Ansys - Modal Analysis of a Composite Monocoque - Mesh

Mesh

Material Properties

The material properties for composite material are different than typical isotropic materials, because different directions have different material properties. Also, monocoque typically have a sandwich structure consists of carbon fiber and aluminum core. Steps blow shows how to enter orthotropic properties into Ansys.

T300 Weave

Double click  Engineering Data 

Add a new material by click into the text box, and name the material "T300 weave"

To enter an orthotropic material property, go to  Linear Elastic  > (Drag) Orthotropic Elasticity onto the new material. A lists of property information will appear in the Property Outline as shown below:

Here are the corresponding properties for this material:

E1 = 8500000 psi
E2 = 8500000 psi
Ez = 1000000 psi
Gxy = 560000 psi
Gxz = 830000 psi
Gyz = 560000 psi
Vxy = 0.06
Vyz = 0.06
Vxz = 0.06

This type of composite is weaved, so you have to define that as well, go to  Physical Properties  > (Drag) Density and Ply Type on to the new material.
In Property out line select  Woven&nbsp from the pull down menu.

Next step, we need to define the stress limits and tsai-wu constants for failure analysis.
Expand  Strength&nbsp > (Drag) Orthotropic Stress Limits and Tsai-Wu Constants on to the new material, and the properties are shown below:

5250 Core

Repeat the steps above to enter the properties for 5250 Core. The values are displayed in figure below:

Steel for the Suspension Links

Suspension links are normal isotropic materials. I have purposely made it really stiff, so we can see more deformation on the monocoque. Here are the properties:

Attach the Suspension Link & Mesh

following video shows how to mesh composite material and how to attach line bodies to surfaces

Go to Step 4 - Setup(Physics)
Go to all ANSYS Learning Modules