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 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.

The properties for the material should appear as follows:

Click the box labeled "Click here to add new material" and enter the name “CZM Material”. This material will specify the formulation used to introduce the fracture mechanism (Cohesive Zone Material method).

Expand the Cohesive Zone option in the Toolbox and right-click Exponential for Interface Delamination. 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 select 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 Tools group on the Home tab, open the Units drop-down menu and select Metric (mm, kg, N, s, mV, mA).

Define 2D behavior.

Apply Material: Expand the Geometry folder and select the Part 2 folder. Set the Assignment property to "Interface Body Material". Selecting the Part 2 folder allows you to assign the material to both parts at the same time.

Suppress Contact.

Right-click the Coordinate Systems object in the tree and select Insert>Coordinate System.

Right-click the new coordinate system object, select Rename, and name the object "High Coordinate System."

In the Details pane of the newly-created Coordinate System object, select the Geometry property field Click to Change.

Select the Edge selection filter (on the Graphics Toolbar) and highlight an edge in the center of the model.

This tutorial employs the Depth Picking tool because of the close proximity of the two edges involved in the interface, as well as the crack. 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.

Click Apply in the Geometry property. The "High Coordinate System" is defined.

Right-click the Coordinate Systems object again and insert another Coordinate System object. Rename this object "Low Coordinate System."

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 Geometry property). This scoping is illustrated below.

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

Right-click the Mesh object and select Insert>Match Control.

Activate the High Geometry Selection property by selecting its field (that is highlighted in yellow). The Apply and Cancel buttons display. Select the Edge selection tool and highlight one of the edges in the center of the model. Use the Depth Picking tool to select the topmost geometry. Click the Apply button.

Perform the same steps to specify the Low Geometry Selection property, as illustrated below.

Change the Transformation property from Cyclic to Arbitrary and specify the High Coordinate System and Low Coordinate System properties using the coordinate systems created in the previous step of the tutorial. The object should appear as illustrated below.

Select the Edge selection filter (on the Graphics Toolbar) and, holding the Ctrl key, select the four side edges.

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 into the tree by highlighting the Model object and selecting the Fracture option from the Define group on the Model Context tab.

Select the Interface Delamination option from the Model group on the Fracture Context tab.

In the Details pane, set the Method property to CZM.

Set the Material property to CZM Material.

Select the Match Control that was created earlier in the tutorial for the Match Control property.

The Interface Delamination object is complete.

Select the Analysis Settings object.

Set the Auto Time Setting property to On and then enter 40 for the Initial Substeps, Minimum Substeps, and Maximum Substeps properties.

In the Details pane, set the Large Deflection property to On to activate geometric nonlinearities.

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 Support option from the Structural group on the Environment Context tab.

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

Highlight the Displacement object in the tree and 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 select the Displacement option from the Structural group on the Environment Context tab. Enter -10 (mm in the negative Y direction) as the loading value for the Y Component property.

Highlight the Solution object. From the Results group of the Solution Context tab, open the Deformation drop-down menu and select Directional.

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

From the Results group of the Solution Context tab, open the Probe drop-down menu and select Force Reaction.

Select Displacement for the Boundary Condition property.

Click the Solve button.

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