1. Chapter 2 General Procedures
Workbench - Mechanical
Structural Nonlinearities

2. Chapter Overview
In this chapter, general tools and procedures, not specific to a particular source of nonlinearity, but useful for achieving convergence and post processing results are introduce:
Building a Nonlinear Model
Analysis Settings
Postprocessing Nonlinear Results
Workshops
In this chapter, we will present an overview of the basics of nonlinear finite-element analysis:
We will start by answering a basic but very important question: What is “Nonlinear” Behavior?
We will then present the strategy used in the ANSYS code for solving a nonlinear solution using linear solvers and discuss the details of exactly what this means.
Three general types of nonlinearities will be introduced.
Issues unique to Structural Nonlinearities will be discussed.
Finally general procedures will be presented for use in nonlinear analysis.
The purpose is to give you an understanding of the fundamental nature of nonlinear finite element analysis.

3. A. Building a nonlinear model
What is different about building a nonlinear model vs. a linear model?
In some cases, there will be no difference!
A model undergoing mildly nonlinear behavior due to large deflection and stress stiffening effects might need no modification with regards to geometry set up and meshing.
In other cases, you must include special features:
Elements with special properties (such as contact elements)
Covered in Chapter 3 & 4
Nonlinear Material data (such as plastic stress-strain data)
Covered in Chapter 5 & 6
Include geometric features to overcome singularities that cause convergence trouble. (i.e. add radius to sharp corner for example)
You might also need to give special attention to:
Load and boundary condition limitations under large deflection
Mesh control considerations under large deflection
Element technology options under large deflection with nonlinear materials
To answer this question, first consider, What is different about building a nonlinear model?
Problem dependencies affect how a nonlinear model will differ from a linear one:
In some cases, there will be no difference!
In other cases, you must include special nonlinear features:
Such as material test data (plastic stress vs strain).
And special elements (such as contact elements).
Later Chapters will provide case-by-case details of modeling tips for different nonlinear situations.

4. ... Building a nonlinear model
It is important to note the orientation of loads and its effect on the structure in large-deflection analyses:
Direction Before Deflection
Direction After Deflection
Load
Acceleration (constant direction)
Force, Moment, Bolt Load (constant direction)
Pressure (always normal to surface)

5. ... Building a nonlinear model
Meshing considerations are usually the same in nonlinear analyses. However, if large strains are expected, the shape checking option may be changed to “Aggressive”
For large-deflection analyses, if elements may undergo some change in shape, this may reduce the fidelity of the solution
By using “Aggressive” shape checking, WB-Mechanical will ensure that the element quality is much better prior to solution in order to anticipate distortion of the element in the course of a large-strain analysis.
The quality of the “Standard” shape checking is suitable for linear analyses, so it does not need to be changed in linear analyses
With “aggressive” shape checking set, some mesh failures may be more likely. See WB-Mechanical - Intro for ways
to detect and remedy mesh failures.
Simulation meshes in ANSYS:
The “Shape Checking” toggle is SHPP,LSTET,ON
Use of Jacobian tests at integration points is the “Standard” or SHPP,LSTET,ON method, suitable for linear analyses
Use of Jacobian tests at corner nodes is the “Aggressive” or SHPP,LSTET,OFF method. This is generally a more conservative approach and may be preferred for nonlinear analyses. This is because elements which undergo distortion during solution should have a good quality shape to begin with.
Because Simulation uses its own criteria for shape tests, SHPP,OFF is set when exporting a mesh to ANSYS. Also, even if SHPP,ON is set, the criteria used for warning/error elements differs between Simulation and ANSYS

6. ... Building a nonlinear model
For any structural element, DOF solution Du is solved at nodes
Stresses and strains are calculated at integration points.
They are derived from DOF.
For example, we can determine strains from displacements via:
Where B is called the strain-displacement matrix
The image on the right shows a 4-node quad element with 2x2 integration, integration points shown in red.
When we post-process results, stress/strain values at integration points are extrapolated or copied to nodal locations
linear results are extrapolated
Nonlinear results are copied
s, e u

7. ... Building a nonlinear model
With Element Control set to Manual, users can manually toggle between Full and Reduced Integration Schemes
This option influences the number of integration points within an element.
This switch only applies to higher order elements.
It is sometimes helpful to force full integration when only one element exists across the thickness of a part for improved accuracy.
ANSYS Details:
In Simulation, the following elements are used:
Solid bodies are meshed with 10-node tetrahedral or 20-node hexahedral elements
SOLID187 and SOLID186
SOLID186 has KEYOPT(3)=2 by default in Simulation. If “Brick Integration Scheme” under the part Details view is changed from “Full” to “Reduced,” then KEYOPT(3)=0 is used. The latter is the default option in ANSYS, and is useful to alleviate volumetric locking.
Surface bodies are meshed with 4-node quad shell elements
SHELL181 using real constants
Section definition (and offsets) are not used
Line bodies are meshed with 2-node beam elements
BEAM188 (with 3rd orientation node)
Section definition and offsets are supported

8. ... Building a nonlinear model
By default, workbench mechanical element technology will mesh geometry with higher order elements (with midside nodes).
Users have the option to drop midside nodes
In challenging large deflection, bending dominated problems with nearly or fully compressible nonlinear materials, it can sometimes be advantageous to drop the midside nodes and allow the code to implement enhanced strain formulations automatically
Refer to Appendix B for a more detailed discussion of element technology.
20-Node Hex
Kept midside nodes
(Quadratic shape function)
8-Node Hex
Dropped midside nodes
(Linear shape function)
ANSYS Details:
In Simulation, the following elements are used:
Solid bodies are meshed with 10-node tetrahedral or 20-node hexahedral elements
SOLID187 and SOLID186
SOLID186 has KEYOPT(3)=2 by default in Simulation. If “Brick Integration Scheme” under the part Details view is changed from “Full” to “Reduced,” then KEYOPT(3)=0 is used. The latter is the default option in ANSYS, and is useful to alleviate volumetric locking.
Surface bodies are meshed with 4-node quad shell elements
SHELL181 using real constants
Section definition (and offsets) are not used
Line bodies are meshed with 2-node beam elements
BEAM188 (with 3rd orientation node)
Section definition and offsets are supported

9. B. Obtaining a nonlinear solution
What is different about obtaining a nonlinear solution?
Multiple matrix solutions:
Linear static requires only one pass through the matrix equation solver (Figure on left)
Nonlinear performs a new solution with every iteration (Figure on right). F F Ki 4 3 2 K 1 u u
What is different about obtaining a nonlinear solution?
The main difference is the need for the Newton-Raphson procedure to build Multiple matrix solutions:
A Linear static analysis requires only one pass through the matrix equation solver.
A Nonlinear analysis requires a new solution with every iteration.
Also, you have many more solution control options to consider in a nonlinear analysis:
A Linear static analysis typically requires no user control of solution options.
A Nonlinear analysis uses solution control options to:
Activate geometric nonlinearities.
Improve convergence behavior.
Manage results file size.
Optimize restart capabilities.
We will discuss the details of nonlinear solution control options in module 5 of this series.
F = Ku
Fi = Kiui

10. ... Obtaining a nonlinear solution
…What is different about obtaining a nonlinear solution?
Analysis settings has many options that need to be considered for a nonlinear run.
Step Control - Load steps and substeps
Solver Control - Solver types
Nonlinear Controls - N-R convergence criteria
Output Controls - controlling what data is saved
thru the load history
In the following slides, we consider each of these tools
What is different about obtaining a nonlinear solution?
The main difference is the need for the Newton-Raphson procedure to build Multiple matrix solutions:
A Linear static analysis requires only one pass through the matrix equation solver.
A Nonlinear analysis requires a new solution with every iteration.
Also, you have many more solution control options to consider in a nonlinear analysis:
A Linear static analysis typically requires no user control of solution options.
A Nonlinear analysis uses solution control options to:
Activate geometric nonlinearities.
Improve convergence behavior.
Manage results file size.
Optimize restart capabilities.
We will discuss the details of nonlinear solution control options in module 5 of this series.

11. ... Obtaining a nonlinear solution
Step Controls
“Auto Time Stepping” under Step Controls, enables user to define an initial, minimum and maximum number of substeps per loadstep.
If Mechanical has trouble converging, it will use these auto time stepping specifications to bisect the solution.
“Bisection applies the load in smaller increments (using more substeps within the specified range) starting from the last successfully converged substep.

12. ... Obtaining a nonlinear solution
Step Controls (cont’d)
If no specifications are defined (Auto Time Stepping = Program Controlled), Mechanical will set specifications automatically depending on the nature of the nonlinearity in the model.
If taking the default auto time stepping specs, user should always verify that these values are adequate by checking the Solution Information folder at the beginning of the run and watching for bisections.
Discussed in more detail in Chapter 7 “Nonlinear Diagnostics”

13. ... Obtaining a nonlinear solution
Solver Controls
Solver Type offers two options, ‘Direct’ and ‘Iterative’.
This is a reference to the way the code builds the stiffness matrix for each Newton-Raphson iteration.
Direct (Sparse) solver is more robust and is recommended for challenging nonlinear models and with noncontinuum elements (shells and beams).
Iterative (PCG) solver is more efficient (in terms of run time) and is recommended for large bulk solid models dominated by linear elastic behavior.
The default ‘Program Controlled” will automatically select a solver based on the problem currently in session.

14. ... Obtaining a nonlinear solution
Solver Controls (cont’d)
By setting “Large Deflection” = ON, in the Solver Control branch of Analysis Settings:
Adjustments will be made to the stiffness matrix over multiple iterations to account for changes in the geometry during the course of the analysis.
Also, stress stiffening effects will be included.

15. ... Obtaining a nonlinear solution
Nonlinear Controls
Tolerances on Convergence are calculated automatically. They are used during the Newton-Raphson process to dictate when a model is Converged or “balanced”
The default convergence criterion works very well for most engineering applications.
For special situations, users can override these defaults to Tighten or loosen the convergence tolerance.
A tighter tolerance gives better accuracy, but can make convergence more challenging

16. ... Obtaining a nonlinear solution
Nonlinear Controls
In addition to force balance, a moment balance will also be included if rotational degrees of freedom (DOF) are present in the model (i.e. when beam and/or shell elements are present for example).

17. ... Obtaining a nonlinear solution
Nonlinear Controls
Balance checks on displacement and/or rotational DOF values can also be added as a supplement to force/moment balances.
When contact nonlinearities are present, these additional checks are not included by default because they are generally considered overly restrictive and can cause unnecessary divergence.

18. ... Obtaining a nonlinear solution
The Force Convergence view shows what the force criterion and residual forces (“force convergence”) are. When the residual forces are less than the criterion, the substep is assumed to be converged.
Additional useful features include the fact that converged substeps and loadsteps are also indicated on this Solution Information chart with a green and blue dotted line, respectively.
Residual
Criteria

19. ... Obtaining a nonlinear solution
Nonlinear Controls (cont’d)
If you change any convergence criteria, the program deletes all the default criteria!
For example, if you override program control by adding a displacement convergence check, the force convergence check will be deleted.
Make sure you reestablish the force convergence check.
After redefining convergence criteria, you should always confirm the specifications reported in the Solution Information branch to ensure intended balance checks are active.

20. ... Obtaining a nonlinear solution
Why must you re-establish a force convergence criterion?
Because displacement-based checking is a relative measure of convergence, it should only be used as a supplement to force-based convergence.
Force-based convergence provides an absolute measure of convergence, as it is a measure of equilibrium between the internal and external forces.
Big Residual
Why must you re-establish a force convergence criterion?
Because displacement-based checking is a relative measure of convergence, it should only be used as a supplement to force-based convergence.
Force-based convergence provides an absolute measure of convergence, as it is a measure of equilibrium between the internal and external forces.
Relying on displacement convergence alone can in some cases lead to erroneous results.
This graph represents the force deflection curve for a fishing rod under large deflection. As expected, the stiffness of the rod increases with increasing deflection. If only a displacement criteria were used to test model convergence for this problem, you run the risk of achieving convergence without adequately balancing the internal reaction with the externally applied load.
Hence, be careful when making adjustments to convergence criteria!
Relying on displacement convergence alone can in some cases lead to erroneous results.

21. ... Obtaining a nonlinear solution
Nonlinear Controls (cont’d)
The Minimum reference value (MINREF) is a safety feature that prevents your solution from trying to converge to a zero tolerance.
If free-body (unconstrained) systems or mechanisms have no external forces, the criterion (eR * ||{F}||2) will be zero. If the criterion is zero, the solution will never converge!
In such cases, the program redefines the criterion to be
(eR * MINREF). Where eR is the convergence tolerance value.
The default value that Simulation uses for MINREF depends on the physics of the problem.
If you do not specify a value for Minimum reference value, you will get a warning.
The Minimum reference value (MINREF) is a safety feature that prevents your solution from trying to converge to a zero tolerance.
If free-body (unconstrained) systems or mechanisms have no external forces, the criterion (eR * ||{F}||2) will be zero. If the criterion is zero, the solution will never converge!
In such cases, the program redefines the criterion to be (eR * MINREF)
The default value that ANSYS uses for MINREF depends on the physics of the problem and SOLCONTROL (ON or OFF).
See documentation on CNVTOL command for MINREF defaults.

22. ... Obtaining a nonlinear solution
Convergence criteria guidelines:
Default convergence criteria work well most of the time.
You should rarely need to change the criteria.
To tighten or loosen a criterion, don’t change the default reference value, but instead change the tolerance factor by one or two orders of magnitude.
Do not use a “loose” criterion to eliminate convergence difficulties.
This simply allows the solution to “converge” to an incorrect result!
Tightening the criterion requires more equilibrium iterations.
Review any MINREF warning messages during solution. Make sure the minimum reference value used makes sense for the problem being solved.
Convergence criteria guidelines:
Default convergence criteria work well most of the time.
You should rarely need to change the criteria.
To tighten or loosen a criterion, don’t change the default reference value, but instead change the tolerance factor by one or two orders of magnitude.
Do not use a “loose” criterion to eliminate convergence difficulties.
This simply allows the solution to “converge” to an incorrect result!
Tightening the criterion requires more equilibrium iterations.
Review any MINREF warning messages during solution. Make sure the minimum reference value used makes sense for the problem being solved.

23. ... Obtaining a nonlinear solution
Nonlinear Controls (cont’d)
Line Search is an additional tool intended to enhance convergence behavior.
When active, line search multiplies the displacement increment by a program-calculated scale factor between 0 and 1, whenever a stiffening response is detected, typical in a contact application.
By default, the program turns line search ON when contact elements are present. You can override the default to turn it on or off explicitly.
Two additional convergence enhancement tools available in the nonlinear tab include:
Line search
Predictor
These tools enlarge the radius of convergence, making convergence behavior more robust and efficient.

24. C. Reviewing nonlinear results
What is different about reviewing nonlinear results?
The procedure for reviewing nonlinear results is similar to that of a linear problem. The difference is that there is usually more information to process
multiple results sets
more information per result set (i.e contact status, pressure, penetration, plastic strain..etc).
A nonlinear analyses produces a response history
A change of status that causes an abrupt change in stiffness is another common cause of nonlinear behavior. For example:
A cable can change status from slack to taut
Two parts in an assembly can come into contact
Machining can remove prestressed material
Animated response history
Response history graph

25. ... Reviewing nonlinear results
In large deformation problems, one usually should view the deformation with “Actual” scaling from the Result toolbar
Any of the structural results may be requested, such as Equivalent Stress, shown below
Model shown is from a sample Unigraphics assembly.

26. ... Reviewing nonlinear results
If contact is defined, a contact tool can be used to postprocess contact related results (pressure, penetration, frictional stress, status,..etc)
We can explore this tool in greater detail in Chapters 3 and 4

27. ... Reviewing nonlinear results
If nonlinear material is defined, various stress and strain components can be requested.
We will explore this in greater detail in Chapters 5 and 6.

28. D. Workshop 2A – Large Deflection
Please refer to your Workshop Supplement for instructions on:
W2A- Small Deflection Vs. Large Deflection Analysis

29. D. Workshop 2B – Assembly Contact
Please refer to your Workshop Supplement for instructions on:
W2B- Assembly Contact