Nonlinear buckling analysis

You can perform ANSYS nonlinear buckling analyses:

• A linear or eigenvalue buckling analysis predicts the theoretical buckling strength of an ideal linear elastic structure. A linear buckling analysis computes the structural eigenvalues for a given system. In a linear buckling analysis, the software applies perturbations to the undeformed geometry and looks for deflections that could be unstable under a specific set of loads.

• A nonlinear buckling analysis predicts the actual response of a structure for each load increment. A nonlinear buckling analysis is more accurate than a linear buckling analysis because it uses nonlinear, large deflection static analysis to predict the buckling loads.

Solution step types

In Pre/Post, when you create a Nonlinear Buckling type of solution, you can create the following types of analysis steps:

• Linear Buckling, in which you perform an initial linear (eigenvalue) buckling analysis to determine the critical loads that induce buckling and possible buckling modes. In this type of step, you can analyze the effects of initial imperfections as well as shape multiplier. After you solve a Linear Buckling step, you can View the buckling mode shapes and load multipliers.Look at the results to find the iteration time step in which the structure becomes unstable. If that occurs, this time step becomes the starting point for the Nonlinear Buckling step.

• Nonlinear Buckling, in which you solve the model with large deflection active (NLGEOM, ON). In this step, the model is stressed to reach its limit or maximum load.

• Post-Buckling, which is a continuation of a Nonlinear Buckling step. After a load reaches its buckling value, the load value may remain unchanged or may decrease while the deformation continues to increase.

As opposed to other analysis types where you perform a single solve, in a Nonlinear Buckling solution, each step is solved separately. The results of the current step are reused for the next step. However, Cumulative Load Options, such as the ANSYS FCUM and BFCUM commands, are not supported in nonlinear buckling analysis. By default, loads and constraints are not propagated from step to step in a Nonlinear Buckling solution. Consequently, you must manually add the appropriate loads and constraints to each step.

Note:

In a large model, adding loads and constraints to each step can be cumbersome. In those cases, you can click the Edit Advanced Solver Options button in the Solve dialog box. You can then use the By card name option in the Output Options group to manually exclude the DDELE, FDELE, and SFEDELE commands from the ANSYS input file.

Nonlinear stabilization

You can include nonlinear stabilization during a Post-Buckling step. Nonlinear stabilization is a tool for managing both local and global instabilities. In ANSYS, nonlinear stabilization consists of adding an artificial damper or dashpot element at each node of an element that supports the technique.

• Before buckling occurs, the system may have low displacements over a given time step. Conceptually, you can think of this as a low pseudo velocity that does not generate much resistive force from the dampers.

• When the buckling occurs, the system may have larger displacements over a small time step. As a result, the pseudo velocity becomes large and does generate a large resistive force from the dampers.

This software supports the use of the ANSYS STABILIZE command to turn nonlinear stabilization either on or off for a particular Post Buckling step. You can specify nonlinear stabilization either by specifying a damping factor or an energy dissipation ratio.

Ability to preview the ANSYS monitor file

In the Solution dialog box, you can use the Preview Ansys monitor file button to examine a summary of your results (the convergence table). You can then determine which sub-step (the sub-step where divergence occurs) to use in the Post-Buckling step.

Look up more details

Transient dynamic analysis

Thermal-structural multiphysics analysis

Performing a nonlinear buckling analysis

Harmonic analysis

Cyclic symmetry analysis in ANSYS

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Nonlinear buckling analysis, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });