Step-by-Step Tutorial Session 1: Hip Joint Prosthesis

AnnaFless · January 24, 2018, 11:39am

Recording

Homework Submission

For your homework, your task is to setup a static structural analysis considering different material combinations for an artificial hip joint to better understand how stresses are transferred to the femur bone.

The step-by-step tutorial below contains all of the steps for setting up the simulation in SimScale and visualizing the results.

To submit your homework assignment, please generate a public link of your project (Sharing a Project)

Homework Deadline: Sunday, February 4th, 11:59 pm CET

Submit your homework here

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 Medicine 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.

To set up the hip model for virtual simulation, the following loading conditions will be used:

The distal end of the bone is assumed to be fully fixed.
The body weight of the person is applied as a fixed force (Force 2).
The hip joint head, which transfers the load from the upper body to the lower body is loaded with a variable force over 100 iterations (Force 1). See the graph below:

In this step-by-step tutorial, we will focus on a hip joint prosthesis 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:

Import Project

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 order: First 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 Setup

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

Since we want to evaluate the displacements, stresses, and strains on the hip prosthesis and femur, select the analysis type Static under Solid mechanics and then click create.

Give the project a name (optional) Co-Cr-Mo on Ti-6Al-4V and set the Nonlinear analysis option to true 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.

Contacts

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.

Click to select all the faces of the head that will come in contact with the stem. Your selections will be automatically assigned to the Master entity (Blue).

Click on the Slave entity assignment box to activate selection.

Then follow the same procedure for selecting the surfaces of the stem that are in contact with the head and assign these faces to the Slave entity.

Hide all the volumes except volumeOnGeoVolumes_3 from the scene viewer in the top right.

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

Create a New Contact called Stem - bones contact and setup 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.

Click on the Slave entity assignment box to activate selection. Do the same for the stem and assign the faces as the Slave entity. Click Save to save the contact definition.

Hint: If you have problems selecting the faces in the Viewer, you can use the Scene viewer on the right of the screen to select faces. Double check that your selected entities match with those provided in the table below:

Trabecular - marrow contact:

Create a New Contact called Trabecular - marrow. Hide all volumes except volumeOnGeoVolumes_0. Select the lower face and assign it as the Master entity.

Click on the Slave entity assignment box to activate selection. 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

Create a New Contact called 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.

Click on the Slave entity assignment box to activate selection. 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].

Materials

Go to the Materials item in the Navigator 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.

Assign the material to volumeOnGeoVolumes_4.