New encapsulation concept for robot controller cabinet
Siyu Guo
Master of Science Thesis TRITA-ITM-EX 2020:321 KTH Industrial Engineering and Management
Machine Design SE-100 44 STOCKHOLM
Examensarbete TRITA-ITM-EX 2020:321
Nytt inkapslingskoncept för robotstyrskåp
Siyu Guo
Godkänt
2020-06-12
Examinator
Ulf Sellgren
Handledare
Kjell Andersson
Uppdragsgivare
ABB
Kontaktperson
John Taavo
Sammanfattning
Robot styrskåp är specificerad med mängder gränssnitt vilket gör det möjligt för anslutning av olika moduler till att kunna fullborda de uppgifterna valda för robot manipulatorerna. Olika gränssnitt utnyttjas beroende på den typ av arbetsuppgift och inställningar valda just för den.
Därför kommer inte alla gränssnitt att kunna tas i bruk i ett styrskåp, vissa lämnas kvar. För att kunna uppfylla inkapslingsstandarden för elektriska kapslingar är dessa obesatta gränssnitt täckt och förseglat med påskruvad täckplåtar och packningar under montering av styrskåp. En ny inkapslingsmetod hoppas att kunna utredas och introduceras till att förbättra den nuvarande lösningen med avseende på de inkapslingskraven från ABB.
Den introducerade lösningen är ett knockout koncept. En detaljerad konstruktion undersöks med hjälp av finita element analys med explicit dynamik som grunden till att simulera knockout processer. Där tre olika design parametrar tas i beaktande för att hitta den mest optimala knockout konstruktionen.
Resultaten visar sig att, för den här särskilda stålplåten som tillhandahålls av ABB, en V-spårad knockout konstruktion med en spårvinkel på 90 grader och en tjocklek på 0.1 mm har den mest tillfredställande prestandan med avseende på jämnhet, d.v.s. reduceringen av vassa kanter, och mängder av plastiska töjningar som inträffas i materialet efter knockout processen.
Traditionella tillverkningsmetoder till att tillverka en sådan knockout konstruktion visar sig vara väldigt tidsödande och anses därför inte vara lönsamt för massproduktion. Emellertid upptäcks det en typ av relativt nyutvecklad spårmaskin, så kallad V-grooving machine, som tros att kunna lösa tillverkningsproblemet.
Nyckelord: ABB Robotik, Elektrisk knockout, Explicit dynamik, FEM, Robot styrskåp
Master of Science Thesis TRITA-ITM-EX 2020:321
New encapsulation concept for robot controller cabinet
Siyu Guo
Approved
2020-06-12
Examiner
Ulf Sellgren
Supervisor
Kjell Andersson
Commissioner
ABB
Contact person
John Taavo
Abstract
Robot controller cabinets are specified with interfaces which make it possible to connect different modules for completing numerous tasks that are chosen for the robot manipulators. Different interfaces will be utilized depend on the kind of tasks and settings that are chosen. Thus not every interface will be put into use in a controller cabinet, some are left behind. In order to fulfill the encapsulation standards of electrical enclosures, the unoccupied interfaces are covered and sealed with on-screwed cover plates and gaskets during the assembly of the cabinet. However, a new method for encapsulation hope to be investigated and introduced to improve the current solution with respect to the encapsulation requirements from ABB.
The introduced new solution is a knockout concept. The detailed design is investigated with the help of finite element analysis with the explicit dynamics method used for simulating the punching processes of the knockout designs. Where three different design variables are put into consideration for finding the most optimum knockout design.
The results show that, for the particular steel plate provided by ABB, a V-grooved knockout design with a grooving angle of 90 degrees and an unaffected thickness of 0.1 mm has the best performance in terms of smoothness at edges and the amount of plastic strain occurred in the material.
Traditional manufacturing methods to manufacture the obtained knockout design appear to be extremely time consuming and thus not profitable for mass production. However, a type of fairly recent developed grooving machines, the so called V-grooving machine, is believed to be able to solve the manufacturing problem.
Keywords: ABB Robotics, Electrical knockout, Explicit dynamics, FEM, Robot controller cabinet
FOREWORD
The work presented in this paper is the master thesis work performed at ABB Robotics in Västerås.
A special thank should be given to my industrial supervisor John Taavo for all his advice and assistance throughout the time. I also would like to thank the department manager Åsa Härdner for all the help and supports during the thesis. It was a pleasure to have my master thesis work at the R&D department.
Furthermore, I would like to thank Ulf Sellgren and Kjell Andersson for all the help they provided.
And many thanks to all people that offered their help during the time.
Siyu Guo Västerås, June 2020
NOMENCLATURE
Notations and Abbreviations that being used in this Master thesis report are compiled and presented in this section.
Notations
Symbol Description
A Initial yield stress
B Strain hardening constant
n Strain hardening exponent
C Strain rate constant
m Thermal softening exponent
E Young´s modulus
Density
Poisson’s ratio
𝐸𝑝𝑙𝑚𝑎𝑥 Maximum equivalent plastic strain
Abbreviations
EMC Electromagnetic compatibility
CAD Computer Aided Design
AWB Ansys Workbench
FEA Finite Element Analysis
FEM Finite Element Method
IP Ingress Protection
WBS Work Breakdown Structure
PDE Partial Differential Equation
EOS Equation of state
%EL Percent Elongation
JC Johnson Cook
EPS Equivalent Plastic Strain
TABLE OF CONTENTS
SAMMANFATTNING (SWEDISH) 1
ABSTRACT 3
FOREWORD 5
NOMENCLATURE 7
TABLE OF CONTENTS 9
1 INTRODUCTION 13
1.1 Background 13
1.2 Purpose 13
1.3 Requirements 13
1.4 Delimitations 14
1.5 Methodology 14
2 FRAME OF REFERENCE 17
2.1 Electrical knockouts 17
2.2 Material properties of the metal sheet 18
2.3 Finite element method 18
2.3.1 Implicit and explicit method 19
2.4 Modeling the material behavior 20
3.1.2 Design variables 24
3.2 Design simulation 26
3.2.1 Geometric modeling 26
3.2.1.1 Selecting the geometry 26
3.2.1.2 Simplification 27
3.2.1.3 Hammering tool 28
3.2.1.4 Symmetry 28
3.2.2 Material modeling 29
3.2.3 Mesh sizing 30
3.2.4 Contact modeling 30
3.2.5 Initial conditions 31
4 RESULTS 33
4.1 Design case set 1 – the unaffected thickness 33
4.1.1 “0.2 mm” 33
4.1.2 “0.15 mm” 34
4.1.3 “0.1 mm” 35
4.1.4 “0.05 mm” 36
4.1.5 “0.04 mm” 37
4.1.6 “0.03 mm” 38
4.1.7 “0.02 mm” 39
4.2 Design case set 2 – Grooving angles 40
4.2.1 “100 degrees” 41
4.2.2 “75 degrees” 42
4.2.3 “30 degrees” 43
4.2.4 “10 degrees” 44
4.3 Design case set 3 – Grooving geometries 45
4.3.1 Asterix formed grooves 45
4.3.1 Half v-formed grooves 47
5 DISCUSSION AND CONCLUSIONS 49
5.1 Discussion 49
5.1.1 The unaffected thickness 49
5.1.2 The grooving angle 49
5.1.3 The grooving geometry 50
5.1.4 Validation 51
5.1.5 The manufacturing method 51
5.2 Conclusions 52
6 RECOMMENDATIONS AND FUTURE WORK 53
7 REFERENCES 55
8 FIGURE REFERENCES 57
APPENDIX A: GANTT CHART 59
APPENDIX B: RISK ANALYSIS 60
APPENDIX C: MATERIAL COMPARISON DC01 AND DX51D 61 APPENDIX D: SIMULATION RESULTS FOR 125 AND 90 GROOVING
ANGLE KNOCKOUT 62
APPENDIX E: SIMULATION RESULTS FOR HALVED 90 V-GROOVED
KNOCKOUT 64
APPENDIX F: V-GROOVING MACHINE SPECIFICATIONS 66
1 INTRODUCTION
This chapter first describes the background and purpose of this thesis work, later the requirements will be presented accordingly. And lastly, the delimitations and methodology that being applied in the project.
1.1 Background
ABB Robotics as one of the biggest supplier of industrial robots, robot software and service of the robots, is world leading at automation within industries. The main focus of automated solutions is to help the manufacturers increase their productivity, product quality and safety in the working environments.
Each robot system contains one or several robot manipulators and a controller. The controller is the brain of the robot system. It offers the robot superior motion control and is the key to the robots’ performance. The controller cabinet hosts a full range of options to accomplish all different kind of customer demands. Therefore, the cabinets are over-specified in terms of interfaces which in many cases consists of holes and cutout patterns.
1.2 Purpose
The controller cabinet of robot manipulators are manufactured in standardized modules, means that the number of holes and cutout patterns are the same for the same type of cabinet. However, robot controller cabinets can be highly customized with the possibility for customers to choose different settings and tasks. This will result in part of the holes and cutouts in many occasions may not be in use. Thus, those unoccupied interfaces with different sizes and geometries need to be covered and sealed in order to make the enclosure to fulfill the IP-54 conditions, EMC
shielding demands and other requirements. The current solution uses screwed on cover plates and gaskets to seal the unoccupied interfaces. However, the cover plates add time and cost in production and have negative impact on the IP class, the EMC shielding and the environment.
Therefore, a new solution that is able to minimize the production time and cost and at the same time fulfill the stated requirements and demands need to be investigated and introduced.
At the end of the project it will be necessary to answer the following research question:
Is it possible to introduce a new encapsulation concept that solves the stated problem?
Other demands or desideratum including minimizing the cost and negative impact on the environments and make it possible for custom services of adding other options and settings after delivery of the system.
1.4 Delimitations
At the beginning, different possible solutions are to be generated for later concept evaluation whereas a solution concerning knockouts, which is suggested by the company, is included.
However, after subsequent discussions with the industrial supervisor it is later agreed that the focus will be laid on the knockouts concept as the only solution to be investigated and researched on.
The reason for this is that the company believes the knockout concept that might solve the problem will be a very exciting and fascinating solution. Moreover, that an IP-54 classed electrical knockout concept on metal sheets will also attain various interesting possibilities in the future.
For sealing the cutouts, the current solution uses screw-on cover plates with M4 fastite-screws.
The screw holes are located around the cutouts. Besides the function of attaching the cover plates in place, these screw holes also attach the relevant components into the place when the interfaces are in use. Another limitation in this work is to leave the screw holes aside, only the cutout part is studied for a knockout design.
1.5 Methodology
After the planning phase the concept generation phase is skipped, instead lot of researches are performed on electrical knockouts that are available on the market today and the material that are being used for electrical knockouts. See the WBS for this project work below.
Figure 1. Work Breakdown Structure.
After the researching, the design and the construction of the knockout are thought thoroughly. The calculations are performed with regards to the requirement specification of the design and the stated demands. The concept is modeled and analyzed. Furthermore, the different manufacturing
New$Encapsulation$Method$for$
Robot$Control$Cabinet
Planning Research Design
Schedule/Gantt Problem$
definition Current$
electrical$
knock@outs
CAD$
Modeling
Manufacturing Method
Calculations Investigation
Evaluation
Risk$
Assessment FEM$analysis
Material$
properties
methods for manufacture the knockout concept are investigated and analyzed from different criterions.
Lot of internet searching and literature studies are done for acquiring the knowledge of current existing electrical knockouts. Material properties and the construction of the cabinets are available using ABBs intranet, further the assembly of controller cabinets can be seen in reality at ABB’s production department. CAD models are modeled in Solid Works and analyzed with FEA.
Finite element analysis, FEA, is the simulation of complicated physical problem utilizing the finite element method (FEM). It is also the key principle in various simulation software. The main advantage of using simulation software for solving the design problem is to reduce the number of physical prototypes and experiments that are needed for an optimal design and thereby save both time and experimental cost.
The simulation program used for simulating the material behavior during the knockout process is the Ansys Workbench finite element simulation software. When punching the metal fragment piece out from the steel plate, the punching process is a relatively fast procedure involving large deformations and strains within a short period of time. Thus, the force that exerted on the metal sheet is in fact an impact force. To analyze such high speed impacts, the general purposed implicit methods is not sufficient to predict the structure responses. It is therefore more convenient to choose the explicit solution methods in AWB. The explicit dynamics is suitable for dynamic analysis of relatively short duration events for structures that undergo highly nonlinear dynamic forces. It is also able to simulate complex material and structure responses due to loadings, for example large material deformations and interactions between structures [ANSYS INC, 2011].
With the necessary input data for failure criteria, the program is also able to visualizing the material failure with eroded elements when exposed to severe loadings in the postprocessor. This is especially helpful when predicting and to the greatest extent avoid burrs formation around the edges after the knockout process.
2 FRAME OF REFERENCE
This chapter presents the theoretical frame that is necessary for the performed research and design.
2.1 Electrical knockouts
Electrical knockouts are intact punched-out patterns on electrical boxes. By intact means that the fragment pieces will still be connected in place by some areas of unaffected material to ensure the intactness. Knockouts serve to allow to quickly create holes or cutouts at the surface of the enclosure by removing the tabs when the holes are needed and allow electrical wires to travel through the interface. At this moment electrical knockouts on metal sheets are only available in low ingress protection classes, which means that they are not able to resist liquid ingress and have poor protection against dust. High IP rated electrical enclosures with knockouts are mainly made of ABS or polycarbonate, often with IP rating as high as IP66, see figure 2. Therefore, a big part of the electrical enclosures with knockouts on the markets today are made of plastic materials whereas knockouts on metals can only be used on electrical steel conduit boxes and junction boxes where high ingress protection is not a requirement. The reason for this is because the high strength of metals compared to ABS and polycarbonate and also the manufacturing method. The knockouts on ABS and polycarbonate are injection molded. Instead, knockouts on metals are made so that the knockouts are cut through completely and leaving some small places of unaffected “tabs” to secure the metal piece in place, see figure 3. This leads to gaps between metals and result in no dust nor liquid ingress protections and thereby the common IP rating is around IP 20. Further the electromagnetic compatibility will also be affected in such cases.
Figure 2. Enclosure with knockouts made of polycarbonate.
Figure 3. Knockouts on metal conduit boxes.
2.2 Material properties of the metal sheet
The material that is being used for the electrical enclosure of the controller cabinet in which the electrical knockouts are going to be placed is EN1037-DX51D+AZ150. DX51D is a low carbon steel for cold forming with bending and profiling quality. Which means that the steel has low yield strength but high ductility. Further, the designation AZ150 stands for the surface coating treatment of hot-dip aluminum-zinc alloy coating with the properties as in table 1. The material properties of the DX51D steel and the chemical composition can be found in table 2 and 3 respectively. The thickness of the steel plate is 1.5 mm. Tolerance on dimensions and shape follows the requirements of EN 10143.
Table 1. Hot-dip aluminum-zinc alloy coating Minimum total coating
mass for both side of the plate
Theoretical values for coating thickness per
surface
Density Composition
150g/m2 20 µm (15-27 µm) 3.8
g/cm3
55% of aluminum, 1.6% of silicone and the balanced
zinc Table 2. Mechanical properties of DX51D without alloy coating.
Steel name Steel number Yield strength Tensile strength
Elongation (minimum)
DX51D 1.0917 Rp0,2 270-500 MPa 22 %
Table 3. Chemical composition of DX51D steel.
C Si Mn P S Ti
0.18 % 0.50 % 1.20 % 0.12 % 0.045 % 0.30 %
2.3 Finite element method
Finite element method or FEM is a numerical method for solving and to comprehensively understand any physical phenomenon that are described by partial differential equations (PDE), especially well suited for complicated physical problems. Typical problem areas for the method
including structural analysis, heat transfer, fluid behavior and wave propagation etc. In order to solve a problem, the finite element method subdivides a large system into smaller and simpler system that are easier to solve, the so called finite elements. This process is named discretization, see figure 4. Those finite elements are then interconnected at discrete points, so called nodal points or nodes. This result in a system of algebraic equations and are then assembled to model the entire problem. The main advantage of subdividing a large system into simpler parts are that it makes the representation of complex geometries accurate and simple representation of the total solution.
Furthermore, it is also possible to capture local effects of a geometry [Reddy 2006].
Figure 4. Discretization of a connecting rod.
2.3.1 Implicit and explicit method
There are two fundamental solving method for finite element analysis, the implicit and the explicit method. They are basically two different time integration methods. The implicit method is suitable for static, quasi-static and highly linear problems and for slow events and where the effect of strain rate is minimal. For example, at creep event. The solutions by implicit analysis is unconditionally stable thus it makes possible for larger time steps. However, when solving for dynamic and non- linear problems the implicit method will be extremely time consuming.
The explicit method is used for non-linear problems. For example, non-linear material models, large strains and high speed impact problems. The stability of the solution depends on the step time, i.e. the method is conditionally stable, thus smaller time step is required in explicit analysis.
Explicit method is therefore well suited for analysis of impact force at collision, ballistic event, contact problem and explosion analysis. In these cases, the material model, besides the stress-strain relationship, will additionally need to take account for the strain rate [Harish 2020]. See figure below for an insight of the implicit and explicit analysis applications.
Figure 5. The implicit and explicit analysis applications.
2.4 Modeling the material behavior
In general, materials that undergo dynamic loadings have complex responses. Such a problem can be broken down into three components: Equations of state (EOS), Material strength model and Material failure model. Where an equation of state provides the hydrodynamic response of material in which the material’s volumetric strength is described. Therefore, the EOS are primarily used for describing gases and liquids but also for describing solids at extremely high strain rates where the hydrodynamic pressure is much greater than the yield stress of the material. The material strength model describe the material behavior of solids subjected to stress and strains. At the beginning the solids may behave elastically, however with higher dynamic loadings, when the stress exceeds the yield stress of the material, the material deforms then plastically. This nonlinear elastic-plastic response of material is provided by this model. With even higher loadings, the material cannot longer withstand the extreme stresses and eventually fail and resulting in crushed or cracked material. The material failure model depicts exactly this kind of material response.
2.4.1 Constitutive material model
For analyzing and to predict the behavior of a structure that consists of metal sheets and undertaking dynamic forces, a material strength model and a material failure model are necessary for implementing an explicit dynamics analysis in Ansys workbench. Several alternatives of the most common used strength models for finite element modeling are supported in the software which are inbuilt in the Engineering data toolbox that can be directly applied to the system when given the necessary model parameters. One of the most widely used material strength model is the Johnson-Cook model which is a material model proposed by Johnson and Cook in 1983. The Johnson-Cook material strength model is purely empirical based and is primarily for computational use. It can describe the stress and strain relationship of metals under conditions of large deformation, high strain rate and high temperatures [Murugesan and Jung 2019]. Johnson- Cook model provides accurate results in predicting deformation profile of steels at room temperature [Banerjee 2012] and at low strain rate [Wang, Jiang and Zhang 2013].
2.4.2 Johnson-Cook strength model
The Johnson-Cook model for the von Mises flow stress/yield stress is expressed as
3 © 2017 ANSYS, Inc. April 28, 2017 ANSYS Confidential
Example Applications - Implicit & Explicit
Problem Time Magnitude
IMPLICIT METHODS
1 year 10 s 1 s 0.1 s 0.01 s 0.001 s 0.0001 s
EXPLICIT METHODS
Creep Static/Dynamic Quasi-Static Detonation
& Blast
Hypervelocity Impact Ballistics
Drop / impact
“Non-linearity”
𝜎 = [𝐴 + 𝐵 ∗ 𝜖𝑛][1 + 𝐶 ∗ 𝑙𝑛𝜖̇∗][1 − (𝑇∗)𝑚] (1)
where A, B, n, C and m are five material constants that can be obtained from tensile or compression tests of the material at elevated temperatures, by fitting the true-stress true-strain curves at different strain rates and temperatures [Zhang et al 2020]. A is the initial yield stress, B and n are the strain hardening constant and strain hardening exponent respectively, C is the strain rate constant and m is the thermal softening exponent of the material. Moreover 𝜖𝑛 is the equivalent plastic strain, 𝜖̇∗ and (𝑇∗)𝑚 are
𝜖̇∗ = 𝜖̇
𝜖̇0 , (𝑇∗)𝑚 = 𝑇 − 𝑇𝑟𝑒𝑓
𝑇𝑚− 𝑇𝑟𝑒𝑓 (2)
is the dimensionless plastic strain rate for reference strain rate 𝜖̇0 or the normalized plastic strain rate and the homologous temperature respectively [Johnson and Cook 1983]. Where T is the material temperature, Tm melting temperature of the material and Tref is the reference temperature.
The first set of brackets in equation 1 describe the effect of strain hardening and the second set represent the strain rate hardening effect and the last bracket represent the temperature softening effect. Each of them influences the flow stress, thus the union of the three components together represent the Johnson Cook material strength model.
2.4.3 Material failure model
The material behavior of knockouts during the punching process or at failure process can be said to be behaved as a ductile failure. Ductile failure is a type of failure that is characterized by large amount of plastic deformation or necking and the DX51D steel is a low carbon steel with a percent elongation (%EL) of 22 percent, where brittle failure is considered on materials to having a fracture strain of less than about 5% [William and David 2015]. There are several material failure models that are widely used and are already implemented in AWB.
The most common failure model that is being used for material failure is the plastic strain failure.
Plastic strain failure can be used to model ductile failure in materials. For a given failure criterion, i.e. a maximum equivalent plastic strain value (Eplmax), the material fails instantaneously if the material effective plastic strain exceeds the given failure criterion. The Eplmax will be the percentage of plastic strain at facture of the given material [William and David 2015].
3 IMPLEMENTATION
In this chapter the working process is described. First presents the knockout design concept and later follows design simulation performed in Ansys Workbench Explicit Dynamics.
3.1 Knockout design
3.1.1 Basic concept
The two most important requirements that needed to be fulfilled were the IP 54 and EMC-shielding demands. In order to make an electrical knockout to achieve the IP 54, i.e. protected against dust and water splashing from any direction towards the enclosure, the knockouts should be similar with the ABS electrical knockouts which meant that the design must be completely tight with no gaps existing in between. Thereby the design would unconditionally prevent water ingress and naturally achieving the EMC-shielding demand. Therefore, the very first idea was to make channels or grooves on the surface of the metal sheet however not cut it thoroughly. Instead leaving some part behind to secure the fragment piece in place. This grooving concept made it possible for later punching the fragment piece out. The very basic concept was a groove in form of a V, see the figures below.
Figure 6. V-Grooving at the surface of metal sheet.
This concept could be called one-sided V-grooving knockouts. Then the next thought followed by this was a two sided V-grooved knockout concept, see figure 8. Instead of having grooves at one side of the metal sheet, this concept utilized both sides and made grooves at front and back.
Figure 8. Two-sided V-grooving in section view.
The advantage of the second concept was the possibility to ignore the material properties brought by the coating layer of Alu-Zinc. Considering that, in this way, the coating would be removed from both sides. Otherwise that coating might slightly affect the mechanical properties of the sheets in total. Further it may at some degree avoid the chance of human injury by burrs as the burrs formation would take place at middle instead of just being exposed at the edges at the surface.
The two-sided V-grooving seemed to be the most advantageous one and therefore further design concept development would be utilizing this two-sided concept as the cornerstone.
3.1.2 Design variables
In order to be able to easily punch the metal piece or the fragment piece out from a metal sheet, the connecting area had to be thin and light. Other design objectives were to minimizing the burrs formation during the punching-out process and minimizing the amount of plastic deformation in the plate afterwards. These three were the main design objectives. Therefore, the designing phase became a parametric analysis and the goal was to investigate what affects the different parameters would influence the final design and thereby find the optimum design.
There were some design variables to be investigated. The first design variable to be thought of was the thickness of the remaining, unaffected metal sheet at grooves, see figure 9. This thickness influenced how easy it would be to knock the fragment piece and of course affected also the burrs formation. This thickness to a large extent would be determined by the machining precision.
Figure 9. The unaffected thickness.
The other designing parameters to take into account were the grooving angle and the grooving geometry. The grooving angle was simply the angle of the machining head when constructing the grooves, figure 10. Lastly, the grooving geometry was the grooving shapes that could be possible to be applied to the knockouts, see figure 11.
Figure 10. Grooving angle.
The design parameters and some of its considering values for evaluation were summarized and presented in the table below.
Table 4. The design parameters.
The unaffected thickness [mm]
Grooving angle []
Grooving geometry [-]
0.20 100 V-formed*
0.15 75 Half V-formed
0.10* 45* Asterix formed
0.05 30
0.04 10
0.03 0.02
Those marked with the * represent the standard cases. The design parameters were investigated one at a time, which meant that when there was one changing parameter under analysis the other two were held constant and the constant values for these were those marked with asterix.
3.2 Design simulation
3.2.1 Geometry modeling
3.2.1.1 Selecting the geometry
There were several cutouts on the controller cabinet that the knockouts concept needed to be implemented on. Cutouts existed both on the front side and the back side of the cabinet and existed in both rectangular shapes and circular shapes. In order to implement a knockout design concept, one of the most “severe” part was selected for analyzing the knockout concept on. See figure 12. This part was a lower plate of the controller cabinet and several rectangular cutouts could be found on this part of plate. The reason of the choice was that this part had the shortest space between cutouts which meant it would be in this place where the risk for suffering of the largest deformation during the punching-out of the knockouts. Furthermore, the rectangular shapes which consist of perpendicular edges would be harder to performing knockouts than circular ones. Therefore, if this parts manage to handle the knockouts then the rest of the parts on the controller cabinet could also be able to manage the punching out process of the knockouts.
Figure 12. The selected part from controller cabinet.
3.2.1.2 Simplification
If the whole steel plate in figure 12 was going to be analyzed in explicit dynamics the
computation time would be incredibly long and this seemed to be unnecessary and time wasting since it would be sufficient to just analyzing a convenient part of the plate and this analysis could cover for the remaining part. Hence in order to minimizing the explicit analysis computation time and for a faster processing speed, the steel plate needed to be “cut down”. And this choice should be made thoughtful with respect to how the different parts were exposed to impact force.
Thus once again, the choice was made as the worst case scenario. The cut down parts could be seen in figure 13 where the new geometry for input into AWB was the colored area.
For modeling knockout design concepts on this geometry, it was simply “refilled” with material, see figure 14.
Figure 14. The new geometry for analysis in Ansys Workbench.
3.2.1.3 Hammering tool
A hammer or a punch was needed for simulating the impact force when punching the knockouts and it was simply achieved by a cuboid that simulating such a hammering tool. The cuboid had a size of 52x140x40mm and was centered at the middle of the cutout leaving a 5mm space all- around.
Figure 15. The geometry with the hammering tool
3.2.1.4 Symmetry
An other thing that could be utilized for a faster computation speed was the possibility to utilizing symmetry. Since the entire geometry in the figure above was symmetric in two planes therefore the remaining geometry would be one forth of the previous one, see the new geometry in figure 16. This simplification would not affect the computation result but instead cut down the computation time needed and used less system resources.
Figure 16. The geometry after utilizing symmetry.
3.2.2 Material modeling
The steel plate was manufactured of the DX51D low carbon steel with bending and profiling quality. In order to start an explicit dynamics analysis and to modeling the material behavior in Ansys Workbench the material data must be input into the program as an explicit material in the Engineering data. Which meant that several material properties were needed in order to form the entire material model. Including the physical material property – density, the linear elasticity, which was derived from material’s Young’s modulus and Poisson’s ratio. Further, a material strength model – the Johnson Cook material model, and lastly a failure model – the plastic strain failure.
However, the Johnson Cook parameters for the material model were not available from any scientific literature and and was neither included in the Ansys Workbench material library.
Consequently, the material data and the JC parameters for an equivalent material was used as the input data. According to the material database Total Materia, which had the most comprehensive recourses for material properties data, that an equivalent substitute to the DX51D steel was the DC01 steel with steel number 1.0330. The DC01 steel was also a low carbon steel and had similar chemical composition as the DX51D. For comparison of the material data between these two low carbon steels can be found in appendix C.
The material data for DC01 was taken from the Total Materia database and the JC parameters was brought from a scientific research with the topic: “Sheets impact simulation for safety guards design: experiments and correlation for FE explicit models of non-alloy steel” by Landi et.al. In which the authors made and presented an improved research of JC parameters for DC01.
A [MPa] 210
B [MPa] 560.5
𝛜̇𝟎 [s-1] 0.0001
Tm [K] 1800
T0 [K] 300
n 0.488
c 0.02
m 0.7
For the hammering tool material selection, a high strength steel was to be chosen in order to be able to punch the knockouts without any significant plastic deformations. Therefore, the steel 4340 with a yield strength at 710 MPa [Total Materia 2020] was chosen. Moreover, this material was included in the Workbench material library and hence could be used directly.
3.2.3 Mesh sizing
For discretization of the geometry model, the steel plate was divided into three parts or bodies where the area nearest the grooves was applied with finer mesh. The “inner” and “outer” areas, with respect to the grooves, had somewhat larger mesh sizing since these areas were less interesting compared the grooves. See figure 17 for the mesh sizing of the geometry model. As mentioned, the most interested parts were the regions near the grooves in order to see how knockouts deformed at these regions and how burrs formation were generated. However, the remaining parts were also important for the reason to examine whether if there were any plastic deformations in the structure existing. And for the same reason, the mesh sizing of the
hammering tool was even coarser.
Figure 17. Mesh sizing of the geometry model.
3.2.4 Contact modeling
For simulating a realistic material contact for the punching process, a contact region and also a body interaction needed to be applied. With a contact in Workbench meant that the contact object could not penetrate inside the target material. The contact region for punching process was obviously the bottom of the hammering tool and the target plate and the contact type was set to
bonded. This was for simulating the contact starting at the moment of impact. For steel to mild steel (low carbon steel) contact the body interaction was set to the frictional contact type and a frictional coefficient at 0.31 was applied [Chowdhury 2016].
Figure 18. The contact region.
3.2.5 Initial conditions
First of all, due to large impact force that generates during the punching process and because of the thin thickness and narrow space between the cutouts of the steel plate, there would
unquestionably give arise to large deformations at the surrounding metals. How big the
deformations would be, whether elastic or plastic, would depend on the surrounding geometric structure. In order to prevent such unwanted deformation and likewise for the general design purpose, it was decided to utilize a physical support underneath the steel plate. Therefore, the two faces, as it shows in the figure below in purple marks, were applied for fixed support to prevent the selected geometric entities from moving.
4 RESULTS
In this chapter the results obtained with help of the implementation methods described in the previous chapter are compiled, analyzed and compared with the existing knowledge presented in the frame of reference chapter.
The main objective of performing explicit dynamics analysis was to see whether if it is possible to achieve a functional electrical knockout on a steel plate that fulfills the stated requirements. The design requirements were first of all that the knockouts must be IP 54 classed, which meant it should be able to protect against water ingress and at same time dustproof. Secondly, it should be easy to punch out the fragment pieces without any deformation occurring at the surrounding regions. Later, the burrs formation should also be minimized. To investigate what affect the design parameters would have on the knockouts, the first tool was to see the simulation. The explicit dynamics simulation gave the possibility to see the material failure with eroded elements and thus able to tell how well the entire punching process went and if there were any fragment pieces left at the edges, i.e. the burrs. Next, the equivalent plastic strain and equivalent stress were also obtained for each of the case to see whether if there were any undesired deformation existing at the surrounding metal.
4.1 Design case set 1 – the unaffected thickness
In design case set 1 the design parameter “unaffected thickness” was investigated by varying the unaffected thickness from 0.2 mm down to 0.02 mm, a total of seven different thicknesses, but the grooving geometry and grooving angle was held constant. Grooving geometry was the standard v- form and the grooving angle was held at 45 degrees.
4.1.1 “0.2 mm”
The first case in this design case set was a v-grooved knockout with a grooving angle of 45 degrees and the unaffected thickness at 0.2 mm. The first figure shows the plate after punching where the undeformed model in semitransparent view could also be viewed. As it is indicated in the figure, the punching process didn’t go well. A great portion of the surrounding metal pieces were pulled away. The second and third figure showing the equivalent stresses and the equivalent plastic strain (EPS) that the plate were subjected to. Where the equivalent plastic strain is a scalar quantity which describes the degree of work hardening in a material. The plate was subjected to a maximum equivalent stress of 480.15 MPa after punching and a maximum EPS of 0.279.
Figure 21. Equivalent stress plot of 0.2 mm case.
Figure 22. EPS plot of 0.2 mm case.
4.1.2 “0.15 mm”
Here the thickness was lowered down to 0.15 mm. The material behavior as well as the and equivalent stress and EPS was more or less same as the previous case, with a max equivalent stress of 494 MPa and a max EPS of 0.278 remained in the frame afterwards.
Figure 23. Material behavior of 0.15 mm.
Figure 24. Equivalent stress plot of 0.15 mm.
Figure 25. EPS plot of 0.15 mm.
4.1.3 “0.1 mm”
The unaffected thickness here was cut down to 0.1 mm. However, there was still large parts of metal pieces pulled away with the fragment piece. The max equivalent stress was at 490 MPa and EPS at 0.279.
Figure 27. Equivalent stress plot of 0.1 mm.
Figure 28. EPS plot of 0.1 mm.
4.1.4 “0.05 mm”
Here, the material behavior was similar to the previous cases. However, the stress distribution seemed to be more concentrated at the edges with less distribution outwards. Moreover, the maximum stress had increased to a value of 756 MPa in the steel. The equivalent plastic strain distribution remained approximately the same as previous, with a max value of 0.276.
Figure 29. Material behavior of 0.05 mm.
Figure 30. Equivalent stress plot of 0.05 mm.
Figure 31. EPS plot of 0.05 mm
4.1.5 “0.04 mm”
In this case the thickness was cut down even more, to 0.04 mm, to see whether if there would be any difference from the previous cases. Finally, the results showed some inspiring phenomenon.
From the material behavior figure, it could be noticed that the entire knockout edge was fairly nice and smooth without leaving or taking any excess metals in a big quantity. Even in a more detailed view it could be observed that there was only a limited amount of tiny particles who had a failure, causing tiny pits at the edges. In the equivalent stress plot the stress distribution was decreased and concentered at the edges of the frame. Moreover, the locations of plastic strain were considerably limited and concentrated in small amount at the edges as well.
Figure 33. Material behavior in detailed view with elements shown.
Figure 34. Equivalent stress plot of the 0.04 mm.
Figure 35. EPS plot of the 0.04 mm.
4.1.6 “0.03 mm”
The material behavior was nice and smooth as the previous case while the stress distribution was further decreased as well as the plastic strain distribution.
Figure 36. Material behavior of 0.03 mm.
Figure 37. Equivalent stress plot of 0.03 mm.
Figure 38. EPS plot of 0.03 mm.
4.1.7 “0.02 mm”
Figure 39. Material behavior of 0.02 mm thickness.
Figure 40. Equivalent stress plot of the 0.02 mm.
Figure 41. EPS plot of the 0.02 mm.
4.2 Design case set 2 – Grooving angles
In the design case set 2, the design parameter grooving angle became the changing parameter where the other two, the unaffected thickness and the grooving geometry, were held constant. The grooving geometry was still in v-form and the unaffected thickness was the standard one of 0.1 mm. The grooving angle varied from 100 degrees down to 10 degrees, including the standard one of 45 degrees, with a total of five cases.
4.2.1 “100 degrees”
The first to come was the case with 100 degrees’ grooving angle. From the figure of material behavior, it could be detected that there were lots of unevenness at the edges although no excess metal was pulled away. Further the stress distribution was concentrated at the periphery with a maximum residual stress at 495 MPa. The EPS was also gathered as a thin rim.
Figure 42. Material behavior of 0.1 mm with 100 degrees’ grooving angle.
Figure 43. Detailed material behavior with the elements shown.
Figure 44. The equivalent stress plot of the 100 degrees’ grooving angle.
Figure 45. The EPS plot of the 100 degrees’ grooving angle.
4.2.2 “75 degrees”
With decreased grooving angle till 75 degrees, the punching did not perform well. There were again big portion of excess metals being pulled away by the fragment piece. Large stress distributions all around and as well as the plastic strain.
Figure 46. Material behavior of 0.1 mm with 75 degrees’ grooving angle.
Figure 47. The equivalent stress plot of the 75 degrees’ grooving angle.
Figure 48. The EPS plot of the 75 degrees’ grooving angle.
4.2.3 “30 degrees”
In this case the grooving angle was decreased down to 30 degrees to investigate if there would be any inspiring difference, however the metals were pulled away even more and there were still large stress and plastic strain distributions all around.
Figure 49. Material behavior of 0.1 mm with 30 degrees’ grooving angle.
Figure 50. The equivalent stress plot of the 30 degrees’ grooving angle.
Figure 51. The EPS plot of the 30 degrees’ grooving angle.
4.2.4 “10 degrees”
At the last case in this design case set, the punching process of the 10 degrees’ grooving angle went surprisingly well. The edges were fairly complete compared to the previous grooving angles with only some small parts being pulled away from the edges. However, the stress distribution was still broad and as well as the plastic strain distribution. The maximum equivalent stress left in the frame was as high as 1154 MPa.
Figure 52. The material behavior of the 0.1 mm with 30 degrees’ grooving angle.
Figure 53. Detailed view of material behavior with elements shown.
Figure 54. The equivalent stress plot of the 30 degrees’ grooving angle.
Figure 55. The EPS plot of the 30 degrees’ grooving angle.
4.3 Design case set 3 – Grooving geometries
In the last design case, the grooving geometry was changed. Here the investigated grooving geometries were an asterix formed grooves and a half v-formed grooves. The unaffected thickness was held at the standard value of 0.1 mm.
Figure 56. Material behavior of the asterix formed grooves.
Figure 57. Detailed view of the material behavior.
Figure 58. The equivalent stress plot of the asterix formed grooves.
Figure 59. The EPS plot of the asterix formed grooves.
4.3.2 Half v-formed grooves
Finally, the last case was the half v-formed grooves. In this case the residual stress was extremely high with a maximum value of 2094 MPa while the stress distribution was very accumulated as well as the plastic strain. These made the material behavior at the edges being quite smooth and nice except few parts of residual metals, especially some at the corner.
Figure 60. Material behavior of the half v-formed grooves.
Figure 61. Equivalent stress plot of the half v-formed grooves.
Figure 62. EPS plot of the half v-formed grooves.
5 DISCUSSION AND CONCLUSIONS
In this chapter, the affect of the three design parameters on the knockout functionality will be discussed from the simulation results. Further the possible manufacturing methods for the knockout design will be discussed and finally the conclusions will be presented.
5.1 Discussion
5.1.1 The unaffected thickness
From the simulation results, the affect of each design parameters could be examined in detail. The first part of the investigation was the unaffected thickness. The first case in this design set was the 0.2 mm grooves. This knockout was obviously not an approved design. A large portion of excess metals were pulled away by the fragment piece during the punching process. The maximum equivalent stress that remained in the material after punching was at 480 MPa, which was above the tensile stress of 410 MPa of the steel DC01 [Appendix C]. This phenomenon was due to the work hardening that occurred in the material during plastic deformation of the plate. The break appeared at the edges of the fixed support instead of at the grooves. The reason for this was believed due to the stress that the grooves exposed to were not high enough to break the connection, instead the stress was concentrated at the edges of unmovable fixed support. Further the stress distribution spread in a great amount to the surroundings. The amount of distribution of the plastic strain was great as well. The first three cases were very similar in both stress and plastic strain distributions and the maximum values.
As the unaffected thickness decreased further, the change began to appear. In the forth case, 0.05 mm thickness, the maximum stress increased to 756 MPa while the distributions of the stress became somewhat more concentrated. Starting from the fifth case and on, the punching processes were very successful. The edges after punching were fairly nice and smooth without any excess metals being pulled away by the fragment piece. The stress distributions at the frame edges were considerably decreased and accumulated. As well as the plastic strain distribution, the locations where the plastic strain occurred were greatly limited. It could be noticed that the deeper the grooves the more the stress will be accumulated at the grooves.
The last 0.02 mm case was expected to behave as same as the previous two cases but there were actually some residual metals left at the corner. When the hammering tool hit the plate, the plate was exposed to stresses that distribute quickly to the surroundings, from the fragment piece continuing to the grooves and further. However due to the geometry, the perpendicular edge will accumulate more stress than other parts. Therefore, the corner of the fragment piece will actually
uneven. The burrs that formed here were instead caused by some excess metals from the fragment piece. The residual stresses were quite concentrated and also the plastic strain. With smaller grooving angle the punching process became worse with large amount of metals were pulled away.
Large areas of stress distribution and locations exposed to plastic strain had increased. It was the same for the remained cases except the last case with 10 degrees grooving angle. Here, different from the observed pattern, instead the most acute angle gave quite satisfying material behavior after punching. The stress distribution was fairly accumulated but much higher residual stress, with a maximum stress at 1154 MPa, and wider plastic strain area compared to 100 degrees’ case.
Further the stress had been accumulated at the screw hole as well, which was undesirable. Because of these, the 100 degrees’ grooving case seemed to be the best choice among the simulated ones for the grooving angle.
Based on the theory of stress concentration, it was believed that with a more acute grooving angle the change in the thickness would be more abrupt and therefore more stress would accumulate around the grooves. Which should lead to well performed punching process with smooth edges the more pointed the angle was. However, the simulation results contradicted this. To make sure if knockouts with larger grooving angles indeed had outstanding performance during the punching process, two extra simulations were done. One for a 125 degrees’ and the other for a 90 degrees’
case. Surprisingly, the 125 degrees one showed instead similar results as the 75 degrees’ case in stress and strain distributions, while the 90 degrees showed more or less similar results as the 100 degrees’ and with somewhat lower maximum stress. Simulation results for these two cases could be viewed in appendix D.
5.1.3 The grooving geometry
The last design parameter was the grooving geometry. The asterix grooves had great performance at the edges. Nevertheless, the residual stresses were widely distributed. Moreover, the plastic strain took place at a wide area. On the other side, the stress distribution in the half v-formed grooves case was highly limited as well as the plastic strain. The plastic strain appeared only at the utmost edges and did not grew any further. This plastic strain behavior was actually the finest among all cases. However, the maximum stress in this case was as high as 2094 MPa. Due to the same reason as the knockout with 0.02 mm grooving thickness, the corner of the fragment plate was left over. The reason to this great limitation of stress distribution might due to the geometry of the half v-grooves. The stress concentration was the accumulation of stresses in a body and occurred whenever there were irregularities or sudden change in the geometry of a body. The abrupt change in thickness of the plate in this half v-grooved knockout caused an interruption to the flow of stress and thus greatly limited and accumulated the stresses.
Figure 63. The half v-formed grooving geometry.
5.1.4 Validation
From the simulation results, there were some outstanding cases in each of the design cases. It could be seen that the grooving angles around 90-100 degrees had best performance in restricting the stress distribution. The grooving geometry of the half v-formed type was excellent in blocking stress distributions as well, further it offered very smooth edges after punching. Therefore, one new case that was inspired from these results was obtained by taking the advantageous design properties from each of the design cases. This became a knockout with halved 90 degrees’ v- grooves with 0.1 mm thickness, see figure 64. This case was then simulated to verify the previous simulation results of the three design sets.
Figure 64. Halved 90 degrees’ v-grooves.
The simulation showed astonishing results. It gave very smooth and fine edges after the punch, completely without any excess metals being pulled away or left over at the edges. The residual stress that remained in the material was among the lowest but at same time the stress distribution was fairly accumulated at the edge without spreading any further. Moreover, and the most important, there were very limited amount of plastic strain existed in the material afterwards. This design showed excellent performance which matched the earlier simulation results. The results of this case could be detailed observed in appendix E.
5.1.5 The manufacturing method
Due to the geometry of the grooves, the manufacturing methods were quite limited. To manufacture the knockout by traditional methods was confirmed with few manufacturers that their milling option was the only possible method to be able to manufacture these grooves, however the processes would be extremely time consuming and expensive due to the size and geometry and was therefore not suitable for mass production. However, there was another type of machine that was able to manufacture the grooves, the so called V-grooving machines.
The V-grooving machines was used for sheet metal grooving before bend forming for making
The v-grooving machine could handle large pieces of metal sheets [Appendix F] and had a positioning accuracy of ± 0.01 mm in z-axis, in the direction of the grooving thickness. It was believed that this type of v-grooving machines could be utilized to manufacture the knockout grooves.
5.2 Conclusions
Generally, in engineering design the stress concentration is something that engineers would like to avoid as much as possible in one’s design. However, in order to get a well performed
punching process and achieve the functionality of this type of knockout, stress concentrations are extremely desirable and important. Among all the investigated knockout designs, those who effectively restricted the stress distribution at the grooves had the best performance during punching process and also less plastic strain existed at the edges.
A new encapsulation concept that solves the stated problem is feasible and can be achieved through a knockout concept. For this particular steel plate, as in the figure 12, the best suited design will be the halved 90 degrees v-grooving that is inspired from earlier simulations. All the concepts are designed to be completely tight without any gap in between, thus they will naturally satisfy the requirements of the IP 54 standard and EMC-shielding demands.
For general design purpose, the factors for obtaining a qualified knockout are to obtain low residual stress in the material and concentrated stress and plastic strain distribution that only accumulate at the edges. According to the simulation results, the deeper the v-grooving the more restricted the stress distribution will be. A grooving angle around 90-100 degrees had great performance at stress distribution control and excellent limitation in the amount of plastic strain in the material. Later, choosing the half v-formed grooving will effectively block the flow of stress at the grooves, further it also offers very nice and smooth edges afterwards. It is believed that by gathering these factors, it will accordingly lead to a satisfied knockout design.
6 RECOMMENDATIONS AND FUTURE WORK
In this chapter, recommendations on more detailed solutions and future work are presented.
The material data used in this thesis work for simulations is the equivalent substitute DC01 steel instead of the actual steel DX51D that being used at ABB for controller cabinet. The chemical compositions and material properties of these two steel are similar but in fact some differences still existed. Therefore, it is recommended to perform own tensile tests performed under various strain rate and temperatures [Landi et.al 2017] for the DX51D+AZ150 steel to later derive own Johnson Cook strength model parameters. This will further improve the simulation results and make the results even more reliable.
In the future it would be preferable to produce physical prototypes for some of the well performed knockout concepts to enable a validation of the simulation results and evaluation of the concepts.
From manufacturing’s point of view, it would be desirable to choose a design that is most beneficial with respect to ease of production, i.e. minimizing the production time and cost.
Therefore, a design that increases the unaffected thickness thus minimizing the processing accuracy of the grooving machine is advantageous.
It might also be necessary to explore a design of one-sided knockout. Although one-sided knockouts are considered to readily give arise to sharp edges at one of the outer surface of the steel plate after punching. Thus one-sided knockout design that avoiding this phenomenon find to be extremely difficult but might be desirable.
7 REFERENCES
ANSYS INC., Explicit Dynamics, 2011.
Reddy, J. N. An Introduction to the Finite Element Method (Third ed.), McGraw-Hill, 2006.
Harish A., Implicit vs Explicit Finite Element Method (FEM): What is the Difference, 2020 March, https://www.simscale.com/blog/2019/01/implicit-vs-explicit-fem/ , Accessed May 2020.
Murugesan M. and Jung D.W., Johnson Cook Material and Failure Model Parameters
Estimation of AISI-1045 Medium Carbon Steel for Metal Forming Applications, Jeju National University Korea, 2019.
Banerjee. B., “MPM Validation: A Myriad of Taylor Impact Tests”, University of Utah USA, 2012.
Wang G., Jiang F. and Zhang L., Mechanical Behavior and Microstructure Evolution in Manufacturing Processes, Tsinghua University Beijing, 2013.
Zhang F. et al., The modified temperature term on Johnson-Cook constitutive model of AZ31 magnesium alloy with {0002} texture, Chongqing University China, 2020.
Johnson R.G. and Cook H.W., A constitutive model and data for metals subjected to large strains, high strain rates and high temperatures, USA, 1983.
William D.C. Jr. and David G.R., Materials Science and Engineering (ninth edition), John Wiley
& Sons, 2015, chap. 8.
Landi et al., Sheets impact simulation for safety guards design: experiments and correlation for FE Explicit models of non-alloy steel, University of Perugia Italy, 2017.
Ansys INC., Explicit Dynamics Analysis Guide, 2020.
Chen X.L. and Liu Y.J., Finite Element Modeling and Simulation with ANSYS Workbench, Second Edition, Taylor & Francis Group, 2019.
Lee. H,.H., Finite Element Simulations with ANSYS Workbench 16, National Cheng Kung University Taiwan, 2015.
8 FIGURE REFERENCES
The figure on the title page: https://new.abb.com/products/robotics/controllers/irc5 Figure 2: https://www.polycase.com/sk-11
Figure 3: https://www.amazon.com/BUD-Industries-JB-3956-KO-Junction- Knockout/dp/B005UP9M3G
Figure 4: https://www.simscale.com/blog/2016/10/what-is-finite-element-method/
Figure 5: Giangiacomo Lazzerini, Ansys Explicit Figure 65: https://www.krrass.com/grooving-machine/
APPENDIX A: GANTT CHART
APPENDIX B: RISK ANALYSIS
No. Possible risks Probability 1-3
Consequence 1-3
Risk
value Actions
1 To wide
assignment tasks 2 2 4 Limiting the
tasks
2
Difficulties in finding useful
literature
2 3 6
Discuss with the industrial supervisor.
3 Delay in the
time plane 2 2 4
Adjust the time plane and discuss it with the supervisor and extend the time plane if
possible.
4
Loss or damaged computer
1 3 3 Always backup
files on drive.
5
Unexpected interruption at
ABB
1 3 3
Implement the work as much as possible at home
and utilizing communication tools like Skype.
6
Design that is not manufacturable
3 3 9 Rework on the
design
7
Impossible of an IP-54 classed
electrical knockout to be
established on the current
2 3 6
Prove and discuss the reason for that and show at what
conditions could IP-54 knockouts
APPENDIX C: MATERIAL COMPARISON DC01 AND
DX51D
APPENDIX D: SIMULATION RESULTS FOR 125 AND 90 GROOVING ANGLE KNOCKOUT
125 grooving angle:
90 grooving angle:
