Fatigue Response of a Random Nonproportional Load

A thin-walled frame member with a central cutout is subjected to a random load scenario. Although the stresses are expected to be far below the yield level of the material, a concern arises whether or not the component fails due to fatigue.

This example demonstrates an approach to damage quantification of a long load history. The rainflow counting algorithm is used to define the load scenario and the Palmgren-Miner linear damage model quantifies the damage.

Model Definition

The load carrying beam is shown in Figure 1. It has a length of 1.1 m, a thin-walled square cross section having the dimension 160 mm x160 mm and a thickness of 6 mm. The cutout is centrally placed on one of the faces and is 100 mm long, 80 mm wide and has a fillet with radius 10 mm in each corner.

Figure 1: Geometry of the frame member.

The loading consists of bending moments in both directions and a twisting moment. All three loads can vary independently. The information about the load is obtained using three strain gauges, which are glued on the bottom and the back sides of the frame. The back side is the one opposite to the face with the hole. The location and position of the strain gauges are shown in Figure 2. Strain gauges 1 and 2 are oriented at a 45° angle to the global coordinate system while the 3rd strain gauge is aligned with the length of the face (the x-axis). Both are located 850 mm from the edge along the length and in the middle along the width of the faces.

Figure 2: Location and orientation of the strain gauges.

The frame is made out of steel with Young’s modulus, Poisson’s ratio, and density given by E = 200 GPa, ν = 0.33, and ρ = 7800 kg/m3, respectively.

The fatigue behavior is described by the material library data for iron alloy 4340 for a variant defined by phase and variation .

The left end of the structure, x = 0, is clamped. One twisting moment, along x, and two bending moments, along y and z, are applied on the right end at x = 1.1 m. The lifetime for which the frame is designed is 10,000 longer than what has been recorded by the strain gauges. The response to one loading cycle block in all three gauges is captured in Figure 3. From the history it is clear that the loading event is nonproportional. However, stress concentrations arise around the cutout where the stress state is uniaxial. Therefore the used models, Rainflow Counting and Palmgren-Miner summation, can be seen as appropriate for fatigue evaluation.

Figure 3: Strain history in the tree strain gauges. The subscript indicates the gauge number.

In order to apply the strain history to the frame, the strain history needs to be transferred to loads which can be applied on the boundary. The transformation can be done in two ways. In the first, a relation between a unit moment and a response in each strain gauge must be obtained using COMSOL Multiphysics. By repeating it for each unit moment and inverting the relation, a transformation matrix relating strains to moments is obtained.

An alternative way is to use an approximate analytical relation based on beam theory with a thin-walled assumption, Hooke’s law, and rotation of stresses in a plane. The result is given below without a detailed derivation.

(1)

where

, and

. The variables t = 6 mm and b = 154 mm define the thickness and the side (using midsurfaces) of the cross section.

Based on the geometrical and material constants, Equation 1 gives the following relation

(2)

Results and Discussion

According to a finite element analysis the, applied moments and gauge strains are related by

(3)

The coefficients differ somewhat when compared to the analytical results, Equation 2. It is reasonable to assume that the final fatigue prediction also differs, depending on used transformation matrix. Since Equation 2 is based on approximations, further results are based on the FE-relation, Equation 3.

Stresses on the inner side of the shell are more critical from the fatigue point of view. The variation of the fatigue usage factor along the fillets is shown in Figure 4. It reaches about 0.11 and thus the examined frame should not fail in fatigue.

Figure 4: Fatigue usage factor along the cutout fillets. The angle is measured in the xz-plane with the angle starting from the x-axis.

In the most loaded point in the structure the stress history seems to be fairly symmetric around a zero mid stress. The mid stress is found in the range from -250 MPa to 250 MPa and the amplitude extend almost up to 600 MPa. The load distribution in the critical point is captured and shown in the Rainflow histogram in Figure 5.

Figure 5: Cycle counting, following the rainflow theory, in the point of the highest fatigue usage factor.

In Figure 6, the relative contribution to the damage is shown for the same location. The dark blue area indicates stress cycles which are nondamaging. This means that they are below the endurance limit in the Wöhler curve, also called the S-N curve. The damaging stress cycles are found for high stress amplitudes. Since the Palmgren-Miner rule scales damage linearly with the number of cycles, when the number of cycles increases by a factor 1/0.11, the fatigue usage factor exceeds 1 and thus a failure occurs. In practice, the linearity assumption of the Palmgren-Miner rule can be questioned, so a proper safety factor should be applied.

An important information when evaluating Figure 5 and Figure 6 is that 37% of the fatigue damage comes from one single event in the load history and that most damage is caused by only few load cycles. This indicates that the load history recorded is too short to make good predictions. Either a new, longer, measurements should be made, or a high safety factor should be used in combination with some statistical considerations.

Figure 6: Relative fatigue usage, following the Palmgren-Miner damage rule, in the point with the highest usage factor.

Notes About the COMSOL Implementation

In COMSOL Multiphysics, several functions with the same argument list can be put in one file. This is demonstrated in the example with three load functions define the moment prescribed on one end of the frame. When an interpolation function is read from a file it treats the first columns as arguments and the following one as function response.

COMSOL Multiphysics provides several options for specification of the S-N curve. Interpolation function with options data type , interpolation ,and extrapolation is recommended. Those options are optimal for search of the life once R-value, and the amplitude stress are known. The input for S-N curve defined in the example is shown in Figure 7.

Figure 7: Wöhler curve of the material.

The fatigue material data in the material library gives the maximum fatigue stress,

, as the function of the number of cycles and R-value. In order to transfer it to the stress amplitude,

,which is required by the Cumulative Damage fatigue feature, just apply following transformation

Fatigue_Module/Damage/frame_with_cutout

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.

In the table, enter the following settings:


Name	Expression	Value	Description
M	1 [N*m]	1 N·m	Unit moment
pt	6 [mm]	0.006 m	Frame thickness
ch	80 [mm]	0.08 m	Hole height
cw	100 [mm]	0.1 m	Hole width
cr	10 [mm]	0.01 m	Hole radius

Geometry 1

Block 1 (blk1)

In the toolbar, click

In the window for , locate the section.

In the text field, type 1.1.

In the text field, type 0.154.

Locate the section. From the list, choose .

Work Plane 1 (wp1)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

On the object , select Boundary 3 only.

Click

Work Plane 1 (wp1)>Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

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

In the text field, type cw.

Work Plane 1 (wp1)>Fillet 1 (fil1)

In the toolbar, click

On the object , select Points 1–4 only.

In the window for , locate the section.

In the text field, type cr.

Create points for strain evaluation where strain gauges are placed.

Point 1 (pt1)

In the window, right-click and choose .

In the window for , locate the section.

In the text field, type 0.3.

In the text field, type -0.077.

Point 2 (pt2)

In the toolbar, click

and choose .

In the window for , locate the section.

In the text field, type 0.3.

In the text field, type 0.077.

Click

Definitions

Create a new coordinate system that is aligned with the strain gauge directions on the bottom side of the frame.

Base Vector System 2 (sys2)

In the toolbar, click

and choose .

In the window for , locate the section.

In the table, enter the following settings:


	x	y	z
x1	cos(pi/4)	sin(pi/4)	0
x2	-sin(pi/4)	cos(pi/4)	0

Find the subsection. Select the check box.

Click the

button in the toolbar.

Shell (shell)

In the window, under click .

Select Boundaries 2–5 only.

Thickness and Offset 1

In the window, under click .

In the window for , locate the section.

In the d text field, type pt.

Linear Elastic Material 2

In the toolbar, click

and choose .

Select Boundary 3 only.

Shell Local System 1

In the window, expand the node, then click .

In the window for , locate the section.

From the list, choose .

Prescribed Displacement/Rotation 1

In the toolbar, click

and choose .

Select Edges 1, 2, 4, and 6 only.

In the window for , locate the section.

Select the check box.

Apply one twisting and two bending unit moments and differentiate them using load cases.

Rigid Connector 1

In the toolbar, click

and choose .

Select Edges 17–20 only.

Twisting Moment (x)

In the toolbar, click

and choose .

In the window for , locate the section.

Specify the M vector as


M	x
0	y
0	z

In the text field, type Twisting Moment (x).

Rigid Connector 1

In the window, click .

Bending Moment (y)

In the toolbar, click

and choose .

In the window for , locate the section.

Specify the M vector as


0	x
M	y
0	z

In the text field, type Bending Moment (y).

Rigid Connector 1

In the window, click .

Bending Moment (z)

In the toolbar, click

and choose .

In the window for , locate the section.

Specify the M vector as


0	x
0	y
M	z

In the text field, type Bending Moment (z).

Twisting Moment (x)

In the window, click .

In the toolbar, click

and choose .

Bending Moment (y)

In the window, click .

Click

and choose .

Bending Moment (z)

In the window, click .

Click

and choose .

Global Definitions

Load Group: Mx

In the window, under click .

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

In the text field, type Load Group: Mx.

Load Group: My

In the window, click .

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

In the text field, type Load Group: My.

Load Group: Mz

In the window, click .

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

In the text field, type Load Group: Mz.

Materials

Material 1 (mat1)

In the window, under right-click and choose .

Select Boundaries 2–5 only.

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	E	200e9	Pa	Young’s modulus and Poisson’s ratio
Poisson’s ratio	nu	0.33	1	Young’s modulus and Poisson’s ratio
Density	rho	7800	kg/m³	Basic