*Tip: Start typing in the input box for immediate search results.Can't find what you're looking for? Submit a support request here.*

# Buckling Analysis Overview

## Buckling Analysis in StressCheck

The goal of a standard buckling analysis is to find the load factor corresponding to a given loading condition, and the corresponding buckling shapes. In some cases, the buckling load may be influenced by the existence of pre-stress, such as residual stresses. For that reason a pre-load buckling option is available when performing an eigenvalue buckling analysis, such that only the buckling load factor for one set of loads is computed while other set of fixed loads are applied to the body.

Buckling analysis is available for three-dimensional problems only.

## Buckling Analysis Setup

Preparation of the input data for modal analysis consists of the following steps:

- Description of the solution domain (geometry/mesh)
- Specification of material properties
- Specification of loading conditions
- Specification of constraints
- Association of a solution name with a constraint name and load name
- Specification of the discretization parameters

Then, select the Buckling tab in the Solve dialog, specify the solution options, and click the Solve button. For an example of setting up and executing a buckling analysis, refer to StressCheck Demo: Shear Panel Buckling Load Factor Analysis.

## Buckling Analysis Considerations

### Units

The units for the material properties should be given in a consistent set. For example, if using US units, the force is given in pound force (lbf), the time in seconds (s), the length in inches (in), the pressure or stress in lbf/in^{2} (psi), the mass in lbf/g (lbf-s^{2}/in), and the specific density in lbf/g-in^{3} (lbf-s^{2}/in^{4}), where g is the gravitational acceleration (g=386.1 in/s^{2}). Using SI units, the force is given in Newtons (N), the mass in kilograms (kg), the time in seconds (s), the length in meters (m), the pressure or stress in N/m^{2} (Pa), and the density in kilogram per cubic meter (kg/m^{3}).

The buckling load factor (BLF) is unitless, and represents the scaling factor required to initiate buckling based on the applied loads.

### Recommended P-Levels

In general, when one dimension of a body is much smaller than the others (e.g. “thin” plates or columns), locking will occur at low p-levels. It is recommended therefore that p-levels should range from not less than p=3 to at least p=6.

When running a downward p-extension, the element stiffness and mass (resp. geometric) matrices corresponding to the highest p-level are saved and reused for all lower p-levels. Thus, the downward p-extension is more efficient than the upward.

### Eigensolver Tolerance

When the buckling load factor values do not decrease monotonically as the number of degrees of freedom are increased (see the below Load Factor Convergence section), determine for which run number (or p-level) the value increases, and then try specifying a higher accuracy by setting parameter _nfig > 6 (_nfig is the number of decimal digits of accuracy desired in the eigensolver. By default _nfig = 6).

Note: if the tolerance is too small, the solver may take too long to compute the eigenpairs. Request a lower accuracy by setting the parameter _nfig < 6.

### Rigid Body Constraints

In general rigid body (RB) constraints are illegal for eigenvalue buckling analysis and should be avoided. For some cases the effect of the RB constraints is not visible because the mode associated with the RB constraint is not exited at low eigenvalues. Therefore the general rule is no RB constraints should be used when performing a buckling analysis. The only exception for using RB constraints is when it is known a priori that the range of eigenmodes of interest do not include rigid body modes.

As a practical rule of practice, when RB would be required, very weak spring boundary conditions (at least 3 orders of magnitude smaller than the modulus of elasticity) should be used. Note also that in this case it is advisable to run parametric studies varying the spring coefficient to evaluate solution independence.

## Buckling Solver Options

### Extension

As in a Linear analysis, you may choose the type of extension to perform during the Buckling analysis, Upward-p or Downward-p. These have the same interpretation as in a Linear analysis, as do the p-limits. NOTE: In the case of “thin” bodies, locking will occur at low p-levels, so let p range between 3 to at least 6.

### Type

The type of Buckling analysis may be “Buckling and shapes” or “Buckling load only”. Buckling load only means that the natural buckling load factors will be computed and stored, but not the mode shapes. Buckling and shapes means that the buckling load factors and the corresponding buckling mode shapes will be computed and stored. Computation of mode shapes requires more CPU time and disk storage.

### Load Numbers

The requested output will be computed from Load factor number 1 to Load factor number j, j is entered in the second Load number field. Typically only the first buckling mode is of interest. Letting the first and second fields to be 1, will save computation.

### Enable Fixed Loading

This option is enabled if more than one solution ID was defined with the objective of performing a pre-load buckling analysis (more information in the following).

## Buckling Results

There are two basic post-solution operations which are relevant to Buckling analysis: buckling load convergence and display of the buckling shapes. The buckling load convergence is performed under the Error estimation option in the Results dialog window, while the display of the deformed shapes is done under the Plot option.

### Load Factor Convergence

From the Main Menu Bar select the View Results icon and when the Results dialog appears select the Error tab. To obtain an error estimate, there must be at least three runs in a sequence. The available solution names and run numbers are displayed in the scrolling list.

The solution corresponding to each eigenpair (load factor and mode shape) is identified by the name provided in the Solution ID class followed by an underscore (_) and a number followed by the letter “B”. For example, the solution corresponding to the first eigenpair is labeled SOL_00001B. The linear solution is also available in the scrolling list of the input area with the name SOL (assuming that SOL is the name given in the Solution ID input form).

To check the convergence of a buckling load factor, select the desired solution and click on the Accept button. As shown in the below animated example (roark_35_12.scw in the 3D-Basic Handbook folder), the estimated error for the first buckling load factor is plotted as a function of the number of degrees of freedom (DOF):

### Mode Shapes

To obtain a deformed configuration, select the Plot tab from the Results dialog. To display the mode shape associated with a given buckling load factor, select the corresponding solution name and run number, select Shape: Deformed and then click on the Plot button:

The Model View has a legend that includes the solution ID, the run number, the degrees of freedom, the buckling load factor, the mode shape number, and the maximum and minimum values of the displayed function. The maximum and minimum values have only relative significance, since mode shapes are known only up to an arbitrary multiplier.

## Executing a Standard Buckling Analysis

To perform a standard bifurcation Buckling analysis, StressCheck first solves the linear problem corresponding to the specified loads and constraints, then, utilizing the stress field computed from the linear solution, computes the geometric stiffness matrix, which is used for the eigenvalue computation. After the Buckling analysis is completed, two sets of solutions are available: the linear solution, which establishes the pre-buckling stress state and the eigenvalue buckling solution.

For an example of a displacement-controlled buckling analysis of a column, refer to StressCheck Tutorial: Displacement-Controlled Buckling Analysis.

## Executing a Pre-Load Buckling Analysis

To perform a pre-load Buckling analysis, StressCheck first solves the linear problem corresponding to the specified loads and constraints (two solutions IDs), then, utilizing the stress field computed from one of the linear solutions (fixed load), computes the geometric stiffness matrix which is added to the stiffness matrix. The linear solution for the other load case is used to compute the second geometric matrix needed for the eigenvalue computation.

After the Buckling analysis is completed, three sets of solutions are available: two linear solutions, corresponding to the pre-load and the pre-buckling stress state and the eigenvalue buckling solution. In the standard buckling analysis the solution of the following eigenvalue problem is obtained:

([*K*] – λ[*G*]){*b*} = 0

where [*K*] is the stiffness matrix, [*G*] is the geometric matrix, {*b*} is the eigenvector (mode shape) associated with the eigenvalue λ (buckling load factor).

For problems involving residual stresses or body forces or any set of thermal or mechanical loads independent of the buckling load factor, the objective is to find the buckling modes and shapes corresponding to the applied loads rather than the total loads. Let F represent the fixed loads applied to the body (residual stresses, body forces, etc.) and B the loads for which the buckling load factor is required with the other loads fixed. Then the pre-load buckling problem can be written as:

([*K*]^{(B)} + [*G*]^{(F)} – λ[*G*]^{(B)}){*b*} = 0

where [G]^{(F)} and [G]^{(B)} are the geometric matrices associated with the solutions for the fixed and buckling loads respectively. As can be seen from the above expression, the geometric matrix corresponding to the fixed load modifies the stiffness matrix of the problem, while the other geometric matrix is multiplied by the buckling load factor.

To perform a pre-load buckling analysis at least two solution IDs must be specified. Each solution ID will correspond to a load and constraint ID pair, therefore the pre-load and the buckling load cases can have different constraints conditions. If two or more solutions are defined then the Enable Fixed Loading option in the Buckling tab will be available to select the solution ID corresponding to the fixed load (Figure 2):

The solution corresponding to each eigenpair (buckling load and mode shape) is identified by the name provided in the Solution ID input form followed by an underscore (_) and a number followed by the letters PB. For example, the solution corresponding to the first buckling load is labeled SOL1_001PB. Two linear solutions will also be available in the scrolling list of the input area with the names SOL1 (assuming that SOL1 is the name given in the Solution ID input form for the for which the buckling load factor is required), and SOL2 (assuming that SOL2 is the name given in the solution ID input for the fixed load case).

The below animation demonstrates the convergence of the pre-load buckling factor for a cantilever column (ColumnPreLoadBuckling.scw in the Tutorial Handbook folder). Two load cases were defined for this problem: LOAD1 is a uniform unit compression (S=1.0 psi), and LOAD2 is a uniform compression with a value S=1891 psi. Two solution IDs were created using the two load cases and a single constraint ID: SOL1 associated with LOAD1 and SOL2 associated with LOAD2; SOL2 was selected as the solution ID corresponding to the fixed load: