USFDC Home  USF Electronic Theses and Dissertations   RSS 
Material Information
Subjects
Notes
Record Information

Full Text 
xml version 1.0 encoding UTF8 standalone no
record xmlns http:www.loc.govMARC21slim xmlns:xsi http:www.w3.org2001XMLSchemainstance xsi:schemaLocation http:www.loc.govstandardsmarcxmlschemaMARC21slim.xsd leader nam Ka controlfield tag 001 001916924 003 fts 005 20071114122707.0 006 med 007 cr mnuuuuuu 008 071114s2007 flu sbm 000 0 eng d datafield ind1 8 ind2 024 subfield code a E14SFE0002017 035 (OCoLC)181160346 040 FHM c FHM 049 FHMM 090 TJ145 (ONLINE) 1 100 Daly, John Louis. 0 245 On comparison of indentation models h [electronic resource] / by John Louis Daly, Jr. 260 [Tampa, Fla.] : b University of South Florida, 2007. 520 ABSTRACT: Thin films that are functionally gradient improve the mechanical properties of filmsubstrate layered materials. Mechanical properties of such materials are found by using indentation tests. In this study, finite element models are developed to simulate the indentation test. The models are based on an axisymmetric half space of a specimen subjected to spherical indentation. The film layer through the thickness is modeled to have either homogeneous material properties or nonhomogeneous material properties that vary linearly. Maximum indenter displacement, and maximum normal and shear stresses at the interface are compared between the homogeneous model and the nonhomogeneous model for pragmatic contact length to film thickness ratios of 0.2 to 0.4, and film to substrate moduli ratios of 1 to 200 to 1.Additionally, a coefficient is derived from regression of the stress data produced by these models and compared to that used to define the pressure field in the axisymmetric Hertzian contact model. The results of this study suggest that a displacement boundary condition to an indenter produces the same results as a pressure distribution boundary condition. The critical normal stresses that occur between modeling a film as a nonhomogeneous and as a homogeneous material vary from 19% for a modulus ratio of 2.5:1 to as high as 66% for a modulus ratio of 200:1 indicating that the modeling techniques produced very different maximum normal stresses. The difference in the maximum shear stress between the nonhomogeneous and the homogeneous models varied from 19% for a 2.5:1 modulus ratio to 57% for the 200:1 modulus ratio but reached values as low as 6% for the 50:1 modulus ratio.The maximum contact depth between the nonhomogeneous and the homogeneous models varied from 14% for the 2.5:1 case to as much as 75% in the 200:1 case. The results from the reapplication of the pressure field derived from the regression coefficients and the R2 values from these regression models indicate the correctness of the regression model used as well as its ability to replicate the normal stresses in the contact area and maximum indenter displacements in a FEA model for both the homogeneous and the nonhomogeneous models for modulus ratios ranging from 2.5:1 to 200:1. The agreement between the regression based coefficients and the force based coefficients suggests the validity for the use of the theoretical axisymmetric Hertzian contact model for defining the pressure field in the contact area and displacements for both the homogeneous case and the nonhomogeneous case for the considered film to substrate moduli ratios and contact length to film thickness ratios. 502 Thesis (M.S.)University of South Florida, 2007. 504 Includes bibliographical references. 516 Text (Electronic thesis) in PDF format. 538 System requirements: World Wide Web browser and PDF reader. Mode of access: World Wide Web. 500 Title from PDF of title page. Document formatted into pages; contains 80 pages. 590 Advisor: Autar Kaw, Ph.D. 653 Functionally gradient materials. FEA. ANSYS. Parabolic contact problem. Hertzian contact model. 690 Dissertations, Academic z USF x Mechanical Engineering Masters. 773 t USF Electronic Theses and Dissertations. 4 856 u http://digital.lib.usf.edu/?e14.2017 PAGE 1 On Comparison of Indentation Models by John Louis Daly, Jr. A thesis submitted in partial fulfillment of the requirement s for the degree of Master of Science in Mechanical Engineering Department of Mechanical Engineering College of Engineering University of South Florida Major Professor: Autar Kaw, Ph.D. Daniel Hess, Ph.D. Craig Lusk, Ph.D. Date of Approval: April 5, 2007 Keywords: functionally gradient materi als, FEA, ANSYS, parabolic contact problem, Hertzian contact model Copyright 2007, John Louis Daly, Jr. PAGE 2 Dedication This thesis is dedicated to my par ents, to my grandmother, and to Dr. Autar Kaw who believed in me through t he most difficult times in my life and provided support far beyond that which was expected of them. PAGE 3 Acknowledgements Thanks to my parents and my grandmot her for helping me get by every single day and to my sister and her family for taking care of me and cooking the worlds best pot roast when my parent s were out of the country. A special thanks to Dr. Autar Kaw not only for his support throughout graduate school, but also for his amaz ing insights into solid mechanics, complicated mathematics, programming, and pop culture. Dr. Kaw has been a teacher, a role model, and a friend to me. I would also like to thank Dr. Glen Besterfield who has been a great inspir ation and who helped get me started in graduate school. I hope that someday he wil l return to the Department of Mechanical Engineering I would like to thanks to Ms. Sue Bri tten who, during my entire time in engineering at USF, has always been in a good mood and extremely helpful. Her contribution to the students in this department over the years has been immeasurable. Thanks to friends Kimberly, Rob, Emmett, Nathan, Billy, James, Phaninder, Saurabh, Jimmie, Abraham, Dani el, Lucas, and all three J. Russels. I would also like my committee mem bers Dr. Daniel Hess and Dr. Craig Lusk for their contributions and for being on my committee. PAGE 4 i Table of Contents List of Tables iii List of Figures iv List of Nomenclature vi Abstract vii Chapter 1: Introduction 1 1.1 Functionally gradient materials 1 1.2 Spherical indentation 2 1.3 Literature survey 3 1.4 Current study 6 Chapter 2: FEA Modeling 8 2.1 Introduction 8 2.2 Modeling film and substrate 10 2.3 Modeling the indenter 14 2.4 Boundary conditions 15 2.5 Meshing the model 17 2.6 Overview 22 Chapter 3: Model Verification 23 3.1 Introduction 23 3.2 Comparison to Hertzian results 24 3.3 Convergence study 29 3.4 Continuity checks 30 Chapter 4: Simulation of the Indentation Process 32 4.1 The displacement boundary condition 32 4.2 Application of the pre ssure boundary condition 34 4.3 Load step and substep procedures 40 4.4 Data post processing 44 Chapter 5: Results and Discussion 47 5.1 Introduction 47 5.2 Hertzian contact assumption 47 PAGE 5 ii 5.3 Contact depth 48 5.4 Maximum normal stress at the films surface 49 5.5 Maximum shear stress at the interface 51 5.6 Pressure models and regression models 52 5.7 Overview of results and discussion 54 References 57 Appendices 59 Appendix A: Convergence study and MathCAD worksheets 60 A.1 Alphabeta convergence 60 A.2 MathCAD program for force calculations 62 Appendix B: Element definitions 63 B.1 CONTA171 full element definition 63 B.2 TARGE169 full element definition 73 PAGE 6 iii List of Tables Table 1: Relevant KEYOPTS for the CONTA171 elements 22 Table 2: Results from sample convergence test 30 Table 3: Substep listing and maxi mum indenter displacement boundary conditions listed for all simulations 44 Table 4: Regression based coefficients for a/Tf=0.3 with R2 values for modulus ratios ranging from 2.5:1 to 200:1 53 Table 5: Regression and force based coefficients for a/Tf=0.3 and percentage di fferences for modulus ratios ranging from 2.5:1 to 200:1 53 PAGE 7 iv List of Figures Figure 1: Material property comparis on of abrupt interface composites and fu nctionally gradient materials 2 Figure 2: Depiction of spherical indentat ion on an axisymmetric half space 3 Figure 3: expansion of the axisymmetr ic FEA model generated by ANSYS 9 Figure 4: Full view of the FEA model in ANSYS depicting the indenter, the film layers, the substrat e, and the boundary conditions 11 Figure 5: Representation of the materi al property distribution used in the la yered nonhomogeneous simulations 14 Figure 6: Graphical repres entation of the boundary co nditions used in the FEA model 16 Figure 7: Structure of the PLANE182 element (ANSYS) 18 Figure 8: Contour plot showi ng the stress continuity in yy for a layered nonhomogeneous model 20 Figure 9: Structure of the CONTA171 element (ANSYS) 20 Figure 10: Structure of the TARGE169 element (ANSYS) 21 Figure 11: Mesh refinements 26 Figure 12: Contact between the in denter and the film surface 28 Figure 13: Displacement plot depicting the contact between the indenter and the film surface 34 Figure 14: Figure depicting the last node in contact used to define the contact length 42 Figure 15: Sample displacement profiles for a/Tf values of 0.2, 0.3, and 0.4 45 PAGE 8 v Figure 16: Sample comparison of normal stresses, yy, along the contact length for homogeneous and nonhomogeneous film models 46 Figure 17: Maximum displacement ratios between the nonhomogeneous and the homogeneous models for Y oungs modulus ratios ranging from 2.5:1 to 200:1 and a/Tf ratios of 0.2 to 0.4 49 Figure 18: Maximum normal stress ratios between the nonhomogeneous and the homogeneous models for Youngs modulus ratios ranging from 2.5:1 to 200:1 and a/Tf ratios of 0.2 to 0.4 51 Figure 19: Maximum shear stress ra tios between the nonhomogeneous and the homogeneous models for Young s modulus ratios ranging from 2.5:1 to 200:1 and a/Tf ratios of 0.2 to 0.4 52 Figure 20: Sample comparison normal st ress for the pressure model to displacement model result s for a nonhomogeneous modulus ratio of 5:1 across a c ontact length of 0.15 54 PAGE 9 vi List of Nomenclature yy y normal stress xy xy shear stress yy(h)max Max. y normal stress in the homogeneous model yy(nh)max Max. y normal stress in the nonhomogeneous model xy(nh)max Max. xy shear stress in the nonhomogeneous model xy(h)max Max. xy shear stress in the homogeneous model Displacement in y (h)max Max. y disp. in the homogeneous model (nh)max Max. y disp. in the homogeneous model a contact length E1 Maximum modulus of the film E2 Modulus of the substrate Ei Modulus of a film layer h Thickness of a single film layer H Model height Tf Thickness of the film R Radius of the indenter PAGE 10 vii On Comparison of Indentation Models John Louis Daly, Jr. ABSTRACT Thin films that are functionally gradi ent improve the mechanical properties of filmsubstrate layered ma terials. Mechanical properti es of such materials are found by using indentation te sts. In this study, fi nite element models are developed to simulate the indentation test. The models are based on an axisymmetric half space of a specimen subj ected to spherical indentation. The film layer through the thickness is m odeled to have either homogeneous material properties or nonhomogeneous material pr operties that vary linearly. Maximum indenter displacement, and maximum normal and shear stresses at the interface are co mpared between the homogeneous model and the nonhomogeneous model for pragm atic contact length to film thickness ratios of 0.2 to 0.4, and film to substrate moduli ratios of 1 to 200 to 1. Additionally, a coefficient is derived from regression of the stress data produced by these models and compared to t hat used to define the pressure field in the axisymmetric Hertzian contact model The results of this study suggest PAGE 11 viii that a displacement boundary condition to an indenter produces the same results as a pressure distribution boundary condition. The critical normal stresses that occur between modelin g a film as a nonhomogeneous and as a homogeneous material vary from 19% for a modulus ratio of 2.5:1 to as high as 66% for a modulus ratio of 200:1 indicating that the modeling techniques produced very diffe rent maximum normal stresses. The difference in the maximum shear stress between the nonhomogeneous and the homogeneous models varied from 19% for a 2.5:1 modulus ratio to 57% for the 200:1 modulus ratio but reached values as lo w as 6% for the 50:1 modulus ratio. The maximum contact depth between the nonhomogeneous and the homogeneous models varied from 14% for the 2.5:1 case to as much as 75% in the 200:1 case. The results from the reappl ication of the pressure field derived from the regression coefficients and the R2 values from these regression models indicate the correctness of the regression model used as well as its ability to replicate the normal stresses in the contact area and maximum indenter displacements in a FEA model for both the homogeneous and the nonhomogeneous models for modulus ratios ranging fr om 2.5:1 to 200:1. The agreement between t he regression based coefficients and the force based coefficients suggests the validit y for the use of the theoretical axisymmetric Hertzian contact model for def ining the pressure field in the contact area and displacements for bot h the homogeneous case and the PAGE 12 ix nonhomogeneous case for the considered fi lm to substrate moduli ratios and contact length to film thickness ratios. PAGE 13 1 Chapter 1: Introduction 1.1 Functionally gradient materials The natural world has historically challenged man by offering seemingly simplistic solutions to design challenges t hat often prove difficult to replicate through technology. Functionally gradient materials (FGM) are an example of this scenario. A material is said to be functionally gradient when its composition gradually varies throughout its volume. This gradual variation in material composition allows for the ma terial properties of a body to vary greatly from the bulk structure of the materi al without experiencing in terface problems that are found in abrupt interface composites. Through gradual transitions in material composition, a structure can benefit from both the proper ties of the substrate and the properties of the materials surface wit h a reduction of interface effects such as thermal stresses and bonding issue that can be found in the discrete bonding of dissimilar materials. In the natural world, functionally gradient materials can be observed in the structure of bam boo, the nanostructure of bones, and the material composition of most trees. T he benefits of functionally gradient material properties have been exploited for years through the process of case hardening of steels. The in itial concept and the developm ent of this technology for dissimilar materials are cr edited to M. Niino at the National Aerospace Laboratory of Japan (R. Narayan, 2006). Niinos c oncept for the development of a FGM PAGE 14 2 coating was born from the need to provide a thermal barrier ma terial for space vehicles and fusion reactors. Since t hen, this technology has found continual applications in the development of thermal coatings as well as applications in mining, and bearing surfaces in human joint replacements. Figure 1: Material property comparis on of abrupt interface composites and functionally gradient materials 1.2 Spherical indentation With the ongoing use of these types of materials in technological applications comes the need for continua l improvement in material testing techniques for both analytical models and experimental proc edures. Indentation has proven itself to be an inva luable material testing tool for many years. Recent improvements in the accuracy of indent ation testing technology have proven PAGE 15 3 indentation as an accurate means of det ermining the material properties of homogeneous thin film coatings for film s as thin an 1m (T. Chudoba, 1999). The success of indentation, particula rly spherical indentation, in the determination of material properties of homogeneous film coating currently makes it of interest with respect to determining the material properties of nonhomogeneous functionally gradient coatings. Figure 2: Depiction of spherical indent ation on an axisymmetric half space 1.3 Literature survey A brief overview of the research in this area begins with Chudoba, et al. (2000) who used an analytical solution for th e elastic deformation of the substrate to simulate loaddisplacement data. The model allowed the modulus of thin films PAGE 16 4 to be determined independently from the effect s of the substrate. Later, in 2004, Chudoba et al. (2004) used a t heoretical model to derive the correct moduli at the lower and top part of the graded coating. These theoretical models proved to be in agreement with values obtai ned from experiments. Chudoba, et al (2002) looked at la yered systems and studied interfacial stresses to show effects of adding inte rmediate layers in improving overall properties of such systems. These results are based on their earlier works (Schwarzer, et al 1999, Schwarzer, 2000) with potential theory. Diaoa and Kandorib (2006) conducted a finite element analysis of the local delamination of a hard coating under sliding contact, and st udied the delamination as a function of the relative shear strengths of t he coating and substrate, and the ratio of coating thickness to contact width. Linss et al (2005) used theoretic al modeling and nanoindentation testing to investigate the mechanical properties of graded thin films with varying Youngs modulus. Their findings showed that thr ough the use of a variety of different spherical indenters that a graded coating could be distinguished from a homogeneous layer. Several studies have been conducted in the last three decades on the contact and indentation problem of nonhom ogeneous materials. Suresh (2001) and Schwarzer (2004) best describe these st udies in their review articles. Recently, Ke and Wang (2006) studied t he problem of frictionless contact analysis of layered materials with ar bitrarily varying elastic moduli. PAGE 17 5 Advancements in the capabilities of computer modeling and processing have allowed for the use of the finite element method to be employed in the modeling of material coatings and s pherical indentation. Additionally, the development of finite element anal ysis (FEA) programs such as ANSYS 10 assists in the use of this method. Early studies using FEA in indentat ion modeling were conducted by K. Sadeghipour (1994), who modeled cracks propagating in polymeric materials subjected to indentation. Sadeghipour ( 1994) ran extensive simulations to determine specimen geometry and boundary contentions suitable for modeling both the specimen and the indenter in s pherical indentation. Many of the modeling techniques used in our study we re, in fact, based on the results from this portion of his study. X. Cai (1995) used the finite element method to simulate the indentation process of a wedgeshaped inde nter into Al/Si and TiN/HSS film and substrate systems. Specimens were built up by a 3m thin coating, a semiinfinite substrate, and a 0.1 m inte rlayer. From the results of this study, X. Cai (1995) was able to investigate the indentati on load vs. indentation displacement relationship and the influence of the interface on hardness measurements and determined interfaces effects on hardness measure was negligible. Chalasani et. al (2006) developed theor etical models of layered film and substrate configurations modeled as both a nonhomogeneous or homogeneous layer. Their study focused on loaddispla cement profiles, cont act pressures, and critical stresses that can lead to debonding in some film and substrate PAGE 18 6 configurations. By comparing contact depth and critical inte rface stresses, the effects of indentation area, film and substrate models, and Youngs Modulus ranging from 1:1 to 200:1 were investigated for nonhomogeneous and homogeneous film configurations. Chalasani modeled the indenter load on the surface as a Hertzian stre ss boundary condition as oppos ed to a mixed boundary value problem. His findings suggested that critical st resses in these two models varied as much as 15% between the nonhomogeneous and the homogeneous models for Youngs modulus ra tios greater than 25:1. 1.4 Current study This study uses finite element analysis (FEA) to investigate the relationship between homogeneous and nonhomogeneous film and substrate geometries subjected to s pherical indentation. This study focuses on three relationships determined through a seri es of FEA simulations conducted on variety of coating models. First, we investigate the validity of the use of a displacement boundary condition by applying a known force from which a maximum displacement is determined in the simulation. Then, th is displacement is reapplied and the resulting critical stresses between the two models are compared. Second, we investigate the effects of modeling the film co ating as either a functionally gradient material with linearl y varying material properties or a homogeneous layer in which the material properties are determined by taking an average of the material properti es of the substrate and the film surface. Critical PAGE 19 7 normal stresses, shear stresses, and ma ximum indentation depths from these models are compared and the force required to create the indentation depth is determined. Third, regression models are devel oped from the results of the FEA models and a coefficient from regr ession is found from each of the nonhomogeneous and homogeneous indentation models at each contact length from the previous simulations. These results are then com pared to the Hertzian contact models by developing a pressure field based on the force determined in the displacement boundary cond ition simulations. The R2 values from the regression models and the relationship bet ween the forcebased coefficient and the regression based coefficient are com pared to assess the validity of the Hertzian contact assumption for bot h the layered nonhomogeneous and the homogeneous modeling techniques. PAGE 20 8 Chapter 2: FEA Modeling 2.1 Introduction ANSYS 10 was used for the finite elem ent simulations conducted in this study. The software was chosen for its ability to solve complex nonlinear problems as well as its ability to empl oy gap elements for contact problems. Additionally, ANSYS load step/substep control made the so ftware capable of retrieving data that occurred at various points along the contact depth as the displacement of the indenter was depressed. This allowed for several contact length to film thickness ratios to be dete rmined in a single simulation given a high enough number of substeps. An axisymmetric half space of th e indentation model was developed for the finite element simulation in order to minimize comput ational time. The symmetric nature of the stresses that o ccur in the spherical indentation process along with ANSYSs ability to simulate this type analysis for a wide variety of elements allow for this assumption. A similar study conducted for a spherical indentation modeling and using the same contact elements and axisymmetric assumption reported a 0.1% deviation from the Hertzian theory (ANSYS) which is known to be exact for a homogeneous hal f space (Schwarzer, 2004). PAGE 21 9 Figure 3: expansion of the axisymme tric FEA model generated by ANSYS PAGE 22 10 2.2 Modeling the film and the substrate The development of the FEA simulati on required that all dimensions used in model be both discrete and based on aspect ratios or geometry that fall within the realm of techniques currently used in the spherical indent ation process and with geometries that allowed for accurate modeling by finite element analysis. An appropriate height of the model was nec essary to minimize the influence of the substrate thickness on the stress results in the film layer(s). The ideal model would be one that had an infinitely thick substrate and discrete thickness for the film layers. This being the case, it was necessary to determine a substrate thickness that was both of a discret e value and thick enough to minimize the effects of the boundary conditions in the st ress results that occurred in the area localized about the interfaces of the laye rs and on the surface contact area. In a study dealing with spherical indentation that used a similar modeling approach and boundary conditions, Sadegh ipour (1994) found, after extensive simulations, that a relatively thick model, one where the ratio of the radi us of the indenter, R and the overall height of the specimen, H was 1/12 ( R/H =1/12) satisfied these conditions for elastic stress modeling. Th is aspect ratio was used for all height and width geometries in the simulations conducted in this study. PAGE 23 11 Figure 4: Full view of the FEA model in ANSYS depicting the indenter, the film layers, the substrate, and the boundary conditions PAGE 24 12 A single film and substrate model was used for all simulations, however, material properties within this model we re changed to represent modulus ratios as well as the nonlinear and homogeneous c oating properties. To model the coating as a nonhomogeneous material, t he film was broken up into ten sub layers that were assigned different materi al properties. Because the focus of this study was to examine the effe cts of modulus ratios, the Poissons ratios for both the substrate and the coat ing were kept at 0.3 for all simulations and configurations. To represent the coating as a nonhomogeneous material, moduli values were assigned to each layer and distribut ed by linear variation with the highest modulus value, E1, on the coating surface at y =0 to the lowest modulus value of E2 which equaled that of the substrate at the lowe r surface of the coating y=Tf. A function was developed from each case to represent the linear variation of the moduli. This model was a simple st raight line modeled by the function: 2 2 1) ( ) ( E y T E E y Ef (1) where E(y) is the value of the Youngs modulus at a vertical depth and y is the vertical depth. PAGE 25 13 Because each material layer was required to have a discrete modulus value, it was then necessary to dete rmine the average modulus value between the upper and lower portions of each la yer. To determine this, the average modulus value, Ei, in each layer was calculated using: i i h h ih h dy y E Ei i 11) ( (2) where hi+1 is the vertical depth in the y direction of the upper surface of the layer and hi is the vertical depth in the y direction of the lower surface of the layer. PAGE 26 14 Figure 5: Representation of t he material property distribution used in the layered nonhomogeneous simulations 2.3 Modeling the indenter Indenter radius was based on aspect ratios to film thickness and was initially altered in the des ign of the FEA model to produce various contact length to film ratios. Film thickness was, however, maintained to be onehalf unit thick and subdivided into multiple layers of vary ing material properties. The overall height and the width of the model were t hen parametrically based on the indenter radius and altered to determine the corre ct indenter radius during the modeling phase. In the end, an indenter radius of 2 units was chosen because, it provided the broadest range of acceptable contact length to film thi ckness ratios that could be achieved for the modulus ratios used in this study. PAGE 27 15 2.4 Boundary conditions The boundary conditions used in the FEA model were based both on the axisymmetric assumption and loading cond itions imposed in the simulation. Boundary conditions were based on those used in an axisymmetric FEA study conducted by Sadeghipour (1994) for spherical indentation. Due to the symmetric nature of stresses that evolve about the vertical axis in a body subjected to spherical indentation an axisymmetric half space model was acceptable for the purpose of simulation. This assumption required that displacements about the vertical axis at the line of symmetr y for both the indenter and the film and substrate model be constrained from movement in the hor izontal direction. The base of the specimen was fixed along its ent ire length in the hor izontal direction ( xdirection) from any displacement that mi ght occur in the vertical direction (ydirection). Movement of the indenter in the y direction was given a fixed negative value by the boundary conditions for displa cement loading. Figure 6 shows a graphical view of t he boundary conditions. PAGE 28 16 Figure 6: Graphical represent ation of the boundary conditions used in the FEA model PAGE 29 17 2.5 Meshing the model After the basic geometry of the model was created in the software, it was necessary to determine the proper mesh for the indenter, the sub layers, and the substrate. Due to the c ontact that occurred between the layers, the interface between film layers, the film and the substrate, and the contact between the indenter and the film surfac e, it was also important that contact (gap) elements be used at the lines that occurred in these regions. Because the model was based on an axisymmetric assumption and de veloped in two dimensions, planar elements for the areas and contact element s for the lines were used. For all areas occurring in the layers, the substr ate, and the indenter, the planar element PLANAR182 was used. The lines betw een upper contact surfaces were meshed as CONTA171 and the lower target surfaces in the contact surface were meshed as TARGA169. PLANE182 was used for all area in the simulations including the indenter, the film layers, and the substrate. PLANE182 is a 2D element used for modeling solid structures. The elem ent was chosen because it has a KEYOPT for use in axisymmetric modeling and it can be coupled with CONTA171 and TARGE169 elements to define contact and ta rget pair relationships. Additionally, PLANE182 is capable of being used in cases of large deflection and large strain. The element is defined by four nodes, each of which has two degrees of freedom for translation in the x and the y directions. The element also has the capability to be used for plasticity, hyperelastic, st ress stiffness, large deflection, and large strain. PAGE 30 18 Figure 7: Structure of t he PLANE182 element (ANSYS) The element CONTA171 is used to represent contact and sliding between two surfaces in a contact/target pair for 2D structural and coupled field analysis. The contact between this element and the target surface occurs when the element surface penetrates one of the target surface el ements. The relationship between a contact and a target pair in AN SYS is accomplished by fixing a set of REAL constants between the contact elements and the target elements and meshing the pair along lines or elements designated in the mesh attributes in preprocessing. For this reason, it was necessary with our model to define a total of 12 contact and target pairs to represent the indenters contact with the target surface of the coating at y =0 and the contact/target rela tionships that occurred between the film layers and the last film layer with t he substrate. An accurate representation of the elements behavior in the indentation model required that the KEYOPTs and the REAL constants for each of the contact and target pairs be defined appropria tely. The most crucial parameters used in this element were those that de scribed the friction that occurred between PAGE 31 19 the indenter and the film surface and thos e that defined the element behavior at the interfaces. In our simulations, the friction betw een the indenter and the film were designated to be zero in all models. The reasoning for this is that the effects of friction between the indenter and the film surface vary between materials and ultimately should be minimized or canc elled out in the stress ratios between these two models. For the interfaces between the film la yers and the interface between the film and the substrate, t he CONTA171 parameter for sl iding was fixed so that nodes on the upper layer of t he interface (TARGE169) and the lower layer of the interface (CONTA171) were fully bonded a nd constrained from any delamination and sliding that may occur. Additiona lly, fixing the laye rs together ensured continuity of displacement between the film layers. Vanimisetti (2005) also used this constraint in the ABAQUS/Standard software for the purposes of modeling the interface between film layers. PAGE 32 20 Figure 8: Contour plot showi ng the stress continuity in yy for a layered nonhomogeneous model A full description of the CONTA1 71 KEYOPTS and REAL constants used in the FEA model are listed in Table 1: Relevant KEYOPTS for the CONTA171 elements. Figure 9: Structure of t he CONTA171 element (ANSYS) Target elements describe the boundary of a deformable body that is potentially in contact with a surfac e element. The element TARGE169 corresponds with the use of the element type CONTA171 for contact and target PAGE 33 21 pairs. TARGE169 was used for all upper surfaces of the film layers and the upper layer of the substrate in the F EA model. The majority of KEYOPTS and REAL constants of interest in the cont act and target pair were fixed by the CONTA171 KEYOPTS and REAL constant s. ANSYS describes the element TARGE169 as the associated target element for the contact elements CONTA171, CONTA172, and CONTA175. A useful trait of the ta rget element TARGE169 is that forces and moments can be imposed on this surface independent of a contact element. For this reason, the pressure displacement model s used in the simulation did not require that the model be reconf igured for analysis. It only required that the corresponding pressures be imposed and the di splacement of the indenter in this case be fixed to zero for all degrees of freedom. Figure 10: Structure of t he TARGE169 element (ANSYS) PAGE 34 22 2.6 Overview The following table provides an over view of the KEYOPTS used in the simulation and the portion of the model to which they correspond. With the exception of the film layer in direct contact with the i ndenter, the KEYOPTS and real constants of the cont act and target pairs were consistent with each other, although defined separately for each surface. For this reason, the following table only needed to be defined in two sections to represent all of the KEYOPTS used in the contact and target pairs in the simulation. Table 1: Relevant KEYOPTS for the CONTA171 elements CONTA171: Lower film layers KEYOPT Description Status Status Description 1 Selects degrees of freedom 0 UX,UY 2 Contact Algorithm 0 Augmented Lagrangian 3 Stress state when superel ements are present 0 NA/Default 4 Location of contact detecti on point 0 On Gauss point 5 CNOF/ICONT automated adjustment 4 Auto ICONT 12 Behavior of contact su rface 5 Bonded (Always) CONTA171: On the indenter surface KEYOPT Description Status Status Description 1 Selects degrees of freedom 0 UX,UY 2 Contact Algorithm 0 Augmented Lagrangian 3 Stress state when superel ements are present 0 NA/Default 4 Location of contact detecti on point 0 On Gauss point 5 CNOF/ICONT automated adjustment 4 Auto ICONT 12 Behavior of contact surfac e 0 Standard (Frictionless) PAGE 35 23 Chapter 3: Model Verification 3.1 Introduction It was determined early on in the develop ment of the FEA model that the proper mesh size and element choice woul d play a vital role in accurately modeling the indention proce ss. A coarser mesh at the lines of contact was found to produce stresses in a fully homogeneous half space model that were both inconsistent and incorrect when comp ared to the exact solution from the theoretical Hertzian contact model. For th is reason, model verification assisted not only with the evaluation of the corre ctness of the model, but also with the overall development of refinements and elem ent choice that were used. Model verification of the FEA model used in th is study consisted of three procedures that will be fully outlined in this chapter. These procedures included: 1.) Comparison to Hertzian theory for axisymmetic geometries when the model was defined as a fully homogeneous halfspace. 2.) A convergence study for the lowest modulus ratio (1:1) and the highest modulus ratio (200:1). 3.) An assessment of stress continuity at the interfaces between the film layers. PAGE 36 24 The model verification process took pl ace each time that the FEA model changed in geometry and load ing configuration. The limited nature of the educational version of ANSYS 10 for educational purposes required that a maximum of nodes be defined in the model. Although the maximum number of nodes was bey ond that necessary for the 2D axisymetric halfspace model, due to t he heavy usage of contact and target elements, it was determined through seve ral attempts to be too low for 3D modeling in this study. 3.2 Comparison to Hertizan results When the mesh in an FEA model that is correctly defined is refined, the overall error in the solution should reduc e, however, the computation time for the solution increases greatly with the number of nodes present in the model. Additionally, the limitations of the software provide an upper limit to the number of nodes that can be defined in a body. For these reasons, mesh refinements at areas of importance with respec t to the final solution as well as to the conditions defined in the loading can o ften be useful in limiting th e processing time without incurring great losses in the solutions accu racy. In our case, the portions of the model determined to be of the greates t importance and thus requiring the heaviest refinements were the contact por tion on the indenter, the contact portion of the film surface, and the contact portions of the individual f ilm layers where the maximum normal stresses, shear stresse s, and displacements occurred. PAGE 37 25 Early models created using a coarser me sh (element lengt h greater than 1/48th of the specimen width) were found to produce such stress results when compared to Hertzian theory that to list the results would be irrelevant. The reason for this was probably the error in curred in the simulation between the contact elements and the tar get elements in the region of the contact area. When meshed coarsely, elements viewed in a displacement plot in the postprocessing phase of the simulation, appeared to pass through each other rather than to induce contact between the specimens. For this reason, the mesh in the extending past the contact area (from x =0 to x =1) was refined at the surface. The mesh was also refined to a depth just past the last film layer into the substrate and refined along the lines betw een the film layers and the last film layer to the substrate. The original guidelines for these re finements came from those used by Vanimisetti (2005) for model ing film and substrat e configurations using FEA, however, refinements along the interface between the last film layer and the substrate were more heavily refined in our study due to the interest in the shear stresses in this region. Th ese refinements alone greatly improved the results, however, it was necessary at this point to determine how much refinement was necessary. PAGE 38 26 Figure 11: Mesh refinements PAGE 39 27 The initial determination of the me sh refinement requirements was an iterative process that involved the following steps: 1.) Defining a course mesh and evaluating the region of contact irrespective of the error in the magnitude of the stresses, 2.) Refining the portions of the previous model and then running the simulation, 3.) Comparing these results to the Hertzian model to determine whether or not additional refinements were necessary. When the error of the FEA model in comparison the Hertzian model was less than 5% for the maximum no rmal stress at the surface, yy, it was necessary to conduct a convergence study on the curre nt mesh to determi ne whether or not further refinements would reduce error. PAGE 40 28 Figure 12: Contact between the indenter and the film surface PAGE 41 29 3.3 Convergence study Convergence testing on an FEA model ca lculates discretization errors by evaluating the results from t he model at several levels of mesh refinement. It also can, in some cases, help to determi ne whether or not a singularity occurs in the model. Using a single geometric model with fixed material properties and geometry, several levels of refinem ent are brought onto the mesh and the simulation is run for each of these levels of refinements. Data at a given point in the model was collected fo r each of the levels of refinement and a convergence test was conducted using the mathematical model. Let RN be the resulting output using N number of elements, then A is the result using an infinite number of elements in ) ( N B A RN (3) where B is a constant and, is the rate of convergence. From equation 3 it can be seen that as N approaches infinity that the value of RN, which represents a theoretical value of the result, with an infinite mesh, becomes A if the term is greater than 1. Also note that there are three unknowns ( A, B, and ) showing that results from th ree meshes must be used for this convergence test to be conducted. PAGE 42 30A sample convergence test of the mesh th at was used in this study produced the following results: Table 2: Results from sample convergence test N A 20 383.76 30 395.78 40 397.76 which resulted in the equations 40 76 397 30 78 395 20 76 3833 2 1B A B A B Ayy yy yy Solving these three simultaneous equations the following results were found 057 4 10 828 2 655 3986 B A which showed that the theoretical va lue of the stress at this point A was equal to 398.655 and that >1, indicating that the result s will converge and that there was a decrease in relative error result ing from the refinem ent of the mesh. 3.4 Continuity checks After evaluating the results from the mesh by comparison to the Hertzian model and developing an adequate mesh as found by convergence testing, the model was arranged in the nonhomogeneous fo rm and the continuity of the PAGE 43 31shear stresses and displacements wa s compared at the top and the bottom interfaces of the last film layer to determine whether or not there was a continuous transfer of stresses and displa cement across the contact and the target elements. Due to the nature of the mesh, some error was inevitable given the placement of the nodes along the cont act surface because node locations at the top and node locations at the bottom of the interface did not necessarily have the same coordinates. The node locations, however, were close enough for comparative purposes (less that 1/10th of a element length in most cases) to make a comparison. The final configur ation of the model showed continuity across the interface for both stresses and displacements with errors were less than 0.5% for both displacements and shear stresses. PAGE 44 32 Chapter 4: Simulation of the Indentation Process 4.1 The displacement boundary condition To simulate a displacement from an indenter onto the surf ace of the film, the base of the film and substrate model, the line of symmetry of the indenter, and the line of symmetry of the film and substrate were fixed according to the boundary conditions and the indenter itse lf was given a fixed downward maximum displacement in the vertical di rection in the ANSYS software. As the indenter passed through various point s along the path to the maximum displacement, data was collected at every su bstep, or vertical position, along its path. By doing this, it was possible to collect data at a variety of points and correlate the position of the indenter to t he contact length to film thickness ratios of interest along the path. The contact length of the indentation is defined as the lengt h from the first point of contact of the indenter to the last point on the indenter surface that direct contact with the indented specimen occurs. Generally, a contact length to film thickness ratio ranging from 0.2 to 0.4 is considered suitable from measure of material properties from spherical i ndentation (Chalasani, 2006). Indentation profiles for displacement resulting from s pherical indentation at the surface of the indented specimen generally are parabo lic in nature and dependent on the material properties of the indented material For this reason, it is difficult to PAGE 45 33assume a contact length based solely on the radius of the indenter and the displacement or force t hat is applied to it. The technique used in this study to overcome this challenge was to overshoot the indention depth necessary to produce the contact length to film thickness ratio, a/Tf, and to examine the data t hat was produced along the path of the indenter to find the di splacements that resulted in the correct ratios based the reaction forces that occurred on the film surface as the indenter penetrated the film. From this data, it was th en possible to narrow down the depths of interest and to identify a maximum indent ation depth that could be used in the final simulations. This procedure reduced the overall processing time by providing more accurate data through a decrease in the number of substeps necessary in the final simulations. PAGE 46 34 Figure 13: Displacement plot depicting t he contact between the indenter and the film surface 4.2 Application of the pr essure boundary condition The pressure models used in this study were developed based on regression models from the data collected in the displa cement simulations. The basis for the creation of these models was to determine if a regression model based on the Hertzian contact assumption and calculated through the data that resulting from the FEA simulations w ould produce a coefficient of similar magnitude to that of the forcebased coefficient used in the Hertzian contact model for spherical indentation. The dev elopment of these two coefficients from PAGE 47 35models independent of each other allo wed for the comparison of the FEA nonhomogeneous and homogeneous model data for film and substrate models to the theoretical Hertzian contact m odel used for fully homogeneous (film and substrate having the same material proper ties) spherical indentation modeling. To describe the procedural basis of t he development of the coefficients, it is first necessary to examine the pressure field as it is modeled by the Hertzian contact assumption. For a spherical indentation study of an axisymmetric homogeneous half space, the known exact technique for modeling a pressure field is given by the equation: 2 2 32 3 ) ( r a a P r p (4) where P is the force applied to the indenter a is the contact length, and r is a point along the contact length PAGE 48 36Examination of equation 4 shows that the constant terms can be collected and rewritten as : 32 3 a P CH (5) for a given contact depth, a and equation 5 can be rewritten as: 2 2) ( r a C r pH (6) where the term CH represents what will be referred to as the forcebased coefficient term. To determine the forcebased coeffici ent term from the data collected through the FEA simulations, data for the normal stress along the surface in the region of the contact length, a, was co llected and then integrat ed accordingly to determine the force by first creating a cubic spline of the data and then integrating the spline to determine the applied force, P using: a yydx x x P0) ( 2 (7) PAGE 49 37Finally, combining the force, P and the remaining terms in CH the forcebased coefficient term can be rewritten as: a yy Hdx x x a C0 3) ( 3 (8) The derivation of the regression bas ed coefficient began with the pressure field, p(r). Assuming that the stresses in t he FEA model for the functionally gradient material followed the Hertzian cont act assumption, it follows that, at the surface: 2 2) ( r a C rR yy (9) where CR is a coefficient determined through regression. From equation 8, the sum of t he square residuals is then: 2 1 2 n i i R i rr a C S (10) PAGE 50 38Minimizing the sum of the square residuals by taking the first partial derivative of SR with respect to CR then gives: 0 22 1 2 i n i i R i R rr a r a C dC dS (11) Whose solution defines the regression based coefficient as: n i i n i i i Rr a r a C1 2 2 1 2 2) ( (12) Once the coefficients were developed, the reapplication of the regression coefficient based pressure field to the model from which the coefficient developed was conducted to ens ure the accuracy of the regression technique as well as to examine the justif ication for the use of this technique in modeling. The reapplication of the pressure field in ANSYS required that the pressure be distributed over the contact area after wh ich the simulation was solved so that the results could be compared. Because the pressure field from the regression model was defined at points along the radius of t he contact length, it was necessary to then determine the value of pressure across individua l element length in the FEA model to PAGE 51 39reapply them in ANSYS. To accomplis h this, the trapezoidal rule was used between the pressure values at indivi dual nodal locations and the pressure determined by this procedure was applied to the element surface between these nodes. The pressure between two consecutive nodes using this method was defined by the trapezoidal rule as: ) ( 22 2 11i i x x yy ix x dx x pi i (13) where pi is the pressure applied to the element surface xi is the xlocation of the first nodal pressure xi+1 is the xlocation of the second nodal pressure The first pressure applied from equat ion 12 was defined across the first element along the line of symme try. As a result of th e method used to distribute the pressure across the contact length, it was not possible to apply a pressure at the last element in the contact length, however, the nodal spacing was created using a very fine mesh and the pressure at this location was significantly low as have a negligible influenc e over the results. PAGE 52 404.3 Load step and substep procedures All simulations required ANSYS to perform nonlinear analysis in the solution phase. Solution controls were se t to large displacement static mode. A range of substeps which varied from si mulation to simulation were used to produce the final results, but the maximum number of substeps ultimately used in the solutions were determined by the AN SYS solver using a modified bisection method. The solution method that was fixed by the PLANE182 element was modified Lagrangian. CONTA171 KEYOPT for AUTO ICONT corrected the initial penetration gap by adjustments in the first substep. Results at every substep were written and saved to the database for postprocessing after the solution completed. The program for the geometry and t he mesh was initially written in the form of an ADPL logfile but was later saved as 15 database (.db) files with varying displacements and material proper ties that corresponded to each of the modulus ratios for the homogeneous and the nonhomogeneous simulations. Simulations were run on two comput ers. The first used a 1.0 GHZ Pentium 4 processor with 1 GB of RAM. The second computer used a 1.0 GHZ Pentium 4 and processor and 512 MB of RAM. Solution times varied by computer and case but generally ran from 3 hours to 5 hours per simulation. Overall, each full batch of simulations took approximately 75 hours of processing time to complete. Simulations were run to determine the stresses and displacements that occurred at the surface and t he interface for homogeneous and PAGE 53 41nonhomogeneouslayered models wit h moduli ranging from 1: 1 to 200:1. Each simulation provided data for a/Tf values ranging from 0.2 to 0.4. To retrieve the data at those values, the l oading was broken up into a series of substeps and the indenter displacement t hat produced the correct a/Tf ratios were determined by the following steps: 1.) Stresses at the nodes corresponding to the a/Tf ratio of interest were written to a lister file at each subs tep after the solution completed and a range of substeps that the correct ratio occurred in was identified. 2.) Reaction forces at the nodes corres ponding to the contact lengths that produced a/Tf ratios of 0.2, 0.3, and 0. 4 were examined throughout the range of substeps identified in step 1 of this procedure. The substep that produced a positive reaction force was isolated and determined to be the nearest correct substep. 3.) A visual inspection of the displa cement plot from ANSYS postprocessor was made to determine if the last node in contact from step 2 of this procedure correctly corresponded with the node required for the proper a/Tf ratio. 4.) If the node from step 2 and step 3 of this procedur e was +/1 node length (element length of 0.001866667) then the data at this substep was read. If not, then the number of substeps wa s increased and the simulation was run again. PAGE 54 42 Figure 14: Figure depicting the last node in contact used to define the contact length PAGE 55 43Initially, the minimum number of subst eps specified for all simulations was fifty. After running all of the cases, it was determined that this number was generally too low for most of the cases, however, the displacements at values of a/Tf = 0.4 for all simulations (which repr esents the maximum displacement that would be required for future si mulations) was determined. By reducing the maximum indenter displacement and increasing the number of substeps through a series of simulations, every time that the simulations were run and step 4 of the procedure above took place, the results became increasingly more accurate. In the end, the majori ty of the cases required at least 200 substeps to provide accu rate results. This being the case, it is interesting to note for future stud ies that the computation time was not significantly increased by the increase in the number of subste ps. Table 2 below shows the number of substeps and t he ultimate maximum displacements specified in the final simulations from which data was collected. PAGE 56 44Table 2: Substep listing and maximu m indenter displacement boundary conditions listed for all simulations 4.4 Data post processing After the substeps corresponding to the correct a/Tf values for each simulation were determined, a program wa s run in APDL that isolated the nodes at the surface ( y=0 ) and at the interface ( y=Tf). Stress and disp lacement data at these substeps were written to lister (. lst) files by the ANSYS postprocessor and later exported to Excel for evaluation. At this poin t, the data was analyzed and critical data points were isolated. The stress profiles in Excel we re imported to MathCAD for the development of the pressure boundary cond ition coefficients. The ability of MathCAD to easily handle large quantitie s of data and perform a wide variety of complicated calculations made it more su itable than Excel for the development of Case Min. number of Substeps Max. Indenter Disp 1:1 200 0.025 2.5:1 H 200 0.025 2.5:1 NH 200 0.025 5:1 H 200 0.035 5:1 NH 200 0.035 12.5:1 H 200 0.045 12.5:1 NH 200 0.045 25:1 H 200 0.065 25:1 NH 200 0.065 50:1 H 200 0.085 50:1 NH 200 0.085 100:1 H 200 0.15 100:1 NH 200 0.15 200:1 H 100 0.2 200:1 NH 100 0.2 PAGE 57 45the pressure boundary condition inputs and the comparisons to the Hertzian contact model (that were used in the model verification). The outputs from the calculatio ns handled by MathCAD were then exported back to an Excel worksheet a fter which ADPL code was developed for the pressure boundary condition simulations. Displacement profiles for 25:1 Homogeneous5.00E02 4.50E02 4.00E02 3.50E02 3.00E02 2.50E02 2.00E02 1.50E02 1.00E02 5.00E03 0.00E+00 00.050.10.150.20.250.30.350.40.450.5 x locationy displacement 0.2 0.3 0.4 Figure 15: Sample displacement profiles for a/Tf values of 0.2, 0.3, and 0.4 PAGE 58 46 yy in in the contact area4 3.5 3 2.5 2 1.5 1 0.5 0 00.020.040.060.080.10.12 x yy Homogeneous Nonhomogeneous Figure 16: Sample comparison of normal stresses, yy along the contact length for homogeneous and nonhomogeneous film models. PAGE 59 47 Chapter 5: Result s and Discussion 5.1 Introduction Data from the FEA simulations was obtained to indicate contact depth, maximum normal stress at on the film surf ace, and maximum shear stress at the film to substrate interface for different values of film to substrate Youngs modulus ratio, contact length to film thickness ratios, and homogeneous or nonhomogeneous representations of the film layer modulus. Results are given for both the linear va riation model for elastic modulus as well as the homogeneous elastic modulus model. The variations in the FEA model results from these modeling tec hniques are examined by comparing the ratios of the nonhomogeneous and the hom ogeneous models as well as through comparisons between coefficient terms der ived from either regression or through calculation of the force applied to the indenter. 5.2 Hertzian contact assumption The validity of the use of a displacement boundary condition was confirmed by first applying a known force to the indenter in the FEA model and collecting this data then, from that data, we apply the resulting maximum displacement of the indenter and compare results. Simulations showed that for every case, the resulting of critical normal stresses, shear stresses at the PAGE 60 48interface, and the displacement profile itself did not vary between the two methods. The accuracy of the FEA model used fo r the layered cases as well as the correctness of the derivati on of the regression coefficient was confirmed by applying a known force to the indenter in a fully homogenous model and comparing the results from th is simulation to the known exact results of Hertzian contact theory for an axisymmetric geomet ry. Based on the results from the 1:1 model, the coefficient from regression was found to have an R2 value of 0.999. Additionally, when comparing the regre ssion based coefficient and the resulting forcebased coefficient used in the Hertzi an contact model from this model, the error resulting between the two that was less than 1%. 5.3 Contact depth Figure 17 depicts the relationship between modulus ratio and contact length to film thickness ratio to th e maximum contact depth. The maximum contact depth between the nonhomogeneo us and the homogeneous models varied from 14% for the 2.5:1 case to as much as 75% in the 200:1 case. The influence contact length to film thickness ra tio effected the variation in the sense that higher a/Tf ratios showed less variation th roughout the modulus ratios range than lower a/Tf ratios. The reason for this may be that the effect of the modeling techniques became more pronounced with i ndentions that penetrated the film layer more heavily. PAGE 61 49 1.00E+00 1.10E+00 1.20E+00 1.30E+00 1.40E+00 1.50E+00 1.60E+00 1.70E+00 1.80E+00 050100150200250Young's modulus ratio, E1/E2Contact depth ratio, dnh/dh 0.2 0.3 0.4 Figure 17: Maximum displacement ra tios between the nonhomogeneous and the homogeneous models for Youngs modulus ra tios ranging from 2.5:1 to 200:1 and a/Tf ratios of 0.2 to 0.4 Note that there is a spreading in t he displacement ratios related to a modulus ratio value of 12.5:1. The reas on for this deviation in the displacement data in Figure 17 is presumed to be relat ed to the local deviation from the trend of the data in the maximu m normal stress at a modulus ratio of 12.5:1 or, conversely, the improvement of the data centered about a modulus ratio of 50:1. 5.4 Maximum normal stress at the films surface Figure 18 depicts the relationship between modulus ratio and contact length to film thickness ratio to the maximum normal stress, max yy, at the surface of the film. The variati on in maximum normal stress at the films surface ranged PAGE 62 50from 19% for the 2.5:1 modulus ratio to as much as 66% for the 200:1 modulus ratio. As with the contact depth variati on, the influence of the contact length to the film thickness ratio, a/Tf, reduced the variation of the stresses between the nonhomogeneous and the homogeneous models. The reason for this is, again, assumed to be the effect of deeper penetra tion of the indenter representing an averaged material property in the f ilm vertical cross section. To validate the planar assumption m ade by Chalasani (2006), for films of different elastic modulus than the substr ate, the film surface was modeled to have a modulus of E1 and the substrate to have a modulus of E2 with the intermediate layers following either nonhomogeneous or a homogeneous material properties to represent a trans itional interface between a fiber and a matrix. The geometry of the FEA model used in this study allowed for the model and the mesh itself to accomplish this simply with a change in material property throughout the layers. The re sults of these tests showed that the ratios between the axisymmetric model and a planar case used by Chalasani differ by less than 6% for the maximum interfacial normal st ress ratio, 2% for the maximum shear stress ratio, and 4% for the maximum indentation depth showing that the assumption for the planar model was, in fact, valid. Additionally, it is interesting to note another similarity to Chalasanis work. From the FEA data it appears that maximu m normal stress variation appear to have peaked out somewhere around a modul us ratio of 12.5:1 and then dropped down around a modulus ratio of 50:1, and then steadily increase thereafter. PAGE 63 51 1.00 1.10 1.20 1.30 1.40 1.50 1.60 1.70 050100150200250Young's modulus ratio, E1/E2Maximum normal stress ratio, yy(nh)max/ yy(h)ma x 0.2 0.3 0.4 Figure 18: Maximum normal stress ra tios between the nonhomogeneous and the homogeneous models for Youngs modulus ra tios ranging from 2.5:1 to 200:1 and a/Tf ratios of 0.2 to 0.4 5.5 Maximum shear stress at the interface The difference in the maximum shear stress between the nonhomogeneous and the homogeneous models va ried from 19% for a 2.5:1 modulus ratio to 57% for the 200:1 modulus ratio, but reached values as low as 6% for the 50:1 modulus ratio. As with the maximum norma l stress data, the ratio appears to have approached a loca l maximum centered about a modulus ratio of 12.5:1 after which the shear stre ss ratios briefly decreases but, again, continued to increase as the mo duli ratios increased to 200:1. PAGE 64 52 0.00E+00 2.00E01 4.00E01 6.00E01 8.00E01 1.00E+00 1.20E+00 1.40E+00 1.60E+00 1.80E+00 050100150200250Young's modulus ratio, E1/E2Maximum shear stress ratio, xy(nh)max/ xy(h)max 0.2 0.3 0.4 Figure 19: Maximum shear stress rati os between the nonhomogeneous and the homogeneous models for Youngs modulus ra tios ranging from 2.5:1 to 200:1 and a/Tf ratios of 0.2 to 0.4 5.6 Pressure models and regression models There was a surprising agreement between the regression based and the pressure based coefficients for both the nonhomogeneous and the homogeneous models as well as the R2 values for the regression models indicating that both models produced data closely related to the theoretical Hertzian contact model. The explanat ion for this is that while the nonhomogeneous and the homogeneous material models for the film layer varied greatly when compared to each other from the standpoint of cr itical stresses and displacements, the overall force applied to the indenter varied accordingly as to be in agreement with Hertzi an contact theory. Table 4 shown below lists the PAGE 65 53regression and the pressure based coefficients related to a contact length to film thickness ratio of 0.3. Data was chosen at this point because it reflects the average contact range of data collected in the experiment and it is based on a higher number of nodal data poi nts (81) than the data th at was collected for a contact length to film thickness ratio of 0.2. This being the case, it should be pointed out that the relati onship between the regression based coefficients and the pressure based coefficients listed for an a/Tf ratio of 0.3 in Table 4 were very similar to those from a/Tf ratios of 0.2 and 0.4. Table 4: Regression based coefficients for a/Tf=0.3 with R2 values for modulus ratios ranging from 2.5:1 to 200:1 Mod. Ratio 2.5 5 12.5 25 50 100 200 Coefficient H NH H NH H NH H NH H NH H NH H NH Regression 0.55 0.72 0.93 1.36 2.19 3.24 4.08 6.21 8.22 11.7 15.4 22.7 30.7 44.5 R Squared 0.97 0.99 0.95 0.99 0.99 0.97 0.98 0.98 0.99 0.98 0.98 0.98 0.99 0.97 Table 5: Regression and forcebased coefficients for a/Tf=0.3 and percentage differences for modulus ratios ranging from 2.5:1 to 200:1 Mod. Ratio 2.5 5 12.5 25 50 100 200 Coefficient H NH H NH H NH H NH H NH H NH H NH Regression 0.55 0.72 0.93 1.36 2.19 3.24 4.08 6.21 8.22 11.7 15.4 22.7 30.7 44.5 Forcebased 0.53 0.72 0.87 1.37 2.17 3.31 3.96 6.50 8.20 11.6 14.9 22.3 29.9 43.8 % Diff. 4.8 0.1 6.0 0.8 0.8 2.2 3.0 4.4 0.2 1.1 2.9 1.7 2.5 1.6 To confirm the ability of the regression models to r eplicate results in the models from which they were derived, the pressure field, p(r) which resulted from the coefficients, was r eapplied for modulus ratios of 2.5:1, 5:1, and 100:1. These simulations showed that the coefficients, when reapplied, produced maximum normal stresses,max yy, to within 5% and maximu m displacement values PAGE 66 54and to within 1% from the displacement simulations from which they were created. Figure 19 shown bel ow depicts a sample stress profile from the results of reapplying the pressure field to a nonhomogeneous layered case with a modulus ratio of 5:1 and a contact lengt h to film thickness ratio of 0.3. 0.25 0.2 0.15 0.1 0.05 0 0.00E+002.00E024.00E026.00E028.00E021.00E011.20E011.40E011.60E01 x locationNormal stress, yy Pressure Model Displacement Model Figure 20: Sample comparison normal st ress for the pressure model to displacement model results for a nonhom ogeneous modulus ratio of 5:1 across a contact length of 0.15 5.7 Overview of results and discussion The results of this study suggest t hat a displacement boundary condition to an indenter produces the same results as a force or pressure distribution boundary condition. The critical normal st resses that occur between modeling a film as a nonhomogeneous and as a homogeneous material vary from 19% for a PAGE 67 55modulus ratio of 2.5:1 to as high as 66% for a modulus ratio of 200:1 indicating that the modeling techniques produced very different maximum normal stresses. Additionally, the ratios for maximum di splacement and maximum shear stress at the interface also suggest that these m odeling techniques produce very different results which become more pronounced as the modulus ratios increase. The results from the reappl ication of the pressure field derived from the regression coefficients and the R2 values from these regression models indicate the correctness of the regression model used as well as its ability to replicate the critical normal stresses in the contact ar ea and displacements in a FEA model for both the nonhomogeneous and the hom ogeneous modeling techniques The agreement between the regressi on based coefficients and the forcebased coefficients suggests the validit y for the use of the theoretical axisymmetric Hertzian contact model for defining pressure field in the contact area and displacements for bot h the homogeneous case and the nonhomogeneous case if the applied force to the indenter is known for contact length to film thicknesses ranging from 0.2 to 0.4. For the nonhomogeneous case, an increas e in the percentage difference between the regression coefficient and the pr essure coefficient did not increase from modulus ratios from 2. 5:1 to 200:1 indicating that the axisymmetric Hertzian contact model should produce relatively accurate results for normal stresses in this range for functionally gradient mate rials with linearly varying modulus. The results from the homogeneous case, due to the average modulus having been used between E1 and E2 only suggest the validity of the PAGE 68 56axisymmetric Hertzian contact model for modulus ratios ranging from 2.5:1 to 100.5:1 for abrupt interface composit es. Like the results from the nonhomogeneous case, there did not appear to be an increase in the percentage difference between the regression bas ed coefficients and the forcebased coefficient indicating no trend in the error associated with the results of critical normal stresses at the surface and increas ing modulus ratios in this range. It would be interesting in future st udies to examine different modeling techniques for the functionally gradient la yer as well as to examine the planar case. While there is a great variati on between modeling the film layer as a homogeneous material having the average properties of the film and the substrate and as a linearly varying materi al, the effects modeling this layer as an exponentially varying material layer and comparing these results to the linear model would be beneficial. PAGE 69 57 References Cai, X., Bangert, H., 1996, Finiteelement analysis of the interface influence on hardness measurements of thin films Surface and Coatings Technology 81, 240255. Chasalani, P., Kaw, A., Da ly, J., Nguyen, C., 2007, Effect of geometrical and material properties in nanoindentation of layered materials with an interphase Int. J. Solids Struc, in press. Chudoba, T., Schwarzer, N., Linss, V., Ritcher, F., 2004. Determination of mechanical properties of graded coatings using nanoindentation Thin Solid Films 239, 469470. Chudoba, T., Schwarzer, N., Richter, F., 2000. Determination of elastic properties if thin films by indentati on measurements with a spherical indenter Surface and Coating Te chnology 127, 917. Chudoba, T., Schwarzer, N., Richter, F., 2002. Steps towards a mechanical modeling of layered systems Surface and Coating Technology 154, 140151. Diao, D., Kandori A., 2006, Finite element analysis of the effect of interfacial roughness and adhesion strength on the local delamination of hard coating under sliding contact Tribology International 39, 849855. Ke, L., Wang, Y., 2006. Twodimensional contact mechanics of functionally graded materials with arbitr ary spatial variations of material properties International Journal of Solid s and Structures 43, 57795798. Linss, V., Schwarzer, N., Chudoba, T. Karniychuk, M., Richter F., 2005. Mechanical properties of a graded BCN sputtered coating with varying Youngs modulus: deposition, theoretical modelin g and nanoindentation. Surface and Coatings Technology 195, 287297. Narayan, R., Hobbs, L. W., Jin, C., Rabiei, A., 2006, The use of functionally gradient materials in medicine JOM 58 (7), 5256. Release 10.0 Documentation fo r ANSYS, 2005, SAS IP, Inc. PAGE 70 58Release 10.0 Documentat ion for ANSYS, 2005, Static Hertz Contact Problem solved using CONTA178 elements, ANSYS Verification Manual 63. Sadeghipour, K., Chen, W., Baran, G., 1994. Spherical microindentation process of polymerbased materials: a finite element study J. Phys. D: Appl. Phys. 27, 13001310. Schwarzer, N., Richter, F., and Hecht, G, 1999, Elastic field in a coated halfspace under Hertzian pressure distribution Surface and Coating Technology 114, 191198. Timoshenko, Goodier, Theory of Elasticity, 3rd Ed., Art. 140. Vanimisetti, S.K., Narasimhan, R., 2005, A numerical analysis of spherical indentation response of thin hard films on so ft substrates, Int. J. Solids Struc., in press. PAGE 71 59 Appendices PAGE 72 60Appendix A: Convergence study and MathCAD worksheets A.1: Alphabeta convergence 1 2 3 .165 .2354 .2415 N 1 N 2 N 3 20 30 40 Initial Guesses A c B c c 2.4 .01 .01 Give n 1 A c B c N 1 c 2 A c B c N 2 c 3 A c B c N 3 c A cs B cscs FindA c B cc A cs B cscs 0.2432.4431065.762 PAGE 73 61Appendix A: (Continued) 1 2 3 3.0215.2346.530 N 1 N 2 N 3 20 30 40 Give n 3 A c B c N 3 c 1 A c B c N 1 c 2 A c B c N 2 c A c B c c 7.1.1 1 Initial Guesses A cs B cscs 14.0857.567 0.551 A cs B cs cs FindA c B cc PAGE 74 62Appendix A: (Continued) A.2: MathCAD program fo r force calculations S02 25H SPL 25H csplinexval 02 S02 25H pfieldH 25 x ()interpSPL 25H xval 02S02 25H x len02lengthxval 02 1 P 25H 6.194104 P 25H 2 xval 020xval 02len02x pfieldH 25 x ()x d PAGE 75 63Appendix B: Elem ent definitions B.1: CONTA171 full element definition Release 10.0 Documentation for ANSYS Element Reference  Part I. Element Library  CONTA171 2D 2Node SurfacetoSurface Contact MP ME ST <> <> PR EM <> <> PP ED CONTA171 Element Description CONTA171 is used to repr esent contact and sliding be tween 2D target surfaces ( TARGE169 ) and a deformable surface, defined by this element. The element is applicable to 2D structural and coupled field contact analys es. This element is located on the surfaces of 2D solid, shell, or beam elements without midside nodes ( PLANE42 PLANE67 PLANE182 VISCO106 SHELL51 SHELL208 BEAM3 BEAM23 PLANE13 PLANE55 or MATRIX50 ). It has the same geometric characteristics as the solid, shell, or beam element f ace with which it is connected (see Figure 171.1: "CONTA171 Geometry" ). Contact occurs when the element surface penetrates one of the target segment elements ( TARGE169 ) on a specified target surface. Coulomb and shear stress friction is allowed. See CONTA171 in the ANSYS, Inc. Theory Reference for more details about this element. Other surfacetosurface contact elements ( CONTA172 CONTA173 CONTA174 ) are also available. Figure 171.1 CONTA171 Geometry CONTA171 Input Data The geometry and node locations are shown in Figure 171.1: "CONTA171 Geometry" The element is defined by two nodes (the underl ying solid, shell, or beam element has no PAGE 76 64Appendix B: (Continued) midside nodes). If the underlying solid, shell, or beam elements do have midside nodes, use CONTA172 The element xaxis is along the IJ li ne of the element. The correct node ordering of the contact element is critical for proper detection of contact. The nodes mustbe ordered such that the target must lie to the right side of the contact element when moving from the first contact element node to the second contact element node as in Figure 171.1: "CONTA171 Geometry" See Generating Contact Elements in the ANSYS Contact Technology Guide for more information on generating elements automatically using the ESURF command. The 2D contact surface elements are associat ed with the 2D target segment elements ( TARGE169 ) via a shared real constant set. ANSYS looks for contact only between surfaces with the same real constant set. Fo r modeling either rigidflexible or flexibleflexible contact, one of the deformable surf aces must be represented by a contact surface. See Designating Contact and Target Surfaces in the ANSYS Contact Technology Guide for more information. If more than one target surface will make contact with the same boundary of solid elements, you must define several contact el ements that share the same geometry but relate to separate targets (targets which ha ve different real cons tant numbers), or you must combine the two target surfaces into one (targets that share the same real constant numbers). This element supports various 2D stress stat es, including plane stre ss, plane strain, and axisymmetric states. The stress state is auto matically detected accord ing to the stress state of the underlying element. However, if the underlying element is a superelement, you must use KEYOPT(3) to specify the stress state. A summary of the element input is given in "CONTA171 Input Summary" A general description of elemen t input is given in Element Input For axisymmetric applications see Axisymmetric Elements CONTA171 Input Summary Nodes KEYOPTs Presented below is a list of KEYOPTS av ailable for this element. Included are links to sections in the ANSYS Contact Technology Guide where more information is available on a particular topic. KEYOPT(1) Selects degrees of freedom: PAGE 77 65Appendix B: (Continued) 0 UX, UY 1 UX, UY, TEMP 2 TEMP 3 UX, UY, TEMP, VOLT 4 TEMP, VOLT 5 UX, UY, VOLT 6 VOLT 7 AZ KEYOPT(2) Contact algorithm: 0 Augmented Lagrangian (default) 1  PAGE 78 66Appendix B: (Continued) Penalty function 2 Multipoint constraint (MPC); see Chapter 8: "Multipoint Constraints and Assemblies" in the ANSYS Contact Technology Guide for more information 3 Lagrange multiplier on contact normal and penalty on tangent 4 Pure Lagrange multiplier on contact normal and tangent KEYOPT(3) Stress state when superelements are present: 0 Use with helements (no superelements) 1 Axisymmetric (use with superelements only) 2 Plane stress/Plane strain (u se with superelements only) Plane stress with thickness input (use with superelements only) KEYOPT(4) Location of contac t detection point: 0 On Gauss point (for general cases) 1  PAGE 79 67Appendix B: (Continued) On nodal point normal from contact surface 2 On nodal point normal to target surface Use nodal points only for pointtosurface contact. When using the multipoint constraint (MPC) approach to define surfacebased constraints, use KEYOPT(4) in the following way: set KEYOPT(4) = 1 for a forcedistributed surface, set KEYOPT(4) = 2 for a rigid constraint surface. See Surfacebased Constraints for more information. KEYOPT(5) CNOF/ICONT Automated adjustment: 0 No automated adjustment 1 Close gap with auto CNOF 2 Reduce penetration with auto CNOF 3 Close gap/reduce penetration with auto CNOF 4 Auto ICONT KEYOPT(6) Contact stiffness variation (used to enhance stiffness updating when KEYOPT(10) > 0): PAGE 80 68Appendix B: (Continued) 0 Use default range for stiffness updating 1 Make a nominal refinement to the allowable stiffness range 2 Make an aggressive refinement to the allowable stiffness range KEYOPT(7) Element level time incrementation control: 0 No control 1 Automatic bisection of increment 2 Change in contact predictions made to maintain a reasonable time/load increment 3 Change in contact predictions made to achieve the minimum time/load increment whenever a change in contact status occurs For KEYOPT(7) = 2 or 3, includes automa tic bisection of increment. Activated only if SOLCONTROL ,ON,ON at the procedure level. KEYOPT(8) Asymmetric contact selection: 0  PAGE 81 69Appendix B: (Continued) No action 2 ANSYS internally selects which asymmetric contact pair is used at the solution stage (used only when symmet ry contact is defined). KEYOPT(9) Effect of initial penetration or gap: 0 Include both initial geometrical penetration or gap and offset 1 Exclude both initial geometrical penetration or gap and offset 2 Include both initial geometrical penetrat ion or gap and offset, but with ramped effects 3 Include offset only (exclude initia l geometrical penetration or gap) 4 Include offset only (exclude initial geom etrical penetration or gap), but with ramped effects For KEYOPT(9) = 1, 3, or 4, the indicated initial gap e ffect is considered only if KEYOPT(12) = 4 or 5. KEYOPT(10) Contact stiffness update: 0 Each load step if FKN is redefined during load step (pair based). PAGE 82 70Appendix B: (Continued) 1 Each substep based on mean stress of unde rlying elements from the previous substep (pair based). 2 Each iteration based on current mean stre ss of underlying elements (pair based). 3 Each load step if FKN is redefined during load step (individual element based). 4 Each substep based on mean stress of unde rlying elements from the previous substep (individual element based). 5 Each iteration based on current mean st ress of underlying elements (individual element based). KEYOPT(10) = 0, 1, and 2 are pair based, meaning that the stiffness and settings for ICONT, FTOLN, PINB, PMAX, and PMIN are averaged across all the contact elements in a contact pair. For KEYOPT( 10) = 3, 4, and 5, the stiffness and settings are based on each individual contact element (geometry and material behaviors). KEYOPT(11) Beam/Shell thickness effect: 0 Exclude 1 Include PAGE 83 71Appendix B: (Continued) KEYOPT(12) Behavior of contact surface: 0 Standard 1 Rough 2 No separation (sliding permitted) 3 Bonded 4 No separation (always) 5 Bonded (always) 6 Bonded (initial contact) CONTA171 Output Data The solution output associated with the element is in two forms: Nodal displacements included in the overall nodal solution Additional element output as shown in Table 171.2: "CONTA171 Element Output Definitions" PAGE 84 72Appendix B: (Continued) A general description of so lution output is given in Solution Output See the ANSYS Basic Analysis Guide for ways to view results. The Element Output Definitions ta ble uses the following notation: A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ ETABLE ESOL ]. The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availabi lity of the items in the results file. In either the O or R columns, Y indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and a indicates that the item is not available. Table 171.2: "CONTA171 Element Output Definitions" gives element output. In the results file, the nodal results are obtaine d from its closest integration point. The 2D contact element must be defined in an XY plane and the Yaxis must be the axis of symmetry for axisymmetric analyses. An axisymmetric structure should be modeled in the +X quadrants. This 2D contact element works with any 3D elements in your model. Do not use this element in any model that contains axisymmetric harmonic elements. Node numbering must coincide with the external surface of the underlying solid, shell, or beam element, or with the original elements comprising the superelement. This element is nonlinear and requires a full Newton iterative solution, regardless of whether large or small deflections are specified. The normal contact stiffness factor (FKN) must not be so large as to cause numerical instability. FTOLN, PINB, and FKOP can be changed between load steps or during restart stages. The value of FKN can be smaller when co mbined with the Lagrangian multiplier method, for which FTOLN must be used. You can use this element in nonlinear static or nonlinear full transient analyses. In addition, you can use it in modal anal yses, eigenvalue buckling analyses, and harmonic analyses. For these analysis type s, the program assumes that the initial status of the element (i.e., the status at the completion of the static prestress analysis, if any) does not change. PAGE 85 73Appendix B: (Continued) When nodal detection is used and the cont act node is on the axis of symmetry in an axisymmetric analysis, the contact pre ssure on that node is not accurate since the area of the node is zero. The contact force is accurate in this situation. This element allows birth and death and w ill follow the birth and death status of the underlying solid, shell, beam, or target elements. CONTA171 Product Restrictions When used in the product(s) listed below, the stated productspecific re strictions apply to this element in addition to the general assump tions and restrictions given in the previous section. ANSYS Professional. The MU material prope rty is not allowed. The birth and death special feature is not allowed. The DAMP material property is not allowed. ANSYS Structural. The VOLT DOF (KEYOPT(1) = 3 through 6) is not allowed. The AZ DOF (KEYOPT(1) = 7) is not allowed. ANSYS Mechanical. The AZ DOF (KEYOPT(1) = 7) is not allowed. B.2 TARGE169 full element definition Release 10.0 Documentation for ANSYS Element Reference  Part I. Element Library  TARGE169 2D Target Segment PAGE 86 74Appendix B: (Continued) MP ME ST <> <> PR EM <> <> PP ED TARGE169 Element Description TARGE169 is used to represent various 2D "t arget" surfaces for th e associated contact elements ( CONTA171 CONTA172 and CONTA175 ). The contact elements themselves overlay the solid elements describing the boundary of a deformable body and are potentially in contact with the target surf ace, defined by TARGE169. This target surface is discretized by a set of target segment el ements (TARGE169) and is paired with its associated contact surface via a shared real constant set. You can impose any translational or rotational displacement, temperature, voltage, and magnetic pot ential on the target segment element. You can also impose forces and moments on target elements. See TARGE169 in the ANSYS, Inc. Theory Reference for more details about this element. To represent 3D target surfaces, use TARGE170 a 3D target segment element. For rigid targets, these elements can easily model complex target shapes. For flexible targets, these elements will overlay the solid elements desc ribing the boundary of the deformable target body. Figure 169.1 TARGE169 Geometry TARGE169 Input Data The target surface is modeled through a set of target segments, typically, several target segments comprise one target surface. The target surface can either be rigid or de formable. For modeling rigidflexible contact, the rigid surface must be represented by a ta rget surface. For flexibleflexible contact, one of the deformable surfaces must be overlayed by a target surface. See the ANSYS Contact Technology Guide for more information about de signating contact and target surfaces. The target and associated contact surfaces ar e identified by a shared real constant set. This real constant set includes all real cons tants for both the target and contact elements. Each target surface can be a ssociated with only one cont act surface, and viceversa. However, several contact elements could make up the contact surface and thus come in contact with the same target surface. Likewise several target elements could make up the target surface and thus come in contact w ith the same contact su rface. For either the target or contact surfaces, you can put many elemen ts in a single target or contact surface, PAGE 87 75Appendix B: (Continued) but doing so may increase computational cost. For a more efficient model, localize the contact and target surfaces by splitting the la rge surfaces into smaller target and contact surfaces, each of which contain fewer elements. If one contact surface may contact more than one target surface, you must define duplicate contact surfaces that share the same geom etry but relate to separate targets, that is, have separate real constant set numbers. For any target surface definition, the node or dering of the target segment element is critical for proper detection of contact. Th e nodes must be ordered so that, for a 2D surface, the associated contact elements ( CONTA171 CONTA172 or CONTA175 ) must lie to the right of the target surface when moving from target node I to target node J. For a rigid 2D complete circle, contact must o ccur on the outside of the circle; internal contacting is not allowed. Considerations for Rigid Targets Each target segment is a single el ement with a specific shape, or segment type. The segment types are defined by one, two, or three nodes and a target shape code, TSHAP and are described in Table 169.1: "TARGE169 2D Segment Types, Target Shape Codes, and Nodes" The TSHAP command indicates the ge ometry (shape) of the element. The segment dimensions are defined by a real constant (R1), and the segment location is determined by the nodes. ANSYS supports six 2D segment types; see Table 169.1: "TARGE169 2D Segment Types, Target Shape Codes, and Nodes" 1. The DOF available depends on the setti ng of KEYOPT(1) for the associated contact element. For more informati on, see the element documentation for CONTA171 CONTA172 or CONTA175 2. When creating a circle via direct gene ration, define the real constant R1 before creating the element. Figure 169.2 TARGE169 2D Segment Types For simple rigid target surfaces, you can define the target segment elements individually by direct generation. You must first specify the SHAPE argument for the TSHAP command. When creating circles through direct generation, you mu st also define the real constant R1 before creating the element. Real constant R1 (see Table 169.1: "TARGE169 2D Segment Types, Target Shape Codes, and Nodes" ) defines the radius of the target circle. PAGE 88 76Appendix B: (Continued) For general 2D rigid surfaces, target segmen t elements can be defined by line meshing ( LMESH ). You can also use keypoint meshing ( KMESH ) to generate the pilot node. If the TARGE169 elements will be created via automatic meshing ( LMESH or KMESH ), then the TSHAP command is ignored and ANSYS chooses the correct shape automatically. The pilot node provides a convenient, power ful way to assign boundary conditions such as rotations, translations, moments, temperatur e, and voltage on an entire rigid target surface. You assign the conditions only to the pilot node, eliminating the need to assign boundary conditions to individual nodes and redu cing the chance of error. The pilot node, unlike the other segment types, is used to de fine the degrees of freedom for the entire target surface. This node can be any of the target surface nodes, but it does not have to be. All possible rigid motions of the target su rface will be a combination of a translation and a rotation around the pilot node. The bounda ry conditions (including displacement, rotation, force, moment, temperature, voltage, and magnetic potential) of the entire target surface can be specified only on pilot nodes. For rotation of a rigid body constrained only by a bonded, rigidflexible contact pair with a pilot node, use the MPC algorithm or a su rfacebased constraint as described in Multipoint Constraints and Assemblies Penaltybased algorithms can create undesirable rotational energies in this situation. By default, ANSYS automatically fixes the de gree of freedom for rigid target nodes if they aren't explicitly constrained (KEYOP T(2) = 0). If you wish, you can override the automatic boundary condition settings by setting KEYOPT(2) = 1. By default, the temperature is set to the valu e of TUNIF, and if this has no explicit value the temperature is set to zero. For therma l contact analysis, such as convection and radiation modeling, the behavior of a therma l contact surface (wheth er a nearfield or free surface) is usually based on the contact status. Contact status affects the behavior of the contact surface as follows: If the contact surface is outs ide the pinball region, its beha vior is as a farfield of free surface. In this instance, convecti on/radiation occurs with the ambient temperature. If the contact surface is inside the pinball region, the behavior is as a nearfield surface. PAGE 89 77Appendix B: (Continued) However, the thermal contact surface status is ignored if KEYOPT(3) = 1 is set, and the surface is always treate d as a free surface (see CONTA171 CONTA172 or CONTA175 for details). Considerations for Defo rmable Target Surfaces For general deformable surfaces, you will normally use the ESURF command to overlay the target elements on the bounda ry of the existing mesh. No te that the segment types ( TSHAP command) should not be used for this case. A summary of the element input is given in "TARGE169 Input Summary" A general description of elemen t input is given in Element Input TARGE169 Input Summary Nodes I, J, K (J and K are not required for all segment types) Degrees of Freedom UX, UY, ROTZ, TEMP, VOLT, AZ (ROTZ is used for the pilot node only ) Real Constants R1, R2, [the others are defined through the associated CONTA171 CONTA172 or CONTA175 element] Material Properties None Surface Loads None Body Loads None PAGE 90 78Appendix B: (Continued) Special Features Nonlinear Birth and death KEYOPT(2) Boundary conditions for rigid target nodes: 0 Automatically constrained by ANSYS 1 Specified by user KEYOPT(3) Behavior of thermal contact surface 0 Based on contact status Treated as freesurface KEYOPT(4) DOF set to be constrained on dependent DOF for internallygenerated multipoint constraints (MPCs), used only for a surfacebased constraint where a single pilot node is used for the target element (see SurfaceBased Constraints in the ANSYS Contact Technology Guide for more information): n Enter a three digit value that represents th e DOF set to be constrained. The first to third digits represent ROTZ, UY, UX, re spectively. The numbe r 1 (one) indicates the DOF is active, and the number 0 (zero) indicates the DOF is not active. For example, 011 means that UX and UY will be used in the multipoint constraint. Leading zeros may be omitted; for example, you can enter 1 to indicate that UX is the only active DOF. If KEYOPT(4) = 0 (w hich is the default) or 111, all DOF are constrained. PAGE 91 79Appendix B: (Continued) TARGE169 Output Data The solution output associated with the element is shown in Table 169.2: "TARGE169 Element Output Definitions" The following notation is used: The Element Output Definitions ta ble uses the following notation: A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ ETABLE ESOL ]. The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availabi lity of the items in the results file. In either the O or R columns, Y indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and a indicates that the item is not available. 1. Determined by ANSYS TARGE169 Assumptions and Restrictions The 2D segment element must be defined in an XY plane. For circular arcs, the third node defines the actual center of the circle and must be defined accurately when the element is ge nerated and must be moved consistently with the other nodes during the deformati on process. If the third node is not moved consistently with th e other nodes, the arc shape will change with that node's movement. To ensure the correct behavior, apply all boundary conditions to a pilot node. For parabolic segments, the third point mu st lie at the middle of the parabola. For rigid surfaces, no external forces can be applied on target nodes except on a pilot node. If a pilot node is specified fo r a target surface, ANSYS will ignore the boundary conditions on any nodes of the ta rget surface except for the pilot nodes. For each pilot node, ANSYS automatically defines an internal node and an internal constraint equation. The rotationa l DOF of the pilot node is connected to the translational DOF of the internal node by the internal constraint equation. You cannot use constraint equations or coupling on pilot nodes. Generally speaking, you should not change the R1 real constant between load steps or during restart stages; otherwise ANSYS assumes the radius of the circle varies between the load steps. When using direct generation, th e real constant R1 for circles may be defined before the input of the element nodes. If multiple rigid PAGE 92 80Appendix B: (Continued) circles are defined, each having a differe nt radius, they must be defined by different target surfaces. TARGE169 Product Restrictions There are no productspecific re strictions for this element. 