Creating the analysis steps

The analysis that you perform on the hinge model will consist of an initial step and two general analysis steps:

  • In the initial step you apply boundary conditions to regions of the model and define contact between regions of the model.

  • In the first general analysis step you allow contact to become established.

  • In the second general analysis step you modify two of the boundary conditions applied to the model and apply a pressure load to one of the hinge pieces.

Abaqus/CAE creates the initial step by default, but you must create the two analysis steps.

  1. In the Model Tree, double-click the Steps container to create a new step.

    The Create Step dialog box appears.

  2. In the Create Step dialog box:
    1. Name the step Contact.
    2. Accept the default procedure type (Static, General), and click Continue.

    The step editor appears.

  3. In the Description field, type Establish contact.
  4. Click the Incrementation tab, and delete the value of 1 that appears in the Initial text field. Type a value of 0.1 for the initial increment size.
  5. Click OK to create the step and to exit the editor.

    The Contact step appears underneath the Steps container in the Model Tree.

  6. Use the same technique to create a second general, static step named Load. Enter Apply load in the description field and an initial increment size of 0.1.

    The Load step appears underneath the Steps container in the Model Tree.