Finite Element Modeling and Validation of a Novel Process for Extruding. Thin Wall Hollow Copper Profiles. A thesis presented to.

Transcription

1 Finite Element Modeling and Validation of a Novel Process for Extruding Thin Wall Hollow Copper Profiles A thesis presented to the faculty of the Russ College of Engineering and Technology of Ohio University In partial fulfillment of the requirements for the degree Master of Science in Mechanical Engineering Jeffrey M. Laing March Jeffrey M. Laing. All Rights Reserved.

2 2 This thesis titled Finite Element Modeling and Validation of a Novel Process for Extruding Thin Wall Hollow Copper Profiles by JEFFREY M. LAING has been approved for the Department of Mechanical Engineering and the Russ College of Engineering and Technology of Ohio University by Frank F. Kraft Associate Professor of Mechanical Engineering Dennis Irwin Dean, Russ College of Engineering and Technology

3 3 ABSTRACT LAING, JEFFREY M., M.S., March 2012, Mechanical Engineering Finite Element Modeling and Validation of a Novel Process for Extruding Thin Wall Hollow Copper Profiles Director of Thesis: Frank F. Kraft The purpose of this research was to develop an approach to simulate a novel, high ratio extrusion process using finite element (FE) software. In order to accomplish this, several techniques were used. These include local mesh refinement, increasing the frequency of remeshing, increasing nodal relaxation and decreasing the duration of the time step. Three simulations were completed using progressively larger billets with the goal of determining the largest billet that could be extruded by a 250 kn, 400 ton or 1600 ton press. Simulation results for the 250 kn press were compared to experimental data from lab-scale testing. The extrusion force predicted was within 2% of the experimental value. Simulations of scaled-up processes, using 400 and 1600 ton presses, were compared to results of a basic extrusion-work calculation, with an uncertainty of 12%. The results of the FE analyses were within 10% of the calculated values and within the expected uncertainty. Approved: Frank F. Kraft Associate Professor of Mechanical Engineering

4 4 ACKNOWLEDGEMENTS I would like to thank the people who have contributed to this work. Of particular importance to the completion of this thesis is my advisor, Dr. Frank Kraft. I would like to thank him for his guidance as well as his technical support and depth of knowledge in the fields and mechanical engineering and manufacturing. I would also like to thank the members of my committee: Dr. Hajrudin Pasic and Dr. John Cotton from the Department of Mechanical Engineering and Dr. William Kaufman from the Mathematics Department for their feedback and contributions. I would like to thank Ohio University and the Russ College of Engineering for their support and facilities, Simufact for use of their software, Arjaan Buijk for his technical support in using the Simufact software, and The International Copper Association Ltd for their financial support. My parents have been a motivating factor in my pursuit of higher education. I would like to thank my father, David Laing, and my mother, Dr. Glynis Laing. It was their support and encouragement that made this work possible. The research in this thesis would have not been possible if it were not for the work done by previous students and researchers. I would like to thank Victor Vaitkus, Jonathan Kochis, Jared Rich and Steven Rogers for their prior work on this copper extrusion process and for providing me with experimental data and key material properties.

5 5 TABLE OF CONTENTS ABSTRACT... 3 ACKNOWLEDGEMENTS... 4 LIST OF FIGURES... 7 LIST OF TABLES... 8 CHAPTER 1: INTRODUCTION... 9 Section 1.1: Extrusion Background... 9 Section 1.2: CAD and FE Software... 9 Section 1.3: FE Formulae Section 1.4: Statement of Initial Goal Section 1.5: Benefits of CAD and FE Section 1.6: Methods of Validation Section 1.7: Current and Previous Work Section 1.8: Importance of Work CHAPTER 2: OBJECTIVES CHAPTER 3: PROCEDURE Section 3.1: Software Used Section 3.2: Running Simulations Efficiently Section 3.3: Geometry and Physical Parameters Section 3.3.1: Geometry Section 3.3.2: Process Parameters and Material Properties Section 3.4: Simulation Completion Section 3.4.1: Simufact settings Section 3.4.2: Solver Time Step Section 3.5: Finite Element Model Set-up Section 3.5.1: Small-Scale Set-up Section 3.5.2: 400 Ton Press Set-up... 55

6 6 Section 3.5.3: 1600 Ton Press Set-up Section 3.5.4: Set-up Summary Section 3.6: Data Validation Section Small Scale Billet Validation Section Ton Press Validation Section Ton Press Validation Section 3.7: Uncertainty Analysis and Data Correlation CHAPTER 4: CONCLUSION Section 4.1: Future Work CHAPTER 5: APPENDIX Section 5.1: Derivation of β Section 5.2: Form of L WORKS CITED... 85

7 7 LIST OF FIGURES Figure 1: FE Process Flow Chart Figure 2: Example of Distortion that Causes Matrix Singularity Figure 3: Element Distortion that Causes a Negative Jacobian Figure 4: Simplified Drawing of the Copper Extrusion Figure 5: Example of Extruded Heat Exchanger Tubing Figure 6: Overhead and Isometric Views of the Planes of Symmetry Figure 7: A Complete Assemly Versious a Sperated Assembly Figure 8: Solid Model of the Extrusion Die Figure 9: Zoomed in View of the Mandrel Teeth Figure 10: Physical and Virtual Extrsion Die Figure 11: Quality Facets Turned Off Versus Quality Facets Turned On Figure 12: Refinement Boxes In the Lab Scale Simulation Figure 13: Placement of Refinement Boxes in the 400 Ton Simulation Figure 14: Placement of Refinement Boxes in the 1600 Ton Simulation Figure 15: Simulation with Removed Billet Figure 16: Simulation Force Prediction for Small Scale Billet Figure 17: Experimental Data on the Lab Scale Extrusion Process Figure 18: Physical and Simulation Force vs Time Figure 19: Dimensions of the Billet Extruded with the 400 Ton Press Figure 20: A Complete Assemly Versious a Sperated Assembly Figure 21: Simulation Force Prediction for the 400 Ton Press Figure 22: Dimensions of the Billet Extruded with the 1600 Ton Press Figure 23: Simulation Force Prediction for the 1600 Ton Press Figure 24: Master Element Used to Define Shape Functions... 80

8 8 LIST OF TABLES Table 1: Thermal Conductivity and Yield Stress of Al and Cu Table 2: Values Needed to Calculate the Time Mean Average Strain Rates Table 3: Simufact Mesh Element Types Table 4: Simufact's Advanced Meshing Options Table 5: Physical and Process Parameters Table 6: Refinement Boxes for Small Billet Extrusion Simulation Table 7: Refinement Box for the 400 ton Press Simulation Table 8: Refinement Boxes for the 1600 ton Press Simulation Table 9: Differences is Simulations Table 10: Uncertainty Analysis Values... 72

9 9 CHAPTER 1: INTRODUCTION Section 1.1: Extrusion Background Extrusion is a forming process that has been used in the manufacturing of metals for over 200 years (AI-Zkeri 1999). There are several types of extrusion that include: forward, backward, hydrostatic, and impact extrusion (Kalpakjian and Schmid 2003), all of which can be performed with the work piece at elevated temperatures, known as hot extrusion, or with the work piece near room temperatures, known as cold extrusion. Simply put, forward extrusion is pushing a work piece, the billet, through a smaller opening, the die, to achieve a desired constant cross-section. A simple example of forward extrusion is pushing toothpaste out of its tube. In principal, one can push a billet (the toothpaste) through a die (the opening of the tube) to produce a constant cross-section (Robert 1990). Hot extrusion is preferred for most processes because of the reduction in the plastic flow stress of the material to be extruded; however, cold extrusion can provide a better surface finish on the final product (Hosford and Caddell 2007). Choosing which process will best fit the needs of a design is a decision made by materials processing engineers. Section 1.2: CAD and FE Software Although the process of extrusion is old, there are still many advancements to be made. Using computer-aided design (CAD) software, these advancements can be made much more quickly, with less cost, and less wasted material. Prior to the introduction of CAD software, process modeling and die design of complex profiles were performed by

10 10 highly experienced engineers who applied their knowledge of previous die designs to create new products. At that time, extrusion design was more of an art than a science. Engineers would correct the die dimensions an average of two times before it would produce the correct profile (Zhengjie 1994). With the high costs of machining and die trials, the design process would have to be streamlined to stay competitive in the marketplace. CAD and finite element (FE) software can be used to virtually model the extrusion process to avoid this unneeded machining and physical testing. FE software uses finite element analysis (FEA) to solve complex problems numerically as opposed to analytically. In general, the software solves equations over a given domain by breaking that domain into smaller, discrete elements. The smaller elements make the solution easier to converge upon because small domains often behave linearly even if the overall system behaves non-linearly (Reddy 2006). In metal forming applications, the FE software breaks the work piece into smaller elements and those elements make the calculation of stress, strain and other quantities easier to carry out. The solutions to those calculations are used to simulate the metal forming process. Using CAD and FE software to design extrusion processes has its own set of challenges to overcome. In the past, FE software had been used to model simple manufacturing processes to save the high costs of creating physical prototypes and correcting problems if they did not perform satisfactorily. Once the extrusion processes became sufficiently complex, the FE software had difficulty in performing a complete simulation. Research needed to be conducted to ensure these complex simulations

11 11 would complete successfully and to verify that these simulations provided reasonable results. Element distortion is a large factor in the inability of a process to be simulated successfully. Element distortion is caused by high strains. High strains, in numerical simulations, are typically considered to be between 1 and 3.5 (Chen 2008, Lou 2008, Son 2007). Simulations with strains at the higher end of this range are usually simple extrusion processes such as ones that produce round profiles from round billets. At high strains, elements that initially resemble cubes become distorted and look more like long, skinny cuboids or other oblong hexahedra. When the elements have large aspect ratios, the mathematical models used to quantify the state of each element break down and the algorithms cannot converge or produce unacceptable results (Lou 2008). To resolve the issues caused by large distortion, remeshing is performed on the work piece. In modern software, remeshing of the entire work piece is not necessary. Remeshing of distinct regions of interest is performed by means of refinement boxes. A refinement box is a volume fixed in space, defined by the user, in which any elements that pass into the box are remeshed with smaller and more consistent edge lengths. Refinement boxes give more accuracy and increase the chances that the numerical methods will converge on a correct solution with a minimal increase in computing time (Simufact 2010).

12 12 Section 1.3: FE Formulae The FE software used for the simulations presented herein was Simufact (Simufact Engineering, Hamburg, Germany). The software uses the updated-lagrangian method which lends itself to high deformation processes such as extrusion (Simufact Engineering 2010). The fundamental equations used in the updated-lagrangian FE process are presented in Equations 1 through 6. These equations use the displacement method. The displacement method starts by determining the distance each node moves in an iteration. The information gathered from the nodal displacements is then used to calculate quantities such as stress and strain, making them derived values. As a result of these quantities being derived, they are slightly less accurate than the values for displacement (Felippa 2004) so proper validation is important. If these nodal displacements are determined to have errors within an acceptable value, the mesh is deformed and the process is repeated until the extrusion simulation is completed. A flow chart of this process is shown in Figure 1.

13 13 Figure 1: FE Process Flow Chart (Simufact Engineering 2010) Finite element modeling is performed using an iterative process. Fundamentally, the software s mathematical solver uses Equation 1 Ku = f (1)

14 14 where K is the stiffness matrix, u is the displacement vector and f is a prescribed force vector. Equation 1 is changed to work in an iterative manner with the FE software and takes the form of Equation 2. Equation 2 is solved in Block 3 of Figure 1 and Equation 3 is used in Block 1. In Equation 2, u (i) is the displacement vector during the i th increment and δu is the change in the displacement vector that occurs during the i th increment. K(u (i) )δu = f I(u (i) ) (2) Equation 2 (Simufact 2010) relates the applied force vector, the internal body force vector and the deformation vector. The applied and internal forces are compared and the difference between the two generates deformation. The internal body force vector, known as the internal nodal-load vector, is calculated with Equation 3. I(u (i) ) = β T σ(u (i) )dv el (3) v el In Equation 3 (Simufact 2010) (Chandrupatla and Belegundu 1997), β is the straindisplacement matrix, σ is the flow stress of the material and v el is the volume of a finite element. Due to its length, the derivation of β is in the appendix of this paper. K, in Equations 2 and 4, is built using the sequence shown in Equation 4. Equation 4 is used in Block 2 of Figure 1. where K = n i=1 K el (4) i K el βt Lβdv el i = (5) v el L is the stress-strain matrix in the 3D generalized form for either the elastic or plastic region which is discussed in the appendix of this paper (Simufact 2010) (Chandrupatla

15 15 and Belegundu 1997). Equation 6 is used to estimate the displacement between increments. u (i+1) = u (i) + δu (6) Equation 2 (Simufact 2010) (Chandrupatla and Belegundu 1997) is solved for an incremental solution, δu (Simufact 2010). In this work, the software uses a frontal solver that has been adapted to take advantage of parallel processing. The adapted numerical method is known as a multifrontal sparse solver (Simufact Engineering 2010). Stress recovery techniques are then used to increase the accuracy of the results (Felippa 2004). This step is shown in Block 4 of Figure 1. At this point the software checks the residual. This is done by comparing left and right sides of Equation 2. Ideally, the left and right sides of Equation 2 would equal each other but in practice there is a slight discrepancy. This discrepancy is called the residual. The default control tolerance for the residual is 1x10-5 N. If the results yield a residual within the tolerance, the results are output; otherwise, another iteration is attempted. These steps are depicted in Block 5 and 6 in Figure 1 (Simufact 2010). The convergence of each iteration, for high deformation processes, is difficult due to the large nodal displacements. When the displacements become large or the finite elements become overly distorted, the numerical method discussed above has difficultly converging to the desired tolerances (Bauer 1993) (Simufact Engineering 2010). δu is kept as low as reasonably possible so displacements and element distortion remain manageable.

16 16 Non-convergence of the iterative process can be caused through a variety of mathematical mechanisms. During the process of numerically solving for displacements, the inverse of a particular matrix needs to be taken. If this matrix has no inverse, a so called singular matrix, the numerical method cannot be completed. Singular matrices can be caused by the elements (of a matrix) of a row or column deviating very little from each other. In FE analysis, matrix singularities occur when the nodes of a finite element lie on the same line. Examples of 2-D elements with this type of distortion are shown in Figure 2 (Reddy 2006). Figure 2: Example of Element Distortion that Causes Matrix Singularities in 2-D FE Analysis (Reddy 2006) Another common cause of non-convergence is element distortion that causes the Jacobian to become negative. The Jacobian is discussed in the appendix in Equation A.12. Two common cases in which the Jacobian becomes negative are shown in Figure 3.

17 17 (a) (b) Figure 3: Element Distortion that Causes a Negative Jacobian a) Highly Deformed Element. b) Inside Out Element (Reddy 2006) In general, these types of deformations will result in non-convergence. In some cases, constant remeshing can avoid these convergence problems. Even if convergence does occur, large element distortions should be avoided for the sake of the accuracy of the simulation. Section 1.4: Statement of Initial Goal This work focused on the finite element modeling of a lab-scale novel hot forward extrusion process to produce hollow profiles from copper alloys. The extrusion process was then modified using larger billets extruded by a 400 ton or 1600 ton press. These simulations could easily be modified to work with other engineering metals. The process being modeled involves simultaneous extrusion of two billets through a die to produce a hollow profile. A simplified isotropic view of the assembly can be seen in Figure 4.

18 18 Figure 4: Simplified Drawing of the Copper Extrusion Process (Adapted From Kraft 2010) Typical extrusion methods use the mandrel to separate a single billet into two material flows. This puts a large amount of stress on the die bridge. Using two billets eliminates adverse stresses on the extrusion die bridge that generally leads to failure during the extrusion of higher flow-stress materials like copper alloys.

19 19 Large element distortion is present in the FE model of the extrusion process presented herein. With high strains between 3.2 and 3.7 and the complex profile being extruded, successful simulation of the process is challenging. The difficulties involved in running a successful high-strain simulation needed to be dealt with by using advanced settings in the FE software. In this case, simply remeshing is not sufficient to correct for the large strains. Research needed to be conducted to determine which methods are the most effective and efficient for solving this model. Section 1.5: Benefits of CAD and FE Determining whether or not a manufacturing process will work is not the only use of FE software. It can also be used to optimize the design of dies and tooling. There are many factors that influence the efficiency of an extrusion process. These factors include but are not limited to: area reduction, die geometry, extrusion speed, lubrication, work piece material, and billet dimensions (Zhengjie 1994). CAD software allows engineers to change these different aspects of their design without the time and cost associated with retooling which may take weeks at considerable expense. The engineer could then compare the results of these designs in a fraction of the time it would take to machine new tools and run a physical experiment. Comparing the virtual models saves time, money, and still leads to the optimal design. Section 1.6: Methods of Validation While FE software is accurate for most simple models, when the design becomes complex it is more difficult to determine if the results given by the software are correct.

20 20 Simple extrusion processes, such as round to round, can be easily analyzed mathematically and with a large degree of confidence. However, when the extruded profile becomes complex, the degree of confidence in the mathematical model decreases. Because of the complex profile extruded in this work and the resulting decreased confidence in the mathematical model, experimental data generated by others during concurrent research at Ohio University was used to validate the lab-scale simulation. The knowledge obtained from the validated lab-scale simulation was combined with classical mathematical models to validate the up-scaled simulations. In this work, extrusion force data is used to validate the results of the simulation. By comparing the experimental extrusion force and the extrusion force predicted by the FE software, the validity of the FE method can be assessed. Correlation within 15% will be considered satisfactory due to uncertainty in experimental parameters such as flow stress, friction conditions, and deformation zone efficiency. In Chapter 3.7, an uncertainty analysis was performed to show this correlation was acceptable. The knowledge obtained from a validated analysis of the lab-scale process will also be applied to the design of a full-scaled operation. Historically, much of the research done on FE modeling of extrusion processes did not validate the results with experimental data. The few cases that were found, in which the authors did validate their results, produced simple profiles or had low strain (Tiernan, et al. 2005, Soury, et al. 2009). There are several classical methods in which one may mathematically analyze an extrusion process to determine the extrusion force. Upper-bound analysis, slip-line field

21 21 analysis, and the work balance model are three of them (Hosford and Caddell 2007). These methods are limited to simple geometries. Upper-bound analysis provides the highest amount of pressure needed to extrude a billet through a die. This model is not very accurate given that the actual extrusion pressure could be almost any magnitude below the upper-bound and above the ideal case. Further complicating upper-bound analysis, the engineer needs to know the flow field which is difficult to determine for detailed cross-sections, hence limiting this method to simple geometries (Hosford and Caddell 2007). Slip-line field analysis, a plane strain analysis, can be very accurate if the flow field is known. However, while analyzing complex models, a precise flow field is almost never known and is not known for this work. The work balance model can be very accurate with knowledge of the geometry of the die and some of the key physical properties of the process. The work balance is given by Equation 7: w a = w i + w f + w r (7) w a = actual work per volume needed to extrude the billet w i = ideal work per volume needed to extrude the billet w f = work per volume attributed to friction w r = redundant or non-uniform deformation work per volume Actual work per material volume equals the extrusion pressure (Hosford and Caddell 2007). The values needed to successfully calculate ideal and friction work are essentially known for this extrusion process. Redundant work is more difficult to calculate and will be found using experimental data generated by others. The work model analysis will

22 22 give a technique to analytically support the results of the FE simulation via extrusion force. Section 1.7: Current and Previous Work Currently, there is research being conducted at Ohio University on the direct hot extrusion of copper multi-channel tubing. The die and tooling used in the physical process will be virtually modeled and used to run numerical simulations. Data are generated during the physical experiments and will be used to validate the simulation in this work. Quantities that are measured during the physical extrusion are: die temperature, container temperature, extrusion force, and ram position with respect to time. Extrusion force with respect to time will be used to estimate a reasonable friction factor. The slope of the extrusion force with respect to time in steady state is the friction factor. Also, in 2008, Victor Vaitkus conducted research on copper extrusion which produced some data on material properties of copper (Vaitkus 2008). These data will allow the FE software to accurately recreate the extrusion process and also allow for validation of the numerical model. Determining strain rate sensitivity is a major factor in producing accurate results when working at elevated temperatures. In 2009, Steven Rogers finished research in which he determined the strain rate sensitivity of oxygen free-high conductivity (OFHC) copper at several elevated temperatures. He used compression testing of cylindrical billets on a servo-hydraulic MTS machine to find these values. These data were used to

23 23 accurately describe the behavior of the material s flow stress at multiple elevated temperatures for different stain rates ranging from 0.01 to 3 sec -1 (Rogers 2009). Section 1.8: Importance of Work The goal of this research is to create an efficient manufacturing process for the extrusion of copper and copper alloy billets through a die to produce profiles with multiple channels. Such profiles are shown in Figure 5. FE software will be used to develop this process. Figure 5: Example of Extruded Copper and Brass Heat Exchanger Tubes (Kraft 2010) The motivation for this work is to produce copper tubing that is currently unavailable for high efficiency heat exchangers in the heating, ventilation, air conditioning and refrigeration (HVACR) industry. Currently, such tubing for HVACR heat exchangers is only available in aluminum. Copper has a higher flow stress at higher working temperatures than aluminum which leads to challenges in manufacturing.

24 24 Copper has the advantage of being anti-microbial and anti-fungal. The antimicrobial and anti-fungal properties of copper may make it desirable for use in heat exchangers since the dissemination of those pathogens can be inhibited. About 15% of people in the Western world are affected by allergies (Skoner 2001). Major causes of allergy attacks are microbes and fungi or their by-products (Bousquet, Cauwenberge and Khaltaev 2001). Using copper as the heat exchanger in HVAC systems can reduce the clinical symptoms of these allergic reactions by reducing the allergen levels in the air (Taggart, et al. 1996). Allergy sufferers are in a niche market that may be willing to pay more for an HVAC unit that has hypoallergenic qualities if the costs are not exorbitant. Another situation in which reducing air borne pathogens is critical is in hospitals. Reducing the level of pathogens is one way to minimize the potential for infection. The thermal conductivity of copper is higher than that of aluminum. Copper s thermal conductivity coefficient is about 400 W/mK while aluminum s is just 250 W/mK (Incropera and DeWitt 1990), possibly making the heat exchanger more efficient. Also, copper is stronger than aluminum. Commercially pure copper s yield stress at room temperature is about 65 MPa (Hosseini, et al. 2009) while commercially pure aluminum s is just 25 MPa (Chinh, et al. 2005). Therefore, a smaller copper profile can support the same loads as larger aluminum one. The increased strength will allow less material to be used in the copper tubing thus saving money and weight. Also, since the copper tubing can support a higher pressure than aluminum when using the same design, the tubing can more easily support the high pressures needed for R410A

25 25 refrigerant, the preferred refrigerant for HVCA systems today (International Copper Association, Ltd. 2007). Reducing the cost of copper tubing and expanding its capabilities is important to the copper manufacturing community. Table 1 provides a summary of the material properties. Table 1: Thermal Conductivity and Yield Stress of Al and Cu Thermal Conductivity (W/mK) Yield Stress (MPa) Aluminum Copper Full-scale process development is a main goal of this work and FE analysis will be used to achieve it. Advantages of using FE analysis are the versatility of the modeling, reduced cost of testing, and reduced time in testing. Because of the flexibility of the models, many different extrusion process designs may be tested. Testing multiple process designs can allow for an efficient full-scale process to be created and validated without excessive prototyping. Using FE analysis to determine the design will reduce the time and costs associated with physically testing the proposed direct extrusion process.

26 26 CHAPTER 2: OBJECTIVES The overall objective of this research is to successfully simulate, using finite element software, the extrusion of copper billets through a die that creates a small and multi-channel profile. The analysis will be validated with experimental lab data which will be provided by others. Also, a full scale process to produce the tubing will be proposed which will be validated by mathematical means. The specific objectives are to: Model the necessary parts to run an FE analysis using CAD software o Parts include: dies, mandrels, plates, and billets Run a FE simulation matching the extrusion process used to create micro-channel copper tubing Compare the extrusion forces given by the simulation to those generated during lab-scale experiments Suggest a scaled-up process for the manufacturing of copper tubing using a 400 short (about 4,000 kn) and 1600 short ton (about 14,500 kn) press and validate it with a work balance model Optimize run parameters to reduce computational load and run time

27 27 CHAPTER 3: PROCEDURE All of the computational work was done on Ohio University s Athens campus in the mechanical engineering Computer Simulation and Design Studio. The lab is equipped with powerful computers that have eight 2.6 GHz Intel Xeon processors, 8 gigabytes of RAM, Simufact (FE software), Solid Edge ST3 (Siemens PLM, Plano, TX, USA) and are running Windows 7. Even with the high computational speed, simulations can take months to run completely so taking advantage of time reducing techniques was important in running the simulation quickly. Remeshing was done sparingly and refinement boxes, which are used to remesh locally, were used only when absolutely necessary. The time step was only shortened when needed and the complexity of the model was reduced. Trying to reduce the computational time is important for the efficiency of this process. Section 3.1: Software Used The computers in the lab have all of the sophisticated software needed to complete these simulations. The software includes Solid Edge version ST3 and Simufact version Solid Edge was used to create a three dimensional solid model of the die, containers and press. These models were then imported into Simufact. Simufact is an FE package used for metal forming simulations. Research was conducted into whether the FE software can accurately simulate the extrusion process.

28 28 Section 3.2: Running Simulations Efficiently Running simulations efficiently is a fundamental concern of using FE software. Reducing the time a simulation takes to run is beneficial because simulation and manufacturing design errors can be found quicker, more designs may be tested in the same amount of time, and computing time is not wasted. The goal of running a simulation efficiently is to reduce the amount of time it takes to obtain usable data. There are four major techniques used to reduce the amount of time the software takes to perform a complete simulation. Using the symmetry of the model is a very common method of reducing computational load and it is dictated by the geometry of the model. Also, using different meshes can save on time by decreasing the number of nodes which saves on calculations. Using multiple processors to solve models is a convenient way of reducing computational time without effecting geometry or mesh. Finally, reducing the size or complexity of the model, without sacrificing its validity, can greatly reduce computational load. Each technique reduces the computational time by different amounts and that reduction can be attributed to reducing the number of nodes or increasing the rate at which calculations proceed. One of the most commonly used techniques to reduce the time required to solve a simulation is using the symmetry of the model. Defining symmetry tells the FE software that the model is mirrored across a plane, saving the software from completing the calculations of one side and allows it to simply use the results from the other side. There are two planes of symmetry in the simulation being modeled in this work. They

29 29 are the planes that are parallel to the stroke of the press and they are illustrated in Figure 6. Symmetry Planes Figure 6: Overhead and Isometric Views of the Planes of Symmetry Used in this Simulation and as well as a Full Die Using this symmetry, the computational load is cut into one fourth of the original load, drastically reducing the time needed to run the simulation. Remeshing is another necessary part of running a successful simulation that can increase the computational load. Remeshing is needed if the initially meshed elements are too large to conform to the small details of the die. It is also needed if a higher degree of accuracy is required in specific areas of the model (Simufact 2010). For example, if knowing the stress at the die opening is more important than knowing the stress in the middle of the unformed billet, the element size near the die opening can be decreased. Element size reduction is done by inserting features in the FE software called refinement boxes. Refinement boxes locally reduce the length of the edges of the

30 30 elements that pass into them making them smaller and more uniform while keeping elements outside of the box the same. Smaller elements significantly increase the load on the computer. Each time the element s edge length is cut in half, the computational load is increased cubically. For a cubic element the load increase is given by Equation 8. N = No so s 3 (8) N = number of elements after remeshing N o = number of elements for original mesh s o = original element edge length s = new edge length If an engineer were to globally remesh a work piece with element lengths one fourth of the original, the calculations would take 64 times longer. The dramatic increase in computational load is why local refinement boxes are a more efficient option than global remeshing. Refinement boxes only refine small portions of the work piece while keeping unimportant portions at their original sizes. Simufact comes with an option to use multiple processors for its calculations. Using multiple processors significantly decreases the amount of time the computer needs to complete the simulation while keeping the computational load the same. There are two ways to use multiple cores in Simufact. One way is by using more than one processor to solve the equations developed during the FE process. In this case, the multi-frontal solver would be used. Another way to use multiple processors is to break the work piece into chucks or domains and use a single processor to solve each

31 31 domain. This method is called the domain decomposition method or DDM. The results from each domain are shared in real time with the other domains to create one cohesive simulation. The DDM requires additional software set-up which, as of December 2011, had not been completed. Therefore, the method in which multiple processors are used to solve the equations will be used. Reducing the size or complexity of a model is a useful technique if the model allows for it. In this technique, one may reduce the size of the work piece if the work per unit volume generated by the removed section of the work piece can be calculated and added to the simulation s output. In this work, the upper part of the billet in each simulation only contributes to friction work, which is known and readily calculated with Equation 9. w frb = m f σ As 3Ab (9) In Equation 9, m f is the friction factor, A s is the surface area of the part of the billet that was cut away, A b is the upset area of the billet and σ is the flow stress. Because of this, the top section of the billet may be removed as long as the friction work is calculated and added to the results of the simulations. Also, removing complex parts of a simulation and modeling them separately can speed up the rate at which usable data are generated. Each separate model can be optimized to run as quickly as possible based on its own requirements for completion. Adding the results of each separate part of the simulation together gives an estimate of the total simulation. Dividing the simulation into stages also avoids repeating results that have already been determined

32 32 in other simulations. In this work, the up-scaled simulations were split into two separate stages, called the Container Section (CS) and the Deformation Zone Section (DZS). The CS is where the up-scaled billet was placed. The DZS was the section of the die that is common to all simulations. See Figure 7 for clarification. Container Section Deformation Zone Section (a) (b) Figure 7: a) Complete Assembly and b) Separated Assembly Simulating the extrusion process in Figure 7a is mathematically equivalent to simulating both sections in Figure 7b separately and adding the work per unit volumes together. Because the work per unit volume generated by the DZS is well known, one may remove it from the up-scaled simulation as long as the equivalent work is added to the CS simulation s output (Domblesky, et al. 1997). The ram pressure can be divided into distinct additive components of extrusion work (per volume), associated with that required in the die and that required in the container. Using this technique also avoids

33 33 large amounts of element deformation which makes convergence of the simulation more likely. This procedure may be used for both the 400 ton up-scaled version as well as the 1600 ton up-scaled version. The techniques described above reduce the time needed to run a complete simulation. They reduce the time by different means, either by reducing the number of nodes or by letting the calculations proceed more quickly. Some of the techniques available to a user are determined by the geometry of the problem and some are determined by the type of system on which the simulation is running. Either way, every effort was made to perform simulations efficiently due to the large amount of calculations required to complete them. Section 3.3: Geometry and Physical Parameters Section 3.3.1: Geometry The first objective of this work was to numerically model an extrusion process that creates tubing containing multiple channels. This process was performed experimentally and the schematics of the tooling were used to create solid models. The apparatus consists of a container, a plate, a mandrel, a press, and two billets. All of these pieces were modeled in the CAD program SolidEdge and imported into Simufact for use in the simulation. Figure 8 shows a complete assembly. All parts of the apparatus were modeled as a single solid model to avoid unwanted gaps between pieces.

34 34 Mandrel Die Body Plate Figure 8: Solid Model of Assembly Used to Extrude the Copper Tubing in this Research (Vaitkus 2008) The apparatus used in early experiments had a plate to create the semi-die angle. The semi-die angle is α = 40 o. The plate had a small opening that produces the outer surface of the tubing at its exit. Protruding into the opening was the mandrel which makes the multiple-channels in the final profile of the tubing. The mandrel used in the extrusion process had small teeth to create those small channels. Those small teeth had areas between them called weld chambers which can be seen in Figure 9. The two billets flow into the weld chambers and form solid state welds where they meet. These solid state welds were at the center of the internal walls of the hollow profile. The material then flows out of the narrow portion creating the final profile.

35 35 Weld Chambers Figure 9: Zoomed in View of the Mandrel Teeth Used to Create the Interior Walls of the Tubing (Vaitkus 2008) The die body used in the extrusion process had compartments for two billets. A photo of the complete assembly is shown in Figure 10.

36 36 Billet Compartments Mandrel Bridge Die Body Plate Figure 10: Physical and Virtual: Die body, Mandrel, and Plate Used in the Extrusion Process (Vaitkus 2008) The process parameters and physical conditions needed to run simulations of the extrusion process were provided by others who were conducting concurrent research on the experimental extrusion of the same multi-channel tubing. These parameters and conditions were friction, die and work piece temperatures, and ram speed (Vaitkus 2008) (Kraft Oct, 2011). Section 3.3.2: Process Parameters and Material Properties Container friction was characterized using the extrusion data generated during physical extrusion. After initial experimental tests, the friction factor, m f, was found to be approximately 0.6 (Kraft Oct, 2011). In Simufact, there are several different ways to model friction. One may select Coulomb friction, plastic shear friction (a.k.a. sticking friction), or a combination of the two called combined friction where at low forces, coulomb friction is applied and at high forces plastic, shear forces are applied. Shear friction was used to accurately model areas of contact between the die and workpiece.

37 37 Equation 10 shows the mathematic modeling for shear friction (otherwise known as a constant interfacial shear stress). Shear Friction = m f k (10) m f = friction factor k = σ 3 (von Mises shear flow stress) σ = von Mises yield (flow) stress Flow stress is an important factor in properly modeling extrusion processes and it is dependent on temperature and strain rate. At elevated temperatures, materials behave differently than at room temperature. For example, when temperature increases, flow stress decreases for a given strain rate. Also, at elevated temperatures, a phenomenon called strain rate sensitivity is more pronounced. Strain rate sensitivity is when the flow stress of a material increases with an increase in strain rate at elevated temperatures (Hosford and Caddell 2007). This relationship is given by Equation 11: σ = C ε ms (11) σ = flow stress C = the strength constant of the material ε = strain rate ms = strain rate sensitivity The above relationship is important and Simufact has provided a way to account for it when defining the material being extruded. In this work, the material is defined manually because this particular copper alloy is not in the pre-installed materials library.

38 38 When defining the material properties, one must include both elastic and plastic coefficients. The elastic part is defined by Young s Modulus, Poisson s Ratio, and the density. The plastic part can be defined for either hot or cold extrusion. In this work, hot extrusion is modeled. For hot extrusion, Simufact gives users the ability to model strain rate dependence. The copper alloy s flow stress in this work is strain rate dependent so this relationship must be defined to accurately model the process. This dependence is modeled by Equation 11 where C = 45 MPa and m s = 0.18 at a temperature of 750 C (Rogers 2009) and because this will be treated as an isothermal model, data at one temperature will be sufficient. The strain rate ε will be determined by the extrusion rate. The ram speed is the rate at which the press moves. Different ram speeds produce different strain rates which yields different flow stresses. The time average mean strain rate can be estimated by Equation 12 (Kraft Oct, 2011). dε = ε = ln(r) dt t (12) ε = time average mean strain rate R = extrusion ratio t = time of the work piece in the deformation zone = Vz (Rv)(Ab) (13) V z = volume in deformation zone R v = Ram velocity A b = Cross sectional area of the deformed billet in the container

39 39 V z, used in Equation 13, was determined to be 6500 mm 3. Currently, a simulated ram velocity, R v, of mm/sec has been selected and the cross-sectional area of the billet, A b, is known to be 350 mm 2. The values needed to calculate flow stress for the up-scaled simulations are presented in Table 2. Table 2: Values Needed to Calculate the Time Mean Average Strain Rates Volume (mm 3 ) Ram Vel (mm/sec) Cross Section (mm 2 ) R Flow Stress (MPa) Lab-Scale 6, Ton 90, , Ton 250, , The flow stresses for the small scale simulation, 400 ton simulation and 1600 ton simulation were 24 MPa, 15 MPa and 12 MPa, respectively. Temperature is another variable that affects the flow stress of the material. There are three temperature settings in Simufact and several heat transfer coefficients. The three temperature settings are billet, die, and ambient temperatures. The heat transfer coefficients dictate the heat transfer properties between the billet and die, die and ambient, and work piece and ambient. The temperatures of all solid elements are set to 750 C o and the ambient temperature is 20 C o. During the physical extrusion experiments, it was determined that the heat generated due to billet deformation dissipated quickly and as a result could be model as an isothermal process. Because the flow stress and friction factor were both determined for 750 C o and the temperature of

40 40 the billet does not change during extrusion, the process was simulated as an isothermal system. Therefore, the temperature effects were turned off to save on computing time. Section 3.4: Simulation Completion When trying to run complex simulations such as the one in this work, simulating the process without simplifications is often challenging or takes long periods of time. Because the long term goal of this project was to determine the press size necessary to extrude larger billets, simulation completion was defined as the point at which the billet has extruded through the die and has reached its maximum extrusion force. The moment the billet leaves the die coincides with the highest extrusion force needed because this is where maximum container friction occurs. The default settings that come with the software are best suited for small deformations. Given that the simulation being attempted has high deformations, the default settings must be modified. The settings come in different categories, ranging from selecting the coordinate system to selecting how the software detects the presence of new edges. The two most important categories for the completion of this simulation are the meshing/remeshing settings and the time step used by the software to determine deformations.

41 41 Section 3.4.1: Simufact settings Tables 3 and 4 summarize the Simufact settings. The settings are then discussed in more detail immediately following the tables. Table 3: Simufact Mesh Element Types Element Shape Tetrahedral Hexahedral Variations Uses Low Deformations High Deformations High Deformations

42 42 Table 4: Simufact's Advanced Meshing Options Categories Setting Name What This Setting Does Grid Type General Edge Detection Element Size Coarsening Level Edge Tolerance Minimum Element Edge Length Edge Angle Detect New Edges Allows users to select the coordinate system to be used Manually input desired element edge length Increases the size of internal elements Defines when an edge will be detected during meshing Sets the smallest edge length that will be detected Sets the minimum angle between surfaces that will be detected Increases the number of edges detected during meshing and remeshing Quality Miscellaneous Use Contact Information Read From Previous Attempts Final Shakes Enhancement Type Gap Distance Creates new edges when the workpiece comes in contact with dies or symmetry planes Allows the software to track edges from initial meshing so they are not "lost" Number of times remeshing is attempted if not successful Allows redistribution of node Controls the size of the elements near the surface of the mesh Controls the distance between what is considered to be an inner or outer element Refinement Box Feedback Level Determines how detailed the mesher messages are Allows the user to define refinement boxes

43 43 The meshing/remeshing category has the most settings that affect the ability of the simulation to run to completion. In this category, the initial mesh of the work piece is defined and can then be refined. Starting from the initial mesh, the user may select elements of different geometric shapes. In Simufact the user may choose tetrahedral elements or hexahedral elements. The different geometric shapes have advantages and disadvantages associated with them. Hexahedral elements have the advantage of being accurate and good for large deformations so they were chosen for use in the simulations in this work. For each element type, there are also different meshers from which to choose. A mesher is an algorithm used to break the work piece into its individual mesh elements. Overlay Hex is the only mesher option for the hexahedral element type, and as such, was used in the simulations (Simufact 2010). Advanced mesh options are also available. In the Advanced Mesh Options dialog, there are six separate categories in which the user can change default settings. The default settings in these categories are used to reduce the computational load; however, they reduce the load at the expense of accuracy and stability. In simulations that are complex and have high strain, maintaining as much stability as possible is important because of the stiff nature of the equations used to solve them. Settings can be selected in the advanced mesh options that will increase accuracy and stability. In the General category of the advanced meshing options, the user sets two low level mesh parameters, Element Size and Coarsening Level. Element Size allows the user to manually input how long the edges of an element should be in the three Cartesian

44 44 directions. This setting is automatically calculated by the software based on the geometry of the work piece and is typically left alone, but may be changed if a different sized mesh is desired. The Coarsening Level is a way to reduce the computational load by reducing the number of elements in unimportant areas. Coarsening Level increases the length of the edges of the elements that are in the interior of the work piece during initial meshing. This setting is an integer and for each incremental increase, the edge lengths are doubled. For instance, if the setting is 1 then the length of the inside elements are twice that of the surface elements. If the setting is 2, the edge length would be twice that of the 1 setting so the length of the inside element s edges would be four times larger than the surface elements. For most cases, setting the coarsening level to 2 is appropriate and this is what the default setting is. Both of these settings have a large impact on how long a simulation runs because it directly affects the size of the elements in the work piece which changes the number of nodes in the mesh. Furthermore, both of these options have only a minimum impact on accuracy and stability of the simulation. These options are usually left alone except for special situations (Simufact 2010). In the Miscellaneous category, there are settings that control the distribution of the initially meshed elements. There are two settings of importance, Enhancement Type and Gap Distance. Enhancement Type defines the limit of refinement that can be applied to the base element of a mesh. Smaller elements allows for more accuracy. Gap Distance defines the size of the gap initially left between the inner elements and

45 45 the surface mesh (Simufact 2010). Setting the Gap Distance allows the mesher to be used more effectively. Verbose Level, which determines how detailed mesher messages are, is also set here. If the Verbose Level is increased, more information about the meshing process will be kept. For instance, at a level of 20 or more, data about all meshing steps will be kept as opposed to just data on the most recent meshing step. At levels above 40, edge detection data as well as tool penetration data will be kept. At the highest Verbose Level, there are 8 files that are generated for each meshing step. For simulations that involve highly complex remeshing procedures, the messages take up large amounts of memory so these settings are typically left to their low default level. The default levels only keep meshing information on the most recent meshing step (MSC Software Corporation 2005). The settings in this section are set by the software using the geometry of the model, but they can be changed if needed. One of the most important categories in the mesh settings is Edge Detection. These are settings to tell the mesher how to handle edges it encounters throughout the simulations. In a simulation such as the one performed in this work, where there are a large number of sharp edges, these settings are important. There are six settings within this category: Edge Tolerance, Minimum Element Edge Length, Edge Angle, Detect New Edges, Use Contact Information, and Read From Previous. Edge Tolerance defines when a new edge will be detected. If an edge is smooth and does not drastically affect the simulation, the user may adjust this setting to filter it out to save on computational load. Edge Tolerance values range from 0 to 1. Higher values make the software more

46 46 sensitive to edges. Minimum Edge Length is a setting in which edges that are small in length can be ignored. If an edge is small and unimportant to running a successful simulation, this setting can be changed to ignore it. In this work, due to the small size and great detail of the profile, all edges are important. Therefore this setting was kept at its default of zero. Edge Angle is another way to filter out unimportant edges. If the angle between two edges is larger than the angle set here, it is ignored. Similar to Minimum Edge Length, due to the details of the profile, all edges are important and this angle will be left at its default of radians. Detect New Edges is a way to detect new edges during the meshing process. It is a toggle on/off option; if toggled on, more edges will be detected throughout the meshing process which will improve the quality of the simulation. Also a toggle, Use Contact Information is an important setting. It is used to tell the software how to create new edges when the work piece comes in contact with the die or the planes of symmetry. Read From Previous is another important setting in the meshing options. When this toggle is selected, the edges from the initial mesh will be tracked so they are not lost. This produces a more accurate simulation. Deselecting this option produces rougher results in the initial stages of extrusion; however, the simulation tends to be more stable. For this work, Read From Previous was toggled on because simulation completion was achieved without the need for increasing stability by decreasing accuracy. These are the major meshing options and a great deal of attention was given to them in trying to achieve convergence (Simufact 2010).

47 47 Quality is another category in the advanced meshing settings. In this category the software allows the user to define what will happen if meshing is unsuccessful. If initial meshing is not successful, one option is increasing the number of attempts made at meshing the workpiece. This setting is called Attempts and was increased from 2 to 5. Another option is allowing the software to redistribute the elements to different parts of the work piece. This option is called Final Shakes and was increased from 20 to 120 and this increases redistribution. Redistribution is done by placing nodes into areas with low energy potentials (Simufact 2010). The FE Contact Table is a significant part of the simulation, particularly if the model contains planes of symmetry. In the FE Contact Table the user defines how the work piece interacts with the dies and symmetry planes in the simulation. Here one may define work piece die contact, work piece symmetry plane contact, as well as work piece work piece contact. The work piece work piece contact occurs when there is folding of the work piece on itself. For each of these contact types, one may specify whether the work piece touches or sticks to the other body. In touching contact, the elements may slide along the surface and will not be let go. In sticking contact the elements are glued to the other body preventing them from moving after contact is made (Simufact 2010). Touching contact will be selected for the symmetry plane and other contact types.

48 48 Section 3.4.2: Solver Time Step The time step of the solver is a major factor in the stability of the model. The time step is the amount of time between remeshing and can be seen as the increment loop in Figure 1. During one time step, the mesh is deformed and the software uses a numerical method to solve the elemental matrix. If the mesh is deformed too much during that time step, solving of the elemental matrix will not be successful causing the simulation to terminate. Reducing the time step will lower the amount the mesh deforms, making it more likely that the calculation will be successful. In low deformation simulations, the default time step, which automatically adapts based on how critical the step is in the simulation, will typically allow for successful completion of the simulation. Unfortunately, it will only adapt its value down to one fifth of its original size. In models with high deformations, such as the one in this work, the default time step is often too large. As a result, the mesh changes too much during that time and the subsequent calculations and remeshes are not possible. Significantly reducing the time step can help with the convergence and can eventually result in a successful simulation. Reducing the time step also increases the amount of simulation run time. Research was conducted into determining longer time step durations that still resulted in simulation competition. Section 3.5: Finite Element Model Set-up In this work, the extrusion of three progressively larger billets was simulated. The first simulation, using the smallest billet, had experimental data so that the

49 49 simulation could be validated. This validation is helpful because it is then possible to better estimate the material and friction properties so they can be applied in this and other simulations. Each of the three simulations needs to be set-up differently to run successfully. In Simufact, setting up a simulation involves six main steps. They are manufacturing simulation selection, importing geometry, in putting physical parameters, miscellaneous parameters, solution settings, and mesh refinement. Each step is equally important to running a complete simulation. However, solution settings and mesh refinement contribute most to minimizing element deformation. Element deformation is the main cause of non-convergence in these simulations and needs to be addressed to run a successful simulation. The steps are detailed below for each of the three simulations performed during this work. Section 3.5.1: Small-Scale Set-up The initial step, manufacturing simulation selection, is the same for all three simulations in this work. The simulation is defined as a hot working, forward extrusion, three-dimensional, finite element problem. These options are selected upon opening a new simulation and need to be selected before any other parameters are configured. The default 3D, forward, hot, finite element extrusion simulation model has three objects that must have their geometries imported. This is performed during the importing geometry step. The objects that must be imported to complete a forward extrusion simulation are the upper die (press-driven die), the lower die (die) and the

50 50 work piece (billet). Each of these objects have been modeled in SolidEdge and saved as.igs files. The.IGS files are imported into Simufact through the CAD preview feature. In the CAD Preview feature the user can adjust the accuracy of the imported model two ways. First, the user can turn on Quality facets which increases the number of elements used to create the geometry of the objects. Second, Facet sag length can be reduced which decreases the size of the elements used to define the geometry of the imported model (Simufact Engineering 2010). Figure 11 shows that results of turning on Quality facets and decreasing Facet sag. (a) (b) Figure 11: a) Quality Facets turned off. b) Quality Facets turned on and Facet sag reduced. (Simufact Engineering 2010) Due to the detailed geometry of the die, the default parameters need to be modified to accurately define the geometry and prevent holes from being formed. In this work, Quality facets were turned on and the Facet sag was decreased from 0.05 mm to 0.01

51 51 mm. Changing these parameters allows the software to accurately define the geometry of the simulation. The next step in setting up a finite element simulation is defining the physical and process parameters. Experimental data were used to accurately define friction, temperature, press position with respect to time, and material properties such as flow stress and strain-rate sensitivity. The friction condition between the die and the billet is a constant interfacial shear stress with a friction factor of 0.6. Interfacial shear friction is a basic option in Simufact and the only data needed to define it is the friction factor. The temperature in this simulation was defined as constant at 750 C to match the approximation in the physical experiments. The speed of the ram was set to mm/sec. This dictates the strain rate and is consistent with the experimental data. Next, the material was defined. The copper exhibits strain-rate sensitivity at elevated temperatures and this was taken into consideration. In the materials feature of Simufact, the user may define strain rate sensitivity using the hot forging material form 2 format. Hot forging material form 2 uses the equation σ = 45 ε 0.18 to define the material s flow stress. The coefficients needed to properly define this form are well known due to concurrent research and are discussed in the Chapter The user also defines the minimum yield stress (MYS) which tells the software to start using the plastic stress equations. The MYS was set to 10 MPa. Ideally, the MYS would be set close to zero but it was increased to 10 MPa to save on computational load. These

52 physical and process parameters cannot change to help convergence because they are set by the physical experiment and are summarized below in Table Table 5: Physical and Process Parameters Property Type Value Friction Sticking m f = 0.6 Temperature Isothermal 750 C Strain Rate Sensitivity Form 2 σ = 45 ε 0.18 MPa Min Yield Stress Von Mises 10 MPa Typically, the solution settings are set next. During this step the user defines data output options as well as settings for the solver. The output options determine which data will be generated and how often. For instance, grain size and die wear can be included as outputs if some information is known about the material and die. Also, the user may set how often data is output. Recording data more often results in simulations taking up more disk space but the results are more detailed. The default data output was kept and the data output rate was set to output data every 0.1% of the total simulation. The solver settings are: numerical solver type, parallel processing or not, DDM or not, and time step. Different solvers have advantages and disadvantages that must be considered when selecting them. After weighing the options, a multifrontal solver was selected because of the parallel processing capabilities and reduction

53 53 of disk space needed. The DDM was not selected because of problems with the software that may be corrected in future releases. The time step was reduced to decrease the element deformation during an increment. The time step was changed to an adaptive time step based on displacement changes with a maximum displacement of mm, which is one half of the edge length of the smallest element. This changes the time step to whatever amount of time would be needed to cause a displacement of mm at any node during an increment. The solver and the time step have a large impact on convergence, simulation completion, disk space usage and computational time. Therefore, careful consideration must be used when defining these settings. The mesh settings are also very important to convergence and running a complete simulation. The meshing/remeshing process has several ways it may be modified to more reliably achieve convergence. One way is to increase the persistence of the mesher at each remeshing step. This is performed by increasing the number of remeshes attempted if a valid mesh could not be initially created. In this work the number of remesh attempts was increased from 3 to 5. Another way to increase the possibility of convergence is increasing the grade of the mesh by increasing the number of shakes. This increases nodal relaxation. In this work, the number of shakes was increased from 20 to 120. A third way of increasing the likelihood of convergence is inserting refinement boxes. Four boxes were defined for the small scale simulation. Table 6 lists the details of each refinement box.

54 54 Table 6: Refinement Boxes for Small Billet Extrusion Simulation Level X-Min X-Max Y-Min Y-Max Z-Min Z-Max Box Box Box Box Figure 12 shows the placement of the refinement boxes. Figure 12: Refinement Boxes In the Lab Scale Simulation These settings and parameters help insure that the mesh will be accurate and this increases the chances of iteration convergence during simulations. The miscellaneous parameters section includes settings such as symmetry and FE contact table. These settings are important but do not fall into any of the categories listed above. The symmetry planes were defined as the planes parallel to the press stroke shown in Figure 6. After the symmetry planes were defined, the FE contact table was defined. The FE contact table tells the software how to handle a situation in which

55 55 one body comes into contact with another body or symmetry plane. For instance, if a node comes into contact with a symmetry plane, the node can either stick to the plane or it can slide along the plane. The contact condition touching was selected in the FE contact table for all contact because it fits the physical conditions well. In touching contact, the nodes slide along a surface rather than sticking. With the definition of these last settings and parameters, the small-scale simulation was ready to be performed. Section 3.5.2: 400 Ton Press Set-up The 400 ton press simulation had all of the same 6 steps as the small scale simulation. Many of the settings were the same and are not repeated in this section. The manufacturing simulation selection, importing geometry, miscellaneous parameters and inputting physical parameters were exactly the same except for the geometry of the imported parts and the press speed. The solution settings and mesh refinement steps were numerically different but use the same concepts. These differences are detailed below. In the inputting physical parameters step, everything is exactly the same except for the press speed. Press speed, in the 400 ton press simulation, was calculated so that material in the DZS of both the small scale and 400 ton simulations would move at the same rate of speed. This ensures that the work per unit volume in each DZS is equal and will be additive. Because the work per unit volume is additive, the parts of the extrusion process common to each simulation were not repeated. The press speed for the 400

56 56 ton press simulation that created the proper speed in the DZS was 0.01 mm/sec. All other settings and properties in the in-putting physical parameters section were the same as the small-scale simulation. Solution settings for the 400 ton press simulation were slightly different. The solver type, parallel processing and DDM were the same. However, the time step was different. The first stage of the 400 ton press simulation is a rather simple extrusion simulation. The reduction ratio in the first stage was 16. Considering this lower reduction ration and the fact that the first stage does not produce a detailed or complex profile, this part of the simulation is easy to simulate. Simple extrusion processes typically can be modeled with the default time step which was done in this work. The time step was left in its default state, a fixed time step that is automatically calculated by the software. The software typically uses a time step that breaks the simulation into 100 to 200 time steps. The default time step was adequate for simulation completion of the first stage of the 400 ton press. The mesh settings for the first stage of the 400 ton press were the same as the small scale simulation except for the refinement boxes. Meshing for the 400 ton simulation is relatively simple so fewer refinement boxes were needed when compared to the small scale simulation. The attempts and shakes settings were kept at their increased 5 and 120 levels, respectively. The details of the refinement box are given in Table 7. Only one refinement box was required.

57 57 Table 7: Refinement Box for the 400 ton Press Simulation Level X-Min X-Max Y-Min Y-Max Z-Min Z-Max Box Figure 13 shows the placement of the refinement boxes. Figure 13: Placement of Refinement Boxes in the 400 Ton Simulation The first stage of the 400 ton simulation was relatively simple for the mesher and solver to handle when compared to the small scale and 1600 ton simulations. The 400 ton simulation had the lowest reduction ratio and a non-detailed final profile. Due to this, there was no need for much change to the default settings. After the above changes were made and parameters set, the simulation was ready to run to completion. Section 3.5.3: 1600 Ton Press Set-up The first stage of the 1600 ton press simulation had all 6 steps. Again, the manufacturing simulation selection, importing geometry, miscellaneous parameters and in putting physical parameters were exactly the same except for press speed and the

58 58 geometries of the models that are imported. The solution settings and the mesh settings were different but used the same concepts. This simulation was more difficult for the mesher than the 400 ton press simulation but not as difficult as the small-scale simulation. The entire in putting physical parameters step is the same except for the press speed. Press speed, in the 1600 ton press simulation, was calculated so that material in the DZS of both the small scale and 1600 ton simulations would move at the same rate of speed. If the material travels through the DZS of both simulations at the same rate, and because deformation work is additive, the need to model the DZS in the 1600 ton simulation was eliminated. Eliminating the DZS avoids large element deformation and reduces the number of nodes. The press speed that produced the same material flow rate through the DZS of the 1600 ton simulation as the DZS of the small scale simulation was calculated to be mm/sec. Keeping all of the other physical properties the same, such as material flow stress and stain rate sensitivity, the simulation set-up was able to continue to the next step. The solution settings for the 1600 ton press were closer to the settings for the small scale simulation than that of the 400 press simulation. The solver settings were the same; however, the time step used for that solver needed to be reduced below the small scale simulation level. The time step was set to an adaptive time step based on displacement changes and a maximum displacement of 0.02 mm, about four fifths of

59 59 the time step used in the small scale simulation. With the small duration of the time step, the simulation proceeded slowly so it was not run to completion. The meshing step is slightly different as well. Given the large reduction ratio between the first stage and the DZS, the remeshing and convergence is difficult. The settings that increase the quality of the mesh are kept at the higher levels. Attempts and shakes are 5 and 120, respectively. Also, more refinement boxes were needed compared to the 400 ton simulation. The details of these boxes are given in Table 8. Table 8: Refinement Boxes for the 1600 ton Press Simulation Level X-Min X-Max Y-Min Y-Max Z-Min Z-Max Box Box Box Figure 14 shows the placement of the refinement boxes. Figure 14: Placement of Refinement Boxes in the 1600 Ton Simulation

60 60 The 1600 ton simulation was more difficult than expected but it ran successfully. Because of the large amounts of refinement and small time step, this simulation proceeded slowly and required much more disk space than the 400 ton press simulation despite appearing to be very similar. With the above settings, the first stage of the 1600 ton press ran to completion. Section 3.5.4: Set-up Summary In summation, each of the three simulations needed to be set-up slightly differently to successfully. The differences in each simulation are listed in Table 9. Table 9: Differences is Simulations Press Speed Simulation Geometry [mm/sec] Levels of Refinement Attempts/ Time Step Shakes Displacement: mm 5/120 Lab-Scale Standard Die Larger Container 400 Ton and Same Die Auto 5/120 Largest Container Displacement: 1600 Ton and Same Die mm 5/120 Section 3.6: Data Validation In finite element analysis, simulation validation is important. From a user s perspective, FE software is typically seen as a black box. An engineer inputs data and an answer is generated. The answer should be checked for validity with as many methods as possible. Experimental validation is ideal; however, mathematical validation is a method that can also be used as an effective approach. Experimental validation is not typically standard because FE simulations are usually performed in the developmental

61 61 stage, but because of the nature of this research, experimental data is available for the small scale extrusion process. Experimental data were generated by Jonathan Kochis and Jared Rich during concurrent research at Ohio University. Once validation with the small-scale billet was achieved, the simulation was compared to a classical mathematical model. Then, a similar mathematical model was used to validate the upscaled simulations. Section Small Scale Billet Validation First, the small scale billet simulation was validated with experimental data. The small scale billet had a length of 100 mm, an upset surface area of 350 mm 2 (within the container) and a circumference of 41 mm. In the small scale simulation, the upper 90 mm of the billet was removed as can be seen in Figure 15. (a) (b) Figure 15: a) Simulation with No Billet Removed b) Simulation with Upper Part of Billet Removed

62 62 The upper part of the billet was removed to reduce the number of nodes per the discussion in Chapter 3.2. The upper part of the billet only contributes a frictional force. That frictional force was calculated and added to the results of the reduced simulation and then compared to the experimental results. The frictional force, F fric, generated by the removed part of the billet was calculated by Equation 14. σ As F fric = Ab m f (14) 3Ab where m f is the friction factor, A s is the surface area of the part of the billet that was cut away, A b is the upset area of the billet and σ is the flow stress. It was calculated that the missing part of the billet would contribute 66 kn to the extrusion force at the start of extrusion. The simulation, with reduced billet length, predicts a total extrusion force of 37 kn for one quarter of the two billets or one half of one billet as can be seen in Figure 16.

63 63 Figure 16: Simulation Prediction for Extrusion Force Needed to Extrude One Half of One Small Scale Billet Combining the calculated frictional force and the software s reduced billet force, the total predicted extrusion force equals 214 kn. When compared to the extrusion force measured during the lab scale experiments, the two match well. Figure 17 shows the experimental data for one such extrusion run.

64 64 Ram Speed (mm/min) Ram Force Ram Speed Ram Position (mm) Die set temp.= 762 o C Die entrance temp.= 727 o C Container set temp. = 755 o C Container temp. = 734 o C Force (kn) Time (min) 100 Figure 17: Experimental Data on the Lab Scale Extrusion Process Showing Ram Force and Ram Speed (Kraft Oct, 2011) The experimental data shows a maximum extrusion force of 218 kn. The discrepancy is about 2% which may be attributed to a slightly lower temperature in the extrusion trial. This discrepancy is within the envelope that was defined as appropriate for validation. The shape of the graph of force versus time can also be compared for the smallscale extrusion process. In Figure 18, the force versus time curves generated during the physical extrusion and the simulation were superimposed on one another. The slope of the curve leading up to the maximum extrusion force, the shape at maximum extrusion force and the small bit after the maximum extrusion force match quite well.

65 65 Figure 18: Physical and Simulation Force vs Time Graphs Superimposed on One Another The simulation was also compared to a work balance mathematical model to build confidence in the mathematical model s ability to accurately model the extrusion process. The mathematical model matches the experimental data nearly perfectly as it was formulated to do so. The formula is given below in Equation 15: F ex = Ab σ ln(r) η + m f As 3Ab (15) m f is the friction factor, R is the extrusion ratio and η is the deformation zone efficiency which allows ideal, friction and redundant work to be lumped into one term. The first term in Equation 15, σ ln(r) η, is the work (per unit volume) required to pass material

66 66 through the deformation zone of the die and encompasses ideal, friction and non- σ As uniform deformations. The second term, m f, is the friction work developed in the billet container. Both terms are added together and multiplied by Ab to obtain the total extrusion force. In the small scale simulation R = 25 and η = (Kraft Oct, 2011). The values of m f and η were determined explicitly from the experimental data. Because the mathematical model was formulated to match the experimental data, the mathematical model and simulation s predictions match within the same 2% as above. The simulation for the small scale extrusion process has been validated using experimental data. The extrusion process s simulation prediction and experimental data correlate within the 15% determined to be acceptable for validation during the research proposal. The knowledge gained from the validated small scale simulation will be applied in the validation of both up-scaled models. The discrepancy of 2% will be discussed in Chapter 3.7. Section Ton Press Validation Validation of the 400 ton press simulation was done by comparing the results of the simulation to a mathematical model. There were three parts that needed to be calculated to mathematically model the extrusion process. They were the work attributed to friction, non-uniform deformation and ideal deformation. Friction, nonuniform and ideal deformations inside of the deformation zone of the container were lumped together by using the CS deformation zone efficiency. The deformation zone efficiency in the container (to the die entrance) was not known but, when no 3Ab

67 67 experimental data is available, one may estimate a deformation zone efficiency of 0.55 for calculations (Siegert, Bauser and Sauer 2006). The CS deformation zone efficiency should not be confused with the DZS deformation zone efficiency. The calculations were carried out using Equation 15 for the billet shown in Figure 19. The billet had a length of 440 mm. Figure 19: Dimensions of the Billet Extruded with the 400 Ton Press in millimeters Upon completing the calculations, the mathematical model predicts a maximum extrusion force of 3,900 kn. This maximum extrusion force will be used to validate the 400 ton simulation. The 400 ton simulation was modeled in stages. The first stage involved the extrusion of the larger billet section to the smaller die opening. The second stage was the extrusion of the small billet through the die in the small scale simulation. See Figure 20 for clarification.

68 68 (a) (b) Figure 20: a) Shows a Total Simulation. b) Shows a Mathematically Equivalent Simulation Broken Into Two Parts. One may add the values of the first and second stage together to predict the work per unit volume required to extrude the billet through the entire die in one pass. Using this method of simulating the total extrusion process is beneficial because it avoids large element deformations as well as avoids duplicating parts of the simulation that were already completed (Domblesky, et al. 1997). The upper part of the large billet was also removed to save on computational load. The removed part of the billet only contributed to frictional work. The amount of frictional work that would have been generated by the missing part of the billet was calculated by dividing Equation 14 by the cross-sectional area of the large billet, Ab. The value of the maximum frictional work developed by the missing part of the billet was 140 N/m 2. The maximum extrusion force to extrude the reduced billet through the first stage was 940 kn as can been seen in

69 Figure 21. This is divided by the cross-sectional area of the billet, Ab, to give a work per unit volume of 150 N/mm y-intercept Line Fit Curve Simulation Data Figure 21: Simulation Prediction for Extrusion Force Needed to Extrude One Half of One 400 Ton Billet The maximum extrusion work developed in the DZS was 400 N/mm 2. These amounts were added and multiplied by the cross-sectional area of the billet, Ab, to determine the force needed to extrude the large billet. After compensating for the reduced simulation as well as the reduced size of the billet, the simulation predicted a maximum extrusion force of 4,300 kn. Upon comparing the simulation s predictions with the mathematical model, the results of both models correlate well. The software predicted a maximum extrusion

70 70 force of 4,300 kn and the mathematical model predicted a maximum extrusion force of 3,900 kn. This gives a difference of 9%, which is within the established envelope. Possible reasons for the discrepancies between the simulation and mathematical models are discussed in the Chapter 3.7. Section Ton Press Validation The last simulation to be validated is one in which a 1600 ton press is used to extrude a larger billet through the same die. The validation was performed in the same manner as the 400 ton press. The 1600 ton press is capable of extruding a billet with dimension shown in Figure 22 and a length of 780 mm Figure 22: Dimensions of the Billet Extruded with the 1600 Ton Press in millimeters The simulation was performed with a shorter billet and the results were modified to account for the missing billet as well as the missing DZS. The results were then compared to the classical mathematical model. The software predicted an extrusion

71 71 force of 1,050 kn for ¼ of the reduced billet with no common DZS as can be seen in Figure 23. Y-intercept Line Fit Curve Simulation Data Figure 23: Simulation Prediction for Extrusion Force Needed to Extrude One Half of One Billet for the 1600 Ton Press The results of the simulation were then modified to account for the missing length and missing DZS which increased the total extrusion force to 14,000 kn. The mathematical model, using an CS deformation zone efficiency of 0.55, predicted a value of 13,000 kn. Upon comparison of the modified results to the mathematical model, the percent difference was found to be 10%, within the established envelope of discrepancy. Section 3.7: Uncertainty Analysis and Data Correlation To address the accuracy of the models used to create the simulations presented herein, an uncertainty analysis was conducted. The method used to perform the

72 72 uncertainty analysis was the Kline and McClintock method (Holman 2001). It is based on the uncertainty inherent in determining the various experimental parameters used to define the simulations. The uncertainty analysis was performed using the extrusion force equation as its basis. Extrusion force uncertainty is a function of three main variables and their uncertainties; the flow stress (σ), the deformation efficiency (η) and the friction factor (m f ). Extrusion force uncertainty is dependent on additional variables, but their uncertainties were considered negligible. The uncertainty of the extrusion force, ω Fex, is given in Equation 16. ω Fex = Fex σ ω σ 2 + Fex η ω η 2 + Fex m f ω mf 2 (16) In Equation 16, ω σ, ω η and ω mf are the uncertainty of flow stress, deformation zone efficiency and friction factor, respectively. The values assigned to them are ±3 MPa, ±0.02 and ±0.05, respectively for the small scale simulation. The values of all three uncertainty analyses are presented in Table 10. Table 10: Uncertainty Analysis Values Flow Flow Stress Stress Uncertainty Efficiency Efficiency Uncertainty Friction Factor Factor Uncertainty Lab Scale 25 MPa ±3 MPa ± ± Ton 16 MPa ±1.9 MPa 0.55 ± ± Ton 13 MPa ±1.5 MPa 0.55 ± ±0.05 The relative uncertainty is then calculated with Equation 17.

73 73 relative uncertainty = ω F ex F ex 100 (17) It was determined the relative uncertainties for the lab-scale simulation, the 400 ton simulation and the 1600 ton simulation were 11%, 12% and 12%, respectively. This is within the 15% difference originally determined to be sufficient in an acceptable simulation. The purpose of this analysis was to determine a reasonable uncertainty of the extrusion force calculated with Equation 15, such that correlations with the finite element modeling can be made. The extrusion force discrepancy between the lab-scale simulation and the experimental data was 2%. The relative uncertainty using Equation 15 was 11%. For the 400 ton and 1600 ton simulations, the discrepancies with Equation 15 were 9 and 10%, respectively. This is within the 12% relative uncertainties calculated with Equations

74 74 CHAPTER 4: CONCLUSION The primary goal of this research was to develop an approach to model and analyze a new copper extrusion process using the finite element method. Objectives also included creating 3D models of the parts needed to perform the FE simulations, simulating up-scaled versions of the extrusion process driven by a 400 ton and 1600 ton press, and validating the simulations by experimental and/or mathematical means. The simulations were also to be optimized to run in a shorter amount of time. This work was completed during the course of the research. To achieve the objectives in this research, specialized software was used. 3D modeling of the parts needed to perform the simulations were created in SolidEdge. The simulations were carried out in the FE software package called Simufact Simufact allowed for control over the necessary parameters to successfully perform the required simulations. Given the high strains and large element deformation present in the simulations, techniques were used and parameters were set to ensure the stability of the simulations. The most important parameter was the time step. It was changed to an adaptive time step based on the amount of time needed to displace a node, during any increment, a distance of mm for the small scale as well as the 400 ton simulations and 0.02 mm for the 1600 ton simulation. Remeshing parameters were also changed to increase the chances of success. Shakes were increased from 20 to 120 and remeshing attempts were increased from 3 to 5. To achieve the detail required in these

75 75 simulations, refinement boxes were inserted to reduce the size of the finite elements. The small scale simulation required 3 levels of refinement, the 400 ton simulation required 1 level and the 1600 ton simulation also required 3 levels. To reduce the element deformation during the up-scaled simulations, a technique was used that separated the simulations into two stages. The first stage simulated the extrusion of the up-scaled billet into the deformation zone section leading up to the die, and then the second stage simulated the billet being extruded through the die s deformation zone. These parameter settings and techniques were necessary for the successful completion of the simulations. The results of the simulations matched the experimental data well. The small scale finite element model was able to predict the extrusion force within 2% of the experimental data. The up-scaled simulations were validated using an extrusion work based analysis. The simulations of the 400 and 1600 ton extrusion processes were within 9 and 10% of the analytical model, and these values were within the 12% relative uncertainty of using that model. The discrepancies are attributed to the experimental uncertainty of the friction factor, deformation zone efficiency and flow stress (which is related to temperature and strain rate). Section 4.1: Future Work In finite element analysis, simulation accuracy and run time are areas that are continually improved. Simulation accuracy is the most important and should be improved at the expense of run time but, when the simulation becomes accurate,

76 76 reducing run time should then become the focus. As for using FE software to improve the actual extrusion process, the extrusion process s efficiency may be increased by researching different die designs without prototyping. These are the areas where there is still room for large scale advancements. Improving accuracy in FE simulations should always be a goal. Unfortunately, higher accuracy often comes with longer run times. Most advancements in accuracy that increase run time are associated with the numerical method or the mesh. Numerical methods, in FE simulation, are solved to convergence within a desired tolerance. Reducing the tolerance for convergence in the numerical method will result in higher accuracy but could result in impractically long run times. One may also improve accuracy by including all parts of the simulation. In this work, the upper parts of the billet, as well as the DZS of the up-scaled simulations were removed. Including these sections would increase accuracy but would cause extremely long run times. Also, increasing the quality of the mesh can increase accuracy but can also increases runtime. The reason these areas were not explored was they would create impractically long run times and without them valid simulations could still be performed. There are ways to reduce the run time of a simulation which can be researched in future work. Running the simulation on more processors is an easy way to increase speed but requires more licenses. Also, properly setting up the domain decomposition method (DDM) on the computers in the lab would be helpful in decreasing time. There are ways of decreasing the number of elements in each simulation. By further

77 77 increasing the size of elements near unimportant areas one many decrease the number of nodes and reduce the time needed to carry out calculations. Also, increasing the duration of the time step to its longest duration that assures convergence would decrease the time needed for a simulation to run. There is another symmetry technique that may be taken advantage of, periodic symmetry. Using periodic symmetry one may model an individual multi-channel as well as the end channel and extrapolated what the total extrusion force would be. These techniques would decrease the run time of simulations but, in some cases, would also decrease accuracy and stability. Ideally, these techniques and parameters would be combined to complete a simulation in a few days or less. There are ways that the extrusion process may be improved using the finite element process as well. Die design is an interesting process that is difficult to break down mathematically. Now that this simulation is possible, one may analyze the material flow to design a die that allows the metal to move more easily. Analysis of the die can include whether the tubing would extrude properly or other utilities that make have required physical testing in the past. Simulations can be performed to look at material flow inside of the billet without prototyping. Also, die stresses can be analyzed. Now, possible die designs can be simulated analyzed in days instead of prototyping and testing over weeks. Along the same line, different shapes and sizes of billets may be analyzed without the need for prototyping. Another interesting aspect of FE simulations is the ability to look inside of the die and billet during extrusion. This allows the

78 78 engineer to analyze material flow, strain rates, stresses and many more variables in an extrusion process. Being able to look at these quantities inside of the process will yield insights that would have otherwise gone unnoticed. Process improvements are likely and much more possible with a process for FE modeling.

79 79 CHAPTER 5: APPENDIX Section 5.1: Derivation of β The variables u, v and w will be defined as the x, y and z components of u, such that the displacement vector would be u = [u, v, w] T. β is a matrix used to define the relationship between strain and displacement in the plastic region. It is needed for the calculation of the internal node-load vector as well as the stiffness matrix, Equations 3 and 5 respectively. β will be defined for a four node tetrahedral element for simplicity. Linear shape functions will also be assumed. The strain tensor is known to be. ε = u x, v y, w z, v + w, z y u + w, z x u + v y x T (A.1) (Chandrupatla and Belegundu 1997) Each of the 4 nodes has three degrees of freedom. One may describe the displacement of each of the 4 nodes using the element displacement vector shown below: q = [q 1, q 2, q 3,, q 12 ] T (A.2) (Chandrupatla and Belegundu 1997) By defining four shape functions N 1, N 2, N 3 and N 4 one can better describe the geometry of each finite element and can linearly interpolate the displacement field within each element. (Chandrupatla and Belegundu 1997)

80 80 Figure 24: Master Element Used to Define Shape Functions (Chandrupatla and Belegundu 1997) With these shape functions defined, the displacement field inside of an element can be defined by A.3 which is dependent upon the shape functions. u = Nq (A.3) N N N N where N = 0 N N N N 4 0 (A.4) 0 0 N N N N 4 (Chandrupatla and Belegundu 1997) Equation A.3 yields the following equations which are used to define the coordinates of a point, inside of an element, displaced a distance u, v and w from its original position.

81 81 x = x 4 +x 14 ξ+x 24 μ+x 34 ζ y = y 4 +y 14 ξ+y 24 μ+y 34 ζ (A.5) z = z 4 +z 14 ξ+z 24 μ+z 34 ζ where x jk = x j -x k and similarly for y and z. (Chandrupatla and Belegundu 1997). Transformation from the ξ, μ, and ζ coordinate system to the x, y, and z coordinate system is performed using the transformation below. It is derived from the equations in A.5. First, convert the displacement in the x direction called u. It is shown that u is a function ξ, μ, and ζ u = u(x(ξ, μ, ζ), y(ξ, μ, ζ), z(ξ, μ, ζ)) (A.6) (Chandrupatla and Belegundu 1997) Taking the partial derivatives of u, it is found that. u = u x + u y + u z ξ x ξ y ξ z ξ u = u x + u y + u z µ x µ y µ z µ (A.7) u = u x + u y + u z ζ x ζ y ζ z ζ (Reddy 2006) (Chandrupatla and Belegundu 1997) A convenient way of writing these equations would be u ξ u = µ u ζ x ξ x µ x ζ y ξ y µ y ζ z ξ z µ z ζ u x u y u z (A.8)

82 82 (Chandrupatla and Belegundu 1997) The derivation for A.8 would then be carried out starting from A.6 for v and w. Note that the (3X3) matrix in A.8 is a transformation matrix, J, and does not change for the derivation with v and w. J = x ξ x µ x ζ y ξ y µ y ζ z ξ z µ z ζ (A.9) (Chandrupatla and Belegundu 1997) After carrying out the partials in J, on the equations in A.5, it is determined that J has a finite value. x 14 y 14 z 14 J = x 24 x 34 y 24 y 34 z 24 z 34 (A.10) (Reddy 2006) (Chandrupatla and Belegundu 1997) The inverse of the J, called A, is found to be y 24z 34 y 34z 24 y 34z 14 y 14z 34 y 14z 24 y 24z 14 A = J -1 = 1 z 24 x 34 z 34 x 24 z 34 x 14 z 14 x 34 z 14 x 24 z 24 x 14 (A.11) det J x 24 y 34 x 34 y 24 x 34 y 14 x 14 y 34 x 14 y 24 x 24 y 14 Where det J = J = So called, Jacobian (A.12) (Reddy 2006) (Chandrupatla and Belegundu 1997). This can be used to define the equations below: u x u ξ u = A µ u ζ y u z u (A.13)

83 (Chandrupatla and Belegundu 1997) Because J does not change for v and w, A does not change either. The same values of A may be used in the below equations. 83 v x v = A y v z v ξ v x ξ w w and = A y µ w z w ζ µ v ζ w w (A.14) (Chandrupatla and Belegundu 1997) Bringing everything together and trying to form A.1 out of what has been derived, specifically A.13, A.14 and the displacement field in A.4 it is found that ε = β q (A.15) where A A A A A A A A A β = A A A 3 0 A 31 A 21 0 A 32 A 22 0 A 33 A 23 0 A 3 A 2 A 31 0 A 11 A 32 0 A 12 A 33 0 A 13 A 3 0 A 1 A 21 A 11 0 A 22 A 12 0 A 23 A 13 0 A 2 A 1 0 (A.16) where A 1 = A 11 + A 12 + A 13, A 2 = A 21 + A 22 + A 23 and A 3 = A 31 + A 32 + A 33. (Chandrupatla and Belegundu 1997) Section 5.2: Form of L In the elastic region, L is the stress-strain matrix in the 3D version of the generalized Hook s law such that σ = L ε

84 84 L = E (1+ν)(1 2ν) (1 ν) ν ν ν (1 ν) ν ν ν (1 ν) (0.5 ν) (0.5 ν) (0.5 ν) (A.17) E = Modulus of Elasticity ν= Poisson s ratio (Chandrupatla and Belegundu 1997) In the plastic region, L is the stress-strain matrix determined by the behavior of the material modeled such that σ = L ε. L is determined by comparing the strain and flow stress which are known during each iteration.

85 85 Works Cited AI-Zkeri, I. A. Flow Analysis Iniside Shear and Streamlined Extrusion Dies. Master's Thesis, Athens: Ohio University, Bauer, J. R. What Every Engineer Should Know About Finite Element Analysis. New York: Marcel Dekker, Bousquet, J., Van Cauwenberge, P., and Khaltaev, N. "Allergic Rhinitis and Its Impact on Asthma." Journal of Allergy and Clinical Immunology, 2001: S147-S334. Chandrupatla, T. R., and Belegundu, A. D. Introduction to Finite Elements in Engineering. Upper Saddle River, New Jersey: Simon and Schuster, Chen, D. "Finite Element Simulation on High Extrusion-Ratio Hydrostatic Extrusion of Porous Material." Advanced Manufacturing Processes and Technologies Conference. Bahrain: The Arabian Journal for Science and Engineering, Chinh, N., Judit, I., Zenji, H., and Langdon, T. "Using the Stress Strain Relationships to Propose Regions of Low and High Temperature Plastic Deformation in Aluminum." Materials Science and Engineering, 2005: Domblesky, J., Kraft, F., Downing, C., and Guzowski, M. "Numerical Modeling and Validation for Extremely High Extrusion Ratio Processes." The Engineering Society for Advancing Mobility Land Sea Air and Space Technical Papers Series, Felippa, C. Introduction to Finite Element Methods. Boulder, Colorado, Goetz, R. L. An Analysis of Canned Extrusion Using Analytical Methods and the Experimental Extrusion of Cast IN100. Master's Thesis, Athens: Ohio University, Holman, J. P. Experimental Methods for Engineers. New York, NY: McGraw-Hill, Hosford, W. F., and Caddell, R. M. Metal Forming Mechanics and Metallurgy. New York: Cambridge University Press, Hosseini, E., Kazeminezhad M., Mani, A., and Rafizadeh, E. "On the Evolution of Flow Stress During Constrained Groove Pressing of Pure Copper Sheet." Computational Materials Science, 2009: Incropera, F. P., and DeWitt, D. P. Introduction to Heat Transfer. New York: John Wiley and Sons, International Copper Association, Ltd. "Copper Applications Technology Roadmap." 2007.

86 86 Kalpakjian, and Schmid. "Materials Processing Lecture." University of Notre Dame (accessed January 13, 2011). Kardestuncer, H. Finite Element Handbook. New York: McGraw-Hill, Kraft, F. "Extrusion of Thin-Wall Multi-Channel Copper Profiles." Material Science and Technology 2011 Conference. Columbus, Oh. Oct, Kraft, F., and Gunasekera, J. S. "Conventional Hot Extrusion." The Materials International Society Handbook 14A, 2005: Lou, S. "Modeling of Aluminum Alloy Profile Extrusion Process Using Finite Volume Method." Journal of Materials Processing Technology, 2008: MSC Software Corporation. Simufact.Forming Program Input sfmarc. Santa Ana, Ca: MSC, Reddy, J. N. An Introduction to the Finite Element Method. New York: McGraw-Hill, Rogers, S. Flow Stress Analysis of Copper at Elevated Temperatures. Undergraduate Research, Athens: Ohio University, Siegert, K., Bauser, M., and Sauer, G. Extrusion. Materials Park, Oh: The Materials Information Society International, Simufact Engineering. Simufact.Forming Tutorial. Hamburg, Germany, Simufact. "Simufact User Manuel." Hamburg: Simufact Engineering, Skoner. "Allergic Rhinitis: Definition, Epidemiology, Pathophysiology, Detection, and Diagnosis." J Allergy Clin Immunol, 2001: 108:S2 S8. Son, I.H. "Sensitivity of Friction Condition in Finite Element Investigation of Equal Channel Angular Extrusion." Materials Science and Engineering A, 2007: Soury, Nasrabadi, and Zolfaghari. "Design and Manufacture of an Extrusion Die for Wood-Plastic Composite." Journal of Reinforced Plastics and Composites, 2009: Taggart, S. C., et al. "Asthmatic Bronchial Hyperresponsiveness Varies with Ambient Levels of Summertime Air Pollution." European Resp J, 1996: 9: Tiernan, Hillery, Draganescu, and Gheorghe. "Modeling of Cold Extrusion with Experimental Verification." Journal of Materials Processing Technology, 2005:

87 87 Vaitkus, V. A Process for the Direct Hot Extrusion of Hollow Copper Profiles. Master's Thesis, Athens: Ohio University, White, R. E. An Introduction to the Finite Element Method with Applications to Nonlinear Problems. New York: Wiley-Interscience, Zhengjie, J. Three Dimensional Simulations of the Hollow Extrusion and Drawing Using the Finite Element Method. Master's Thesis, Athens: Ohio University, 1994.

88 !!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!! Thesis and Dissertation Services!