COMSOL 6.4 - Stress and Modal Analysis of a Composite Wheel Rim

Stress and Modal Analysis of a Composite Wheel Rim

Nowadays, there is a trend to manufacture wheel rims using composite material instead of aluminum. The primary reason is to reduce the unsprung mass which leads to a faster response time and thus better acceleration, braking and cornering performances. Typically, a carbon fiber composite material is used to manufacture a composite wheel rim.

To understand and improve the design of a composite wheel rim, an example model is built in COMSOL. The example demonstrates the modeling of a wheel rim made up of a carbon–epoxy laminate.

The composite laminate has a different number of plies in different regions of the wheel rim. First, a stress analysis of the wheel rim is performed in which the rim is subjected to the inflation pressure and the tire load. In order to compute the modal response of the wheel rim, a prestressed eigenfrequency analysis is performed in which the rim is subjected to the rotating frame forces.

•

Introduction to the Composite Materials Module.

•

Optimizing Composite Wheel Rim Designs with COMSOL Multiphysics®.

Model Definition

The wheel rim geometry is shown in Figure 1.

Figure 1: Model geometry of a composite wheel rim.

The geometry consists of two main regions which have different laminate stacking sequences:

•

Rim region with a 16 layer laminate

•

Hub-spoke region with a 8 layer laminate

Stacking Sequence

A symmetric ply layup is considered in all the regions. The stacking sequence for the two regions is as follows:

•

Hub and spokes: [0/45/90/-45]s (Figure 2)

•

Rim: [[0/45/90/-45]s]2 (Figure 3)

Figure 2: Stacking sequence [0/45/90/-45]s in hub-spoke region.

Each ply is made up of carbon–epoxy material and has a thickness of 0.4 mm.

The normal vector orientations for the hub-spoke and rim regions are shown in Figure 4 and Figure 5, respectively. This is the direction in which layer stacking is interpreted from bottom to top. Note that the geometric surface (that is, the meshed boundary) represents the laminate’s top surface. This is defined using the corresponding setting in the Layered Material Link and Layered Material Stack nodes.

Figure 3: Stacking sequence [[0/45/90/-45]s]2 in rim region.

Figure 4: The normal vector on each hub and spokes boundary. This is the direction in which the layer stacking is interpreted from bottom to top.

Figure 5: The normal vector on each rim boundary. This is the direction in which the layer stacking is interpreted from bottom to top.

Material Properties

Each ply is made up of AS4/APC carbon–thermoplastic composite material. The AS4/APC carbon–thermoplastic is a built-in material in the material library. The transversely isotropic material properties (Young’s modulus, shear modulus, and Poisson’s ratio) are given in Table 1.

Table 1: Material properties of a lamina.
Material property	Value
ρ	1570 kg/m3
{E11, E22}	{138, 8.7} GPa
G12	5 GPa
{υ12, υ23}	{0.28, 0.45}

Finite Element Mesh

The structure is discretized using a free triangular mesh, as shown in Figure 6.

Figure 6: The finite element mesh for the wheel rim.

Constraints

•

Each bolt hole where the wheel rim is attached to the wheel hub is fixed.

Loads

Two types of analyses are performed:

•

Stationary analysis: This analysis is performed for the tire pressure and total load on the wheels. The overpressure is 2 bar = 200 kPa. The total load carried by the wheel corresponds to a weight of 1120 kg. It is applied as a pressure on the rim surfaces where the tire is in contact. Assume that the load distribution in the circumferential direction can be approximated as p = p0 cos ( 3 ϑ ), where ϑ is the angle from the point of contact between the road and the tire. The loaded area thus extends 30° in each direction from the load peak.

•

Prestressed Eigenfrequency analysis: This analysis is performed with rotating frame forces when the wheel rim rotates with 3000 rpm.

Results and Discussion

Figure 7 shows the stress in the fiber direction in each layer of the rim and hub-spokes regions under inflation pressure and the tire load. High stresses are present in the spoke where the tire load is acting.

The stress in the fiber direction for each hub-spoke and rim layer is shown in Figure 8 and Figure 9, respectively. High stresses occur in layer 3 (symmetric) of the hub-spoke region and layer 14, 15 of the rim region.

Figure 7: The stress distribution in a composite wheel rim.

The through-thickness variations of the transverse shear stress in first tangent direction of laminate at two points on the rim and spoke region are shown in Figure 10 and Figure 11, respectively. Each ply exhibits different stress levels depending on the fiber orientation.

Figure 12 shows the first four eigenmodes of composite wheel rim when the rim is rotating at 3000 rpm. The first natural frequency found for the composite wheel rim corresponds to approximately 8000 rpm. This is much higher compared to the operating range of the wheel and hence the structure is in a safe zone and does not have a critical speed. A rather high natural frequency is obtained because of the high strength-to-weight ratio of the carbon–epoxy composite material.

Figure 8: The stress distribution in each layer of hub and spokes region.

Figure 9: The stress distribution in each layer of rim region.

Figure 10: Through-thickness variation of laminate transverse shear stresses for a point on rim.

Figure 11: Through-thickness variation of laminate transverse shear stresses for a point on hub.

Figure 12: First four Eigenfrequency and mode shapes of the composite wheel rim.

Notes About the COMSOL Implementation

•

Modeling a composite laminate as a layered shell requires a surface geometry, in general referred to as a base surface, and a node which adds an extra dimension (1D) to the base surface geometry in the surface normal direction. You can use the functionality to model several layers stacked on top of each other having different thicknesses, material properties, and fiber orientations. You can optionally specify the interface materials between the layers, and control the number of through-thickness mesh elements for each layer.

•

The third direction for the selected coordinate system in the , , or represents the normal direction of the or physics. This is also the direction in which the layer stacking is interpreted from bottom to top, and therefore, it is crucial to know it during modeling. There are two ways to achieve this:

Using physics symbols: Go to the physics settings, find the section, and select the checkbox. Then go to the material feature, for instance, , to see the normal direction represented by green arrows in the geometry.

Using result templates: When a solution dataset is available, use the result template to plot the normal direction.

•

From a constitutive model point of view, you can either use the Layerwise (LW) theory based interface, or the Equivalent Single Layer (ESL) theory based node in the interface. The laminated composite shell presented in the current model is modeled using a node in the interface.

•

The built-in material library contains data for fiber and matrix constituents as well as for unidirectional and bidirectional laminae.

•

By default, loads are assumed to be applied on the shell's midsurface. In reality, however, loads may often act on the top or bottom surface such as the tire pressure and weight in this case. If forces are applied on a different surface than the midsurface, the actual area of applied load may also differ, which is generally true for curved surfaces. The forces applied away from the midsurface also gives rise to moments which are significant for thick shells. To take this effect into account loads must be scaled properly to achieve a correct load contribution. In particular for curved and/or tick shells care must be taken with respect to the load's location. The load location is be specified using the section in the feature.

•

In this example, the coriolis force giving rise to gyroscopic damping effect is neglected. The gyroscopic damping can change the eigenmodes and natural frequencies especially at high angular velocities.

Composite_Materials_Module/Dynamics_and_Vibration/composite_wheel_rim

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > .

Click .

Click

In the tree, select > .

Click

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

Click

Browse to the model’s Application Libraries folder and double-click the file composite_wheel_rim_parameters.txt.

Definitions

Analytic 1 (an1)

In the window, expand the > node.

Right-click and choose > .

In the window for , type loadDistr in the text field.

Locate the section. In the text field, type (abs(atan2(x,y)-z*pi/180)<pi/6)*cos(3*(atan2(x,y)-z*pi/180)).

In the text field, type x, y, z.

Locate the section. In the table, enter the following settings:


Argument	Unit
x	m
y	m
z	1

In the text field, type Pa.

Cylindrical System 2 (sys2)

In the toolbar, click

and choose .

Geometry 1

Import 1 (imp1)

In the window, expand the > node.

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Click

Browse to the model’s Application Libraries folder and double-click the file composite_wheel_rim.mphbin.

Click

Rim

In the toolbar, click

and choose .

In the window for , type Rim in the text field.

Locate the section. From the list, choose .

On the object , select Boundaries 11–19, 24, 26, 28, and 34–36 only.

HubAndSpokes

In the toolbar, click

and choose .

In the window for , type HubAndSpokes in the text field.

Locate the section. From the list, choose .

Locate the section. Click

In the dialog, select in the list.

Click .

TireAttachment

In the toolbar, click

and choose .

In the window for , type TireAttachment in the text field.

Locate the section. From the list, choose .

On the object , select Boundaries 16–19, 24, 26, 35, and 36 only.

FixedToHub

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the text field, type FixedToHub.

On the object , select Boundaries 8 and 30 only.

Rotate 1 (rot1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

In the text field, type range(0,72,288).

Click

SprokeRimUnit

In the toolbar, click

and choose .

In the window for , type SprokeRimUnit in the text field.

Locate the section. From the list, choose .

Locate the section. In the text field, type inf.

In the text field, type 18.

In the text field, type 90.

Locate the section. From the list, choose .

Disable the analysis of the geometry as the remaining small geometric details can be kept.

In the window, click .

In the window for , locate the section.

Clear the checkbox.

In the toolbar, click

Definitions

Integration 1 (intop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Global Definitions

COMSOL Multiphysics is equipped with built-in material properties for a number of lamina materials. Select the materials needed from the material folder in the built-in material library.

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > > .

Right-click and choose .

In the toolbar, click

to close the window.

Global Definitions

Layered Material 1 (lmat1)

The laminate is symmetric. Therefore, it is sufficient to define only a part of it in the node; the transformation into the full laminate is performed through the layered material settings in the and the nodes.

In the window, under right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Layer	Material	Rotation	Value	Thickness	Mesh elements
Layer 1	Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 58%] (mat1)	0	0 rad	th	1

Click three times.

In the table, enter the following settings:


Layer	Material	Rotation	Value	Thickness	Mesh elements
Layer 2	Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 58%] (mat1)	45	0.7854 rad	th	1
Layer 3	Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 58%] (mat1)	90	1.5708 rad	th	1
Layer 4	Unidirectional fiber lamina: AS4/APC2 carbon/PEEK thermoplastic [fiber volume fraction 58%] (mat1)	-45	-0.7854 rad	th	1