ANSYS Analysis of a Cardiac Stent

Figure 1: Contour plot of the martensitic volume fraction of an implanted stent

Introduction

Blood vessels are essential for transporting oxygen and nutrients to the cells in the body and for disposing of cellular waste. Unfortunately, over half of American adults can experience some form of cardiovascular disease. Cardiovascular disease may come in the form of blood vessel restriction, usually caused by the buildup of plaque in a blood vessel. These restrictions can be treated with the implantation of cardiovascular stents.

These stents come in two varieties, balloon expandable stents and self-expanding stents. Balloon-expanding stents are implanted using a balloon that plastically deforms the lattice to its final diameter inside the blood vessel. Self-expanding stents are at their final diameter at rest but are compressed for insertion. Due to the large deformations required, most self-expanding stent designs require super-elastic metal alloys, such as nitinol. The complex geometry and unique physical properties of nitinol present a unique challenge for FEA simulation. The following report details an FEA analysis of a self-expanding stent design performed in ANSYS.

Mechanical Properties of Nitinol

Nitinol is a nickel-titanium alloy that exhibits super-elastic properties due to its phase transition between its Austenite and martensite phases. When deformed, the austenitic material will stretch with a proportional stress/strain profile. At a transition stress, the austenite crystal structure (Body-Centered-Cubic) will begin to transform into the martinsite phase (Simple-Cubic). This will continue to elongate with a new lower modulus until it reaches a stress level where all the austinite has transformed into martensite. The material will then deform with a new modulus. Unloading the material shows similar behavior, however, the transition stresses will be lower, creating a hysteresis response.

As shown in Figure 2, the strain response is temperature-dependent. When cooled the austenite phase will transform into the martensite phase. This may lead to deformation occurring completely in the martensitic phase, or partial austinite transformation. If cooled sufficiently, nitinol will behave as an isometric metal.

Figure 2: Stress-Strain-Temperature diagram

Figure 3: ANSYS Constitutive Model for superelastic alloys

Super-elastic Constitutive model in ANSYS

ANSYS simplifies the behavior of superelastic alloys using a seven-parameter model in addition to the isometric model. The four transition stress levels have the syntax Sigma[start/finish][starting material][ending material]. Note that martensite is labeled as "S". For example, sigma SAS is the stress where the material starts to transition from austinite to martensite. Other values include epsilon (maximum residual strain), and Es (modulus of martensite phase). Alpha is the parameter measuring the difference between tension and compression responses. Figure 3 illustrates the constitutive model parameters.

Simulation Process Map

The analysis of the stent is performed following the process map illustrated in Figure 4. Module A is a static structural simulation modeling the response of a stent cut at a smaller diameter, then permanently expanded to the desired diameter. Module D creates the model of the blood vessel and plaque and validates the response of the model when loaded with typical blood pressure cycles. Module B creates a mesh of an outer sheath that can compress the stent model to the insertion diameter. Module C is the final Static Structural model that stimulates crimping the stent, releasing it into the blood vessel, and the application of normal blood pressures. For continuity, the solution of module A is passed to module C.

Figure 4: Simulation Process map

Figure 5: Equivalent Plastic Strain of stent following expansion

Module A: Expansion of the Stent

Nitinol self-expanding stents are manufactured by laser cutting the scaffold out of a nitinol tube. These tubes commonly come in standardized diameters and thicknesses, so it is sometimes more economical to cut a stent out of tube stock and then expand the stent to the final diameter. The stent is then heat treated to set the dimensions. Module A simulates the expansion of a stent from a smaller diameter to a final diameter.

It is assumed the deformation occurs in a pure martensite state, allowing the use of an isometric model with a bilinear isotropic hardening behavior. The design is verified if the stent remains below its ultimate strain value. The model simulates the expansion through contact with an internal body. Contact is defined as frictionless and asymmetric. The inner body is meshed with shell elements. The stent is a swept mesh with linear quadrilateral elements and a nonlinear mechanical physics preference. A quarter of the stent is modeled to take advantage of symmetry. Frictionless supports are created on cut faces and a displacement is created on one node to avoid sliding. The inner body has a nodal displacement in the radial direction, with all other directions fixed. Large deflection is enabled.

The results of the simulation are shown in Figure 5. The maximum strain is 0.083. This strain value can be compared with material property documents to verify the ultimate strain has not been exceeded. If the strain has been exceeded, the stent may need to be constructed from larger tube stock to reduce the required deformation.

Module D: Model of Blood Vessel and Plaque

Blood vessels develop with three distinct layers: the intima, media, and adventitia. These layers have distinct material properties but do not experience sliding between the layers. As such, the blood vessel is modeled as 3 separate bodies with shared topologies at their contacting faces (Shared topologies instructs ANSYS to mesh the bodies with shared nodes at their contacting faces). The material constitutive model is created by curve-fitting experimental data. The blood vessel layers are adequately approximated using a third-order Yeoh model. Plaque is added to the middle section of the blood vessel in a similar manner. Model validation is performed in multiple steps. First, an axial displacement is applied to the vessel to mimic in vivo conditions. Then alternating internal pressures are applied to the blood vessel matching typical systolic and diastolic pressures. The vessel is modeled in quarters with corresponding boundary conditions. Large deflections are enabled. The model is validated if the simulated displacements agree with real-world measurements. Note that a blood vessel can be modeled as a homogenous cylinder with reduced accuracy on internal stresses and strains.

The results of Module D are shown in Figure 6. The illustrated results show the equivalent strain in the blood vessel during systolic pressures.

Figure 6: Equivalent strain in blood vessel during systolic pressure

Module B: Introduction of an Outer Sheath

The addition of a mechanical model to the process map allows for the introduction of a new mesh into the model when a simulation is unneeded. A surface body is meshed with shell elements that will be used to compress the stent to its implantation diameter. This model is built on the geometry of the original expansion step so that it remains concentric with the stent.

Model C: Implantation and the Blood Vessel Mechanics

The simulation of the implantation of the stent and the behavior inside the vessel is performed in 6 steps:

Crimping of the stent
Pre-tensioning the blood vessel
Pressurizing the blood vessel to diastolic pressure
Retracting the sheath
Increasing blood pressure to systolic pressure
Reducing the blood pressure to diastolic pressure

All steps are performed on a quarter model, and contact between the stent and blood vessel is disabled during the first step. Contact is defined as frictionless. A penetration tolerance is defined to aid in convergence. The formulation is set as Augmented Lagrange.

The fourth step presents unique challenges for convergence as ANSYS is a static solver and the stent undergoes free deflection while the sheath is retracted. This can be addressed using stabilization methods that create a pseudo-dynamic simulation in ANSYS. A damping stabilization method is applied to step 4, which creates pseudo forces that resist movement. This allows for the model to converge.

The simulation needs to answer the following questions to validate the stent design:

Does the stent experience plastic deformation during implantation?
Are the contact pressures on the vessel tissue below the desired threshold to avoid damage?
Is the expansion force sufficient to dilate the constricted blood vessel?
Is the fatigue life of the stent sufficient? (Explored in a future portfolio report)

Figure 7: Animation of simulation steps

Figure 8: Deflection Plot during sheath retraction.

Figure 9: Maximum strain experienced by stent

Figure 10: Contact pressures on vessel walls

Analysis and Results

The final simulation is able to produce the values necessary for the validation of the stent. If in a product design setting, the results presented here would be compared to a design inputs document to ensure the design meets requirements. The purpose of this report is not to dictate what those inputs should be, as such, results will be shown without comment on their propriety in a stent.

The stent experiences maximum deformation during its crimping. The maximum equivalent strain is 8.7934e-002 mm/mm. A contour plot of this stage is shown in Figure 9. As expected, the maximum strain occurs on the inside radius of the scaffolding where large compressive strains would occur.

Contact pressures between the stent and the blood vessel walls are shown in Figure 10. The maximum pressure is relatively consistent never exceeding 1MPa and averaging around 0.8MPa. These pressures should be compared with research to ensure the stent does not cause damage to the blood vessel walls that can lead to restenosis.

The simulation estimates a radial force of 0.9833N in the quarter model. Multiplying this value by 4 gives an expanding force of approximately

4N.

The fatigue life of nitinol structures presents unique challenges explored here.

A final analysis I want to share is the ability of ANSYS to calculate the martensite fraction inside the nitinol structure. A contour plot of the martensite fraction is shown in Figure 1. The contour colors show a martensite volume fraction ranging from zero to one. This plot can show the regions of high transformation and the gradient between a fully austenite microstructure to a fully martensite structure. This contour plot is created using the nlepeq command, as ANSYS treats martensite transformation as plastic strain.

Page updated

Google Sites

Report abuse