Hello and welcome!
Many system components around us experience cyclic loading.
This fluctuation or harmonic loading may cause microcracks to form and coalesce to cause fatigue failure.
In such cases, catastrophic failure may occur without warning,
even at a much lower stress level than those required to cause yielding of the components.
To increase the reliability of products, it is very important to study the fatigue life of the components.
In this video, we will discuss how we can use Ansys Mechanical Fatigue Tool to determine the fatigue life
and damage caused by the harmonic loading.
Ready! Let's go.
Generally speaking, in Ansys Mechanical, fatigue analysis can be performed using several methods,
including the Stress-Life and the Strain-Life methods.
Fatigue calculations using Harmonic Analysis are based on the Stress-Life method.
Please note that while Mechanical offers different fatigue analysis options,
our discussion will be focused on harmonic fatigue.
The Stress-Life method, also designated as the “S-N method”, assumes that the fatigue damage is caused by fluctuating stress,
which is also known as “alternating stresses”.
This method is suitable for low-stress and high-cycle applications since it does not consider the effects of plasticity.
So, in the case of ductile materials, the fatigue failure would usually occur when they are subjected to more than a hundred thousand cycles.
The fatigue life of a material is characterized by the alternating stress range and stress-life, or S-N, curves.
This S-N curve is a plot of stress range or alternating stress (S) versus the total cycles to failure (N),
usually obtained through experimental testing.
This is the additional material information needed before performing a fatigue analysis.
In Ansys Mechanical, fatigue calculations are performed using the Fatigue Tool.
In the Details panel of the Fatigue Tool, you can see various options.
Let’s start with two parameters that can be used for scaling.
The Fatigue Strength reduction factor Kf can be included to add conservatism into the results
since the actual life may not be as high as from the test environment used to get the S-N curves.
The Scale Factor is a way to see the effects on life with a different load magnitude
without having to run a separate simulation since S-N curves are not linear.
These two parameters both default to a value of 1, meaning that no changes are included in the fatigue analysis.
The Stress Component provides you with an option to select the stress component on which the fatigue calculations will be carried out,
defaulting to Equivalent Stress.
Note that, ideally, the stress state of the experimental data for the SN curve
and the stress used in fatigue calculations should be similar,
but this is often not the case, so the user should be aware of this point.
Harmonic analysis is performed in the frequency domain, but we usually measure life in the time domain,
so we need two parameters to do this conversion – the exposure duration and the frequency.
The Exposure Duration option is used to specify the time duration for which the loading is applied, defaulting to 1 second.
Using the Frequency option, you can specify one or more frequencies from which the alternating stresses will be taken.
By knowing the frequency, which is in Hertz or cycles per second, and exposure duration, in seconds,
we can calculate the number of cycles experienced by the parts.
In terms of the methods available, we can solve for a single frequency, multiple user-specified frequencies, or perform a sweep of a frequency range.
After fatigue calculations are performed, we can evaluate the product’s life and damage.
The Fatigue Life result provides a contour plot showing the available life, in seconds, across the component.
It’s worth noting here that, traditionally, fatigue life is expressed in cycles.
However, in harmonic fatigue, we can have multiple frequencies,
so a higher frequency will have more cycles per second than a lower frequency excitation and comparison of ‘cycles’ becomes confusing –
that is why, to account for different frequencies, life is expressed in seconds rather than in cycles.
The Fatigue Damage result is a contour plot showing design life divided by the available life.
Damage greater than 1 indicates that the part will fail for the given exposure duration.
An important point to consider is that results for single and multiple frequency cases
will use the number of cycles of the last defined S-N data point for undefined, low-stress values.
Extrapolation of the S-N curve is not done outside of your data points.
For example, if your last data point on the S-N curve is 1e8 cycles at 70 MPa,
a value of 30 MPa will be considered to have a life of 1e8 cycles if not defined directly.
This is important to note because, at high frequencies, there will be many cycles per second,
so a shortened life could be predicted if your S-N data does not cover an appropriate stress range.
When performing a fatigue analysis of a sine sweep, a value of roughly 1e32 cycles is used for undefined, low-stress amplitudes.
Let’s now get a better understanding of these concepts with the help of a walkthrough example in Ansys Mechanical.
For the walkthrough, we will consider an example of a Mounting Bracket
which is generally an overhanging member that projects from a structure
and is usually designed to support a vertical load or to strengthen an angle.
In our case, the bracket is designed to support external components connected to it and to absorb the generated vibrations.
These vibrations lead to the bracket experiencing a fluctuating or harmonic load
that may result in the structural fatigue of the bracket.
The bracket has been assigned with an Aluminum Alloy material.
Mounting Brackets are generally not designed to handle a large load exciting it at resonance.
Hence, our goal through this analysis would be to determine how long the bracket would last
if a large fluctuating load of 10,000 N is applied for 10 mins at resonance.
After solving the model, fatigue results which will include the life, damage, and alternating stress
would be analyzed using the Fatigue Tool in Ansys Mechanical.
Without further ado, let’s get started.
Go to the project page and pick File, Open.
Select the Workbench project archive file Mounting Bracket.wbpz
Save the project to the desired location. We will keep the filename as specified.
We could see a Harmonic Response Analysis coupled with Modal Analysis is already added on the project page.
Double click on the Model cell to open Mechanical.
Let’s review the results of the Modal Analysis.
We can review the mode shapes, and the first mode is of primary interest.
We’ll look at the response for excitation from 0 to 500 Hz,
which will cover the first two modes that have a high effective mass in the Z-direction.
Let’s now apply the loads for Harmonic Response Analysis.
We are considering a situation where the external component is connected to the bracket through the hole
located at the end of the overhanging region.
Right-click on Harmonic Response, Insert, and select Force.
Scope it to the inner face of the connecting hole.
Change the ‘Define by’ option to Components and enter a Z-Component of minus 10,000 N.
This force will represent the fluctuating load that the externally mounted components would apply on the bracket in the negative Z-direction.
Lastly, let's modify the Analysis Settings.
Set the frequency range from 0 to 500 Hz as noted earlier.
Change the ‘Cluster Results’ option to ‘Yes’ and define ‘Cluster Number’ as 10 for higher resolution and accurate prediction of peak frequencies.
Under Damping Controls set the Damping Ratio to 0.02, which represents 2% damping.
Insert Frequency Response, Deformation,
scope it to the body,
and change the Orientation to Z-Axis which is the direction of excitation.
The model is now ready to be solved.
Right-click on Harmonic Response and Solve.
As the model is now solved, click on Frequency Response to inspect the solution.
We can observe two peaks that are clustering around the natural frequencies.
Notice that the bracket experiences most deformation when it is excited at a frequency near the 1st mode.
Under Frequency Response expand Results to view the Maximum Amplitude, Frequency, and Phase Angle.
Now, right-click on Frequency Response, select ‘Create Contour Results’ and evaluate the results.
We can observe that the overhanging region of the bracket undergoes maximum deformation of magnitude 8.73 mm.
Insert Equivalent Stress and evaluate at the same frequency and phase angle obtained from the Contour Results.
We can observe the region which is experiencing the maximum stress.
Now, let’s check the Fatigue Results using the Fatigue Tool.
Right-click on Solution, Insert, Fatigue, and pick Fatigue Tool.
Define an Exposure Duration of 600 secs or 10 mins at a frequency of 162.1 Hz
which is the natural frequency where the bracket experiences most deformation.
Insert Life, Damage, Equivalent Alternating Stress and Evaluate All Results.
The Fatigue Life Results show that the failure occurs at 3447 secs,
so we can conclude that the Mounting Bracket will be able to sustain the heavy loading at resonance for more than 10 minutes.
From the Fatigue Damage, we can identify the region which is experiencing the maximum damage.
I hope that this simulation example has helped you understand
the process to perform a Frequency-based Fatigue Analysis for Harmonic Loadings.
So, let’s summarize the learning points of this video.
Failure due to fatigue can occur at low-stress levels, so investigating fatigue can be an important part of ensuring structural reliability.
While Ansys Mechanical has several different methods for evaluating fatigue failure,
we focused our attention on harmonic fatigue that allows us to explore the life
and damage of a structure under excitations at single or multiple frequencies.
Instead of the traditional approach of looking at the number of cycles to failure,
with harmonic fatigue, we look at the time to failure since more than one frequency may be involved.
I hope you have found this video informative. Do not forget to check out our other courses to discover more useful learning resources.