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.
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:
Click the Pick All button to create a single area.
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.
Under Element behavior K3 select Axisymmetric.
In the window that appears, enter the following geometric properties for steel:
For this example we will use an element edge length of 2mm.
Your model should know look like this:
Pick the two edges on the left, at x=0, as shown below. By using the symmetry B.C. command, ANSYS automatically calculates which DOF's should be constrained for the line of symmetry. Since the element we are using only has 2 DOF's per node, we could have constrained the lines in the x-direction to create the symmetric boundary conditions.
Select Nodes and By Location from the scroll down menus. Click Y coordinates and type 50 into the input box as shown below, then click OK.
Solution > Define Loads > Apply > Structural > Displacement > On Nodes > Pick All
Constrain the nodes in the y-direction (UY). This is required to constrain the model in space, otherwise it would be free to float up or down. The location to constrain the model in the y-direction (y=50) was chosen because it is along a symmetry plane. Therefore, these nodes won't move in the y-direction according to theory.
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.
Hand calculations were performed to verify the solution found using ANSYS:
The stress across the thickness at y = 50mm is 0.182 MPa.
Select Nodes > By Location > Y coordinates and type 45,55 in the Min,Max box, as shown below and click OK.
The following list should pop up.
The following window will appear. By clicking on 3/4 expansion you can produce the figure shown at the beginning of this tutorial.
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.