Open Ansys Workbench.

On the Workbench Project page, drag a Static Structural system from the Toolbox to the Project Schematic. The Project Schematic should appear as follows. The properties window does not display unless you have made the required selection; right-click a cell and select Properties.

In the Static Structural schematic, right-click the Engineering Data cell and choose Edit. The Engineering Data tab opens and displays Structural Steel as the default material.

Click the box below the field labeled "Click here to add new material" and enter the name "Interface Body Material".

Expand the Linear Elastic option in the Toolbox and right-click Orthotropic Elasticity. Select Include Property. The required properties for the material are highlighted in yellow.

Define the new material by entering the following property values and units of measure into the corresponding fields.

Once complete, the properties for the material should appear as follows.

Now, create a new Material that specifies the formulation used to introduce the fracture mechanism. For this tutorial, the Cohesive Zone Material (CZM) method is used. Click the field labeled "Click here to add new material" and enter the name “CZM Crack Material”.

Expand the Cohesive Zone option in the Toolbox and right-click Fracture-Energies based Debonding. Select Include Property. The required properties for the material are highlighted in yellow.

Define the new material by entering the following property values and units of measure into the corresponding fields.

The properties for the material should appear as follows.

In the Static Structural schematic, right-click the Geometry cell and choose Import Geometry>Browse.

Browse to the proper location and open the file 2D_Fracture_Geom.agdb. This file is available here on the Ansys customer site.

Right-click the Geometry cell and select Properties. In the Properties window, set the Analysis Type property to 2D.

The Project Schematic should appear as follows:

Launch Mechanical. Right-click the Model cell and then choose Edit. (Tip: You can also double-click the cell to launch Mechanical).

Define unit system. From the Home tab, open the Units drop-down menu and select Metric (mm, kg, N, s, mV, mA).

Select the Geometry folder.

In the Details pane, set the 2D Behavior property to Plane Strain. This constrains all of the UZ degrees of freedom. See the 2D Analyses section of the Mechanical User's Guide for additional information about this property.

Expand the Connections folder and the Contacts folder. A Contact Region object was automatically generated for the entire interface of the two parts.

Select the Edge selection filter (on the Graphics Toolbar) and highlight an edge in the center of the model. Using the Depth Picking tool, select the first rectangle in the stack, and then scope the edge as the geometry (Apply in the Contact property).

This tutorial employs the Depth Picking tool because of the close proximity of the two edges involved in the interface. As illustrated here, the graphics window displays a stack of rectangles in the lower left corner. The rectangles are stacked in appearance, with the topmost rectangle representing the visible (selected) geometry and subsequent rectangles representing additional geometry selections. For this example, the topmost geometry is the "high" edge.

Select the Edge selection filter and highlight an edge in the center of the model. Using the Depth Picking tool, select the second rectangle in the stack, and then scope the edge as the geometry (Apply in the Target property).

Verify that Bonded is selected as the contact Type and that Pure Penalty is set as the Formulation.

Rename the contact "Body".

Select the Mesh object. Define the following Mesh object properties:

Right-click the Mesh object and select Insert>Sizing. This mesh sizing control should be scoped to the four side edges.

In the Details view, enter 0.75 mm as the Element Size.

Select the Edge selection filter (on the Graphics Toolbar) and highlight an edge in the center of the model. Use the Depth Picking tool and, holding the Ctrl key, select both rectangles in the lower left corner of the graphics window. Continue to hold the Ctrl key, and select an edge of the crack. Again, use the Depth Picking tool and select both rectangles in the lower left corner of the graphics window. Still holding the Ctrl key, select the top and bottom edges on the model.

Right-click the Mesh object and select Insert>Sizing. This mesh sizing control should be scoped to six (top and bottom and the four interface edges) edges.

In the Details view, enter 0.5 mm as the Element Size.

Right-click the Mesh object and select Generate Mesh.

Insert a Fracture folder by highlighting the Model object and then selecting the Fracture option in the Define group of the on the Model Context tab.

Insert a Contact Debonding object by selecting the Contact Debonding option from the Model group on the Fracture Context tab.

In the Details pane, set the Material property to CZM Crack Material.

In the Details pane, set the Contact Region property to Body.

The Contact Debonding object is complete.

Select the Analysis Settings object.

Set the Auto Time Setting property to On and then enter 100 for the Initial Substeps, Minimum Substeps, and Maximum Substeps properties.

Select the Edge selection filter and select the two edges on the side of the model that is opposite of the crack. Select one edge, press the Ctrl key, and then select the next edge.

Highlight the Static Structural object and select the Fixed option from the Structural group of the Environment Context tab.

Highlight the Static Structural object. With the Vertex selection filter active, select the vertex illustrated below and then select the Displacement option from the Structural group of the Environment Context tab.

In the Details pane, enter 10 (mm in the positive Y direction) as the loading value for the Y Component property.

Create another Displacement. With the Vertex selection filter active, select the bottom vertex, and then select the Displacement option. Enter -10 (mm in the negative Y direction) as the loading value for the Y Component property.

Highlight the Solution object, select the Deformation menu on the Solution Context Toolbar, and then select Directional Deformation.

Under the Definition category in the Details view, set the Orientation property to Y Axis.

Highlight the Solution object, select the Probe menu on the Solution Context Toolbar, and then select Force Reaction.

Select Displacement for the Boundary Condition property of the probe.

Click the Solve button.

Highlight the Directional Deformation and Force Reaction objects. Results appear as follows: