Auricchio, Ferdinando

Conti, Michele

De Beule, Matthieu

Mortier, Peter

Segers, Patrick

Verdonck, Pascal

Verhegghe, Benedict

Ghent University Academic Bibliography

Second African Conference on Computational Mechanics – An International Conference – AfriCOMP11 January 5 – 8, 2011, Cape Town A.G. Malan, P. Nithiarasu and B.D. Reddy (eds)   FINITE ELEMENT ANALYSIS OF SELF EXPANDING BRAIDED WIRE STENTS  M. De Beule*, M. Conti*,**, P. Mortier*, P. Verdonck*, P. Segers*, F. Auricchio** and B. Verhegghe* *IBiTech-bioMMeda, Ghent University, De Pintelaan 185, 9000 Gent, Belgium, Matthieu.DeBeule@UGent.be ** Department of Structural Mechanics, University of Pavia, Pavia, Italy Key Words: braided wire stent, finite element analysis, mechanical behavior, pyFormex  1. INTRODUCTION  A stent is an expandable tube-like device that is inserted into a natural conduit of the body to restore a disease-induced localized stenosis or aneurysm, allowing minimally invasive interventions.  Several stent designs, both balloon and self-expandable, are available in the fast growing market, covering a wide range of clinical applications, ranging from coronary arteries to gastrointestinal strictures.  Particularly, braided wire stents are a class of self-expandable stents consisting from a set of interwoven ultra fine wires and currently manufactured in a wide range of braiding patterns (single or multilayer) and materials (e.g. metallic materials, such as Phynox and Nitinol, or polymers) and bare wire stents can also be coupled with polymeric covers in order to create covered stents or stent grafts suited for aneurysm treatment.  Despite the positive clinical outcomes of braided wire stents, some drawbacks (e.g. restenosis, stent migration, artery straightening, side branch covering, …) still need further attention and additional investigation.  At present, in addition to a variety of analytical models, experimental in vitro tests and in vivo observations, advanced computational models offer interesting insights in the mechanical behavior of stents [1]. However, literature dedicated to the simulation of the mechanical behavior of braided wire stents is very scarce and often simplifying the analysis assuming the wire stent as virtual single sheets neglecting the actual wire stent composition.   2. MATERIALS AND METHODS  In this study, pyFormex (version 6.3) [2] was used as a pre-processor to build a geometrical and finite element model of a braided Wallstent®. This in-house developed, open source, software provides a Python based scripting language to build a geometrical model by means of subsequent mathematical transformations. This strategy is suitable to generate parametric models and specifically to generate the geometry of the braided wire stent, allowing the model to reproduce the criss-cross pattern of the stent design. Moreover the mesh generation procedure includes a connection element when two wires cross each other in the criss-cross pattern. This connection element has the function to maintain constant the distance lconn between the centerlines of two wires at the crossing point, consequently this distance is automatically set to the value wire diameter d. Consequently the contact between the crossing wires is virtually established by connecting the crossing nodes with a specific JOIN connector (fixing these node positions relative to each other, though allowing their relative rotations). The finite element model of the stent is defined by 20160 2 node linear beam elements (b31). A sensitivity test, performed to control the influence of the element number on the stress computation, has showed a very limited difference (1.5%) between the chosen mesh (20196 nodes-20160 elements) and a finer one (40356 modes-40320 elements). The considered stent model is combined with three currently used stent materials: stainless steel (316L SS), high strength Phynox and shape memory Nitinol. Nitinol superelasticity is modeled as a predefined user material in the proprietary finite element solver package ABAQUS/STANDARD 6.6 (Abaqus Inc., Providence, RI, USA), whereas Phynox and stainless steel are modeled as classic elasto-plastic materials The objective of this study was to develop a virtual benchmark test to assess the equivalent stress state of the stent wires when the diameter of the braided stent is reduced, simulating the insertion of the stent into the catheter. For this purpose, the process of insertion of the stent into the catheter is assumed similar to the effect of stent axial loading. Accordingly to this hypothesis, one end of the stent is constrained in both the tangential and axial direction while in the other an increasing concentrated force F, ranging from 0 to 0.6 N as the time simulation increases, is applied on each wire. The applied forces result in an axial elongation of the stent. Consequently, this test permits to compute the equivalent von Mises stress state in the stent wires and compare it with the mechanical properties assumed for the different stent materials. Following the hypothesis of Wang and Ravi-Chandar [3], no initial residual stresses imparted by winding/braiding of the stent wires are taken into account in the model. For validation purposes, the numerical results are compared with the experimentally confirmed analytical model described by Jedwab and Clerc [4]. Under the action a force Flong acting on the longitudinal axis of the stent, wire stent diameter experiences longitudinal elongation (d) and a consequent diameter reduction (from D0 to D) and pitch angle change (from b0 to b) as shown in fig. 1. Using spring mechanics theory it is possible to relate the force F with both the stent material properties and its specific geometry.  Figure 1: Braided wire stent elongation under the action of an axial force Flong  3. RESULTS AND DISCUSSION  The equivalent stress σe in the stent wires is computed using the analytical model as well as through the finite element computations for the Phynox, stainless steel and Nitinol stent. Over the whole range of loading, the simulation corresponds well with the analytical model for both the Phynox and Nitinol stent and offering an approximation of the equivalent stress state (Figure 2). However, reducing the diameter of the stainless steel stent to a value less than 14 mm induces plastic deformations, logically not captured by the elastic analytical approximation. In the investigation of the equivalent stresses it is important to notice, when using Phynox, the equivalent stress does not exceed the maximum stress allowed by the von Mises criterion. Consequently, it seems possible to reduce the actually used catheter size (i.e. 10 Fr) for the considered stent design and high strength material without plastic deformations of the stent. On the other hand, it should be noted that the nitinol superelastic properties are not exploited for the considered stent design and material properties as the transformation stress (i.e. 489 N/mm²) is not reached during the stent diameter reduction.   Figure 2: Comparison of analytically calculated and FEM based equivalent von Mises stress (distribution) in Phynox, stainless steel and Nitinol stent wire.  Moreover the implementation of the connectors allow to compute the reaction force acting in crossing point of wires. In fig. 3 the reaction force in the connector elements lying on the same longitudinal direction with respect to their position along the stent length. The assumption of the independent coiled springs bases analytical model, consequently assuming that the reaction force between the crossing wires is neglectable. Computing the reaction in the connector element in the proposed model, it is possible to notice that such assumption is acceptable for the wires lying on transversal section (40.5 mm) and with small connector length (d=0.001)  as shown in fig. 3. Consequently the numerical model would be useful for further investigation about friction mechanisms within the stent wires.   4. CONCLUSIONS  Accurate geometrical models can quickly be built using the pyFormex modeling tool, consequently allowing finite element simulations for studying the mechanical behavior of the stent under different mechanical loading and boundary conditions.    Figure 3: Reaction force of the connectors: comparison between different connector length. In this study, an analytically confirmed virtual test is described to evaluate the stress state of the stent wires when the stent diameter of the braided Wallstent® is reduced to several catheter sizes. It seems possible to reduce the actually used catheter size for the considered stent design and Phynox material without plastically deforming the stent. Such a catheter size reduction would increase in-situ lesion access, but could decrease the ease of the actual stent delivery (i.e. higher force necessary to release the stent out of the catheter). Furthermore, the use of high strength steels (i.e. characterized by high yield stress values) seems required to avoid undesirable plastic deformation of the braided stent. Braiding the stent for example from 316L stainless steel wires (characterized by a yield stress in the range of 205 to 375 N/mm² and a modulus of Young comparable to the one of Phynox) definitely induces such plastic deformations. Subsequently, an experimentally validated methodology to analyze the free expanding stent exiting the catheter is developed and shows that the material properties (from Phynox and Nitinol) have limited influence on the stent expansion behavior. While the expansion behavior of the stainless steel stent is compromised by plastic deformations. It may be concluded that the finite element model developed seems a promising tool for stent developers during the design phase to investigate the geometrical and mechanical properties of self-expanding braided wire stents implementing arbitrary geometry and stent material. The developed pyFormex modeling strategy is a solid base for further study of the mechanical behavior of braided wire stents in real life conditions (e.g. patient-specific stent vessel interaction) and might be useful in the quest for the optimal stent.   REFERENCES  [1] De Beule, M., “Finite Element Stent Design”, Ph.D. thesis, Ghent University, Belgium [2] Internet site address: http://pyFormex.berlios.de  [3] Wang, R., Ravi-Chandar, K., 2004, “Mechanical Response of a Metallic Aortic Stent - Part I. Pressure-Diameter Relationship”, ASME J. Appl. Mech., 71, pp. 697–705.  [4] Jedwab, M., and Clerc, C., 1993, “A Study of the Geometrical and Mechanical Properties of a Self-Expanding Metallic Stent - Theory and Experiment”, J. of Appl. Biom., 4, pp. 77-85. 

Finite element analysis of self expanding braided wire stents

https://biblio.ugent.be/publication/1152425/file/1152428

Finite element analysis of self expanding braided wire stents

Abstract

Similar works

Full text

Available Versions

Ghent University Academic Bibliography