Eigenvalue Buckling Analysis

Background

An Eigenvalue Buckling analysis predicts the theoretical buckling strength of an ideal elastic structure. This method corresponds to the textbook approach to an elastic buckling analysis: for instance, an eigenvalue buckling analysis of a column matches the classical Euler solution. However, imperfections and nonlinearities prevent most real-world structures from achieving their theoretical elastic buckling strength. Therefore, an Eigenvalue Buckling analysis often yields quick but non-conservative results.

A more accurate approach to predicting instability is to perform a nonlinear buckling analysis. This involves a static structural analysis with large deflection effects turned on. A gradually increasing load is applied in this analysis to seek the load level at which your structure becomes unstable. 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, as illustrated below).

(a) Nonlinear load-deflection curve, (b) Eigenvalue buckling curve.

Eigenvalue Buckling in Mechanical

In Mechanical, an Eigenvalue Buckling analysis is a linear analysis and therefore cannot account for nonlinearities. It employs the Linear Perturbation Analysis procedure of Mechanical APDL. This procedure requires a pre-loaded environment from which it draws solution data for use in the Eigenvalue Buckling analysis. Based on this requirement, an Eigenvalue Buckling analysis can consider nonlinearities that are present in the pre-stressed environment allowing you to attain a more accurate real-world solution as compared to a traditional linear preloaded state.


Note:  The content of this Help page is based on the use of the ANSYS Mechanical APDL Solver.


Points to Remember

Linear-based Eigenvalue Buckling Analysis

Note the following when you have created an Eigenvalue Buckling analysis when the base analysis is linear:

  • For a linear upstream Static Structural Analysis, you can define loading conditions only in the upstream analysis.

  • The results calculated by the Eigenvalue Buckling analysis are buckling load factors that scale all of the loads applied in the Static Structural analysis. Thus for example if you applied a 10 N compressive load on a structure in the static analysis and if the Eigenvalue Buckling analysis calculates a load factor of 1500, then the predicted buckling load is 1500x10 = 15000 N. Because of this it is typical to apply unit loads in the static analysis that precedes the buckling analysis.

  • The buckling load factor is to be applied to all the loads used in the static analysis.

  • Note that the load factors represent scaling factors for all loads. If certain loads are constant (for example, self-weight gravity loads) while other loads are variable (for example, externally applied loads), you need to take special steps to ensure accurate results.

    One strategy that you can use to achieve this end is to iterate on the Eigenvalue buckling solution, adjusting the variable loads until the load factor becomes 1.0 (or nearly 1.0, within some convergence tolerance).

    Consider, for example, a pole having a self-weight W0, which supports an externally-applied load, A. To determine the limiting value of A in an Eigenvalue Buckling analysis, you could solve repetitively, using different values of A, until by iteration you find a load factor acceptably close to 1.0.

  • If you receive all negative buckling load factor values for your Eigenvalue Buckling analysis and you wish to see them in the positive values, or vice versa, reverse the direction of all of the loads you applied in Static Structural analysis.

  • You can apply a nonzero constraint in the static analysis. The load factors calculated in the buckling analysis should also be applied to these nonzero constraint values. However, the buckling mode shape associated with this load will show the constraint to have zero value.

Nonlinear-based Eigenvalue Buckling Analysis

Note the following when you have created an Eigenvalue Buckling analysis when the base analysis is nonlinear:

  • At least one form of nonlinearity must be defined in the pre-requisite static analysis.

  • In addition to the loads defined in Static Structural Analysis, you must define at least one load in the buckling analysis to proceed with the solution. To enable this, setting the Keep Pre-Stress Load-Pattern property to Yes (default setting) retains the loading pattern from the Static Structural Analysis in the Eigenvalue Buckling analysis. Settings the property to No requires you to define a new loading pattern for the Eigenvalue Buckling analysis. This new loading pattern can be completely different from that of the prestress analysis.

  • In a nonlinear-based Eigenvalue Buckling analysis, load multipliers scale the loads applied in buckling analysis ONLY. When estimating the ultimate buckling load for the structure, you must account for the loading applied in both static structural and eigenvalue analyses. The equation to calculate the ultimate buckling load for the Nonlinear-based Eigenvalue Buckling analysis is:

    FBUCKLING = FRESTART + λi · FPERTRUB

    where:

    • FBUCKLING = The ultimate buckling load for the structure.

    • FRESTART = Total loads in Static Structural analysis at the specified restart load step.

    • λi = Buckling load factor for the "i'th" mode.

    • FPERTRUB = Perturbation loads applied in buckling analysis.

    For example, if you applied a 100 N compressive force on a structure in the static analysis and a compressive force of 10 N in the Eigenvalue Buckling analysis and you get a load factor of 15, then the ultimate buckling load for the structure is 100 + (15 x 10) = 250 N.


    Note:  You can verify the ultimate buckling load of the above equation using the buckling of a one dimensional column. However, calculating the ultimate buckling load for 2D and 3D problems with different combinations of loads applied in the Static Structural and Eigenvalue Buckling analyses may not be as straightforward as the 1D column example. This is because the FRESTART and FPERTRUB values are essentially the effective loading values in the static and buckling analyses, respectively.


  • Consider, for example, a cantilever beam that has a theoretical ultimate buckling strength of 1000N and which is subjected to a compressive force (A) of 250N. The procedure to calculate the ultimate buckling load (F), based on the load factors evaluated by Mechanical for Linear-Based and Nonlinear-Based Eigenvalue Buckling analyses is illustrated in the following schematic.


    Note:  As illustrated, cases (3) and (5) are identical. In Case (3), setting the Keep Pre-Stress Load-Pattern property to Yes automatically retains the loading from pre-stress analysis for the buckling analysis. As a result, there is no need to define new loads for the buckling analysis in Case 3. For Case 5, the Keep Pre-Stress Load-Pattern property is set to No, allowing you to define a new load pattern in the buckling analysis which can be completely different from that of the Static Structural analysis.


  • The buckling load factor evaluated in nonlinear-based Eigenvalue Buckling should be applied to all the loads used in the buckling analysis.

  • If you receive all negative buckling load factor values for your Eigenvalue Buckling analysis and you wish to see them in the positive values, or vice versa, reverse the direction of all of the loads you applied in the Static Structural analysis when the Keep Pre-Stress Load-Pattern property is set to Yes. If this property is set to No, reverse the direction of all of the loads that you applied in Eigenvalue Buckling analysis.

Preparing the Analysis

Create Analysis System

  Basic general information about this topic

  ... for this analysis type:

Because this analysis is based on the Static Structural solution, a Static Structural analysis is a prerequisite. This linked setup allows the two analysis systems to share resources such as engineering data, geometry, and boundary condition type definitions made in Static Structural analysis.

From the Toolbox, drag a Static Structural template to the Project Schematic. Then, drag an Eigenvalue Buckling template directly onto the Solution cell of the Static Structural template.

Define Engineering Data

  Basic general information about this topic

  ... for this analysis type:

  • Young's modulus (or stiffness in some form) must be defined.

  • Material properties can be linear, nonlinear, isotropic or orthotropic, and constant or temperature-dependent.

Attach Geometry

  Basic general information about this topic

  ... for this analysis type:

There are no specific considerations for an Eigenvalue Buckling analysis.

Define Part Behavior

  Basic general information about this topic

  ... for this analysis type:

There are no specific considerations for an Eigenvalue Buckling analysis.

Define Connections

  Basic general information about this topic

  ... for this analysis type:

Linear-based Eigenvalue Buckling Analysis

The following contact settings are considered linear contact behaviors for Eigenvalue Buckling analyses. If any other contact settings are used, the analysis will be considered a Nonlinear-based Eigenvalue Buckling analysis.

  • The Formulation property is set to MPC or Beam.

    Or...

  • The Type property is set to Bonded or No Separation and Small Sliding is active.

Springs with linear stiffness definition are taken into account if they are present in the static analysis.

Only Bushing and General joints enable you to solve an analysis with nonlinear Joint Stiffness. Mechanical considers all other joint types to be linear. The application accounts for linear joints if they are present in the static analysis.

Nonlinear-based Eigenvalue Buckling Analysis

All nonlinear connections (including nonlinear springs and joints) are allowed. Any contact options other than the ones mentioned above would trigger a nonlinear based Eigenvalue Buckling analysis.

Apply Mesh Controls/Preview Mesh

  Basic general information about this topic

  ... for this analysis type:

There are no considerations specifically for an Eigenvalue Buckling analysis.

Establish Analysis Settings

  Basic general information about this topic

  ... for this analysis type:

For an Eigenvalue Buckling analysis, the basic Analysis Settings include:

Options
  • Use the Max Modes to Find property to specify the number of buckling load factors and corresponding buckling mode shapes of interest. Typically the first (lowest) buckling load factor is of interest. The default value for this field is 2. You can change this default setting under the Buckling category of the Frequency options in the Options preference settings tool.

  • The Keep Pre-Stress Load-Pattern property is available for nonlinear-based Eigenvalue Buckling analyses. Use this property to specify whether you want to retain the pre-stress loading pattern to generate the perturbation loads in the Eigenvalue Buckling analysis. The default setting for this property is Yes, which automatically retains the structural loading pattern for the buckling analysis (refer to the ALLKEEP LoadControl key setting for PERTURB command). Setting the property to No requires you to define a new loading pattern for the Eigenvalue Buckling analysis (refer to PARKEEP LoadControl key setting for PERTURB command).


    Important:  The PARKEEP LoadControl key retains all displacements applied in Static Structural analysis for reuse in Eigenvalue Buckling analysis. Any non-zero displacements applied in static analysis act as loads in Eigenvalue Buckling analysis. If you specifying different load types in the buckling analysis that are scoped to the same geometric entities and in the same direction, may be ignored. Define your new loading pattern carefully.


Solver Controls
  • Solver Type: The default option, Program Controlled, allows the application to select the appropriate solver type. Options include Program Controlled, Direct, and Subspace. By default, the Program Controlled option uses the Direct solver for Linear-based Eigenvalue Buckling and Subspace solver for Nonlinear-based Eigenvalue Buckling analyses.


    Note:  Both the Direct and Subspace solvers evaluate the buckling solutions for most engineering problems. If you experience a solution failure using one of the solvers because it cannot find the requested modes, it may help to switch the solvers. If both of the solvers fail to find the solution, then review your model carefully for possible stringent input specifications or loading conditions.


  • Include Negative Load Multiplier: The default option Program Controlled and Yes will extract both the negative and positive eigenvalues (load multipliers). Set the property to No to extract only positive eigenvalues (load multipliers).

Output Controls

By default, only buckling load factors and corresponding buckling mode shapes are calculated. You can request Stress and Strain results to be calculated but note that “stress” results only show the relative distribution of stress in the structure and are not real stress values.


Note:   Output Controls are only exposed for the ANSYS solver.


Analysis Data Management

These properties enable you to define whether or not to save the Mechanical APDL application database as well as automatically delete unneeded files.

Define Initial Conditions

  Basic general information about this topic

  ... for this analysis type:

You must point to a static structural analysis of the same model in the initial condition environment.

  • An Eigenvalue Buckling analysis must be preceded by a Static Structural analysis and the same solver type must be used for each (ANSYS or Samcef).

  • The Pre-Stress Environment property in the Pre-Stress (Static Structural) Initial Condition object displays whether the pre-stress environment is considered linear or nonlinear for the Eigenvalue Buckling analysis.

  • If the Static Structural analysis has multiple result sets, the value from any restart point available in the Static Structural analysis can be used as the basis for the Eigenvalue Buckling analysis. See the Restarts from Multiple Result Sets topic in the Applying Pre-Stress Effects Help section for more information.

Apply Loads and Supports

  Basic general information about this topic

  ... for this analysis type:

Loads are supported by Eigenvalue Buckling analysis only when the pre-stressed environment has nonlinearities defined.

The following loads are allowed for a nonlinear-based Eigenvalue Buckling analysis:


Note:
  • Choosing to keep the default setting (Yes) for the Keep Pre-Stress Load-Pattern property retains the pre-stress loading pattern for the buckling analysis and no additional load definition is necessary.

  • For Nodal Pressure, the only definition option is Normal To. This results in the "pressure load stiffness" effect. To avoid the pressure stiffness effect, apply an equivalent Nodal Force load to the same surface and set the Divide Load by Nodes property to Yes. The equivalent force is equal to the value of the pressure multiplied by the area of the scoped surface.

  • The node-based Named Selections used with the above Direct FE Loads cannot contain nodes scoped to a rigid body.


No loading conditions can be created in a linear-based Eigenvalue Buckling analysis. The supports as well as the stress state from the linked Static Structural analysis are used in the linear-based Eigenvalue Buckling analysis. See the Apply Pre-Stress Effects for Implicit Analysis Help section for more information about using a pre-stressed environment.

Solve

  Basic general information about this topic

  ... for this analysis type:

Solution Information continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis.

Review Results

  Basic general information about this topic

  ... for this analysis type:

You can view the buckling mode shape associated with a particular load factor by displaying a contour plot or by animating the deformed mode shape. The contours represent relative displacement of the part.

Buckling mode shape displays are helpful in understanding how a part or an assembly deforms when buckling, but do not represent actual displacements.

“Stresses” from an Eigenvalue Buckling analysis do not represent actual stresses in the structure, but they give you an idea of the relative stress distributions for each mode. You can make Stress and Strain results available in the buckling analysis by setting the proper Output Controls before the solution is processed.


Release 18.2 - © ANSYS, Inc. All rights reserved.