Versions Compared


  • This line was added.
  • This line was removed.
  • Formatting was changed.
Comment: Migrated to Confluence 5.3

Include Page
ANSYS Google Analytics
ANSYS Google Analytics
Include Page
High Resolution FE Model of Bone - Panel
High Resolution FE Model of Bone - Panel

Physics Setup

Create a material

Drag Static Structural into the Project Schematic page.

We have not defined the material for this model so we will do that before we proceed. Double click on Engineering Data. Click on "click here to add a new material" to create a new material. Name the new material "bone". Expand Linear Elastic and double click on Isotropic Elasticity.

In the properties window, expand Isotropic Elasticity and enter 1e9 Pa for Young's Modulus and 0.3 for Poisson's Ratio.

Click on the Project tab, next to the Engineering Data tab, to return to the Project Schematic page.

Assign Material

The default material used for Mechanical is structural. We need to change it to the new material we defined earlier (Tissue). In the outline window, expand Geometry and highlight Solid 1. The bone model will now be highlighted in green, meaning it is being selected. Right below the outline window you will see "Details of Solid 1". Expand Material, and change the assignment to Bone. The material properties we defined for Bone will now be assigned to the bone model.

Named Selection

We will assign deformation to the positive y face and roller support to the negative y face. The geometry of the model makes it difficult to select all the faces in a given plane. However, we can easily assign the BC using name selection.

Click on the z axis in the coordinate axis viewer to view the XY plane. Use the vertex selection tool and select a point on the top edge. Right below the model you will see the coordinates of this point. The y position is 4.98mm.

Right click on Named Selections and insert a new named selection. Change the Scoping Method to Worksheet.

In the main window you will see an empty table. Right click on the empty table and click on Add Row.

We will now enter the appropriate information that will help us create a named selection that includes all the faces in the top edge of the model viewed from the XY plane.

Select Face for Entity Type.
Select Location y for Criterion.
Select Equal for Operator.
Enter 4.98 for Value.

Click on Generate to generate the named selection. Rename it top y.

We will repeat the same steps to create a named selection for all the faces on the bottom edge of the model viewed from the XY plane.

The y coordinate for the bottom edge is 3.3e-2 mm. Rename the second named selection bottom y

Boundary Conditions

Right click on Static Structural (B4) and insert a displacement.

Change the Scoping Method to Named Selection and select top y. Enter -0.5 mm for the Y Component. This will assign a 0.5 mm displacement to the model in the -y direction on the faces selected for top y.

We can model the roller support as frictionless support in Mechanical. Right click on Static Structural (B4) and insert a frictionless support. Similarly, change the scoping method to Named selection but select bottom y.

This will constraint the displacement in the y direction but the model is allowed to displace in the x direction. This is very similar to the conditions of a roller support.

The setup is finished. You may move on to setting up the solution.

Go to Step 5: Numerical Solution

Go to all ANSYS Learning Modules