This tutorial was completed using ANSYS 7.0 The purpose of the tutorial is to describe how to utilize contact elements to simulate how two beams react when they come into contact with each other.
The beams, as shown below, are 100mm long, 10mm x 10mm in cross-section, have a Young's modulus of 200 GPa, and are rigidly constrained at the outer ends. A 10KN load is applied to the center of the upper, causing it to bend and contact the lower.
We are going to define 2 rectangles as described in the following table:
| Rectangle | Variables (WP X,WP Y,Width,Height) |
| 1 | (0, 15, 100, 10) |
| 2 | (50, 0, 100, 10) |
For this problem we will use the PLANE42 (Solid, Quad 4node 42) element. This element has 2 degrees of freedom at each node (translation along the X and Y).
In the 'Real Constants for PLANE42' window, enter the following geometric properties:
This defines a beam with a thickness of 10 mm.
In the window that appears, enter the following geometric properties for steel:
For this example we will use an element edge length of 2mm.
For this problem we will use the CONTAC48 (Contact, pt-to-surf 48) element. CONTAC48 may be used to represent contact and sliding between two surfaces (or between a node and a surface) in 2-D. The element has two degrees of freedom at each node: translations in the nodal x and y directions. Contact occurs when the contact node penetrates the target line.
It is important to note, CONTAC48 elements are created in the space between two surfaces prescribed by the user. This will be covered below. As the surfaces approach each other, the contact element is slowly "crushed" until it's upper node(s) lie along the same line as the lower node(s). Thus, ANSYS can calculate when the two prescribed surfaces have made contact. Other contact elements, such as CONTA175, require a target element, such as TARGE169, to function. When using contact elements in your own analyses, be sure to understand how the elements work. The ANSYS help file has plenty of useful information regarding contact elements and is worth reading.
In the 'Real Constants for CONTAC48' window, enter the following properties:
The other real constants can be used to model sliding friction, tolerances, etc. Information about these other constants can be found in the help file.
First, the source nodes will be selected.
It is important to try and limit the number of nodes you use to create contact elements. If you have a lot of contact elements, it takes a great deal of computational time to reach a solution. In this case, the only nodes that could make contact with the lower beam are those directly above it, thus those are the only nodes we will use to create the contact elements.
Now select the target nodes.
Using the same procedure as above, select the nodes on the lower beam directly
under the upper beam. Be sure to reselect all nodes before starting to select
others. This is done by opening the entity select menu, Utility Menu >
Select > Entities..., clicking the Also Select radio button, and
click the Sele All button.
These values will be the ones you'll use.
When creating the component this time, enter the name Target.
IMPORTANT: Be sure to reselect all the nodes before continuing. This is done by opening the entity select menu, Utility Menu > Select > Entities..., clicking the Also Select radio button, and click the Sele All button.
Fill the window in as shown below. This ensures ANSYS knows that you are dealing with the contact elements and the associated real constants.
Main Menu > Preprocessor > Modeling> Create > Elements > Surf / Contact > Node to Surf
The following window will pop up. Select the node set SOURCE from the first drop down menu (Ccomp) and TARGET from the second drop down menu (Tcomp). The rest of the selections remain unchanged.
At this point, your model should look like the following.
Unfortunately, the contact elements don't get plotted on the screen so it is sometimes difficult to tell they are there. If you wish, you can plot the elements (Utility Menu > Plot > Elements) and turn on element numbering (Utility Menu > PlotCtrls > Numbering > Elem/Attrib numbering > Element Type Numbers). If you zoom in on the contact areas, you can see little purple stars (Contact Nodes) and thin purple lines (Target Elements) numbered "2" which correspond to the contact elements, shown below.
The preprocessor stage is now complete.
The following image will appear:
Ensure the following selections are made under the 'Basic' tab (as shown above)
Ensure the following selection is made under the 'Nonlinear' tab (as shown below)
NOTE
There are several options which have not been changed from their default values.
For more information about these commands, type help followed by the command into the command line.
These solution control values are extremely important in determining if your analysis will succeed or fail. If you have too few substeps, the contact nodes may be driven through the target elements before ANSYS "realizes" it has happened. In this case the solution will resemble that of an analysis that didn't have contact elements defined at all. Therefore it is important to choose a relatively large number of substeps initially to ensure the model is defined properly. Once everything is working, you can reduce the number of substeps to optimize the computational time. Also, if the maximum number of substeps or iterations is left too low, ANSYS may stop the analysis before it has a chance to converge to a solution. Again, leave these relatively high at first.
Fix the left end of the upper beam and the right end of the lower beam (ie all DOF constrained)
Apply a load of -10000 in the FY direction to the center of the top surface of the upper beam. Note, this is a point load on a 2D surface. This type of loading should be avoided since it will cause a singularity. However, the displacement or stress near the load is not of interest in this analyis, thus we will use a point load for simplicity.
The applied loads and constraints should now appear as shown in the figure below.
Click the 1.0 (true scale) radio button, then click ok. This is of huge importance! I lost many hours trying to figure out why the contact elements weren't working, when in fact it was just due to the displacement scaling to which ANSYS defaulted. If you leave the scaling as default, many times it will look like your contact nodes have gone through the target elements.
Fill in the window as follows:
This should produce the following stress distribution plot:
As seen in the figure, the load on the upper beam caused it to deflect and come in contact with the lower beam, producing a stress distribution in both.
