This tutorial was completed using ANSYS 7.0. The purpose of this tutorial is to explain how to apply distributed loads and use element tables to extract data. Please note that this material was also covered in the 'Bicycle Space Frame' tutorial under 'Basic Tutorials'.

A distributed load of 1000 N/m (1 N/mm) will be applied to a solid steel beam with a rectangular cross section as shown in the figure below. The cross-section of the beam is 10mm x 10mm while the modulus of elasticity of the steel is 200GPa.

  1. Open preprocessor menu /PREP7

  2. Give example a Title Utility Menu > File > Change Title ...
    /title, Distributed Loading

  3. 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 (1000,0)

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

    Create a line between Keypoint 1 and Keypoint 2.

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

    For this problem we will use the BEAM3 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: 100
    2. Area Moment of Inertia IZZ: 833.333
    3. Total beam height HEIGHT: 10

    This defines an element with a solid rectangular cross section 10mm x 10mm.

  9. 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

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

    For this example we will use an element length of 100mm.

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

  12. Plot Elements Utility Menu > Plot > Elements

    You may also wish to turn on element numbering and turn off keypoint numbering

    Utility Menu > PlotCtrls > Numbering ...

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

  3. Apply Constraints
  4. Solution > Define Loads > Apply > Structural > Displacement > On Keypoints

    Pin Keypoint 1 (ie UX and UY constrained) and fix Keypoint 2 in the y direction (UY constrained).

  5. Apply Loads
  6. We will apply a distributed load, of 1000 N/m or 1 N/mm, over the entire length of the beam.

    The applied loads and constraints should now appear as shown in the figure below.


    To have the constraints and loads appear each time you select 'Replot' you must change some settings. Select Utility Menu > PlotCtrls > Symbols.... In the window that appears, select 'Pressures' in the pull down menu of the 'Surface Load Symbols' section.

  7. Solve the System
  8. Solution > Solve > Current LS

  1. Plot Deformed Shape General Postproc > Plot Results > Deformed Shape

  2. Plot Principle stress distribution

    As shown previously, we need to use element tables to obtain principle stresses for line elements.

    1. Select General Postproc > Element Table > Define Table

    2. Click 'Add...'

    3. In the window that appears
      1. enter 'SMAXI' in the 'User Label for Item' section
      2. In the first window in the 'Results Data Item' section scroll down and select 'By sequence num'
      3. In the second window of the same section, select 'NMISC, '
      4. In the third window enter '1' anywhere after the comma

    4. click 'Apply'

    5. Repeat steps 2 to 4 but change 'SMAXI' to 'SMAXJ' in step 3a and change '1' to '3' in step 3d.
    6. Click 'OK'. The 'Element Table Data' window should now have two variables in it.
    7. Click 'Close' in the 'Element Table Data' window.
    8. Select: General Postproc > Plot Results > Line Elem Res...

    9. Select 'SMAXI' from the 'LabI' pull down menu and 'SMAXJ' from the 'LabJ' pull down menu


    As shown in the plot below, the maximum stress occurs in the middle of the beam with a value of 750 MPa.

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.