, K is the bulk viscosity of the solid element, A is the contact

segment area and V is the element volume.

If shell elements are used for modelling the contact interface, the stiffness used is related to the characteristic length (L) of the element as (Livermore Software Technology Corporation 2005):

𝑘_{𝑐𝑜𝑛𝑡𝑎𝑐𝑡}𝑠ℎ𝑒𝑙𝑙 = (𝑆𝑓𝐾𝐴)⁄ , _𝐿 (7)

Figure 7: Simplified version of a penalty-based contact

As mentioned earlier, the contacting bodies are termed as master and slave bodies. Usually, the selection of the slave body is done in such a way that its stiffness is less than or equal to that of the master side. Traditionally, the contact is detected by the master body by searching for the nearest point on the slave body. This method is called the one-way treatment of contact. However, in case of large deformations, this may lead to an unwanted penetration of the slave body into the master body as this condition is not checked for. To check this condition, two-way treatment of contacts is needed. In such a case, the selection of the master and slave sides becomes redundant as both the bodies are checked for penetration into each other.

As the penalty-based contact work with nodes contacting the master and slave nodes or segments, there is a high dependency of the element type used in the contacting surfaces. Due to this, this method has drawbacks like poor contact in deformable bodies, failure in general patch tests, and

(20)

13

reduced convergence rate and low robustness (Yang et al. 2004). To improve these conditions, two numerical approaches can be added to the traditional penalty-based contact. Firstly, a soft constraint method, where the excess penetration is removed by the calculation of an additional stiffness based on the Courant-Freidrichs-Lewy stability conditions in such a way that the contact stiffness is given by (Baranowski et al. 2006):

𝑘𝑐ontact=

1

2𝑆𝐹𝑠𝑜𝑓𝑡𝑚

∗₍ 1

Δ𝑡_𝑖) (8)

Where, 𝑚 ∗ is function dependent on the master and slave side nodes and ∆𝑡𝑖 is the initial timestep

for the simulation.

A second method for improving the standard penalty-based contact is by adding an algorithm for the detection of segments in the contacting bodies. However, neither of these methods guarantee a solution for any contact conditions. To have a robust contact algorithm which can handle a wide range of materials and geometries a so-called mortar formulation for the contact was developed. This formulation involves the decomposition of the domains of the contacting parts (Belgacem et al. 1998). It can also be classified as an advanced segment-to-segment penalty-based contact. This method couples the different variational approximations for interacting bodies and is a relatively new method for numerical approximations. In the domain decomposition, large computational problems are broken down into several smaller size problems. In contact problems, this method divides the element boundaries into different sub-domains (Nikishkov 2007).The decomposition of the domain is implemented with the help of a direct method or a iterative solver. As a result of advances in computational capabilities, an active strategy was derived by applying a semi-smooth Newton method. This strategy is known as primal-dual active set strategy or PDASS (Hintermuller et al. 2003). This strategy was further developed by carrying out a linearization of the normal and frictional contact forces (Gitterle et al. 2010). This linearization results in so-called ‘mortar surfaces’ at the contacting element boundaries. Due to the discretized nature of these surfaces, the contact kinematics are relatively easily evaluated as compared to traditional segment-based contacts. Through this discretization, it is possible to apply the continuity conditions of the contact in a more efficient way. This provides an accurate modelling of the contact conditions (McDevitt and Laursen 2000).

Through these mortar surfaces, the transfer of contact stress is facilitated. The contact stresses observed are given by (Borrvall 2012):

𝜎𝑐 = 𝑆𝑓ε𝐾slave𝑓 (

x

𝜀𝑑_𝑐) (9)

where 𝑆𝑓 is the scale factor for the contact stiffness, 𝐾𝑠𝑙𝑎𝑣𝑒 is the stiffness modulus of the slave

side segment, x is the penetration depth, 𝑑𝑐 is the characteristic length of the element used for

modelling the body and 𝜀 is a constant (= 0.03).

Previously, this method was widely used in implicit calculations as it is an accurate and robust contact algorithm, capable of handling geometrical and material non-linearities, which led to higher likelihood for convergence. But due to advances in computational capacities, this method is now being used for explicit simulations as well. This procedure is computationally expensive for implementation in explicit simulations involving large problems (Livermore Software Technology Corporation 2006).

(21)

14

5 Metamodel Based Optimization

This chapter discusses the approach of metamodel-based optimization used in this thesis. When a component or a product is in the development stage, it is often needed to find out the correct geometrical parameters that achieve an optimal performance for its design. If the finite element simulations are performed for these models, then it is possible to achieve this optimal design by manually changing the required geometrical parameters and then simulating the design again based on the behaviour of the insert. Such a process can be called as an iterative optimization. However, this process can be repetitive and expensive as it increases the computational cost significantly and affects the efficiency of the development process.

Moreover, when complex models and multiple geometrical parameters are involved, this iterative analysis can be difficult. In such cases, a metamodel based optimization can be performed. This technique can significantly reduce the computational time and cost required to find the optimal design parameters. In this process, the repeated analyses are replaced by simpler lower order models. These simpler models or metamodels can be very useful in optimization problems which involve multiple objective and constraints. Through this technique, not only an optimization is achieved but it can also help in understanding the problem formulation for multiple variables and also predict the value of outputs of design variables (Bonte et al. 2005).

This chapter is divided into 4 stages essential stages in an optimization algorithm: sampling of variables, building of metamodels and domain reduction.

5.1 Sampling of Design Points

For an optimization, a set of design variables need to be tested to find their optimum values. The design variables can be a set of continuous points between two given limits or can be discrete value based on the design values. For example, if the upper and lower limits of a certain design space are 1 and 4 respectively, the discrete values can be (1.0, 1.2, 2.5, 2.8…) and a continuous set of points can be (1.00, 1.01, 1.02, 1.03…).A continuous set of points is simulated to explore the entire design space. While using such an input, the random design points are used to simulate the load case and record the response. The selection of design points from a design space is called sampling. Various algorithms are available in commercial FE-programs which select pseudo-random points from the design space provided. Some of the widely used sampling methods are:

i. Monte Carlo Method: This method is an adaptation of the direct Monte Carlo method

to a metamodel based optimization. In the direct Monte Carlo method, the sampling is based on random variables an no meta model is built. In case of the adapted method, the sampling is done based on metamodels and it is based on the probability distribution of the variables. Through this technique, the different possibilities of the values of the design variables occurring are established and then, a random set of values for these design variables is selected from the design space. The results from the optimization are then saved to the corresponding design points so that the results or responses can be used in later processes for statistical modelling (Paltani 2010).

ii. Latin Hypercube Method: The Latin Hypercube sampling method is used for

improving the sampling efficiency of the sampling problem. This method is superior to the Monte Carlo methods (Olsson et al. 2003). The increased efficiency of this method is due the joint probability density function that are constructed for the problem (Huntington and Lyrintzis 1998). The method reduces the design space of each of the

(22)

15

variables into smaller spaces based on the probability distribution. Then a single value is chosen from each of these intervals and then paired with random values of the other design variables to form randomly unique design points.

iii. Space Filling: Space-filling algorithms are modifications of the traditional latin

hypercube method. For a good optimization problem, it is essential that the design points are random but cover the entire range of the variables being tested. Space-filling algorithms are useful tools for replicating such conditions. They do not impose strong constraints on the model and thus allow different number of subsets for each variable (Stander et al. 2019). Space filling sampling schemes work by maximizing the minimum distance between two design points in the design space. This kind of algorithm is being widely used as a basis to set up different metamodeling techniques like neural networks and radial basis functions.

iv. D-optimal: This method is used to generate model-specific design points. This is done

by selecting the best set of points for the response surface from a given set of points. This method is useful when having several variables with a large design space. The algorithm for the d-optimal design is based on iterative search algorithm and have the objective to maximize the determinant 𝐷 = |𝑋𝑇_{𝑋| , Where X is the design matrix of}

model terms evaluated in specific design spaces (Tu and Choi 1999).

5.2 Metamodeling Techniques

Once the sampling of the design variables is completed, the simulations are run to find the responses for each of the set of design variables. Using these design points and the respective responses, metamodels are constructed. By using metamodel based methods, the simulation time is significantly reduced which makes such methods favorable to use. A few ways these metamodels can be built are explained in short below.

i. Polynomial: In this method, the metamodels are based on first order or second order polynomials which can be linear, elliptical, or quadratic. When the order of the polynomial is increased, the number of unknown coefficients to be determined increases as the number of terms in the polynomial are increased. Increasing the order results in better accuracy but also requires additional computational time. The polynomials are used to determine the significance of the design variables on the responses from the simulation.

ii. Neural Networks: This method is an extension of the linear regression methods. Neural networks are series of algorithms of these linear regressions with the objective to recognize the relationships between different design variables and responses. These algorithms adapt to changes in input and thus the algorithm can optimize to find the best solution without a need to re-simulate based on the progress in iterations. The algorithms learn more and more about the nature of the responses by reducing the mean square error between the predicted and computed responses. However, the results from such an algorithm are dependent on the input of the design variables chosen and thus can lead to unexpected errors. Neural networks can be of two types – feed forward network or the radial basis function network. While feed forward networks use non-linear regression, they tend to cost more compared to radial basis functions which use linear regression.

iii. Kriging: Kriging is a gaussian process regression which uses weights functions on design points to predict the joint probability distribution. This method is based on empirical observations from the response surface, which makes it more useful in generating estimated response surfaces. The main advantage of this technique is that it generates the uncertainty of each design point in the model (Remy et al.). This method is highly dependent on the correlation

(23)

16

of the spatial design points and is used mostly as a prediction tool to find a response to a given set of design points.

5.3 Domain Reduction

This stage of the optimization is used to reduce the design space in successive iterations of the simulations. The method used to reduce the domain is known as ‘Sequential Response Surface Methodology (SRSM). This method uses information gained from previous iteration to design the subsequent iteration. This is done by identifying the region of interest from the given design space to form a sub-space based on the approximate optimal solution of each iteration. This makes the optimization more efficient as the area of design space is reduced. If the distance between the starting design point and the predicted design point is smaller, the region of interest is reduced rapidly (Stander et al. 2019). If the optimum point lies outside the region of interest, then the region of interest remains unchanged for the next iteration in the simulation. The movement of the reduction of the design space is based on two factors - contraction and zooming parameters- which are designed to prevent premature convergence. The design spaces created strictly use a d-optimal algorithm to create new design points (Stander and Craig 2002). When using coarse convergence criteria, this method provides good accuracy when compared with direct-optimization techniques and it is also more stable and has robust convergence characteristics.

(24)

17

6 Model Building

This section discusses the model building phase of the thesis. For pre-processing (meshing and applying boundary conditions), Hypermesh from Altair was used while for model building, the solver template for LS-DYNA was used.

6.1 Model Geometry and Properties

The area of concentration of this thesis is the wings of the insert and its surrounding areas. Therefore, the part of the insert which is distant from these wings was not considered in the mesh models in order to reduce the computational costs by reducing the number of FE-entities (nodes and elements). It is noted that the geometries of the insert are symmetrical in at least 2 planes and Insert-1 has cyclic symmetry. Hence, only a quarter portion of the insert was modelled, and symmetry conditions were used as described below. The geometries of the insert that were used in the verification of the pull-in and push-out forces are shown in Figure 8 along with the modelled part.

Figure 8: Geometries of the inserts used for verifying push-in and pull-out forces

The inserts were modelled primarily using hexahedral elements while pentahedral elements were used where sharp corner was observed. The mesh models were divided into three categories - fine, medium, and coarse to check the effect of mesh densities on the contact forces of each insert as shown in Figure 9. In case of Insert-1, an additional model using axisymmetric elements was

(25)

18

created. Table 1 summarizes the number of FE-entities present in each model for the 3 designs of the insert.

Figure 9: Classification of models based on mesh properties (* indicates applicable to Insert-1 only)

For hexahedral and pentahedral elements, different formulations were tested for the boundary and contact conditions. Through trial-and-error, it was found that the element formulation ‘Fully integrated selectively reduced (S/R) elements (Livermore Software Technology Corporation 2017) intended for poor aspect ratios worked best for all conditions of mesh and contact for hexahedron elements. These elements result in improved behavior over conventional fully integrated elements by reducing the transverse shear locking observed in the later formulation of elements. For pentahedron elements, automatic sorting was used which sorted hexahedrons to the above element formulation and pentahedrons to 2-point integrated formulation.

In case of the model for the pipe, the hexahedral elements were used. As the pipe was considered rigid, and deformation of the pipe and the stresses observed on the pipe were not calculated in the FE program. Hence, it was possible to reduce the calculation times and costs. As the geometry of the pipe was fairly simple, tetrahedral elements were not used.

Table 1: Summary of number of nodes and elements used in different types of models

Nodes Elements Nodes Elements Nodes Elements

Fine 150944 119390 106358 88743 130538 110762 Medium 82685 56262 68103 56900 60074 51632 Coarse 10952 7172 29442 19662 20364 16580 Tetrahedrons 9076 22168 25168 75432 18820 54898 Axisymmetric Elements 1324 1029 Mesh Density/Type

Insert-1 Insert-2 Insert-3

(26)

19

Figure 10: Overview of Boundary Conditions used in the simulations

6.2 Initial and Boundary Conditions

6.2.1 Constraints and Loading:

As only a quarter portion of the insert was modelled, appropriate constraints were used at faces of the cross section of the insert. Single point constraints (SPCs) were used for this purpose to restrict the movement of the nodes in these respective symmetry planes. The insert position was fixed in space with the help of SPC-constraints at the bottom face of the insert which constrained the nodes in all directions. An overview of the boundary conditions is shown in Figure 10. To simulate the motion during assembly and dis-assembly, displacement was applied to the pipe using a displacement-time curve as shown in Figure 11.

6.2.2 Contact Conditions:

Initially, the well-established penalty-based surface to surface contact was tested using nominal values of friction coefficients. It was observed that for coarse meshes, large amounts of penetrations were observed. As it was important to have minimal penetration in the contacting surfaces, the stiffness scale factor for the master side elements was increased. Even though the penetration observed by changing this scale factor was less, it was observed that the scale factor was dependent on the area of the contact and the mesh size. Thus, different scale factors were needed for different insert designs and mesh densities. It was noted that by using a mortar contact formulation, this parameter tuning for scale factors was reduced, thereby reducing the number of variable parameters in the contact algorithm. With the use of such a contact algorithm, it was possible to obtain a reasonable behavior of the insert under heavy deformation. For the preliminary simulations, the values of static friction and dynamic friction were both set to 0.2 as per standard practices for preliminary simulations for the manufacturer. After the inserts were tested, the

(27)

20

diameter of the tube was modified as per the observations during the testing phase. Also, the friction parameters were set to 0.4 and 0.1 for static and kinetic friction coefficients, respectively as observed from the literature (Lancaster 1968) and design handbooks (American Institute of Physics 1972).

Figure 11: Example of displacement applied to the pipe in the simulations 6.2.1 Material Parameters:

As discussed above, the pipe was considered as rigid, the material assigned to the pipe was steel using the MAT020 material card in LS-DYNA. Nominal values of Young’s Modulus (207 GPa), density (7890 km/m3) and Poisson’s ration (0.3) were used for the purpose of mass calculations. For the insert, a linear elastic-plastic material was assigned using the MAT024 material card in LS-DYNA. The stress-strain response for this material was obtained from the material testing and material database from the manufacturer. For confidentiality purposes, the data for material data for the thermoplastic insert is not provided in the current thesis. However, a representative data for the thermoplastic of a similar type is shown in the subsequent sections.

(28)

21

7 Testing of Inserts

In this phase, the inserts were physically tested to measure the push-in and the pull-out forces. The experimental phase can be divided into 3 stages, which are explained in the subsections below.

7.1 Preparation of Samples

This procedure is applicable to inserts made of PA-6 material i.e. Insert-2 and Insert-3, because of their inherent capacity of PA-6 to absorb moisture. The inserts produced are transported by various means for a period of 2-3 weeks. Hence, environmental factors affect the moisture content in these inserts. The insert is classified as a dry sample if there is no water absorption whereas it is classified as a conditioned sample if the water absorbed by the material of the insert is maximum. A comparison of the of the stress-strain curves is seen in Figure 12, where a significant difference in the Young’s modulus and the yield limit is observed for dry and conditioned states of the material. Thus, while testing, it is important to determine the state of the samples to know the correct material parameters for the simulation. Before placing the samples in the climate chamber, the baseline mass of the samples was noted, and the procedure stated in ISO 62:2008 (International Organization for Standardization 2008) was followed. To measure and remove the absorbed water, the insert samples were place in a climate chamber at 50° C for a period of one week and weighed every 2 days. This standard states that the samples can be considered as completely dry if the change in mass between two successive weight measurements is less than ±0.001 grams. At the same time another set of samples was kept in a controlled climatic condition of temperature 70⁰ Celsius and humidity of 62% relative humidity for a period of 4 weeks. Like the dry samples, the baseline mass of the samples was noted and the procedure per ISO1110:2019 (International Organization for Standardization 2019) was followed. This standard states that the samples can be considered as completely conditioned when the change in the mass of the samples for 2 successive measurements during the climatization is less than ±0.1 grams. Both the conditioned and the dry samples were then scanned as described in Section 7.2 and tested as described in Section 7.3 and Section 7.4 below.

Figure 12: Example of difference between stress-strain curves for dry and conditioned PA6 material

(29)

22

7.2 Measuring the Samples

As the samples are made from injection molding, there are possible deviations in the manufactured components as the mold cannot have sharp edges unlike in CAD models, i.e., they will always have a small radius in place of sharp corners due to manufacturing constraints. In addition to this, the contraction of the manufactured part depends on the mold temperature and the material liquid temperature and the moisture content in the material. These parameters are difficult to control during the manufacturing process which result in the component deviating from the ideal geometry. To measure these deviations, the insert samples were scanned in a 3D scanner. As shown in Figure 13, the actual geometry of the insert varies from the ideal design (CAD design) by a substantial amount in the region of interest. The color contour plots indicate deviation in geometries of the designed and manufactured part. This deviation can lead to a change in the contact area of the insert resulting in a higher push-in and pull-out forces. In addition to this, the diameters for the pipes in which the inserts are assembles were measured. As the pipes were not perfectly circular, the average diameters were calculated based on 5 readings of each of the pipes. 4 such pipes were used to simultaneously test multiple inserts.

Figure 13: Comparison in geometries of the designed and manufactured insert

7.3 Testing for Push-in Force

To test the push-in forces, an Instron 5944 Universal Testing machine was used along with a load cell having an upper limit of 2000 Newtons. The resolution of the load cell was 0.02 Newtons and an accuracy of ±0.5% of the reading. The forces were reported at time intervals of 60 milliseconds during the test duration. The pipe was placed in a vice grip and the insert was placed lightly on the top opening of the tube as shown in Figure 14. The UTM machine was then started and the insert was pushed inside the tube with the help of an extension arm. A set of force vs displacement graphs were obtained from the test as shown in Figure 15. From this set of graphs, an average graph was obtained for each insert which was then compared to the corresponding curves from the simulations.

(30)

23

Figure 14: Experimental setup for mapping the push-in forces

Figure 15: Example of set of curves obtained from the experiments for push-in force.

7.4 Testing for Pull-out Force

After testing the samples for the push-in force, the pipe along with the inserted sample was turned 180° so that the end which did not have the insert faced the arm of the testing machine. The arm was then replaced with a solid pipe of a diameter smaller than the inner diameter of the insert as

(31)

24

shown in Figure 16. Displacement was applied to the solid pipe through the machine, which pulled the insert out from the pipe. The force required for this displacement was measured through the force transducer. The set of graphs for pull-out forces against the displacement that was obtained from the testing for each insert. An example of this set of graphs is shown in Figure 17.

Figure 16: Experimental setup for mapping the pull-out forces

(32)

25

8 Results

After the experimental phase, the results from each set of samples were processed and an average curve was obtained for the both push-in and pull-out cases for all the inserts. This average curve was then compared to the contact forces observed in the simulation.

8.1 Push-in Forces

It was observed that from Figure 18 for Insert-1, that the forces from the simulation are about 80% of the actual forces observed from the experiments. For Insert-2 and Insert-3 it can been from Figure 19 and Figure 20 respectively that the results from the simulation are significantly lower than the forces observed in the experiments for samples in the dry state. However, for the conditioned samples, the experimental forces were close to contact forces obtained from the simulations. It can also be observed from the graph that the simulations were fairly converged as the mesh density parameter did not affect the contact forces to a large extent.

Figure 18: Comparison of simulated and experimental push-in forces for Insert-1

In case of Insert-2, as seen in Figure 19, breakage of the first two wings was observed, which resulted in a higher displacement of the wings than the ideal. Due to this breakage, the peaks in the force-displacement curve appear to be spread out over a larger displacement. This results in a deviation of the experimental curve from the simulated curves as the damage and failure was not captured through the material model used in the simulation. Also, it was found that a higher push-in force is required for the dry samples. This force is approximately 1.4 to 1.7 times the push-push-in forces observed for the conditioned samples. For conditioned samples, the simulations predict the experimentally observed forces accurately. These predicted forces are 85-90% of the experimental forces. The peculiar nature of this graph results from successive deformation of the wings. Thus, each peak indicates the forces required to deform the wing.

(33)

26

Figure 19: Comparison of simulated and experimental push-in forces for Insert-2

Unlike Insert-2, no breakage was observed for Insert-3. As shown in Figure 20, this results in better correlation in terms of the peaks for the experimental and simulation curves. The simulations for this insert resulted in a lower convergence. In this case, the model with a fine mesh, predicts the experimental forces to about 80-85% of the actual push-in forces. Like Insert-2, the experimental forces observed for the dry samples are 1.45 to 1.6 times the forces observed for conditioned samples.

(34)

27

It can be concluded from the above section that finite element simulations can be used to predict the actual behavior of the insert for the push-in case with a reasonably accuracy.

8.2 Pull-out Forces

For pull-out forces, the simulations predict a considerably higher force compared to the experimental forces for all insert designs. From Figure 21, Figure 22 and Figure 23, for the simulations, as the insert is pulled out of the pipe, due to the successive disengagement of the wings, the forces required keeps decreasing with the displacement. However, in the experimental curve for Insert-1, a local peak in the forces is observed just before the disengagement of a wing. This peak maybe due to the cyclic geometry of the insert due to which may cause the air to be trapped in between the spaces of two wings. These peaks are less distinct in case of Insert-2 and Insert-3 which have cut-outs in the wings.

Figure 21: Comparison of simulated and experimental pull-out forces for Insert-1

In case of dry samples of the insert, the forces pull-out forces are considerably lower compared to the conditioned inserts. This large difference can be due to the breakage of the wings of the insert during the push-in tests. The breakage may result in a lower contact area between the insert and the tube which contributes to a decreased stiffness of the insert during the pull-out condition. In case of a conditioned sample, no such breakage was observed, which show higher pull out forces. In general, the forces obtained through simulations were about 70-80% of the experimental forces for conditioned samples, whereas the simulated forces were 1.5 to 2 times the experimental forces observed for dry inserts.

(35)

28

Figure 22: Comparison of simulated and experimental pull-out forces for Insert-2

(36)

29

9 Discussion of Results

In this section, the results from the simulations and experiments stage are critically assessed. The sources of errors that may have occurred in theses stages are listed and their impacts on the results are evaluated. This section is divided into three sections based on major sources of error.

9.1 Friction Coefficients in Simulations

The friction coefficients used in the simulations were obtained from published values found in the literature review. These studies do not take the surface roughness and the surface finish into consideration. The manufactured pipes for the furniture have a surface coating made of a fine powder or paint. These surface finishes will alter the coefficient of friction, both static and dynamic, and it will rarely be close to the values found in the literature. A study of these friction coefficients was conducted to observe the effect of change in friction coefficients on the contact forces. The effect of change in static coefficient on the contact forces can be seen in Figure 24. It is observed that the coefficient of static friction significantly alters the peaks observed in the contact forces. In contrast, there is no effect of the altering of the kinetic/dynamic friction coefficient as seen in Figure 25. Only the amount of noise observed changes when varying this parameter

(37)

30

9.2 Limitations of the Material Model

For the simulations, the material model used was a MAT24 LS-Dyna material model, which uses a stress vs plastic strain curve (or the plasticity curve) to estimate the strains in the simulation. However, in this material model, the elastic region is independent of the strain rate up to the yield point of the material. Another drawback of this material model is that variation in the failure strains because of the strain rate is not considered. Although the MAT24 material model is useful in most applications while modelling the behavior of metals, it can seldom exhibit high accuracy for plastics. The damage accumulation in the material is not considered, which limits the modelling of the failure at large strains. This incapability of modelling the failure of the material will have a larger impact in the pull-out forces than the push in forces.

Figure 25: Effect of change in coefficient of kinetic friction on contact force

9.3 Geometrical Deviations in the Manufactured Parts

As seen from the discussion in the Section 7.2, as the manufactured part deviates from the nominal dimensions. These deviations are enough to alter the dimensions to the extent that they affect the result. This is because these deviations change the contact area between the insert and the pipe and thus in turn will affect the push-in and pull-out forces. The following geometrical deviations were observed during the testing phases.

9.3.1 Circularity of the Pipe:

The manufactured part is not perfectly circular. The dimensions of the pipe are altered in the production of the pipe due to improper cooling and minute warping of the pipe due to cooling. Moreover, clamping of the pipe in the vice during the experimental phases results in the pipe attaining a slightly elliptical shape. In the simulations, a perfectly circular pipe was used.

Design Parameter Identification and Verification for Thermoplastic Inserts