Nonlinear Analysis:

Nonlinear Analysis is required when a useful answer cannot be determined by linear methods.

• yielding/plasticity (beyond Hooke's law: s = Ee)
  [Requires: material property definition: s-e curve model]
• changing contact or interference between parts of an assembly
  [Requires: contact/target elements on surfaces which may change contact, plus settings and properties for the contact surface]
• large displacement, large rotation, large strain, stress stiffening (fishing pole, guitar string, drum head), sin(q)=q, tan(q)=0, and cos(q) =1
  [Requires: activate large deformation "switch," NLGEOM,ON]
• manufacturing processes (mold filling, forging, rolling, stamping, welding, coating)
  [may require several nonlinear effects (plasticity, contact, large deformation) and birth & death of elements feature]
• specialty: hyperelastic (elastomer), viscoelastic
  [Requires: unique material property definition]

Procedure:

Apply Loads GRADUALLY (incremental solution)

• Load steps: user selected points which describe the load history (convenient to the analyst). 
  TIME: even though we are doing a static analysis, time is used simply as a counter during the solution.  If the analyst doesn't set the value for time, ANSYS increases time by one for each load step (i.e. time always increases during a solution).
• Substeps: incremental solutions within a load step (for stability and accuracy); too small = long runs; too big = error or divergence.
  Ramped loading (KBC,0) increases the load linearly from the previous step's level to the current load step's final value (default).  The opposite of ramped loading is "stepped" loading (KBC,1).
• Equilibrium iterations: solutions without increment in loading, just correction of imbalance caused by nonlinear behavior.  To establish a "stable" solution (equilibrium) before additional loading is introduced.
  NON-Linear Analysis CONVERGENCE: A nonlinear solution is a series of successive linear (solution) steps, i.e., substeps, along a path that is not straight.  Each small step must converge, i.e., must be in equilibrium, before the load is increased.

In ANSYS Main Menu > Solution > Analysis Type > Sol'n Controls

General guidelines:

• The first load step should not cause yielding
• Take small steps at an abrupt transition.
• "Mildly" nonlinear problems can take larger steps
• Let the FEA program adjust the time stepping process.  Better to get a solution with less of your time spent trying to control it.  ANSYS does a fairly good job. (Activate automatic time stepping: AUTOTS , ON plus initial/min/max stepping)

Control Output to Results File

Why ? 

• More results available for nonlinear, iterative solution

• May need MORE for debugging (output of intermediate load steps and substeps)

• May need LESS to conserve disk space  

• In ANSYS Main Menu > Solution > Analysis Type > Sol'n Controls

MESH ERROR ?

Mesh error energy calculations (SERR, SEPC) are invalid for nonlinear solutions. 
Structural mesh error calculations should be linear elastic and may use solid elements having only structural degrees of freedom and 3D shell elements. [ANSYS Commands Reference Guide, PRERR command]

How do we evaluate mesh quality for a nonlinear solution ?

READING ASSIGNMENT:

ANSYS Help System

Structural Analysis Guide, Nonlinear Structural Analysis

Chapter 8, sections 8.1 - 8.6