This tutorial was created using ANSYS 7.0 to solve a simple 2D Truss problem. This is the first of four introductory ANSYS tutorials.

Determine the nodal deflections, reaction forces, and stress for the truss system shown below (E = 200GPa, A = 3250mm2).

Truss Bridge Geometry

(Modified from Chandrupatla & Belegunda, Introduction to Finite Elements in Engineering, p.123)


  1. Give the Simplified Version a Title (such as 'Bridge Truss Tutorial').

    In the Utility menu bar select File > Change Title:

    ANSYS/ResearchFS Utility Menu

    The following window will appear:

    Change Title

    Enter the title and click 'OK'. This title will appear in the bottom left corner of the 'Graphics' Window once you begin. Note: to get the title to appear immediately, select Utility Menu > Plot > Replot

  2. Enter Keypoints

    The overall geometry is defined in ANSYS using keypoints which specify various principal coordinates to define the body. For this example, these keypoints are the ends of each truss.

    • We are going to define 7 keypoints for the simplified structure as given in the following table
      keypointcoordinate
      x y
      100
      218003118
      336000
      454003118
      572000
      690003118
      7108000
      (these keypoints are depicted by numbers in the above figure)

    • From the 'ANSYS Main Menu' select:
      Preprocessor > Modeling > Create > Keypoints > In Active CS

      ANSYS Main Menu

      The following window will then appear:

    • To define the first keypoint which has the coordinates x = 0 and y = 0:
      Enter keypoint number 1 in the appropriate box, and enter the x,y coordinates: 0, 0 in their appropriate boxes (as shown above).
      Click 'Apply' to accept what you have typed.

    • Enter the remaining keypoints using the same method.

      Note: When entering the final data point, click on 'OK' to indicate that you are finished entering keypoints. If you first press 'Apply' and then 'OK' for the final keypoint, you will have defined it twice!
      If you did press 'Apply' for the final point, simply press 'Cancel' to close this dialog box.

    Units
    Note the units of measure (ie mm) were not specified. It is the responsibility of the user to ensure that a consistent set of units are used for the problem; thus making any conversions where necessary.

    Correcting Mistakes
    When defining keypoints, lines, areas, volumes, elements, constraints and loads you are bound to make mistakes. Fortunately these are easily corrected so that you don't need to begin from scratch every time an error is made! Every 'Create' menu for generating these various entities also has a corresponding 'Delete' menu for fixing things up.

  3. Form Lines
  4. The keypoints must now be connected

    We will use the mouse to select the keypoints to form the lines.

    Disappearing Lines
    Please note that any lines you have created may 'disappear' throughout your analysis. However, they have most likely NOT been deleted. If this occurs at any time from the Utility Menu select:

    Plot > Lines

  5. Define the Type of Element
  6. It is now necessary to create elements. This is called 'meshing'. ANSYS first needs to know what kind of elements to use for our problem:

  7. Define Geometric Properties
  8. We now need to specify geometric properties for our elements:

  9. Element Material Properties
  10. You then need to specify material properties:

  11. Mesh Size
  12. The last step before meshing is to tell ANSYS what size the elements should be. There are a variety of ways to do this but we will just deal with one method for now.

  13. Mesh
  14. Now the frame can be meshed.

    Your model should now appear as shown in the following window

    Truss Outline

Plot Numbering
To show the line numbers, keypoint numbers, node numbers...

Saving Your Work

Save the model at this time, so if you make some mistakes later on, you will at least be able to come back to this point. To do this, on the Utility Menu select File > Save as.... Select the name and location where you want to save your file.

It is a good idea to save your job at different times throughout the building and analysis of the model to backup your work in case of a system crash or what have you.


You have now defined your model. It is now time to apply the load(s) and constraint(s) and solve the the resulting system of equations.

Open up the 'Solution' menu (from the same 'ANSYS Main Menu').

  1. Define Analysis Type
  2. First you must tell ANSYS how you want it to solve this problem:

  3. Apply Constraints
  4. It is necessary to apply constraints to the model otherwise the model is not tied down or grounded and a singular solution will result. In mechanical structures, these constraints will typically be fixed, pinned and roller-type connections. As shown above, the left end of the truss bridge is pinned while the right end has a roller connection.

  5. Apply Loads
  6. As shown in the diagram, there are four downward loads of 280kN, 210kN, 280kN, and 360kN at keypoints 1, 3, 5, and 7 respectively.

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

    [Loads & Constraints]

  7. Solving the System
  8. We now tell ANSYS to find the solution:


  1. Hand Calculations
  2. We will first calculate the forces and stress in element 1 (as labeled in the problem description).

  3. Results Using ANSYS
  4. Reaction Forces

    A list of the resulting reaction forces can be obtained for this element

    Deformation

    Deflection

    Axial Stress

    For line elements (ie links, beams, spars, and pipes) you will often need to use the Element Table to gain access to derived data (ie stresses, strains). For this example we should obtain axial stress to compare with the hand calculations. The Element Table is different for each element, therefore, we need to look at the help file for LINK1 (Type help link1 into the Input Line). From Table 1.2 in the Help file, we can see that SAXL can be obtained through the ETABLE, using the item 'LS,1'

    Note that the axial stress in Element 1 is 82.9MPa as predicted analytically.


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.

To quit ANSYS, select 'QUIT' from the ANSYS Toolbar or select Utility Menu/File/Exit.... In the dialog box that appears, click on 'Save Everything' (assuming that you want to) and then click on 'OK'.