This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to outline the steps required to do a simple nonlinear analysis of the beam shown below.

There are several causes for nonlinear behaviour such as Changing Status (ex. contact elements), Material Nonlinearities and Geometric Nonlinearities (change in response due to large deformations). This tutorial will deal specifically with Geometric Nonlinearities .

To solve this problem, the load will added incrementally. After each increment, the stiffness matrix will be adjusted before increasing the load.

The solution will be compared to the equivalent solution using a linear response.


  1. Give example a Title Utility Menu > File > Change Title ...

  2. Create Keypoints Preprocessor > Modeling > Create > Keypoints > In Active CS

    We are going to define 2 keypoints (the beam vertices) for this structure to create a beam with a length of 5 inches:

    Keypoint Coordinates (x,y)
    1 (0,0)
    2 (5,0)

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

    Create a line between Keypoint 1 and Keypoint 2.

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

    For this problem we will use the BEAM3 (Beam 2D elastic) element. This element has 3 degrees of freedom (translation along the X and Y axis's, and rotation about the Z axis). With only 3 degrees of freedom, the BEAM3 element can only be used in 2D analysis.

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

    In the 'Real Constants for BEAM3' window, enter the following geometric properties:

    1. Cross-sectional area AREA: 0.03125
    2. Area Moment of Inertia IZZ: 4.069e-5
    3. Total beam height HEIGHT: 0.125

    This defines an element with a solid rectangular cross section 0.25 x 0.125 inches.

  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: 30e6
    2. Poisson's Ratio PRXY: 0.3

    If you are wondering why a 'Linear' model was chosen when this is a non-linear example, it is because this example is for non-linear geometry, not non-linear material properties. If we were considering a block of wood, for example, we would have to consider non-linear material properties.

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

    For this example we will specify an element edge length of 0.1 " (50 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 -100 lb*in moment in the MZ direction at the right end of the beam (Keypoint 2)

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

    The following will appear on your screan for NonLinear Analyses

    This shows the convergence of the solution.


  1. View the deformed shape General Postproc > Plot Results > Deformed Shape... > Def + undeformed
    PLDISP,1

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

  3. List Horizontal Displacement If this example is performed as a linear model there will be no nodal deflection in the horizontal direction due to the small deflections assumptions. However, this is not realistic for large deflections. Modeling the system non-linearly, these horizontal deflections are calculated by ANSYS.
    General Postproc > List Results > Nodal Solution...> DOF solution, UX

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 and the step sizes of the load.

As you recall, the load was applied in steps. The step size was automatically determined in ANSYS

  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.