This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to outline the steps required to plot Vertical Deflection vs. Length of the following beam using tables, a special type of array. By plotting this data on a curve, rather than using a contour plot, finer resolution can be achieved.

This tutorial will use a steel beam 400 mm long, with a 40 mm X 60 mm cross section as shown above. It will be rigidly constrained at one end and a -2500 N load will be applied to the other.

  1. Give the example a Title Utility Menu > File > Change Title ...
    /title, Use of Tables for Data Plots

  2. Open preprocessor menu ANSYS Main Menu > Preprocessor

  3. Define Keypoints Preprocessor > Modeling > Create > Keypoints > In Active CS...

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

    Keypoint Coordinates (x,y,z)
    1 (0,0)
    2 (400,0)

  4. Create Lines Preprocessor > Modeling > Create > Lines > Lines > In Active Coord

    Create a line joining Keypoints 1 and 2

  5. Define the Type of Element
  6. 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 axes, and rotation about the Z axis).

  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: 2400
    2. Area moment of inertia IZZ: 320e3
    3. Total beam height: 40

    This defines a beam with a height of 40 mm and a width of 60 mm.

  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 edge length of 20mm.

  11. Mesh the frame Preprocessor > Meshing > Mesh > Lines > 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 Keypoints

    Fix keypoint 1 (ie all DOF constrained)

  5. Apply Loads
  6. Solution > Define Loads > Apply > Structural > Force/Moment > On Keypoints
    Apply a load of -2500N on keypoint 2.

    The model should now look like the figure below.

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

It is at this point the tables come into play. Tables, a special type of array, are basically matrices that can be used to store and process data from the analysis that was just run. This example is a simplified use of tables, but they can be used for much more. For more information type help in the command line and search for 'Array Parameters'.

  1. Number of Nodes
  2. Since we wish to plot the verticle deflection vs length of the beam, the location and verticle deflection of each node must be recorded in the table. Therefore, it is necessary to determine how many nodes exist in the model. Utility Menu > List > Nodes... > OK. For this example there are 21 nodes. Thus the table must have at least 21 rows.

  3. Create the Table
  4. Enter Data into Table
  5. First, the horizontal location of the nodes will be recorded

  6. Arrange the Data for Ploting
  7. Users familiar with the way ANSYS numbers nodes will realize that node 1 will be on the far left, as it is keypoint 1, node 2 will be on the far right (keypoint 2), and the rest of the nodes are numbered sequentially from left to right. Thus, the second row in the table contains the data for the last node. This causes problems during plotting, thus the information for the last node must be moved to the final row of the table. This is why a table with 22 rows was created, to provide room to move this data.

  8. Plot the Data

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.