PDF
Hyperelastic Seal
Introduction
In this example you study the force-deflection relation of a car door seal made from a soft rubber material. The model uses a hyperelastic material model together with formulations that can account for the large deformations and contact conditions.
It is of special interest to investigate the effect of air confined within the seal.
See the Nonlinear Structural Materials Module User’s Guide for theory about hyperelastic material.
Model Definition
The seal is compressed between a stationary plane surface and an indenting cylinder. There is also a vertical rigid wall at a distance of 1 mm from the initial position of the seal. Figure 1 shows the undeformed geometry of the seal and the contacting surfaces.
Figure 1: Model geometry.
The model describes a cross section of the seal assuming plane strain conditions. The (arbitrary) thickness in the out-of-plane direction is chosen as 50 mm. The contacting surfaces are rigid when compared to the seal.
When computing the pressure from the air compressed inside the seal, the current cross-section area is required. A useful method for computing an area is by using the divergence theorem, and converting the original surface integral to a contour integral:
You need to compute the integral in the deformed geometry, which is the default.
Material Properties
•
The rubber is hyperelastic and is modeled as a Mooney-Rivlin material with C10 = 0.37 MPa and C01 = 0.11 MPa. The material is almost incompressible, so the bulk modulus is set to 104 MPa. A mixed formulation is automatically used for this material model.
•
The compression of the confined air is assumed to be adiabatic, giving the pressure-density relation
Here the cross-section area is denoted by A, with the undeformed value A0 = 123.63 mm2. The constant γ has the value 1.4 and p0 = 0.1 MPa is the standard air pressure. The load acting on the interior of the seal is then
Constraints and Loads
•
One contact pair is used between the cylinder and the seal.
•
One contact pair is used between the stationary plates and the seal.
•
The lower straight part of the seal is glued to the car body. This is modeled with an adhesion condition.
•
The rigid cylinder is lowered using the parameter of the parametric continuation solver as the negative y displacement. It starts with a gap of 0 mm and is lowered 4 mm.
Results and Discussion
Figure 2 shows the deformed shape at the lowest cylinder position — corresponding to an indentation of 4 mm — without internal pressure. The deformation scale is 1:1, that is, a true shape. The plot shows a detachment region of significant size.
Figure 2: Seal deformation at 4 mm indentation without internal pressure.
Figure 3 shows the corresponding contact pressure plot. The detachment region appears first at an indentation just over 2.5 mm and grows as the indentation increases further. The actual contact areas are reduced to two spots at the sides.
Such a significant change in the contact pressure distribution indicates that the computations must be performed using a fine mesh together with sufficiently small steps in the parametric analysis with respect to the indentation value.
Figure 3: The contact pressure distribution over the area between the seal and cylinder for different indentations without internal pressure.
Figure 4 shows the result of the computations with the internal pressure taken into account. The seal profile appears inflated. The contact pressure plot in Figure 5 confirms that the detachment region never appears even though the contact pressure has a pronounced minimum in the middle part.
Figure 4: Seal deformation at 4 mm indentation with the internal pressure.
Figure 5: The contact pressure distribution for different indentations with the internal pressure taken into account.
Figure 6 contains a plot of the force per unit length versus the indentation of the rigid cylinder, with and without the internal pressure taken into account. The distinct change in slope of the curves is when the rightmost part of the seal comes into contact with the vertical wall, and no longer can deform in that direction.
Notice that the forces needed to compress the seal can be almost one order of magnitude larger when the effect of the confined air is taken into account.
In reality, a car door seal contains small holes through which the air can escape as long as the compression is not too fast. Thus the computed values are the limits corresponding to very slow and very fast compression, respectively.
Figure 6: Compressive force per unit length versus indentation with and without internal pressure.
Notes About the COMSOL Implementation
As an optional feature of the model, an Elastic Predeformation node is added to the physics. This feature updates the geometry with the deformation from the previous increment, meaning that, for example, the ‘incremental’ deformation gradient becomes smaller, which can improve convergence when deformations are large. Note that the total deformation gradient still considers the deformation with respect to the reference configuration of the geometry. Adding this feature speeds up the convergence of the model, but it would solve and converge to the same results also without the Elastic Predeformation node.
Application Library path: Nonlinear_Structural_Materials_Module/Hyperelasticity/hyperelastic_seal
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.
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
If you do not want to build all the geometry, you can load the geometry sequence from the stored model. In the Model Builder window, under Component 1 (comp1) right-click Geometry 1 and choose Insert Sequence. Browse to the model’s Application Libraries folder and double-click the file hyperelastic_seal.mph. You can then continue to the Global Definitions section below.
To build the geometry from scratch, continue from here.
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.
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 6.
4
In the Sector angle text field, type 180.
5
Locate the Position section. In the y text field, type 6.
6
Locate the Rotation Angle section. In the Rotation text field, type 90.
7
Click to expand the Layers section. In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
1.5
Circle 2 (c2)
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 4.
4
In the Sector angle text field, type 90.
5
Locate the Position section. In the x text field, type 8.
6
In the y text field, type 8.
7
Locate the Layers section. In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
1.5
Circle 3 (c3)
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 4.
4
In the Sector angle text field, type 90.
5
Locate the Position section. In the x text field, type 8.
6
In the y text field, type 4.
7
Locate the Rotation Angle section. In the Rotation text field, type -90.
8
Locate the Layers section. In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
1.5
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 8.
4
In the Height text field, type 12.
5
Click to expand the Layers section. In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
1.5
Layer 2
9
Rectangle 2 (r2)
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 1.5.
4
In the Height text field, type 4.
5
Locate the Position section. In the x text field, type 10.5.
6
In the y text field, type 4.
7
Click  Build Selected.
8
Click the  Zoom Extents button in the Graphics toolbar.
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 2 only.
5
On the object c2, select Domain 1 only.
6
On the object c3, select Domain 1 only.
7
On the object r1, select Domain 2 only.
Union 1 (uni1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Union.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
3
In the Settings window for Union, locate the Union section.
4
Clear the Keep interior boundaries check box.
Create the indentor.
Indenter
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, type Indenter in the Label text field.
3
Locate the Size and Shape section. In the Radius text field, type 12.
4
In the Sector angle text field, type 90.
5
Locate the Position section. In the x text field, type 4.
6
In the y text field, type 24.
7
Locate the Rotation Angle section. In the Rotation text field, type -135.
8
Locate the Selections of Resulting Entities section. Select the Resulting objects selection check box.
9
From the Show in physics list, choose Boundary selection.
Create the support.
Rectangle 3 (r3)
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 20.
4
Locate the Position section. In the x text field, type -7.
5
In the y text field, type -1.
6
Locate the Selections of Resulting Entities section. Select the Resulting objects selection check box.
7
From the Show in physics list, choose Boundary selection.
8
Find the Cumulative selection subsection. Click New.
9
In the New Cumulative Selection dialog box, type Rigid base in the Name text field.
10
Click OK.
Rectangle 4 (r4)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Height text field, type 12.
4
Locate the Position section. In the x text field, type 13.
5
Locate the Selections of Resulting Entities section. Find the Cumulative selection subsection. From the Contribute to list, choose Rigid base.
Convert to Curve 1 (ccur1)
1
In the Geometry toolbar, click  Conversions and choose Convert to Curve.
2
Select the objects c4, r3, and r4 only.
3
In the Settings window for Convert to Curve, click  Build Selected.
Delete Entities 2 (del2)
1
Right-click Geometry 1 and choose Delete Entities.
2
On the object ccur1, select Boundaries 1, 2, 4–6, and 8–10 only.
Form Union (fin)
1
In the Model Builder window, under Component 1 (comp1)>Geometry 1 click Form Union (fin).
2
In the Settings window for Form Union/Assembly, locate the Form Union/Assembly section.
3
From the Action list, choose Form an assembly.
4
Clear the Create pairs check box.
5
Click  Build Selected.
6
Click the  Zoom Extents button in the Graphics toolbar.
The model geometry is now complete.
Inner seal boundary
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type Inner seal boundary in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Boundary.
4
Select the Group by continuous tangent check box.
5
Select one of the boundaries on the inside of the seal.
Outer seal boundary
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type Outer seal boundary in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Boundary.
4
Select the Group by continuous tangent check box.
5
Select one of the boundaries on the outside of the seal.
Glued seal boundary
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type Glued seal boundary in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Boundary.
4
On the object fin, select Boundary 4 only.
Global Definitions
Add a parameter that you can use to gradually increase the vertical displacement.
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
para
0
0
Vertical displacement parameter
d
50[mm]
0.05 m
Out-of-plane thickness
Definitions
Contact Pair 1 (p1)
1
In the Definitions toolbar, click  Pairs and choose Contact Pair.
2
In the Settings window for Pair, type upper in the Pair name text field.
3
Locate the Source Boundaries section. From the Selection list, choose Indenter.
4
Locate the Destination Boundaries section. From the Selection list, choose Outer seal boundary.
Contact Pair 2 (p2)
1
In the Definitions toolbar, click  Pairs and choose Contact Pair.
2
In the Settings window for Pair, type lower in the Pair name text field.
3
Locate the Source Boundaries section. From the Selection list, choose Rigid base.
4
Locate the Destination Boundaries section. From the Selection list, choose Outer seal boundary.
The boundaries in the contact pairs are unnecessarily large because it was convenient to reuse existing selections. In large 3D models, you should however keep down the size of the contact boundaries for performance reasons.
Prescribe the deformation of the indentor by using a moving mesh with prescribed deformation. An alternative would have been to include the indentor in the Solid Mechanics interface, and prescribe its deformation.
Prescribed Deformation 1
1
In the Definitions toolbar, click  Moving Mesh and choose Prescribed Deformation.
2
In the Settings window for Prescribed Deformation, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Indenter.
5
Locate the Prescribed Deformation section. Specify the dx vector as
0
X
-para*1[mm]
Y
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 Thickness section.
3
In the d text field, type d.
In the plane strain approximation, this setting only affects total force computations.
Hyperelastic Material 1
1
In the Physics toolbar, click  Domains and choose Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, locate the Domain Selection section.
3
From the Selection list, choose All domains.
4
Locate the Hyperelastic Material section. From the Material model list, choose Mooney-Rivlin, two parameters.
5
In the κ text field, type 1e4[MPa].
Contact 1
1
In the Physics toolbar, click  Pairs and choose Contact.
2
In the Settings window for Contact, locate the Pair Selection section.
3
Under Pairs, click  Add.
4
In the Add dialog box, select Contact Pair 1 (upper) in the Pairs list.
5
Click OK.
The source boundaries are not within the Solid Mechanics interface itself. This must be indicated.
6
In the Settings window for Contact, locate the Contact Surface section.
7
Select the Source external to current physics check box.
Friction 1
1
In the Physics toolbar, click  Attributes and choose Friction.
2
In the Settings window for Friction, locate the Friction Parameters section.
3
In the μ text field, type 0.3.
Contact 2
1
In the Physics toolbar, click  Pairs and choose Contact.
2
In the Settings window for Contact, locate the Pair Selection section.
3
Under Pairs, click  Add.
4
In the Add dialog box, select Contact Pair 2 (lower) in the Pairs list.
5
Click OK.
6
In the Settings window for Contact, locate the Contact Surface section.
7
Select the Source external to current physics check box.
Friction 1
1
In the Physics toolbar, click  Attributes and choose Friction.
2
In the Settings window for Friction, locate the Friction Parameters section.
3
In the μ text field, type 0.3.
Add an adhesion condition to model the glue layer at the bottom of the seal.
Contact 2
In the Model Builder window, click Contact 2.
Adhesion 1
1
In the Physics toolbar, click  Attributes and choose Adhesion.
2
In the Settings window for Adhesion, locate the Adhesive Activation section.
3
From the Activation criterion list, choose User defined.
4
In the text field, type dom==4.
5
Locate the Adhesive Stiffness section. From the Adhesive stiffness list, choose User defined.
6
Specify the k vector as
1e10[N/m^3]
t1
2e10[N/m^3]
n
Definitions
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, type AreaInt in the Operator name text field.
3
Locate the Source Selection section. From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Inner seal boundary.
Variables 1
1
In the Definitions toolbar, click  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
p0
0.1[MPa]
Pa
Initial air pressure
A0
123.63[mm^2]
m²
Undeformed enclosed area
gamma
1.4
 
Adiabatic constant
EnclosedArea
AreaInt(-x*solid.nx)
m²
Enclosed area
int_p
p0*((A0/EnclosedArea)^gamma-1)
Pa
Air pressure
Solid Mechanics (solid)
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
In the Settings window for Boundary Load, locate the Boundary Selection section.
3
From the Selection list, choose Inner seal boundary.
4
Locate the Force section. From the Load type list, choose Pressure.
5
In the p text field, type int_p.
Since large relative displacements and large deformations are expected in this model, the use of deformed geometry can give a substantial speed up of the computations.
Elastic Predeformation 1
In the Physics toolbar, click  Domains and choose Elastic Predeformation.
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
Model parameters
C10
0.37[MPa]
Pa
Mooney-Rivlin
Model parameters
C01
0.11[MPa]
Pa
Mooney-Rivlin
Density
rho
1100[kg/m^3]
kg/m³
Basic
Mesh 1
Edge 1
1
In the Mesh toolbar, click  Edge.
2
Select Boundaries 1–3 only.
Distribution 1
1
Right-click Edge 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 1.
4
Locate the Boundary Selection section. From the Selection list, choose Rigid base.
Distribution 2
1
In the Model Builder window, right-click Edge 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 50.
4
Locate the Boundary Selection section. From the Selection list, choose Indenter.
Free Triangular 1
In the Mesh toolbar, click  Free Triangular.
Size 1
1
Right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Outer seal boundary.
5
Locate the Element Size section. Click the Custom button.
6
Locate the Element Size Parameters section. Select the Maximum element size check box.
7
In the associated text field, type 0.2.
8
Click  Build All.
Study 1
Step 1: Stationary
In the first study, disable the effect of the internal pressure.
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 Physics and variables selection tree, select Component 1 (comp1)>Solid Mechanics (solid), Controls spatial frame>Boundary Load 1.
5
Click  Disable.
Set up an auxiliary continuation sweep for the para parameter. Start at a nonzero value to avoid ill-conditioning during initiation of the contact.
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
para (Vertical displacement parameter)
1e-3 range(0.1,0.1,4)
 
4
In the Model Builder window, click Study 1.
5
In the Settings window for Study, type Study: Without Pressure in the Label text field.
6
In the Study toolbar, click  Get Initial Value.
Solver Configurations
In the Model Builder window, expand the Study: Without Pressure>Solver Configurations node.
Solution 1 (sol1)
1
In the Model Builder window, expand the Study: Without Pressure>Solver Configurations>Solution 1 (sol1) node.
The default scale for the displacement variables is calculated from the entire geometry size. For models with prescribed displacements as domain or boundary constraints, the maximum prescribed displacement usually gives a better estimate of the scale.
2
In the Model Builder window, expand the Study: Without Pressure>Solver Configurations>Solution 1 (sol1)>Dependent Variables 1 node, then click Displacement field (comp1.u).
3
In the Settings window for Field, locate the Scaling section.
4
In the Scale text field, type 1e-4.
Change the scale for the auxiliary pressure to account for the material properties of the seal made of soft rubber.
5
In the Model Builder window, click Auxiliary pressure (comp1.solid.pw).
6
In the Settings window for Field, locate the Scaling section.
7
In the Scale text field, type 1e5.
Step 1: Stationary
1
In the Model Builder window, click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Results While Solving section.
3
Select the Plot check box.
Results
Stress, without Pressure
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 2D Plot Group, type Stress, without Pressure in the Label text field.
3
Locate the Plot Settings section. From the Frame list, choose Spatial  (x, y, z).
Study: Without Pressure
In the Study toolbar, click  Compute.
Results
Stress, without Pressure
1
Click the  Zoom Extents button in the Graphics toolbar.
The default plot shows the von Mises stress distribution in the seal, see Figure 2.
The following steps show how to display the contact pressure at the bottom of the seal.
Contact Pressure without Confined Air
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Contact Pressure without Confined Air in the Label text field.
3
Locate the Data section. From the Parameter selection (para) list, choose Manual.
4
In the Parameter indices (1-41) text field, type range(10,5,40).
5
Click to expand the Title section. From the Title type list, choose Manual.
6
In the Title text area, type Contact pressure profile.
Line Graph 1
1
Right-click Contact Pressure without Confined Air and choose Line Graph.
2
Select Boundaries 7, 11, and 17 only.
3
In the Settings window for Line Graph, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Solid Mechanics>Contact>Contact 1>solid.cnt1.Tn - Contact pressure - N/m².
4
Click to expand the Legends section. Select the Show legends check box.
5
Click to expand the Coloring and Style section. In the Width text field, type 2.
6
In the Contact Pressure without Confined Air toolbar, click  Plot.
The plot in the Graphics window should now look like that in Figure 3.
Now you can compute the solution including the internal pressure.
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>Stationary.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Stationary
1
In the Settings window for Stationary, locate the Study Extensions section.
2
Select the Auxiliary sweep check box.
3
Click  Add.
4
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para (Vertical displacement parameter)
1e-3 range(0.1,0.1,4)
 
5
In the Model Builder window, click Study 2.
6
In the Settings window for Study, type Study: With Pressure in the Label text field.
Use Get Inital Value to get the default plots generated, so that you can select the correct plot for Results While Solving.
7
In the Study toolbar, click  Get Initial Value.
8
In the Model Builder window, click Step 1: Stationary.
9
In the Settings window for Stationary, locate the Results While Solving section.
10
Select the Plot check box.
11
From the Plot group list, choose Stress (solid).
Solver Configurations
In the Model Builder window, expand the Study: With Pressure>Solver Configurations node.
Solution 2 (sol2)
1
In the Model Builder window, expand the Study: With Pressure>Solver Configurations>Solution 2 (sol2)>Dependent Variables 1 node, then click Displacement field (comp1.u).
2
In the Settings window for Field, locate the Scaling section.
3
In the Scale text field, type 1e-3.
4
In the Model Builder window, click Auxiliary pressure (comp1.solid.pw).
5
In the Settings window for Field, locate the Scaling section.
6
In the Scale text field, type 1e5.
Results
Stress, with Pressure
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 2D Plot Group, type Stress, with Pressure in the Label text field.
3
Locate the Plot Settings section. From the Frame list, choose Spatial  (x, y, z).
4
In the Study toolbar, click  Compute.
5
Click the  Zoom Extents button in the Graphics toolbar.
You can see that the detachment region has disappeared as a result of the seal pressurization, compare with Figure 4.
Contact Pressure with Confined Air
1
In the Model Builder window, right-click Contact Pressure without Confined Air and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Contact Pressure with Confined Air in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: With Pressure/Solution 2 (sol2).
4
In the Contact Pressure with Confined Air toolbar, click  Plot.
Finally, compute the force needed for the compression as the sum of all vertical reaction forces on the indentor.
Compressive Force vs. Indentation
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Compressive Force vs. Indentation in the Label text field.
3
Locate the Title section. From the Title type list, choose Label.
Global 1
1
In the Compressive Force vs. Indentation toolbar, click  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
-solid.cnt1.T_toty/d
N/m
Without confined air
4
Click to expand the Coloring and Style section. In the Width text field, type 2.
Global 2
1
Right-click Global 1 and choose Duplicate.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Study: With Pressure/Solution 2 (sol2).
4
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
-solid.cnt1.T_toty/d
N/m
With confined air
Compressive Force vs. Indentation
1
In the Model Builder window, click Compressive Force vs. Indentation.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
Select the x-axis label check box.
4
Select the y-axis label check box.
5
In the x-axis label text field, type Indentation (mm).
6
In the y-axis label text field, type Force (N/mm).
7
Locate the Legend section. From the Position list, choose Upper left.
Compare with the plot shown in Figure 6.