U of A ANSYS Tutorials - Buckling Page 1 of 16
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.
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 2 of 16
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
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 3 of 16
5. Define the Type of Element
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).
6. Define Real Constants
Preprocessor > Real Constants... > Add...
In the 'Real Constants for BEAM3' window, enter the following geometric properties:
i. Cross-sectional area AREA: 100
ii. Area moment of inertia IZZ: 833.333
iii. Total Beam Height HEIGHT: 10
This defines a beam with a height of 10 mm and a width of 10 mm.
7. 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:
i. Young's modulus EX: 200000
ii. Poisson's Ratio PRXY: 0.3
8. 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).
9. Mesh the frame
Preprocessor > Meshing > Mesh > Lines > click 'Pick All'
LMESH,ALL
1. Define Analysis Type
Solution > Analysis Type > New Analysis > Static
ANTYPE,0
2. Activate prestress effects
To perform an eigenvalue buckling analysis, prestress effects must be activated.
You must first ensure that you are looking at the unabridged solution menu so that you can
select Analysis Options in the Analysis Type submenu. The last option in the solution
menu will either be 'Unabridged menu' (which means you are currently looking at the
abridged version) or 'Abriged Menu' (which means you are looking at the unabridged
menu). If you are looking at the abridged menu, select the unabridged version.
Select Solution > Analysis Type > Analysis Options
In the following window, change the [SSTIF][PSTRES] item to 'Prestress ON', which
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 4 of 16
ensures the stress stiffness matrix is calculated. This is required in eigenvalue buckling
analysis.
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On Keypoints
Fix Keypoint 1 (ie all DOF constrained).
4. Apply Loads
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.
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 5 of 16
5. Solve the System
Solution > Solve > Current LS
SOLVE
6. Exit the Solution processor
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.
7. Define Analysis Type
Solution > Analysis Type > New Analysis > Eigen Buckling
ANTYPE,1
8. Specify Buckling Analysis Options
Select Solution > Analysis Type > Analysis Options
Complete the window which appears, as shown below. Select 'Block Lanczos' as an
extraction method and extract 1 mode. The 'Block Lanczos' method is used for large
symmetric eigenvalue problems and uses the sparse matrix solver. The 'Subspace' method
could also be used, however it tends to converge slower as it is a more robust solver. In
more complex analyses the Block Lanczos method may not be adequate and the Subspace
method would have to be used.
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 6 of 16
9. Solve the System
Solution > Solve > Current LS
SOLVE
10. Exit the Solution processor
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).
11. Expand the solution
Select Solution > Analysis Type > Expansion Pass... and ensure that it is on. You may
have to select the 'Unabridged Menu' again to make this option visible.
Select Solution > Load Step Opts > ExpansionPass > Single Expand > Expand
Modes ...
Complete the following window as shown to expand the first mode
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 7 of 16
12. Solve the System
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
Select General Postproc > Read Results > Last Set to bring up the data for the last mode
calculated.
Select General Postproc > Plot Results > Deformed 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
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 8 of 16
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
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
Preprocessor > Real Constants... > Add...
In the 'Real Constants for BEAM3' window, enter the following geometric properties:
i. Cross-sectional area AREA: 100
ii. Area Moment of Inertia IZZ: 833.333
iii. Total beam height HEIGHT: 10
This defines an element with a solid rectangular cross section 10 x 10 millimeters.
7. 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:
i. Young's modulus EX: 200e3
ii. Poisson's Ratio PRXY: 0.3
8. 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
9. Mesh the frame
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 9 of 16
Preprocessor > Meshing > Mesh > Lines > click 'Pick All'
LMESH,ALL
1. Define Analysis Type
Solution > New Analysis > Static
ANTYPE,0
2. Set Solution Controls
Select Solution > Analysis Type > Sol'n Control...
The following image will appear:
Ensure the following selections are made under the 'Basic' tab (as shown above)
A. Ensure Large Static Displacements are permitted (this will include the effects of large
deflection in the results)
B. Ensure Automatic time stepping is on. Automatic time stepping allows ANSYS to
determine appropriate sizes to break the load steps into. Decreasing the step size
usually ensures better accuracy, however, this takes time. The Automatic Time Step
feature will determine an appropriate balance. This feature also activates the ANSYS
bisection feature which will allow recovery if convergence fails.
C. Enter 20 as the number of substeps. This will set the initial substep to 1/20 th of the
total load.
D. Enter a maximum number of substeps of 1000. This stops the program if the solution
does not converge after 1000 steps.
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 10 of 16
E. Enter a minimum number of substeps of 1.
F. Ensure all solution items are writen to a results file.
Ensure the following selection is made under the 'Nonlinear' tab (as shown below)
A. Ensure Line Search is 'On'. This option is used to help the Newton-Raphson solver
converge.
B. Ensure Maximum Number of Iterations is set to 1000
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.
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On Keypoints
Fix Keypoint 1 (ie all DOFs constrained).
4. Apply Loads
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.
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 11 of 16
5. Solve the System
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
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 12 of 16
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).
General Postproc > Plot Results > Deformed Shape... > Def + undeformed
PLDISP,1
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 13 of 16
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
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 14 of 16
time history results such as the deflection of the object over time.
1. Define Variables
Select: Main Menu > TimeHist Postpro. The following window should open
automatically.
If it does not open automatically, select Main Menu > TimeHist Postpro > Variable
Viewer
Click the add button in the upper left corner of the window to add a variable.
Double-click Nodal Solution > DOF Solution > Y-Component of displacement (as
shown below) and click OK. Pick the uppermost node on the beam and click OK in the
'Node for Data' window.
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 15 of 16
To add another variable, click the add button again. This time select Reaction Forces >
Structural Forces > Y-Component of Force. Pick the lowermost node on the beam and
click OK.
On the Time History Variable window, click the circle in the 'X-Axis' column for FY_3.
This will make the reaction force the x-variable. The Time History Variables window
should now look like this:
2. Graph Results over Time
Click on UY_2 in the Time History Variables window.
Click the graphing button in the Time History Variables window.
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
U of A ANSYS Tutorials - Buckling Page 16 of 16
The labels on the plot are not updated by ANSYS, so you must change them manually.
Select Utility Menu > Plot Ctrls > Style > Graphs > Modify Axes and re-label the X and
Y-axis appropriately.
The plot shows how the beam became unstable and buckled with a load of approximately
40,000 N, the point where a large deflection occured due to a small increase in force. This is
slightly less than the eigen-value solution of 41,123 N, which was expected due to non-
linear geometry issues discussed above.
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.
file://D:\ankur\cad\ansya\ANSYST~1\U%20of%20A%20ANSYS%20Tutorials%20-%20B... 8/7/2007
