PDF
Chloroprene Rubber Compression Test
Introduction
Elastomers and biological materials exhibit strain-rate dependent mechanical behavior and hysteresis when subjected to cyclical loads. The Bergstrom–Boyce material model has been successfully used to capture such phenomena in applications where these nonequilibrium effects are important. This example demonstrates the use of the Polymer Viscoplasticity feature available in the Nonlinear Structural Materials Module. The simulation results are compared with results found in the literature.
Model Definition
In this model, a cylindrical rubber specimen with a height, H, of 13 mm and a diameter, D, of 68 mm, is subjected to compression following the true strain history shown in Figure 1. The specimen is loaded at a constant true strain rate of 0.002 1/s and the strain is held constant for 120 s when the strain level reaches 0.3 and 0.6. The unloading phase is symmetric with respect to the loading phase. This strain history has been used to conduct the experimental tests on carbon-black-filled chloroprene rubber shown in Ref. 2, and constitutes a test benchmark for the Bergstrom–Boyce numerical material model used also in Ref. 1.
The geometry exhibits 2D axial symmetry as well as a reflection symmetry in the mid cross section of the cylinder. It is therefore possible to reduce the model geometry to a rectangle with height equal to half of the length of the specimen and a width equal to its radius.
Figure 1: True strain time history.
Material Model
The rheology of the Bergstrom–Boyce material model is shown in Figure 2. It features a so-called equilibrium network that can be schematized as a simple hyperelastic spring characterized by an Arruda–Boyce strain energy, in parallel with a second network that models the nonequilibrium behavior. This latter network comprises an isochoric Arruda–Boyce spring in series with a viscoplastic element whose rate multiplier is given by
(1)
when σvm − σco is positive and zero otherwise. Here, σvm is the von Mises stress of the nonequilibrium network and σco is a material parameter identifying a cutoff stress. The symbols A, c, n, and σres identify material properties. Moreover
(2)
is a measure of the stretch in the viscoplastic element, Fvp being its deformation gradient. A small parameter
is used to avoid singularities when Fvp is identity and the exponent c is negative.
The numerical values of the material properties used in the model are given in Table 1. They are adapted from those used in Ref. 1 and Ref. 2 for the COMSOL Multiphysics implementation of the Bergstrom–Boyce model.
Table 1: material properties.
Constant
Value
 σco
0[MPa]
 A
7*sqrt(2/3)[1/s]
 σres
sqrt(3)[MPa]
 n
4
 c
-1
Figure 2: Rheology of the Bergstrom–Boyce material model.
Results and Discussion
Figure 3 shows the true stress versus true strain curve, comparing results with those found in the literature. It can be observed that during both the loading phase and the unloading phase, when the strain is held constant, the stress tends to the same equilibrium value, that is, the one given by the pure elastic network only at that strain value. This can seen in Figure 4, where the stress–strain curve obtained with the Bergstrom–Boyce model is compared to that obtained when the same strain history is applied to a pure hyperelastic Arruda–Boyce model with the same material parameter as the equilibrium network of the Bergstrom–Boyce model. Note that the same equilibrium behavior can also be obtained performing a static analysis with the Bergstrom–Boyce material while using the Long term option for the stiffness used in stationary solver, that is, modeling the stress after infinite time.
Figure 3: True stress versus true strain curve.
Figure 4: Comparison between the nonequilibrium behavior of the elastomeric material and the equilibrium one.
Figure 5 shows the total stretch of the specimen, along with the elastic and viscoplastic stretches of the nonequilibrium network. This shows that the stretch in the viscoplastic element is delayed with respect to the total stress, which makes the elastic stretch change sign during the unloading phase. The elastic element of the nonequilibrium element will thus be in tension during unloading instead of in compression, which reduces the overall compressive stress with respect to the equilibrium behavior.
Figure 5: Comparison between the total stretch of the material, with the viscoplastic and elastic part of the stretch in the nonequilibrium network.
Figure 6 shows the magnitude of the force developed in the nonequilibrium network, normalized with respect to its maximum along the time axis. It can be observed how the force relaxes during the time spans where the strain is kept fixed.
Figure 6: Force developed in the nonequilibrium network.
Notes About the COMSOL Implementation
•
You can use the Bergstrom–Boyce material model by adding a Polymer Viscoplasticity node under Hyperelastic Material.
•
The desired true strain history can be imposed by applying a Predescribed Displacement node on the top surface of the specimen. The displacement can be computed as
where ε (t) is the true strain.
•
You find the Domain ODEs option in the Time stepping section of the Polymer Viscoplasticity node. This option can be faster than Backward Euler when the number of degrees of freedom is small.
References
1. D. Husnu and M.Kaliske, “Bergstrom-Boyce model for nonlinear finite rubber viscoelasticity: theoretical aspects and algorithmic treatment for the FE method,” Comput. Mech., vol. 44, pp. 809–823, 2009.
2. J.S. Bergström and M. Boyce, “Constitutive modeling of the large strain time-dependent behavior of elastomers,” J. Mech. Phys. Solids, vol. 46, pp. 931–954, 1998.
Application Library path: Nonlinear_Structural_Materials_Module/Viscoplasticity/chloroprene_rubber_compression_test
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 > Time Dependent.
6
Click  Done.
Global Definitions
Geometrical Parameters
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, type Geometrical Parameters in the Label text field.
3
Locate the Parameters section. In the table, enter the following settings:
Name
Expression
Value
Description
H
13[mm]
0.013 m
Height of test specimen
D
28[mm]
0.028 m
Diameter of test specimen
A0
pi*D^2/4
6.1575E-4 m²
Surface area of test specimen
Strain History Data
1
In the Home toolbar, click  Parameters and choose Add > Parameters.
2
In the Settings window for Parameters, type Strain History Data in the Label text field.
3
Locate the Parameters section. In the table, enter the following settings:
Name
Expression
Value
Description
edot
0.002[1/s]
0.002 1/s
True strain rate
Dt
150[s]
150 s
Time before relaxation
Rt
120[s]
120 s
Relaxation time
endTime
1280[s]
1280 s
Total simulation time
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
Rectangle 1 (r1)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type D/2.
4
In the Height text field, type H/2.
5
Click  Build Selected.
6
Click  Build All Objects.
Definitions
Logarithmic Strain
1
In the Definitions toolbar, click  Piecewise.
2
In the Settings window for Piecewise, locate the Definition section.
3
In the Argument text field, type time.
4
Find the Intervals subsection. In the table, enter the following settings:
Start
End
Function
0
Dt
edot*time
Dt
Dt+Rt
edot*Dt
Dt+Rt
2*Dt+Rt
edot*(time-Rt)
2*Dt+Rt
2*(Dt+Rt)
2*edot*Dt
2*(Dt+Rt)
2*(Dt+Rt)+2*Dt/3
edot*(time-2*Rt)
2*(Dt+Rt)+2*Dt/3
2*(Dt+Rt)+4*Dt/3
1+edot*(2*(Dt+Rt)-time)
2*(Dt+Rt)+4*Dt/3
2*Dt+3*Rt+4*Dt/3
2*edot*Dt
2*Dt+3*Rt+4*Dt/3
3*(Dt+Rt)+4*Dt/3
0.4+edot*(3*Rt+4*Dt-time)
3*(Dt+Rt)+4*Dt/3
3*Dt+4*Rt+4*Dt/3
edot*Dt
3*Dt+4*Rt+4*Dt/3
4*(Dt+Rt)+4*Dt/3
0.4+edot*(4*Rt+4*Dt-time)
5
Locate the Units section. In the Arguments text field, type s.
6
In the Function text field, type 1.
7
Click  Plot.
8
In the Label text field, type Logarithmic Strain.
Top Surface Average
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 Boundary.
4
Select Boundary 3 only.
5
In the Label text field, type Top Surface Average.
Solid Mechanics (solid)
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, locate the Structural Transient Behavior section.
3
From the list, choose Quasistatic.
Symmetry Plane 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry Plane.
2
Select Boundary 2 only.
Hyperelastic Material 1
1
In the Physics toolbar, click  Domains and choose Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, locate the Hyperelastic Material section.
3
From the Material model list, choose Arruda–Boyce.
4
From the Compressibility list, choose Compressible, uncoupled.
5
From the Volumetric strain energy list, choose Miehe.
6
Select Domain 1 only.
Polymer Viscoplasticity 1
1
In the Physics toolbar, click  Attributes and choose Polymer Viscoplasticity.
2
In the Settings window for Polymer Viscoplasticity, locate the Viscoplasticity Model section.
3
Find the Hyperelastic element subsection. In the βv text field, type 1.6.
4
Locate the Time Stepping section. From the Method list, choose Domain ODEs.
Prescribed Displacement 1
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
3
From the Displacement in z direction list, choose Prescribed.
4
In the u 0 z text field, type 0.5*H*(exp(-pw1(t))-1).
5
Select Boundary 3 only.
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
Bulk modulus
K
2[GPa]
N/m²
Bulk modulus and shear modulus
Number of segments
Nseg
8
1
Arruda-Boyce
Macroscopic shear modulus
mu0
0.6[MPa]
N/m²
Arruda-Boyce
Density
rho
0
kg/m³
Basic
Viscoplastic rate coefficient
A_BB
7*sqrt(2/3)[1/s]
1/s
Bergstrom-Boyce viscoplasticity
Flow resistance
sigRes_BB
sqrt(3)[MPa]
N/m²
Bergstrom-Boyce viscoplasticity
Stress exponent
n_BB
4
1
Bergstrom-Boyce viscoplasticity
Cutoff stress
sigmaco_BB
0
N/m²
Bergstrom-Boyce viscoplasticity
Strain exponent
c_BB
-1
1
Bergstrom-Boyce viscoplasticity
Mesh 1
Mapped 1
In the Mesh toolbar, click  Mapped.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundaries 2 and 4 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 1.
5
Click  Build All.
Nonequilibrium Modeling
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Nonequilibrium Modeling in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots checkbox.
Step 1: Time Dependent
1
In the Model Builder window, under Nonequilibrium Modeling click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type range(0,8,endTime).
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 Nonequilibrium Modeling > Solver Configurations > Solution 1 (sol1) > Time-Dependent Solver 1 node.
4
In the Model Builder window, expand the Nonequilibrium Modeling > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 node, then click Displacement Field (comp1.u).
5
In the Settings window for Field, locate the Scaling section.
6
In the Scale text field, type 0.005.
7
In the Model Builder window, under Nonequilibrium Modeling > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 click Equivalent Viscoplastic Strain (comp1.solid.hmm1.pvp1.evpe).
8
In the Settings window for Field, locate the Scaling section.
9
In the Scale text field, type 1.
10
In the Model Builder window, under Nonequilibrium Modeling > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 click Viscoplastic Strain Tensor, Local Coordinate System (comp1.solid.hmm1.pvp1.evp).
11
In the Settings window for Field, locate the Scaling section.
12
In the Scale text field, type 1.
13
In the Model Builder window, under Nonequilibrium Modeling > Solver Configurations > Solution 1 (sol1) click Time-Dependent Solver 1.
14
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
15
From the Steps taken by solver list, choose Strict.
16
In the Study toolbar, click  Compute.
Set default units for result presentation.
Results
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, select Solid Mechanics > Stress tensor (N/m^2) in the tree.
5
Click OK.
6
In the Settings window for Preferred Units, locate the Units section.
7
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Stress tensor
N/m^2
MPa
8
Select the Apply conversions to expressions with the same dimensions checkbox.
9
Click  Apply.
Revolution 2D 1
1
In the Model Builder window, expand the Results > Datasets node.
2
Right-click Results > Datasets and choose Revolution 2D.
Mirror 3D 1
1
In the Results toolbar, click  More Datasets and choose Mirror 3D.
2
In the Settings window for Mirror 3D, locate the Plane Data section.
3
From the Plane list, choose XY-planes.
Displacements
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Displacements in the Label text field.
3
Locate the Data section. From the Dataset list, choose Mirror 3D 1.
4
Click to expand the Title section. From the Title type list, choose Manual.
5
In the Title text area, type Displacement magnitude [mm].
6
In the Parameter indicator text field, type Time=eval(t) s.
Volume 1
1
Right-click Displacements and choose Volume.
2
In the Settings window for Volume, locate the Coloring and Style section.
3
From the Color table list, choose SpectrumLight.
Deformation 1
1
Right-click Volume 1 and choose Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor checkbox. In the associated text field, type 1.
Displacements
1
In the Model Builder window, under Results click Displacements.
2
In the Displacements toolbar, click  Plot.
Stretch History
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Stretch History in the Label text field.
3
Click to expand the Title section. From the Title type list, choose Manual.
4
In the Title text area, type Deformation Gradient.
5
Locate the Plot Settings section.
6
Select the y-axis label checkbox. In the associated text field, type Stretch (1).
Global 1
1
Right-click Stretch History and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
aveop1(solid.FdzZ)
1
Total stretch
aveop1(solid.hmm1.pvp1.Fvpl33)
1
Viscoplastic stretch
aveop1(solid.hmm1.pvp1.Fvpil33*solid.FdzZ)
1
Elastic stretch
4
Click to expand the Coloring and Style section. From the Width list, choose 2.
Stretch History
1
In the Model Builder window, click Stretch History.
2
In the Settings window for 1D Plot Group, locate the Legend section.
3
From the Position list, choose Center.
4
In the Stretch History toolbar, click  Plot.
True Stress
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type True Stress in the Label text field.
3
Locate the Title section. From the Title type list, choose Manual.
4
In the Title text area, type True Stress.
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type True strain (1).
7
Select the y-axis label checkbox. In the associated text field, type True stress (MPa).
Global 1
1
Right-click True Stress and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
aveop1(-solid.szz)
MPa
Top Surface Average
4
Locate the x-Axis Data section. From the Parameter list, choose Expression.
5
In the Expression text field, type aveop1(abs(solid.elogzz)).
6
Locate the Coloring and Style section. From the Width list, choose 2.
7
Click to expand the Legends section. From the Legends list, choose Manual.
8
In the table, enter the following settings:
Legends
Comsol
True Stress
1
In the Model Builder window, click True Stress.
2
In the Settings window for 1D Plot Group, locate the Legend section.
3
From the Position list, choose Upper left.
Import results from Ref. 1 in a table to plot them along with the simulation results.
Reference Results
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type Reference Results in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file chloroprene_rubber_compression_test_numerical.txt.
Table Graph 1
1
Right-click True Stress and choose Table Graph.
2
In the Settings window for Table Graph, locate the Coloring and Style section.
3
Find the Line style subsection. From the Line list, choose None.
4
Find the Line markers subsection. From the Marker list, choose Circle.
5
Click to expand the Legends section. Select the Show legends checkbox.
6
From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Reference
Experimental Results
1
In the Results toolbar, click  Table.
2
In the Settings window for Table, type Experimental Results in the Label text field.
3
Locate the Data section. Click  Import.
4
Browse to the model’s Application Libraries folder and double-click the file chloroprene_rubber_compression_test_experimental.txt.
Table Graph 2
1
Right-click True Stress and choose Table Graph.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Table list, choose Experimental Results.
4
Locate the Coloring and Style section. Find the Line style subsection. From the Line list, choose None.
5
Find the Line markers subsection. From the Marker list, choose Circle.
6
Locate the Legends section. Select the Show legends checkbox.
7
From the Legends list, choose Manual.
8
In the table, enter the following settings:
Legends
Experiments
9
In the True Stress toolbar, click  Plot.
Comparison 1
1
In the Model Builder window, right-click Global 1 and choose Comparison.
2
In the Settings window for Comparison, locate the Comparison section.
3
From the Metric list, choose Coefficient of determination.
4
In the True Stress toolbar, click  Plot.
Inelastic Force Contribution
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Inelastic Force Contribution in the Label text field.
3
Locate the Title section. From the Title type list, choose Manual.
4
In the Title text area, type Normalized Inelastic Force: P<SUB>33</SUB>A<SUB>0</SUB>/max(P<SUB>33</SUB>A<SUB>0</SUB>).
5
Locate the Plot Settings section.
6
Select the y-axis label checkbox. In the associated text field, type Normalized force (1).
Global 1
1
Right-click Inelastic Force Contribution and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
aveop1(abs(solid.elogzz))
1
True strain
4
Locate the Coloring and Style section. From the Width list, choose 2.
Max Inelastic Force
1
In the Results toolbar, click  Point Evaluation.
2
In the Settings window for Point Evaluation, type Max Inelastic Force in the Label text field.
3
Select Point 2 only.
4
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
timemax(0,endTime,abs(solid.Fdlz3*solid.Siel33*A0))
N
 
5
Locate the Data section. From the Time selection list, choose First.
6
Click  Evaluate.
Global 1
1
In the Model Builder window, under Results > Inelastic Force Contribution click Global 1.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
aveop1(abs(solid.Fdlz3*solid.Siel33*A0)/146.75[N])
1
Inelastic force
4
In the Inelastic Force Contribution toolbar, click  Plot.
Add a new study to compute the equilibrium behavior.
Add Study
1
In the Home 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 > Time Dependent.
4
Click the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Equilibrium Modeling
1
In the Settings window for Study, type Equilibrium Modeling in the Label text field.
2
Locate the Study Settings section. Clear the Generate default plots checkbox.
Step 1: Time Dependent
1
In the Model Builder window, under Equilibrium Modeling click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type range(0,8,endTime).
4
Locate the Physics and Variables Selection section. Select the Modify model configuration for study step checkbox.
5
In the tree, select Component 1 (comp1) > Solid Mechanics (solid), Controls spatial frame > Hyperelastic Material 1 > Polymer Viscoplasticity 1.
6
Right-click and choose Disable.
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 Time-Dependent Solver 1.
3
In the Settings window for Time-Dependent Solver, locate the Time Stepping section.
4
From the Steps taken by solver list, choose Strict.
5
In the Model Builder window, expand the Equilibrium Modeling > Solver Configurations > Solution 2 (sol2) > Time-Dependent Solver 1 node, then click Fully Coupled 1.
6
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
7
From the Nonlinear method list, choose Automatic (Newton).
8
In the Model Builder window, expand the Equilibrium Modeling > Solver Configurations > Solution 2 (sol2) > Dependent Variables 1 node, then click Displacement Field (comp1.u).
9
In the Settings window for Field, locate the Scaling section.
10
In the Scale text field, type 0.005.
11
In the Study toolbar, click  Compute.
Results
Nonequilibrium vs. Equilibrium
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Nonequilibrium vs. Equilibrium in the Label text field.
3
Locate the Title section. From the Title type list, choose Manual.
4
In the Title text area, type True Stress.
5
Locate the Plot Settings section.
6
Select the x-axis label checkbox. In the associated text field, type True strain (1).
7
Select the y-axis label checkbox. In the associated text field, type True stress (MPa).
8
Locate the Legend section. From the Position list, choose Upper left.
Nonequilibrium
1
Right-click Nonequilibrium vs. Equilibrium and choose Global.
2
In the Settings window for Global, type Nonequilibrium in the Label text field.
3
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
aveop1(-solid.szz)
MPa
Top Surface Average
4
Locate the Coloring and Style section. From the Width list, choose 2.
5
Locate the Legends section. Find the Include subsection. Select the Label checkbox.
6
Clear the Solution checkbox.
7
Clear the Description checkbox.
8
Locate the x-Axis Data section. From the Parameter list, choose Expression.
9
In the Expression text field, type aveop1(abs(solid.elogzz)).
Equilibrium
1
Right-click Nonequilibrium and choose Duplicate.
2
In the Settings window for Global, type Equilibrium in the Label text field.
3
Locate the Data section. From the Dataset list, choose Equilibrium Modeling/Solution 2 (sol2).
Difference
1
In the Model Builder window, right-click Nonequilibrium and choose Duplicate.
2
In the Settings window for Global, type Difference in the Label text field.
3
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
aveop1(-solid.szz)-withsol('sol2',aveop1(-solid.szz),setval(t,t))
MPa
 
4
In the Nonequilibrium vs. Equilibrium toolbar, click  Plot.