METBD 450 Lecture Notes

Text: Building Better Products with FEA,
by V. Adams & A. Askenazi, (Read pp. 449-475)

Reference:  ANSYS Structural Analysis Guide

• Chapter 7: Buckling Analysis

Other types of Nonlinearity: 

• Hyperelasticity
  • rubber or elastomers
  • strain-displacement is nonlinear even at small strain
  • Hooke's law is not used, strain energy density
  • Mooney-Rivlin material constants
• Viscoplasticity and viscoelasticity
  • metal at high temperature and glass/plastics
  • time dependent plasticity (depends on the rate of loading)
• Nonlinear transient
  • crash or impact
  • properties and boundary conditions may change over time
  • implicit (LS-DYNA) or explicit (ANSYS) time integration methods
  • "convergence nightmare"
• Creep
  • time varying permanent strain due to stress and temperature
  • material "relaxes" under long term loading
• Nonlinear Buckling
  • to find behavior after buckling or secondary states of stability
  • requires eccentricity/imperfection of the FEA model
• Metal Forming
  • large strain
  • forging, stamping, cold heading, rolling
  • may need a program that re-meshes during the analysis

LINEAR BUCKLING ANALYSIS (Eigenvalue Buckling)

• to determine the lack of stability in a structure due to compressive load
• predicts the theoretical buckling strength of an ideal elastic structure
• is often unconservative
• reports the critical load factor
• shows the buckled mode shape = the shape of the part as it buckles

Consider buckling when:

• there are high compressive loads in your system
• the structure appears long and slender
• when the structure is thin-walled

ANSYS LINEAR BUCKLING PROCEDURE:

Solve the linear, static analysis of a structure

Include the calculation of the stress stiffness matrix PSTRES,ON from Solution > Analysis Options

Follow with an "Eigenvalue Buckling" analysis (the .emat and .esav files from the previous static solution are required for this analysis)

Select the Eigenvalue extraction method (usually: Subspace) and the number of modes to extract from Solution > Analysis Options

The solution gives the critical load factor and you can postprocess to see both the buckled mode shape and the critical load factor.

NONLINEAR BUCKLING ANALYSIS

• eccentric loading or geometry / imperfection is required
• is more accurate then linear buckling solutions
• requires gradual loading to find the point of instability
• can model "post-buckling" response of a structure

ANSYS NONLINEAR BUCKLING PROCEDURE:

1. (OPTIONAL) CLEAR the Options of previous analyses on the same model, see Solution > Reset Options ...
2. Solve the linear, static analysis of a structure
3. Include large deformation effects NLGEOM,ON from Solution > Analysis Options
4. Use Output Controls to insure data other than the Last Step is available for postprocessing (use ALL SUBSTEPS, if possible)
5. Use gradual (ramped) loading and automatic time stepping from Solution > Time/Frequenc > Time and Substeps
6. Control convergence behavior for number of equilibrium iteration, convergence criteria, etc. under Solution > Nonlinear ...
7. Difficult problems (or analysis of post-buckling) may require use of the "Arc Length" convergence enhancement tool for a successful run.

NONLINEAR RESULTS DATA

• more results info to deal with
• output of intermediate load steps and substeps
• you can limit the output data (to save disk space):
  • in initial debugging runs, try storing only the displacement results for large models
  • if convergence is a problem, storing every solution can help you find problems

Methodology

• Use small, simple test models to debug new features/elements
• run a linear solution first:
  • to debug boundary conditions
  • to evaluate mesh quality
• Add each nonlinearity after you have control of the previous one
• add each nonlinearity from easiest to hardest degree of difficulty:
  • large deflection effects
  • contact
  • plasticity

WHAT TO DO WHEN IT WON'T CONVERGE

• check the solution output and error log file for messages
• apply the load in more, smaller substeps
• allow more equilibrium iterations
• try alternative material models (bilinear vs. multilinear, different hardening rules, etc.)
• inspect the mesh in high stress regions for poor element shapes
• re-evaluate you choice of loads (get rid of point loads, overconstrained edges)
• look at the last good solution for any irregularities
• re-check element options (and material properties, and real constants, and load values, and dimensions)
• experiment with convergence enhancement tools in the code
• deactivate one or more of the nonlinear conditions to find the problem
• (rarely) loosen the convergence criteria - to find the problem - then tighten it up again

RESTARTING a Solution

When a job stops due to failure to converge, you can adjust solution parameters (substep size, convergence criteria, no. of equilibrium iterations) and "restart" the analysis from where it stopped. 

Sometimes, this can help you get past a difficult load increment.

A restarted analysis will continue to write results on the same results file, as good solutions are completed.  Some of the files from the prior run must be available for the restart analysis.