Chapter 7: Buckling Analysis

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 loads-critical loads at which a structure becomes unstable-and buckled mode shapes-the 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 7-1(a).

Using the nonlinear technique, your model can include features such as initial imperfections, plastic behavior, gaps, and large-deflection response. In addition, using deflection-controlled loading, you can even track the post-buckled performance of your structure (which can be useful in cases where the structure buckles into a stable configuration, such as "snap-through" 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 7-1(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 real-world structures from achieving their theoretical elastic buckling strength. Thus, eigenvalue buckling analysis often yields unconservative results, and should generally not be used in actual day-to-day engineering analyses.

Figure 7-1 (a) Nonlinear load-deflection 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 re-solution 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.

7.4.3 Important

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 load-deflection 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 arc-length 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 arc-length method itself to obtain a precise buckling load, but this method requires you to adjust the arc-length radius by trial-and-error in a series of manually directed re-analyses.

7.4.4 Points to Remember

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 five-step 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

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:

Figure 7-2 Adjusting variable loads to find an eigenvalue of 1.0

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 7-1 Analysis types and analysis options

Option

Command

GUI Path

New Analysis

ANTYPE

Main Menu>Solution>-Analysis Type-New 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.

7.5.3.1 Option: New Analysis [ANTYPE]

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.

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.

Command(s):

GUI:

Main Menu>Solution>-Load Step Opts-Output Ctrls>Solu Printout

4. Save a back-up 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>-Solve-Current LS

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

7.5.4.2 Expanding the Solution

The procedure to expand the mode shapes is explained below.

1. Re-enter SOLUTION.

Command(s):

GUI:

Main Menu>Solution

Note-You must explicitly leave SOLUTION (using the FINISH command) and re-enter (/SOLUTION) before performing the expansion pass.

2. Activate the expansion pass and its options. The following options are required for the expansion pass:

Table 7-2 Expansion pass options

Option

Command

GUI Path

Expansion Pass On/Off

EXPASS

Main Menu>Solution>-Load Step Opts-ExpansionPass>ON

No. of Modes to Expand

MXPAND

Main Menu>Solution>-Load Step Opts-ExpansionPass>
Expand Modes

Stress Calculations On/Off

MXPAND

Main Menu>Solution>-Load Step Opts-ExpansionPass>
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.

Command(s):

GUI:

Main Menu>Solution>-Load Step Opts-Output Ctrl>Solu Printout

Command(s):

GUI:

Main Menu>Solution>-Load Step Opts-Output Ctrl>DB/Results File

Note-The FREQ field on OUTPR and OUTRES can only be ALL or NONE, that is, the data can be requested for all modes or no modes-you cannot write information for every other mode, for instance.

4. Start expansion pass calculations.

Command(s):

GUI:

Main Menu>Solution>-Solve-Current LS

5. Leave the SOLUTION processor. You can now review results in the postprocessor.

Command(s):

GUI:

Close the Solution menu.

Note-The 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 Opts-ExpansionPass) 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.

Note-To 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 Results-load 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 Plot-Nodal Solution or
Main Menu>General Postproc>Plot Results>-Contour Plot-Element 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 cross-sectional height h, and area A. Only the upper half of the bar is modeled because of symmetry. The boundary conditions become free-fixed for the half-symmetry model. A total of 10 master degrees of freedom in the X-direction are selected to characterize the buckling mode. The moment of inertia of the bar is calculated as I = Ah2/12 = 0.0052083 in4.

7.6.2 Problem Specifications

The following material properties are used for this problem:

The following geometric properties are used for this problem:

Loading for this problem is:

7.6.3 Problem Sketch

Figure 7-3 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, 52083e-7 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> -Constant-Isotropic. 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>-Modeling-Create> 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>-Modeling-Create> 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>-Modeling-Create> Elements>-Auto Numbered-Thru Nodes. The Elements from Nodes picking menu appears.

11. Click on nodes 1 and 2, then click on OK.

12. Choose menu path Main Menu>Preprocessor>-Modeling-Copy> -Elements-Auto Numbered. The Copy Elems Auto-Num picking menu appears.

13. Click on Pick All. The Copy Elems Auto-Num 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 Type-New 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 Steady-State 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>-Loads-Apply>-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>-Loads-Apply>-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>-Solve-Current 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 Type-New Analysis.

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 Selected-Define. The Define Master DOFs picking menu appears.

9. Click on nodes 2-11. 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>-Solve-Current 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 Results-First 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.

7.6.3.9 Exit ANSYS

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,.25,52083E-7,.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 step-by-step 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:


Go to the beginning of this chapter