This tutorial was completed using ANSYS 7.0 This tutorial is intended to outline the steps required to create an axisymmetric model.

The model will be that of a closed tube made from steel. Point loads will be applied at the center of the top and bottom plate to make an analytical verification simple to calculate. A 3/4 cross section view of the tube is shown below.

As a warning, point loads will create discontinuities in the your model near the point of application. If you chose to use these types of loads in your own modelling, be very careful and be sure to understand the theory of how the FEA package is appling the load and the assumption it is making. In this case, we will only be concerned about the stress distribution far from the point of application, so the discontinuities will have a negligable effect.


  1. Give example a Title Utility Menu > File > Change Title ...
    /title, Axisymmetric Tube

  2. Open preprocessor menu ANSYS Main Menu > Preprocessor
    /PREP7

  3. Create Areas Preprocessor > Modeling > Create > Areas > Rectangle > By Dimensions
    RECTNG,X1,X2,Y1,Y2

    For an axisymmetric problem, ANSYS will rotate the area around the y-axis at x=0. Therefore, to create the geometry mentioned above, we must define a U-shape.

    We are going to define 3 overlapping rectangles as defined in the following table:

    Rectangle X1 X2 Y1 Y2
    1 0 20 0 5
    2 15 20 0 100
    3 0 20 95 100

  4. Add Areas Together Preprocessor > Modeling > Operate > Booleans > Add > Areas
    AADD,ALL

    Click the Pick All button to create a single area.

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

    For this problem we will use the PLANE2 (Structural, Solid, Triangle 6node) element. This element has 2 degrees of freedom (translation along the X and Y axes).

    Many elements support axisymmetry, however if the Ansys Elements Reference (which can be found in the help file) does not discuss axisymmetric applications for a particular element type, axisymmetry is not supported.

  7. Turn on Axisymmetry
  8. While the Element Types window is still open, click the Options... button.

    Under Element behavior K3 select Axisymmetric.

  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 > Areas > All Areas

    For this example we will use an element edge length of 2mm.

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

    Your model should know look like this:


  1. Define Analysis Type
  2. Solution > Analysis Type > New Analysis > Static
    ANTYPE,0

  3. Apply Constraints
  4. Utility Menu > Select > Entities

    In the select entities window, click Sele All to reselect all nodes. It is important to always reselect all entities once you've finished to ensure future commands are applied to the whole model and not just a few entities. Once you've clicked Sele All, click on Cancel to close the window.

  5. Apply Loads
  6. Solve the System
  7. Solution > Solve > Current LS
    SOLVE

  1. Hand Calculations

    Hand calculations were performed to verify the solution found using ANSYS:

    The stress across the thickness at y = 50mm is 0.182 MPa.

  2. Determine the Stress Through the Thickness of the Tube

  3. Plotting the Elements as Axisymmetric Utility Menu > PlotCtrls > Style > Symmetry Expansion > 2-D Axi-symmetric...

    The following window will appear. By clicking on 3/4 expansion you can produce the figure shown at the beginning of this tutorial.

  4. Extra Exercise

    It is educational to repeat this tutorial, but leave out the key option which enables axisymmetric modelling. The rest of the commands remain the same. If this is done, the model is a flat, rectangular plate, with a rectangular hole in the middle. Both the stress distribution and deformed shape change drastically, as expected due to the change in geometry. Thus, when using axisymmetry be sure to verify the solutions you get are reasonable to ensure the model is infact axisymmetric.


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.