METBD 450 Lecture Notes

Text: Building Better Products with FEA,
by V. Adams & A. Askenazi, (Read pp. 425-448)

Reference:  ANSYS Structural Analysis Guide

• Chapter 8: Nonlinear Structural Analysis
• Chapter 9: Contact

"... most of the world is nonlinear." 

"In many cases, simply understanding the effects of the nonlinearity can enable a design engineer to make sound design decisions on linear results".

When you start doing nonlinear analyses:

• move slowly
• research your software's capabilities
• have a "coach"

All problems could be run as nonlinear analyses, but is that necessary ?

A nonlinear solution is a series of successive linear steps (iterations) along a path that is not straight.

WHY USE NONLINEAR ANALYSIS ?

when the answer cannot be found in linear solutions.

• nonlinear solutions require more data
• can take more time to setup and solve (= more costly)

Types of nonlinear behavior:

• yielding/plasticity (beyond Hooke's law: s = Ee)
• changing contact or interference
• large displacement, large rotation, large strain, stress stiffening (fishing pole, guitar string, drum head), sin(q)=q and tan(q)=0.
• manufacturing processes (mold filling, forging, rolling, stamping, welding, coating)

Beware: yield stress in the handbook is an estimated quantify, may vary around some mean and may be subject to experimental error.

LOOK AT YOUR RESULTS: check for large displacement, penetration/interference

SOLUTION APPROACH

Iterative solution: uses previous step results, to correct behavior and try again (Newton-Raphson)

Apply the loads GRADUALLY (incremental solution)

• In ANSYS, Load steps: user selected points which describe the load history (convenient to the analyst). 
• In ANSYS, 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).
• In ANSYS, Substeps: incremental solutions within a load step (for stability and accuracy); too small = long runs; too big = error or divergence.
• In ANSYS, ramped loading (KBC,0) increases the load linearly from the previous step's level to the current load step's final value.  The opposite of ramped loading is "stepped" loading (KBC,1).
• In ANSYS, 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.

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 STEPPING PROCESS.   Author: this may slow down the run.  Mr. J: better to get a solution with less of your time spent trying to control it.  ANSYS does a fairly good job.

Ever since ANSYS 5.5 the default setting for SOLCON = ON (automatic solution controls).  Based on the types of and severity of nonlinearities in your model, ANSYS sets many solution options in a manner which is usually appropriate for success in solving.

Solution Controls makes automatic settings for:

• load increments
• automatic adjustment of load increments during the solution
• convergence tolerances
• convergence enhancement "tools" (algorithms)
• reasonable limit on equilibrium iterations
• activates prediction of contact changes and onset of yielding

ANSYS makes these settings based on years of experience in solving nonlinear analyses.  However, the analyst can override any of the automatic settings.

During a nonlinear analysis, ANSYS writes a solution monitor text file (extension: mntr) which you can view to check on the progress of the analysis.

Graphical Solution Tracking:  during an interactive nonlinear analysis, ANSYS shows a graph of convergence norm values vs. criteria.

NEWTON-RAPHSON

• method for correcting the stiffness matrix between solution iterations based on the nonlinear behavior experienced.
• uses a "tangent" modulus corresponding to the previous iteration.

Types of Nonlinear Behavior

Material Nonlinearity: plasticity

• based on a yield criteria (Tresca, vonMises, Mohr-Coulomb, Drucker-Prager)
• requires definition of a hardening rule if unloading/reversed loading occurs:
  • isotropic hardening (no Bauschinger effect) compressive yield = tensile yield
  • kinematic hardening (w/ Bauschinger effect) tensile yielding changes the compressive yield
• Bi-linear (two straight lines); elastic modulus, tangent modulus, meet at the yield point
• Multilinear ( > two straight lines); enter the stress vs. strain points along the curve.
• temperature and strain rate can effect the material data
• true stress-strain vs. engineering stress-strain data

In ANSYS 5.7: Preprocessor > Material Props > Material Models ... >

• click on the material number you want to add data to
• double-click "Structural"
• double-click "Nonlinear"
• double-click "Inelastic"
• double-click on the hardening rule choice (e.g., Kinematic hardening),
• double-click on the data format (e.g., Bilinear)
• pick the appropriate stress-strain options (e.g., to account for stress relaxation with increasing temperature)
• for each temperature, enter the yield stress and the tangent modulus
• "Exit" Material Models, once you have entered the data. 
• You can graph or list the nonlinear data that you defined in the material model tables from the ANSYS Utility Menu: 
  • Plot > Data Tables ...
  • List > Properties > Data Tables ...

Geometric Nonlinearity

accounts for changes in stiffness that are not from material properties (things like large deflection, large rotation, large strain, stress stiffening).

In ANSYS, Solution > Analysis Options >

Large Deformation Effects = ON (or NLGEOM,ON)

Boundary Nonlinearity

CONTACT ELEMENTS

• you can specify "contact pairs,"  ANSYS: Contact wizard for elements TARGE169, 170 and CONTA171, 172, 173, 174
• point-to surface contact, ANSYS: CONTAC48, 49
• point-to-point contact, ANSYS CONTAC12, 52
• slide line contact, ANSYS CONTAC26

Contact can be difficult to set up.  Often it is used "only when necessary".  Use it "judiciously", but don't be afraid to use it !

ANSYS contact models (element options, real constants, material properties):

• formulation: penalty method or penalty + LaGrange multipliers
• predictions: for best performance
• specialty: sticking, hook, initial interference, sliding with friction, bonded, and more
• open = no stiffness, closed = stiff spring (stiffness may default or may require user specification)

Guidelines for Target/Contact Surfaces:

• if a convex face will contact a flat or concave face, the flat or concave face should be the target surface.
• if one surface has a coarser mesh, it should be the target surface.
• if one surface is stiffer than the other, it should be the target surface.
• if one surface is higher-order and the other is lower-order, the lower-order surface should be the target surface.
• if one surface is larger, it should be the target.

FOLLOWER FORCES

Loads can vary in large displacement/large rotation analyses.  Should the load follow the part as it bends or keep its original orientation ?

In ANSYS, with large deformation effects ON, pressure loads follow the surface as it bends, while force loads keep their original vector direction.