This file describes the GUI (Graphic User Interface) steps to create the following cantilever beam in ANSYS.

  1. Open preprocessor menu

  2. Give example a Title Utility Menu > File > Change Title ...

  3. Give example a Jobname Utility Menu > File > Change Jobname ...

    Enter 'Dynamic' for the jobname

  4. Create Keypoints Preprocessor > Modeling > Create > Keypoints > In Active CS

    We are going to define 2 keypoints (the beam vertices) for this structure as given in the following table:

    Keypoint Coordinates (x,y)
    1 (0,0)
    2 (1,0)

  5. Define Lines Preprocessor > Modeling > Create > Lines > Lines > Straight Line

    Create a line between Keypoint 1 and Keypoint 2.

  6. Define Element Types
    7. Preprocessor > Element Type > Add/Edit/Delete...

    For this problem we will use the BEAM3 (Beam 2D elastic) element. This element has 3 degrees of freedom (translation along the X and Y axis's, and rotation about the Z axis). With only 3 degrees of freedom, the BEAM3 element can only be used in 2D analysis.

  7. Define Real Constants
    8. Preprocessor > Real Constants... > Add...

    In the 'Real Constants for BEAM3' window, enter the following geometric properties:

    1. Cross-sectional area AREA: 0.0001
    2. Area Moment of Inertia IZZ: 8.33e-10
    3. Total beam height HEIGHT: 0.01

    This defines an element with a solid rectangular cross section 0.01 m x 0.01 m.

  8. Define Element Material Properties Preprocessor > Material Props > Material Models > Structural > Linear > Elastic > Isotropic

    In the window that appears, enter the following geometric properties for steel:

    1. Young's modulus EX: 2.068e11
    2. Poisson's Ratio PRXY: 0.3

    To enter the density of the material, double click on 'Linear' followed by 'Density' in the 'Define Material Model Behavior' Window

    Enter a density of 7830

    Note: For dynamic analysis, both the stiffness and the material density have to be specified.

  9. Define Mesh Size Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All Lines...

    For this example we will specify 10 element divisions along the line.

  10. Mesh the frame Preprocessor > Meshing > Mesh > Lines > click 'Pick All'

Close this window to return to the Dynamic Analysis Tutorials.