Go to the Next Chapter
Go to the Previous Chapter
Go to the Table of Contents for This Manual
Go to the Guides Master Index
Chapter 1 *
Chapter 2 *
Chapter 3 *
Chapter 4 *
Chapter 5 *
Chapter 6 *
Chapter 7 *
Chapter 8 *
Chapter 9 *
Chapter 10 *
Chapter 11 *
Chapter 12 *
Chapter 13 *
Chapter 14
7.1 Definition of Buckling Analysis
Buckling analysis is a technique used to determine buckling loadscritical loads
at which a structure becomes unstableand buckled mode shapesthe
characteristic shape associated with a structure's buckled response.
7.2 Types of Buckling Analyses
Two techniques are available in the ANSYS/Multiphysics, ANSYS/Mechanical,
ANSYS/Structural, and ANSYS/LinearPlus programs for predicting the buckling
load and buckling mode shape of a structure: nonlinear buckling analysis, and
eigenvalue (or linear) buckling analysis. Since these two methods frequently yield
quite different results, let's examine the differences between them before
discussing the details of their implementation.
7.2.1 Nonlinear Buckling Analysis
Nonlinear buckling analysis is usually the more accurate approach and is
therefore recommended for design or evaluation of actual structures. This
technique employs a nonlinear static analysis with gradually increasing loads to
seek the load level at which your structure becomes unstable, as depicted in
Figure 71(a).
Using the nonlinear technique, your model can include features such as initial
imperfections, plastic behavior, gaps, and largedeflection response. In addition,
using deflectioncontrolled loading, you can even track the postbuckled
performance of your structure (which can be useful in cases where the structure
buckles into a stable configuration, such as "snapthrough" buckling of a shallow
dome).
7.2.2 Eigenvalue Buckling Analysis
Eigenvalue buckling analysis predicts the theoretical buckling strength (the
bifurcation point) of an ideal linear elastic structure. (See Figure 71(b).) This
method corresponds to the textbook approach to elastic buckling analysis: for
instance, an eigenvalue buckling analysis of a column will match the classical
Euler solution. However, imperfections and nonlinearities prevent most realworld
structures from achieving their theoretical elastic buckling strength. Thus,
eigenvalue buckling analysis often yields unconservative results, and should
generally not be used in actual daytoday engineering analyses.
Figure 71 (a) Nonlinear loaddeflection curve (b) Linear (Eigenvalue)
buckling curve
7.3 Commands Used in a Buckling Analysis
You use the same set of commands to build a model and perform a buckling
analysis that you use to do any other type of finite element analysis. Likewise, you
choose similar options from the graphical user interface (GUI) to build and solve
models no matter what type of analysis you are doing.
Section 7.7, "Sample Buckling Analysis (Command or Batch Method)," shows you
the sequence of commands you would issue (either manually or while running
ANSYS as a batch job) to perform an example eigenvalue buckling analysis.
Section 7.6, "Sample Buckling Analysis (GUI Method)," shows you how to execute
the same sample analysis using menu choices from the ANSYS GUI. (To learn
how to use the commands and GUI selections for building models, read the ANSYS Modeling and Meshing Guide.)
For detailed, alphabetized descriptions of the ANSYS commands, see the ANSYS Commands Reference.
7.4 Procedure for Nonlinear Buckling
Analysis
A nonlinear buckling analysis is a static analysis with large deflections turned on
[NLGEOM,ON], extended to a point
where the structure reaches its limit load or maximum load. Other nonlinearities
such as plasticity may be included in the analysis. The procedure for a static
analysis is described in Chapter 2, and nonlinearities are described in
Chapter 8.
7.4.1 Applying Load Increments
The basic approach in a nonlinear buckling analysis is to constantly increment the
applied loads until the solution begins to diverge. Be sure to use a sufficiently fine
load increment as your loads approach the expected critical buckling load. If the
load increment is too coarse, the buckling load predicted may not be accurate.
Turn on bisection and automatic time stepping [AUTOTS,ON] to help avoid this problem.
7.4.2 Automatic Time Stepping
With automatic time stepping on, the program automatically seeks out the
buckling load. If automatic time stepping is ON in a static analysis having ramped
loading and the solution does not converge at a given load, the program bisects
the load step increment and attempts a new solution at a smaller load. In a
buckling analysis, each such convergence failure is typically accompanied by a
"negative pivot" message indicating that the attempted load equals or exceeds the
buckling load. You can usually ignore these messages if the program successfully
obtains a converged solution at the next, reduced load. If stress stiffness is active
[SSTIF,ON], you should run without adaptive
descent active [NROPT,FULL,,OFF] to
ensure that a lower bound to the buckling load is attained. The program normally
converges to the limiting load as the process of bisection and resolution
continues to the point at which the minimum time step increment (specified by DELTIM or NSUBST) is achieved. The minimum time
step will directly affect the precision of your results.
Remember that an unconverged solution does not necessarily mean that the
structure has reached its maximum load. It could also be caused by numerical
instability, which might be corrected by refining your modeling technique. Track
the loaddeflection history of your structure's response to decide whether an
unconverged load step represents actual structural buckling, or whether it reflects
some other problem. Perform a preliminary analysis using the arclength method
[ARCLEN] to predict an approximate
value of buckling load. Compare this approximate value to the more precise value
calculated using bisection to help determine if the structure has indeed reached its
maximum load. You can also use the arclength method itself to obtain a precise
buckling load, but this method requires you to adjust the arclength radius by
trialanderror in a series of manually directed reanalyses.
7.4.4 Points to Remember
 If the loading on the structure is perfectly inplane (that is, membrane or
axial stresses only), the outofplane deflections necessary to initiate
buckling will not develop, and the analysis will fail to predict buckling
behavior. To overcome this problem, apply a small outofplane
perturbation, such as a modest temporary force or specified displacement,
to begin the buckling response. (A preliminary eigenvalue buckling
analysis of your structure may be useful as a predictor of the buckling
mode shape, allowing you to choose appropriate locations for applying
perturbations to stimulate the desired buckling response.) The
imperfection (perturbation) induced should match the location and size of
that in the real structure. The failure load is very sensitive to these
parameters.
 In a largedeflection analysis, forces (and displacements) will maintain their
original orientation, but surface loads will "follow" the changing geometry of
the structure as it deflects. Therefore, be sure to apply the proper type of
loads.
 You should carry your stability analysis through to the point of identifying
the critical load in order to calculate the structure's factor of safety with
respect to nonlinear buckling. (Merely establishing the fact that a structure
is stable at a given load level is generally insufficient for most design
practice; you will usually be required to provide a specified safety factor,
which can only be determined by establishing the actual limit load.)
 You can extend your analysis into the postbuckled range by activating the
arclength method [ARCLEN].
Use this feature to trace the loaddeflection curve through regions of
"snapthrough" and "snapback" response.
 For most solid elements, you do not need to use stress stiffening in a
nonlinear buckling analysis. Do not use stress stiffening on "discontinuous"
elements (nonlinear elements that experience sudden discontinuous
changes in stiffness due to status changes, such as various contact
elements, SOLID65, etc.) or on elements
adjacent to discontinuous elements.
 For those elements that support the consistent tangent stiffness matrix (BEAM4, SHELL63, and SHELL181), activate the consistent tangent
stiffness matrix (KEYOPT(2)=1 and NLGEOM,ON) to enhance the
convergence behavior of your nonlinear buckling analyses and improve the
accuracy of your results. This element KEYOPT must be defined before
the first load step of the solution and cannot be changed once the solution
has started.
7.5 Procedure for Eigenvalue Buckling
Analysis
Again, remember that eigenvalue buckling analysis generally yields
unconservative results, and should usually not be used for design of actual
structures. If you decide that eigenvalue buckling analysis is appropriate for your
application, follow this fivestep procedure:
1. Build the model.
2. Obtain the static solution.
3. Obtain the eigenvalue buckling solution.
4. Expand the solution.
5. Review the results.
7.5.1 Build the Model
In this step, you specify the jobname and analysis title and then use PREP7 to
define the element types, element real constants, material properties, and the
model geometry. These tasks are common to most analyses. The ANSYS Modeling and Meshing Guide explains them
in detail.
7.5.1.1 Points to Remember
 Only linear behavior is valid. Nonlinear elements, if any, are treated as
linear. If you include contact elements, for example, their stiffnesses are
calculated based on their status after the static prestress run and are never
changed.
 Young's modulus (EX) (or stiffness in some form) must be defined.
Material properties may be linear, isotropic or orthotropic, and constant or
temperaturedependent. Nonlinear properties, if any, are ignored.
7.5.2 Obtain the Static Solution
The procedure to obtain a static solution is the same as described in Chapter
2, with the following exceptions:
 Prestress effects [PSTRES] must
be activated. Eigenvalue buckling analysis requires the stress stiffness
matrix to be calculated.
 Unit loads are usually sufficient (that is, actual load values need not be
specified). The eigenvalues calculated by the buckling analysis represent
buckling load factors. Therefore, if a unit load is specified, the load factors
represent the buckling loads. All loads are scaled. (Also, the maximum
permissible eigenvalue is 1,000,000you must use larger applied loads if
your eigenvalue exceeds this limit.)
 Note that eigenvalues represent scaling factors for all loads. If certain
loads are constant (e.g., selfweight gravity loads) while other loads are
variable (e.g., externally applied loads), you need to ensure that the stress
stiffness matrix from the constant loads is not factored by the eigenvalue
solution.
One strategy that you can use to achieve this end is to iterate on the
eigensolution, adjusting the variable loads until the eigenvalue becomes
1.0 (or nearly 1.0, within some convergence tolerance). Design
optimization could be useful in driving this iterative procedure to a final
answer.
Consider, for example, a pole having a selfweight W_{0}, which supports an
externallyapplied load, A. To determine the limiting value of A in an
eigenvalue buckling solution, you could solve repetitively, using different
values of A, until by iteration you find an eigenvalue acceptably close to1.0.
Figure 72 Adjusting variable loads to find an eigenvalue of 1.0
 You can apply a nonzero constraint in the prestressing pass as the static
load. The eigenvalues found in the buckling solution will be the load factors
applied to these nonzero constraint values. However, the mode shapes
will have a zero value at these degrees of freedom (and not the nonzero
value specified).
 At the end of the solution, leave SOLUTION [FINISH].
7.5.3 Obtain the Eigenvalue Buckling Solution
This step requires files Jobname.EMAT and Jobname.ESAV from the static
analysis. Also, the database must contain the model geometry data (issue RESUME if necessary). The following tasks
are involved in obtaining the eigenvalue buckling solution:
1. Enter the ANSYS solution processor.
Command(s):
GUI:
Main Menu>Solution
2. Define the analysis type and analysis options. ANSYS offers these options
for a buckling analysis:
Table 71 Analysis types and analysis options
Option

Command

GUI Path

New Analysis

ANTYPE

Main Menu>Solution>Analysis TypeNew
Analysis

Analysis Type: Eigen Buckling

ANTYPE

Main Menu>Solution>Analysis Type
New Analysis>Eigen Buckling

Eigenvalue Extraction Method

BUCOPT

Main Menu>Solution>Analysis Options

No. of Eigenvalues to be Extracted

BUCOPT

Main Menu>Solution>Analysis Options

Shift Point for Eigenvalue Calculation

BUCOPT

Main Menu>Solution>Analysis Options

No. of Reduced Eigenvectors to Print

BUCOPT

Main Menu>Solution>Analysis Options

Each of these options is explained in detail below.
Choose New Analysis. Restarts are not valid in an eigenvalue buckling analysis.
7.5.3.2 Option: Analysis Type: Eigen Buckling [ANTYPE]
Choose Eigen Buckling analysis type.
7.5.3.3 Option: Eigenvalue Extraction Method [BUCOPT]
Choose one of the following solution methods. The Block Lanczos or subspace
iteration methods are generally recommended for eigenvalue buckling because
they use the full system matrices. (If you choose the reduced method, you will
need to define master degrees of freedom before initiating the solution.) See
Section 3.4.2.3, "Option: Mode Extraction Method," in this manual for more
information about these solution methods.
 Reduced (Householder) method
 Block Lanczos method
 Subspace iteration method
7.5.3.4 Option: Number of Eigenvalues to be Extracted [BUCOPT]
Defaults to one, which is usually sufficient for eigenvalue buckling.
7.5.3.5 Option: Shift Point for Eigenvalue Calculation [BUCOPT]
This option represents the point (load factor) about which eigenvalues are
calculated. The shift point is helpful when numerical problems are encountered
(due to negative eigenvalues, for example). Defaults to 0.0.
7.5.3.6 Option: Number of Reduced Eigenvectors to Print [BUCOPT]
This option is valid only for the reduced method. This option allows you to get a
listing of the reduced eigenvectors (buckled mode shapes) on the printed output
file (Jobname.OUT).
3. Specify load step options.
The only load step options valid for eigenvalue buckling are expansion
pass options and output controls. Expansion pass options are explained
next in Section 7.5.4. You can request buckled mode shapes from the
reduced method to be included in the printed output. No other output
control is applicable.
Command(s):
GUI:
Main Menu>Solution>Load Step OptsOutput Ctrls>Solu Printout
4. Save a backup copy of the database to a named file.
Command(s):
GUI:
Utility Menu>File>Save As
5. Start solution calculations.
Command(s):
GUI:
Main Menu>Solution>SolveCurrent LS
The output from the solution mainly consists of the eigenvalues, which are
printed as part of the printed output (Jobname.OUT). The eigenvalues
represent the buckling load factors; if unit loads were applied in the static
analysis, they are the buckling loads. No buckling mode shapes are written
to the database or the results file, so you cannot postprocess the results
yet. To do this, you need to expand the solution (explained next).
Sometimes you may see both positive and negative eigenvalues
calculated. Negative eigenvalues indicate that buckling occurs when the
loads are applied in an opposite sense.
6. Leave the SOLUTION processor.
Command(s):
GUI:
Close the Solution menu.
7.5.4 Expand the Solution
If you want to review the buckled mode shape(s), you must expand the solution
regardless of which eigenvalue extraction method is used. In the case of the
subspace iteration method, which uses full system matrices, you may think of
"expansion" to simply mean writing buckled mode shapes to the results file.
7.5.4.1 Points to Remember
 The mode shape file (Jobname.MODE) from the eigenvalue buckling
solution must be available.
 The database must contain the same model for which the solution was
calculated.
7.5.4.2 Expanding the Solution
The procedure to expand the mode shapes is explained below.
1. Reenter SOLUTION.
Command(s):
GUI:
Main Menu>Solution
NoteYou must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLUTION) before performing the
expansion pass.
2. Activate the expansion pass and its options. The following options are
required for the expansion pass:
Table 72 Expansion pass options
Option

Command

GUI Path

Expansion Pass On/Off

EXPASS

Main Menu>Solution>Load Step OptsExpansionPass>ON

No. of Modes to Expand

MXPAND

Main Menu>Solution>Load Step OptsExpansionPass>
Expand Modes

Stress Calculations On/Off

MXPAND

Main Menu>Solution>Load Step OptsExpansionPass>
Expand Modes

7.5.4.3 Option: Expansion Pass ON/OFF [EXPASS]
Choose ON.
7.5.4.4 Option: Number of Modes to Expand [MXPAND]
Defaults to all modes that were extracted.
7.5.4.5 Option: Stress Calculations On/Off [MXPAND]
"Stresses" in an eigenvalue analysis do not represent actual stresses, but give
you an idea of the relative stress or force distribution for each mode. By default,
no stresses are calculated.
3. Specify load step options.
The only options valid in a buckling expansion pass are the following output
controls:
Use this option to include any results data on the output file
(Jobname.OUT).
Command(s):
GUI:
Main Menu>Solution>Load Step OptsOutput Ctrl>Solu Printout
 Database and Results File Output
This option controls the data on the results file (Jobname.RST).
Command(s):
GUI:
Main Menu>Solution>Load Step OptsOutput Ctrl>DB/Results File
NoteThe FREQ field on OUTPR and OUTRES can only be ALL or NONE, that is,
the data can be requested for all modes or no modesyou cannot write
information for every other mode, for instance.
4. Start expansion pass calculations.
The output consists of expanded mode shapes and, if requested, relative
stress distributions for each mode.
Command(s):
GUI:
Main Menu>Solution>SolveCurrent LS
5. Leave the SOLUTION processor. You can now review results in the
postprocessor.
Command(s):
GUI:
Close the Solution menu.
NoteThe expansion pass has been presented here as a separate step. You can
make it part of the eigenvalue buckling solution by including the MXPAND command (Main
Menu>Solution>Load Step OptsExpansionPass) as one of the analysis
options.
7.5.5 Review the Results
Results from a buckling expansion pass are written to the structural results file,
Jobname.RST. They consist of buckling load factors, buckling mode shapes, and
relative stress distributions. You can review them in POST1, the general
postprocessor.
NoteTo review results in POST1, the database must contain the same model for
which the buckling solution was calculated (issue RESUME if necessary). Also, the results file
(Jobname.RST) from the expansion pass must be available.
1. List all buckling load factors.
Command(s):
GUI:
Main Menu>General Postproc>Results Summary
2. Read in data for the desired mode to display buckling mode shapes. (Each
mode is stored on the results file as a separate substep.)
Command(s):
GUI:
Main Menu>General Postproc>Read Resultsload step
3. Display the mode shape.
Command(s):
GUI:
Main Menu>General Postproc>Plot Results>Deformed Shape
4. Contour the relative stress distributions.
Command(s):
GUI:
Main Menu>General Postproc>Plot Results>Contour PlotNodal
Solution or
Main Menu>General Postproc>Plot Results>Contour PlotElement
Solution
See the ANSYS Commands Reference for a
discussion of the ANTYPE, PSTRES, D,
F, SF, BUCOPT, EXPASS, MXPAND, OUTRES, SET, PLDISP, and PLNSOL commands.
7.6 Sample Buckling Analysis (GUI Method)
In this sample problem, you will analyze the buckling of a bar with hinged ends.
7.6.1 Problem Description
Determine the critical buckling load of an axially loaded long slender bar of length
with hinged ends. The bar has a crosssectional height h, and area A. Only the
upper half of the bar is modeled because of symmetry. The boundary conditions
become freefixed for the halfsymmetry model. A total of 10 master degrees of
freedom in the Xdirection are selected to characterize the buckling mode. The
moment of inertia of the bar is calculated as I = Ah^{2}/12 = 0.0052083 in^{4}.
7.6.2 Problem Specifications
The following material properties are used for this problem:
The following geometric properties are used for this problem:
= 200 in
A = 0.25 in^{2}
h = 0.5 in
Loading for this problem is:
7.6.3 Problem Sketch
Figure 73 Diagram of Bar with Hinged Ends
7.6.3.1 Set the Analysis Title
After you enter the ANSYS program, follow these steps to set the title.
1. Choose menu path Utility Menu>File>Change Title.
2. Enter the text "Buckling of a Bar with Hinged Ends" and click on OK.
7.6.3.2 Define the Element Type
In this step, you define BEAM3 as the element type.
1. Choose menu path Main Menu>Preprocessor>Element Type>
Add/Edit/Delete. The Element Types dialog box appears.
2. Click on Add. The Library of Element Types dialog box appears.
3. In the scroll box on the left, click on "Structural Beam" to select it.
4. In the scroll box on the right, click on "2D elastic 3" to select it.
5. Click on OK, and then click on Close in the Element Types dialog box.
7.6.3.3 Define the Real Constants and Material Properties
1. Choose menu path Main Menu>Preprocessor>Real Constants. The
Real Constants dialog box appears.
2. Click on Add. The Element Type for Real Constants dialog box appears.
3. Click on OK. The Real Constants for BEAM3
dialog box appears.
4. Enter .25 for area, 52083e7 for IZZ, and .5 for height.
5. Click on OK.
6. Click on Close in the Real Constants dialog box.
7. Choose menu path Main Menu>Preprocessor>Material Props>
ConstantIsotropic. The Isotropic Material Properties dialog box
appears.
8. Click on OK to specify material number 1. The Isotropic Material Properties
dialog box appears.
9. Enter 30e6 for Young's modulus, and click on OK.
7.6.3.4 Define Nodes and Elements
1. Choose menu path Main Menu>Preprocessor>ModelingCreate>
Nodes>In Active CS. The Create Nodes in Active Coordinate System
dialog box appears.
2. Enter 1 for node number.
3. Click on Apply. Node location defaults to 0,0,0.
4. Enter 11 for node number.
5. Enter 0,100,0 for the X,Y,Z coordinates.
6. Click on OK. The two nodes appear in the ANSYS Graphics window.
7. Choose menu path Main Menu>Preprocessor>ModelingCreate>
Nodes>Fill between Nds. The Fill between Nds menu appears.
8. Click on node 1, then 11, and click on OK. The Create Nodes Between 2
Nodes dialog box appears.
9. Click on OK to accept the settings (fill between nodes 1 and 11, and
number of nodes to fill 9).
10. Choose menu path Main Menu>Preprocessor>ModelingCreate>
Elements>Auto NumberedThru Nodes. The Elements from Nodes
picking menu appears.
11. Click on nodes 1 and 2, then click on OK.
NoteThe triad, by default, hides the node number for node 1. To turn the
triad off, choose menu path Utility Menu>PlotCtrls>Window Controls>
Window Options and select the "Not Shown" option for Location of triad.
12. Choose menu path Main Menu>Preprocessor>ModelingCopy>
ElementsAuto Numbered. The Copy Elems AutoNum picking menu
appears.
13. Click on Pick All. The Copy Elems AutoNum dialog box appears.
14. Enter 10 for total number of copies and enter 1 for node number increment.
15. Click on OK. The remaining elements appear in the ANSYS Graphics
window.
7.6.3.5 Define the Boundary Conditions
1. Choose menu path Main Menu>Solution>Analysis TypeNew
Analysis. The New Analysis dialog box appears.
2. Click OK to accept the default of "Static."
3. Choose menu path Main Menu>Solution>Analysis Options. The Static
or SteadyState Analysis dialog box appears.
4. In the scroll box for stress stiffness or prestress, scroll to "Prestress ON" to
select it.
5. Click on OK.
6. Choose menu path Main Menu>Solution>LoadsApply>Structural
Displacement>On Nodes. The Apply U,ROT on Nodes picking menu
appears.
7. Click on node 1, then click on OK. The Apply U,ROT on Nodes dialog box
appears.
8. Click on "All DOF" to select it, and click on OK.
9. Choose menu path Main Menu>Solution>LoadsApply>Structural
Force/Moment>On Nodes. The Apply F/M on Nodes picking menu
appears.
10. Click on node 11, then click OK. The Apply F/M on Nodes dialog box
appears.
11. In the scroll box for Direction of force/mom, scroll to "FY" to select it.
12. Enter 1 for the force/moment value, and click on OK. The force symbol
appears in the ANSYS Graphics window.
7.6.3.6 Solve the Static Analysis
1. Choose menu path Main Menu>Solution>SolveCurrent LS.
2. Carefully review the information in the status window, and click on Close.
3. Click on OK in the Solve Current Load Step dialog box to begin the
solution.
4. Click on Close in the Information window when the solution is finished.
7.6.3.7 Solve the Buckling Analysis
1. Choose menu path Main Menu>Solution>Analysis TypeNew
Analysis.
NoteClick on Close in the Warning window if the following warning
appears: Changing the analysis type is only valid within the first load step.
Pressing OK will cause you to exit and reenter solution. This will reset the
load step count to 1.
2. Click the "Eigen Buckling" option on, then click on OK.
3. Choose menu path Main Menu>Solution>Analysis Options. The
Eigenvalue Buckling Options dialog box appears.
4. Click the "Reduced" option on, and enter 1 for number of modes to extract.
5. Click on OK.
6. Choose menu path Main Menu>Solution>Load Step Opts
ExpansionPass>Expand Modes.
7. Enter 1 for number of modes to expand, and click on OK.
8. Choose menu path Main Menu>Solution>Master DOFs>User
SelectedDefine. The Define Master DOFs picking menu appears.
9. Click on nodes 211. Click on OK. The Define Master DOFs dialog box
appears.
10. In the scroll box for 1st degree of freedom, scroll to UX to select it.
11. Click on OK.
12. Choose menu path Main Menu>Solution>SolveCurrent LS.
13. Carefully review the information in the status window, and click on Close.
14. Click on OK in the Solve Current Load Step dialog box to begin the
solution.
15. Click on Close in the Information window when the solution is finished.
7.6.3.8 Review the Results
1. Choose menu path Main Menu>General PostProc>Read ResultsFirst
Set.
2. Choose menu path Main Menu>General PostProc>Plot Results>
Deformed Shape. The Plot Deformed Shape dialog box appears.
3. Click the "Def + undeformed" option on. Click on OK. The deformed and
undeformed shapes appear in the ANSYS graphics window.
1. In the ANSYS Toolbar, click on Quit.
2. Choose the save option you want and click on OK.
7.7 Sample Buckling Analysis (Command or
Batch Method)
You can perform the example buckling analysis of a bar with hinged ends using
the ANSYS commands shown below instead of GUI choices. Items prefaced by
an exclamation point (!) are comments.
/PREP7
/TITLE, BUCKLING OF A BAR WITH HINGED SOLVES
ET,1,BEAM3 ! Beam element
R,1,.25,52083E7,.5 ! Area,IZZ, height
MP,EX,1,30E6 ! Define material properties
N,1
N,11,,100
FILL
E,1,2
EGEN,10,1,1
FINISH
/SOLU
ANTYPE,STATIC ! Static analysis
PSTRES,ON ! Calculate prestress effects
D,1,ALL ! Fix symmetry ends
F,11,FY,1 ! Unit load at free end
SOLVE
FINISH
/SOLU
ANTYPE,BUCKLE ! Buckling analysis
BUCOPT,REDUC,1 ! Use Householder solution method, extract 1 mode
MXPAND,1 ! Expand 1 mode shape
M,2,UX,11,1 ! Select 10 UX DOF as masters
SOLVE
FINISH
/POST1
SET,FIRST
PLDISP,1
FINISH
7.8 Where to Find Other Examples
Several ANSYS publications, particularly the ANSYS Verification Manual, describe
additional buckling analyses.
The ANSYS Verification Manual consists of test case analyses demonstrating the
analysis capabilities of the ANSYS program. While these test cases demonstrate
solutions to realistic analysis problems, the ANSYS Verification Manual does not
present them as stepbystep examples with lengthy data input instructions and
printouts. However, most ANSYS users who have at least limited finite element
experience should be able to fill in the missing details by reviewing each test
case's finite element model and input data with accompanying comments.
The following list shows you the variety of buckling analysis test cases that the
ANSYS Verification Manual includes:
VM17 SnapThrough Buckling of a Hinged Shell
VM127 Buckling of a Bar with Hinged Ends (Line Elements)
VM128 Buckling of a Bar with Hinged Ends (Area Elements)
Go to the beginning of this chapter