FINITE ELEMENT MODELLING OF COMPACT GEARS USING STRAIN MEASUREMENTS

(1)

FINITE ELEMENT MODELLING OF COMPACT GEARS USING

STRAIN MEASUREMENTS

Saujanya Shah

Master of Science Thesis TRITA-ITM-EX 2020:519 KTH Royal Institute of Technology

Industrial Engineering and Management Machine Design

SE-100 44, STOCKHOLM

(2)

(3)

Examensarbete TRITA-ITM-EX 2020:519

Finita element modellering av kompaktväxlar med hjälp av töjningsmätning

Saujanya Shah

Godkänt

2020-09-16

Examinator

Ulf Sellgren

Handledare

Ulf Sellgren

Uppdragsgivare

ABB Robotics, ABB AB

Kontaktperson

Sara Ekermann

Sammanfattning

Robotdesign har varit ryggraden inom industriell automation och är i framkanten av utvecklingen inom alla områden. Robotdesigners använder sig av simuleringar för att korta utvecklingstider. Med växande krav på snabbare, effektiva och noggranna robotar, har kraven på datorsimuleringar ökat.

Medan huvuddelen av strukturen är utvecklad från grunden, är några komponenter köpta från leverantörer vilket skapar ett glapp i kunskapen för att kunna modellera en hel robot.

Det här examensarbetet använder en strukturerad metod för att utveckla en "grey-box" modell av en kompaktväxel, vilken tillåter robotens mångsidighet i ett kompakt format.

Metoden använder töjningsmätningar till grund för att bygga modellen. Experimentell design används som en guide för att utföra FE analyser på robotdelar med enhetslastfall, vilka skalas till verkliga lastfall.

Simulerade och uppmätta spänningar jämförs för att optimera modelleringen. Det föreslås även en metod där kompaktväxlarna inte modelleras som solider. Metoden fungerar väl för robotarmar som ingick i denna studie, dock bör den verifieras på andra modeller och delar.

Slutligen föreslås implementering av metoden som tagits fram i denna rapport samt ytterligare arbete för att verifiera metoden.

Nyckelord: Design av experiment för finita elementanalys, gråboxmodellering, skalning av spänning, simulerad och avmätt spänning.

(4)

(5)

Master of Science Thesis TRITA-ITM-EX 2020:519

FINITE ELEMENT MODELLING OF COMPACT GEARS USING STRAIN MEASUREMENTS

Saujanya Shah

Approved

2020-09-16

Examiner

Ulf Sellgren

Supervisor

Ulf Sellgren

Commissioner

ABB Robotics, ABB AB

Contact person

Sara Ekermann

Abstract

Robot design and development has been the backbone of industrial automation and is in the forefront of accelerated development across all areas. Robot designers have been using simulations for reducing product development lead times. With growing demand for faster, precise and efficient robots, the requirements on computerized simulation for stress analysis has become stringent. While the product structure is mostly designed and developed from scratch, some components are sourced from suppliers, leaving a gap in the knowledge for modelling an entirety of a robot.

This thesis applies a structured method to develop a grey-box model of the compact gears, which provides the robots its dexterity in a compact form factor. The method utilizes experimental strain measurements as a basis for building the model. Design of experiment is used as the guide for conducting FE analysis on robot links with unit load case, followed by scaling of stresses to actual load case. Simulated and measured stress plots are compared to conclude on optimum modelling approach.

Further, the thesis proposes an alternative method for stress analysis of robot links by omitting the compact gear embodiment. While the method applies well on the robot links considered during the study, its validation across other links and robot architecture is yet to be performed.

Finally, recommendations for implementation of proposed method and areas for expanding this thesis work are proposed.

Keywords: Design of experiment for finite element analysis, grey-box modelling, scaling of stress, simulated and measured stress.

(6)

(7)

FOREWORD

I would like to begin by thanking everyone who have been there with me during the turmoil and calmness throughout my life. This includes Swedish Institute for offering me the prestigious Swedish Institute Scholarship for Future Global Leaders for this platform in Sweden.

You have made me who I am today.

This thesis work was possible due to the faith bestowed upon me at ABB Robotics, by my manager Sara Ekermann and supervisor Mattias Tallberg. Andréas Göransson, Magnus Trostén and Robert Hansson have equally contributed in filling the knowledge gap and answering my questions during their busy hours. I would like to extend my gratitude towards my university supervisor Ulf Sellgren for guiding me through this thesis.

Finally, I would also like to thank my parents for guiding and believing in me throughout my journey.

Saujanya Shah Västerås, September 2020

(8)

ACRONYMS

CAD Computer Aided Design

FE Finite Element

FEA Finite Element Analysis

FEM Finite Element Model

DOE Design of Experiments

MBS Multi-Body Simulation

RMSE Root Mean Squared Error

Ax Axis

(9)

LIST OF FIGURES

Figure 1: Compact gear (Nabtesco, 2020) ... 1

Figure 2: IRB 6700 (ABB) ... 3

Figure 3: Methodology ... 6

Figure 4: Overview of robot design procedure ... 7

Figure 5: Load definition and geometry behaviour with rigid connection ... 10

Figure 6: Load definition and geometry behaviour with deformable connection ... 11

Figure 7: Stacked rectangular rosette (Micro-Measurements)... 14

Figure 8: Fractional factorial design specification ... 18

Figure 9: Dimensional parameters of compact gear embodiment ... 20

Figure 10: Robotic arm; Left: Robot A, Right: Robot B ... 21

Figure 11: Surface patch representing effective mating surface on arm for Robot A ... 22

Figure 12: Surface patch representing effective mating surface on compact gear embodiment for Robot A ... 22

Figure 13: Surface patch representing effective mating surface on arm for Robot B ... 23

Figure 14: Surface patch representing effective mating surface on compact gear embodiment for Robot B ... 23

Figure 15: Coordinate system definition ... 24

Figure 16: Mesh on lower arm of Robot A ... 25

Figure 17: Mesh on lower arm of Robot B ... 25

Figure 18: Boundary condition for Robot A ... 26

Figure 19: Boundary condition for Robot B ... 27

Figure 20: Flowchart for verifying validity of linear analysis ... 28

Figure 21: Strain gauge location on Robot A ... 29

Figure 22: Strain gauge location on Robot B ... 29

Figure 23: Effect of factors for Robot A ... 33

Figure 24: Effect of factors for Robot B ... 34

Figure 25: Principle strains and von Mises stress for Robot A, gauge LA01 (Rank 1/16) ... 34

Figure 29: Principle strains and von Mises stress for Robot B, gauge U01 (Rank 1/16) ... 36

Figure 33: Principle strain and von Mises strain with direct attachment of remote points on Robot A . 39 Figure 34: Principle strain and von Mises strain with direct attachment of remote points on Robot B . 40 Figure 35: Relative penalty across two gauges - Robot A ... 41

Figure 36: Relative penalty across two gauges - Robot B ... 41

(10)

(11)

1 INTRODUCTION

This chapter sheds light on the origin of this master thesis project, its impact on the sponsor organization, the proponent and to the community in general. The limitations implied by time, resources and capacity are also highlighted. The method chosen to proceed in the thesis work is also described in brief.

ABB AB, a leading manufacturer and supplier of industrial robots (also called Flexible Manipulators) is working continuously to optimize its robots to reduce cost, improve precision and lower robot weight to payload ratio. This goal requires greater accuracy in modelling the behaviour of every component that comprises the robot. Individual components are assessed, validated and approved for incorporation into the system. Many components are based on industrial trade secrets and pose difficulties in inclusive assessment. One such component is the compact gears.

Compact gears are the heart of modern industrial robots, providing it with the dexterity and load capacity in a small form factor. These compact gears usually use cycloid gear reduction technique due to their ability to provide great gearing ratio, high stiffness and high load carrying capacity. The internal components and details are trade secrets of the compact gear manufacturer, limiting knowledge to the robot manufacturer using these compact gears.

Figure 1: Compact gear (Nabtesco, 2020)

(14)

In (Moberg, 2010) various established methods of modelling a robot: flexible joint model, flexible link model and the extended flexible joint model are delineated. In (Moberg, 2010), these models are introduced in relation to robot system modelling, but the importance of stiffness of various components that is necessary to accurately represent a robot is also emphasized. Increasing the modelling complexity increases the lead time for a robot development. Solid models used for simulation also need to be accurate enough to suffice requirements from finite element analysis. Current development time for a robot family ranges from 5 to 10 years or more. During this development process, various iterations are performed, individual component performance is verified, and the system is analysed. Mechanical analysis of robot arms play an important role in assessing load bearing characteristics and fatigue life.

The time required for modelling and simulation must be maintained as low as possible, to allow various iterations to be tested.

The issue being investigated in this thesis has its root in the lack of knowledge on interfacing component – the compact gear. A compact gear is often the only interface between adjacent arms. However, these compact gears are grey-box models, severely limiting the possibility of correctly modelling boundary conditions during mechanical structural analysis. Simulation results at locations close to boundary conditions, is often erroneous, thus, validation is done at multiple locations away from boundary conditions to validate a finite element model.

1.1 Background

1.1.1 Robot structure

A serial N link robot has N+1 serially mounted bodies connected by N revolute joints. The position and orientation of the end effector of a robot with N ≥ 6 actuated links can be fully controlled, and is thus used for most industrial applications (Moberg, 2010, p. 23). There are de facto specialized robots with lesser actuated links for application specific requirements, but a general-purpose robot has 6 actuated joints, which is commonly called a 6-axis robot. Some terminologies necessary to follow through this thesis work are shown in Figure 2. Focus of this thesis work is on Lower arm, which is coupled to neighbouring links at Axis 2 and Axis 3.

Lower arm transfers load from upper structure of the robot to the frame. Lower arm is also the longest link in this robot.

(15)

Figure 2: IRB 6700 (ABB)

1.1.2 Need for Mechanical Analysis

Demand for robust, efficient and compact robots coupled with shortened development timeframes cannot be met by traditional engineering methods. Mechanical analysis is performed to understand the physical response of components under load. Computational tools are employed to minimize the lead time from market requirement to finished product.

Computational tools also minimize the cost associated with development activities viz.

manufacturing and physical testing of prototypes. Mechanical analysis in a generalized setup focuses on stress analysis to predict failures and design against failure. Mechanical analysis also ensures fatigue life and enables optimization to lower robot to payload weight ratio.

The Research and Development team is responsible for designing robots within quality guidelines. To maintain its position in the market, ABB needs to continuously improve its processes, including design practices. Mechanical Analysis thrives to improve its capability to provide necessary simulation results in the most accurate, yet efficient way as possible.

1.2 Purpose

Loads acting on every joint are derived from a multibody simulation model in an in-house software, are applied on the components as remote loads in a FEM. Since remote loads pose serious alterations in the observed stresses near the boundary conditions, it is important to correctly model these boundary conditions to minimize adverse variations. Correct

(16)

distribution of stress near boundary conditions is necessary to completely assess a robotic arm by FE analysis. With growing demand for optimized robots, topology optimization is of interest. For topology optimization to work effectively, load paths need to be modelled accurately. Fatigue life analysis is also sensitive to local stresses and its distribution. These requirements underscore the necessity for a robust method for FE analysis. Effect due to remote boundary condition is of focus due to known deviations occurring from the simplifications in modelling.

Various sub-modelling approaches exist, which focus on improving stress results in a localized zone of interest, where stress concentrations occur. On FEA, sub-modelling can be applied by transferring nodal displacements and refining mesh locally on the sub-model. Sub-model can also be built with increased geometric details at the region of interest. Such work can be found in the academia and the industry (Ahlbert, 2012). However, this approach is applicable when details about the models are well known, unlike the case in this thesis work.

This thesis concerns with modelling and simulation of robotic arms and support structures.

Robotic arms are modelled and simulated at a component level. Robotic arms are connected to the next robotic arm, usually in series, with a compact gear between consecutive arms.

Compact gears are Grey-box models, with known torsional rigidity and bending stiffness.

However, stiffness imparted to the mating surface is unknown. Even an approximate model of compact gear requires correctly modelling of the various components housed within the compact gears (bearings, pretension, materials, treatments, structure to name a few). Contacts are non-linear and is known to drastically increase the simulation time. Modelling of such components is also time consuming and resource intensive. These lead to forfeiture of including its effects on the neighbouring components.

Loads that are applied on the robotic components during its load cycle varies drastically.

During a complete load cycle, components can experience load reversals. Such high number of load cases are virtually impossible to simulate in a FEA. Maximum loads are extracted from load cycles and applied to the FEM to check worst case scenarios.

Components are also tested by placing strain gauges in regions of interest. These readings upon post-processing, yield a stress curve, which is then used to verify the FEA. For this verification, FEA is conducted with a unit load case, generating a stress tensor for the point of interest.

Then, the stress tensor is simulated with every load case at every time step of the live test.

Resulting simulated stress readings is the basis for comparison with experimental stress readings, to verify the correctness of the FEA. This method of using stress tensor is only possible if the model is linear, thus averting modelling non-linear (contact) models.

The viable alternative is to create a simplified component to emulate the interaction of compact gears with the component of interest. This thesis explores parametric optimization of a simplified gear model, to realize the best match between experimental stresses and simulated stresses at regions of interest. The level of simplicity is bare minimum, to minimize the time required for iterative simulations during the product development process.

1.3 Research questions

a) How can effects from adjacent components be modelled in a simplified FEM?

b) How can a simplified FEM be validated?

(17)

c) How can components with incomplete details (trade secrets) be modelled in FEA?

d) What parameters defining a compact gear embodiment has influence on results of FEA?

e) Can a solid model be used to emulate compact gears for FEA?

f) What method of remote load application (software specific) must be used?

1.4 Delimitations

To achieve the goal within the provided timeframe, the following delimitations were imposed.

 Validation of the proposed method across different compact gears and robot architecture is not performed.

 Compact gear in itself is not modelled to study its characteristics;

 Validation by analytical methods is not performed;

 Thermo-mechanical effects during operation is not considered;

 Dynamic characteristics and influence from simplified models on a dynamic model are not considered;

 Linear behaviour of material under loading is verified and enforced;

 Contact phenomenon underlying at compact gear – robot arm interface is not simulated.

1.5 Limitations

During this thesis work, owing to limitation in time and availability of resources, the following limitations were inevitable.

 Strain measurement data for Robot A is performed during this thesis work but the strain measurement data for Robot B is gathered from ABB’s database.

 The number of strain gauges used, are limited; the necessity of more gauges was not foreseen during the measurement phase.

 Gauges on Robot B were decided and applied before conceptualizing this thesis work, thus do not have gauges very close to boundary conditions.

 Lack of know-how of internal tool used for generating loads during test cycles has inhibited verification of load matrices.

1.6 Methodology

The thesis begins with a study of robotic architecture, familiarization with experimental strain measurement and task specific knowledge. Review of former work conducted in similar areas in the academia and within the organization is performed. This study leads to a refined understanding of the task at hand. A preliminary approach of tackling the work is formulated as expressed in the flowchart in Figure 3.

(18)

Figure 3: Methodology

Research questions are formulated in draft, followed by setup of delimitations to complete the thesis work in time. A design of experiment is then built with the simulation time of FE model in mind. Experimental strain measurement data is gathered. The set of experiments is conducted on Ansys and required data is extracted from every experiment. Post-processing of this data leads to results from the DOE. The results from DOE are analysed and further simulations are conducted to assert the findings and amend the method followed during the thesis work.

Background study Build a Design of Experiment.

Build FE model on Ansys

Extract tensors from Ansys for the Design Table.

Compare simulated and measured strains and stresses.

Analyze and interpret DOE to find major effects.

Quantify and minimize differences in various design points Run additional simulations if necessary

(19)

2 FRAME OF REFERENCE

This chapter presents independent theoretical substances which are applied simultaneously during implementation. This chapter is important in understanding concepts and its limitations, as applicable to this thesis work.

2.1 Robot design process

A schematic of the robot design procedure is shown in Figure 4.

Figure 4: Overview of robot design procedure

Detailed design is a complex task accomplished collectively by specialized cross functional teams. A typical sequence of product development applies to robot development, viz. solid models of components are designed to meet dimensional requirements, multibody simulation of the robot is performed, structural integrity is verified by FEA, followed by manufacturing of a prototype. Experimental tests are then performed to verify correctness of simulations.

Mechanical Analysis team performs analysis on solid components for structural performance and life. Loads are generated from an in-house multibody simulation software adapted for robot design. Solid models are acquired from the design team, simplification of model is done, boundary conditions established, and finite element model is setup and the process are iterated until requirements are met.

(20)

2.2 Mechanical analysis

2.2.1 Normal Strain

In (Sundström, 2010), a concise definition of stress and strain is provided. As described in (Sundström, 2010, pp. 14-16), it is sufficient to specify three normal strain components in three orthogonal directions together with three shear components along the same axes. These six quantities are called strain components and can be represented as

𝜀 = [𝜀_𝑥𝑥 𝜀_𝑦𝑦 𝜀_𝑧𝑧 𝛾_𝑥𝑦 𝛾_𝑦𝑧 𝛾_𝑥𝑧] (1) In Matrix form, strain matrix T is a symmetric matrix represented as

𝑇 = [

𝜀_𝑥𝑥 𝜀_𝑥𝑦 𝜀_𝑥𝑧 𝜀_𝑦𝑥 𝜀_𝑦𝑦 𝜀_𝑦𝑧

𝜀_𝑧𝑥 𝜀_𝑧𝑦 𝜀_𝑧𝑧] (2)

where,

𝜀_𝑥𝑦= 𝜀_𝑦𝑥 𝜀_𝑦𝑧 = 𝜀_𝑧𝑦 𝜀_𝑥𝑧 = 𝜀_𝑧𝑥

(3)

It is important to recall that strain component ε is related to shear component γ as, 𝜀_𝑥𝑦 = 𝜀_𝑦𝑥 = 1

2 𝛾_𝑥𝑦 𝜀_𝑦𝑧= 𝜀_𝑧𝑦 = 1

2 𝛾_𝑦𝑧 𝜀_𝑥𝑧 = 𝜀_𝑧𝑥= 1

2 𝛾_𝑥𝑧

(4)

Equation (1) can thus be expressed as

𝜀 = [𝜀_𝑥𝑥 𝜀_𝑦𝑦 𝜀_𝑧𝑧 2𝜀_𝑥𝑦 2𝜀_𝑦𝑧 2𝜀_𝑥𝑧] (5) 2.2.2 Principle Strain

For each point in a body, there is at least one coordinate system in which shear components are zero. The strains in this coordinate system are called principle strains 𝜀₁ > 𝜀₂ > 𝜀₃. These principle strains are the eigenvalues of the matrix T given in (2). 𝜀1 is called the maximum principle strain with maximum positive value while 𝜀₃ is called the minimum principle strain.

2.2.3 Normal Stress

The state of stress at a point in space is uniquely defined by nine stress components σxx , σyy , σzz , τ^{xy ,}τ^{yx ,}τ^{yz ,}τ^{zy ,}τ^{zx ,}τ^xz. Moment equilibrium requires that shear stresses on opposite faces are equal in magnitude.

𝜏_𝑥𝑦= 𝜏_𝑦𝑥 𝜏_𝑦𝑧= 𝜏_𝑧𝑦 𝜏_𝑥𝑧 = 𝜏_𝑧𝑥

(6)

(21)

Normal stress is often represented in a vector notation as vector σ. Note the change in notation of shear stress from τ to σ. Also, (6) has been applied to reduce the stress components from nine to six unique components.

𝜎 = [𝜎_𝑥𝑥 𝜎_𝑦𝑦 𝜎_𝑧𝑧 𝜎_𝑥𝑦 𝜎_𝑦𝑧 𝜎_𝑧𝑥] (7) In matrix form, stress matrix S is a symmetric matrix represented as

𝑆 = [

𝜎_𝑥𝑥 𝜎_𝑥𝑦 𝜎_𝑥𝑧 𝜎_𝑥𝑦 𝜎_𝑦𝑦 𝜎_𝑦𝑧

𝜎_𝑥𝑧 𝜎_𝑦𝑧 𝜎_𝑧𝑧] (8)

2.2.4 Principle Stress

For each point in a body, there is at least one coordinate system in which shear stresses are zero. The stresses in this coordinate system are called principle stresses σ¹ > σ²> σ³. These principle stresses are eigenvalues of the matrix S given in (8). σ1 is called the maximum principle stress with maximum positive value while σ³is called the minimum principle stress.

2.2.5 Hooke’s Law

The most basic form of Hooke’s law is written as

𝜎 = 𝐸𝜀 (9)

where σ is the stress, E is the modulus of elasticity and ε is the strain. This is applicable to materials within the linear elastic limit.

A matrix notation of Hooke’s law is found in (Larson & Bengzon, 2013, p. 265). For a homogeneous isotropic linear elastic material, Hooke’s law is represented as

𝜎^𝑇 = 𝐷𝜀^𝑇 (10)

where the 6 x 6 matrix D is given by

𝐷 = [

𝜆 + 2𝜇 𝜆 𝜆 0 0 0

𝜆 𝜆 + 2𝜇 𝜆 0 0 0

𝜆 𝜆 𝜆 + 2𝜇 0 0 0

0 0 0 𝜇 0 0

0 0 0 0 𝜇 0

0 0 0 0 0 𝜇]

(11)

in three-dimensions. The elastic moduli μ and λ are called Lamé’s parameters (Larson &

Bengzon, 2013, p. 259), defined by

𝜇 = 𝐸

2(1 + 𝜈) ,

𝜆 = 𝐸𝜈

(1 + 𝜈)(1 − 2𝜈)

(12)

where E is Young’s elastic modulus, and ν is the Poisson’s ratio.

2.3 Ansys

Ansys is an engineering simulation and analysis suite. Ansys mechanical provides necessary tools for structural analysis. It provides stress analysis results in a user-friendly manner. Ansys

(22)

Workbench has been used in this thesis work for FE simulations and generation of Strain Tensors. It should be noted that there isn’t a user-friendly method for extracting the said tensors. However, the probe tool can be used to extract the required results, exported into an excel sheet and built into tensors.

2.3.1 Remote Boundary Conditions

In reality, every component is a part of a bigger system. Level of detail and the total number of components in a simulation study is often not comparable to reality, implying various boundary conditions. Often, components are simulated individually. During such a simulation, remote boundary conditions are used to transfer loads and displacements from connected bodies. The components that are not modelled, but the resulting loads and displacements are transferred are called abstracted objects. Remote boundary conditions are simplifications, thereby limiting the extent of information, such as stiffness, being transferred. ANSYS mechanical provides different options for applying remote loads and displacements to the body under investigation. Rigid, Deformable, Coupled and Beam method of attachment to geometry are available to choose from. These are briefly discussed in the following section, which has been extracted from the software documentation (ANSYS, 2019).

2.3.2 Behaviour of attached geometry

Rigid method stiffens the attached surface infinitely, thus attached surface maintains its geometric shape under load, see Figure 5, where the highlighted red area is used as the attachment surface. This attachment method is useful when the abstracted object significantly stiffens the model at the attachment point.

Figure 5: Load definition and geometry behaviour with rigid connection

Deformable method as shown in Figure 6, allows the attached geometry to deform under load.

The software distributes applied loads to the scoped nodes, considering the geometry as well as weighting factors. An important distinguishing feature of this attachment mechanism is that the constraint equations generated by the software is such that the motion of the remote point/master node is the average of attached/slave nodes. For moments, a least squares

(23)

approach is used to define the average rotation at the remote point from the translations of the slave nodes.

Figure 6: Load definition and geometry behaviour with deformable connection

Coupled scoping method couples scoped nodes, meaning the scoped nodes share the same degree of freedom and displacements. When displacements or forces are applied to a remote point that is coupled to a surface, all underlying nodes bear the same displacement or forces as the remote point.

Beam scoping is a rather direct method of scoping remote loads to the scoped nodes. This option creates linear massless beam elements to connect remote points to scoped geometry.

Material properties and radius of beam can be set in options for this scoping method. It is often useful when working with shells.

2.4 Modelling complexities

Fully defined models have underlying physics embedded in the model data, to reproduce effects from changes in the inputs. When underlying physics are unknows or complex to model or consume extensive computational resources, a method of co-relating outputs to the inputs is performed, producing the grey-box model. Outputs from known inputs are measured and a simplified function is generated to emulate the output back from the input. In relation to this thesis, compact gearboxes are defined in terms of bending stiffness and torsional rigidity. This does not provide sufficient information to fully construct a computational model to calculate stiffness imparted to the mating surface on the robotic arm.

2.4.1 Full model

A full model of compact gears with included components like bearings, gear contacts, fasteners, enclosure with the right material properties and contact phenomena can be used to correctly include all effects into adjacent robotic components - the robotic arms. Work has been done in this field and suitable methods have been devised. (Lee & Tesar, 2011) evaluated bearing choices for robotic applications. The importance of higher stiffness for robotic

(24)

can be modelled using method suggested by (Guo & Parker, 2012) where they populate full stiffness matrix of rolling element bearings. This can be coupled with contact mechanics applied on cycloidal gear profile generated by methods adapted by (Nachimowicz & Stanislaw, 2016). Accurate details about the construction of compact gear should be known to proceed with a full model FEA. It should also be noted that these methods provide rather accurate, time dependent, non-linear model. This model, however, violates condition for stress and strain scaling, discussed in section 3.4.

2.4.2 Simplified model

Needless to mention, simplification is a common approach to solving complex physical phenomena. Simplified bearings as performed by (Adolfsson, 2015), instead of contact mechanics is a simplification that can be applied in a compact gear model. Simplified gear contact models and material properties can be used to generate a model of compact gears. Even for a simplified model, internal details of vital components should be known to a high accuracy to correctly build a simplified model of compact gears, deeming it unsuitable during this thesis work.

2.4.3 Grey-box model

A behavioural model assumes experimental measurements as the basis for formulating a simple embodiment of material which provides the stiffness transferred to the object of interest. This is an open-ended approach as to how the embodiment is formulated and what parameters are varied for achieving results close to experimental measurements. A FE model comprises of solid bodies, connections and material properties. Adjacent components are only modelled to correctly achieve stress results in the body of interest. All variable parameters can be changed to achieve targeted results.

An alternative approach is to create an embodiment with varying stiffness in different directions, such as a cube with orthotropic material properties and tune the properties to match experimental measurements. Geometrical parameters of embodiment and material properties, such as modulus of elasticity and poisons ratio are some of the parameters that affect the overall stiffness of the body. The embodiment can be attached to robotic arms by appropriate software specific attachment mechanisms, see section 2.3.1 and 2.3.2.

2.5 Principle of superposition

Principle of superposition as given in (Karasudhi, 2012, p. 235), is a concept in the analysis of structures, which states that the deflection at a given point in an object produced by several loads acting simultaneously on the object can be obtained by superposing deflections at the same point produced by loads acting individually. The same can be extended for stresses. This concept is only applicable for a linear elastic material if the deformation is within the linear elastic range.

If 𝜀₁ and 𝜀₂ are the deformations along an axis, corresponding stresses are 𝜎₁ and 𝜎₂, then the deformation due to load 𝐴1𝜎₁+ 𝐴₂𝜎₂ is

𝜀 = 𝜀₁+ 𝜀₂ (13)

where 𝐴₁ and 𝐴₂ are constants.

(25)

2.6 Design of Experiments

Design of experiment is a technique that is often employed for optimizing parametric studies.

In order to develop a grey-box model, the output corresponding to various input parameters must be studied and co-related. This particular task is the core expertise of experimental design. As excerpted from (NIST, 2020), In an experiment, we deliberately change one or more process variables (or factors) in order to observe the effect that the changes have on one or more response variables. DOE allows screening of factors, quantify individual influence and the combined effects of one or many factors on the response.

To construct a grey box model, variables/factors are selected, response is identified, and an experimental setup is selected. DOE is a set of tools that also enable minimization of required experiments at the cost of not being able to correctly identify interaction effects of one or many input factors. This is oftentimes acceptable as higher order interactions of factors do not have prominent effects on the response.

2.7 Experimental measurement

2.7.1 Strain measurements

Strain gauges facilitate experimental measurement of state of strain. The working principle behind metal strain gauges is that electrical conductors change its resistance in response to strain. This resistance change is very small. A Wheatstone bridge circuit is used to convert change in resistance to a change in voltage, which is then amplified using amplifying circuitry to a level suitable for indicating or recording instruments. Strain gauges are well discussed in (Hoffmann, 1989).

0-45-90 ROSETTE

Commonly called rectangular rosette, the 0-45-90 rosette is the most common choice for strain measurements. They contain three individual strain gauges in a backing with the second and third at an angle of 45° and 90° from the first, respectively. They are available in stacked (shown in Figure 7) as well as planar configurations, of which stacked is a common choice for its compactness (Micro-Measurements, 2008). Stacked rectangular rosette also have an advantage in applications with high stress gradients in the region of interest.

(26)

Figure 7: Stacked rectangular rosette (Micro-Measurements)

There are analytical equations, (Hoffmann, 1989) and (Micro-Measurements, 2008), for calculating principle strains, principle stresses and equivalent von Mises stresses, given respectively in (14), (15), (16) and (17). εa, εb, εc are measured strains along the three directions respectively in an anti-clockwise order. E is the Young’s modulus of elasticity for the material and ν is the Poisson’s ratio. ε^1,2 are principle strains, σ¹,σ² are principle stresses and σ^vMis the equivalent von Mises stress.

𝜀_1,2 =(𝜀_𝑎+ 𝜀_𝑐)

2 ±√(𝜀_𝑎− 𝜀_𝑏)²+ (𝜀_𝑏− 𝜀_𝑐)²

√2 (14)

𝜎₁ = 𝐸

(1 − 𝜈²)(𝜀₁− 𝜈𝜀₂) (15)

𝜎₂ = 𝐸

(1 − 𝜈²)(𝜀₂− 𝜈𝜀₁) (16)

𝜎_𝑣𝑀= √𝜎₁²− 𝜎₁𝜎₂+ 𝜎₂² (17)

An equivalent alternative form for calculation of principle stresses can be found that uses measured strains and material properties, given as

𝜎_1,2=𝐸

2[(𝜀_𝑎 + 𝜀_𝑐)

1 − 𝜈 ± √2

1 + 𝜈√(𝜀_𝑎− 𝜀_𝑏)²+ (𝜀_𝑏− 𝜀_𝑐)²] (18) 0-60-120 ROSETTE

Delta rosette has three individual strain measurement with the second and third direction at an angle of 60° and 120° respectively, from the first. These gauges are no different in functional characteristics but traditionally not preferred due to complexities in the calculation of related strain and stress measures. However, with today’s computational resources, it is analogous to rectangular rosettes but has not gained much popularity. The equations associated with delta gauges are as follows.

𝜀_1,2=(𝜀_𝑎+ 𝜀_𝑏+ 𝜀_𝑐)

3 ±√2

3 √(𝜀_𝑎− 𝜀_𝑏)²+ (𝜀_𝑏− 𝜀_𝑐)²+ (𝜀_𝑐− 𝜀_𝑎)² (19)

(27)

(15), (16) and (17) holds true for delta rosette for calculation of principle stresses and equivalent von Mises stress from principle strains. An alternative form of calculating principle stresses is given in (20)

𝜎_1,2=𝐸

3[(𝜀_𝑎+ 𝜀_𝑏+ 𝜀_𝑐)

1 − 𝜈 ± √2

1 + 𝜈√(𝜀_𝑎− 𝜀_𝑏)²+ (𝜀_𝑏− 𝜀_𝑐)²+ (𝜀_𝑐− 𝜀_𝑎)²] (20)

(28)

(29)

3 IMPLEMENTATION

In this chapter, chosen method is applied. The chapter provides adequate knowledge for the reproduction of the structured method and the corresponding results. Numerical data is avoided where it would be too specific, to deter reverse engineering of ABB’s proprietary details.

3.1 Component considered for the study

Two lower arms (as seen in Figure 2 and Figure 10), one from Robot A and the other from Robot B are considered for this study. Robot A and Robot B are different in various aspects, including but not limited to payload capacity, dimensions, reach, speed and self-weight. Robot B also has a balancing cylinder attached to it near Axis 2, for which necessary loads are applied during FEA. However, this variation assists in validating the methodology in a rather robust manner. The process described in this section is cloned to gather results for both robotic arms.

3.2 Design of Experiment

The objective of this DOE is to match simulated stresses with measured stresses. The process variables are the factors assumed to influence the stiffness transferred to the robotic arm, are listed in Table 1. A two-level full factorial design for k factors would result in 2^kexperiments.

For seven factors, a two-level full factorial design results in 128 experiments. The experiment in this case are the FE simulations, which are computation intensive.

Table 1: Factors under study

Robot A Robot B

Factor Low setting

[-]

High setting [+]

Low setting [-]

High setting [+]

[X1] Connection type Deformable Rigid Deformable Rigid

[X2] Young’s modulus [Pa] 1e10 1e13 1e10 1e13

[X3] Poisson’s ratio 0.01 0.49 0.1 0.49

[X4] Axis 3 Gear

embodiment length [mm]

50 200 50 200

[X5] Axis 3 Gear

embodiment hole radius [mm]

1 91 1 68

[X6] Axis 2 Gear

embodiment length [mm]

50 200 50 200

[X7] Axis 2 Gear

embodiment hole radius [mm]

1 78 1 110

(30)

The time required to perform a FEA on 128 different setups is huge. In order to reduce the number of experiments and computation time, a 2^7-3 fractional factorial design is chosen. By choosing this fractional factorial design, the required number of experiments reduces to 16, which also needs to be performed on the lower arm from the other robot. Further reading relating to DOE is suggested, which is available in the public domain (NIST, 2020). The specification of the chosen fractional factorial design is given in Figure 8. The DOE setup is shown in Table 2. Dimensional parameters considered on the compact gear embodiment are shown in Figure 9.

Figure 8: Fractional factorial design specification

2

^7-3

7 16 5 = ±123

6 = ±234 7 = ±134

Number of factors

Number of experiments

Design generators

(31)

Table 2: Fractional factorial design table

S. No X1 X2 X3 X4 X5 X6 X7

1 -1 -1 -1 -1 -1 -1 -1

2 1 -1 -1 -1 1 -1 1

3 -1 1 -1 -1 1 1 -1

4 1 1 -1 -1 -1 1 1

5 -1 -1 1 -1 1 1 1

6 1 -1 1 -1 -1 1 -1

7 -1 1 1 -1 -1 -1 1

8 1 1 1 -1 1 -1 -1

9 -1 -1 -1 1 -1 1 1

10 1 -1 -1 1 1 1 -1

11 -1 1 -1 1 1 -1 1

12 1 1 -1 1 -1 -1 -1

13 -1 -1 1 1 1 -1 -1

14 1 -1 1 1 -1 -1 1

15 -1 1 1 1 -1 1 -1

16 1 1 1 1 1 1 1

(32)

Figure 9: Dimensional parameters of compact gear embodiment

3.3 FE model setup

FE models of the robotic arms are setup in Ansys. These FE models consists of a solid model of the robotic arm attached to an embodiment representing compact gear at both axes. The embodiments for compact gears are designed parametrically in Ansys SpaceClaim while the solid models for robotic arms, shown in Figure 10, are provided by the design team at ABB Robotics. These robotic arms are manufactured by casting nodular iron. Material properties are defined in Engineering Data by creating a new material as given in Table 3. A second material is also defined in Ansys to enable parameterization of material properties of the compact gear embodiments.

Length of Compact Gear embodiment

Internal Radius of Compact Gear embodiment

(33)

Figure 10: Robotic arm; Left: Robot A, Right: Robot B Table 3: Material properties of the robotic arms under study

Material Nodular Iron, EN-GJS-500-7 Young’s modulus (E) 169000 MPa

Poisson’s ratio (ν) 0.275 Fatigue limit 130 MPa

Yield limit 320 MPa

Fracture limit 500 MPa 3.3.1 Contact surface preparation

Both robotic arms are attached to the compact gears by bolts. To simulate contact area, a surface patch around the bolt holes on the arm is created. The same surface patch is created on the mating compact gear embodiment. For FEA of Robot A, this patch is created on the lower arm with an offset of 3 mm is created around the holes, leaving 0.5 mm towards the flange as

Axis 3

Axis 2

(34)

shown in Figure 11, where the left represents axis 2 and the right represents axis 3. The same surface patch is created on the compact gear embodiment as shown in Figure 12 for Robot A;

left represents axis 2 and right represents axis 3.

Figure 11: Surface patch representing effective mating surface on arm for Robot A

Figure 12: Surface patch representing effective mating surface on compact gear embodiment for Robot A

For FEA of Robot B, surface patch is created on the lower arm with an offset of 8.5 mm around the bolt holes, leaving 1 mm towards the flange as shown in Figure 13. The compact gear embodiment also bears the same surface patch around the bolt holes, as shown in Figure 14.

(35)

Figure 13: Surface patch representing effective mating surface on arm for Robot B

Figure 14: Surface patch representing effective mating surface on compact gear embodiment for Robot B

3.3.2 Coordinate system definition

To apply loads generated from the in-house multi body simulation software as introduced in section 2.1, coordinate systems in Ansys must be aligned as defined in MBS. Applicable offset is applied, and coordinate systems are setup as shown in Figure 15, for Robot A and Robot B respectively. The origin of these coordinate systems serve as the location for remote load application.

(36)

Figure 15: Coordinate system definition

As robots move about its axes, loads should also be rotated to be aligned to the axis attached to the arm. This is achieved by transformation from the global axis at the base to the coordinate system following the robotic arm.

3.3.3 Meshing

Fine mesh is required to correctly realize localized stresses. But a fine mesh dramatically increases the computational footprint. A body sizing of 8 mm and refinement at level 1 is applied to the lower arm of Robot A, resulting in a mesh that is shown in Figure 16. A body sizing of 10 mm and surface sizing around region of interest of 2 mm is created on the lower arm of Robot B resulting in a mesh shown in Figure 17. Mesh convergence has not been checked during this thesis work, instead a thumb rule has been applied.

Axis 3 is located D1 mm from bolt plane

(37)

Figure 16: Mesh on lower arm of Robot A

Figure 17: Mesh on lower arm of Robot B

Refinement applied at corners

Surface sizing around region of interest

(38)

3.3.4 Boundary condition

Loads are applied as remote loads at the origin of coordinate systems established in section 3.3.2. There are two load sets applicable to the lower arm – one set that defines loads acting from axis 3, and the other acting from section 2. These loads vary during motions due to inertia from self-weight of the lower arm. Center of mass of the arm lies closer to axis 2. Axis 2 loads include effects from self-weight of the lower arm and provides a conservative design due to an overestimation of stresses on the lower arm. Loads defined at Axis 2 are used in this study.

Loads are vectors consisting of 6 unique load components. In the case of Robot B, an additional load has been defined as the balancing force in the attachment point for balancing cylinder.

The balancing force is calculated using balancing cylinder properties. For verifying applicability of linear-elastic principles (see section 3.3.5), maximum load cases are scanned in the load file and 8 load cases are extracted - 3 load cases with maximum forces, 3 with maximum moments and additional 2 with maximum resultant force and moment. After verification, the loads are changed to unit load cases to extract strain tensors to post-process stresses for the entire load history, as discussed in section 3.4. The boundary condition for Robot A is shown in Figure 18 and for Robot B in Figure 19.

Figure 18: Boundary condition for Robot A

Axis 3: Fixed

Axis 2: Loads applied

(39)

Figure 19: Boundary condition for Robot B

3.3.5 Applicability of linear-elastic principles

A robot has different operating regimes viz. normal operation, emergency stop and mechanical stop, with different load cases, but this thesis relates to normal operation. Normal operation requires stresses to be within fatigue limit to ensure operating life. Fatigue limit is considerably lower than applicable linear elastic limit. A generalized flowchart for confirming validity of linear analysis is shown in Figure 20. This is important to apply principle of superposition which forms fundament applied in the following sections.

Principle of superposition (introduced in section 2.5) is applied in a more generalised form when FEA is used to compute stresses and strains. In applications where load cases are generated from multi body simulation, quasi-static analysis or experimentation, each load case is not simulated on FEA. Maximum forces and moments are scanned from the load cases and simulated on a FEA and checked for stress limits. If stress limits are within material elastic limit, principle of superposition is applied to emulate state of strain and stress at any point in the material at every load case. This is useful while comparing simulated strains or stresses to physical measurements performed using experimental techniques such as strain gauges. This is further discussed with applicable method in section 3.4.

Section 3: Fixed

Section 2: Loads applied Balancing loads applied

(40)

Figure 20: Flowchart for verifying validity of linear analysis

A Matlab implementation of equations in section 2.2 and 3.4 is used to calculate principle strains, principle stresses and equivalent von Mises stress. Plots of measured vs simulated strains and stresses are plotted to discern between various DOE experiments.

3.3.6 Region of interest

Strain gauges are placed on the Robot A in locations close to peak stress areas, near boundary conditions as shown in Figure 21. Robot B has strain gauges in an internal corner and one on a flat area along the length of the arm, seen in Figure 22. These locations are marked using coordinate systems and probed on Ansys using the probe tool to extract strain tensors.

(41)

Figure 21: Strain gauge location on Robot A

Figure 22: Strain gauge location on Robot B

3.4 Computation of stresses

Consider a force vector F being applied on a body is defined as

𝐹 = [𝐹𝑥 𝐹_𝑦 𝐹_𝑧 𝑀_𝑥 𝑀_𝑦 𝑀_𝑧] (21)

Let the stress state after application of forces due to each force componentbe 𝜎_𝐹𝑥= [𝜎𝑥𝑥 𝜎_𝑦𝑦 𝜎_𝑧𝑧 𝜎_𝑥𝑦 𝜎_𝑦𝑧 𝜎_𝑧𝑥]

𝜎_𝐹𝑦 = [𝜎^𝑥𝑥 𝜎_𝑦𝑦 𝜎_𝑧𝑧 𝜎_𝑥𝑦 𝜎_𝑦𝑧 𝜎_𝑧𝑥] 𝜎_𝐹𝑧 = [𝜎^𝑥𝑥 𝜎_𝑦𝑦 𝜎_𝑧𝑧 𝜎_𝑥𝑦 𝜎_𝑦𝑧 𝜎_𝑧𝑥] 𝜎_𝑀𝑥 = [𝜎^𝑥𝑥 𝜎_𝑦𝑦 𝜎_𝑧𝑧 𝜎_𝑥𝑦 𝜎_𝑦𝑧 𝜎_𝑧𝑥] 𝜎_𝑀𝑦= [𝜎^𝑥𝑥 𝜎_𝑦𝑦 𝜎_𝑧𝑧 𝜎_𝑥𝑦 𝜎_𝑦𝑧 𝜎_𝑧𝑥] 𝜎_𝑀𝑧 = [𝜎𝑥𝑥 𝜎_𝑦𝑦 𝜎_𝑧𝑧 𝜎_𝑥𝑦 𝜎_𝑦𝑧 𝜎_𝑧𝑥]

(22)

respectively.

Applying principle of superposition, the resulting stress state σ is given by the sum of individual stress state as

𝜎 = 𝜎_𝐹𝑥+ 𝜎_𝐹𝑦+ 𝜎_𝐹𝑧+ 𝜎_𝑀𝑥+ 𝜎_𝑀𝑦+ 𝜎_𝑀𝑧 (23) LA01

Axis 2

LA02

Axis 3

U01

Axis 2

U02 Axis 3

Axis 2

(42)

For strains, principle of superposition can be applied as a sum of individual strain state from each force component of F. If strain state due to each force component is

𝜀_𝐹𝑥 = [𝜀𝑥𝑥 𝜀_𝑦𝑦 𝜀_𝑧𝑧 2𝜀_𝑥𝑦 2𝜀_𝑦𝑧 2𝜀_𝑧𝑥] 𝜀_𝐹𝑦 = [𝜀𝑥𝑥 𝜀_𝑦𝑦 𝜀_𝑧𝑧 2𝜀_𝑥𝑦 2𝜀_𝑦𝑧 2𝜀_𝑧𝑥] 𝜀_𝐹𝑧= [𝜀𝑥𝑥 𝜀_𝑦𝑦 𝜀_𝑧𝑧 2𝜀_𝑥𝑦 2𝜀_𝑦𝑧 2𝜀_𝑧𝑥] 𝜀_𝑀𝑥 = [𝜀𝑥𝑥 𝜀_𝑦𝑦 𝜀_𝑧𝑧 2𝜀_𝑥𝑦 2𝜀_𝑦𝑧 2𝜀_𝑧𝑥] 𝜀_𝑀𝑦 = [𝜀𝑥𝑥 𝜀_𝑦𝑦 𝜀_𝑧𝑧 2𝜀_𝑥𝑦 2𝜀_𝑦𝑧 2𝜀_𝑧𝑥] 𝜀_𝑀𝑧 = [𝜀𝑥𝑥 𝜀_𝑦𝑦 𝜀_𝑧𝑧 2𝜀_𝑥𝑦 2𝜀_𝑦𝑧 2𝜀_𝑧𝑥]

(24)

Then the resulting strain state ε is given by the sum of individual strain state as

𝜀 = 𝜀_𝐹𝑥+ 𝜀_𝐹𝑦+ 𝜀_𝐹𝑧+ 𝜀_𝑀𝑥+ 𝜀_𝑀𝑦+ 𝜀_𝑀𝑧 (25) This principle is applied to scale strains and stresses from unit load cases to actual load cases.

This technique forms the basis for comparison using experimental strain measurements.

The load vector at every load case is represented in a six-component vector F, given in (21). A FE model is built with unit load cases, each in a separate time-step. Software specific settings such as analysis settings is set to include different load steps. Table 4 shows the load case built into multiple time steps.

Table 4: Unit load case setup

Time-Step Fx [N] Fy [N] Fz [N] Mx [Nm] My [Nm] Mz [Nm]

1 1 0 0 0 0 0

2 0 1 0 0 0 0

3 0 0 1 0 0 0

4 0 0 0 1 0 0

5 0 0 0 0 1 0

6 0 0 0 0 0 1

Points of interest is scoped for normal strain and stress components and recorded. A 6x6 matrix of strain as well as stress is built as

𝜀_{𝑢𝑛𝑖𝑡} = [

𝜀_𝐹𝑥 𝜀_𝐹𝑦 𝜀_𝐹𝑧 𝜀_𝑀𝑥 𝜀_𝑀𝑦 𝜀_𝑀𝑧]

(26)

where the components are taken from (24).

The stress components are built into a 6x6 matrix as

(43)

𝜎_{𝑢𝑛𝑖𝑡} = [

𝜎_𝐹𝑥 𝜎_𝐹𝑦 𝜎_𝐹𝑧 𝜎_𝑀𝑥 𝜎_𝑀𝑦 𝜎_𝑀𝑧]

(27)

The strains at the load case F is then given by matrix product.

𝜀 = 𝐹𝜀_{𝑢𝑛𝑖𝑡} (28)

and the stresses are given by

3.5 Comparison of simulated and measured strain/stress

The surface of a solid, not part of boundary conditions is under plane stress. The stress components associated with the direction perpendicular to surface should be zero. This is implied by the fact that there is no material on the other side to allow stress in that direction.

There is, however, a strain in the direction perpendicular to surface due to Poisson’s effect.

Plane stress condition enables experimental measurements using strain gauges applied on the surface. Only three stress components are required to fully define the state of stress. For strain gauges of specific types, there exists analytical equations to calculate related strain states and stresses, already mentioned in section 2.7.1.

While conducting a FE analysis, cartesian coordinates are often not aligned to surface normal directions, resulting in a 3-dimensional representation of state of strain and stress. Comparison by means of normal strains and stresses needs transformation. Principle strains and stresses, and von Mises stress are however best suited for comparison with experimental strain measurements. Principle strains and stresses are calculated using eigenvalues of the strain and stress matrices. Von mises stress is calculated using equation (17).

Introduced in section 3.2, the objective of DOE is to minimize difference between simulated and measured stresses. However, the stress is not a unique value, rather a time series data, bearing unique stress values during the entire operating cycle of the robot. To enable quantitative comparison, a measure called the RMSE (Root mean squared error) is used. RMSE is a basic measure of deviation between two curves. It is unable to discern if a curve is above or below another. If y and y’ are the ordinate of a data point, where time data is along the abscissa, and n represents the number of observations along the abscissa, then,

𝑅𝑀𝑆𝐸 = √∑(𝑦_𝑖− 𝑦_𝑖^′)² 𝑛

𝑛

𝑖=1

(30)

𝜎 = 𝐹𝜎_{𝑢𝑛𝑖𝑡} (29)

(44)

RMSE cannot be compared across fundamentally different curves, leading to introduction of another comparative measure between the various design points for a region of interest, herein called the Rank. This is an overview of how a design point stands amongst other candidates. A lower value means that the design point meets the objective better (RMSE closer to zero).

(45)

4 RESULTS AND DISCUSSION

The results obtained with the process/methods described in the previous chapter are compiled, analysed and compared with the existing knowledge and/or theory presented in the frame of reference chapter.

4.1 Results

The use of fractional factorial design of experiment provides the effect of factors as one of its results, shown in Figure 23 for Robot A and in Figure 24 for Robot B. Effect of factors is scalar and provides a comparative estimate amongst factors. A negative effect, as mentioned in Figure 23 and Figure 24 means that increasing these factors result in a lower RMSE, essentially meaning a better match between simulated and measured stresses. In Figure 23 and Figure 24, it is evident that modulus of elasticity has the most effect on the objective. According to the Pareto principle, adjusting only the modulus of elasticity can result in considerable changes.

On the left (for gauges closer to Axis 2), the effect of increasing modulus of elasticity reduces the RMSE, while on the right (for gauges closer to Axis 3), decreasing modulus of elasticity reduces the RMSE.

Figure 23: Effect of factors for Robot A

(46)

Figure 24: Effect of factors for Robot B

In the following Figure 25 to Figure 32, plots of principle strains and von Mises stresses are shown. The table at the bottom of every figure represents the configuration of variables for that instance. On the top of the figure, the last four characters represent the gauge names (LA01, LA02, U01 or U02), introduced in preceding sections. Only graphs for extreme rank values are shown in this report to keep it concise. For the upper graph representing strain, solid black represents measured maximum principle strain, dashed black represents measured minimum principle strain, solid red represents simulated maximum principle strain and solid blue represents simulated minimum principle strain. In the lower graph representing von Mises stress, solid black represents computed von Mises stress from measured data and the solid red represents computed von Mises stress from simulation.

Figure 25: Principle strains and von Mises stress for Robot A, gauge LA01 (Rank 1/16)

(47)

(48)

Figure 29: Principle strains and von Mises stress for Robot B, gauge U01 (Rank 1/16)

(49)

(50)

These results led to an observation and discussion (see section 4.2), suggesting an additional experimental run of FE simulations without the compact gear embodiment, by directly attaching the loads to the surface patch on the robotic arm. Surface patch at Axis 2 is attached to the remote point by rigid connection and surface patch at Axis 3 is attached to the remote point by deformable connection. The results are shown in Figure 33 and Figure 34.

(51)

Figure 33: Principle strain and von Mises strain with direct attachment of remote points on Robot A

FINITE ELEMENT MODELLING OF COMPACT GEARS USING STRAIN MEASUREMENTS