FEA of NIKE AIR

kenperry — Thu, 30 Apr 2009 01:41:09 +0000

My first job out of graduate school and post-doctorate work was with the footwear company, NIKE. I was fortunate to hire into the heart of the most advanced footwear technology department in the world and I could not have had a more exciting job description. I began by learning how to design NIKE AIR cushioning bladders. After becoming familiar with the design and development process I was able to make my first contribution, which was to pioneer the use of Finite Element Analysis to predict the inflated geometries of NIKE AIR bladders.

The engineers in the NIKE AIR Technology Lab were very proficient at design and had established an efficient process for prototyping new designs-at least for components based on flat film and lay-flat tubing. However, blow molded AIR bladders which were becoming quite popular required building mold tooling prior to prototyping. A design tool that allowed the refinement of a design prior to cutting tools was needed. These molds were expensive and involved several weeks of lead time. The biggest benefit of an FEA method, however, was the ability to predict the geometry of the bladders so that midsole tooling could be made for production. The current practice was to inflate ten AIR bladders, set them aside, allow them to equilibrate for 6-8 weeks and then measure them with calipers. Several mechanisms affected their change in shape but viscoelastic creep was primarily responsible for the time dependent shape change.

There had been several previous attempts to predict the inflated geometries of NIKE AIR bladders prior to my working at the company. It was generally believed that FEA would not be able to predict inflated geometries with sufficient accuracy. Furthermore, the viscoelastic behavior of the urethane elastomers was considered too complicated to characterize. Having been an ardent experimentalist challenging FEA codes for advanced elastic-plastic fracture and rock mechanics problems, I thought for sure that we would be able to utilize FEA for NIKE AIR bladders.

Force deflection data was available for the NIKE AIR bladder material but before I embarked on fitting that data to a hyperelastic model, I was curious to know what strain levels were associated with an inflated bladder. One of the first things I did was to scrounge up some polarizing filters and rig up a crude polariscope to estimate the strain in the film of an inflated bag. My estimate surprised me—less than 1% strain. I verified my measurement using a grid method and sure enough, the strains were really that low. (I also explored using mercury strain gages for directly measuring strains with some success.)

Armed with this simplification, some basic creep data for urethane, and the help of some software vendors, I was able to demonstrate excellent predictive ability of FEA in determining inflated AIR bladder shape and growth over time. The application of FEA helped reduce product development lead times and significantly decreased the cost and time to develop complex blow molded designs. This last figure illustrates how FEA could help identify “hot spots” that would not inflate uniformly. I have since left NIKE and the AIR Technology Lab but not before seeing a whole department grow up to apply FEA to cushioning technology and many other aspects of footwear and athletic equipment.

Contact Interaction for Medical Implants

kenperry — Sat, 25 Apr 2009 07:05:11 +0000

There are many circumstances when it is necessary to model contact and contact interactions when analyzing medical implants. Such circumstances arise when devices interact with tooling, catheters, vessels and when self-contact occurs. This latter situation arises for example when a stent is crimped down tightly to catheter dimensions.

ABAQUS/Standard provides a range of methods for defining and managing contact in FEA simulations. One first defines a master surface and a slave surface which can be based on node or elements sets and/or analytically defined surfaces. Then one must select a contact interaction model and ascribe specific properties to that model. The image on the left shows both node and element sets used in a typical contact definition for self-contact of a stent.

Considerable care must be used to define appropriate surfaces. Contact interactions are computationally expensive and although ABAQUS efficiently manages their computational cost, considerations such as smoothness, consistency and other geometric factors need to be considered to maintain solution stability.

ABAQUS provides a variety of contact interaction models for mechanical contact. These include “hard” contact, “softened contact”, “no separation” to name just a few. Hard contact is the most simple as it simulates no reaction pressure until contact occurs then a quick ramp up as “penetration” increases. Softened contact provides a small, exponentially increasing contact pressure just prior to penetration and increasing pressure thereafter. The no separation model provides increasing pressure as penetration is increased and maintains contact with negative pressure if the surfaces attempt to move away from one another. The behavior of softened contact and no separation contact models are illustrated in the plots below.

Each of these various models have utility in simulating implantable medical devices. For example, the hard contact model and occasionally the no separation model are useful in simulating the interaction of devices with tooling during processing and manufacture and also modeling the interaction of the device with a catheter. The softened contact model is useful for simulating a device when interacting with tissue. Regardless of the model chosen, it is important to experiment with and evaluate the effects of the chosen parameters for the models. The selection of these parameters will affect the solution and therefore it is important to study such effects and verify that the results make sense for the problem being considered.

The Table below summarizes one such study using different models and sets of parameters for typical stent analysis scenarios. For this Table, a two-strut model is crimped to catheter dimensions using different contact interaction models. As much as 0.2% strain difference occurs between the hardest and the softest of the various models considered.

Interpreting FEA Results: Integration Point Data

kenperry — Wed, 15 Apr 2009 23:50:56 +0000

Finite Element Analysis (FEA) can produce an enormous amount of data as output. Solution variables such as stress and strain are computed throughout an analysis for each increment and at each location within the model. These solution variables are computed at what are called “integration points”. These locations ARE NOT the same as the nodes of an element and it is important when post-processing FEA results to understand how the actual solution data is used to create contour plots, and how to extract accurate data representing the solution of the problem you are modeling. As is generally the case, it is the responsibility of the analyst to make sure the engineering is consistent with the problem at hand.

During a typical non-linear FEA solution process, numerous increments are taken to establish an equilibrated solution for the given applied loading. Stress equilibrium, strain compatibility and other mechanics equations are simultaneously “solved” by adjusting local solution variables such as stress and strain throughout the entire model being analyzed. These equations are written in such a way as to ultimately satisfy equilibrium conditions at an elemental level—the details of which depend on the shape function of the element being used. Regardless of element type and formulation, the shape functions determine how the discrete solutions for field variables like stress and strain are represented throughout an element, and compared with forces and displacements to evaluate the various equations governing the solution of the problem.

What is important to understand is that while forces and displacements are computed at nodal locations, stresses and strains are computed at integration points. The figure above for a typical 8-noded, linear, three-dimensional element illustrates the difference between nodal locations and integration points. The nodal locations are at the corners of the cube while the integration points are located within the element.

In order to generate contour plots from FEA results, it is necessary to extrapolate the stress or strain values from the integration points to the nodal locations. Since each node in a model will generally be shared by more than one element these extrapolated values will also have to be averaged in order to produce a smooth contour plot. While there are parameters that can be set to control how this process is handled by your post-processing software, there are many factors which can affect the accuracy of the extrapolated values.

The degree to which the contour plot data differs from the actual data depends on the element type/formulation and particularly on the steepness of the underlying field variable gradient and to a large extent the quality of the underlying finite element mesh. Large gradients and a coarse mesh will obviously produce a greater degree of difference between the integration point data and extrapolated nodal averages.

Relying upon discrete data taken from contour plots for stress or strain can be misleading and inconsistent between various analysis runs. One reliable method for extracting specific stress and strain values is to use “integration point” data. In this way, you are assured of getting an accurate stress or strain value that relates directly to the solution of the underlying mechanics equations. However, in the case of performing a fatigue analysis, for example, stresses and strains at the surface of a component may be more relevant, as it is well known that cracks and defects generally initiate on the surface a part. In such a case, it is the analysts responsibility to understand the impact of using either integration point data or averaged nodal data.

The contour plot below on the left was produced with the nodal averaging turned off. You can see that when the nodal data is extrapolated for each element that the result produces discontinuities between adjacent elements. This is inevitable because the variation of stress and strain over an element is much more complicated than a simple linear relationship. The contour plot on the right was produced by turning nodal averaging back on. It is much smoother, but that smoothness comes with a loss of information.

Evaluating Design Instabilities with FEA

kenperry — Fri, 10 Apr 2009 16:41:07 +0000

Finite Element Analysis is routinely used to evaluate the performance and durability of medical devices. When using an implicit method such as ABAQUS/Standard, FEA can also be used to evaluate the geometric stability of a proposed design. Such issues could arise for example when designing stents for large vessels, such as the aorta, when the large diameters exceed the length of the stent. When the length/diameter aspect ratio of a stent exceeds one, stability of a design could be an issue, with unstable deformation occurring causing the stent to dislodge and turn sideways in the vessel.

We routinely evaluate stent components for stability and occasionally are required to make suggestions for improving a component’s stability. In the plot above showing lateral force as a function of diameter, the original (in blue) and improved design (in red) demonstrate the tendency of a device to remain stable. The further into negative territory of lateral force for any given design directly correlates to a device becoming unstable. The design represented by the blue curve quickly turns into negative territory and remains there throughout most of the loading. The curve in red shows a dramatic improvement with only a portion of the loading curve becoming negative and then with only a small magnitude.

The images below illustrate buckling behavior of a stent with the image on the right becoming unstable.

FEA Geometry and Edge Detail

kenperry — Mon, 06 Apr 2009 22:32:47 +0000

A typical process for making stents is electropolishing to remove material and processing defects and to impart a smooth finish with rounded corners. It is well known that a polished part will have superior fatigue resistance, but how much does the rounding of edges affect the stress and strain in the stent when loaded?

We studied the effect of material removal using a generic Nitinol two-strut stent model. In the figure to the left are four models: From left to right, a typical stent geometry meshed with no consideration for edge detail; a model with a 50 micron chamfer; a model with a 100 micron chamfer; and finally, a model with a 100 micron radius. These four geometries were analyzed by simulating catheter crimp loading. When crimped to minimum dimensions, the strains were as follows:

As can be seen, there is very little impact of the chamfer or the radius on the predicted strain values. These results give credence to the standard practice of neglecting the effect of edge features. It is common, however, to account for the effects of electropolishing by removing an appropriate amount from the as-cut laser geometry. As will be discussed in subsequent posts, verification of actual component geometry is a very important part of the FEA process.<-->

Finite Element Optimization of Medical Implants

kenperry — Fri, 27 Mar 2009 09:05:14 +0000

Finite Element Analysis is an excellent engineering tool for optimizing medical implants. It provides a fast and reliable method for evaluating both the performance and safety issues associated with any given product. A variety of design concepts can be evaluated and relative safety factors determined for the full size range of an intended product.

Parametric studies are conveniently carried out and relative improvements in performance are clearly distinguished in objective engineering terms. Interactions of the device with the human body can be performed and can incorporate bench, animal and human data to improve predictive capabilities. Self-consistent methodology provides a rational foundation to make improvements on existing technology.

Advances in mechanical testing, materials selection and processing continue to provide more choices for the design and implementation of existing and new concepts for minimally invasive medical therapies. Finite Element Analysis provides the capability to keep up with these changes and offers an ideal methodology to minimize risk, shorten development time and increase confidence in the development of life saving technology.

The Selection of Nitinol Material Models for FEA Simulations

kenperry — Fri, 02 Jan 2009 04:54:03 +0000

Nitinol is a unique metallic alloy that is ideally suited to use in medical devices. It has excellent biocompatibility and most of all it has the ability to undergo significant recoverable deformations. This allows devices made with Nitinol to be reduced to catheter dimensions and expanded at the implant site.

Much work has been done to characterize Nitinol from a materials science perspective. It is a multi-phase material with a parent and a transformed phase. In its most common application, the parent phase is transformed under the application of stress to yield stress-induced martensite. This results in a stress-strain curve with a plateau that is primarily a function of the austenite transformation temperature of the material. Complications arise because the material has multiple phases, the loading curve involves hysteresis, the material response is history dependent and the material is particularly sensitive to processing conditions.

Finite Element Analyses of Nitinol medical implants require the analyst to choose a material model and calibrate that material model. This poses a challenge as a comprehensive description of Nitinol’s unique response remains incomplete. The choices range from complex micromechanical models that involve keeping up with 18 or more crystallographic representations to simplified phenomenological models that capture the austenite loading slope, plateau and martensite loading slope. Some models capture the difference between tension and compression behavior, some can accomodate shake-down effects and others cover both superelastic and shape memory characteristics.

There is no clear answer as to which material model is most appropriate for a given application. It all depends on the purpose of the analysis. For many applications involving predicting the safe fatigue life of a component, generally, a simple tri-linear phenomenological model that is calibrated appropriately is sufficient and appropriately conservative. In cases where shape memory recovery is involved, a more sophisticated material model would be required.

The more important questions to ask and answer depend on the calibration of the material model and the application to the in-use conditions. This includes both the stress-strain of force-deflection behavior as well as the material limit criteria. Because Nitinol is so sensitive to processing history it is generally far more effective to establish a self-consistent quality program based on readily measurable parameters than to involve complex representations of constitutive behavior with inadequate calibration. In this way, statistics and experience can help strengthen the confidence in engineering judgments made in the course of developing implantable medical devices.

Complex loading conditions involving superimposed torsion, bending, axial extension and compression challenge ALL material fatigue theories. Medical devices are unique in that they are architectural structures where designers and engineers need to assure safe lifetimes with an incredibly low tolerable failure rate. A common approach that has gained much acceptance is to utilize a calibrated material model for Nitinol and a Finite Element Analysis of a fatigue coupon sample to generate a fatigue limit in terms of local strain versus number of cycles to failure. While this is only a one-dimensional approach, it has proven quite useful and can be implemented with readily available test equipment.

While much work remains to be done to develop, validate and generalize predictive methods for evaluating the safe lifetime for implantable devices, there are many successful examples of self-consistent approaches for specific device families.

Some general guidelines to follow are:

1) Start simple and add complexity to your model step by step.

2) Validation is a process: go back and forth between computational and experimental result.

3) Bound all unkown parameters and do systematic studies to identify sensitive factors.

4) Remember: “The purpose of computing is insight, not numbers”. Learn as you go and keep the focus on improving the design and manufacturing of the product.

Medical Implant Material Fatigue Research

kenperry — Thu, 18 Dec 2008 06:39:54 +0000

With the growing use of Nitinol in medical implants, there is a need for improved characterization of the material behavior of Nitinol and methodologies for better product design and engineering. While it is a good starting point, the typical approach of employing the force-deformation response from uniaxial tension tests for input and validation of material models is rather limited. In particular, the ambiguities associated with the global versus local stress strain curve make the interpretation of finite element analysis non-trivial.

To address these concerns, we’ve developed sophisticated methods in our laboratory to study the initiation of cracks in Nitinol. We have studied closely fatigue loading of carefully designed coupon samples to differentiate between cracks forming in austenite, martensite and mixed phase conditions. Usisng closed loop cyclic loading and real time interferometric measurements we continue to make advances in understanding the complex fatugue behavior of implantable metal alloys.

You can download a draft of our paper to be published in the second ASTM Special Technical Publication on Metallic Medical Implant Alloys.

Medical Imaging Data and Computational Fluid Dynamics

kenperry — Fri, 24 Oct 2008 05:02:58 +0000

Significant advances are being made in simulations for medical devices. The picture on the left, shared with me by Dr. Tina Morrison, former post-graduate student in Charles Taylor’s group at Stanford University shows the predicted pressures in a patient specific aorta.

Flow and pressure waves emanate from the heart and travel through the major arteries where they are damped, dispersed and reflected due to changes in vessel caliber, tissue properties and branch points. For example you can learn about the coupled multidomain method which was successfully applied to solve the non-linear one-dimensional equations of blood flow with a variety of models of the downstream domain and recently extended to three-dimensional finite element modeling of blood flow and pressure in the major arteries in Comput. Methods Appl. Mech. Engrg. 195 (2006) 3776–3796.

The ability to utilize patient specific medical imaging data depends is revolutionizing the treatment of individual patients and providing a means to better understand the boundary conditions experienced by implantable medical devices. In another image shared with me by Dr. Morrison below a stent is imaged in a descending aorta aneurism. By combining advanced imaging techniques, computational fluid mechanics simulations and Finite Element Analysis (FEA) engineers are taking one step closer to fully describing the mechanics of a medical implant in the human body.

Suture Clip for Percutaneous Mitral Valve Repair

kenperry — Fri, 24 Oct 2008 01:55:43 +0000

This is a picture of an excised mitral valve from a pig with suture and a clip holding the leaflets together in a novel approach to treating mitral valve regurgitation. It was placed percutaneously using a specially designed catheter. The superelastic Nitinol clip was designed and developed using Finite Element Analysis (FEA).

You can download the patent protecting this remarkable technology that describes in detail the mitral valve repair system capable of applying a suture to the tissue and a fastener to the suture.

Computing Alternating and Mean Stresses During Fatigue for a Cardiovascular Stent

kenperry — Mon, 20 Oct 2008 23:32:40 +0000

Finite Element Analysis (FEA) is routinely used to perform fatigue analyses of cardiovascular stents. For the case of balloon expandable stents, this means modeling the crimping of the stent onto the delivery balloon, the expansion and recoil of the stent as would occur during deployment and finally the simulation of fatigue deformations. Fatigue deformations typically involve uniform radial pulsatile loading and/or bending of the stent between two different radii of curvature. A safety factor is determined by computing the alternating and mean stresses for the given cyclic loading conditions and comparing them to allowable material limits using a Goodman-type approach.

A simple method for determining the safety factor is to compute the alternating and mean stresses from the principle stress components for the minimum and maximum extremes of the cyclic loading conditions. The ratios of the alternating stress and endurance limit and the mean stress and the ultimate strength are combined and equated to the reciprocal of the safety factor, N.

This equation is evaluated for each integration point in the model. But as was discussed in our most recent ASTM F04.30.06 Fatigue to Fracture task group, this approach has several shortcomings.

An alternative approach is to use the individual stress components with respect to the global coordinate system for the two fatigue conditions and compute the individual alternating and mean stress components according to

These individual alternating and mean stress components are used to compute an effective alternating and an effective mean stress using

Subsequently, the effective alternating and mean stress values are used to compute a safety factor according to

An alternative approach would be to use the three principle stress components and compute the three alternating and mean principle stresses and then compute the effective stress according to the Gough–Pollard model; however, this approach still does not account for the effect of rotations in stress space on the mean and effective stress.

A more rigorous approach is to compute the alternating and mean stress components according to an element local coordinate system. Principal values of the stress tensor and associated maximum planes can then used in subsequent fatigue analysis.

Consistency and careful comparison to experimental data are indicated as large deformations and non proportional loading are common to most if not all implantable medical devices.

ASTM Standard for FEA of Metallic Vascular Stents

kenperry — Wed, 16 Jul 2008 00:54:06 +0000

Follow this link to the ASTM website and find the long awaited for “Standard Guide for Finite Element Analysis of Metallic Vascular Stents Subjected to Uniform Radial Loading”.

This guide establishes general requirements and considerations for using finite element analysis techniques for the numerical simulation of metallic stents subjected to uniform radial loading. These stents are intended for use within the human vascular system.

It was developed in the F04.30.06 subcommittee for Cardiovascular Device Standards. The co-chairs of the group are Ken Cavanaugh and Eitan Konstantino and we have about 40 active members with two face to face meetings per year. There are numerous work items under way and new members are always welcome. Please contact me for more information on joining our group.

Comprehensive Fatigue Analysis: Complex Loading of Implantable Medical Device

kenperry — Sat, 23 Feb 2008 00:36:05 +0000

Medical device manufacturers are increasingly required to demonstrate that their products are safe and effective when subjected to complex loading conditions in the human body such as when the device may experience combinations of bending, twisting and compression. Physical test methods are difficult to implement in such cases, can only consider a finite number of conditions and do not provide prompt relevant feedback to the medial device design process.

Dr. Paul and I have developed a comprehensive methodology for quantifying the fatigue performance of devices subjected to multiple coupled loading conditions. It is relevant for quantifying the fatigue performance as required by the FDA of peripheral vascular stents and other devices with FEA that experience coupled multiple loading conditions and is based on a stochastic implementation of Miners rule.

Please contact me for more information.

Carotid Artery Stent Fractures: An Engineer’s Perspective

kenperry — Wed, 13 Feb 2008 01:47:31 +0000

You can download my presentation at the 2007 Cleveland Clinic Stent Summit on carotid artery stent fractures from an engineers perspective which discusses combined loading conditions, fatigue, material limits and other factors.

Characterization of Nitinol Material Behavior for the Design and Validation of Medical Implants

kenperry — Mon, 08 Oct 2007 01:05:12 +0000

: Direct strain measurements in AAA stent using phase shifted moire interferometry.

You can download a poster I presented at the MPMD fall 2007 conference illustrating our method for characterizing Nitinol material behavior for the design and validation of medical implants.

Real Time Moire Interferometric Measurements of Nitinol Fatigue

kenperry — Wed, 06 Jun 2007 01:12:54 +0000

You may view an animation in real time of a crack growing in a Nitinol fatigue specimen observed using moire interferometry while the test was being conducted in our Bose Electroforce test machine that shows a moving transformation zone and perceptible fringes captured at 30 frames per second.

Stent Performance Characterization

kenperry — Sun, 03 Jun 2007 06:35:57 +0000

Radial force behavior is one of many engineering design criteria important to the design of implantable medical devices such as stents. Interpretation and extrapolation of bench-top data to predict in-vivo performance necessitates a thorough understanding of influence parameters such as boundary conditions and material uncertainty. An integrated modeling and test validation approach is needed to fully understand interactions of the influence parameters. This understanding helps establish reliable fatigue prediction methodologies that combines the load and displacement type boundary conditions. The approach is more broadly applicable to the unusual and complicated superelastic transformation behavior observed in Nitinol.

You can download our paper presented at the Symposium on Implant Mechanics during the Society for Experimental Mechanics 2007 Spring Conference where we discuss stent radial force performance, FEA, contact issues, experimental and material parameters associated with different radial force test methods and much more.

Full-field Measurement of Fracture Initiation in Nitinol

kenperry — Fri, 01 Jun 2007 07:02:43 +0000

Phase shifted moire interferometry of crack and transformation zone in Nitinol fatigue specimen.

You can download our presentation of Nitinol fatigue and fracture initiation using phase shifted moire interferometry.

Biological and Implant Mechanics Symposium at the 2007 SEM Annual Conference in Boston

kenperry — Sun, 06 May 2007 01:29:09 +0000

You can download the brochure for this special symposium that brings together state-of-the-art developments in clinical imaging techniques, computer modeling, medical device testing and materials characterization with a focus on medical implants, their design and the Experimental Mechanics underlying device interaction with the human body.

Full-Field Measurement of Strain and Transformation in Nitinol

kenperry — Wed, 31 May 2006 23:51:11 +0000

Phase shifted moiré interferometry is used to measure full-field strain during uniaxial tension and four point bend loading of nitinol test samples. Differences between global and full field measurements reveal the effects of localized transformation behavior. Results for two heat treatments of commercially available superelastic Nitinol are presented for tests conducted under controlled temperature conditions. The results highlight the effect of martensite, austenite and R-phase transformations on the thermomechanical response of superelastic nitinol. Finally, the technique is applied to a nitinol implantable medical component to demonstrate the opportunities for improved material characterization, numerical modeling and design validation.

You can download our paper on strain measurement and phase transformation in Nitinol using moire interferometry that we presented at the 2006 SMST conference.

FEA and Nitinol: Beyond the Fundamentals

kenperry — Fri, 05 May 2006 06:15:29 +0000

At the 2006 SMST Conference in Asilomar Dr. Paul and I had he privilege of sharing our experience of working with Nitinol and particularly FEA of Nitinol during a full day tutorial. It was an honor to have an hour to discuss the ins and outs of modeling Nitinol using FEA. You can download our presentation of the fundementals of modeling Nitinol using Finite Element Analysis (FEA) including all the details of nonlinear constitutive behavior, contact, boundary conditions, element choices, validation and much more.

Emerging Transcatheter Technologies

kenperry — Fri, 03 Mar 2006 03:44:30 +0000

You can download a presentation of emerging transcatheter devices and technologies that I put together from the engineering design perspective that includes AAA solutions, fenestrated grafts, embolic protection devices, vena cava filters, stents, closure devices coronary sinus devices and percutaneous heart valves and repair technologies.

Thermoelastic Transformation Behavior of Nitinol

kenperry — Mon, 05 Dec 2005 06:24:56 +0000

The transformation behavior of Nitinol under uniaxial tension and four-point bending was investigated. A novel sample geometry produced from drawn tubing was used to observe the differences caused by localized phase transformation effects between the two types of loading and between samples with different process and load histories. Phase shifted moiré interferometry was used to provide full-field measurement of strain during the experiments. Optical resolution and grating coherence were sufficient to simultaneously resolve the strain fields within both the parent and transformed phases of the material. Evidence of both localized and uniformly distributed phase transformation is observed for the samples tested in tension while the bending results clearly indicate an asymmetric neutral axis and a complex reverse bending response for samples containing a strong R-phase component and tested at temperatures below critical transformation temperatures. You can download our paper that describes our approach of using moire interferometry to characterize the mechanical behavior of Nitinol and our novel four-point bending test rig and our results showing the influence of R-phase and phase transformations.. It was published by ASTM in 2005.

Phase Transformations in Nitinol

kenperry — Fri, 27 Aug 2004 02:41:15 +0000

Nitinol is well suited to the design constraints imposed by medical device applications, however, only modest progress has so far been made regarding long term predictions of the structural integrity of such components.

Challenges in predicting long term reliability of superelastic NiTi medical components include the consequences of manufacturing tolerances, uncertainty with regard to in vivo loading and the inherent complexity of superelastic material behavior. In this article, we focus on the latter challenge and discuss ongoing research to characterize the effects of phase transformation and accurately obtain calibrated material constitutive relations for polycrystalline Nitinol materials.

Our approach involves a combination of full-field strain measurements using phase shifted Moiré interferometry and the development of improved finite element methodology to account for various material behaviors and simulated conditions. As you can see in our presentation, phase shifted Moiré interferometry provides unprecedented accuracy in the measurement of strains and displacements in the vicinity of stress risers such as notches and can be used to guide and verify finite element models for implantable superelastic devices.

We originally presented this work at the American Society for Materials (ASM) conference in 2004.

Reliability Assessment of Superelastic Medical Devices

kenperry — Fri, 16 Jul 2004 00:22:03 +0000

A series of phase shifted moiré interferograms showing a NiTi dogbone experiencing increased tensile loading. The two images on the right exhibit clear Luders bands.

You can download our brief paper describing our use of moire interferometry to measure properties of superelastic Nitinol for the reliability assessment of medical devices.

LifeStent NT Self-Expanding Helical Stent

kenperry — Sun, 16 Nov 2003 00:09:30 +0000

The 6F LifeStent NT is an implantable self-expanding nickel titanium alloy (Nitinol) stent. The stent is manufactured from small diameter Nitinol tubing and is loaded into a delivery catheter for placement/deployment into a vessel.

The stent is based on a helical design which offers a wide range of performance advantages when compared to stents with circumferential hoops. The helix pattern is inherently more flexible than circumferential hoop designs because a helix has an additional degree of flexibility (torsion) with respect to longitudinal bending. This additional degree of freedom imparts a high degree of kink resistance and enables the helical stent to maintain excellent wall apposition under the combined effects of bending, twisting and stretching.

The LifeStent NT achieves this enhanced flexibility while maintaining the same radial force characteristics as similar 6F circumferential designs manufactured from Nitinol tubing. This is possible because radial stiffness and chronic outward forces depend primarily on the dimensions of the struts and the helical design dictates only the patterns of connections, or bridges, between the struts. The LifeStent NT therefore combines the flexibility benefits of a helical architecture and the radial force and tight mesh density of a Nitinol tubing stent.

You can download an abstract describing the benefits of the LifeStent NT Self-Expanding Helical Stent.

You can also download a presentation describing my inspiration for the LifeStent NT Self-Expanding Helical Stent based on biomimicry and the mathematical beauty of the helix in nature.

I’ve also included here a link to the patent that describes a highly flexible stent having a central helical wound portion, and another link to a patent that describes the bridges and the transition zone utilized in the Lifestent NT.

Effects of Notches and Grain Size on Transformations in Nitinol

kenperry — Wed, 07 May 2003 03:43:25 +0000

In this paper, we present a research methodology to characterize the effects of crystallographic orientation and grain size on the deformations and transformations in Nitinol.

The approach involves a combination of full-field strain measurements using Moiré interferometry and finite element modeling. We explore the effects of localized stress raisers such as notches and grain boundaries, and discuss implications for medical device design.

FEA and Experimental Evaluation of Superelastic Stent

kenperry — Tue, 06 May 2003 03:51:39 +0000

The mechanical properties of Nitinol stents are normally evaluated experimentally due to complexities resulting from large deformations and material nonlinearity. Despite difficulties associated with Finite Element Analysis (FEA), the success of computational analysis in combination with experimental study leads to better understanding of stent performance. This paper compares experimentally evaluated radial resistive forces of a Nitinol stent to predictions based on nonlinear FEA. The FEA was performed using ABAQUS with two user material subroutines independently developed specifically for Nitinol. Good agreements between the FEA and the experiments are shown for both user material subroutines.

In this work I debuted the ABAQUS user material subroutine that we developed in my lab for modeling noth superelastic and shape memory Nitinol applications. It is based on the Boyd-Lagoudas formulation which is a phenominalogical thermodynamic model that we implemented for industrial use in medical device validation analyses.

You can download this paper on superelastic stents, radial force, nonlinear FEA, ABAQUS and user masterial subroutines that was originally published in the SMST 2003 Proceedings.

Modeling Polycrystaline Nitinol

kenperry — Sun, 25 Aug 2002 04:32:26 +0000

There are many ways to model Nitinol using Finite Element Analysis. Over the years we have studied them all, from rigorous analytical implementations based on micromechanical descriptions to phenomenological models based on thermodynamics. As with all simulations, the level of detail and approach taken to implement the constitutive behavior of a material is driven by the specific purpose of the analysis and the available information.

The picture above illustrates a particularly creative approach that was developed by my very good friend and colleague Paul Labossiere. In this work, he utilized our thermodynamic user subroutine (UMAT) for ABAQUS but implemented it with a very clever script that generated finite elements with random properties for our UMAT. With this model, we were able to explore numerous aspects of modeling the constitutive properties of Nitinol and the limitations of different assumptions.

The image above compares a continuum model with a polycrystalline model. All of our analysis results were compared to experimental measurements and as a result of this research we were able to definitively identify the critical attributes of modeling superelastic Nitinol.

Nonzero Mean Fatigue Testing of Nitinol

kenperry — Wed, 02 Jan 2002 03:22:27 +0000

This paper describes a fatigue test protocol that was used to determine the factor of safety for a superelastic Nitinol implantable medical device. A rotating cam test apparatus was designed to collect the necessary life-cycle data. Fatigue test specimens were designed as scaled-up versions of the implantable device and processed in accord with the established manufacturing specifications for the actual device. This insured that the local strain conditions as well as material processing effects would be accounted for in the characterization of the material’s fatigue limit. You can download our paper on superelastic Nitinol fatigue that was published in the Society for Experimental Mechanics journal Experimental Techniques. The work was also published in the SMST 2000 Proceedings.

Original Inspiration for ECHOBIO

kenperry — Sun, 21 Nov 1999 06:32:37 +0000

In 1998 I founded ECHOBIO to invent and develop new materials that would transform the world. It was a heady goal but I strongly believed—and still do—that there is an enormous, untapped potential in looking to nature for inspiration and opporunities for sustainable solutions to technical problems.

My original plan was to develop novel materials for medical applications where the high margins and low volumes would be conducive to starting from scratch with a new material. Once we were succesful in these markets, we would work to roll these materials out to other industrial markets where the volumes would be higher and the margins smaller.

I got as far as raising money to explore a solution for repairing Anterior Cruciate Ligaments (ACL) using mussel adhesive protein. Inspired by the inital work of Herb Waite, I sought out utilizing a chemical mimic of mussel adhesive protein and began working with Professor Tim Deming. Prof. Deming had succesfully isolated a critical component of the protein responsible for the remarkable, aqueous adhesion of mussel adhesive protein. Unfortunately, there were still some missing elements of the process that we needed for a succesful product. Despite several attempts to attach chicken ligaments with our synthetic analogs, we were not able to achieve sufficient bond strengths. I estimated that it would take hundreds of thousands of dollars to adequately research and identify the missing chemical elements and that was well beyond the risk tolerance of any investor.

My vision of “Knee Glue” didn’t make it into the 21st century, but my passion for finding a way to bring organic solutions into the world continues on.

Transrenal AAA Stent

kenperry — Fri, 01 Jan 1999 04:23:23 +0000

One of the very first stent designs I worked on was the transrenal stent for TeraMED’s Ariba bifurcated graft system. This was an early generation Nitinol AAA stent system made from superelastic tubing. What was remarkable about this product was the high level of integrity that TeraMED insisted on from everyone involved in the design and development.

I’ll never forget how the product champion described the level of rigor that TeraMED required – “Would you put this in your grandmother?” I have worked with only a few companies that even compare to how eager TeraMED was to insure the safety and efficacy of their product. It is fair to say that my high standards in the field of engineering medical devices got a great head start through my involvement with this product.

Terms Of Use

andyux — Tue, 20 Oct 1992 00:27:16 +0000

By using echobio.com and drperry.org, you are agreeing to comply with and be bound by the following terms of use. Please review the following terms carefully. If you do not agree to these terms, you should not review information on this site.

Echobio.com and drperry.org makes no representations or warranties, express or implied, with respect to the document, or any part thereof, including any warrantees of title, noninfringement of copyright or patent rights of others, merchantability, or fitness or suitability for any purpose.

Acceptance of Agreement. You agree to the terms and conditions outlined in this Terms of Use Agreement (“Agreement”) with respect to our site (the “Site”). This Agreement constitutes the entire and only agreement between us and you, and supersedes all prior or contemporaneous agreements, representations, warranties and understandings with respect to the Site, the content, products or services provided by or through the Site, and the subject matter of this Agreement. This Agreement may be amended at any time from time to time by us without specific notice to you. The latest Agreement will be posted on the Site, and you should review this Agreement prior to using the Site.

Copyright. The content, organization, graphics, design, compilation, magnetic translation, digital conversion and other matters related to the Site are protected under applicable copyrights, trademarks and other proprietary (including but not limited to intellectual property) rights. The commercial copying, redistribution, use or publication by you of any such matters or any part of the Site is strictly prohibited. You do not acquire ownership rights to any content, document or other materials viewed through the Site. The posting of information or materials on the Site does not constitute a waiver of any right in such information and materials.

Trademarks. Any mark, logo, symbol, nickname, letter(s), word(s) or combination of these that can be associated with echobio.com and drperry.or qualifies as a trademark. “drperry.org”, “echobio”, as well as logos, seals, are either trademarks or registered trademarks. Other product and company names mentioned on the Site may be trademarks of their respective owners.

Information on Site. We cannot and do not warrant that the information on the site is absolutely current, although every effort is made to ensure that it is kept as current as possible. Individual Web sites have modification dates that can be used as guides to the timeliness of the data; however, we cannot warrant that no changes have been made to the source information since that date. Similarly, We cannot and do not warrant the accuracy of these documents beyond the source documents, although we do make every attempt to work from authoritative sources.

Editing, Deleting and Modification. We reserve the right in our sole discretion to edit or delete any documents, information or other content appearing on the Site.

Indemnification. You agree to indemnify, defend and hold the owners of echobio.com and drperry.org, and our partners, officers, directors, attorneys, staff, employees and affiliates (collectively, “Affiliated Parties”) harmless from any liability, loss, claim and expense, including reasonable attorneys’ fees, related to your violation of this Agreement or use of the Site.

Nontransferable. Your right to use the Site is not transferable. Any password or right given to you to obtain information or documents is not transferable.

Disclaimer and Limits. THE INFORMATION FROM OR THROUGH THE SITE IS PROVIDED “AS IS,” “AS AVAILABLE,” AND ALL WARRANTIES, EXPRESS OR IMPLIED, ARE DISCLAIMED (INCLUDING, BUT NOT LIMITED TO, THE DISCLAIMER OF ANY IMPLIED WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE). THE INFORMATION AND SERVICES MAY CONTAIN BUGS, ERRORS, PROBLEMS OR OTHER LIMITATIONS. WE AND OUR AFFILIATED PARTIES HAVE NO LIABILITY WHATSOEVER FOR YOUR USE OF ANY INFORMATION OR SERVICE. IN PARTICULAR, BUT NOT AS A LIMITATION THEREOF, WE AND OUR AFFILIATED PARTIES ARE NOT LIABLE FOR ANY INDIRECT, SPECIAL, INCIDENTAL OR CONSEQUENTIAL DAMAGES (INCLUDING DAMAGES FOR LOSS OF BUSINESS, LOSS OF PROFITS, LITIGATION, OR THE LIKE), WHETHER BASED ON BREACH OF CONTRACT, BREACH OF WARRANTY, TORT (INCLUDING NEGLIGENCE), PRODUCT LIABILITY OR OTHERWISE, EVEN IF ADVISED OF THE POSSIBILITY OF SUCH DAMAGES. THE NEGATION OF DAMAGES SET FORTH ABOVE IS A FUNDAMENTAL ELEMENT OF THE BASIS OF THE BARGAIN BETWEEN US AND YOU. THIS SITE AND THE INFORMATION WOULD NOT BE PROVIDED WITHOUT SUCH LIMITATIONS. NO ADVICE OR INFORMATION, WHETHER ORAL OR WRITTEN, OBTAINED BY YOU FROM US THROUGH THE SITE SHALL CREATE ANY WARRANTY, REPRESENTATION OR GUARANTEE NOT EXPRESSLY STATED IN THIS AGREEMENT.

ALL RESPONSIBILITY OR LIABILITY FOR ANY DAMAGES CAUSED BY VIRUSES CONTAINED WITHIN THE ELECTRONIC FILE CONTAINING THE FORM OR DOCUMENT IS DISCLAIMED. WE WILL NOT BE LIABLE TO YOU FOR ANY INCIDENTAL, SPECIAL OR CONSEQUENTIAL DAMAGES OF ANY KIND THAT MAY RESULT FROM USE OF OR INABILITY TO USE OUR SITE. OUR MAXIMUM LIABILITY TO YOU UNDER ALL CIRCUMSTANCES WILL BE EQUAL TO THE PURCHASE PRICE YOU PAY FOR ANY GOODS, SERVICES OR INFORMATION.

Use of Information. We reserve the right, and you authorize us, to use and assign all information regarding Site uses by you and all information provided by you in any manner consistent with our Privacy Policy.

Links to Other Web Sites. The Site contains links to other Web sites. We are not responsible for the content, accuracy or opinions express in such Web sites, and such Web sites are not investigated, monitored or checked for accuracy or completeness by us. Inclusion of any linked Web site on our Site does not imply approval or endorsement of the linked Web site by us. If you decide to leave our Site and access these third-party sites, you do so at your own risk.

Information and News Releases. The Site contains information and news releases about us. While this information was believed to be accurate as of the date prepared, we disclaim any duty or obligation to update this information or any news releases. Information about companies or organizations other than ours contained in the news release or otherwise, should not be relied upon as being provided or endorsed by us.