PDF
Tire Inflation
Introduction
Tires play a fundamental structural role in vehicle dynamics by transmitting loads to the ground, thus making it possible for traction and brake to develop. At the same time, tires must contribute to limit the effect of road irregularity, concurring to the overall vibration isolation capability of the vehicle. These two functions require modern tires to have substantial structural loading capability, while at the same time being compliant enough to provide better comfort with respect to a solid wheel. A tire is thus a complicated composite made of various types of soft rubber locally reinforced by stiff cords usually made by steel and nylon.
Tire simulation requires the use of appropriate nonlinear anisotropic constitutive models to describe the rubber behavior with the inclusion of the effect of the cord reinforcements. This model showcases how to use fibers in thin layers to model thin anisotropic composites embedded in a solid without explicitly drawing either the layer of material or the reinforcing fibers. In particular, this is used to model steel cords in tire belts that are used to provide structural support to the tire below the treads. Moreover, a curvilinear coordinate system is used to define the anisotropic material properties of the carcass ply.
Model Definition
Both the geometry of the tire and the applied loads during inflation show axial symmetry. For this reason, you do not need to model the entire three dimensional tire, but a 2D axisymmetric model can be used to save computational time. Moreover, a plane of symmetry can be identified for the tire cross section. Figure 1 illustrates a simplified geometry of half of the cross section of a tire, along with the cross section of the rim in the locations where it enters in contact with the tire.
Note that when exploiting symmetries for reducing the computational cost in simulations care must be taken to check that the material properties show the same symmetry as exhibited by loads and geometry.
In the case of tires, the orientation of cords in the reinforcing plies usually induces displacements that have non zero components in the azimuthal direction, and that are not symmetric with respect to the plane of symmetry of the geometry. COMSOL Multiphysics provides a specific formulation for the 2D axisymmetric problem that allows to include the azimuthal “twist” without the need to switch to a full 3D model.
For what concerns the lack of symmetry with respect to the midplane of the cross section, it can be shown that by using an antisymmetry condition for the circumferential displacement on the symmetry plane of the geometry, the difference in the solution obtained with respect to the one computed with a full cross section is very small.
In Figure 1 different colors have been used to highlight different domains, based on the material properties used.
Figure 1: Geometry of the tire and rim cross sections.
The following modeling assumptions have been made:
•
Sidewall and tread are assumed to be made by the same material, modeled with the Yeoh hyperelastic constitutive law.
•
Bead wires are modeled as a single uniform steel domain.
•
Bead filler can be also modeled with the Yeoh hyperelastic material modeled.
•
The carcass is modeled using a linear elastic, transversely isotropic material model, that captures in a homogenized way the nylon and steel reinforcements.
•
The three belts are modeled as thin hyperelastic layers made by the same rubber as the sidewall and tread, with embedded steel cords.
•
The rim is considered to be rigid.
The material properties for each material domain are collected in Table 1 (Ref. 1 and Ref. 2).
Table 1: Material properties.
Material properties
Sidewall and tread
Bead
Carcass
 c1
1 MPa
1.6 MPa
-
 c2
-0.3 MPa
-1.4 MPa
-
 c3
0.1 MPa
0.9 MPa
-
 K
100 MPa
100 MPa
-
 E1
-
-
7 GPa
 E2
-
-
25 MPa
 ν1
-
-
0.45
 ν2
-
-
0.4
 G
-
-
4 MPa
Table 2 collects the orientation of the cords in each belt with respect to the azimuthal direction. The orientation of the cords, along with the first principal direction of the transversely isotropic material used for the carcass are represented in Figure 2.
The tire is inflated to reach an inner pressure of 2 bar.
Table 2: orientation of cords.
Belt 1
Belt 2
Belt 3
+20°
-20°
0°
Figure 2: Cords orientation.
Results and Discussion
Figure 3 shows the twist displacement in the tire, and Figure 4 shows the von Mises stress in the cords and in the bead wires.
Figure 3: Azimuthal displacement.
Figure 4: The von Mises stress at the end of inflation.
Notes About the COMSOL Implementation
•
You find the Include circumferential displacement checkbox in the Axial Symmetry Approximation section in the settings window of the Solid Mechanics interface. This allows you to enable the 2D axisymmetric formulation that includes the twist degree of freedom.
•
You can add a Initial Stress and Strain node under Linear Elastic Material to model the prestress in the bead wires, resulting after the mounting of the tire on the rim.
•
You can use a Curvilinear Coordinates interface to compute the direction of anisotropy in the carcass.
•
To model the belts without explicitly drawing their thickness, you can simply add a Thin Layer and add a Hyperelastic Material to it. Use the Solid approximation to create a slit for the displacement variable at the selected boundary.
•
Add three Fiber nodes to the Hyperelastic Material under the Thin Layer in order to model the three different orientations of the cords. You can directly specify the orientation with respect to the boundary coordinate system without further computations. Choose a Linear elastic material model for the cords, to model steel.
•
You find the Antisymmetry option under the Circumferential Condition section when you add the Symmetry Plane.
References
1. T. Király, P. Primusz and C. Tóth, “Simulation of Static Tyre-Pavement Interaction Using Two FE Models of Different Complexity,” Appl. Sci., vol. 12, no. 5, p. 2388, 2022.
2. H.S. Aldhufairi, O. Olatunbosun, and K. Essa, “Determination of a Tyre’s Rolling Resistance Using Parallel Rheological Framework,” SAE Technical Paper, no. 2019-01-5069, 2019.
Application Library path: Nonlinear_Structural_Materials_Module/Hyperelasticity/tire_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.
Geometry 1
First, import the geometry of the tire cross section and the geometry of the rim.
Tire Section
1
In the Model Builder window, right-click Global Definitions and choose Geometry Parts > 2D Part.
2
In the Settings window for Part, type Tire Section in the Label text field.
Import 1 (imp1)
1
In the Home toolbar, click  Import.
2
In the Settings window for Import, locate the Source section.
3
Click  Browse.
4
Browse to the model’s Application Libraries folder and double-click the file tire_inflation.mphbin.
5
In the Home toolbar, click  Build All.
Tire Section
In the Model Builder window, collapse the Global Definitions > Geometry Parts > Tire Section node.
Rim
1
In the Model Builder window, under Global Definitions right-click Geometry Parts and choose 3D Part.
2
In the Settings window for Part, type Rim in the Label text field.
3
Locate the Advanced section. From the Geometry representation list, choose CAD kernel.
4
In the Geometry toolbar, click  Import.
1
In the Settings window for Import, locate the Source section.
2
Click  Browse.
3
Browse to the model’s Application Libraries folder and double-click the file wheel_rim.x_b.
4
In the Geometry toolbar, click  Build All.
Rim
In the Model Builder window, collapse the Global Definitions > Geometry Parts > Rim node.
Generate the 2D axisymmetric geometry.
2D Axisymmetric [Tire]
1
In the Model Builder window, click Component 1 (comp1).
2
In the Settings window for Component, type 2D Axisymmetric [Tire] in the Label text field.
Geometry 1
1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose cm.
Tire Section 1 (pi1)
1
In the Geometry toolbar, click  Part Instance and choose Tire Section.
2
In the Settings window for Part Instance, click  Build Selected.
In order to add the rim to the 2D axisymmetric component, you need to create a cross section of the 3D geometry.
Add Component
Right-click Tire Section 1 (pi1) and choose 3D.
3D [Rim]
In the Settings window for Component, type 3D [Rim] in the Label text field.
Geometry 2
1
In the Model Builder window, under 3D [Rim] (comp2) click Geometry 2.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose cm.
4
Locate the Advanced section. From the Geometry representation list, choose CAD kernel.
Rim 1 (pi1)
1
In the Geometry toolbar, click  Part Instance and choose Rim.
2
In the Settings window for Part Instance, click  Build Selected.
Set the plane of the cross section.
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Plane Definition section.
3
From the Plane list, choose xz-plane.
4
Click  Build Selected.
Geometry 1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) click Geometry 1.
Cross Section 1 (cro1)
1
In the Geometry toolbar, click  Cross Section.
2
In the Settings window for Cross Section, click  Build Selected.
3
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 cro1, select Domains 1–3 only.
5
Click  Build Selected.
6
Click the  Zoom Extents button in the Graphics toolbar.
Only half of the domain will be included in the study by adopting a symmetry boundary condition. Modify the geometry accordingly.
Line Segment 1 (ls1)
1
In the Geometry toolbar, click  More Primitives and choose Line Segment.
2
On the object pi1, select Point 80 only.
3
In the Settings window for Line Segment, locate the Endpoint section.
4
From the Specify list, choose Coordinates.
5
In the r text field, type 20.
6
In the z text field, type -7E-2.
7
Click  Build Selected.
Partition Objects 1 (par1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Partition Objects.
2
Select the objects del1 and pi1 only.
3
In the Settings window for Partition Objects, locate the Partition Objects section.
4
Click to select the  Activate Selection toggle button for Tool objects.
5
Select the object ls1 only.
6
Click  Build Selected.
Delete Entities 2 (del2)
1
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
Click the  Select Box button in the Graphics toolbar.
5
On the object par1(1), select Domain 1 only.
6
On the object par1(2), select Domains 1, 2, 6, 8, and 10 only.
7
Click  Build Selected.
8
Click the  Zoom Extents button in the Graphics toolbar.
Add now mesh control edges, needed later on in order to mesh properly the component.
Import 1 (imp1)
1
In the Geometry toolbar, click  Import.
2
In the Settings window for Import, locate the Source section.
3
Click  Browse.
4
Browse to the model’s Application Libraries folder and double-click the file tire_inflation_meshcontrol.mphbin.
5
Click to expand the Selections of Resulting Entities section. Select the Resulting objects selection checkbox.
6
From the Show in physics list, choose Boundary selection.
7
Click  Build Selected.
8
Click the  Zoom Extents button in the Graphics toolbar.
Union 1 (uni1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Union.
2
Select the objects del2(2) and imp1 only.
3
In the Settings window for Union, click  Build Selected.
An assembly is needed between the rim and the tire, in order to set properly the contact between them.
Form Union (fin)
1
In the Model Builder window, under 2D Axisymmetric [Tire] (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 checkbox.
5
Click  Build Selected.
Mesh Control Edges 1 (mce1)
1
In the Geometry toolbar, click  Virtual Operations and choose Mesh Control Edges.
2
In the Settings window for Mesh Control Edges, locate the Input section.
3
From the Edges to include list, choose Import 1.
4
Click  Build Selected.
5
Click the  Zoom Extents button in the Graphics toolbar.
Set the contact pair between rim and tire.
Definitions (comp1)
Contact Pair 1 (p1)
1
In the Model Builder window, expand the 2D Axisymmetric [Tire] (comp1) > Definitions node.
2
Right-click 2D Axisymmetric [Tire] (comp1) > Definitions and choose Pairs > Contact Pair.
3
Select Boundaries 7, 8, and 10 only.
4
Click the  Zoom Extents button in the Graphics toolbar.
5
In the Settings window for Pair, locate the Destination Boundaries section.
6
Click to select the  Activate Selection toggle button.
7
Select Boundaries 30, 31, 44, and 46 only.
Add material properties.
Global Definitions
Steel [Bead Wires]
1
In the Model Builder window, under Global Definitions right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Steel [Bead Wires] in the Label text field.
3
Click to expand the Material Properties section. In the Material properties tree, select Basic Properties > Young’s Modulus.
4
Click  Add to Material.
5
In the Material properties tree, select Basic Properties > Poisson’s Ratio.
6
Click  Add to Material.
7
In the Material properties tree, select Basic Properties > Density.
8
Click  Add to Material.
9
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
210[GPa]
Pa
Basic
Poisson’s ratio
nu
0.3
1
Basic
Density
rho
7800[kg/m^3]
kg/m³
Basic
Steel [Cords]
1
Right-click Steel [Bead Wires] and choose Duplicate.
2
In the Settings window for Material, type Steel [Cords] in the Label text field.
3
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
170[GPa]
Pa
Basic
Rubber [Sidewall and Tread]
1
In the Model Builder window, right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Rubber [Sidewall and Tread] in the Label text field.
3
Click to expand the Material Properties section. In the Material properties tree, select Solid Mechanics > Hyperelastic Material > Yeoh.
4
Click  Add to Material.
5
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Model parameters
c1YE
1[MPa]
Pa
Yeoh
Model parameters
c2YE
-0.3[MPa]
Pa
Yeoh
Model parameters
c3YE
0.1[MPa]
Pa
Yeoh
6
Locate the Material Properties section. In the Material properties tree, select Solid Mechanics > Linear Elastic Material > Bulk Modulus and Shear Modulus > Bulk modulus (K).
7
Click  Add to Material.
8
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Bulk modulus
K
100[MPa]
N/m²
Bulk modulus and shear modulus
9
Locate the Material Properties section. In the Material properties tree, select Basic Properties > Density.
10
Click  Add to Material.
11
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Density
rho
1100[kg/m^3]
kg/m³
Basic
Rubber [Bead]
1
Right-click Rubber [Sidewall and Tread] and choose Duplicate.
2
In the Settings window for Material, type Rubber [Bead] in the Label text field.
3
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Model parameters
c1YE
1.6[MPa]
Pa
Yeoh
Model parameters
c2YE
-1.4[MPa]
Pa
Yeoh
Model parameters
c3YE
0.9[MPa]
Pa
Yeoh
Reinforced Rubber [Carcass]
1
In the Model Builder window, right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Reinforced Rubber [Carcass] in the Label text field.
3
Click to expand the Material Properties section. In the Material properties tree, select Solid Mechanics > Linear Elastic Material > Transversely Isotropic.
4
Click  Add to Material.
5
In the Material properties tree, select Basic Properties > Density.
6
Click  Add to Material.
7
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Density
rho
1750[kg/m^3]
kg/m³
Basic
Young’s modulus
{Evect1, Evect2}
{7[GPa],25[MPa]}
Pa
Transversely isotropic
Poisson’s ratio
{nuvect1, nuvect2}
{0.45, 0.4}
1
Transversely isotropic
Shear modulus
Gvect1
4[MPa]
N/m²
Transversely isotropic
Assign material properties to domains.
Materials
Material Link: Steel [Bead Wires]
1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) right-click Materials and choose More Materials > Material Link.
2
In the Settings window for Material Link, type Material Link: Steel [Bead Wires] in the Label text field.
3
Locate the Geometric Entity Selection section. Click  Clear Selection.
4
Select Domain 7 only.
5
Click  Create Selection.
6
In the Create Selection dialog, type Bead Wires in the Selection name text field.
7
Click OK.
8
In the Settings window for Material Link, click to expand the Appearance section.
9
From the Material type list, choose Steel.
Material Link: Rubber [Sidewall and Tread]
1
Right-click Materials and choose More Materials > Material Link.
2
In the Settings window for Material Link, locate the Link Settings section.
3
From the Material list, choose Rubber [Sidewall and Tread] (mat3).
4
In the Label text field, type Material Link: Rubber [Sidewall and Tread].
5
Select Domains 2, 3, and 5 only.
6
Locate the Geometric Entity Selection section. Click  Create Selection.
7
In the Create Selection dialog, type Sidewall and Tread in the Selection name text field.
8
Click OK.
9
In the Settings window for Material Link, click to expand the Appearance section.
10
From the Material type list, choose Rubber.
11
From the Color list, choose Black.
Material Link: Rubber [Bead]
1
Right-click Materials and choose More Materials > Material Link.
2
In the Settings window for Material Link, type Material Link: Rubber [Bead] in the Label text field.
3
Select Domain 6 only.
4
Locate the Link Settings section. From the Material list, choose Rubber [Bead] (mat4).
5
Locate the Geometric Entity Selection section. Click  Create Selection.
6
In the Create Selection dialog, type Bead Rubber in the Selection name text field.
7
Click OK.
8
In the Settings window for Material Link, click to expand the Appearance section.
9
From the Material type list, choose Rubber.
10
From the Color list, choose Black.
Material Link: Reinforced Rubber [Carcass]
1
Right-click Materials and choose More Materials > Material Link.
2
In the Settings window for Material Link, type Material Link: Reinforced Rubber [Carcass] in the Label text field.
3
Select Domain 4 only.
4
Locate the Link Settings section. From the Material list, choose Reinforced Rubber [Carcass] (mat5).
5
Locate the Geometric Entity Selection section. Click  Create Selection.
6
In the Create Selection dialog, type Carcass in the Selection name text field.
7
Click OK.
8
In the Settings window for Material Link, click to expand the Appearance section.
9
From the Color list, choose Gray.
Definitions (comp1)
Hyperelastic Domains
1
In the Definitions toolbar, click  Union.
2
In the Settings window for Union, type Hyperelastic Domains in the Label text field.
3
Locate the Input Entities section. Under Selections to add, click  Add.
4
In the Add dialog, in the Selections to add list, choose Sidewall and Tread and Bead Rubber.
5
Click OK.
Enclosing Boundaries
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Enclosing Boundaries in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 3, 5–7, 13, 30, 45, and 48 only.
Exclude the rim from Solid Mechanics, since it is modeled as a rigid boundary.
Solid Mechanics (solid)
1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) click Solid Mechanics (solid).
2
Select Domains 2–7 only.
Assign the hyperelastic material model to domains made of rubber.
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 Hyperelastic Domains.
4
Locate the Hyperelastic Material section. From the Material model list, choose Yeoh.
5
From the Compressibility list, choose Compressible, uncoupled.
Assign a transversely isotropic linear elastic material model to the tire carcass.
Linear Elastic Material [Carcass]
1
In the Physics toolbar, click  Domains and choose Linear Elastic Material.
2
In the Settings window for Linear Elastic Material, type Linear Elastic Material [Carcass] in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose Carcass.
4
Locate the Linear Elastic Material section. From the Material symmetry list, choose Orthotropic.
5
Select the Transversely isotropic checkbox.
Linear Elastic Material [Bead Wires]
1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
2
In the Settings window for Linear Elastic Material, type Linear Elastic Material [Bead Wires] in the Label text field.
Add a Curvilinear Coordinates physics interface in order to compute principal directions of anisotropy for the reinforced rubber.
Add Physics
1
In the Physics toolbar, click  Add Physics to open the Add Physics window.
2
Go to the Add Physics window.
3
In the tree, select Mathematics > Curvilinear Coordinates (cc).
4
Click the Add to 2D Axisymmetric [Tire] button in the window toolbar.
5
In the Physics toolbar, click  Add Physics to close the Add Physics window.
Curvilinear Coordinates (cc)
1
In the Settings window for Curvilinear Coordinates, locate the Domain Selection section.
2
From the Selection list, choose Carcass.
3
Locate the Settings section. Select the Create base vector system checkbox.
Diffusion Method 1
In the Physics toolbar, click  Domains and choose Diffusion Method.
Inlet 1
1
In the Physics toolbar, click  Attributes and choose Inlet.
2
Select Boundary 21 only.
Diffusion Method 1
In the Model Builder window, click Diffusion Method 1.
Outlet 1
1
In the Physics toolbar, click  Attributes and choose Outlet.
2
Select Boundary 17 only.
Solid Mechanics (solid)
Linear Elastic Material [Carcass]
1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) > Solid Mechanics (solid) click Linear Elastic Material [Carcass].
2
In the Settings window for Linear Elastic Material, locate the Coordinate System Selection section.
3
From the Coordinate system list, choose Curvilinear System (cc) (cc_cs).
Define geometric parameters of the belts’ cord reinforcements.
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
dcord_belts
0.5[mm]
5E-4 m
Diameter of belt cords
spcord_belts
1.16[mm]
0.00116 m
Spacing between belt cords
alpha_belt
70[deg]
1.2217 rad
Angle of belt cords
Add the belts.
Solid Mechanics (solid)
Thin Layer 1
1
In the Physics toolbar, click  Boundaries and choose Thin Layer.
2
Select Boundaries 57–59 only.
3
In the Settings window for Thin Layer, locate the Boundary Selection section.
4
Click  Create Selection.
5
In the Create Selection dialog, type Belts in the Selection name text field.
6
Click OK.
7
In the Settings window for Thin Layer, locate the Boundary Properties section.
8
In the Lth text field, type dcord_belts.
Hyperelastic Material 1
1
In the Physics toolbar, click  Attributes and choose Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, locate the Boundary Selection section.
3
From the Selection list, choose Belts.
4
Locate the Hyperelastic Material section. From the Material model list, choose Yeoh.
5
From the Compressibility list, choose Compressible, uncoupled.
Materials
Material Link: Rubber [Belts]
1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) > Materials right-click Material Link: Rubber [Sidewall and Tread] (matlnk2) and choose Duplicate.
2
In the Settings window for Material Link, type Material Link: Rubber [Belts] in the Label text field.
3
Locate the Geometric Entity Selection section. From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Belts.
Solid Mechanics (solid)
Hyperelastic Material 1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) > Solid Mechanics (solid) > Thin Layer 1 click Hyperelastic Material 1.
Fiber [Cords, Belt 1]
1
In the Physics toolbar, click  Attributes and choose Fiber.
2
In the Settings window for Fiber, type Fiber [Cords, Belt 1] in the Label text field.
3
Locate the Fiber Model section. From the Material model list, choose Linear elastic.
4
From the Material list, choose Steel [Cords] (mat2).
5
Locate the Distribution and Orientation section. From the a list, choose User defined.
6
Specify the Direction vector as
cos(alpha_belt)
t1
sin(alpha_belt)
to
7
In the dfiber text field, type dcord_belts.
8
In the sfiber text field, type spcord_belts.
9
Locate the Boundary Selection section. Click  Clear Selection.
10
Select Boundary 57 only.
11
Click  Create Selection.
12
In the Create Selection dialog, type Belt 1 in the Selection name text field.
13
Click OK.
Fiber [Cords, Belt 2]
1
Right-click Fiber [Cords, Belt 1] and choose Duplicate.
2
In the Settings window for Fiber, type Fiber [Cords, Belt 2] in the Label text field.
3
Locate the Boundary Selection section. Click  Clear Selection.
4
Select Boundary 58 only.
5
Click  Create Selection.
6
In the Create Selection dialog, type Belt 2 in the Selection name text field.
7
Click OK.
8
In the Settings window for Fiber, locate the Distribution and Orientation section.
9
Specify the Direction vector as
-cos(alpha_belt)
t1
Fiber [Cords, Belt 3]
1
Right-click Fiber [Cords, Belt 2] and choose Duplicate.
2
In the Settings window for Fiber, type Fiber [Cords, Belt 3] in the Label text field.
3
Locate the Boundary Selection section. Click  Clear Selection.
4
Select Boundary 59 only.
5
Click  Create Selection.
6
In the Create Selection dialog, type Belt 3 in the Selection name text field.
7
Click OK.
8
In the Settings window for Fiber, locate the Distribution and Orientation section.
9
From the a list, choose Second axis.
Thin Layer 1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) > Solid Mechanics (solid) click Thin Layer 1.
Roller 1
1
In the Physics toolbar, click  Attributes and choose Roller.
2
Select Points 46, 48, and 49 only.
Because of the orientation of the fibers, the circumferential displacement will not be zero.
3
In the Model Builder window, click Solid Mechanics (solid).
4
In the Settings window for Solid Mechanics, locate the Axial Symmetry Approximation section.
5
Select the Include circumferential displacement checkbox.
Set the prestress in the bead wires.
Linear Elastic Material [Bead Wires]
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) > Solid Mechanics (solid) click Linear Elastic Material [Bead Wires].
Initial Stress and Strain 1
1
In the Physics toolbar, click  Attributes and choose Initial Stress and Strain.
2
In the Settings window for Initial Stress and Strain, locate the Initial Stress and Strain section.
3
Specify the S0 matrix as
0
0
0
0
300[MPa]
0
0
0
0
Contact 1
1
In the Model Builder window, under 2D Axisymmetric [Tire] (comp1) > Solid Mechanics (solid) click Contact 1.
2
In the Settings window for Contact, locate the Contact Pressure Penalty Factor section.
3
From the Penalty factor control list, choose Manual tuning.
4
In the fp text field, type 2.
Set up the inner pressure.
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
p0
200[kPa]
2E5 Pa
Inflation pressure
para
0
0
Continuation parameter for inflation
Solid Mechanics (solid)
Enclosed Cavity 1
1
In the Physics toolbar, click  Boundaries and choose Enclosed Cavity.
Select the Enclosing Boundaries to define the tire volume. Notice that the rim boundaries, which are not included in the Solid Mechanics interface, will be marked as "not applicable". These boundaries have to be explicitly allowed.
2
In the Settings window for Enclosed Cavity, locate the Boundary Selection section.
3
From the Selection list, choose Enclosing Boundaries.
4
Click to expand the Advanced section. Select the Include boundaries external to current physics checkbox.
When including external boundaries, a normal direction has to be specified. By convention, the normal for external boundaries has to point toward the fluid. In this case, the normal of the referenced default boundary system is oriented correctly.
5
Locate the Volume Definition section. From the Volume type list, choose Open surface.
6
Locate the Reference Point section. Click to select the  Activate Selection toggle button.
7
Select Point 4 only.
8
Locate the Volume Definition section. In the fV text field, type 2.
Remove the Fluid node, and use a Prescribed Pressure node instead to apply a known pressure load on the tire boundary.
Fluid 1
In the Model Builder window, right-click Fluid 1 and choose Delete.
Prescribed Pressure 1
1
In the Physics toolbar, click  Attributes and choose Prescribed Pressure.
2
In the Settings window for Prescribed Pressure, locate the Prescribed Pressure section.
3
In the p text field, type if(solid.incontact, 0, p0*para).
Set up the symmetry plane.
Symmetry Plane 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry Plane.
2
Click the  Select Box button in the Graphics toolbar.
3
Select Boundaries 20–23, 25, and 26 only.
4
In the Settings window for Symmetry Plane, locate the Circumferential Condition section.
5
From the list, choose Antisymmetry.
Set up the mesh.
Mesh 1
Free Quad 1
1
In the Mesh toolbar, click  Free Quad.
2
In the Settings window for Free Quad, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 2–4, 8, and 19 only.
5
Click to expand the Control Entities section. From the Smooth across removed control entities list, choose Off.
Distribution 1
1
Right-click Free Quad 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
Select Boundaries 15, 95, and 96 only.
Distribution 2
1
In the Model Builder window, right-click Free Quad 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
From the Distribution type list, choose Predefined.
4
Select Boundaries 55, 56, and 70 only.
5
In the Number of elements text field, type 6.
6
In the Element ratio text field, type 1.2.
7
From the Growth rate list, choose Exponential.
Distribution 3
1
Right-click Free Quad 1 and choose Distribution.
2
Select Boundary 45 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
From the Distribution type list, choose Predefined.
5
In the Number of elements text field, type 15.
6
In the Element ratio text field, type 1.4.
7
From the Growth rate list, choose Exponential.
8
Select the Reverse direction checkbox.
Distribution 4
1
Right-click Distribution 3 and choose Duplicate.
2
Select Boundary 71 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Element ratio text field, type 1.6.
5
Clear the Reverse direction checkbox.
Distribution 5
1
Right-click Distribution 4 and choose Duplicate.
2
Select Boundary 72 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Element ratio text field, type 1.8.
Distribution 6
1
In the Model Builder window, right-click Free Quad 1 and choose Distribution.
2
Select Boundary 63 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 6.
5
Select Boundaries 42–44, 51, 52, and 63 only.
Distribution 7
1
Right-click Free Quad 1 and choose Distribution.
2
Select Boundaries 34 and 37 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 2.
Distribution 8
1
Right-click Free Quad 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
From the Distribution type list, choose Predefined.
4
In the Element ratio text field, type 1.5.
5
Select Boundary 30 only.
Distribution 9
1
Right-click Free Quad 1 and choose Distribution.
2
Select Boundaries 32 and 35 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 3.
Distribution 10
1
Right-click Free Quad 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
From the Distribution type list, choose Predefined.
4
In the Number of elements text field, type 10.
5
In the Element ratio text field, type 1.5.
6
From the Growth rate list, choose Exponential.
7
Select the Symmetric distribution checkbox.
8
Select Boundaries 31, 33, and 36 only.
Distribution 11
1
Right-click Free Quad 1 and choose Distribution.
2
Select Boundaries 46, 53, and 54 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
From the Distribution type list, choose Predefined.
5
In the Number of elements text field, type 10.
6
In the Element ratio text field, type 5.
7
From the Growth rate list, choose Exponential.
8
Click  Build All.
Refine 1
1
In the Mesh toolbar, click  Modify and choose Refine.
2
In the Settings window for Refine, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 2–4 only.
5
Click  Build Selected.
Mapped 1
1
In the Mesh toolbar, click  Mapped.
2
In the Settings window for Mapped, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Click  Paste Selection.
5
In the Paste Selection dialog, type 5, 9-18, 21-37, 39-45 in the Selection text field.
6
Click OK.
7
In the Settings window for Mapped, click to expand the Control Entities section.
8
From the Smooth across removed control entities list, choose Off.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundaries 24, 26, 27, 50, and 59–62 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 2.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 3.
4
Select Boundary 49 only.
Distribution 3
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundary 47 only.
Distribution 4
1
Right-click Mapped 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
Select Boundaries 101–103 only.
Distribution 5
1
Right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 12.
4
Select Boundary 131 only.
Distribution 6
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundary 130 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
From the Distribution type list, choose Predefined.
5
In the Number of elements text field, type 12.
6
In the Element ratio text field, type 1.2.
7
From the Growth rate list, choose Exponential.
8
Select the Reverse direction checkbox.
9
Click  Build Selected.
Mapped 2
1
In the Mesh toolbar, click  Mapped.
2
In the Settings window for Mapped, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 38 only.
5
Locate the Control Entities section. From the Smooth across removed control entities list, choose Off.
Free Triangular 1
1
In the Mesh toolbar, click  Free Triangular.
2
In the Settings window for Free Triangular, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 7 and 20 only.
5
Click to expand the Control Entities section. From the Smooth across removed control entities list, choose Off.
Size
1
In the Model Builder window, click Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extra coarse.
Size 1
1
In the Model Builder window, right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Coarser.
4
Click  Build Selected.
Free Triangular 2
1
In the Mesh toolbar, click  Free Triangular.
2
In the Settings window for Free Triangular, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 6 only.
Edge 1
1
In the Mesh toolbar, click  More Generators and choose Edge.
2
Select Boundaries 8, 10, and 31 only.
3
In the Settings window for Edge, locate the Boundary Selection section.
4
In the list box, select 31.
5
Click  Remove from Selection.
6
Select Boundaries 8, 10, and 30 only.
7
In the list box, select 30.
8
Click  Remove from Selection.
9
Select Boundaries 7, 8, and 10 only.
Size 1
1
Right-click Edge 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely fine.
4
Click the Custom button.
5
Locate the Element Size Parameters section.
6
Select the Maximum element size checkbox. In the associated text field, type 0.05.
7
Click  Build Selected.
Free Triangular 3
In the Mesh toolbar, click  Free Triangular.
Size 1
1
Right-click Free Triangular 3 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely coarse.
4
Click  Build All.
Mesh 2
1
In the Model Builder window, click Mesh 2.
2
In the Geometry Cleanup dialog that opens, click Clean up Automatically to automatically clean up the geometry.
Refine the mesh for the 3D rim to improve visualization.
3
In the Model Builder window, click Mesh 2.
4
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
5
From the Element size list, choose Fine.
Study: Fiber Direction
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Study: Fiber Direction in the Label text field.
Step 1: Stationary
1
In the Model Builder window, under Study: Fiber Direction 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 checkbox.
4
In the tree, select 2D Axisymmetric [Tire] (comp1) > Definitions > Contact Pair 1 (p1).
5
Click  Disable.
6
In the tree, select 2D Axisymmetric [Tire] (comp1) > Solid Mechanics (solid), Controls spatial frame.
7
Click  Disable in Model.
8
In the Study toolbar, click  Compute.
Results
Coordinate System Surface 1
1
In the Model Builder window, expand the Coordinate system (cc) node, then click Coordinate System Surface 1.
2
In the Settings window for Coordinate System Surface, locate the Positioning section.
3
From the Placement list, choose Element centers.
4
In the Coordinate system (cc) toolbar, click  Plot.
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 the Add Study button in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study: Inflation
1
In the Settings window for Study, type Study: Inflation in the Label text field.
2
Locate the Study Settings section. Clear the Generate default plots checkbox.
Step 1: Stationary
1
In the Model Builder window, under Study: Inflation click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under 2D Axisymmetric [Tire] (comp1), clear the checkbox for Curvilinear Coordinates (cc).
4
Click to expand the Values of Dependent Variables section. Find the Values of variables not solved for subsection. From the Settings list, choose User controlled.
5
From the Method list, choose Solution.
6
From the Study list, choose Study: Fiber Direction, Stationary.
7
Click to expand the Study Extensions section. Select the Auxiliary sweep checkbox.
8
Click  Add.
9
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para (Continuation parameter for inflation)
range(0, 0.1, 1)
 
10
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 General > Displacement (m) 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
Displacement
m
mm
8
Click  Add Physical Quantity.
9
In the Physical Quantity dialog, select Solid Mechanics > Stress tensor (N/m^2) in the tree.
10
Click OK.
11
In the Settings window for Preferred Units, locate the Units section.
12
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Stress tensor
N/m^2
MPa
13
Click  Apply.
Use Result Templates to generate plots of the von Mises stress and the circumferential displacement.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study: Inflation/Solution 2 (sol2) > Solid Mechanics > Stress (solid).
4
Click the Add Result Template button in the window toolbar.
5
In the tree, select Study: Inflation/Solution 2 (sol2) > Solid Mechanics > Displacement (solid).
6
Click the Add Result Template button in the window toolbar.
7
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Stress (solid)
1
In the Settings window for 2D Plot Group, locate the Color Legend section.
2
Select the Show maximum and minimum values checkbox.
Surface 1
Change the range of the plot to highlight the stress in the carcass.
1
In the Model Builder window, expand the Stress (solid) node, then click Surface 1.
2
In the Settings window for Surface, click to expand the Range section.
3
Select the Manual color range checkbox.
4
In the Maximum text field, type 15.
5
In the Stress (solid) toolbar, click  Plot.
Modify the plot of displacements in order to show the circumferential component.
Out-of-Plane Displacement (solid)
1
In the Model Builder window, under Results click Displacement (solid).
2
In the Settings window for 2D Plot Group, type Out-of-Plane Displacement (solid) in the Label text field.
Surface 1
1
In the Model Builder window, expand the Out-of-Plane Displacement (solid) node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type v.
4
In the Out-of-Plane Displacement (solid) toolbar, click  Plot.
Tire Volume
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Tire Volume in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Inflation/Solution 2 (sol2).
4
Locate the Legend section. From the Position list, choose Upper left.
Global 1
1
Right-click Tire Volume 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 2D Axisymmetric [Tire] (comp1) > Solid Mechanics > Enclosed cavities > Enclosed Cavity 1 > solid.enc1.V - Total volume, deformed configuration - m³.
3
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
solid.enc1.V
l
Total volume, deformed configuration
4
Locate the x-Axis Data section. From the Parameter list, choose Expression.
5
In the Expression text field, type p0*para.
6
From the Unit list, choose bar.
7
Select the Description checkbox. In the associated text field, type Pressure.
Add revolution datasets to plot the stress in 3D.
8
In the Model Builder window, click Results.
9
In the Settings window for Results, locate the Update of Results section.
10
Select the Only plot when requested checkbox.
Revolution 2D: Tire
1
In the Results toolbar, click  More Datasets and choose Revolution 2D.
2
In the Settings window for Revolution 2D, type Revolution 2D: Tire in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Inflation/Solution 2 (sol2).
4
Click to expand the Revolution Layers section. In the Start angle text field, type -90.
5
In the Revolution angle text field, type 225.
Selection
1
Right-click Revolution 2D: Tire and choose Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 2–6 only.
Mirror 3D: Tire
1
In the Results toolbar, click  More Datasets and choose Mirror 3D.
2
In the Settings window for Mirror 3D, type Mirror 3D: Tire in the Label text field.
3
Locate the Plane Data section. From the Plane list, choose xy-planes.
4
In the z-coordinate text field, type -7E-2.
Stress, 3D (solid)
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Stress, 3D (solid) in the Label text field.
3
Locate the Data section. From the Dataset list, choose Mirror 3D: Tire.
4
Click to expand the Title section. From the Title type list, choose Manual.
5
In the Title text area, type von Mises stress (MPa).
6
In the Parameter indicator text field, type para=eval(para).
7
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
8
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
Tire
1
Right-click Stress, 3D (solid) and choose Volume.
2
In the Settings window for Volume, locate the Expression section.
3
In the Expression text field, type solid.misesGp.
4
Click to expand the Range section. Select the Manual color range checkbox.
5
In the Maximum text field, type 180.
6
Locate the Coloring and Style section. From the Color table list, choose Prism.
7
In the Label text field, type Tire.
Add a dedicated dataset for the bead wires.
Revolution 2D: Bead Wires
1
In the Model Builder window, right-click Revolution 2D: Tire and choose Duplicate.
2
In the Settings window for Revolution 2D, type Revolution 2D: Bead Wires in the Label text field.
3
Locate the Revolution Layers section. In the Revolution angle text field, type 275.
Selection
1
In the Model Builder window, expand the Revolution 2D: Bead Wires node, then click Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Selection list, choose Bead Wires.
Mirror 3D: Bead Wires
1
In the Model Builder window, right-click Mirror 3D: Tire and choose Duplicate.
2
In the Settings window for Mirror 3D, type Mirror 3D: Bead Wires in the Label text field.
3
Locate the Data section. From the Dataset list, choose Revolution 2D: Bead Wires.
Bead Wires
1
In the Model Builder window, right-click Tire and choose Duplicate.
2
In the Settings window for Volume, type Bead Wires in the Label text field.
3
Locate the Data section. From the Dataset list, choose Mirror 3D: Bead Wires.
4
From the Solution parameters list, choose From parent.
5
Click to expand the Inherit Style section. From the Plot list, choose Tire.
Generate dedicated revolution datasets also for the belts.
Revolution 2D: Belt 1
1
In the Model Builder window, right-click Revolution 2D: Bead Wires and choose Duplicate.
2
In the Settings window for Revolution 2D, type Revolution 2D: Belt 1 in the Label text field.
3
Locate the Revolution Layers section. In the Start angle text field, type 135.
4
In the Revolution angle text field, type 40.
5
From the Number of layers list, choose Fine.
Selection
1
In the Model Builder window, expand the Revolution 2D: Belt 1 node, then click Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Belt 1.
Mirror 3D: Belt 1
1
In the Model Builder window, right-click Mirror 3D: Bead Wires and choose Duplicate.
2
In the Settings window for Mirror 3D, type Mirror 3D: Belt 1 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Revolution 2D: Belt 1.
Use a Streamline Surface plot to show the cords in the belt.
Stress, 3D (solid)
In the Model Builder window, under Results click Stress, 3D (solid).
Belt 1
1
In the Stress, 3D (solid) toolbar, click  More Plots and choose Streamline Surface.
2
In the Settings window for Streamline Surface, type Belt 1 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Mirror 3D: Belt 1.
4
From the Solution parameters list, choose From parent.
5
Locate the Expression section. In the r-component text field, type solid.tl1.hmm1.fibt1.a0R*((mir1side*2)-1).
6
In the phi-component text field, type solid.tl1.hmm1.fibt1.a0PHI.
7
In the z-component text field, type solid.tl1.hmm1.fibt1.a0Z*((mir1side*2)-1).
8
Select Domain 5 only.
9
Locate the Streamline Positioning section. From the Positioning list, choose Uniform density.
10
In the Density level text field, type 7.7.
11
Locate the Coloring and Style section. Find the Line style subsection. From the Type list, choose Tube.
12
In the Tube radius expression text field, type solid.tl1.hmm1.fibt1.d/2.
13
Select the Radius scale factor checkbox. In the associated text field, type 2.
14
Click to expand the Inherit Style section. From the Plot list, choose Tire.
Color Expression 1
1
Right-click Belt 1 and choose Color Expression.
2
In the Settings window for Color Expression, locate the Expression section.
3
In the Expression text field, type solid.tl1.hmm1.fibt1.mises.
Revolution 2D: Belt 2
1
In the Model Builder window, right-click Revolution 2D: Belt 1 and choose Duplicate.
2
In the Settings window for Revolution 2D, type Revolution 2D: Belt 2 in the Label text field.
3
Locate the Revolution Layers section. In the Revolution angle text field, type 30.
Selection
1
In the Model Builder window, expand the Revolution 2D: Belt 2 node, then click Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Selection list, choose Belt 2.
Mirror 3D: Belt 2
1
In the Model Builder window, right-click Mirror 3D: Belt 1 and choose Duplicate.
2
In the Settings window for Mirror 3D, type Mirror 3D: Belt 2 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Revolution 2D: Belt 2.
Belt 2
1
In the Model Builder window, right-click Belt 1 and choose Duplicate.
2
In the Settings window for Streamline Surface, type Belt 2 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Mirror 3D: Belt 2.
4
Locate the Expression section. In the r-component text field, type solid.tl1.hmm1.fibt2.a0R*((mir1side*2)-1).
5
In the phi-component text field, type solid.tl1.hmm1.fibt2.a0PHI.
6
In the z-component text field, type solid.tl1.hmm1.fibt2.a0Z*((mir1side*2)-1).
7
Locate the Coloring and Style section. Find the Line style subsection. In the Tube radius expression text field, type solid.tl1.hmm1.fibt2.d/2.
Color Expression 1
1
In the Model Builder window, expand the Belt 2 node, then click Color Expression 1.
2
In the Settings window for Color Expression, locate the Expression section.
3
In the Expression text field, type solid.tl1.hmm1.fibt2.mises.
4
In the Stress, 3D (solid) toolbar, click  Plot.
Revolution 2D: Belt 3
1
In the Model Builder window, right-click Revolution 2D: Belt 2 and choose Duplicate.
2
In the Model Builder window, click Revolution 2D: Belt 2.1.
3
In the Settings window for Revolution 2D, type Revolution 2D: Belt 3 in the Label text field.
4
Locate the Revolution Layers section. In the Revolution angle text field, type 20.
Selection
1
In the Model Builder window, click Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Selection list, choose Belt 3.
Mirror 2D: Belt 3
1
In the Model Builder window, right-click Mirror 3D: Belt 2 and choose Duplicate.
2
In the Settings window for Mirror 3D, locate the Data section.
3
From the Dataset list, choose Revolution 2D: Belt 3.
4
In the Label text field, type Mirror 2D: Belt 3.
Belt 3
1
In the Model Builder window, right-click Belt 2 and choose Duplicate.
2
In the Settings window for Streamline Surface, type Belt 3 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Mirror 2D: Belt 3.
4
Locate the Expression section. In the r-component text field, type solid.tl1.hmm1.fibt3.a0R.
5
In the phi-component text field, type solid.tl1.hmm1.fibt3.a0PHI.
6
In the z-component text field, type solid.tl1.hmm1.fibt3.a0Z.
7
Locate the Streamline Positioning section. In the Density level text field, type 9.
8
From the Advanced parameters list, choose Manual.
9
In the Terminating distance factor text field, type 0.1.
10
Locate the Coloring and Style section. Find the Line style subsection. In the Tube radius expression text field, type solid.tl1.hmm1.fibt3.d/2.
Color Expression 1
1
In the Model Builder window, expand the Belt 3 node, then click Color Expression 1.
2
In the Settings window for Color Expression, locate the Expression section.
3
In the Expression text field, type solid.tl1.hmm1.fibt3.mises.
4
In the Stress, 3D (solid) toolbar, click  Plot.
Rim geometry
1
In the Model Builder window, under Results > Datasets right-click Study: Inflation/Solution 2 (sol2) and choose Duplicate.
2
In the Settings window for Solution, type Rim geometry in the Label text field.
3
Locate the Solution section. From the Component list, choose 3D [Rim] (comp2).
Rim
1
In the Model Builder window, right-click Stress, 3D (solid) and choose Surface.
2
In the Settings window for Surface, type Rim in the Label text field.
3
Locate the Data section. From the Dataset list, choose Rim geometry (sol2).
4
Locate the Expression section. In the Expression text field, type 1.
5
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
6
Click to expand the Quality section. From the Evaluation settings list, choose Manual.
7
From the Resolution list, choose Fine.
Material Appearance 1
1
Right-click Rim and choose Material Appearance.
2
In the Stress, 3D (solid) toolbar, click  Plot.
Material and Fiber Direction
1
In the Model Builder window, right-click Stress, 3D (solid) and choose Duplicate.
2
In the Model Builder window, click Stress, 3D (solid) 1.
3
In the Settings window for 3D Plot Group, type Material and Fiber Direction in the Label text field.
4
Locate the Title section. From the Title type list, choose None.
Tire
1
In the Model Builder window, click Tire.
2
In the Settings window for Volume, locate the Expression section.
3
In the Expression text field, type 1.
Material Appearance 1
1
Right-click Tire and choose Material Appearance.
2
In the Settings window for Material Appearance, locate the Appearance section.
3
From the Material list, choose Material Link: Rubber [Sidewall and Tread] (matlnk2).
4
In the Material and Fiber Direction toolbar, click  Plot.
Material Appearance 1
1
In the Model Builder window, right-click Bead Wires and choose Material Appearance.
2
In the Material and Fiber Direction toolbar, click  Plot.
Color Expression 1
1
In the Model Builder window, expand the Results > Material and Fiber Direction > Belt 1 node.
2
Right-click Color Expression 1 and choose Delete.
Belt 1
1
In the Settings window for Streamline Surface, locate the Inherit Style section.
2
From the Plot list, choose None.
3
Locate the Coloring and Style section. Find the Point style subsection. From the Color list, choose Custom.
4
On Windows, click the colored bar underneath, or — if you are running the cross-platform desktop — the Color button.
5
Click Define custom colors.
6
Set the RGB values to 253, 185, and 19, respectively.
7
Click Add to custom colors.
8
Click Show color palette only or OK on the cross-platform desktop.
Color Expression 1
1
In the Model Builder window, expand the Results > Material and Fiber Direction > Belt 2 node.
2
Right-click Color Expression 1 and choose Delete.
Belt 2
1
In the Settings window for Streamline Surface, locate the Inherit Style section.
2
From the Plot list, choose None.
3
Locate the Coloring and Style section. Find the Point style subsection. From the Color list, choose Custom.
4
On Windows, click the colored bar underneath, or — if you are running the cross-platform desktop — the Color button.
5
Click Define custom colors.
6
Set the RGB values to 54, 140, and 203, respectively.
7
Click Add to custom colors.
8
Click Show color palette only or OK on the cross-platform desktop.
Color Expression 1
1
In the Model Builder window, expand the Belt 3 node.
2
Right-click Color Expression 1 and choose Delete.
Belt 3
1
In the Settings window for Streamline Surface, locate the Inherit Style section.
2
From the Plot list, choose None.
3
Locate the Coloring and Style section. Find the Point style subsection. From the Color list, choose Custom.
4
On Windows, click the colored bar underneath, or — if you are running the cross-platform desktop — the Color button.
5
Click Define custom colors.
6
Set the RGB values to 166, 214, and 208, respectively.
7
Click Add to custom colors.
8
Click Show color palette only or OK on the cross-platform desktop.
Revolution 2D: Carcass
1
In the Model Builder window, right-click Revolution 2D: Belt 1 and choose Duplicate.
2
In the Model Builder window, click Revolution 2D: Belt 1.1.
3
In the Settings window for Revolution 2D, type Revolution 2D: Carcass in the Label text field.
4
Locate the Revolution Layers section. In the Revolution angle text field, type 50.
Selection
1
In the Model Builder window, click Selection.
2
Select Boundaries 35–37, 42, 52, 53, and 56 only.
Mirror 3D: Carcass
1
In the Model Builder window, right-click Mirror 3D: Belt 1 and choose Duplicate.
2
In the Settings window for Mirror 3D, type Mirror 3D: Carcass in the Label text field.
3
Locate the Data section. From the Dataset list, choose Revolution 2D: Carcass.
Carcass
1
In the Model Builder window, right-click Belt 1 and choose Duplicate.
2
In the Settings window for Streamline Surface, type Carcass in the Label text field.
3
Locate the Data section. From the Dataset list, choose Mirror 3D: Carcass.
4
Click Replace Expression in the upper-right corner of the Expression section. From the menu, choose 2D Axisymmetric [Tire] (comp1) > Curvilinear Coordinates > cc.e1R,cc.e1PHI,cc.e1Z - First basis vector.
5
Locate the Expression section. In the r-component text field, type cc.e1R*((mir1side*2)-1).
6
In the z-component text field, type cc.e1Z*((mir1side*2)-1).
7
Locate the Surface Selection section. Click to select the  Activate Selection toggle button.
8
Select Domain 4 only.
9
Locate the Streamline Positioning section. In the Density level text field, type 9.
10
Locate the Coloring and Style section. Find the Line style subsection. In the Tube radius expression text field, type dcord_belts/2.
11
Find the Point style subsection. From the Color list, choose Red.
12
In the Material and Fiber Direction toolbar, click  Plot.
13
Click  Plot.
14
In the Model Builder window, click Results.
15
In the Settings window for Results, locate the Update of Results section.
16
Clear the Only plot when requested checkbox.
Generate a dedicated view for the 3D plots.
View 3D 8
In the Model Builder window, under Results right-click Views and choose View 3D.
Camera
1
Click the  Show Grid button in the Graphics toolbar.
2
Click the  Show Axis Orientation button in the Graphics toolbar.
3
In the Model Builder window, expand the View 3D 8 node, then click Camera.
4
In the Settings window for Camera, in the Graphics window toolbar, clicknext to  Scene Light, then choose Ambient Occlusion.
5
In the Graphics window toolbar, clicknext to  Scene Light, then choose Direct Shadows.
6
In the Graphics window toolbar, clicknext to  Scene Light, then choose Outdoor.
7
In the Graphics window toolbar, clicknext to  Scene Light, then choose Floor Shadows.
8
Locate the Camera section. In the Zoom angle text field, type 5.
9
Locate the Position section. In the x text field, type -263.
10
In the y text field, type -195.
11
In the z text field, type 373.
12
Locate the Target section. In the x text field, type 0.78.
13
In the y text field, type 0.
14
In the z text field, type -0.04.
15
Locate the Up Vector section. In the x text field, type -0.7.
16
In the y text field, type 0.71.
17
In the z text field, type -0.12.
18
Locate the Center of Rotation section. In the x text field, type 0.78.
19
In the y text field, type -0.005.
20
In the z text field, type 0.044.
Material and Fiber Direction
1
In the Model Builder window, under Results click Material and Fiber Direction.
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
From the View list, choose View 3D 8.
4
In the Material and Fiber Direction toolbar, click  Plot.
5
Click the  Zoom Extents button in the Graphics toolbar.
Make the cords unaffected by lighting such that results remain clear to be read.
Visual Effects 1
1
In the Model Builder window, right-click Belt 1 and choose Visual Effects.
2
In the Settings window for Visual Effects, locate the Visual Effects section.
3
Clear the Affected by lighting checkbox.
4
Find the Ambient occlusion subsection. From the Mode list, choose Manual.
5
Clear the Casts shadows checkbox.
6
Clear the Receives shadows checkbox.
7
Find the Direct shadows subsection. From the Mode list, choose Manual.
8
Clear the Casts shadows checkbox.
9
Clear the Receives shadows checkbox.
10
Right-click Visual Effects 1 and choose Copy.
Visual Effects 1
In the Model Builder window, right-click Belt 2 and choose Paste Visual Effects.
Visual Effects 1
In the Model Builder window, right-click Belt 3 and choose Paste Visual Effects.
Visual Effects 1
1
In the Model Builder window, right-click Carcass and choose Paste Visual Effects.
2
In the Material and Fiber Direction toolbar, click  Plot.
Stress, 3D (solid)
1
In the Model Builder window, under Results click Stress, 3D (solid).
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
From the View list, choose View 3D 8.
4
In the Stress, 3D (solid) toolbar, click  Plot.
Visual Effects 1
In the Model Builder window, right-click Belt 1 and choose Paste Visual Effects.
Visual Effects 1
In the Model Builder window, right-click Belt 2 and choose Paste Visual Effects.
Visual Effects 1
In the Model Builder window, right-click Belt 3 and choose Paste Visual Effects.