Tutorial: Combining Loading Conditions in Fatigue Studies

With SOLIDWORKS Simulation, the engineer has many ways to analyze a design against loads. For example, a static simulation will determine the stresses and a factor of safety.

The design may pass a static simulation, but another mode of failure should be considered: fatigue. Fatigue failure results in a part that has been subjected to loading and unloading for many cycles—to the point where microscopic defects in the material grow into cracks, which eventually causes the part to fail.

It is extremely important to consider this mode of failure if the part will be in use for a long time. SOLIDWORKS Simulation has a fatigue study functionality built in, so it can take loading conditions and determine the consumption of usable life after a set number of cycles.

SOLIDWORKS Simulation fatigue studies work on the principle of high cycle fatigue, which is when the stresses experienced by the part result in negligible plastic deformations for any given cycle. Low cycle fatigue is when significant plastic deformation occurs causing the part to fail in a low number of cycles, as the name implies. Low cycle fatigue is currently not supported with fatigue studies and the engineer should seek to use an analytical strain-based life approach.

We need to know what the load is in order to run the study. Therefore, the first task is to define and run one or more static studies.

If you would like to follow along, you can download the file SimplePulley.SLDPRT (SOLIDWORKS 2020+).

For this exercise, we will investigate how multiple loading conditions can be taken into consideration for this fatigue study. There will be two: the stresses caused by an axially directed load, and the stresses caused by a radially directed load.

First Study: Static – Radial Load

Step 1

After making sure the simulation add-in is active, start a new static study named “Static 1.”

Step 2

For fixtures, add the inner cylindrical face as Fixed Geometry. (This is assumed to be keyed or held mechanically fixed with some other method, but we will neglect the stresses caused by this in this study.)

Step 3

For Loads, add a Force to the recessed groove, selecting “Plane1” as the Selected Direction. Enable to “Normal to Plane” option and enter 10,000N (10kN). Direction does not matter.

Step 4

For the mesh, set up a standard mesh with the slider all the way to fine. Mesh the part.

Step 5

Run the study. You should get a result similar to the one below.

Second Study: Static – Axial Load

In addition to the radial load, the machine part experiences a smaller—but significant—amount of axial load. This will be accounted for in our fatigue study.

Step 6

Similar to the previous part, create a new static study named “Static 2.”

Step 7

The fixture will be identical to the previous study, the internal cylindrical face.

Step 8

The load will differ. Add a Force load to the annular face on the front with a magnitude of 2,000N (2kN) normal to the face.

Step 9

Mesh the part with the exact same settings as the previous study (standard with the slider all the way to fine). This is not coincidental. In order for the fatigue study to run, the meshes need to be the same in all studies that it is considering.

Step 10

Run the study and look at the results. They should be similar to the image below.

We are now at the halfway point. Time for the fatigue study.

Final Study: Fatigue Study

With all the requisite data, we can now move on to the fatigue study.

Step 11

Start a new study and specify a fatigue study. There are several kinds of fatigue study, but in order to use the results from our static studies we will use “Constant Amplitude Events with Defined Cycles.” Other fatigue studies available are variable amplitude studies and harmonic or random vibration.

The first thing we need to do is add an event. An event is analogous to a load in a static study, as it is the main input for a fatigue study. Notice that there are no nodes for “Loads,” “Fixtures,” or “Mesh.” All of that information is defined in their respective studies. (This is also why the mesh must be the same across all studies to consider.)

Step 12

Right Click on the Loading node and click “Add Event…” The property manager will change.

The first box is the number of cycles to test; this could be anywhere from hundreds to millions. For this example, we will subject the part to 100k cycles of the loading from the first study.

The next parameter is the nature of loading. This could either be Fully Reversed, meaning that the load will alternate stress directions, or Zero Based, which is just loaded and unloaded. It is assumed that this machine part will be changing directions and loads, so we will choose Fully Reversed.

The third section is how to tell which study we are considering. For this, make sure the drop down is set to “Static 1.”

All these parameters are described in the following image.

Step 13

Set the other event and repeat step 12—except use 50,000 for the number of cycles, Fully Reversed for loading type, and select “Static 2” from the drop down.

Now we must verify or enter the S-N material data. It is important that the material has an S-N curve, as this is what SOLIDWORKS checks against to determine the amount of damage sustained by the part. This information can be found in many engineering resources for common materials (such as bronze, aluminum, etc.). If the material is specially alloyed by a company, then that company should have the S-N data for the material they make.

SOLIDWORKS can also derive the S-N curve from the elastic modulus. This should be only done on austenitic materials (such as carbon steel).

As the results of the study directly relies on the S-N curve data, extra effort should be made to ensure that the data is as accurate and trustworthy as possible.

Step 14

Right Click on the node where it shows the name of the part, in this case “SimplePulley,” and click on “Apply/Edit Fatigue Data.”

The material window will pop up with an opportunity to enter or derive an S-N curve; for this example, we will derive the data from the ASME Carbon Steel Curves. Make sure to hit “Apply.”

Step 15

We now have all the information to run the study! But first, we will point out a few of the settings you can change in a fatigue study. If you right click “Fatigue1” (the top node) and click on “Properties…” more information about how the fatigue study will solve can be accessed.

In this example, we do not need to change any of these settings, but wanted to point out the event integration options.

If we are sure that the loadings we have specified will never happen at the same time, we can select “No interaction.” If there is a chance that the loading conditions can happen at the same time, it is recommended to select “Random interaction.” This is the case for our machine part, so we will leave as is.

Step 16

Right Click and run the study.

These results can be a bit tricky to read, so we will change the chart to be more readable.

Step 17

Right click on the “Results1” Plot and hit “Chart options.” We like to have the “Show Max Annotation” enabled, to show the location that is receiving the most damage. We also like to change the “Automatically defined maximum and minimum value” to 100 and 0, respectively. That way, anything that appears red is 100% damaged (or at end of life) and blue means 0%.

Lastly, we like to change the numbers from scientific to general, to make it easier to read.

From here, we can analyze the data. By default, it will display the damage percentage (usable life consumed) throughout different regions of the part. We can observe that the part is approximately 40% through its usable life (as denoted by the Max annotation). The location of this damage is where we would expect to find it, at the small radius of the spokes.

Other than the rest of the fillets also being around 40%, the rest of the part is around 15% through its usable life, denoted with the washed-out blue color (but which could be more accurately determined with the probe tool).

With that, we can determine what 100k cycles of primary loading amounts to in time, and determine whether that fits the part’s expected service life.

Learn more about SOLIDWORKS with the whitepaper Understanding Nonlinear Analysis.

Recent Articles

Related Stories

Enews Subscribe