PDF
Plastic Deformation During the Expansion of a Biomedical Stent
Introduction
Percutaneous transluminal angioplasty with stenting is a widely spread method for the treatment of atherosclerosis. During the procedure, a stent is deployed into the artery by using a balloon as an expander. Once the balloon-stent package is in place, the balloon is inflated to expand the stent. The balloon is then deflated and removed, but the stent remains expanded to act as a scaffold, keeping the blood vessel open.
Stent design is of significance for this procedure, since serious damage can be inflicted to the artery during the expansion procedure. One of the most common defect is the non-uniform deformation of the stent, where the ends expand more than the middle section, phenomenon which is also called dogboning. Foreshortening of the stent can also damage the artery, and it could make the positioning difficult.
The dogboning is defined according to
where rdistal and rcentral are the radii at the end and middle of the stent, respectively.
The foreshortening is defined as
here, L0 is the original length of the stent and Lload is the deformed length of the stent.
Other common parameters in stent design are the longitudinal and radial recoil. These parameters give information on the stent behavior when removing the inflated balloon.
The longitudinal recoil is defined as
here, Lunload is the length of the stent once the balloon is removed, and Lload is the length of the stent when the balloon is fully inflated.
The radial recoil can be defined as follow
here, Runload is the radius of the stent once the balloon is removed, and Rload is the radius of the stent when the balloon is fully inflated.
To check the viability of a stent design, you can study the deformation process under the influence of the radial pressure that expands the stent. With this example you can both monitor the dogboning and foreshortening effects, and draw conclusions on how to change the geometry design parameters for optimum performance.
Model Definition
The model studies the Palmaz-Schatz stent model. Due to the stent’s circumferential and longitudinal symmetry, it is possible to model only one twenty-forth of the geometry. Figure 1 shows the geometry used in the study, represented with the meshed domain.
Figure 1: The reduced geometry used in the study (meshed) and the full stent geometry.
The main focus of the study consists in the stress evaluation in the stent. The angioplasty balloon is assumed to stretch with a maximum expansion radius of 2 mm.
Material
The stent is made of stainless steel. The material parameters are given in the following table.
Material Property
Value
Young’s modulus
193[GPa]
Poisson’s ratio
0.27
Initial yield stress
207[MPa]
Isotropic tangent modulus
692[MPa]
Loads
Apply a radial outward pressure on the inner surface of the stent to represent the balloon expansion.
Results and Discussion
The stent is expanded from an original diameter of 0.74 mm to a diameter of 2 mm in the middle section. Figure 2 shows the stress distribution at maximum balloon inflation, and Figure 3 shows the residual stress after the balloon deflation. The residual stress follows form the plastic deformation as shown in Figure 4.
Figure 2: Maximum stress in the stent during the balloon inflation.
Figure 3: Residual stress in the stent after deflation of the balloon.
Figure 4: Equivalent plastic strain in the stent after deflation of the balloon.
In Figure 5, you can see the evolution of the dogboning and foreshortening effects with respect to the pressure during the inflation of the balloon. The longitudinal recoil is about −0.9%, the distal radial recoil is about 0.4%, and the central radial recoil is about 0.7%.
Figure 5: Stent dogboning (blue) and foreshortening (green) versus pressure inside the angioplasty balloon.
Notes About the COMSOL Implementation
The maximum radius of the angioplasty balloon is represented with a step function, the pressure is applied as long as the inner radius of the stent is smaller than the maximum balloon radius. Above this limit the pressure is set to zero.
For a highly nonlinear problem like this, the choice of the continuation parameter can improve the convergence during the computation of the solution. A displacement control parameter is usually better than a load parameter. In this example, the average displacement of the stent’s inner radius is prescribed, and a Global Equation is used to compute the corresponding applied pressure load.
Application Library path: Nonlinear_Structural_Materials_Module/Plasticity/biomedical_stent
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics>Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
Geometry 1
Import 1 (imp1)
1
In the Home toolbar, click  Import.
2
In the Settings window for Import, locate the Import section.
3
From the Source list, choose COMSOL Multiphysics file.
4
Click  Browse.
5
Browse to the model’s Application Libraries folder and double-click the file biomedical_stent.mphbin.
6
Click  Import.
7
Click the  Zoom Extents button in the Graphics toolbar.
Solid Mechanics (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics (solid) click Linear Elastic Material 1.
Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Plasticity.
2
In the Settings window for Plasticity, locate the Plasticity Model section.
3
From the Formulation list, choose Large strains.
Materials
Material 1 (mat1)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
193[GPa]
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.27
1
Young’s modulus and Poisson’s ratio
Density
rho
7050
kg/m³
Basic
Initial yield stress
sigmags
207[MPa]
Pa
Elastoplastic material model
Isotropic tangent modulus
Et
692[MPa]
Pa
Elastoplastic material model
Choose the steel material type to improve the visualization of the stent during postprocessing.
4
Click to expand the Appearance section. From the Material type list, choose Steel.
Definitions
Step 1 (step1)
1
In the Home toolbar, click  Functions and choose Local>Step.
2
In the Settings window for Step, locate the Parameters section.
3
In the Location text field, type 2[mm].
4
In the From text field, type 1.
5
In the To text field, type 0.
6
Click to expand the Smoothing section. In the Size of transition zone text field, type 1e-5.
Variables 1
1
In the Home toolbar, click  Variables and choose Local Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
r
sqrt(y^2+z^2)
m
Radial distance from x-axis
Average 1 (aveop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, locate the Source Selection section.
3
From the Geometric entity level list, choose Edge.
4
Select Edge 28 only.
5
Locate the Advanced section. From the Frame list, choose Material  (X, Y, Z).
Piecewise 1 (pw1)
1
In the Definitions toolbar, click  Piecewise.
2
In the Settings window for Piecewise, type r0 in the Function name text field.
3
Locate the Definition section. In the Argument text field, type t.
4
Find the Intervals subsection. In the table, enter the following settings:
Start
End
Function
0
1
(2e-3-7.1e-4)*t+7.1e-4
1
2
(2e-3-7.1e-4)*(1-t)+2e-3
5
Locate the Units section. In the Arguments text field, type s.
6
In the Function text field, type m.
7
Click  Plot.
Solid Mechanics (solid)
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundaries 5, 12, 18, 24, 30, and 31 only.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 4 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Pressure.
5
In the p text field, type p*step1(r).
6
Click the  Show More Options button in the Model Builder toolbar.
7
In the Show More Options dialog box, in the tree, select the check box for the node Physics>Equation-Based Contributions.
8
Click OK.
Global Equations 1
1
In the Physics toolbar, click  Global and choose Global Equations.
2
In the Settings window for Global Equations, locate the Global Equations section.
3
In the table, enter the following settings:
Name
f(u,ut,utt,t) (1)
Initial value (u_0) (1)
Initial value (u_t0) (1/s)
Description
p
aveop1(r)-r0(t)
0
0
Pressure
4
Locate the Units section. Click  Select Dependent Variable Quantity.
5
In the Physical Quantity dialog box, type pressure in the text field.
6
Click  Filter.
7
In the tree, select General>Pressure (Pa).
8
Click OK.
9
In the Settings window for Global Equations, locate the Units section.
10
Click  Select Source Term Quantity.
11
In the Physical Quantity dialog box, type length in the text field.
12
Click  Filter.
13
In the tree, select General>Length (m).
14
Click OK.
Mesh 1
Free Triangular 1
1
In the Mesh toolbar, click  Boundary and choose Free Triangular.
2
Select Boundary 3 only.
Size 1
1
Right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
Click the Custom button.
4
Locate the Element Size Parameters section.
5
Select the Maximum element size check box. In the associated text field, type 4.5e-5.
6
Select the Minimum element size check box. In the associated text field, type 4e-6.
7
Select the Maximum element growth rate check box. In the associated text field, type 1.4.
8
Select the Curvature factor check box. In the associated text field, type 0.3.
Swept 1
In the Mesh toolbar, click  Swept.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 2.
4
Click  Build All.
Definitions
Create variables for the results processing.
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Point.
4
Select Point 57 only.
5
In the Operator name text field, type central.
6
Locate the Advanced section. From the Frame list, choose Material  (X, Y, Z).
Integration 2 (intop2)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Point.
4
Select Point 3 only.
5
In the Operator name text field, type distal.
6
Locate the Advanced section. From the Frame list, choose Material  (X, Y, Z).
Variables 1
1
In the Model Builder window, click Variables 1.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
dogboning
(distal(r)-central(r))/distal(r)
 
Dogboning
length
2*abs(distal(x)-central(x))
m
Length of the deformed stent
L0
2*abs(distal(X)-central(X))
m
Length of the undeformed stent
foreshortening
(length-L0)/length
 
Foreshortening
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
t
0[s]
0 s
Time
Study 1
Step 1: Stationary
Set up an auxiliary continuation sweep for the t parameter.
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Study Extensions section.
3
Select the Auxiliary sweep check box.
4
Click  Add.
5
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
t (Time)
range(0,1e-2,1.5)
s
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1>Solver Configurations>Solution 1 (sol1)>Dependent Variables 1 node, then click Pressure (comp1.ODE1).
4
In the Settings window for State, locate the Scaling section.
5
From the Method list, choose Manual.
6
In the Scale text field, type 1e6.
Add a stop condition to prevent the computed pressure from becoming negative.
7
In the Model Builder window, expand the Study 1>Solver Configurations>Solution 1 (sol1)>Stationary Solver 1 node.
8
Right-click Study 1>Solver Configurations>Solution 1 (sol1)>Stationary Solver 1>Parametric 1 and choose Stop Condition.
9
In the Settings window for Stop Condition, locate the Stop Expressions section.
10
Click  Add.
11
In the table, enter the following settings:
Stop expression
Stop if
Active
Description
comp1.p<0
True (>=1)
√
Stop expression 1
Specify that the solution is to be stored just before the stop condition is reached.
12
Locate the Output at Stop section. From the Add solution list, choose Step before stop.
13
In the Study toolbar, click  Compute.
14
In the Home toolbar, click  Add Predefined Plot.
Add Predefined Plot
1
Go to the Add Predefined Plot window.
2
In the tree, select Study 1/Solution 1 (sol1)>Solid Mechanics>Equivalent Plastic Strain (solid).
3
Click Add Plot in the window toolbar.
4
In the Home toolbar, click  Add Predefined Plot.
Results
Stress (solid)
Use mirror 3D and sector 3D datasets to display the solution on the full geometry.
Mirror 3D 1
1
In the Model Builder window, expand the Results>Datasets node.
2
Right-click Results>Datasets and choose More 3D Datasets>Mirror 3D.
Mirror 3D 2
1
In the Results toolbar, click  More Datasets and choose Mirror 3D.
2
In the Settings window for Mirror 3D, locate the Data section.
3
From the Dataset list, choose Mirror 3D 1.
4
Locate the Plane Data section. From the Plane list, choose zx-planes.
Sector 3D 1
1
In the Results toolbar, click  More Datasets and choose Sector 3D.
2
In the Settings window for Sector 3D, locate the Data section.
3
From the Dataset list, choose Mirror 3D 2.
4
Locate the Axis Data section. In row Point 2, set x to 1 and z to 0.
5
Locate the Symmetry section. In the Number of sectors text field, type 6.
Stress (solid)
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Sector 3D 1.
4
Locate the Plot Settings section. Clear the Plot dataset edges check box.
Volume 1
1
In the Model Builder window, expand the Stress (solid) node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
Use a Surface Plot with a Material Appearance subnode to visualize the stent in its original state.
Surface 1
1
In the Model Builder window, right-click Stress (solid) and choose Surface.
2
In the Settings window for Surface, click to expand the Title section.
3
From the Title type list, choose None.
Material Appearance 1
1
Right-click Surface 1 and choose Material Appearance.
2
In the Stress (solid) toolbar, click  Plot.
Stress (solid)
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, click  Plot Previous twice to plot the maximum stress.
3
In the Stress (solid) toolbar, click  Plot.
Equivalent Plastic Strain (solid)
1
In the Model Builder window, click Equivalent Plastic Strain (solid).
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Sector 3D 1.
4
Locate the Plot Settings section. Clear the Plot dataset edges check box.
Surface 2
1
In the Model Builder window, expand the Equivalent Plastic Strain (solid) node.
2
Right-click Results>Equivalent Plastic Strain (solid)>Surface 1 and choose Duplicate.
Deformation 1
1
Right-click Surface 1 and choose Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor check box. In the associated text field, type 1.
Surface 2
1
In the Model Builder window, under Results>Equivalent Plastic Strain (solid) click Surface 2.
2
In the Settings window for Surface, locate the Title section.
3
From the Title type list, choose None.
Material Appearance 1
1
Right-click Surface 2 and choose Material Appearance.
2
In the Equivalent Plastic Strain (solid) toolbar, click  Plot.
Dogboning and Foreshortening
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Dogboning and Foreshortening in the Label text field.
3
Locate the Data section. From the Time selection list, choose From list.
4
In the parameter values list, select all solution steps between 0 and 1.
Global 1
1
Right-click Dogboning and Foreshortening and choose Global.
2
In the Settings window for Global, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>dogboning - Dogboning.
3
Click Add Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>foreshortening - Foreshortening.
4
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Solid Mechanics>p - Pressure - Pa.
5
In the Dogboning and Foreshortening toolbar, click  Plot.
Evaluate the longitudinal recoil, the distal radial recoil, and the central radial recoil using the Evaluation Group.
Click on the check box in the Results node to enable automatic reevaluation of evaluation groups when the model is resolved.
6
In the Model Builder window, click Results.
7
In the Settings window for Results, locate the Update of Results section.
8
Select the Reevaluate all evaluation groups after solving check box.
Recoil Evaluation
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Recoil Evaluation in the Label text field.
3
Locate the Data section. From the Time selection list, choose From list.
4
In the Parameter values (t (s)) list, select 1.
Global Evaluation 1
1
Right-click Recoil Evaluation and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
(length-with(103,length))/length
1
Longitudinal recoil
(distal(r)-with(103,distal(r)))/distal(r)
1
Distal radial recoil
(central(r)-with(103,central(r)))/central(r)
1
Central radial recoil
4
In the Recoil Evaluation toolbar, click  Evaluate.
The steps below illustrate how to display the geometry as in Figure 1.
Full Geometry and Mesh
1
In the Home toolbar, click  Add Plot Group and choose 3D Plot Group.
2
In the Settings window for 3D Plot Group, type Full Geometry and Mesh in the Label text field.
3
Click to expand the Title section. From the Title type list, choose None.
Surface 1
1
Right-click Full Geometry and Mesh and choose Surface.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Sector 3D 1.
Material Appearance 1
Right-click Surface 1 and choose Material Appearance.
Mesh 1
1
In the Model Builder window, right-click Full Geometry and Mesh and choose Mesh.
2
In the Settings window for Mesh, locate the Coloring and Style section.
3
From the Element color list, choose None.
4
In the Full Geometry and Mesh toolbar, click  Plot.