FINITE ELEMENT ANALYSIS OF BREAST IMPLANTS by Kelly Anne Wilson Thesis submitted to the Faculty of the Virginia Polytechnic

Institute and State University in partial fulfillment of the requirements for the degree of MASTER OF SCIENCE in Engineering Mechanics

Approved:

__________________________ J. W. Grant

______________________ N. E. Dowling

_____________________ B. J. Love

May, 1999 Blacksburg, Virginia

FINITE ELEMENT ANALYSIS OF BREAST IMPLANTS by Kelly Anne Wilson Committee Chairman: J. W. Grant Engineering Mechanics

(ABSTRACT) The Breast Implant Lifetime Study at Virginia Tech, on which this thesis is based, seeks to develop methods and data for predicting the lifetime of saline-filled implants. This research developed Finite Element Analysis (FEA) models to evaluate the stresses that are present in the silicone breast implant material under different loading situations. The FEA work was completed using the commercial codes PATRAN and ABAQUS. PATRAN was used for pre- and post-processing, while ABAQUS was used for the actual analysis and to add fluid and contact elements not supported by PATRAN. Many different loading situations and constraints were applied to these models, as well as variations in the material and model properties. Varying the Poissons ratio of the implant material from 0.45 to 0.49 did not make a significant difference in the results. Changing the elastic modulus of the implant material from the modulus of a Smooth implant to the modulus of a Siltex implant had a noticeable effect on the stress results, increasing the maximum stresses by almost 8%. Changing the modulus of the surrounding tissue had marked effects as well, with stiffer tissue (E=300 psi) decreasing the implants stresses by about 60% as compared to softer tissue (E=100 psi). A ten percent decrease in implant thickness yielded a 17% average increase in stress experienced by the implant. For both the 2.5 radius and the 4 radius tissue models, using CAX4 elements produced higher overall stresses in the tissue with the same loading conditions. However, in the 2.5 tissue model, the implant itself experienced less stress with the CAX4 tissue than the CAX3 tissue. In the 4 tissue model, the implant experienced more stress when surrounded by the CAX4 tissue elements. These models will be combined with implant fatigue data to develop a life prediction method for the implant membrane.

ACKNOWLEDGMENTS
I would like to first thank Dr. J. W. Grant, who advised me through my undergraduate senior research project as well as my graduate work. Not only did he give countless words of advice on the technical aspects of my research, he helped make the mounds of administrative paperwork at Virginia Tech bearable. I would also like to thank Dr. B. Love and Dr. N. Dowling for their support and service on my graduate committee. Their advice on my research as well as my career plans was invaluable. I would also like to thank Mentor Corporation for their financial and technical support of this project.

I would like to thank my labmates, J. Cotton and A. Merkle, for their patience with my idle chatter and complaints about the temperature. John, thanks for sharing the SGI and showing me the UNIX ropes. Andrew, I hope you gain control of the lab soon and bring in a radio to break the silence without me there.

Throughout my six years at Virginia Tech, I have grown intellectually as well as psychologically because of the great experience this university provides. I would like to thank all the friends I have made through my college career, with whom I have shared laughs and tears. Finally, I would like to thank my family for their love and

encouragement, which they have given me unconditionally for 23 years.

ACKNOWLEDGMENTS

iii

TABLE OF CONTENTS
LIST OF FIGURES ................................................................................................ vi LIST OF TABLES ................................................................................................. ix 1.0 INTRODUCTION................................................................................................... 1
1.1 1.2 1.3 RELEVANCE AND MOTIVATION ................................................................... 1 ANATOMY AND PHYSIOLOGY....................................................................... 6 BASICS OF BREAST IMPLANT SURGERY..................................................... 8

2.0

METHODOLOGY................................................................................................ 15
2.1 2.2 2.3 THE FINITE ELEMENT METHOD .................................................................. 15 COMPUTATIONAL TOOLS ............................................................................. 16 PRE-PROCESSING CONSIDERATIONS ......................................................... 17 2.3.1 Element Types ........................................................................................ 17 2.3.2 Loading Situations.................................................................................. 21 ANALYSIS METHOD ....................................................................................... 22

2.4

3.0

GEOMETRIC MODEL FORMULATION........................................................... 24

3.1 IMPLANT PROPERTIES ................................................................................... 24 3.1.1 Mechanical Testing ................................................................................ 24 3.1.2 Poissons Ratio ....................................................................................... 32 3.1.3 Material Thickness ................................................................................. 32 GEOMETRY IN PATRAN................................................................................. 33

3.2

4.0

FINITE ELEMENT MODEL FORMULATION.................................................. 37

4.1 4.2 4.3 4.4 4.5 MODELING THE MEMBRANE ....................................................................... 37 MODELING THE INNER FLUID ..................................................................... 39 MODELING THE CONTACT SURFACE ........................................................ 41 MODELING THE SURROUNDING TISSUE................................................... 42 THE ANALYSIS PROCEDURE ........................................................................ 43

5.0

FINITE ELEMENT MODEL CASE STUDIES ................................................... 51

5.1 FEA MODEL BASIC CASES ............................................................................ 51 5.1.1 Implant Without Surrounding Tissue ..................................................... 51 5.1.2 Implant With Surrounding Tissue .......................................................... 53 VERIFICATION CASES .................................................................................... 57 5.2.1 Internal Pressure Comparison................................................................. 57 5.2.2 Displacement Comparison...................................................................... 59

5.2

TABLE OF CONTENTS

iv

6.0

FINITE ELEMENT MODEL VARIABLE STUDIES ......................................... 60

6.1 6.2 POISSONS RATIO COMPARISON................................................................. 60 ELASTIC MODULUS COMPARISON ............................................................. 64 6.2.1 Elastic Modulus of Implant .................................................................... 64 6.2.2 Elastic Modulus of Surrounding Tissue ................................................. 65 IMPLANT THICKNESS COMPARISON.......................................................... 69 SURROUNDING TISSUE RADIUS COMPARISON ....................................... 72 COMPARISON OF TISSUE ELEMENT TYPE................................................ 74 6.5.1 Element Type of 2.5 Radius Surrounding Tissue................................. 74 6.5.2 Element Type of 4 Radius Surrounding Tissue.................................... 76

6.3 6.4 6.5

7.0 8.0

SUMMARY AND CONCLUSIONS.................................................................... 78 FUTURE WORK .................................................................................................. 81 REFERENCES...................................................................................................... 82 APPENDIX A ....................................................................................................... 84 APPENDIX B........................................................................................................ 90 VITA ................................................................................................................... 100

TABLE OF CONTENTS

LIST OF FIGURES
FIGURE 1.1 FIGURE 1.2 FIGURE 1.3 FIGURE 1.4 FIGURE 2.1 FIGURE 2.2 FIGURE 2.3 FIGURE 2.4 FIGURE 3.1 FIGURE 3.2 FIGURE 3.3 FIGURE 3.4 FIGURE 3.5 FIGURE 3.6 FIGURE 3.7 FIGURE 3.8 FIGURE 3.9 FIGURE 3.10 FIGURE 3.11 FIGURE 3.12 FIGURE 3.13 FIGURE 3.14 FIGURE 3.15 FIGURE 4.1 FIGURE 4.2 FIGURE 4.3 FIGURE 4.4
LIST OF FIGURES

Anatomy of the breast ........................................................................... 7 Submuscular placement of breast implant ............................................ 9 Subglandular placement of breast implant .......................................... 10 Incision locations................................................................................. 12 Common element families .................................................................. 17 Examples of linear and quadratic elements......................................... 18 Cylindrical bodies of revolution shown with reference cross-sections ...................................................................................... 19 Diagram of analysis procedure............................................................ 23 Schematic of relationship between E, , and ................................... 25 Stress-strain data for Smooth sample #1 ............................................. 26 Stress-strain data for Smooth sample #2 ............................................. 27 Stress-strain data for Smooth sample #3 ............................................. 27 Stress-strain data for Siltex sample #1 ................................................ 28 Stress-strain data for Siltex sample #2 ................................................ 28 Stress-strain data for Siltex sample #3 ................................................ 29 Stress-strain data for Siltex sample #4 ................................................ 29 Low-modulus slope area for Smooth sample #2 ................................. 30 Front and back views of filled implant................................................ 34 Side view of filled implant .................................................................. 34 Axisymmetric representation of filled implant ................................... 35 Axisymmetric geometric model of breast implant .............................. 35 Geometric dimensions of implant with surrounding tissue................. 36 Axisymmetric geometric model of breast implant with surrounding tissue ............................................................................... 36 Axisymmetric shell elements .............................................................. 37 SAX1 element ..................................................................................... 37 Coordinate system used for axisymmetric elements ........................... 38 10-element mesh of breast implant model .......................................... 38
vi

FIGURE 4.5 FIGURE 4.6 FIGURE 4.7 FIGURE 4.8 FIGURE 4.9 FIGURE 4.10 FIGURE 4.11 FIGURE 5.1 FIGURE 5.2 FIGURE 5.3 FIGURE 5.4 FIGURE 5.5 FIGURE 5.6 FIGURE 5.7 FIGURE 5.8 FIGURE 5.9 FIGURE 5.10 FIGURE 5.11 FIGURE 6.1 FIGURE 6.2 FIGURE 6.3 FIGURE 6.4 FIGURE 6.5 FIGURE 6.6 FIGURE 6.7 FIGURE 6.8 FIGURE 6.9 FIGURE 6.10 FIGURE 6.11 FIGURE 6.12

48- element mesh of breast implant model ......................................... 38 FAX2 element ..................................................................................... 39 Breast implant mesh with cavity reference node, node 100 ................ 39 Breast implant mesh supported by rigid surface ................................. 41 Axisymmetric solid elements .............................................................. 42 Implant with 2.5 radius surrounding tissue, CAX3 element mesh .... 42 Implant with 2.5 radius surrounding tissue, CAX4 element mesh .... 42 Undeformed 20-element mesh of Example 5.1................................... 51 Deformation and stress levels (psi) for Example 5.1 .......................... 52 Implant with 2.5 radius surrounding tissue, CAX3 elements labeled 53 Implant with 2.5 radius surrounding tissue, nodes labeled................ 53 Deformation and stress levels (psi) for Example 5.2 .......................... 54 Deformation and stress levels (psi) for Example 5.2, implant only.... 54 Implant with 4 radius surrounding tissue, CAX4 elements labeled .. 55 Implant with 4 radius surrounding tissue, nodes labeled................... 55 Deformation and stress levels (psi) for Example 5.3 .......................... 56 Deformation and stress levels (psi) for Example 5.3, implant only.... 56 Deformation and stress levels (psi) for Example 5.4 .......................... 58 Deformation and stress levels (psi) for Example 5.4 .......................... 62 Deformation and stress levels (psi) for Example 6.1 .......................... 62 Deformation and stress levels (psi) for Example 6.2 .......................... 62 Deformation and stress levels (psi) for Example 6.3 .......................... 62 Deformation and stress levels (psi) for Example 6.4 .......................... 62 Deformation and stress levels (psi) for Example 6.5 .......................... 64 Deformation and stress levels (psi) for Example 6.6 .......................... 67 Deformation and stress levels (psi) for Example 6.6, implant only.... 67 Deformation and stress levels (psi) for Example 6.7 .......................... 67 Deformation and stress levels (psi) for Example 6.7, implant only.... 67 Deformation and stress levels (psi) for Example 6.8 .......................... 67 Deformation and stress levels (psi) for Example 6.8, implant only.... 67

LIST OF FIGURES

vii

FIGURE 6.13 FIGURE 6.14 FIGURE 6.15 FIGURE 6.16 FIGURE 6.17 FIGURE 6.18 FIGURE 6.19 FIGURE 6.20 FIGURE 6.21 FIGURE 6.22 FIGURE 6.23 FIGURE 6.24 FIGURE 6.25 FIGURE 6.26

Deformation and stress levels (psi) for Example 6.9 .......................... 70 Deformation and stress levels (psi) for Example 5.4 .......................... 70 Deformation and stress levels (psi) for Example 6.10 ........................ 70 Deformation and stress levels (psi) for Example 6.11 ........................ 70 Deformation and stress levels (psi) for Example 6.12 ........................ 73 Deformation and stress levels (psi) for Example 6.12, implant only.. 73 Deformation and stress levels (psi) for Example 6.13 ........................ 73 Deformation and stress levels (psi) for Example 6.13, implant only.. 73 Deformation and stress levels (psi) for Example 6.14 ........................ 74 Deformation and stress levels (psi) for Example 6.14, implant only.. 74 Deformation and stress levels (psi) for Example 6.15 ........................ 74 Deformation and stress levels (psi) for Example 6.15, implant only.. 74 Deformation and stress levels (psi) for Example 6.16 ........................ 77 Deformation and stress levels (psi) for Example 6.16, implant only.. 77

LIST OF FIGURES

viii

LIST OF TABLES
TABLE 3.1 TABLE 3.2 TABLE 3.3 TABLE 5.1 TABLE 5.2 TABLE 5.3 TABLE 5.4 TABLE 5.5 TABLE 5.6 TABLE 5.7 TABLE 5.8 TABLE 6.1 TABLE 6.2 TABLE 6.3 TABLE 6.4 TABLE 6.5 TABLE 6.6 TABLE 6.7 TABLE 6.8 TABLE 6.9 TABLE 6.10 TABLE 6.11 TABLE 6.12 TABLE 6.13 TABLE 6.14 TABLE 6.15 TABLE 6.16 TABLE 6.17 Elastic modulus results for Smooth samples ........................................ 31 Elastic modulus results for Siltex samples ........................................... 31 Thickness measurements of a Smooth implant .................................... 33 Input data for Example 5.1 ................................................................... 52 Result data for Example 5.1.................................................................. 53 Input data for Example 5.2 ................................................................... 54 Result data Example 5.2 ....................................................................... 55 Input data for Example 5.3 ................................................................... 56 Result data Example 5.3 ....................................................................... 56 Input data for Pressure Verification Example, Example 5.4 ................ 58 Result data for Pressure Verification Example, Example 5.4............... 59 Input data for Pressure Verification Example, Example 5.4 ................ 60 Input data for Example 6.1 ................................................................... 61 Input data for Example 6.2 ................................................................... 61 Input data for Example 6.3 ................................................................... 61 Input data for Example 6.4 ................................................................... 62 Result data for Pressure Verification Example, Example 5.4............... 63 Result data for Example 6.1.................................................................. 63 Result data for Example 6.2.................................................................. 63 Result data for Example 6.3.................................................................. 63 Result data for Example 6.4.................................................................. 64 Input data for Example 6.5 ................................................................... 64 Result data for Example 6.5.................................................................. 65 Input data for Example 6.6 ................................................................... 66 Input data for Example 6.7 ................................................................... 66 Input data for Example 6.8 ................................................................... 67 Result data for Example 6.6.................................................................. 67 Result data for Example 6.7.................................................................. 67

LIST OF TABLES

ix

TABLE 6.18 TABLE 6.19 TABLE 6.20 TABLE 6.21 TABLE 6.22 TABLE 6.23 TABLE 6.24 TABLE 6.25 TABLE 6.26 TABLE 6.27 TABLE 6.28 TABLE 6.29 TABLE 6.30 TABLE 6.31 TABLE 6.32 TABLE 6.33 TABLE 6.34 TABLE 6.35 TABLE 6.36

Result data for Example 6.8.................................................................. 68 Input data for Example 6.9 ................................................................... 69 Input data for Example 5.4 ................................................................... 69 Input data for Example 6.10 ................................................................. 70 Input data for Example 6.11 ................................................................. 70 Result data for Example 6.9.................................................................. 71 Result data for Example 5.4.................................................................. 71 Result data for Example 6.10................................................................ 71 Result data for Example 6.11................................................................ 71 Input data for Example 6.12 ................................................................. 72 Input data for Example 6.13 ................................................................. 73 Result data for Example 6.12................................................................ 73 Result data for Example 6.13................................................................ 73 Input data for Example 6.14 ................................................................. 75 Input data for Example 6.15 ................................................................. 75 Result data for Example 6.14................................................................ 75 Result data for Example 6.15................................................................ 76 Input data for Example 6.16 ................................................................. 77 Result data for Example 6.16................................................................ 77

LIST OF TABLES

1.0 INTRODUCTION
1.1 RELEVANCE AND MOTIVATION
In todays society, more emphasis is placed on physical appearance than ever before. Women are constantly comparing themselves to the perfect bodies of

advertisements, television and cinema. In a psychological study, women associated the female breasts with the most highly prized physical attributes of women, symbols of motherhood and fertility, erotically sensitive and important in sexual relations (Strombeck 174). For many women, having their breasts surgically enhanced improves their physical appearance as well as their self-esteem. Such women need their breasts as concrete and visible evidence that they are real women and worthy of sexual relations and motherhood (Strombeck 175).

Some women are unhappy with the appearance of their breasts because of a mastectomy or other cancer therapy surgery, whereas some are not satisfied with their natural development size or shape. Regardless of the motivation, breast implant surgery has become very popular and a relatively minor procedure. In the last year alone, 122,285 U.S. women opted for the procedure (Drell 1).

Breast augmentation began in the 1940s in the United States as a major procedure using a dermafat graft (skin and subcutaneous fat) from the buttocks. In a large

percentage of these surgeries, the women experienced resorption and infection. In the late 1950s, the introduction of prosthetic materials yielded simplicity, good early results, and increased popularity, but later results were unsatisfactory. Since their invention in the 1960s, silicone implants have been widely used with various useful modifications (Strombeck 312).

Although the initial results with silicone breast implants were positive, there has been astounding controversy surrounding these medical prostheses. When silicone breast implants were introduced in the early 1960s, medical devices were not yet regulated by

CHAPTER 1: INTRODUCTION

the FDA (Vasey 77). In 1976, the FDA was granted authority over medical devices, but only to regulate new medical devices, which did not include these breast prostheses. Safety studies were requested of the breast implant manufacturers at this time, but it was not until 1988 that the FDA required them to submit this data (Vasey 77). By then, there was an increasing prevalence of implant-related problems reported to the FDA, which was beginning to cause significant public concern.

Silicone breast implants were blamed mostly for connective tissue disease linked to the bodys auto-immune response, including lupus, scleroderma, Sjogrens Syndrome, and others. However, women who had been implanted also complained of chronic fatigue, swollen lymph nodes, muscle pain, joint pain, joint swelling, low-grade fever, and night sweats (Vasey 25). Due to the possibility that silicone-gel filled implants could cause these complications, the FDA and the implant manufacturers agreed to ban the use of this type of implant in January 1992. Since this ruling, only saline-filled implants can be used for breast augmentation. However, the FDA amended its policy in April of 1992 to allow silicone-gel filled implants to be used for reconstructive surgery and a limited number of research cases (Vasey 86).

Litigation over breast implants started in 1977 with individual lawsuits, most of which blamed the implant manufacturers for negligence and a lack of sufficient testing, which plaintiffs claimed led to their illnesses. This trend continued, building up to several class action lawsuits against the manufacturers. In March 1994, the largest class action settlement in history to that date was reached between the manufacturers and the several hundred thousand women who registered claims (Frontline 5). Just this past July, Dow-Corning and 170,000 women who filed a class action suit reached a 3.2 billion dollar compensation agreement (Josefson 1).

The manufacturers spent billions of dollars compensating women who claimed links between their ruptured implants and connective tissue disorders. However, they maintained that these settlements were not an admission of guilt. They contested that

CHAPTER 1: INTRODUCTION

there is no scientific evidence linking silicone breast implants with autoimmune diseases. More than 20 studies failed to find a link, including experiments led by several prestigious medical organizations, including the American Medical Association, the American College of Rheumatology, and the American Society of Plastic and Reconstructive Surgery (Josefson 1).

The British governments Independent Review Group, which is responsible for investigating breast implants, recently cleared implants of causing illness. The report, the third in six years to proclaim the devices safe, stated that women with silicone gel breast implants are at no greater risk of connective tissue disease or an abnormal inflammatory response than those without. The group also determined that the common complaints such as fatigue and muscle weakness are symptomatic of a low-grade infection, which can occur with any type of implant. The report concludes that no further studies into the issue of connective disease can be justified, but it recommends more research into nonspecific symptoms, particularly the incidence of rupture and the possible cause of symptoms (Kmietowicz 1).

Breast implant research has been occupied for years with studying the safety of these silicone prostheses. Now that silicone implants have been cleared of causing connective tissue disorders, research can study the many other mysteries surrounding these controversial medical devices.

One of the most discussed issues is the rupturing of implants, a topic of great concern for women who have had the operation. When breast implants were introduced into the plastic surgery market, Dow-Corning printed in the accompanying literature given to women that Based on laboratory findings together with human experience to date, one would expect that a mammary prosthesis would last for a natural lifetime (Byrne 54). As decades of headlining news stories have told the country, this is obviously not the case. The manufacturers as well as breast implant recipients know that their prostheses will surely not last a lifetime. But how long will the implants last?

CHAPTER 1: INTRODUCTION

The research supporting this thesis is part of one such study to determine the lifetime of a breast implant. This study is funded by the Mentor Corporation, one of two companies still manufacturing breast implants. The overall project is divided into several sections, all of which will combine to develop methods and data to predict an implants lifetime. One section of the project is to determine the usage spectrum of the implant, which involves determining what types of loading events the implant experiences and what number of these events occur. Another section is to study the mechanical properties of the implant material, through mechanical testing and fatigue tests. A third section is to study the biological effects of these implants being in the human body, through materials aging studies and chemical studies. A fourth section is to determine the stress levels experienced by the implant material, through stress analysis with Finite Element Analysis (FEA) methods. These four sections will combine to form the final section of the study, the life prediction.

The basic approach for this lifetime study is a stress-based approach to fatigue life prediction which incorporates variable amplitude loading. This approach accounts for the combined effect of various loading events, ranging from low stress situations to very high stress situations, and the number of these events. This life prediction involves the following algorithm:

1. For each type of loading event, determine the cyclic stress range in the implant material. (From FEA results) 2. Use the stress vs. cycles to failure curve (S-N curve) for the implant material to determine the life, Nfi , for the particular loading event. (From mechanical and chemical testing) 3. Determine the number of occurrences per year, Ni , of the loading event. (From usage spectrum results) 4. Find the life fraction per year for this event: Ni Nfi

Repeat steps 1-4 to find the life fractions for all events of interest.
CHAPTER 1: INTRODUCTION 4

5. To estimate the number of years to failure, Yf , use the Palmgren-Miner Rule Yf = 1 Ni peryear Nfi

by finding the sum of all the life fractions found in Step 4 and taking its inverse.

As shown by this procedure, the four sections leading up to the life prediction stage are crucial to the determination of the implant lifetime. This thesis will provide the background work for Step 1 described above, which is to determine the stress ranges in the implant material. Its purpose is to develop a finite element model of the silicone implant shell and to analyze the stresses in the model with many different loading conditions.

The remainder of this introduction will review the basic anatomy and physiology of the breast as well as the techniques of the implant surgery. Chapter 2 explains the basic methodology of finite element analysis and how it is applied to the breast implant model. Chapter 3 discusses the geometric model formulation, including the material studies of the implant. Chapter 4 discusses the finite element model formulation and presents an example of an analysis code, explaining each step. Chapters 5 and 6 review the many cases analyzed with different meshes, loading conditions, displacement conditions, and material properties. Finally, Chapter 7 summarizes the research, and Chapter 8 recommends future work on this project.

CHAPTER 1: INTRODUCTION

1.2 ANATOMY AND PHYSIOLOGY

In order to understand the breast model and its many variables, it is necessary to have a basic understanding of the anatomy of the female breast, shown in Figure 1.1. The breast consists of the mammary glands and adipose tissue. Adipose tissue is fat-storing loose connective tissue which determines the size of the breast. The mammary glands are modified sweat glands that are responsible for milk production. Each gland consists of 15 to 20 lobes separated by adipose tissue. In each lobe of the mammary gland are smaller sections called lobules, which contain milk-secreting glands called alveoli. The alveoli convey the milk into secondary tubules and further to the mammary ducts. As the mammary ducts approach the nipple, they expand to form the lactiferous sinuses. These sinuses store the milk until it is transferred through the lactiferous ducts, which terminate in the nipple. The circular area of pigmented skin around the nipple is the areola (Tortora 946).

The breast lies over the pectoralis major and minor muscles and is attached to them by a layer of connective tissue. Strands of connective tissue called the suspensory ligaments of the breast run between the skin and deep fascia, supporting the breast (Tortora 946).

CHAPTER 1: INTRODUCTION

Suspensory ligament of the breast (Coopers ligament) Secondary tubule Mammary duct Lactiferou s sinus Lactiferou s duct Fat in superficial fascia Areola Nipple

Intercostal muscles Deep fascia Pectoralis major muscle

Nipple Areola Lobule containing alveoli

Rib Fat in superficial fascia

Figure 1.1 Anatomy of the breast.

CHAPTER 1: INTRODUCTION

1.3 BASICS OF BREAST IMPLANT SURGERY

Breast implant surgery is based on one underlying concept: to clear a pocket in the breast and insert an implant into this pocket. However, there are many different options for a surgeon to consider. Based on the individual patient, a surgeon must decide what type of implant to select, where to place the implant, and where to make the incision.

Because the type of implant does not significantly affect the surgical technique, this consideration will be discussed in the Implant Properties section later in this thesis (Section 3.1).

There are two general approaches to the placement of breast implants: the submuscular approach and the subglandular approach. In the submuscular approach, the implant is placed beneath the pectoralis major muscle. As shown in Figure 1.2, the upper part of the implant is between the pectoralis major and minor muscles, while the lower part is between the mammary gland and the connective tissue in front of the ribcage. In the subglandular approach, the implant is placed in front of both pectoralis muscles and behind the mammary glands and natural breast adipose tissue, as shown in Figure 1.3.

CHAPTER 1: INTRODUCTION

Pectoralis major muscle

Pectoralis minor muscle

Mammary glands

Breast implant

Figure 1.2 Submuscular placement of breast implant.

CHAPTER 1: INTRODUCTION

Mammary glands

Pectoralis muscles

Breast implant

Figure 1.3 Subglandular placement of breast implant.

CHAPTER 1: INTRODUCTION

10

Although the placement decision is dependent on the patients anatomy and the surgeons personal preference, there are some general trends observed with the two approaches. If the submuscular approach is used, there is less likelihood of feeling the implant through the skin and a decrease in capsular contracture. This contracting

capsule of hardened tissue forms in 10 to 30% of breast implant patients, and can lead to distortion of the breast and a poor aesthetic result (Bern 1037). The submuscular However, the

approach also lessens the implants interference in mammography.

appearance of the breast will change with flexure of the pectoralis major muscle. In addition, in some women who already have significant breast tissue, the natural tissue will drop with time while the implant remains supported by the muscle, causing a bilobed breast. With the subglandular approach there may be less postoperative pain and a more natural appearance for some women (Plastic Surgery Info. Service 4). Due to the many small blood vessels in this location, there may be more bleeding. Capsular

contracture is an increased risk with the subglandular approach as well (Hudson 1) .

Another decision a patient and surgeon must consider is the placement of the incision itself. The most common choices are axillary, submammary, periareolar, and endoscopic incisions, the first three of which are shown in Figure 1.4. An axillary incision is a cut in the armpit, which is a direct route to the pocket, and is commonly used for the submuscular approach. A submammary incision is made on the undersurface of the breast, in the crease where the breast meets the chest. This incision is also a direct route to the pocket. A periareolar incision is made around one-third of the

circumference of the areola, surrounding the nipple. The endoscopic incision, the least used, is an incision in the navel. The surgeon then burrows up under the skin into the breast area.

CHAPTER 1: INTRODUCTION

11

Periareolar incision

Axillary incision

Submammary incision

Figure 1.4 Incision locations.

CHAPTER 1: INTRODUCTION

12

Once these decisions are made by the patient and surgeon, the breast augmentation surgery is performed with the same general method. Although either local or general anesthesia can be administered, most surgeons and patients prefer general anesthesia for patient comfort. Once the patient is sedated, the surgeon makes the

incision and reaches the pocket area. Using various surgical tools and tissue expanders, the surgeon stretches out the skin and clears room for the implant. When silicone gelfilled implants were used, the implants were pre-filled and sealed by the manufacturer and larger incisions were required. With the current saline-filled implants, the empty implant is inserted into the pocket area with the injection dome and filling tube still attached. The surgeon fills the implanted capsule with saline to the desired volume and repeats the entire process for the other breast. The breasts are then checked for symmetry in the horizontal position and often with the table tilted up at least 45. Depending on the patients skin flexibility, the surgeon can fill the implants to the desired volume during the initial surgery, or increase the volume periodically over a few weeks. With the former choice, the injection dome and filling tube are removed during the initial surgery and the incision is stitched. For the latter technique the filling tube is left connected to the implant and the injection tube left just under the skins surface so that it can be easily accessed with a hypodermic needle in an office setting. Once the implants are at the desired volume, the injection dome and filling tube are removed. Although this tube can be left implanted up to six months from the surgery, it is usually removed in three to four months. A self-sealing valve in the implant shell allows the tube to be gently pulled out without having to access the implant itself. This slow-filling method may decrease capsular contracture and gives the patient more flexibility in the final breast implant volume achieved.

With an understanding of the anatomy of the breast and the surgical techniques of breast augmentation, one can start to see the many variables involved in modeling the breast implant membrane. Because this research studies an object implanted into the human body, there are chemical and physical patient-dependent factors that could never be individually modeled. This thesis will present models with many different loading

CHAPTER 1: INTRODUCTION

13

cases which represent a generalization of implant situations, generating membrane stress ranges which are not exact, but a realistic look at the stress levels which an average implant experiences.

CHAPTER 1: INTRODUCTION

14

2.0 METHODOLOGY
2.1 THE FINITE ELEMENT METHOD
Many problems in engineering and science, including the breast implant model, involve complicated systems of differential equations which are too difficult to exactly solve due to their complex geometry. Finite element analysis, which has evolved over the past three decades, involves a method of breaking up a continuum into discrete, coupled components that approximate the overall solution. The geometric domain is broken into these non-overlapping coupled components called elements. These elements are

represented by a linear combination of polynomial functions with undetermined coefficients, which form the approximate numerical solution to the governing differential equations. The undetermined coefficients are represented by nodes, which are located on the element. The solutions are found at these nodes using the polynomial functions and prescribed boundary conditions. The linear combination of the assumed algebraic

polynomials forms the continuous solution. Thus the simplified local representations are patched together to form an approximate global solution.

Because the local form of the solution needs to be kept simple, accuracy is increased by making the elements as small as possible. This makes the approximation defined by a larger number of equations, which increases with every increase in the number of elements used. However, it reduces the differential equation into many

algebraic equations, which leads to the possibility of solving more complicated problems.

Although finite element analysis (FEA) was originally done with personally written computer programs to carry out the analysis, there are many commercially available computer programs now which eliminate the need to write an individual code. This chapter will describe the FEA packages used for this project, the types of elements considered, and the analysis method.

CHAPTER 2: METHODOLOGY

15

2.2 COMPUTATIONAL TOOLS

The computational finite element analyses were performed on UNIX-based Silicon Graphics workstations. The pre-processing, which includes the geometric models and initial finite element models, was completed using PATRAN v.6 software. Some additional elements not supported by PATRAN, which are described later, were added using ABAQUS v.5.6. The ABAQUS algorithm also was the main processor, which analyzed the actual load cases and geometries. PATRAN was used again for postprocessing, which involved analyzing and viewing the various results cases.

The basic method for performing the analysis has several steps utilizing both PATRAN and ABAQUS. The geometric breast implant model is first created using the computer aided design (CAD)-like capabilities of PATRAN. The next step is to select an element type and decide how many elements to use. This step is called meshing the geometry. A course mesh is a rough approximation of the overall solution, and does not involve large computing time. A fine mesh will be a better approximation of the actual solution, and involves significantly larger computation time. At this point, the accuracy of the solution needed must be weighed against the computation time available to determine how fine a mesh should be used.

Once the mesh is created, the elements are associated with the actual material involved so that the behavior of the silicone rubber is accounted for in the model. The next step is to impose the necessary boundary conditions and simulated loading on the finite element model. After adding fluid and contact elements using ABAQUS,

ABAQUS performs the analysis. Finally, the results are exported from ABAQUS back to PATRAN and viewed there. This process will be explained in much further detail throughout the course of this thesis.

CHAPTER 2: METHODOLOGY

16

2.3 PRE-PROCESSING CONSIDERATIONS

2.3.1 Element Types One of the first considerations in creating a finite element model is what element type to use. Five aspects of an element characterize its behavior in ABAQUS: family, degrees of freedom, number of nodes, formulation, and integration. Figure 2.1 shows the element families that are used most commonly in a stress analysis.

Shell elements Continuum (solid) elements Beam elements

Rigid elements

Connector elements such as dashpots

Figure 2.1 Common element families.

One major difference between these element families is the geometry type that each family assumes. The degrees of freedom are the fundamental variables calculated during the analysis. For example, in a stress/displacement simulation with shell and beam elements, the degrees of freedom are the translations and rotations at each node. The number of nodes per element determine the order of interpolation over that element. Once the degrees of freedom are calculated at the elements nodes, the same variables are determined at any other point in the element using interpolation from the nodes. For elements with nodes only at their corners, as in Figure 2.2, linear interpolation is used between the nodes, making these linear or first-order elements. Elements with midside nodes, as shown in Figure 2.2, use quadratic interpolation and are called quadratic or

CHAPTER 2: METHODOLOGY

17

second-order elements. The formulation of an element refers to the mathematical theory used to define the elements behavior. All of ABAQUS stress/displacement elements are based on the Langrangian description of behavior, whereas Eulerian elements are used in modeling heat transfer. ABAQUS uses numerical methods to evaluate the material response at each integration point in each element, allowing complete generality in material behavior. In choosing an element type, full or reduced integration must be chosen, which can significantly affect the elements accuracy. In summation, all five of these aspects must be considered in choosing an appropriate element type for one application (ABAQUS 13.1.1).

Linear element (8-node brick, C3D8)

Quadratic element (20-node brick, C3D20)

Figure 2.2 Examples of linear and quadratic elements.

As shown above in Figure 2.1, there are two element types that could apply for the curved breast implant capsule shape: shell and membrane elements. Shell elements are curved structural elements of constant thickness, which is small compared to the other two dimensions. The basic approach is that by integrating over the thickness, a two dimensional model is formulated on the midsurface of the shell (shown in dotted lines in Figure 2.1), which approximates the three dimensional model. There are two different theories associated with shell elements, membrane theory and bending or general theory. The membrane elements, which follow membrane theory, are used to represent thin surfaces that offer in-plane strength but no bending stiffness, like a balloon (ABAQUS 15.1.1-1). These elements only consider membrane forces, not moments or shear forces, and therefore do not require material properties. The shell elements, which follow the

CHAPTER 2: METHODOLOGY

18

bending or general theory, consider both the membrane forces and the bending effects (moments and shear forces). In summary, membrane elements are a simplified form of shell elements which consider membrane forces only. Shell elements consider bending effects as well as membrane effects (Ugural 199).

Another

element

option

to

be

considered

is

axisymmetric

elements.

Axisymmetric elements provide for the modeling of bodies of revolution under axially symmetric loading conditions. A body of revolution is generated by revolving a plane cross-section about the symmetry axis and can be described in polar coordinates (r, z, and ) (ABAQUS 13.1.2-4). Figure 2.3 shows a reference cross-section at = 0 and the corresponding body of revolution is the cylindrical solid shown with dotted lines.
z(Y)

Cross section at =0

r(X)

Figure 2.3 Cylindrical bodies of revolution shown with reference cross-sections.

The advantage of using axisymmetric elements comes through the simplification of the problem. If the loading and material properties are independent of , the solution in any

CHAPTER 2: METHODOLOGY

19

r-z plane defines the solution over the whole body (ABAQUS 13.1.2-4). Therefore, the whole three dimensional problem can be solved by discretizing the reference crosssection, which significantly reduces both modeling time and computing time.

For the breast implant model, axisymmetric shell elements were chosen, which follow general shell theory. Although the bending effects should be minimal compared to the membrane stresses in this model, shell elements were chosen to see if bending effects could be neglected. In addition, membrane theory fails to predict the state of stress at the boundary and in certain other areas of the shell. These shortcomings are avoided by the application of bending theory, considering membrane forces, shear forces, and moments to act on the shell structure (Ugural 231). The axisymmetric nature of the shell elements allow the modeling of the entire three dimensional structure with a single two dimensional reference cross-section. Therefore, the axisymmetric shell elements were the best choice for the breast implant capsule.

In order to model the fluid-filled nature of the breast implants interior, fluid elements were also needed. Because ABAQUS only has one type of axisymmetric fluid element, choosing a fluid element type was a simpler task to complete. ABAQUS supports hydrostatic fluid elements, which are applicable for fluid-filled cavities which have uniform pressure and temperature at any point in time. The fluid elements share a common cavity reference node, located somewhere in the fluid cavity, which has a single degree of freedom representing the pressure inside the cavity (ABAQUS 18.2.1-2). The breast implants saline-filled cavity was represented with axisymmetric fluid elements around the boundary of the cavity, which will be demonstrated later in the detailed modeling.

CHAPTER 2: METHODOLOGY

20

2.3.2 Loading Situations Before creating a finite element model, a general idea of what types of loading situations to be considered may help with the modeling itself. Discussions with Dr. Kel Cohen, a plastic surgeon at the Medical College of Virginia, provided a surgeons experience on where ruptured implants usually fail and why this may occur. There are three main types of failure causes: edge creases, low stress / repeated loading, and high stress / short duration loading.

Edge creases, folds in the edge of the implant capsule, are almost always the location of implant failure when they develop. The creases act as a stress raiser and thus fail with much fewer cycles than without the crease. Many of Dr. Cohens patients experience implant failure due to this imperfection (Cohen 1997).

The low stress / repeated loading situation involves activities which do not put a high level of stress on the implant, but cause a failure with enough repetitions over time. This is called cyclic loading, and can be likened to bending a paper clip in half, unbending it, and repeating. Bending the paper clip once doesnt break it, but after bending it enough times, this cyclic loading effect causes the metal to fail. For the breast implant, there are many situations that can be in this classification. Some are static loading examples, such as sleeping on the stomach and wearing a tight athletic bra. There are many dynamic examples as well, such as running, walking, and playing tennis. Although breast implants were initially used for breast cancer reconstruction in older patients, the majority of implants are cosmetic augmentations for more active younger women. Therefore, athletic activity commonly puts this type of dynamic loading on the implants.

The high stress / short duration loading situation involves rapid impact situations, which put a very high stress level on the implant in an instantaneous manner. Severe chest trauma, such as a blow to the chest or car accident injury, are examples of this type

CHAPTER 2: METHODOLOGY

21

of loading situation. These experiences would obviously cause implant rupture in many cases, but are not easily studied or controlled by the implant manufacturer.

This thesis will begin the modeling process by looking at the low stress / repeated loading situation. Even though the FEA model does not consider the repetition of the loading, it will determine what stresses are created in the implant capsule under these smaller loading situations. The fatigue analysis will combine the stress ranges with the number of cycles of loading. Eventually, this model would like to include the edge crease effect, but that will be reserved for future work on this project. The high stress / short duration loading conditions, which are essentially through chest trauma, will not be considered. This type of loading is an unusual effect that is beyond the normal usage spectrum of a breast implant.

2.4 ANALYSIS METHOD

The PATRAN software package supports many different analysis packages, one of which is ABAQUS. PATRAN has a conversion program which creates an ABAQUS input file from the geometry description created in PATRAN. After the model is created in PATRAN, as described in Section 2.2, the conversion program PAT3ABA translates the PATRAN model into an ABAQUS input file. The ABAQUS input file can be viewed in a text editor, as was done for this project using JOT software on the Silicon Graphics desktop. This is necessary for adding elements or commands not supported by PATRAN, such as the fluid elements needed for this model. The JOT software is also useful for editing the ABAQUS input file after an analysis has revealed programming errors. The errors can be changed directly in the ABAQUS program more efficiently than changing the model in PATRAN and re-creating the ABAQUS input file. After the input file has been completed in the text editor, it is submitted to ABAQUS for the processing analysis. After the analysis is complete, another conversion program in PATRAN called ABAPAT3 converts the ABAQUS results file into a PATRAN results file so that the result variables can be viewed in the PATRAN graphics. The most efficient method is to view the ABAQUS results file using the text editor, in order to see the errors and results

CHAPTER 2: METHODOLOGY

22

from each analysis. Once the ABAQUS analysis is satisfactory, ABAPAT3 is used to translate the results to PATRAN. This process is illustrated in Figure 2.4.

PATRAN

PATRAN model created

Results viewed in PATRAN

File converted into ABAQUS input file using PAT3ABA

File converted into PATRAN using ABAPAT3

ABAQUS input file edited and submitted for analysis

ABAQUS results file created

View results file

ABAQUS
If errors or unsatisfactory results exist, edit ABAQUS input file

Resubmit analysis to ABAQUS

Figure 2.4 Diagram of analysis procedure.

CHAPTER 2: METHODOLOGY

23

3.0 GEOMETRIC MODEL FORMULATION

As described in Chapter 2, the first step in the finite element modeling process is to create the geometric model to serve as the basis for the FEA model. In order to understand the geometry of the breast implant, variations in implant sizes, material types, and wall thickness were first studied. This chapter will discuss the mechanical testing and other research to determine the material properties of the implant material. It will then discuss the creation of the geometric model in PATRAN.

3.1 IMPLANT PROPERTIES

Every breast implant manufacturer has various implant sizes and types available. Mentor Corporation supplied many different sample sizes for this research, which are designated by the minimum volume of saline they can contain. In addition to size variations, there are two different implant material types to choose from with Mentor breast implants. Although both are made of a silicone rubber-like solid material, the Siltex model has a textured, slightly opaque outer surface. The Smooth model has a shiny, smooth transparent surface. With these observations and some general product literature, it was concluded that the silicone implant capsule was an elastomeric material, but additional material information was needed.

3.1.1 Mechanical Testing Beyond the general material description given above, no detailed material information was provided by the Mentor Corporation. In order to perform a static stress analysis, one of the basic material properties needed is the elastic modulus, E. Hookes law, =E

(Equation 3.1)

states that the stress, , is directly proportional to the strain, , within the elastic limit of the material. The elastic modulus, E, the coefficient in Hookes law, has units of stress,

CHAPTER 3: GEOMETRIC MODEL FORMULATION

24

since the strain is dimensionless. Figure 3.1 shows a schematic of the relationship between the stress, strain and elastic modulus. As Hookes law shows, the elastic

modulus is needed for the analysis to determine the amount of stress associated with a given strain.

Stress

Slope = E

0 0 Strain

Figure 3.1 Schematic of relationship between E, and . Although Figure 3.1 above shows the stress-strain relationship as strictly linear, real materials do not behave this way beyond small strains. This region, the linear elastic region, will give way to a plastic deformation region, in which the deformation is not recoverable. Because the breast implant shell is an elastomeric material, the silicone rubber should elastically stretch a significant amount as the molecular cross-links and chains stretch out. However, elastomers can stiffen as the chains straighten, and this varies depending on the type of material being considered. Many elastomeric models are available which account for the modulus changes with deformation. However, the best approach is to test the material directly and observe its stress-strain response.

For the mechanical testing, dogbone samples were punched from the front center of the implants, away from the patch and edge (or radius) areas. Three samples were taken from Smooth implants and four were taken from Siltex implants. The resulting samples were 7.10 mm in length and 2.89 mm in width, with thicknesses varying from

CHAPTER 3: GEOMETRIC MODEL FORMULATION

25

0.48 to 0.53 mm for the Smooth samples and 0.69 to 0.74 mm for the Siltex samples. These specimens were punched with this small scale in order to be tested in a Miniature Materials Tester (Minimat). This is a desktop size loadframe with a lower maximum load than a conventional mechanical test frame. The smaller load cell for the Minimat is much more sensitive to small loads.

The Minimat is driven by a PC computer program which collects the load versus extension data as the motor pulls the specimen at a given rate. The stress vs. strain data is then derived from the load vs. extension data. After tightening the grips onto the ends of each specimen, the samples were pulled at a strain rate of 10 millimeters per minute up to about 400% strain. Although strain rate does affect stress-strain behavior, the low strain rate was chosen to represent slow fatigue wear. The resulting stress-strain data is shown below in Figures 3.2 through 3.8.

Smooth Sample #1
1.2 1 0.8 0.6 0.4 0.2 0 0 50 100 150 200 Strain, % 250 300 350 400

Stress, MPa

Figure 3.2 Stress-strain data for Smooth sample #1.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

26

Smooth Sample #2
1.2 1 0.8 0.6 0.4 0.2 0 0 50 100 150 200 Strain, % 250 300 350 400

Stress, MPa

Figure 3.3 Stress-strain data for Smooth sample #2.

Smooth Sample #3
1.2 1 Stress,MPa 0.8 0.6 0.4 0.2 0 0 50 100 150 200 Strain, % 250 300 350 400

Figure 3.4 Stress-strain data for Smooth sample #3.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

27

Siltex Sample #1
1.8 1.5 1.2 Stress, MPa 0.9 0.6 0.3 0 0 50 100 150 200 Strain, % 250 300 350 400

Figure 3.5 Stress-strain data for Siltex sample #1.

Siltex Sample #2
1.2 1 0.8 0.6 0.4 0.2 0 0 50 100 150 200 Strain, % 250 300 350 400

Stress, MPa

Figure 3.6 Stress-strain data for Siltex sample #2.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

28

Siltex Sample #3
0.9 0.8 0.7 Stress. MPa 0.6 0.5 0.4 0.3 0.2 0.1 0 0 50 100 150 200 Strain, % 250 300 350 400

Figure 3.7 Stress-strain data for Siltex sample #3.

Siltex Sample #4
1.2

0.9 Stress, MPa

0.6

0.3

0 0 50 100 150 200 Strain, % 250 300 350 400

Figure 3.8 Stress-strain data for Siltex sample #4.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

29

Both the Smooth and Siltex stress-strain curves have a varying slope, starting with one slope and then gradually changing to a second lower modulus slope. Physically, this is elastomeric material behavior, which is represented by an initial stiffness resisting extension of the material, which becomes more ductile after a certain strain. For the Smooth samples, Figures 3.2 to 3.4, the first approximately 40% is at a higher modulus than beyond 40% strain. For the Siltex samples, Figures 3.5 to 3.8, the modulus change is shown by a change in slope at about 50% strain. The elastic modulus was calculated by fitting a line through the data in each region and finding the slope of each, as shown in Figure 3.9 for the low modulus stress-strain data. Tables 3.1 and 3.2 summarize the elastic modulus results.

Smooth Sample #2
0.35 0.3 Stress, MPa 0.25 0.2 0.15 0.1 0.05 0 0 0.1 0.2 Strain 0.3 0.4 Data Linear Trendline

Figure 3.9 Low-modulus slope area for Smooth sample #2.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

30

Table 3.1 Elastic modulus results for Smooth samples. Sample Type Low Strain (<40%) Modulus, E < MPa Smooth #1 Smooth #2 Smooth #3 Average 0.5695 0.6924 0.5448 0.6022 psi 82.60 100.43 79.02 87.35 High Strain (>40%) Modulus, E > MPa 0.2353 0.2411 0.2654 0.2473 psi 34.13 34.97 38.50 35.87

Table 3.2 Elastic modulus results for Siltex samples. Sample Type Low Strain (<50%) Modulus, E < MPa Siltex #1 Siltex #2 Siltex #3 Siltex #4 Average 0.5838 0.4289 0.5566 0.5872 0.5391 psi 84.67 62.20 80.73 85.16 78.19 High Strain (>50%) Modulus, E > MPa 0.3981 0.1810 0.1228 0.2336 0.2339 psi 57.74 26.25 17.81 33.88 33.92

As the modulus data in Tables 3.1 and 3.2 show, the elastic modulus decreases significantly once the strain traverses the threshold strain. For the Smooth implants, the average low-strain modulus is about 87 psi, which decreases by 59% to about 36 psi beyond 40% strain. For the Siltex implants, the average modulus below 50% strain is 78 psi, which decreases by 56% to 34 psi beyond 50% strain. Which modulus should be used for the FEA model? Since this research is analyzing low-stress loading situations, strains within 40-50% are well within the testing situations. For a Smooth implant, an elastic modulus of 100 psi is used for the implant capsule material. Although this is higher than the average modulus for Smooth implants, this value had already been used previously for the model and was retained for consistency. For a Siltex implant, 78 psi is used for the materials elastic modulus. Therefore, a linear model was used with constant elastic modulus based on the testing results.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

31

3.1.2 Poissons Ratio Another material property needed for the static stress analysis is the Poissons ratio, . When a tensile stress is applied to a specimen, elongation and strain results in the direction of the applied stress. However, this elongation will also cause constrictions in the directions perpendicular to the applied stress. The Poissons ratio is the absolute value of the ratio of lateral strain to axial strain, as shown in Equation 3.2.

lateralstrain axialstrain

(Equation 3.2)

Although this ratio varies for different materials, the Poissons ratio is 0.5 if the assumption of no volume change is assumed. For the breast implant material, it can be assumed that there is little or no net volume change with the implants deformation. However, using a Poissons ratio of 0.5 causes numerical problems for the finite element analysis. For the model, cases with Poissons ratio varying from 0.45 to 0.49 were tested, which will be discussed in the FEA Model Variable Studies, Chapter 6. This range is also realistic since elastomeric materials are often in the Poissons ratio range of 0.4 to 0.5, although no specific data for the breast implant silicone rubber could be found (Andrew).

3.1.3 Material Thickness It is obviously crucial to the stress analysis to know the thickness of the material in question before creating the geometry. It is also necessary to look at variations in this thickness at different locations in the implant capsule, to determine whether a uniform thickness can be approximated. Cutting open a Smooth implant with a 225 cc minimum fill level and measuring the thickness with a pair of calipers showed some variation in thickness. Table 3.3 shows that the silicone implant material is about 0.019 thick, except in the slightly thicker patch area.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

32

Table 3.3 Thickness measurements of a Smooth implant. Sample location back, patch area back, away from patch edge (radius) front, several locations front center Thickness, inches (mm) 0.023 (0.584) 0.018 (0.457) 0.019 (0.483) 0.018-0.019 (0.457-0.483) 0.019 (0.483)

For the purposes of the stress analysis, the thickness does not vary enough to be considered non-uniform. Therefore, a material thickness of 0.019 is assumed for the Smooth implant.

3.2 GEOMETRY IN PATRAN

Once the general material properties of the capsule material were found, the next step was to create the geometric model using PATRAN graphics. Because there are different materials and model volumes available, one sample type was chosen for the initial model. A Mentor Smooth implant with a minimum volume level of 225 cc was chosen. The Smooth material type was chosen because of its popularity with plastic surgeons. It is easier to fold when empty, easier to implant with smaller incisions, and results in less encapsulation. The volume chosen is a mid-range volume which is

commonly used for both cosmetic and reconstructive surgery.

In order to obtain geometric measurements on which to base the mathematical model, the implant was filled with 250 cc of tap water using a 60 cc syringe with an 18 gauge needle. After injecting the desired volume of water through the injection dome and filling tube, the empty syringe was left penetrating the injection dome and the air bubbles were extracted from the filled implant. Laying the implant on a table with the back (patch side) down, the general geometric shape was easily observed. Looking from above at the front of the implant, the diameter at its widest place, which is the edge or radius, is 4.25

CHAPTER 3: GEOMETRIC MODEL FORMULATION

33

inches. Figure 3.10 shows the front and back of the implant, which would be the top and underside views while the implant is lying on the table.

FRONT

BACK

patch

d = 4.25

d = 4.25

Figure 3.10 Front and back views of filled implant. Looking at the side view of the implant, with eye-level at the height of the table, the tallest part of the implant is at its center. The height at the center measures 1.3 from the bottom of the implant (on the table surface) to the top, as shown in Figure 3.11. This geometric information was sufficient to create the PATRAN model, since it was to be a general model of the breast implant, not an exact replica.

SIDE VIEW

1.3

edge or radius d = 4.25

Figure 3.11 Side view of filled implant.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

34

For the PATRAN geometric model, the full shape shown in the side view of Figure 3.11 is not needed. As described in Chapter 2, axisymmetric elements can be used for this model. By creating only the right half of the implant capsule shown in Figure 3.12, and telling PATRAN that the vertical axis at the center of the implant is the axis of rotation, the axisymmetric elements will take care of the remaining three dimensional geometry. Therefore the implant shown in Figure 3.11 can be represented by the

geometry shown in Figure 3.12.

1.3 axis of rotation

2.125

Figure 3.12 Axisymmetric representation of filled implant.

Using the point and curve generation capabilities of PATRAN, this geometry was created and is shown in Figure 3.13. This geometric model was used as the basis for the finite element model of the breast implant capsule, to be discussed in Chapter 4.

Once the geometry of the implant capsule alone had been completed, the tissue surrounding the implant in the body was added. The type of surrounding tissue depends on whether the implant was inserted using the submuscular or the subglandular approach, and on the patients physical characteristics. However, a general geometry can be

created, and the material properties of the associated elements can be changed for different surrounding tissue. Figure 3.14 shows the general geometry created to model the surrounding tissue. This geometry will be used as the basis for solid axisymmetric elements, so like the capsule itself, only a two dimensional view is needed. Other geometries were also created to represent more surrounding tissue, simply by increasing

CHAPTER 3: GEOMETRIC MODEL FORMULATION

35

the radius (the 2.5 measurement in Figure 3.14). Several of these examples will be shown in later chapters.

surrounding material implant axis of rotation 2

2.5

Figure 3.14 Geometric dimensions of implant with surrounding tissue.

This PATRAN creation of this geometry is shown in Figure 3.15.

Now that the geometric models have been created for both the implant capsule and the surrounding material, the finite element models can be created.

CHAPTER 3: GEOMETRIC MODEL FORMULATION

36

4.0 FINITE ELEMENT MODEL FORMULATION

Once the geometric models were complete, the development of the finite element models was the next step in the PATRAN creation process. This chapter will discuss in detail the elements that were chosen for this model and their application to its geometry. To conclude the chapter, a general model creation and analysis will be reviewed, accompanied by the associated computer code.

4.1 MODELING THE MEMBRANE

As introduced in Section 2.3.1, the breast implant membrane was modeled using axisymmetric shell elements. Figure 4.1 shows the general axisymmetric shell element. These elements are one-dimensional, deforming in a radial plane.

z S n Shell normal

Shell middle surface

Figure 4.1 Axisymmetric shell elements.

The

particular

elements

used

were

SAX1

elements,

which

are

two-node

stress/displacement elements that use one point integration of the linear interpolation function for the distribution of loads (ABAQUS 3.6.1-1). Figure 4.2 shows the SAX1 two-node element.
1 2

2 - node element

Figure 4.2 SAX1 element.

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

37

These elements have three degrees of freedom, corresponding to the polar coordinate system shown below in Figure 4.3. Coordinate 1 is the radial direction, r, coordinate 2 is the vertical direction, z, and coordinate 6 is the angle in the r-z plane, .

Figure 4.3 Coordinate system used for axisymmetric elements.

Following from these coordinates, degree of freedom 1 is the displacement in the radial direction, ur, degree of freedom 2 is the displacement in the vertical direction, uz, and degree of freedom 6 is the rotation in the r-z plane, called .

Once these SAX1 elements were selected, they were applied over the breast implant geometry using PATRAN. Of course, the number of elements used determined how well the finite element model approximated the actual geometry. Figure 4.4 shows the membrane with only 10 elements, a rather rough mesh. Figure 4.5 shows a 48element mesh, an obviously more accurate model.

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

38

4.2 MODELING THE INNER FLUID

In accounting for the fluid-filled nature of the breast implant capsule, fluid elements must be applied to the inner boundary of the implant. ABAQUSs hydrostatic fluid element family can be used to represent fluid-filled cavities under hydrostatic conditions, which is acceptable for this application. The FAX2 element type is a twonode, first order axisymmetric fluid element which maintains displacement compatibility with the SAX1 elements. Figure 4.6 shows the fluid element FAX2 and its positive normal toward the fluid.

fluid

FAX2

Figure 4.6 FAX2 element.

By distributing FAX2 elements just inside the SAX1 elements, with the same length, the fluid inside the cavity is introduced. Because PATRAN does not support fluid elements, these must be programmed directly into the ABAQUS input file created by PATRAN (described in Section 2.4). This is easily done since the fluid elements are the same length and orientation as the SAX1 elements already created by PATRAN. The FAX2 elements can be created using the same nodes used for the SAX1 elements, with the one exception of reversing the order of the nodes of each element. The nodes must be numbered opposite the numbering of the SAX1 elements in order to have the positive normals pointing inward toward the fluid.

Once the cavity is lined with hydrostatic fluid elements, the fluid properties of these elements are assigned using a cavity reference node. All fluid elements associated with a particular cavity share this cavity reference node, which can be anywhere on the cavity border or within the cavity. Figure 4.7 shows the node used as the reference node

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

39

for this model, node 100, located at the origin of the coordinate system. This cavity reference node has only one degree of freedom, which represents the fluid pressure in the cavity. By applying the pressure at this node, this pressure is distributed across the whole fluid cavity throughout the analysis.

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

40

4.3 MODELING THE CONTACT SURFACE

Because the breast implant model deforms against some type of rigid surface, contact modeling must also be considered. There are many different types of surfacebased contact simulations available, for example with both bodies deformable or with sliding contact between two surfaces. For the breast implant model, contact between a rigid surface and a deformable body is most appropriate, with the breast implant capsule being the deformable body and the rigid surface being a general modeling surface representing the chest wall. This is also appropriate for the initial analyses with the rigid surface being a table surface onto which the implant deforms.

There are three steps needed to define surface-based interaction: creating the surfaces involved, specifying which surfaces interact, and defining the behavior of the surfaces when they are in contact, such as frictional properties (ABAQUS 21.1.1-2).

In creating the rigid surface, one simple approach is to use a subroutine provided by ABAQUS which creates an analytical rigid surface. This option is available for simple geometric surfaces that can be described with straight or curved line segments. These profiles are swept along a generator direction to form the analytical rigid surface (ABAQUS 2.3.3-1).

The two-dimensional rigid surface is the simplest to create, with a segment-type denotation applying for an axisymmetric model in the (r,z) plane (ABAQUS 23.17.17-1). By identifying within ABAQUS the local coordinates of the starting and ending points of the line, a two-dimensional rigid surface can be created right beneath the implant, as shown in Figure 4.8 below. This example shows the rigid surface created to simulate a table or other flat surface supporting the implant.

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

41

Once this surface is created beneath the implant, the contact pairs must be defined in order to establish contact between the implant and the rigid surface. ABAQUS uses a master-slave algorithm to define contact conditions, with the rigid surface being the master and the deformable body being the slave surface. This defines smooth interaction between the two surfaces, with the designated slave surface, the implant, deforming onto the master surface, as will be visible on the deformation plots in Chapter 5.

4.4 MODELING THE SURROUNDING TISSUE

To model the surrounding material, axisymmetric solid elements were used to fill the geometric space shown in Figure 3.14. The particular elements used were CAX3 and CAX4 elements, which are three-node and four-node, respectively, stress/displacement elements that use one point integration of the linear interpolation function, like the SAX1 elements. Figure 4.9 shows the CAX3 and CAX4 element, which has two active degrees of freedom, the first being radial deformation, ur, and the second vertical deformation, uz.
3 4 face 2 face 3 face 4 face 2 face 3 3

face 1 3 - node element, CAX3

face 1 4 - node element, CAX4

Figure 4.9 Axisymmetric solid elements. These elements were applied in a mesh using PATRAN to the geometric tissue area, which is user-specified. To show examples of the meshed surrounding tissue, the geometric model with the 2.5 radius tissue, as shown in Figure 3.14, was used as the base geometry. Figures 4.10 and 4.11 show this geometry meshed with CAX3 and CAX4 elements, respectively. Many different levels of mesh refinement were tested, as will be demonstrated in the examples described later. Note that contact elements are not needed for the analyses with surrounding tissue since the implant is in direct contact with the tissue on all sides.

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

42

4.5 THE ANALYSIS PROCEDURE

In Chapter 4, the modeling of different aspects of the breast implant was discussed. In this section, the creation of a general model will be reviewed. This general model is an implant without surrounding tissue. At the conclusion of this section, the changes required for a model with surrounding tissue will be explained.

Although PATRAN shows the best view of the model and the analysis results, the ABAQUS input file is submitted to the processor. Therefore, this file contains the real details of the model. Sections of the code copied from the input file will be incorporated throughout this example as it is presented. Note that the ABAQUS code commands all begin with a single asterisk (*), those lines without an asterisk are continuations of a previous code line, and those lines with two asterisks (**) are comment lines.

The first section of code defines all the nodal coordinates, with each node number listed followed by its radial and axial location coordinates. If any nodes are grouped into a certain set, this is also defined here. This section, shown below, is automatically coded by PATRAN from the model. One node must be coded directly into the ABAQUS input file: the fluid cavity reference node, described in Section 4.2. Because PATRAN does not yet provide fluid elements, this node must be user-defined. In the example shown below, the cavity reference node, node 100, is the only node assigned to a particular set, in this case called cavity.

*NODE 1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 13, 14,

0., 0.238712, 0.477431, 0.715784, 0.953628, 1.19042, 1.42513, 1.65543, 1.87444, 2.05694, 2.125, 2.05694, 1.87436,

0.65 0.646988 0.639266 0.62579 0.605067 0.574875 0.531653 0.469127 0.374961 0.223692 0. -0.223682 -0.375011

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

43

15, 1.65542, 16, 1.4251, 17, 1.19034, 18, 0.953524, 19, 0.715683, 20, 0.477316, 21, 0.23869, 22, 0., 100,0.,0. ** *NSET,NSET=CAVITY 100 **

-0.46913 -0.531659 -0.574888 -0.605078 -0.625797 -0.639271 -0.646989 -0.65

The next section of code is very similar to the node section, except that it defines the models elements. Each element set is defined by stating the element type, the set name, and a list consisting of each element number and its associated node numbers. This element definition, also coded by PATRAN, is shown below.

*ELEMENT, TYPE=SAX1, ELSET=MEMBRANE 1,1,2 2,2,3 3,3,4 4,4,5 5,5,6 6,6,7 7,7,8 8,8,9 9,9,10 10,10,11 11,11,13 12,13,14 13,14,15 14,15,16 15,16,17 16,17,18 17,18,19 19,20,21 20,21,22

The next step is to define the material properties for each element set. In this example, the properties of the implant element set, named MEMBRANE are defined. For the shell elements of this particular set, the shell section option is assigned with the

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

44

material assigned as SILICONE. The second line defines the thickness of the shell section, in this case 0.019, and the number of integration points, which is 3.

*SHELL SECTION, ELSET=MEMBRANE, MATERIAL=SILICONE 0.019, 3

In the previous paragraph, the material type SILICONE was assigned for the implant element set, but this material type must also be created. The code below shows the creation of the material and the assignment of material properties for this material. After assigning the material name, the material is defined as an isotropic linear elastic material. The last line below lists the elastic modulus, 100 psi, followed by the Poissons ratio, 0.45.
** Silicone ** Date: 08-Jul-98 Time: 13:23:07 ** *MATERIAL, NAME=SILICONE ** *ELASTIC, TYPE=ISO 100., 0.45

Now that the implant and its properties are coded, the other aspects of the model must be considered. For this implant example, a rigid surface is created under the implant as described in Section 4.3. This section of the code also must define the interaction of this surface with the implant surface. Following the code listed below, the first step is the generation of an element set consisting of implant elements. This set, named ECON, includes the elements from 12 to 20, incrementing by 1. Next the rigid surface is created, called BSURF, by starting a line at Node 22, whose coordinates are cited in the START line. The line continues to the coordinates cited in the LINE line, which is 3 inches radially. The next command creates a surface from the ECON element set called ASURF, whose positive normal is in the same direction as the associated elements normals, designated by SPOS. The code to this point has defined the implant elements 12-20 as ASURF, and the rigid surface as BSURF. The

remaining two commands in the code below define smooth interaction between the two

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

45

surfaces, with the first surface listed, ASURF, being the slave surface, and the second surface, BSURF, being the master surface.
** ** CONTACT ELEMENTS (TABLE IS RIGID SURFACE) ** *ELSET,ELSET=ECON,GENERATE 12,20,1 *RIGID SURFACE, TYPE=SEGMENTS, NAME=BSURF, REF NODE=22 START,0.,-.65 LINE,3.,-.65 *SURFACE DEFINITION,NAME=ASURF ECON,SPOS *CONTACT PAIR, INTERACTION=SMOOTH ASURF,BSURF *SURFACE INTERACTION, NAME=SMOOTH **

Most of the afore-mentioned code was programmed directly from the PATRAN model, but the following section of code is an example of user-created code. The code below shows the creation of the fluid implants which line the inside of the implant. As described in Section 4.2, these elements are created using the same nodes as the implant elements, but reversing the node order to get the proper orientation. After defining the FLUID element set, it is defined as a hydraulic fluid with cavity reference node 100. It is given a fluid density of 0.0368 lbs/in3, which is the density of water at standard temperature and pressure.
**FLUID ELEMENTS FOR INTERIOR OF IMPLANT MEMBRANE ** ELEMENT, TYPE=FAX2, ELSET=FLUID 101,2,1 102,3,2 104,4,3 105,6,5 106,7,6 107,8,7 108,9,8 109,10,9 110,11,10 111,13,11 112,14,13 113,15,14 114,16,15

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

46

115,17,16 116,18,17 117,19,17 118,20,19 119,21,20 120,22,21 *FLUID PROPERTY, REF NODE=100, TYPE=HYDRAULIC, ELSET=FLUID *FLUID DENSITY 0.0368 **

The final section before the analysis defines the initial displacement boundary conditions. These are defined by listing the node to be constrained, the first degree of freedom (d.o.f.) to be constrained, the last degree of freedom to be constrained, and the amount of displacement permitted in that direction. For this example, nodes 1-21 were to be fixed in the 1- and 6-directions, but free in the 2-direction. Therefore, the command applied to a starting d.o.f. 1 to a final d.o.f. 6 would not be correct since that would include the 2-d.o.f. Therefore, each d.o.f. must have a separate line for each node, listing the appropriate direction as the first d.o.f. and leaving the final d.o.f. spot blank, as shown below. The other justification for listing each degree of freedom separately is

demonstrated by the last node, node 22, to be constrained in this section. Because all three degrees of freedom associated with an axisymmetric element are to be fixed for this node, it would make sense to list the 1-direction as the first d.o.f., and the 6-direction as the last, automatically including the 2-direction. However, this would also automatically include the 3-, 4-, and 5- degrees of freedom, which do not exist in this model. This would not affect the analysis, but it generates many lines of warning statements in the analysis output, so these constraints are listed separately as well.
*BOUNDARY 1,1,,0. 1,6,,0. 2,1,,0. 2,6,,0. 3,1,,0. : : 18,1,,0. 18,6,,0.

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

47

19,1,,0. 19,6,,0. 20,1,,0. 20,6,,0. 21,1,,0. 21,6,,0. 22,1,,0. 22,2,,0. 22,6,,0. **

The analysis itself is a nonlinear static stress analysis, because of several sources of nonlinearities. One cause is geometric nonlinearity, which necessitates the inclusion of large-displacement effects. In addition, the contact analysis between the implant and rigid surface is a boundary nonlinearity. However, the results of linear analysis for this model were a more obvious proof of the nonlinearity. The results were inconsistent, scattered, and very unrealistic, in contrast with the reasonable results from nonlinear analysis.

The analysis was divided into two steps, as are shown below. The nonlinear method used in this step, Step 1, uses automatic incrementation, in which ABAQUS selects the increment size as it develops the response. The boundary condition for node 100, the cavity reference node, specifies the filling of the implant cavity. Its only degree of freedom, 8, represents the pressure in the cavity. By specifying a pressure of zero (gage pressure) to this node, the cavity geometry is filled just to capacity, matching the fluid volume to the cavity volume. The remaining commands in this section are print commands which request printouts of contact interactions and the cavity volume and final pressure of the cavity.

** Step 1 - INFLATION STEP ** *STEP, NLGEOM *STATIC 0.1, 1. *PRINT, CONTACT=YES *BOUNDARY 100,8,8,0. *NODE PRINT, NSET=CAVITY PCAV,CVOL

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

48

*END STEP **

The second step of the analysis seals the cavity and applies the load boundary condition to the model. This example uses 25 increments instead of the automatic incrementation used in Step 1, and was determined from many attempts at the analysis. The boundary conditions are reapplied in this step with the added OP=NEW command. This erases all previous conditions, and seals the cavity volume for the remainder of the analysis. After applying this volume conservation command, the boundary conditions are reapplied and the analysis continued. The final boundary condition of Step 2 is the load boundary condition, which for this case is a 3 psi pressure on Elements 1-7 in the negative 2-direction. The remainder of this step is several lines of print commands which include the cavity volume and pressure, to check volume conservation and final pressure. These print commands also output each elements stress, displacement, and strain results.
** Step 2 - SEAL CAVITY, LOAD TOP ** *STEP,NLGEOM,INC=25 *STATIC 0.1, 1.0 *BOUNDARY, OP=NEW 1,1,,0. 1,6,,0. 2,1,,0. 2,6,,0. 3,1,,0. : : 18,1,,0. 18,6,,0. 19,1,,0. 19,6,,0. 20,1,,0. 20,6,,0. 21,1,,0. 21,6,,0. 22,1,,0. 22,2,,0. 22,6,,0. ** *DLOAD 1,P,-3.0 2,P,-3.0 3,P,-3.0

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

49

4,P,-3.0 5,P,-3.0 6,P,-3.0 7,P,-3.0 ** *NODE PRINT,NSET=CAVITY PCAV,CVOL *NODE PRINT, FREQ=1 U, *NODE FILE, FREQ=1 U, : : ** *END STEP

The code presented in this section is from Example 5.4, which is an implant model without surrounding tissue that is presented in Chapter 5. The complete code listing is in Appendix A.

For a model without surrounding tissue, there are a few differences in the analysis code. Of course, there are additional node and element sets for the surrounding tissue, and additional material definitions for those elements. However, there are no contact surface definitions because the surrounding tissue becomes the other surface, which deforms with the implant itself. No rigid surfaces are needed, since the bottom surface of the tissue is fixed like a rigid surface. With these exceptions, the remainder of the code is written with the same order and method. A code for a model with surrounding tissue is included in Appendix B for comparison, and its model will be presented in Chapter 6 as Example 6.6.

CHAPTER 4: FINITE ELEMENT MODEL FORMULATION

50

5.0 FINITE ELEMENT MODEL CASE STUDIES

In Chapter 4, the model formulation was described and the analysis procedure was explained. Chapter 5 will present several basic analysis cases and provide two

verification cases.

For each case presented in this thesis, a table summarizing the input variables will be provided, along with an explanation of these variables. A table presenting the results will also be given in addition to a stress contour plot of the deformed model and a discussion of the results. Note that the maximum displacement given in the results tables are for all nodes in the model, including both the implant and the surrounding tissue. However, the maximum stress considers only the implant elements, not the surrounding tissue. On the result plots, the deformation plotted is the resultant of the displacements u1 and u2; the stress contours are based on the Von Mises stress.

5.1 FEA MODEL BASIC CASES

As described in Section 3.2, there are a few geometric models which serve as the basis for all the different meshes and cases studied in this research. There is a basic implant model supported by a rigid surface (Figure 3.13), and another model of the same implant surrounded by tissue (Figure 3.15). This section will present the three basic cases first, in preparation for the variations on these cases which comprise the remainder of the research.

5.1.1 Implant Without Surrounding Tissue Example 5.1 The first basic case, Example 5.1, is similar to that shown in Figure 4.4, the 10element mesh of the implant. This mesh is a finer mesh consisting of 20 SAX1 elements, 10 on the upper half and 10 on the lower half of the implant, as shown in Figure 5.1. The elements are labeled in blue font while the nodes are labeled in red. Notice that the fluid elements and the contact surface under the implant are not visible in this type of

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

51

PATRAN plot. Because these elements are not supported by PATRAN, as discussed in Sections 4.2 and 4.3, they are not shown in the PATRAN plots.

Table 5.1 shows the load case and parameters inputted for this example. For the implant itself, the 20 SAX1 elements had an elastic modulus of 100 psi, a Poissons ratio of 0.45, and a shell thickness of 0.019 inches. These are the implant properties discussed in Section 3.1, and are used as the default properties in most cases. The load condition was a CLOAD type, meaning that a concentrated, or point, load was applied to the specified node(s). In this case, 1 pound was applied to node 1, the top center node of the implant. The displacement boundary condition fixed node 22, the bottom center node of the implant, in all directions. Nodes 13-22, the remainder of the nodes on the bottom half of the implant, were fixed in the 1 and 6 directions, radially and rotationally, respectively. These nodes were unlimited vertically. All of the nodes on the upper half of the implant were free to move in all three directions.

Table 5.1 Input data for Example 5.1. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load CLOAD: 1 lb. on Node 1 (in -2 direction) Displacement Node 22: fixed 1,2,6 Nodes 13-21: fixed 1,6

Figure 5.2 shows the stress contours of the 20-element breast implant model overlaid on the deformed geometry. With this mesh, the volume of the cavity was 13.41 in3, and the final internal pressure was about 0.09 psi. As can be seen in Figure 5.2, node 1 had the maximum displacement of 1.15 inches. Element 1, the element associated with

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

52

nodes 1 and 2, experienced the highest stress level of 98.63 psi. These results are summarized in Table 5.2.

Table 5.2 Result data for Example 5.1. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 0.0858 Max. Displacement, in. u1 -0.056 @ Node 11 u2 -1.15 @ Node 1 Max. Stress, psi S11 98.63 @ Element 1 S22 12.36 @ Element 1

Example 5.1 is a simple case of point loading without surprising results. The node of load application had the most deformation, as expected, and its associated element experienced the highest stress level. The elements on the bottom half of the implant deformed as the slave surface elements should against the rigid master surface. Although the rigid surface is not shown in the plot, it is obvious that the implant elements are deforming onto it as intended.

5.1.2 Implant With Surrounding Tissue Example 5.2 The next example, Example 5.2, is based also on a model introduced in Chapter 4. The implant model with 2.5 radius surrounding tissue, shown below in Figure 5.3, with CAX3 elements, is used for Example 5.2. Figure 5.4 shows the nodes associated with this model, for future reference. Table 5.3 shows the input for Example 5.2. The same implant mesh and default material properties described in Example 5.1 were used for this model. In addition, the material properties for the 138 surrounding tissue elements were added. For the solid axisymmetric elements, the elastic modulus chosen was 100 psi, as shown in Table 5.3, which is a modulus between that of collagen and elastin, two human tissue components. The load condition was a DLOAD type, meaning that a distributed load, or pressure, was applied to the specified element(s). In this case, 10 psi

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

53

was applied to the elements along the upper surface of the tissue. The displacement boundary condition fixed all of the nodes along the bottom and right side edge of the tissue in all directions. These nodes correspond to the entire bottom surface and outside circumference of the surrounding tissue on a non-axisymmetric model. Of course, all of the models remaining nodes were free to move in all three directions.

Table 5.3 Input data for Example 5.2. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi 100 Type CAX3 No. 138

Boundary Conditions Load DLOAD: 10 psi (in -2 dir.) on Elements 64,83-87,92-93,98,135 (top edge of tissue) Displacement Nodes 2,6-20,65-69: fixed 1,2 (edge and bottom nodes of tissue)

Figure 5.5 shows the stress contours of the 138-element breast tissue model overlaid on the deformed geometry. With this mesh, the volume of the cavity was 13.41 in3, the same volume as in Example 5.1 since the same implant mesh was used. The final internal pressure was about 10 psi. As can be seen in Figure 5.5, the entire upper surface of the tissue deformed, decreasing closer to the right edge of the tissue because of the boundary conditions at that edge. Node 79, close to the upper center of the tissue, had the maximum vertical displacement of 0.07 inches. These results are summarized in Table 5.4.

Although it is interesting to see the stress distribution in the tissue elements, the main focus of this research is the stress in the implant itself. Figure 5.6 isolates the implant elements of this model, which were hidden by the tissue elements in Figure 5.5. Similar to the tissue elements, the implant elements closest to the center of the model

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

54

experienced the highest stress levels, with Element 149 having the highest S22 of about 2.5 psi.

Table 5.4 Result data for Example 5.2. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 9.997 Max. Displacement, in. u1 0.014 @ Node 59 u2 -0.0659 @ Node 79 Max. Stress, psi S11 2.611 @ Elem. 139 S22 2.478 @ Elem. 149

Example 5.3 As described in Section 3.2, the 2.5 radius tissue model was not the only tissue model created for this research. Another model was created which increased the

surrounding tissues radius from 2.5 to 4. This is the basis for Example 5.3, shown in Figure 5.7. This model was meshed using a different type of element, the CAX4 element, introduced in Section 4.4. Figure 5.8 shows this mesh with the nodes labeled, instead of the elements as shown in Figure 5.7.

Table 5.5 shows the load case and parameters inputted for this example. The implant was meshed with 48 SAX1 elements, with upper and lower halves having 24 each. The default material properties were used, as in Examples 5.1 and 5.2. The tissue model was meshed with 599 CAX4 elements having an elastic modulus of 100 psi, also similar to Example 5.2. The load and displacement boundary condition are analogous to Example 5.2 as well, with 10 psi pressure applied to the upper tissue surface elements and the right side and bottom edge tissue elements fixed in all directions.

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

55

Table 5.5 Input data for Example 5.3. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 48 Tissue Elements E, psi 100 Type CAX4 No. 599

Boundary Conditions Load DLOAD: 10 psi (in -2 dir.) on Elements 1,5-43 (top edge of tissue) Displacement Nodes 26,46-55,360,364-403,405-413: fixed 1,2 (edge and bottom nodes of tissue)

Figure 5.9 shows the resulting deformation created by these boundary conditions. Like Example 5.2, the upper surface elements experienced the most strain, again decreasing from a maximum at the left edge of the model to a minimum at the right edge, where the nodes were fixed. Node 56, the top left corner node, corresponding to the top center of the breast tissue, had the maximum vertical displacement of 0.2 inches. These results are summarized in Table 5.6. Figure 5.10 isolates the implant elements of this model, showing their deformation and stress contours. Once again, the elements closest to the center of the implant experienced the most stress, with Element 601 having both S11 and S22 about 30 psi.

Table 5.6 Result data for Example 5.3. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 3.77 Max. Displacement, in. u1 0.1766@ Node 75 u2 -0.2008 @ Node 56 Max. Stress, psi S11 30.66 @ Elem. 601 S22 30.53 @ Elem. 601

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

56

5.2 VERIFICATION CASES

Although the cases presented in Section 5.1 resulted in realistic deformation schemes, some other corroboration would provide a higher confidence in the FEA results. Two such comparisons were used to verify the FEA results: an internal pressure measurement and a displacement measurement. Both of these comparisons were used to verify the FEA model without surrounding tissue. Of course, neither of these

comparisons were expected to closely match, since these are initial FEA models which are constantly being adjusted and improved. However, some similarities could ensure that the models are progressing towards realistic behavior.

5.2.1 Internal Pressure Comparison Internal pressure is one of the variables monitored by the ABAQUS program whenever specified. For each case in this thesis, the internal pressure was reported throughout the analysis and noted in the results, as exhibited in the previous examples of Section 5.1. Another student working on breast implant studies, Kristen Droesch of the Materials Science and Engineering Department at Virginia Tech, built a pressure transducer system which measures the internal pressure of the cavity fluid even in a loading situation. The results of her study were used to judge the accuracy of the FEA models.

The pressure measurements were performed by reading the pressure after a person would lie down on an implant, distributing their body weight on the implant and on the floor at their head, buttocks and feet. The weight distributed to the implant could be estimated at about a third of their body weight, which for the 150-pound test subject would be 50 pounds. Estimating the area of application of this weight was done by taking the cross-sectional area of the horizontal implant, as shown in Figure 3.10. This area, based on the radius of 2.125 inches, is 14.19 inches2. 50 pounds applied to a 14.19 in2 area results in a pressure of 3.5 psi. Of course, this is a rough estimate of the loading situation, but adequate for a quick verification. The resulting pressures taken by the

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

57

transducer for this experiment, which will be compared to the models final pressure, varied from 1.5 to 2.6 psi.

In order to compare this laboratory test to the FEA model, this Pressure Verification Example, Example 5.4, was based on the model from Example 5.1 with the default material properties, as shown in Table 5.7. The loading boundary condition was applied as a 3 psi load pressure to most of the upper surface of the implant, elements 1-7. Node 22, the node which would be the bottom center of the implant on a 3-D model, was fixed in all three directions. The other nodes of the model were limited to vertical movement, so that no rocking or rotating of the implant would exist, as was attained in the laboratory experiment.

Table 5.7 Input data for Pressure Verification Example, Example 5.4. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

Figure 5.11 shows the model results, showing reasonable deformations. Node 1 had the maximum vertical displacement of 0.6059 inches, almost to the mid-plane of the implant horizontally. The final internal pressure was about 2.5 psi, which is in the range of pressures obtained by the transducer. Table 5.8 summarizes the analysis results.

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

58

Table 5.8 Result data for Pressure Verification Example, Example 5.4. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.483 Max. Displacement, in. u1 0 u2 -0.6059 @ Node 1 Max. Stress, psi S11 S22

49.55 @ 22.30 @ Element 11 Element 11

5.2.2 Displacement Comparison Another variable easy to compare for verification purposes is displacement. Using the same implant used to determine the geometry for the model, described in Section 3.2, it was again filled with water to a nominal level of 250 cc. The implant was sitting on a flat surface, similar to the situation described for the internal pressure comparison. A spring force gauge was used to apply a point load to the top center point of the filled implant. The displacement was then measured while holding the applied force on the implant.

In order to compare the displacement measurement to the existing case described in Section 5.1.1, Example 5.1, the force gauge was used to apply 1 pound to the top center point. With this load held in place, the displacement of the top center point was measured to be 0.95 inches. This can be compared to the 1.15 inch displacement of the same point in Example 5.1. Considering the models approximations and many variables, this 17% difference is within the range of realistic expectations for the model. In

addition, the deformation of the implant had a profile similar in appearance to the models prediction, shown in Figure 5.2.

CHAPTER 5: FINITE ELEMENT MODEL CASE STUDIES

59

6.0 FINITE ELEMENT MODEL VARIABLE STUDIES

Once the basic FEA models were analyzed and produced acceptable results, as described in Chapter 5, the next step was to study the effects of changing the many variables associated with the model. This chapter will discuss those variable studies and their significance.

6.1 POISSONS RATIO COMPARISON

The first variables to be altered were the material properties studied in Section 3.1. As discussed in Section 3.1.2, the Poissons ratio, , was chosen at 0.5. However, because that numerical value creates trivial solutions to the finite element equations, the processor will not accept 0.5 for a Poissons ratio choice. A value of 0.45 was chosen for the introductory cases, but the following examples study the effects of varying the Poissons ratio from 0.45 to 0.49.

Comparing to the case presented in Example 5.4, the Poissons Ratio was changed for each of the four cases, Examples 6.1-6.4, ranging from 0.46 to 0.49 respectively, and increasing by 0.01. All of the other default properties were used for each case, as summarized in Tables 6.1-6.5. The load and displacement boundary conditions of

Example 5.4 were used for Examples 6.1-6.4 as well.

Table 6.1 Input data for Pressure Verification Example, Example 5.4. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

60

Table 6.2 Input data for Example 6.1. INPUT DATA Implant Elements E, psi 100 0.46 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

Table 6.3 Input data for Example 6.2. INPUT DATA Implant Elements E, psi 100 0.47 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

Table 6.4 Input data for Example 6.3. INPUT DATA Implant Elements E, psi 100 0.48 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

61

Table 6.5 Input data for Example 6.4. INPUT DATA Implant Elements E, psi 100 0.49 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

Figures 6.1-6.5 (Figures 6.1, 6.2, 6.3, 6.4, 6.5) show the displacement and stress results for each case. Although the differences in Figures 6.1-6.5 are subtle, it is clear in all five of these examples that the highest stress area is the outside edge of the implant. This is interesting to note because this is the area where creases can form, so loading which creates high stresses in this area should be avoided.

Using Figures 6.1-6.5 and Tables 6.6-6.10 to compare these cases, several differences are noted. With increasing the Poissons ratio by 0.01, the displacement of Node 1 decreased an average of 0.41% per case. Looking at Element 11, which

experienced the highest stresses, S11 increased an average of 0.146% per case. Its S22 increased an average of 1.19% per case. The final cavity pressure increased an average of 0.13% per 0.01 increase in . Based on these very small result changes with increases in the Poissons ratio, it can be concluded that the approximation of as 0.45 instead of 0.5 is acceptable.

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

62

Table 6.6 Result data for Pressure Verification Example, Example 5.4. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.483 Max. Displacement, in. u1 0 u2 -0.6059 @ Node 1 Max. Stress, psi S11 S22

49.55 @ 22.30 @ Element 11 Element 11

Table 6.7 Result data for Example 6.1. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.483 Max. Displacement, in. u1 0 u2 -0.6043 @ Node 1 Max. Stress, psi S11 S22

49.64 @ 22.84 @ Element 11 Element 11

Table 6.8 Result data for Example 6.2. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.489 Max. Displacement, in. u1 0 u2 -0.5998 @ Node 1 Max. Stress, psi S11 S22

49.66 @ 23.34 @ Element 11 Element 11

Table 6.9 Result data for Example 6.3. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.493 Max. Displacement, in. u1 0 u2 -0.5979 @ Node 1 Max. Stress, psi S11 S22

49.75 @ 23.88 @ Element 11 Element 11

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

63

Table 6.10 Result data for Example 6.4. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.496 Max. Displacement, in. u1 0 u2 -0.5959 @ Node 1 Max. Stress, psi S11 S22

49.84 @ 24.42 @ Element 11 Element 11

6.2 ELASTIC MODULUS COMPARISON

6.2.1 Elastic Modulus of Implant In Section 3.1, the elastic modulus was decided to be 100 psi for a Smooth implant analysis, and 78 psi for a Siltex implant. However, all analyses were done for Smooth implants. To understand what effect this modulus change from Smooth to Siltex implant has, Example 5.4 of Section 5.2.1 was again used. Running the same analysis with the implant elastic modulus changed to 78 psi, the displacement and stress effects were examined. Table 6.11 shows the input data for this case, Example 6.5. Note that its only variation from Example 5.4, shown in Table 6.1, is the elastic modulus change. Figure 6.6 shows the displacement and stress distributions of this case, and Table 6.12 shows the numerical data results.

Table 6.11 Input data for Example 6.5. INPUT DATA Implant Elements E, psi 78 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

64

Table 6.12 Result data for Example 6.5. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.44 Max. Displacement, in. u1 0 u2 -0.7613 @ Node 1 Max. Stress, psi S11 S22

53.31 @ 23.99 @ Element 10 Element 10

Comparing these results to Example 5.4, shown in Figure 6.1, there is a marked increase in deformation with this decrease in elastic modulus. In fact, Node 1 of Example 6.5 displaced vertically almost 26% more than the same node in Example 5.4. Comparing the stresses, the edge of the implant remains the highest stress area. However, Example 6.5s maximum stresses occurred in Element 10 instead of Element 11. In addition, both the S11 and S22 maximum stresses were about 7.6% higher than the maximum stresses in Example 5.4. The cavity pressure in Example 6.5 decreased 1.73% from the pressure in Example 5.4.

It is clear from these results that this decrease in elastic modulus from 100 psi to 78 psi caused a significant increase in both the stress and displacement results from the model. This may be the reason that the Siltex implants are manufactured with larger thicknesses than the Smooth implants.

6.2.2 Elastic Modulus of Surrounding Tissue In addition to studying the modulus of the implant, variations in the stiffness of the surrounding material must also be considered. The model with 2.5 radius

surrounding tissue was chosen, with the mesh introduced in Example 5.2. For this study, the loading condition was a distributed load on the top 10 surface elements of the tissue, starting at a maximum of 10 psi at the center and decreasing to 1 psi at the outside edge, with increments of 1 psi. The displacement boundary condition fixed the nodes along the bottom edge of the tissue both radially and vertically. The nodes along the outside edge of the tissue were fixed radially. The default properties of the implant were used for all

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

65

three cases of this study, with the only variation being the tissue modulus. Example 6.6 uses the standard modulus of this model, 100 psi, while Example 6.7s modulus decreases to 87 psi, and Example 6.8s modulus increases to 300 psi. Tables 6.13-6.15 summarize the input data for Examples 6.6-6.8.

Table 6.13 Input data for Example 6.6. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi 100 Type CAX3 No. 138

Boundary Conditions Load DLOAD: 10 psi (in -2 dir.) on Elem. 64, 9 on 98, 8 on 93, 7 on 92, 6 on 87, 5 on 86, 4 on 85, 3 on 84, 2 on 83, 1 on 135 (top edge of tissue) Displacement Nodes 2, 6-15: fixed 1,2 (bottom) Nodes 16-20, 65-69: fixed 1 (side)

Table 6.14 Input data for Example 6.7. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi 87 Type CAX3 No. 138

Boundary Conditions Load DLOAD: 10 psi (in -2 dir.) on Elem. 64, 9 on 98, 8 on 93, 7 on 92, 6 on 87, 5 on 86, 4 on 85, 3 on 84, 2 on 83, 1 on 135 (top edge of tissue) Displacement Nodes 2, 6-15: fixed 1,2 (bottom) Nodes 16-20, 65-69: fixed 1 (side)

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

66

Table 6.15 Input data for Example 6.8. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi 300 Type CAX3 No. 138

Boundary Conditions Load DLOAD: 10 psi (in -2 dir.) on Elem. 64, 9 on 98, 8 on 93, 7 on 92, 6 on 87, 5 on 86, 4 on 85, 3 on 84, 2 on 83, 1 on 135 (top edge of tissue) Displacement Nodes 2, 6-15: fixed 1,2 (bottom) Nodes 16-20, 65-69: fixed 1 (side)

The results are summarized in Tables 6.16-6.18. Figures 6.7-6.12 (Figures 6.7, 6.8, 6.9, 6.10, 6.11, 6.12) show the deformed shapes and stress profiles of these three cases, showing the tissue model and the implant model for each example. Refer to Figures 5.3 and 5.4 for element and node locations for this model.

Table 6.16 Result data for Example 6.6. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 5.887 Max. Displacement, in. u1 0.0418 @ Node 54 u2 -0.2706 @ Node 80 Max. Stress, psi S11 18.69 @ Elem. 149 S22 19.52 @ Elem. 149

Table 6.17 Result data for Example 6.7. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 5.858 Max. Displacement, in. u1 0.0466 @ Node 54 u2 -0.3028 @ Node 80 Max. Stress, psi S11 20.67 @ Elem. 149 S22 21.57 @ Elem. 149

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

67

Table 6.18 Result data for Example 6.8. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 6.021 Max. Displacement, in. u1 0.016 @ Node 54 u2 -0.1 @ Node 80 Max. Stress, psi S11 7.398 @ Elem. 149 S22 7.753 @ Elem. 149

First comparing Example 6.6 to Example 6.7, the results vary as expected for a tissue modulus decrease of 13%. The maximum radial displacement, at Node 54, The maximum vertical displacement

increased 11.5% with the decreased modulus.

increased as well, by 11.9% at Node 80. Both S11 and S22 increased by about 10.5% in Element 149 with the decrease in modulus. Finally, the pressure decreased by about 0.5% from Example 6.6 to Example 6.7.

Comparing Example 6.6 to Example 6.8, the 200% increase in the tissues elastic modulus had an even more significant impact, as expected. The maximum radial

displacement, at Node 54, decreased by 61.7%. The maximum vertical displacement, at Node 80, decreased by 63.1%. The stresses were similarly decreased with the increase in modulus. Element 149 experienced a decrease in both S11 and S22 of about 60%. Finally, the cavity pressure increased about 2.3% from Example 6.6 to Example 6.8.

These cases demonstrate the significance of the surrounding tissues elastic modulus. Most notable is the 60% decrease in stress in the implant with the tissues modulus increased to 300 psi. This suggests that placing the implant surgically between denser tissues will decrease the amount of load absorbed by the implant.

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

68

6.3 IMPLANT THICKNESS COMPARISON

Recall from Section 3.1.3 that the thickness of the implant specimen, although it does vary with the implant location of the sample, has a mean value of 0.019. However, different implant specimens can have different thickness dimensions, especially with the large number of implant volume sizes available. This section studies the effects of small changes in the thickness dimension, small meaning two-thousands of an inch.

Again Example 5.4 was used as a basis model, with the default properties used. Only the thickness of the implant elements were changed from case to case, starting at 0.021 and decreasing by 0.002 with each case, ending at a thickness of 0.015. These input properties are shown in Tables 6.19-6.22. Table 6.19 Input data for Example 6.9. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.021 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

Table 6.20 Input data for Example 5.4. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

69

Table 6.21 Input data for Example 6.10. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.017 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

Table 6.22 Input data for Example 6.11. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.015 Type SAX1 No. 20 Tissue Elements E, psi n/a Type n/a No. n/a

Boundary Conditions Load DLOAD: 3 psi (in -2 dir.) on Elements 1-7 (top of implant) Displacement Node 22: fixed 1,2,6 Nodes 1-21: fixed 1,6

Figures 6.13-6.16 (Figures 6.13, 6.14, 6.15, 6.16) show the deformation and stress results, while the result data is shown in Tables 6.23-6.26. Looking at Figures 6.13-6.16, there is a noticeable increase in stress and displacement results as the thickness is decreased with each case. The maximum vertical displacement, at Node 1, in increased by an average of 12.5% with each 0.002 reduction in implant thickness. Both S11 and S22 increase by an average of 16.6% with each decrease in thickness. Finally, the cavity pressure decreases by an average of 0.6% with each decrease in thickness.

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

70

Table 6.23 Result data for Example 6.9. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.494 Max. Displacement, in. u1 0 u2 -0.5390 @ Node 1 Max. Stress, psi S11 43.52 @ Elem. 11 S22 19.59 @ Elem. 11

Table 6.24 Result data for Example 5.4. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.483 Max. Displacement, in. u1 0 u2 -0.6059 @ Node 1 Max. Stress, psi S11 S22

49.55 @ 22.30 @ Element 11 Element 11

Table 6.25 Result data for Example 6.10. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.473 Max. Displacement, in. u1 0 u2 -0.670 @ Node 1 Max. Stress, psi S11 S22

58.24 @ 26.21 @ Element 10 Element 10

Table 6.26 Result data for Example 6.11. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 2.449 Max. Displacement, in. u1 0 u2 -0.7676 @ Node 1 Max. Stress, psi S11 S22

68.93 @ 31.02 @ Element 10 Element 10

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

71

These results demonstrate the impact these small changes make in the stress experienced by the implant elements. This may be another proof that increasing the thickness of Siltex implants does significantly reduce the stress increase caused by its decreased modulus, as compared to the Smooth implants, as suggested in Section 6.2.1.

6.4 SURROUNDING TISSUE RADIUS COMPARISON

Two different tissue geometries have been used: the 2.5 radius tissue model and the 4 radius tissue model. This section studies the effects of increasing the amount of tissue for a given loading situation.

Similar to the model used in Example 5.2, Example 6.12 is the standard 2.5 radius tissue model using the default material properties. Example 6.13 is the 4 radius tissue model with CAX3 elements. Both cases have a load boundary condition of 1 psi across the top tissue elements, and a displacement boundary condition fixing the outside edge and bottom nodes both radially and vertically. This input information is displayed in Tables 6.27 and 6.28.

Table 6.27 Input data for Example 6.12. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi 100 Type CAX3 No. 138

Boundary Conditions Load DLOAD: 1 psi (in -2 dir.) on Elements 64,83-87,92-93,98,135 (top edge of tissue) Displacement Nodes 2,6-20,65-69: fixed 1,2 (edge and bottom nodes of tissue)

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

72

Table 6.28 Input data for Example 6.13. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 48 Tissue Elements E, psi 100 Type CAX3 No. 1284

Boundary Conditions Load DLOAD: 1 psi (in -2 dir.) on Elements 648,702-740 (top edge of tissue) Displacement Nodes 482,501-510,823,827-866, 868-876: fixed 1,2 (edge and bottom nodes of tissue)

Figures 6.17-6.20 (Figures 6.17, 6.18, 6.19, 6.20) show the stress and displacement results, which are summarized in Tables 6.29 and 6.30.

Table 6.29 Result data for Example 6.12. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 1.002 Max. Displacement, in. u1 0.0014 @ Node 59 u2 -0.0068 @ Node 79 Max. Stress, psi S11 0.2659 @ Elem. 149 S22 0.2640 @ Elem. 149

Table 6.30 Result data for Example 6.13. RESULTS Cavity Volume, in3 13.56 Final Internal Pressure, psi 1.031 Max. Displacement, in. u1 -0.0024 @ Node 2 u2 -0.0056 @ Node 534 Max. Stress, psi S11 0.2238 @ Elem. 623 S22 0.1841 @ Elem. 614

Both tissue models experience low stress levels, overall less than 1psi, for this load condition. It is interesting to note that in Example 6.13, with increased tissue
CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES 73

volume, the tissue absorbs more of the load and the implant absorbs less. In Example 6.12, the implant absorbs more of the load. In Example 6.12, the maximum stress, S22, in the implant is 43% higher than the maximum in Example 6.13.

These results show that by increasing the volume of tissue around the implant, the tissue may absorb more of the applied load. This corresponds to lower stress levels in the implant itself.

6.5 COMPARISON OF TISSUE ELEMENT TYPE

Two solid element types have been used to model the surrounding tissue: CAX3 and CAX4 elements. In order to compare these, the results will be studied for both the 2.5 radius tissue model and the 4 radius tissue model.

6.5.1 Element Type of 2.5 Radius Surrounding Tissue For the 2.5 radius tissue model, CAX3 elements are usually used, as in Example 6.14 below. To compare the same models results with CAX4 elements, the same analysis was performed changing only the tissue element type. Both Examples 6.14 and 6.15 use the load and displacement boundary conditions used in Section 6.2.2. Notice that the only difference in the input data, shown in Tables 6.31 and 6.32, is the tissue element type.

The results for these two examples are summarized in Tables 6.33 and 6.34 below, and the stress and displacement plots are shown in Figures 6.21-6.24 (Figures 6.21, 6.22, 6.23, 6.24).

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

74

Table 6.31 Input data for Example 6.14. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi 100 Type CAX3 No. 138

Boundary Conditions Load DLOAD: 10 psi (in -2 dir.) on Elem. 64, 9 on 98, 8 on 93, 7 on 92, 6 on 87, 5 on 86, 4 on 85, 3 on 84, 2 on 83, 1 on 135 (top edge of tissue) Displacement Nodes 2, 6-15: fixed 1,2 (bottom) Nodes 16-20, 65-69: fixed 1 (side)

Table 6.32 Input data for Example 6.15. INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 20 Tissue Elements E, psi 100 Type CAX4 No. 67

Boundary Conditions Load DLOAD: 10 psi (in -2 dir.) on Elem. 164, 9 on 188, 8 on 189, 7 on 187, 6 on 186, 5 on 185, 4 on 184, 3 on 176, 2 on 175,1 on 174 (top edge of tissue) Displacement Nodes 174,179-188: fixed 1,2 (bottom) Nodes 117,122-126,175-178: fixed 1 (side)

Table 6.33 Result data for Example 6.14. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 5.887 Max. Displacement, in. u1 0.0418 @ Node 54 u2 -0.2706 @ Node 80 Max. Stress, psi S11 18.69 @ Elem. 149 S22 19.52 @ Elem. 149

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

75

Table 6.34 Result data for Example 6.15. RESULTS Cavity Volume, in3 13.41 Final Internal Pressure, psi 1.34 Max. Displacement, in. u1 0.011 @ Node 52 u2 -0.2067 @ Node 137 Max. Stress, psi S11 8.32 @ Elem. 149 S22 10.64 @ Elem. 149

There are several differences comparing the models with CAX3 and CAX4 elements. Example 6.14s maximum vertical displacement is 31% larger than the The stress in the CAX4 tissue

maximum vertical displacement in Example 6.15.

elements of Example 6.15 is overall higher than that in the CAX3 tissue elements of Example 6.14. However, the implant elements in Example 6.15 experience about 50% less maximum stress than the implant elements of Example 6.14.

These results suggest that in choosing a solid element type for the 2.5 radius tissue model, the CAX4 elements will absorb more of the applied load than the CAX3 elements, sending less stress to the implant itself.

6.5.2 Element Type of 4 Radius Surrounding Tissue In order to compare the use of CAX3 and CAX4 elements with the 4 radius tissue model, this section will contrast Example 6.16, introduced below, and a previous case, Example 6.13. Refer to Section 6.4, Table 6.28 for the input data for Example 6.13. The input data for Example 6.16 is shown below in Table 6.35. Both examples have a 1 psi pressure applied to the elements bordering the top surface of the tissue. Both

examples also have all nodes along the outside and bottom tissue edges fixed radially and vertically. The only difference between Examples 6.13 and 6.16 is the type of solid element used to mesh the surrounding tissue.

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

76

Table 6.35 Input data for Example 6.16. 7INPUT DATA Implant Elements E, psi 100 0.45 t, in. 0.019 Type SAX1 No. 48 Tissue Elements E, psi 100 Type CAX4 No. 599

Boundary Conditions Load DLOAD: 1 psi (in -2 dir.) on Elements 1,5-43 (top edge of tissue) Displacement Nodes 26,46-55,360,364-403,405-413: fixed 1,2 (edge and bottom nodes of tissue)

The results for Example 6.13 are shown in Table 6.30 and Figures 6.19-6.20 (Section 6.4); the results for Example 6.16 are shown in Table 6.36 and Figures 6.25-6.26 below. Table 6.36 Result data for Example 6.16. RESULTS Cavity Volume, in3 13.56 Final Internal Pressure, psi 0.405 Max. Displacement, in. u1 0.017 @ Node 74 u2 -0.0223 @ Node 56 Max. Stress, psi S11 2.931 @ Elem. 603 S22 2.879 @ Elem. 603

Comparing the two cases, the maximum vertical displacement was 75% smaller using CAX3 tissue elements than CAX4 tissue elements. The overall stress in Example 6.16 is significantly higher than the stress in Example 6.13 for these loading conditions. Notice that the maximum element stress in Example 6.13 (CAX3 elements) is almost 100% lower than that in Example 6.16 (CAX4 elements). These results show that for this geometry, meshing the tissue model with CAX4 elements will yield higher stress results and deformations than using CAX3 elements.

CHAPTER 6: FINITE ELEMENT MODEL VARIABLE STUDIES

77

7.0 SUMMARY AND CONCLUSIONS

This thesis presents the research to develop a realistic finite element model of a breast implant to be incorporated in the life prediction model. Many different analyses were performed with varied mechanical properties, load conditions, displacement boundary conditions, and element meshes. Some of these cases are presented here to demonstrate the effects of these variables and the realistic deformation and stress ranges produced.

The basic model was created based on the 225 cc Smooth implants geometry, with an elastic modulus of 100 psi, Poissons ratio of 0.45, and thickness of 0.019. The material behavior was assumed to be within the linear elastic range, because of the small loads and deformations experienced by these models. This axisymmetric geometric

model was created in PATRAN and served as the basis for the finite element model.

The finite element model consisted of axisymmetric elements (SAX1) for the element itself. The implant model was lined with axisymmetric fluid elements (FAX2) to convey the fluid-filled nature of the implants cavity. These elements were created with the fluid properties of saline solution, which is the standard filling liquid for these implants. Beneath the implant were contact elements onto which the implant deformed. For the implant model surrounded with tissue, a geometric tissue model was created. This was meshed with solid axisymmetric elements, CAX3 or CAX4 elements.

PATRAN was used to create the geometric model and several aspects of the finite element model. This input information was translated into ABAQUS, which performed the actual analysis as well as added the fluid elements and contact elements. ABAQUS analyzed the case study and sent the results back to PATRAN, where they were viewed and further studied.

Three basic geometries were studied: the implant model only, the implant surrounded by 2.5 radius tissue, and the implant surrounded by 4 radius tissue. The

CHAPTER 7: SUMMARY AND CONCLUSIONS

78

implant model was verified with an experimental cavity pressure comparison and deformation comparison. The general implant stresses varied with different loading conditions and boundary conditions, as well as the type of tissue and elements surrounding the implant. As expected, the stress levels in the implant itself are decreased with the addition of the surrounding tissue, which cushions the implant and absorbs some of the applied load. With larger tissue volume added around the implant, the stress in the implant is decreased even further.

Several variable studies were performed throughout this research. Varying the Poissons ratio of the implant material from 0.45 to 0.49 did not make a significant difference in the results. Changing the elastic modulus of the implant material from the modulus of a Smooth implant to the modulus of a Siltex implant has a noticeable effect on the stress results, increasing the maximum stresses by almost 8%. Changing the modulus of the surrounding tissue had marked effects as well, with stiffer tissue (E=300 psi) decreasing the implants stresses by about 60% as compared to softer tissue (E=100 psi). Another variable studied was the implant thickness, which does vary from sample to sample of breast implants. A ten percent decrease in implant thickness yielded a 17% average increase in stress experienced by the implant. Considering the element type of the surrounding tissue, changing its element type from CAX3 elements to CAX4 elements had a significant effect as well. For both the 2.5 radius and the 4 radius tissue models, using CAX4 elements produced higher overall stresses in the tissue with the same loading conditions. However, in the 2.5 tissue model, the implant itself

experienced less stress with the CAX4 tissue than the CAX3 tissue. In the 4 tissue model, the implant experienced more stress when surrounded by the CAX4 tissue elements.

The result of this effort has been the creation of a working initial finite element model of a breast implants deformation under simulated loading, examining its fundamental behavior and adjusting the model until it produced realistic shape deformations. Many different analyses were studied, producing varied stress ranges and

CHAPTER 7: SUMMARY AND CONCLUSIONS

79

results. Because there are so many variables and approximations in a model such as this, the exact results such as displacement and stress should not be taken as absolute answers, but as trends to study as the model evolves. The model is a reliable simulation of general implant behavior and will serve as a good basis for future models of this study.

CHAPTER 7: SUMMARY AND CONCLUSIONS

80

8.0 FUTURE WORK

The finite element model created for this thesiss research should be considered an initial phase of the modeling effort. There are many aspects of this model which were simplified for an initial look at the model, but should be investigated in the future.

The axisymmetric modeling approach is a good technique to optimize computing time and file size, but eventually a three-dimensional model should be created. This will significantly increase the amount of complexity involved in the model.

A concern than was mentioned in Chapter 3 is the mechanical behavior of the elastomeric silicone rubber implant material. Strain rate effects should be considered in the mechanical testing of the material. In addition, an elastomeric material behavior model could be used to obtain the material properties. Another aspect of the material behavior which could be added is the degradation effects of the bodys chemistry on the implant material.

Edge creases, which were mentioned in Chapter 2, are a common site of implant failure. This is an area of research which is currently in the stage of addition to the model. By incorporating the crease into the model, and analyzing a load case on that model, stress levels in the crease could be studied. The effects of adjusting the material thickness in this crease area could be investigated as well, suggesting design modifications which may decrease the incidence of failure due to crease formation.

Of course, the biggest area of future work is the incorporation of the finite element model into the life prediction methodology described in Chapter 1. This fatigue approach will combine the FEA results, the mechanical testing, the loading spectrum, and the fatigue analysis to predict a lifetime for a saline-filled breast implant.

CHAPTER 8: FUTURE WORK

81

REFERENCES
ABAQUS Manuals, (1997). Pawtucket, RI: Hibbitt, Karlsson, and Sorenson, Inc. Andrew, William, Inc. (1991). The effect of creep and other time related factors on plastics. Plastics Design Library, Volume 2. Bern, S., Burn, A., May, J. (June 1992). The biophysical and histologic properties of capsules formed by smooth and textured silicone implants in the rabbit. Plastic and Reconstructive Surgery, Volume 89, Number 6, 1037-1042. Byrne, J.A. (1996). Informed Consent. New York: McGraw-Hill. Cohen, K., Plastic Surgeon, Medical College of Virginia. Personal Communications, 1997. Drell, A. (1998, Sept. 6). Breast implants popular again. Chicago Sun-Times [On-line], 1-3. Available: http://www.suntimes.com/ Frontline, Public Broadcasting Systems (1998). Chronology of Silicone Breast Implants. Available: http://www2.pbs.org/wgbh/pages/frontline/implants/cron.html Hudson, P., Plastic Surgery Webpage. Available: http://phudson.com/BAM/BAMmethod.html Josefson, D. (1998). Deal expected over breast implants. British Medical Journal [Online serial], 317, 161. Available: http://www.bmj.com/ Kmietowicz, Z. (1998). Breast implants deemed safe - again. British Medical Journal [On-line serial], 317, 230. Available: http://www.bmj.com/ Plastic Surgery Information Service, Webpage Available: http://www.plasticsurgery.org/surgery/brstaugm.htm#7 Strombeck, J., Rosato, F. (1986). Surgery of the Breast. Stuttgart, Germany: Thieme Inc. Tortora, G., Grabowski, S. (1993). Principles of Anatomy and Physiology. Seventh Edition. New York: Harper Collins. Ugural, A. (1981). Stresses in Plates and Shells. New York: McGraw-Hill.

REFERENCES

82

Vasey, F.B. & Feldstein, J. (1993). The Silicone Breast Implant Controversy: What Women Need to Know. Freedom, CA: Crossing Press.

REFERENCES

83

APPENDIX A

APPENDIX A

84

*HEADING ABAQUS job created on 08-Jul-98 at 13:37:58 ** *RESTART, WRITE, FREQUENCY=1 ** *NODE 1, 0., 0.65 2, 0.238712, 0.646988 3, 0.477431, 0.639266 4, 0.715784, 0.62579 5, 0.953628, 0.605067 6, 1.19042, 0.574875 7, 1.42513, 0.531653 8, 1.65543, 0.469127 9, 1.87444, 0.374961 10, 2.05694, 0.223692 11, 2.125, 0. 13, 2.05694, -0.223682 14, 1.87436, -0.375011 15, 1.65542, -0.46913 16, 1.4251, -0.531659 17, 1.19034, -0.574888 18, 0.953524, -0.605078 19, 0.715683, -0.625797 20, 0.477316, -0.639271 21, 0.23869, -0.646989 22, 0., -0.65 100,0.,0. ** *NSET,NSET=CAVITY 100 ** *ELEMENT, TYPE=SAX1, ELSET=MEMBRANE 1,1,2 2,2,3 3,3,4 4,4,5 5,5,6 6,6,7 7,7,8 8,8,9 9,9,10 10,10,11 11,11,13 12,13,14 13,14,15 14,15,16 15,16,17 16,17,18 17,18,19 18,19,20 19,20,21 20,21,22 *SHELL SECTION, ELSET=MEMBRANE, MATERIAL=SILICONE 0.019, 3 ** ** Silicone

APPENDIX A

85

** Date: 08-Jul-98 Time: 13:23:07 ** *MATERIAL, NAME=SILICONE ** *ELASTIC, TYPE=ISO 100., 0.45 ** ** CONTACT ELEMENTS (TABLE IS THE RIGID SURFACE) ** *ELSET,ELSET=ECON,GENERATE 12,20,1 *RIGID SURFACE,TYPE=SEGMENTS, NAME=BSURF, REF NODE=22 START,0.,-.65 LINE,3.,-.65 *SURFACE DEFINITION,NAME=ASURF ECON,SPOS *CONTACT PAIR, INTERACTION=SMOOTH ASURF,BSURF *SURFACE INTERACTION, NAME=SMOOTH ** ** FLUID ELEMENTS FOR INTERIOR OF IMPLANT MEMBRANE ** *ELEMENT, TYPE=FAX2, ELSET=FLUID 101,2,1 102,3,2 103,4,3 104,5,4 105,6,5 106,7,6 107,8,7 108,9,8 109,10,9 110,11,10 111,13,11 112,14,13 113,15,14 114,16,15 115,17,16 116,18,17 117,19,18 118,20,19 119,21,20 120,22,21 *FLUID PROPERTY, REF NODE=100, TYPE=HYDRAULIC, ELSET=FLUID *FLUID DENSITY 0.0368 ** *BOUNDARY 1,1,,0. 1,6,,0. 2,1,,0. 2,6,,0. 3,1,,0. 3,6,,0. 4,1,,0. 4,6,,0.

APPENDIX A

86

5,1,,0. 5,6,,0. 6,1,,0. 6,6,,0. 7,1,,0. 7,6,,0. 8,1,,0. 8,6,,0. 9,1,,0. 9,6,,0. 10,1,,0. 10,6,,0. 11,1,,0. 11,6,,0. 13,1,,0. 13,6,,0. 14,1,,0. 14,6,,0. 15,1,,0. 15,6,,0. 16,1,,0. 16,6,,0. 17,1,,0. 17,6,,0. 18,1,,0. 18,6,,0. 19,1,,0. 19,6,,0. 20,1,,0. 20,6,,0. 21,1,,0. 21,6,,0. 22,1,,0. 22,2,,0. 22,6,,0. ** ** Step 1 - INFLATION STEP ** *STEP, NLGEOM *STATIC 0.1, 1. **PRINT,CONTACT=YES *BOUNDARY 100,8,8,0. *NODE PRINT,NSET=CAVITY PCAV,CVOL *END STEP ** ** Step 2 - SEAL CAVITY, LOAD TOP ** *STEP,NLGEOM,INC=25 *STATIC 0.1, 1.0 *BOUNDARY,OP=NEW 1,1,,0. 1,6,,0. 2,1,,0.

APPENDIX A

87

2,6,,0. 3,1,,0. 3,6,,0. 4,1,,0. 4,6,,0. 5,1,,0. 5,6,,0. 6,1,,0. 6,6,,0. 7,1,,0. 7,6,,0. 8,1,,0. 8,6,,0. 9,1,,0. 9,6,,0. 10,1,,0. 10,6,,0. 11,1,,0. 11,6,,0. 13,1,,0. 13,6,,0. 14,1,,0. 14,6,,0. 15,1,,0. 15,6,,0. 16,1,,0. 16,6,,0. 17,1,,0. 17,6,,0. 18,1,,0. 18,6,,0. 19,1,,0. 19,6,,0. 20,1,,0. 20,6,,0. 21,1,,0. 21,6,,0. 22,1,,0. 22,2,,0. 22,6,,0. *DLOAD 1,P,-3.0 2,P,-3.0 3,P,-3.0 4,P,-3.0 5,P,-3.0 6,P,-3.0 7,P,-3.0 *NODE PRINT,NSET=CAVITY PCAV,CVOL *NODE PRINT, FREQ=1 U, *NODE FILE, FREQ=1 U, ** *EL PRINT, POSITION=INTEGRATION POINT, FREQ=1 S,

APPENDIX A

88

E, ** *EL PRINT, POSITION=INTEGRATION POINT, FREQ=1, ELSET=MEMBRANE 2 3 4 S, E, *EL FILE, POSITION=INTEGRATION POINT, FREQ=1 S, E, ** *EL FILE, POSITION=INTEGRATION POINT, FREQ=1, ELSET=MEMBRANE 2 3 4 S, E, ** *EL PRINT, POSITION=NODES, FREQ=0 ** *EL FILE, POSITION=NODES, FREQ=0 ** *EL PRINT, POSITION=CENTROIDAL, FREQ=0 ** *EL FILE, POSITION=CENTROIDAL, FREQ=0 ** *EL PRINT, POSITION=AVERAGED AT NODES, FREQ=0 ** *EL FILE, POSITION=AVERAGED AT NODES, FREQ=0 ** *MODAL PRINT, FREQ=99999 ** *MODAL FILE, FREQ=99999 ** *ENERGY PRINT, FREQ=0 ** *ENERGY FILE, FREQ=0 ** *PRINT, FREQ=1 ** *END STEP showpage

APPENDIX A

89

APPENDIX B

APPENDIX B

90

*HEADING ABAQUS job created on 11-Aug-98 at 11:31:42 ** *RESTART, WRITE, FREQUENCY=1 ** *NODE 1, 1.02812E-10, -0.65 2, 0., -1. 3, 0., -0.7375 4, 0., -0.825 5, 0., -0.9125 6, 2.5, -1. 7, 0.25, -1. 8, 0.5, -1. 9, 0.75, -1. 10, 1., -1. 11, 1.25, -1. 12, 1.5, -1. 13, 1.75, -1. 14, 2., -1. 15, 2.25, -1. 16, 2.5, -2.52724E-8 17, 2.5, -0.8 18, 2.5, -0.6 19, 2.5, -0.4 20, 2.5, -0.2 21, 2.125, -2.52724E-8 22, 2.40625, 2.52724E-8 23, 2.3125, -2.52724E-8 24, 2.21875, 2.52724E-8 25, 2.05694, -0.223682 26, 1.87436, -0.375011 27, 1.65502, -0.469263 28, 1.42469, -0.53175 29, 1.18963, -0.574997 30, 0.952806, -0.605154 31, 0.714962, -0.625848 32, 0.476593, -0.639302 33, 0.237967, -0.647004 34, 0.12305, -0.759874 35, 0.340601, -0.832944 36, 0.619858, -0.811238 37, 0.878183, -0.811438 38, 1.14077, -0.797944 39, 1.39122, -0.77595 40, 2.16454, -0.806281 41, 2.27508, -0.629641 42, 2.19614, -0.154379 43, 2.05836, -0.550776 44, 1.9137, -0.723668 45, 1.65748, -0.738554 46, 0.120022, -0.886768 47, 2.35188, -0.322995 48, 2.32219, -0.115921 49, 2.16267, -0.384956 50, 0., 0.65 52, 0.238712, 0.646988

APPENDIX B

91

53, 0.477431, 0.639266 54, 0.716029, 0.625773 55, 0.953499, 0.605081 56, 1.1903, 0.574895 57, 1.42477, 0.531734 58, 1.65508, 0.469245 59, 1.87412, 0.375144 60, 2.05671, 0.223991 65, 2.5, 1. 66, 2.5, 0.2 67, 2.5, 0.4 68, 2.5, 0.6 69, 2.5, 0.8 70, 0., 1. 71, 2.25, 1. 72, 2., 1. 73, 1.75, 1. 74, 1.5, 1. 75, 1.25, 1. 76, 1., 1. 77, 0.75, 1. 78, 0.5, 1. 79, 0.25, 1. 80, 0., 0.9125 81, 0., 0.825 82, 0., 0.7375 83, 0.131899, 0.823365 84, 0.361182, 0.826555 85, 0.632088, 0.816948 86, 0.878344, 0.804611 87, 1.11857, 0.793616 88, 1.37488, 0.771929 89, 1.78556, 0.620325 90, 1.99092, 0.480206 91, 2.20349, 0.129339 92, 2.37724, 0.147047 93, 2.38068, 0.338555 94, 2.35846, 0.554459 95, 2.31742, 0.818494 96, 2.10792, 0.856537 97, 1.83514, 0.829093 98, 1.59297, 0.757333 99, 2.13213, 0.368884 100, 2.179, 0.699162 101, 2.2469, 0.482532 102, 2.26243, 0.271419 103, 1.95134, 0.69416 104, 2.10353, 0.561597 1000,0.,0. ** *NSET,NSET=CAVITY 1000 ** *ELEMENT, TYPE=SAX1, ELSET=MEMBRANE 139, 21, 25 140, 25, 26 141, 26, 27

APPENDIX B

92

142, 27, 28 143, 28, 29 144, 29, 30 145, 30, 31 146, 31, 32 147, 32, 33 148, 33, 1 149, 50, 52 150, 52, 53 151, 53, 54 152, 54, 55 153, 55, 56 154, 56, 57 155, 57, 58 156, 58, 59 157, 59, 60 158, 60, 21 *ELEMENT, TYPE=CAX3, ELSET=TISSUE 1, 4, 34, 3 2, 9, 36, 8 3, 10, 37, 9 4, 11, 38, 10 5, 12, 39, 11 6, 13, 45, 12 7, 14, 44, 13 8, 15, 40, 14 9, 15, 6, 17 10, 19, 41, 18 11, 20, 47, 19 12, 20, 16, 22 13, 23, 48, 22 14, 24, 48, 23 15, 21, 42, 24 16, 25, 42, 21 17, 27, 44, 26 18, 28, 45, 27 19, 29, 39, 28 20, 11, 39, 38 21, 38, 39, 29 22, 30, 38, 29 23, 10, 38, 37 24, 37, 38, 30 25, 31, 37, 30 26, 9, 37, 36 27, 36, 37, 31 28, 32, 36, 31 29, 8, 36, 35 30, 35, 36, 32 31, 33, 35, 32 32, 46, 7, 35 33, 34, 35, 33 34, 34, 46, 35 35, 46, 2, 7 36, 2, 46, 5 37, 8, 35, 7 38, 42, 48, 24 39, 25, 49, 42

APPENDIX B

93

40, 41, 42, 43, 44, 45, 46, 47, 48, 49, 50, 51, 52, 53, 54, 55, 56, 57, 58, 59, 60, 61, 62, 63, 64, 65, 66, 67, 68, 69, 70, 71, 72, 73, 74, 75, 76, 77, 78, 79, 80, 81, 82, 83, 84, 85, 86, 87, 88, 89, 90, 91, 92, 93, 94, 95, 96,

43, 44, 45, 45, 41, 20, 48, 44, 44, 40, 40, 43, 43, 48, 42, 41, 3, 33, 5, 34, 18, 40, 43, 25, 80, 81, 82, 82, 53, 54, 55, 56, 57, 58, 59, 60, 21, 24, 23, 22, 67, 68, 69, 72, 73, 74, 75, 76, 86, 87, 88, 76, 77, 78, 84, 85, 86,

26, 27, 28, 39, 19, 48, 20, 45, 14, 15, 43, 40, 41, 42, 49, 47, 34, 1, 46, 4, 41, 17, 49, 26, 79, 83, 83, 50, 84, 85, 86, 87, 88, 98, 89, 90, 91, 91, 91, 92, 93, 94, 95, 96, 97, 98, 88, 87, 55, 56, 75, 86, 86, 85, 53, 54, 77,

44 45 39 12 47 47 22 13 40 17 44 41 49 47 47 49 1 34 4 46 17 41 26 49 70 80 81 52 52 53 54 55 56 57 58 59 60 21 24 23 66 67 68 71 72 73 74 75 87 88 87 87 76 77 85 86 85

APPENDIX B

94

97, 78, 84, 85 98, 79, 84, 78 99, 79, 80, 83 100, 83, 82, 52 101, 52, 84, 83 102, 83, 84, 79 103, 92, 91, 23 104, 92, 66, 93 105, 93, 67, 94 106, 95, 71, 96 107, 96, 72, 97 108, 97, 73, 98 109, 98, 74, 88 110, 98, 88, 57 111, 89, 98, 58 112, 89, 59, 90 113, 60, 99, 90 114, 89, 97, 98 115, 89, 103, 97 116, 103, 89, 90 117, 104, 100, 103 118, 95, 100, 94 119, 100, 95, 96 120, 101, 104, 99 121, 104, 101, 100 122, 68, 95, 94 123, 92, 102, 91 124, 102, 101, 99 125, 93, 94, 101 126, 101, 94, 100 127, 101, 102, 93 128, 92, 93, 102 129, 97, 103, 96 130, 100, 96, 103 131, 99, 104, 90 132, 103, 90, 104 133, 66, 92, 16 134, 22, 16, 92 135, 71, 95, 65 136, 69, 65, 95 137, 91, 102, 60 138, 99, 60, 102 ** FLUID ELEMENTS FOR INTERIOR OF IMPLANT MEMBRANE ** *ELEMENT, TYPE=FAX2, ELSET=FLUID 239, 25, 21 240, 26, 25 241, 27, 26 242, 28, 27 243, 29, 28 244, 30, 29 245, 31, 30 246, 32, 31 247, 33, 32 248, 1, 33 249, 52, 50 250, 53, 52

APPENDIX B

95

251, 54, 53 252, 55, 54 253, 56, 55 254, 57, 56 255, 58, 57 256, 59, 58 257, 60, 59 258, 21, 60 ** *FLUID PROPERTY, REF NODE=1000, TYPE=HYDRAULIC, ELSET=FLUID *FLUID DENSITY 0.0368 ** ** membrane ** *SHELL SECTION, ELSET=MEMBRANE, MATERIAL=SILICONE 0.019, 5 ** ** tissue ** *SOLID SECTION, ELSET=TISSUE, MATERIAL=SILICONE 1., ** ** Silicone ** Date: 27-Jul-98 Time: 14:29:40 ** *MATERIAL, NAME=SILICONE ** *ELASTIC, TYPE=ISO 100., 0.45 ** *BOUNDARY, OP=NEW 2, 1,, 0. 2, 2,, 0. 6, 1,, 0. 6, 2,, 0. 7, 1,, 0. 7, 2,, 0. 8, 1,, 0. 8, 2,, 0. 9, 1,, 0. 9, 2,, 0. 10, 1,, 0. 10, 2,, 0. 11, 1,, 0. 11, 2,, 0. 12, 1,, 0. 12, 2,, 0. 13, 1,, 0. 13, 2,, 0. 14, 1,, 0. 14, 2,, 0. 15, 1,, 0. 15, 2,, 0. 16, 1,, 0. 17, 1,, 0. 18, 1,, 0.

APPENDIX B

96

19, 20, 65, 66, 67, 68, 69,

1,, 1,, 1,, 1,, 1,, 1,, 1,,

0. 0. 0. 0. 0. 0. 0.

** ** Step 1, inflation ** LoadCase, top_pressure ** *STEP, AMPLITUDE=RAMP, INC=10, NLGEOM This load case is the default load case that always appears *STATIC 0.1, 1. ** *BOUNDARY 1000,8,8,0. *NODE PRINT,NSET=CAVITY PCAV,CVOL *END STEP ** ** Step 2 - SEAL CAVITY, LOAD TOP ** *STEP,NLGEOM,INC=25 *STATIC 0.1, 1.0 *BOUNDARY, OP=NEW 2, 1,, 0. 2, 2,, 0. 6, 1,, 0. 6, 2,, 0. 7, 1,, 0. 7, 2,, 0. 8, 1,, 0. 8, 2,, 0. 9, 1,, 0. 9, 2,, 0. 10, 1,, 0. 10, 2,, 0. 11, 1,, 0. 11, 2,, 0. 12, 1,, 0. 12, 2,, 0. 13, 1,, 0. 13, 2,, 0. 14, 1,, 0. 14, 2,, 0. 15, 1,, 0. 15, 2,, 0. 16, 1,, 0. 17, 1,, 0. 18, 1,, 0. 19, 1,, 0. 20, 1,, 0. 65, 1,, 0. 66, 1,, 0.

APPENDIX B

97

67, 1,, 0. 68, 1,, 0. 69, 1,, 0. ** anterior_pressure ** *DLOAD, OP=NEW 64, P2, 10. 83, P3, 2. 84, P3, 3. 85, P3, 4. 86, P3, 5. 87, P3, 6. 92, P3, 7. 93, P3, 8. 98, P3, 9. 135, P3, 1. ** *NODE PRINT,NSET=CAVITY PCAV,CVOL *NODE PRINT, FREQ=1 U, *NODE FILE, FREQ=1 U, ** *EL PRINT, POSITION=INTEGRATION POINT, FREQ=1 S, E, ** *EL PRINT, POSITION=INTEGRATION POINT, FREQ=1, ELSET=MEMBRANE 2 3 4 S, E, *EL FILE, POSITION=INTEGRATION POINT, FREQ=1 S, E, ** *EL FILE, POSITION=INTEGRATION POINT, FREQ=1, ELSET=MEMBRANE 2 3 4 S, E, ** *EL PRINT, POSITION=NODES, FREQ=0 ** *EL FILE, POSITION=NODES, FREQ=0 ** *EL PRINT, POSITION=CENTROIDAL, FREQ=0 ** *EL FILE, POSITION=CENTROIDAL, FREQ=0 ** *EL PRINT, POSITION=AVERAGED AT NODES, FREQ=0 ** *EL FILE, POSITION=AVERAGED AT NODES, FREQ=0 ** *MODAL PRINT, FREQ=99999 ** *MODAL FILE, FREQ=99999 **

APPENDIX B

98

*ENERGY PRINT, FREQ=0 ** *ENERGY FILE, FREQ=0 ** *PRINT, FREQ=1 ** *END STEP

APPENDIX B

99

VITA
Kelly Anne Wilson was born in Washington, D.C. on August 15, 1975. She spent her childhood in La Plata, Maryland, and graduated as valedictorian of Saint Marys Ryken High School in 1993. She received her Bachelor of Science in 1997 from Virginia Polytechnic Institute and State University, majoring in Engineering Science and Mechanics, minoring in Mathematics and concentrating in Biomechanics. In addition to her academic pursuits, Ms. Wilson enjoys many different athletic activities, especially tennis, snow skiing, and water sports. She also spends free time drawing and playing the piano. Upon graduation, she will pursue a career in the biomedical engineering industry.

VITA

100