This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to outline the steps required to view cross sectional results (Deformation, Stress, etc.) of the following example.

  1. Give example a Title Utility Menu > File > Change Title ...
    /title, Cross-Sectional Results of a Simple Cantilever Beam

  2. Open preprocessor menu ANSYS Main Menu > Preprocessor

  3. Create Block Preprocessor > Modeling > Create > Volumes > Block > By 2 Corners & Z

    Where: Width: 40mm
    Height: 60mm
    Length: 400mm

  4. Define the Type of Element
  5. Preprocessor > Element Type > Add/Edit/Delete...

    For this problem we will use the SOLID45 (3D Structural Solid) element. This element has 8 nodes each with 3 degrees of freedom (translation along the X, Y and Z directions).

  6. 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: 200000
    2. Poisson's Ratio PRXY: 0.3

  7. Define Mesh Size Preprocessor > Meshing > Size Cntrls > ManualSize > Global > Size

    For this example we will use an element size of 20mm.

  8. Mesh the volume Preprocessor > Meshing > Mesh > Volumes > Free > click 'Pick All'

  1. Define Analysis Type
  2. Solution > Analysis Type > New Analysis > Static

  3. Apply Constraints
  4. Solution > Define Loads > Apply > Structural > Displacement > On Areas
    Fix the left hand side (should be labeled Area 1).

  5. Apply Loads
  6. Solution > Define Loads > Apply > Structural > Force/Moment > On Keypoints
    Apply a load of 2500N downward on the back right hand keypoint (Keypoint #7).

  7. Solve the System
  8. Solution > (-Solve-) Current LS

Now since the purpose of this tutorial is to observe results within different cross-sections of the colume, we will first outline the steps required to view a slice.

  1. Deflection

    Before we begin selecting cross sections, let's view deflection of the entire model.

    To illustrate how to take a cross section, let's take one halfway through the beam in the YZ plane

  2. Equivalent Stress

    Again, let's view stresses within the entire model.

  3. Animation

    Now, for something a little more impressive, let's show an animation of the Von Mises stress through the beam. Unfortunately, the ANSYS commands are not as user friendly as they could be... but please bear with me.

The above example was solved using a mixture of the Graphical User Interface (or GUI) and the command language interface of ANSYS. This problem has also been solved using the ANSYS command language interface that you may want to browse. Open the .HTML version, copy and paste the code into Notepad or a similar text editor and save it to your computer. Now go to 'File > Read input from...' and select the file. A .PDF version is also available for printing.