5.5.7.3. Interface Delamination and Ansys Composite PrepPost (ACP)

Mechanical allows you to import interface layer(s) from the Ansys Composite PrepPost (ACP) application. You can define interface layers in ACP, import them into Mechanical, and use them to define Interface Delamination objects. You can automatically insert Interface Delamination objects into the Fracture folder when importing composite section data into Mechanical by setting the Create Delamination Objects property (see Specifying Options) to Yes. Alternatively, you can generate Interface Delamination objects automatically after you have imported Composite Section data by selecting the Generate All Interface Delaminations option in the context menu of the Fracture object.

Unexpected Penetration during Nonlinear Analysis

If you experience penetration at the interface layers during separation, you may wish to create a Contact condition for the interface where the penetration is taking place. A Contact Region can be applied to a Pre-Generated Interface provided by ACP. Although all contact Type settings are supported for Pre-Generated Interfaces, the Frictionless setting is recommended for this case when specifying the contact condition. Other contact properties can be set to the default, Program Controlled, settings.

Apply Interface Delamination via ACP

To specify Interface Delamination using the ACP application:

Note:  The following steps assume that you have properly defined your interface layer in the ACP application.

VCCT Method (Default)

  1. From the Workbench Project page, link your Static Structural or Transient Structural analysis to the ACP (Pre) system and then launch Mechanical.

    A Fracture folder is automatically created and includes an Interface Delamination object.

  2. Select the new Interface Delamination object.

  3. Specify the Failure Criteria Option property: either Energy-Release Rate (default) or Material Data Table.

  4. Based on the selected Failure Criteria Option:

    • If specified as Energy-Release Rate: enter a Critical Rate value. This value determines the energy release rate in one direction.

    • If specified as Material Data Table: specify a Material. This property defines the energy release rate in all three fracture modes. This property is defined in ACP.

  5. The automatic setting for the Generation Method property is Pre-Generated Interface. Accept this setting.

  6. As necessary, select the appropriate Interface Layer from the Interface property drop-down menu.

  7. Define the Initial Crack by selecting the Pre-Meshed Crack created by ACP.

  8. Specify the Auto Time Stepping property as either Program Controlled (default) or Manual. The following properties can be modified if Manual is selected, otherwise they are read-only.

    1. Initial Time Step

    2. Minimum Time Step

    3. Maximum Time Step

    Note:

    • The Auto Time Stepping property must be set to On in the Step Controls category of the Analysis Setting object.

    • Time stepping values take effect when crack growth is detected.

CZM Method

  1. From the Workbench Project page, link your Static Structural or Transient Structural analysis to the ACP (Pre) system and then launch Mechanical.

    A Fracture folder is automatically created and includes an Interface Delamination object.

  2. Select the new Interface Delamination object.

  3. Specify the Material property. This property provides a fly-out menu to make a material selection that was defined in the ACP (Pre) system.

  4. The automatic setting for the Generation Method property is Pre-Generated Interface. Accept this setting.

  5. As necessary, select the appropriate Interface Layer from the Interface property drop-down menu.