PDF
Inflation of a Spherical Rubber Balloon
Introduction
This example aims to investigate the inflation of a rubber balloon using different hyperelastic material models, and to compare the results to analytical expressions.
A controlled inflation could be of importance in clinical applications, cardiovascular research, and medical device industry (Ref. 2), among others. This example demonstrates such controlled inflation of balloon based on radial stretch.
The example is taken from the book Nonlinear Solid Mechanics by G. Holzapfel (Ref. 1).
Model Definition
This example compares the hoop stress and inflation pressure as a function of the stretch for a spherical rubber balloon.
Figure 1: Model geometry. The initial inner radius is set to 10 cm, and the initial thickness to 1 mm.
In this example, the following four hyperelastic material models are compared: neo-Hookean, Money-Rivlin, Ogden, and Varga.
Due to the spherical symmetry, an arbitrary sector in the azimuthal direction can be used. Here, a 20 degrees sector is modeled in a 2D axial symmetry plane.
Figure 2: 2D axisymmetric geometry and mesh.
Results and Discussion
The results are compared to the analytical expression for a thin-walled vessel. The inflation pressure is a function of the hoop stress σθ, current inner radius r and current thickness h
For spherical balloons, the hoop stress σθ is equal to the largest principal stresses σ1 and σ2. Two of the principal stretches are in the plane tangential to the sphere and are equal, λ = λ1 = λ2 = r/R, which is typical for equibiaxial deformation. Here, r and R are the current and initial inner radii, respectively.
Due to the nearly incompressibility assumption, the third principal stretch (this is the stretch in the radial direction) is equal to λ3 = 1/λ2 = h/H, where h and H are the current and initial balloon thicknesses, respectively.
The analytical expression for the hoop stress for the Ogden material model becomes (Ref. 1)
where αp and μp are Ogden parameters, and λ is the largest principal stretch.
Because r = Rλ and h = H/λ2, the analytical expression for the inflation pressure is calculated as a function of Ogden parameters, stretch, initial thickness and initial inner radius
The results are in excellent agreement with experimental results and the figures portrayed in Ref. 1.
The experiments show a rapid rise in the internal pressure until reaching a maximum value, followed by a pressure decrease until reaching a minimum, and then increasing again. The local maximum and local minimum for pressure are called as limit points, where the sign of stiffness changes. Some material models, like Mooney-Rivlin and Ogden, can show more than one limit point. A snap-through phenomenon is observed for Ogden and Mooney-Rivlin material models. The neo-Hookean and Varga material models can only reproduce balloon inflations at small strain levels.
The computed inflation pressure and hoop stress as functions of the applied stretch are shown in Figure 3 and Figure 4, respectively. Both figures include the computed results for all different material models, and are in a excellent agreement with the results described in Ref. 1, page 241.
Figure 5 shows the distribution of the von Mises stress for a neo-Hookean material at the final step of the solution..
Figure 3: Computed inflation pressure as a function of circumferential stretch for different material models, compared to the analytical expression for the Ogden material model.
Figure 4: Computed hoop stress as a function of circumferential stretch for different material models, compared to the analytical expression for the Ogden material.
Figure 5: Distribution of von Mises stress on the modeled 2D cross section for the neo-Hookean material at maximum inflation.
Notes About the COMSOL Implementation
Different hyperelastic material models are constructed by specifying different elastic strain energy density expressions. The Nonlinear Structural Materials Module provides several predefined material models together with an option to enter user defined expressions for the strain energy density.
The predefined nearly incompressible version of the neo-Hookean material with quadratic volumetric strain energy formulation uses the isochoric invariant and the initial bulk modulus κ
In this example, μ = 422.5 kPa and κ = 105μ. The Lamé parameter μ can be seen as representing the shear modulus at small strains.
The predefined nearly incompressible Mooney-Rivlin material with quadratic volumetric strain energy formulation has an elastic strain energy density written in terms of the two isochoric invariant of the elastic right Cauchy-Green deformation tensors and , and the elastic volume ratio Jel
The material parameters C10 and C01 are related to the shear modulus μ = 2(C10+C01). In this example, they are set as C10 = 7/16μ and C01 = μ/16, so that the relation C10 = 7C01 is fulfilled.
The predefined nearly incompressible Ogden material with quadratic volumetric strain energy formulation is implemented with the isochoric elastic stretches and the initial bulk modulus κ
with N = 3, and the Ogden parameters as written in Table 1.
Table 1: Ogden parameters.
 p
 αp
 μp (kPa)
1
1.3
630
2
5.0
1.2
3
-2.0
-10
The Varga material model is implemented with a user defined strain energy density
When the relation between the applied load and the displacement is not unique, a suitable modeling technique is to use an algebraic equation that controls the applied pressure, so that the model reaches the desired displacement increments. In this example, a Global Equation uses the radial displacement at point 3 to add an extra degree of freedom for the inflation pressure.
Global equations are a way of adding an additional equation to a model. A global equation can be used to describe a load, constraint, material property, or anything else in the model that has a uniquely definable solution. In this example, the model is augmented by a global equation which solves for the inflation pressure to achieve a desired applied stretch.
References
1. G.A. Holzapfel, Nonlinear Solid Mechanics: A Continuum Approach for Engineering, John Wiley & Sons, 2000.
2. H. Azarnoush, S. Vergnole, B. Boulet, R. DiRaddo, and G. Lamouche, “Real-time control of angioplasty balloon inflation based on feedback from intravascular optical coherence tomography: preliminary study on an artery phantom,” IEEE Trans Biomed Eng. vol. 59, pp. 697–705, 2012.
Application Library path: Nonlinear_Structural_Materials_Module/Hyperelasticity/balloon_inflation
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  2D Axisymmetric.
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.
Global Definitions
Begin by defining model parameters.
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
Ri
10[cm]
0.1 m
Inner radius
H
1[mm]
0.001 m
Thickness
mu
4.225e5[Pa]
4.225E5 Pa
Shear modulus
kappa
1e5*mu
4.225E10 Pa
Bulk modulus
stretch
1
1
Applied stretch
Setting the bulk modulus to 10^5 times the shear modulus is based on the assumption that the material is incompressible.
Definitions
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
u_appl
(stretch-1)*Ri
m
Applied displacement
Use the applied stretch and the inner radius of the balloon to compute the applied displacement.
Geometry 1
Due to symmetry, it suffices to model a 20-degree sector of the balloon.
Circle 1 (c1)
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type Ri+H.
4
In the Sector angle text field, type 20.
5
Click to expand the Layers section. In the table, enter the following settings:
Layer name
Thickness (m)
Layer 1
H
6
Click  Build All Objects.
Delete Entities 1 (del1)
1
In the Model Builder window, right-click Geometry 1 and choose Delete Entities.
2
In the Settings window for Delete Entities, locate the Entities or Objects to Delete section.
3
From the Geometric entity level list, choose Domain.
4
On the object c1, select Domain 1 only.
5
Click  Build All Objects.
Solid Mechanics (solid)
Add the four hyperelastic material models to be studied.
Neo-Hookean
1
In the Model Builder window, under Component 1 (comp1) right-click Solid Mechanics (solid) and choose Material Models>Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, type Neo-Hookean in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose All domains.
4
Locate the Hyperelastic Material section. From the Compressibility list, choose Nearly incompressible material, quadratic volumetric strain energy.
5
In the κ text field, type kappa.
6
From the μ list, choose User defined. In the associated text field, type mu.
Mooney-Rivlin
1
In the Physics toolbar, click  Domains and choose Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, type Mooney-Rivlin in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose All domains.
4
Locate the Hyperelastic Material section. From the Material model list, choose Mooney-Rivlin, two parameters.
5
From the C10 list, choose User defined. In the associated text field, type 0.4375*mu.
6
From the C01 list, choose User defined. In the associated text field, type 0.0625*mu.
7
In the κ text field, type kappa.
Ogden
1
In the Physics toolbar, click  Domains and choose Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, type Ogden in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose All domains.
4
Locate the Hyperelastic Material section. From the Material model list, choose Ogden.
5
Click Add twice.
6
In the Ogden parameters table, enter the following settings:
p
Shear modulus (Pa)
Alpha parameter (1)
1
6.3e5
1.3
2
0.012e5
5
3
-0.1e5
-2
7
In the κ text field, type kappa.
Varga
1
In the Physics toolbar, click  Domains and choose Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, type Varga in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose All domains.
4
Locate the Hyperelastic Material section. From the Material model list, choose User defined.
5
From the Compressibility list, choose Nearly incompressible material.
6
In the Wsiso text field, type 2*mu*(solid.stchelp1+solid.stchelp2+solid.stchelp3-3).
7
In the Wsvol text field, type 0.5*kappa*(solid.Jel-1)^2.
To enforce a symmetry constraint, add a Roller node.
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 1 and 2 only.
Control the inflation of the balloon by the pressure.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 3 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_f.
You will define the pressure p_f using a Global Equation feature shortly. First, define a nonlocal integration coupling to evaluate the displacement at point 3.
Definitions
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 3 only.
5
Locate the Advanced section. From the Frame list, choose Material  (R, PHI, Z).
6
Clear the Compute integral in revolved geometry check box.
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
ub
intop1(u)
m
Radial displacement, inner boundary
Solid Mechanics (solid)
1
Click the  Show More Options button in the Model Builder toolbar.
2
In the Show More Options dialog box, in the tree, select the check box for the node Physics>Equation-Based Contributions.
3
Click OK enable global equations and other advanced modeling features to the Solid Mechanics interface.
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_f
ub-u_appl
0
0
 
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 displacement in the text field.
12
Click  Filter.
13
In the tree, select General>Displacement (m).
14
Click OK.
Mesh 1
Mapped 1
In the Mesh toolbar, click  Mapped.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundary 2 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 3.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
Select Boundary 3 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 50.
5
In the Model Builder window, right-click Mesh 1 and choose Build All.
Study 1
The first study solves the problem with a neo-Hookean material model.
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step check box.
4
In the tree, select Component 1 (Comp1)>Solid Mechanics (Solid)>Mooney-Rivlin, Component 1 (Comp1)>Solid Mechanics (Solid)>Ogden, and Component 1 (Comp1)>Solid Mechanics (Solid)>Varga.
5
Right-click and choose Disable.
Use an Auxiliary sweep to ramp up the applied stretch from 1.1 to 10.
1
Click to expand the Study Extensions section. Select the Auxiliary sweep check box.
2
Click  Add.
3
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
stretch (Applied stretch)
range(1, 0.1, 2) range(2.2, 0.2, 10)
 
4
In the Model Builder window, click Study 1.
5
In the Settings window for Study, type Neo-Hookean in the Label text field.
Modify the default solver to improve convergence.
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
Use manual scaling to help the nonlinear solver at the first steps. A constant predictor is also suitable for nonlinear materials.
2
In the Model Builder window, expand the Solution 1 (sol1) node, then click Dependent Variables 1.
3
In the Settings window for Dependent Variables, locate the Scaling section.
4
From the Method list, choose Manual.
5
In the Model Builder window, expand the Neo-Hookean>Solver Configurations>Solution 1 (sol1)>Stationary Solver 1 node, then click Direct.
6
In the Settings window for Direct, locate the General section.
7
From the Solver list, choose PARDISO.
8
In the Model Builder window, under Neo-Hookean>Solver Configurations>Solution 1 (sol1)>Stationary Solver 1 click Parametric 1.
9
In the Settings window for Parametric, click to expand the Continuation section.
10
From the Predictor list, choose Constant.
11
In the Model Builder window, under Neo-Hookean>Solver Configurations>Solution 1 (sol1)>Stationary Solver 1 click Fully Coupled 1.
12
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
13
From the Nonlinear method list, choose Constant (Newton).
14
In the Study toolbar, click  Compute.
Add a second study to solve for the Mooney-Rivlin material model, then repeat the steps described above.
Add Study
1
In the Study toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies>Stationary.
4
Click Add Study in the window toolbar.
Mooney-Rivlin
1
In the Model Builder window, click Study 2.
2
In the Settings window for Study, type Mooney-Rivlin in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots check box.
Step 1: Stationary
1
In the Model Builder window, under Mooney-Rivlin click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step check box.
4
In the tree, select Component 1 (Comp1)>Solid Mechanics (Solid)>Neo-Hookean, Component 1 (Comp1)>Solid Mechanics (Solid)>Ogden, and Component 1 (Comp1)>Solid Mechanics (Solid)>Varga.
5
Right-click and choose Disable.
Use an Auxiliary sweep to ramp up the applied stretch from 1.1 to 5.
1
Locate the Study Extensions section. Select the Auxiliary sweep check box.
2
Click  Add.
3
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
stretch (Applied stretch)
range(1, 0.1, 5)
 
Solution 2 (sol2)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 2 (sol2) node, then click Dependent Variables 1.
3
In the Settings window for Dependent Variables, locate the Scaling section.
4
From the Method list, choose Manual.
5
In the Model Builder window, expand the Mooney-Rivlin>Solver Configurations>Solution 2 (sol2)>Stationary Solver 1 node, then click Direct.
6
In the Settings window for Direct, locate the General section.
7
From the Solver list, choose PARDISO.
8
In the Model Builder window, under Mooney-Rivlin>Solver Configurations>Solution 2 (sol2)>Stationary Solver 1 click Parametric 1.
9
In the Settings window for Parametric, locate the Continuation section.
10
From the Predictor list, choose Constant.
11
In the Model Builder window, under Mooney-Rivlin>Solver Configurations>Solution 2 (sol2)>Stationary Solver 1 click Fully Coupled 1.
12
In the Settings window for Fully Coupled, locate the Method and Termination section.
13
From the Nonlinear method list, choose Constant (Newton).
14
In the Study toolbar, click  Compute.
Continue with a third study for the Ogden material model.
Add Study
1
Go to the Add Study window.
2
Find the Studies subsection. In the Select Study tree, select General Studies>Stationary.
3
Click Add Study in the window toolbar.
Odgen
1
In the Model Builder window, click Study 3.
2
In the Settings window for Study, type Odgen in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots check box.
Step 1: Stationary
1
In the Model Builder window, under Odgen click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step check box.
4
In the tree, select Component 1 (Comp1)>Solid Mechanics (Solid)>Neo-Hookean, Component 1 (Comp1)>Solid Mechanics (Solid)>Mooney-Rivlin, and Component 1 (Comp1)>Solid Mechanics (Solid)>Varga.
5
Click  Disable.
6
Locate the Study Extensions section. Select the Auxiliary sweep check box.
7
Click  Add.
8
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
stretch (Applied stretch)
range(1, 0.1, 2) range(2.2, 0.2, 10)
 
Solution 3 (sol3)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 3 (sol3) node, then click Dependent Variables 1.
3
In the Settings window for Dependent Variables, locate the Scaling section.
4
From the Method list, choose Manual.
5
In the Model Builder window, expand the Odgen>Solver Configurations>Solution 3 (sol3)>Stationary Solver 1 node, then click Direct.
6
In the Settings window for Direct, locate the General section.
7
From the Solver list, choose PARDISO.
8
In the Model Builder window, under Odgen>Solver Configurations>Solution 3 (sol3)>Stationary Solver 1 click Parametric 1.
9
In the Settings window for Parametric, locate the Continuation section.
10
From the Predictor list, choose Constant.
11
In the Model Builder window, under Odgen>Solver Configurations>Solution 3 (sol3)>Stationary Solver 1 click Fully Coupled 1.
12
In the Settings window for Fully Coupled, locate the Method and Termination section.
13
From the Nonlinear method list, choose Constant (Newton).
14
In the Study toolbar, click  Compute.
Finally, add a fourth study for the Varga material model.
Add Study
1
Go to the Add Study window.
2
Find the Studies subsection. In the Select Study tree, select General Studies>Stationary.
3
Click Add Study in the window toolbar.
4
In the Study toolbar, click  Add Study to close the Add Study window.
Study 4
1
In the Model Builder window, click Study 4.
2
In the Settings window for Study, locate the Study Settings section.
3
Clear the Generate default plots check box.
Step 1: Stationary
1
In the Model Builder window, under Study 4 click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step check box.
4
In the tree, select Component 1 (Comp1)>Solid Mechanics (Solid)>Neo-Hookean, Component 1 (Comp1)>Solid Mechanics (Solid)>Mooney-Rivlin, and Component 1 (Comp1)>Solid Mechanics (Solid)>Ogden.
5
Click  Disable.
6
Locate the Study Extensions section. Select the Auxiliary sweep check box.
7
Click  Add.
8
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
stretch (Applied stretch)
range(1, 0.1, 2) range(2.2, 0.2, 10)
 
9
In the Model Builder window, click Study 4.
10
In the Settings window for Study, type Varga in the Label text field.
Solution 4 (sol4)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 4 (sol4) node, then click Dependent Variables 1.
3
In the Settings window for Dependent Variables, locate the Scaling section.
4
From the Method list, choose Manual.
5
In the Model Builder window, expand the Varga>Solver Configurations>Solution 4 (sol4)>Stationary Solver 1 node, then click Direct.
6
In the Settings window for Direct, locate the General section.
7
From the Solver list, choose PARDISO.
8
In the Model Builder window, under Varga>Solver Configurations>Solution 4 (sol4)>Stationary Solver 1 click Parametric 1.
9
In the Settings window for Parametric, locate the Continuation section.
10
From the Predictor list, choose Constant.
11
In the Model Builder window, under Varga>Solver Configurations>Solution 4 (sol4)>Stationary Solver 1 click Fully Coupled 1.
12
In the Settings window for Fully Coupled, locate the Method and Termination section.
13
From the Nonlinear method list, choose Constant (Newton).
14
In the Study toolbar, click  Compute.
The first default plot shows the von Mises stress on the modeled 2D cross section for the neo-Hookean material at maximum inflation. When you adjust the scaling, the plot should become similar to Figure 5.
Results
Surface 1
1
In the Model Builder window, expand the Results>Stress (solid) node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose MPa.
Deformation
1
In the Model Builder window, expand the Surface 1 node, then click Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
In the Scale factor text field, type 0.05.
4
In the Stress (solid) toolbar, click  Plot.
5
Click the  Zoom Extents button in the Graphics toolbar.
The second default plot shows the von Mises stress in a 3D revolved plot. To reproduce Figure 3, proceed as follows.
Inflation Pressure
1
In the Model Builder window, under Results click 1D Plot Group 4.
2
In the Settings window for 1D Plot Group, type Inflation Pressure in the Label text field.
3
Locate the Plot Settings section. Select the x-axis label check box.
4
In the associated text field, type Applied stretch.
5
Select the y-axis label check box.
6
In the associated text field, type Inflation pressure (100 Pa).
7
Click to expand the Title section. From the Title type list, choose Manual.
8
In the Title text area, type Inflation Pressure vs. Prescribed Stretch.
Point Graph 1
1
Right-click Inflation Pressure and choose Point Graph.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Neo-Hookean/Solution 1 (sol1).
4
Select Point 3 only.
5
Locate the y-Axis Data section. In the Expression text field, type p_f/100.
6
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Global definitions>Parameters>stretch - Applied stretch.
7
Click to expand the Legends section. Select the Show legends check box.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
Neo-Hookean
10
In the Inflation Pressure toolbar, click  Plot.
Point Graph 2
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Mooney-Rivlin/Solution 2 (sol2).
4
Locate the Legends section. In the table, enter the following settings:
Legends
Mooney-Rivlin
5
In the Inflation Pressure toolbar, click  Plot.
Point Graph 3
1
In the Model Builder window, under Results>Inflation Pressure right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Odgen/Solution 3 (sol3).
4
Locate the Legends section. In the table, enter the following settings:
Legends
Ogden
5
In the Inflation Pressure toolbar, click  Plot.
Point Graph 4
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Varga/Solution 4 (sol4).
4
Locate the Legends section. In the table, enter the following settings:
Legends
Varga
5
In the Inflation Pressure toolbar, click  Plot.
Point Graph 5
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type 2*(H/Ri)*((6.3e5[Pa]*(stretch^(1.3-3)-stretch^(-2*1.3-3)))+(0.012e5[Pa]*(stretch^(5-3)-stretch^(-2*5-3)))-(0.1e5[Pa]*(stretch^(-2-3)-stretch^(2*2-3))))/100.
4
Click to expand the Coloring and Style section. Find the Line style subsection. From the Line list, choose None.
5
From the Color list, choose From theme.
6
Find the Line markers subsection. From the Marker list, choose Asterisk.
7
In the Number text field, type 40.
8
Locate the Legends section. In the table, enter the following settings:
Legends
Analytical
9
In the Inflation Pressure toolbar, click  Plot.
To reproduce Figure 4, proceed as follows.
First Principal Stress
1
In the Model Builder window, right-click Inflation Pressure and choose Duplicate.
2
In the Settings window for 1D Plot Group, type First Principal Stress in the Label text field.
3
Locate the Title section. In the Title text area, type First Principal Stress vs. Prescribed Stretch.
4
Locate the Plot Settings section. In the y-axis label text field, type First principal stress (MPa).
5
Locate the Axis section. Select the Manual axis limits check box.
6
In the y maximum text field, type 40.
Point Graph 1
1
In the Model Builder window, expand the First Principal Stress node, then click Point Graph 1.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type solid.sp1.
4
From the Unit list, choose MPa.
Point Graph 2
1
In the Model Builder window, click Point Graph 2.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type solid.sp1.
4
From the Unit list, choose MPa.
Point Graph 3
1
In the Model Builder window, click Point Graph 3.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type solid.sp1.
4
From the Unit list, choose MPa.
Point Graph 4
1
In the Model Builder window, click Point Graph 4.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type solid.sp1.
4
From the Unit list, choose MPa.
Point Graph 5
1
In the Model Builder window, click Point Graph 5.
2
In the Settings window for Point Graph, locate the y-Axis Data section.
3
In the Expression text field, type ((6.3e5[Pa]*(stretch^(1.3)-stretch^(-2*1.3)))+(0.012e5[Pa]*(stretch^(5)-stretch^(-2*5)))-(0.1e5[Pa]*(stretch^(-2)-stretch^(2*2)))).
4
From the Unit list, choose MPa.
5
In the First Principal Stress toolbar, click  Plot.