This tutorial was completed using ANSYS 7.0 The purpose of the tutorial is to describe how to include material nonlinearities in an ANSYS model. For instance, the case when a large force is applied resulting in a stresses greater than yield strength. In such a case, a multilinear stress-strain relationship can be included which follows the stress-strain curve of the material being used. This will allow ANSYS to more accurately model the plastic deformation of the material.
For this analysis, a simple tension speciment 100 mm X 5 mm X 5 mm is constrained at the bottom and has a load pulling on the top. This specimen is made out of a experimental substance called "WhoKilledKenium". The stress-strain curve for the substance is shown above. Note the linear section up to approximately 225 MPa where the Young's Modulus is constant (75 GPa). The material then begins to yield and the relationship becomes plastic and nonlinear.
We are going to define 2 keypoints (the beam vertices) for this structure to create a beam with a length of 100 millimeters:
Create a line between Keypoint 1 and Keypoint 2.
For this problem we will use the LINK1 (2D spar) element. This element has 2 degrees of freedom (translation along the X and Y axis's) and can only be used in 2D analysis.
In the 'Real Constants for LINK1' window, enter the following geometric properties:
This defines an element with a solid rectangular cross section 5 x 5 millimeters.
In the window that appears, enter the following geometric properties for steel:
Now that the initial properties of the material have been outlined, the stress-strain data must be included.
Preprocessor > Material Props > Material Models > Structural > Nonlinear > Elastic > Multilinear Elastic
The following window will pop up.
Fill in the STRAIN and STRESS boxes with the following data. These are points from the stress-strain curve shown above, approximating the curve with linear interpolation between the points. When the data for the first point is input, click Add Point to add another. When all the points have been inputed, click Graph to see the curve. It should look like the one shown above. Then click OK.
To get the problem geometry back, select Utility Menu > Plot > Replot. /REPLOT
For this example we will specify an element edge length of 5 mm (20 element divisions along the line).
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)
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.
Fix Keypoint 1 (ie all DOFs constrained).
Place a 10,000 N load in the FY direction on the top of the beam (Keypoint 2).
The following will appear on your screen for NonLinear Analyses
This shows the convergence of the solution.
Other results can be obtained as shown in previous linear static analyses.
As shown, you can obtain the results (such as deflection, stress and bending moment diagrams) the same way you did in previous examples using the General Postprocessor. However, you may wish to view time history results such as the deflection of the object over time.
If it does not open automatically, select Main Menu > TimeHist Postpro > Variable Viewer
This plot shows how the beam deflected linearly when the force, and subsequently the stress, was low (in the linear range). However, as the force increased, the deflection (proportional to strain) began to increase at a greater rate. This is because the stress in the beam is in the plastic range and thus no longer relates to strain linearly. When you verify this example analytically, you will see the solutions are very similar. The difference can be attributed to the ANSYS solver including large deflection calculations.