DrPerry.org

An important input to FEA is material characterization and limit information.  In our laboratory we use  a Bose 3230 test system for achieving test speeds up to 200Hz.   Depending on the project, we may test complete devices, sub-components, coupon samples and/or simple material characterization samples.  Many times, we will test more than one configuration to make sure our data are consistent and ultimately demonstrates the validation of an implantable medical device’s safety and efficacy.

Many factors are involved in deciding what testing would be most efficient to support a product’s validation effort.  Characterization of material properties is typically the first step.  For medical implants that utilize advanced materials, fine geometric features and deliberate metallurgical processing, it is important to capture these in the specimen design.  Fabrication of appropriate samples takes the most effort compared to the relatively short test times and the simplicity of material characterization tests.

After material characterization, testing to validate the performance features of an implant are typically necessary.  These tests may also require the fabrication of appropriate samples but can additionally involve the reproduction of complex in vivo load states.  Besides verifying that the test setup reproduces the desired load state, performance testing is short term and individual samples can be tested in series to study the effect of loading magnitudes, variations in processing, load combinations, etc.  Many times, these studies to quantify the impact of such variables play an important role in a validation strategy and can be efficiently performed since only one or a few cycles of loading are required.

Beyond material characterization and performance testing, material limit properties are the next category of data necessary for input to FEA models.  When the required number of cycles is low, say 10 million or fewer, accelerated testing can be performed on individual samples tested in series or multiple samples tested simultaneously.  The advantage of testing individual samples was mentioned above while testing multiple samples simultaneously produces stronger statistics more quickly.

When the required number of cycles reaches 100 million or more, a balance between testing enough samples for the desired confidence level and testing the samples to run out at the high cycle limit must be reached.  A typical strategy might involve a combination of testing individual samples  to 10 million cycles and then selecting one or more loading conditions/levels for testing multiple samples simultaneously.  Such a scenario takes advantage of the relatively short testing time frame for a 10 million cycle test (on the order of 1-2 days, compared to 4-6 weeks for testing to 400 million cycles) and the statistical advantage of testing multiple samples.

In the photo above, a multiple sample fixture capable of testing 12 fatigue coupon samples in a controlled temperature chamber is shown.  Such a fixture must be fabricated and aligned very carefully to insure identical loading conditions are achieved for all of the samples.  Stroboscopic verification, randomized experimental design, fracture surface investigation and other experimental mechanics techniques also help to build confidence in a validation test methodology.

For medical devices, rarely does “one size fit all”.  The human body is extremely variable and patient populations, especially those with disease present a wide range of differences that the medical device design engineer must consider.

Identifying the worst case size for a product family is an important part of the validation process for implantable medical devices.  Understanding your product and especially the in vivo loading conditions are essential for engineering the structure and material specifications for each size over the intended product range.

Typically, there are numerous sources of nonlinearity associated with implantable medical device design.  The materials we use, the geometries and especially the physiology we treat all respond in ways that are difficult to describe in simple terms.  It is tempting to design a product by considering an idealized patient population and then simply “scale” that design to smaller and larger sizes.  But this approach can can result in a poorly optimized product family.  Furthermore, when one considers device/lumen ineraction and teh resulting compliance under physiological loads, identifying the worst case loading condition is not a straightforward activity.

The figure above illustrates how the alternating fatigue strain for a stent-like product can vary for deployment to different diameters.  It is based on an analytic model of lumen compliance and finite element analysis models of the two device sizes.  Clearly, the results indicate a highly nonlinear system that precludes the selection of a single worst case device size and implant condition based on the “four corners” approach.  Assuming that the largest device put into the smallest lumen will result in the most challenged loading condition is niave.

When it is possible, it is preferred to model ALL device sizes to determine the worst case size. It is also advantageous to develop and validate a simulated model of the intended physiology for the implant and use this model to verify the performance of each size in a design family.  Parameters such as radial force, anchoringg, dynamic compliance, vessel tortuosity and fatigue loading conditions can then all be evaluated for each device size and safety established for the complete instructions for use (IFU) for the product.

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.

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.<-->

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.