FE-modeling of Hertzian Contact

Finite Element modeling software gives users the ability to evaluate contact like never before. Contact analysis can be extremely useful for a variety of problems such as identifying bearing stresses, bolted joints, interference fits, tribological investigations and many more. However contact, especially detailed Hertzian contact isn't something most engineers are familiar with like stress and strain. Let's run through a simple Hertzian contact example and see if ANSYS can accurately predict contact width and maximum pressure.

In this problem we have a Cylinder set into a Cylinder Groove with a 2000 lb. force pressing the cylinder into the groove. We are interested in finding the contact distance (b) and the maximum pressure in this contact region.

Let's begin by finding the true solution based upon Hertzian Equations.

1/2 Contact Width (b) = 0.1985 in, Maximum Pressure (P) = 64,150 psi

Now let's use ANSYS 2025 to see if we can identify a Finite Element solution to this Hertzian contact problem.

We are starting with a simple CAD model that precisely represents the Cylinder in a Cylindrical Groove Example Problem. If you need this geometry please let me know! This problem is almost ideal for a 2-D FE-model, however with powerful FE software like ANSYS, a 3-D FE-model solves very quickly. Since we aren't learning about 2-D models today let's stick with a 3-D model for now, we can cover 2-D analysis in the future.

We have meshed this model using a global mesh size of 0.02 inches and we have defined 2 elements across the thickness. This model is constructed of 6,266 Parabolic Elements with 35,721 Nodes. Even this course mesh should get us a reasonable solution to this problem.

6,266 Parabolic Elements with 35, 721 Nodes

Frictionless Contact was created between the Cylinder and Cylindrical groove. In order to get a nearly perfect solutions we have defined the Contact Formulation as Augmented Lagrange and Pinball Radius of 0.05, all other settings are default.

Frictionless Contact, Formulation: Augmented Lagrange, Pinball Region = 0.05 in

When setting up a model such as this we need the model to be fully constrained. In this instance we will use Frictionless Supports to fully constrain the model in all axes with the exception of Cylinder in the Vertical Axis. As there is a small gap between the Cylinder and Cylindrical Groove we have set this model up in two steps. Step one, the Cylinder is displaced 0.01 inches vertically using a displacement constraint, this will allow contact to initiate. Step two, the displacement constraint is deactivated and a Force load of 1,000 lbf is applied vertically. This is a symmetric model so 1,000 lbf acting on half of the model is equivalent to 2,000 lbf acting on the entire model. This model was solved with Large Deflection "On".

Frictionless Support All Steps, Step 1 Displacement = 0.01 in, Step 2 Pressure = 1,000 psi

This model converges in under 8 seconds, but your results will vary based upon your computers performance. Let's take a look at the results.

ANSYS Output: 1/2 Contact Width (b) = 0.200 in, Maximum Pressure (P) = 64,874 psi

Let's summarize our findings.

Using ANSYS we were able to create a simple 3-D FE-model that aligns with the Hertzian Equations for both 1/2 Contact Width (b) and the Maximum Contact Pressure (P) between a Cylinder and Cylindrical Groove. This model was quick to set-up and both steps were solved in less than 8 seconds total.

This problem was specific chose to work with a lower mesh count and still return reasonable results. In the future we will look into more challenging Hertzian contact problems that will require much higher level of mesh refinement.

The Finite Element Method has come a long way from its humble beginnings. Thank you for taking the time to read this article and please let me know what you want to learn about in the future.

John Parsons

Analyst

MESim LLC

John.Parsons@MESim.us

www.MESim.us