This tutorial was created using ANSYS 7.0 to solve a simple buckling problem.

It is recommended that you complete the NonLinear Tutorial prior to beginning this tutorial

Buckling loads are critical loads where certain types of structures become unstable. Each load has an associated buckled mode shape; this is the shape that the structure assumes in a buckled condition. There are two primary means to perform a buckling analysis:

  1. Eigenvalue

    Eigenvalue buckling analysis predicts the theoretical buckling strength of an ideal elastic structure. It computes the structural eigenvalues for the given system loading and constraints. This is known as classical Euler buckling analysis. Buckling loads for several configurations are readily available from tabulated solutions. However, in real-life, structural imperfections and nonlinearities prevent most real-world structures from reaching their eigenvalue predicted buckling strength; ie. it over-predicts the expected buckling loads. This method is not recommended for accurate, real-world buckling prediction analysis.

  2. Nonlinear

    Nonlinear buckling analysis is more accurate than eigenvalue analysis because it employs non-linear, large-deflection, static analysis to predict buckling loads. Its mode of operation is very simple: it gradually increases the applied load until a load level is found whereby the structure becomes unstable (ie. suddenly a very small increase in the load will cause very large deflections). The true non-linear nature of this analysis thus permits the modeling of geometric imperfections, load perterbations, material nonlinearities and gaps. For this type of analysis, note that small off-axis loads are necessary to initiate the desired buckling mode.

This tutorial will use a steel beam with a 10 mm X 10 mm cross section, rigidly constrained at the bottom. The required load to cause buckling, applied at the top-center of the beam, will be calculated.


  1. Open preprocessor menu /PREP7
  2. Give example a Title Utility Menu > File > Change Title ...
    /title,Eigen-Value Buckling Analysis

  3. Define Keypoints Preprocessor > Modeling > Create > Keypoints > In Active CS ...
    K,#,X,Y

    We are going to define 2 Keypoints for this beam as given in the following table:

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

  4. Create Lines Preprocessor > Modeling > Create > Lines > Lines > In Active Coord
    L,1,2

    Create a line joining Keypoints 1 and 2

  5. Define the Type of Element
  6. 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 axes, and rotation about the Z axis).

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

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

    1. Cross-sectional area AREA: 100
    2. Area moment of inertia IZZ: 833.333
    3. Total Beam Height HEIGHT: 10

    This defines a beam with a height of 10 mm and a width of 10 mm.

  9. 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: 200000
    2. Poisson's Ratio PRXY: 0.3

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

    For this example we will specify an element edge length of 10 mm (10 element divisions along the line).

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

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

  3. Activate prestress effects

    To perform an eigenvalue buckling analysis, prestress effects must be activated.

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

    Fix Keypoint 1 (ie all DOF constrained).

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

    The eignenvalue solver uses a unit force to determine the necessary buckling load. Applying a load other than 1 will scale the answer by a factor of the load.

    Apply a vertical (FY) point load of -1 N to the top of the beam (keypoint 2).

    The applied loads and constraints should now appear as shown in the figure below.

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

  10. Exit the Solution processor
  11. Close the solution menu and click FINISH at the bottom of the Main Menu.
    FINISH

    Normally at this point you enter the postprocessing phase. However, with a buckling analysis you must re-enter the solution phase and specify the buckling analysis. Be sure to close the solution menu and re-enter it or the buckling analysis may not function properly.

  12. Define Analysis Type
  13. Solution > Analysis Type > New Analysis > Eigen Buckling
    ANTYPE,1

  14. Specify Buckling Analysis Options

  15. Solve the System
  16. Solution > Solve > Current LS
    SOLVE

  17. Exit the Solution processor
  18. Close the solution menu and click FINISH at the bottom of the Main Menu.
    FINISH

    Again it is necessary to exit and re-enter the solution phase. This time, however, is for an expansion pass. An expansion pass is necessary if you want to review the buckled mode shape(s).

  19. Expand the solution

  20. Solve the System
  21. Solution > Solve > Current LS
    SOLVE

  1. View the Buckling Load

    To display the minimum load required to buckle the beam select General Postproc > List Results > Detailed Summary. The value listed under 'TIME/FREQ' is the load (41,123), which is in Newtons for this example. If more than one mode was selected in the steps above, the corresponding loads would be listed here as well.
    /POST1
    SET,LIST
  2. Display the Mode Shape

Ensure that you have completed the NonLinear Tutorial prior to beginning this portion of the tutorial

  1. Open preprocessor menu /PREP7

  2. Give example a Title Utility Menu > File > Change Title ...
    /TITLE, Nonlinear Buckling Analysis

  3. Create Keypoints Preprocessor > Modeling > Create > Keypoints > In Active CS
    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)

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

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

  5. Define Element Types
  6. 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.

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

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

    1. Cross-sectional area AREA: 100
    2. Area Moment of Inertia IZZ: 833.333
    3. Total beam height HEIGHT: 10

    This defines an element with a solid rectangular cross section 10 x 10 millimeters.

  9. 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: 200e3
    2. Poisson's Ratio PRXY: 0.3

  10. Define Mesh Size Preprocessor > Meshing > Size Cntrls > Lines > All Lines...

    For this example we will specify an element edge length of 1 mm (100 element divisions along the line).
    ESIZE,1

  11. 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 -50,000 N load in the FY direction on the top of the beam (Keypoint 2). Also apply a -250 N load in the FX direction on Keypoint 2. This horizontal load will persuade the beam to buckle at the minimum buckling load.

    The model should now look like the window shown below.

  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. View the deformed shape

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.