*3.2.2 Material properties and modeling*

Material properties need to be input into Abaqus during this simulation step, each component should have the following material property data including hardness, density, stress, strain, Young's modulus, mu, Kappa, C10, and D1. **Table 2** exhibits the full material properties of all tyre components under study.

A model that represents the stress–strain relationship of the material is needed in finite element analyses of rubber components. There are several material models available In Abaqus to describe the mechanical behavior of rubber. The model to be

**Figure 3.** *Tyre meshing of axisymmetric model in Abaqus [7].*

**Figure 4.** *Pressurized axisymmetric (left) and full axisymmetric Tyre model (right).*

used in the analyses depends on several factors such as availability of experimental data, strain range, and complexity of loading.

Each tyre component shows different deformation response under external loading. Rubber exhibits non linear deformation and almost incompressible response, while fabric cords and steel wire withstand most both tension and compressions loads and therefore produce small strain. For rubber, hyper-elastic material models are used to describe high deformation. In this study, Yeoh's model was chosen to define hyperelastic property of rubber materials and Marlow model for reinforcements such as fabric and steel cords. Bead was modeled as an elastic material.

The Yeoh material model had a cubic form with only *I1* dependence and is applicable to purely incompressible materials. The strain energy density for Yeoh model is written as

$$\mathcal{W} = \sum\_{i=1}^{3} \mathcal{C}\_{i} (I\_{1} - \mathbf{3})^{i} \tag{2}$$

where *Ci* are material constants. *Ci* quantity is 0.5 of the initial shear modulus.

The reason for using the Yeoh's model in the rubber material model, despite the fact that Abaqus supports other material models like Neo-Hookean and Mooney-Rivlin, because it is capable of predicting different deformation modes using data from a simple deformation mode like uni-axial tension test. A review by Wei et al. [8] found that most of material models are determined based on the polynomial expression of strain energy function. Although Mooney-Rivlin energy density function has been widely applied for tyre dynamic properties analysis, the function has a limitation that it could not be accurately applied to large deformation problems of the rubber material. Neo-Hookean material model also has a limitation that the coefficients derived from uni-axial deformation tests are not suitable to describe other deformation modes. In order to determine the parameters of rubber hyperelastic property, most of the material models need to combine three deformation tests (uni-axial, biaxial tension and pure shear), which is recognized as a complex and time consuming procedure.


**Table 2.** *Material properties.* *Rolling Resistance Estimation for PCR Tyre Design Using the Finite Element Method DOI: http://dx.doi.org/10.5772/intechopen.94144*

#### *3.2.3 Footprint and radial stiffness analysis*

After completing the axisymmetric tyre modeling, the next step is the simulation of tyre under static loading. From this simulation there are two analyses can be further performed: footprint analysis and radial stiffness analysis. For footprint analysis, the load needs to be applied on the tyre to represent the normal load according to the specified load index of the tyre. **Figure 5** shows the tyre under static loading and its respective footprint result.

For designing a new PCR tyre, there are three different tyre were taken for benchmark. The tyre being simulated is of the size 175/65 R14 and were inflated at 2.1 bar (30.5 psi) with various loads of 100 kg, 150 kg, and 200 kg using three types of tyre, called tyre A, tyre B, and tyre C. Tyre A has two grooves, tyre B has three grooves, and tyre C has four grooves.

To obtain more accurate footprint result, the full tyre with tread was modeled so that the contact pressure distribution on the tread which in contact with the road can be evaluated. **Figure 6** exhibits the footprint comparison of these three tyres.

In Abaqus, footprint simulation is performed under static loading and needs several input files for defining geometry, boundary condition, sequence and load of tyre and rim. The result of Abaqus footprint analysis as it is shown in **Figure 6**, suggests that the tyre having two grooves shows the largest contact area at shoulder. Large contact area on shoulder indicates better cornering stability.

The second simulation result is about radial stiffness of the tyre. The radial stiffness mainly depends on sidewall stiffness and affects the transversal bending of tyre. This transversal bending causes the tyre to lose its height by certain value, from initial radius *R* becomes deflected radius *Rdef*, as shown in **Figure 7**.

The *Rdef* resulted from simulation of two groove tyre is the largest (see **Table 3**), that means that its radial stiffness is also the largest. Larger radial stiffness gives more cornering stability.

By looking at footprint and radial stiffness, the two groove tyre indicates a better cornering stability compared to the other tyre types.

**Figure 5.** *Footprint simulation under static loading.*

