Biomedical Engineering Workshop Session 1: Stress shielding in a Hip joint prosthesis

nava · August 9, 2016, 8:55am

Recording

Introduction

A hip joint prosthesis is used to replace a damaged hip joint. The most common materials used for artificial hip joints are metal alloys, ceramic or certain types of plastic. It is important to study these prostheses to understand how much compressive force will be transferred directly to the femur bone.

Ideally we would want a prosthetic joint component to carry stress in the same way as the original bone, however, this does not happen in real life.

According to the Department of Radiology at the University of Washington:

In a hip prosthesis, much of the load applied to the femoral component tends to be transmitted to the bone near its distal tip. The bone near the proximal part of the component tends to have less force transmitted through to it. What happens to the native bone that is now no longer receiving its usual loading? Bone loss occurs here. This phenomenon is called “stress shielding”. Since one can get quite a bit of stress shielding around a prosthesis, it’s no mystery why one sees progressive bone loss around prosthetic components over the years on follow-up radiographs.

The concept of stress shielding helps to explain the usual life course of a joint prosthesis. A hip prosthesis, for example, may last for 5 – 10 years before sufficient stress shielding occurs that the prosthesis loosens enough to be symptomatic. The loose prosthesis is then removed by the orthopedist, and a new one is put in. However, the native bone around the original femoral component now generally has substantially diminished bone stock. Therefore, the new one has to have a longer stem so that it will reach down far enough to seat in normal bone. This new prosthesis works for another 5 – 10 years, until stress shielding has caused enough bone resorption around this new prosthesis for it too to become symptomatically loosened. Then, a newer, even longer prosthesis is placed, and the cycle continues. Obviously, this process can’t go on forever, since you eventually run out of undisturbed bone in which to seat the prosthesis.

In this exercise, we will focus on a hip joint prothesis model considering different material combinations for our artificial hip joint to better understand how stresses are transferred to the femur bone. You will perform 3 different simulations using the same geometry with different material combinations as shown:

The image below shows settings of loading conditions for all of the 3 cases. The loading is assumed to be generated by a human walking at speed of 1 km/h ^[1].

$$~$$
To start this exercise, please import the project into your workspace by clicking on the link below:

Mesh Generation

In the Mesh Creator tab, click on the geometry hip_joint_prosthesis

Then, click on the New Mesh button in the options panel.

Select the mesh Type Tet-dominant. This operation will automatically create a mesh for the geometry. The cell size and refinement will be adapted automatically. Please choose the following parameters:

Element sizing Automatic
Mesh fineness 3-Moderate
Element orderFirst order
Number of computing cores 8

Click on Save to preserve the mesh settings

Now click the Start button to begin the mesh operation. The meshing job will start in a few moments (all of the computation is done via cloud computing).

The mesh operation takes about 5 minutes to complete. You will see the Finished status in the lower left corner when it is ready.

Simulation

For setting up the simulation switch to the Simulation Designer tab and click +New to create a new simulation.

A pop-up will appear. Give the project a name (optional) Co-Cr-Mo on Ti-6Al-4V and click Create

Since our load will be static and the deformation will be small, select the analysis type Static analysis - advanced under Solid mechanics. Let the Nonlinear analysis remain set to false and click Save.

After saving, the Navigator now looks as shown below. Here the entries in red must be completed.

Click the Domain item in the Navigator and select the mesh that you just created. Click Save. The mesh will then automatically load in the viewer.

Next, change the render mode to Surfaces in the top viewer bar to interact with the mesh more easily.

Due to different material definitions for the bone and hip joint, we have to have a geometry that contains multiple volumes. These need to be bonded together so that the solver knows that they are connected. We will proceed with defining the bonded contacts between all of the solids.

Go to Contacts and click +New to create a new contact.

Head - stem contact:

For creating a bonded contact between the head and stem of the hip joint, rename the contact definition to Head - stem contact (optional).

Hide all the volumes except volumeOnGeoVolumes_4 from the scene viewer in the top right.

Select all the faces that will come in contact with the stem. Add your selection from viewer under Master entity. This will add all the selected faces. (Note: make sure you are in Pick faces mode before the selection)

Click Clear selection to clear the selected surfaces.

Follow the same procedure for selecting the surfaces of the stem and assign these faces to the Slave entity. Click Save to create the contact.

To reconfirm, please make sure your selected entities match with those provided in the table below:

Stem - bones contact:

Now create the contact between the stem and bones. Hide all of the solids except volumeOnGeoVolumes_0,volumeOnGeoVolumes_1 and volumeOnGeoVolumes_2

Select all of the internal surfaces that are in contact with the stem. Assign them as the Master entity.

Do the same for stem and assign the faces as the Slave entity. Click Save to save the contact definition. (make sure to clear the previous selection before doing this)

To reconfirm, please make sure your selected entities match with those provided in the table below:

Trabecular - marrow contact:

Hide all volumes except volumeOnGeoVolumes_0. Select the lower face and assign it as the Master entity

Hide all volumes except volumeOnGeoVolumes_1. Select the lower face and assign it as the Slave entity. Click Save to save the contact definition.

To reconfirm, please make sure your selected entities match with those provided in the table below:

Cortical - trabecular - marrow contact:

Hide all volumes except volumeOnGeoVolumes_0 and volumeOnGeoVolumes_1. Select all of the outer faces and assign them as the Master entity.

Now hide all volumes except volumeOnGeoVolumes_2. Select all of the internal faces and assign them as the Slave entity. Click Save to save the contact definition.

To reconfirm, please make sure your selected entities match with those provided in the table below:

Now that the contacts are set up, we will define the material definition for all of our volumes. The material definition for the bones and the hip joint are taken from reference ^[1].

Go to Materials under tree and click + New

Head (Co-Cr-Mo alloy):

First we will define the material for the hip joint head. Rename the newly created material to Head (Co-Cr-Mo alloy) (optional).

Change the Young’s modulus, Poisson’s ratio and Density values to 210e9, 0.3, and 8800 as shown in the figure below.

Select volumeOnGeoVolumes_4 under Topological Mapping