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.


  1. Give example a Title Utility Menu > File > Change Title ...
    /title, NonLinear Materials

  2. Create Keypoints Preprocessor > Modeling > Create > Keypoints > In Active CS
    /PREP7
    K,#,X,Y

    We are going to define 2 keypoints (the beam vertices) for this structure to create a beam with a length of 100 millimeters:

    Keypoint Coordinates (x,y)
    1 (0,0)
    2 (0,100)

  3. Define Lines Preprocessor > Modeling > Create > Lines > Lines > Straight Line

    Create a line between Keypoint 1 and Keypoint 2.
    L,1,2

  4. Define Element Types
  5. Preprocessor > Element Type > Add/Edit/Delete...

    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.

  6. Define Real Constants
  7. Preprocessor > Real Constants... > Add...

    In the 'Real Constants for LINK1' window, enter the following geometric properties:

    1. Cross-sectional area AREA: 25
    2. Initial Strain: 0

    This defines an element with a solid rectangular cross section 5 x 5 millimeters.

  8. 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: 75e3
    2. Poisson's Ratio PRXY: 0.3

    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.

    Curve Points Strain Stress
    1 0 0
    2 0.001 75
    3 0.002 150
    4 0.003 225
    5 0.004 240
    6 0.005 250
    7 0.025 300
    8 0.060 355
    9 0.100 390
    10 0.150 420
    11 0.200 435
    12 0.250 449
    13 0.275 450

    To get the problem geometry back, select Utility Menu > Plot > Replot.
    /REPLOT

  9. Define Mesh Size Preprocessor > Meshing > Manual Size > Size Cntrls > Lines > All Lines...

    For this example we will specify an element edge length of 5 mm (20 element divisions along the line).

  10. Mesh the frame Preprocessor > Meshing > Mesh > Lines > click 'Pick All'
    LMESH,ALL

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

  3. Set Solution Controls

  4. Apply Constraints
  5. Solution > Define Loads > Apply > Structural > Displacement > On Keypoints

    Fix Keypoint 1 (ie all DOFs constrained).

  6. Apply Loads
  7. Solution > Define Loads > Apply > Structural > Force/Moment > On Keypoints

    Place a 10,000 N load in the FY direction on the top of the beam (Keypoint 2).

  8. Solve the System
  9. Solution > Solve > Current LS
    SOLVE

    The following will appear on your screen for NonLinear Analyses

    This shows the convergence of the solution.

  1. To view the element in 2D rather than a line: Utility Menu > PlotCtrls > Style > Size and Shape and turn 'Display of element' ON (as shown below).

  2. View the deflection contour plot General Postproc > Plot Results > Contour Plot > Nodal Solu... > DOF solution, UY
    PLNSOL,U,Y,0,1

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.

  1. Define Variables

  2. Graph Results over Time

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.