Nonlinear Structural

1
Nonlinear Structural

• Chapter 2

2
Chapter Overview

• The following will be covered in this Chapter
• General Background on Nonlinear Theory
• Setting Up Nonlinear Analyses
• Metal Plasticity
• Solving Nonlinear Models
• Reviewing Results
• The capabilities described in this section are
  generally applicable to ANSYS Structural licenses
  and above.
• Exceptions will be noted accordingly

3
A. Background on Linear Analysis

• In Chapter 4 of the Workbench Simulation Intro
  course, the assumptions and restrictions related
  to performing linear static structural analysis
  were covered
• The matrix equation solved for is Hookes Law
• Because K is assumed to be constant,
  essentially only linear behavior is allowed
• As shown on the figure on the right, if theforce
  doubles, the displacement (and stresses)are
  assumed to double in linear analysis
• In many real-world situations, however, this
  small-displacement theory may not be valid. In
  these situations, nonlinear analysis may be
  required.

4
Background on Nonlinear Analysis

• There are three main sources of nonlinearities
• Geometric nonlinearities If a structure
  experiences large deformations, its changing
  geometric configuration can cause nonlinear
  behavior.
• Material nonlinearities A nonlinear
  stress-strain relationship, such as metal
  plasticity shown onthe right, is another source
  of nonlinearities.
• Contact Include effects of contact is a typeof
  changing status nonlinearity, where anabrupt
  change in stiffness may occur whenbodies come
  into or out of contact with eachother.

5
Background on Nonlinear Analysis

• In a nonlinear static analysis, the stiffness K
  is dependent on the displacement x
• The resulting force vs. displacement curvemay be
  nonlinear, as shown on the right, sodoubling the
  force does not necessarilyresult in doubling of
  the displacementsand stresses
• A nonlinear analysis is an iterative
  solutionbecause this relationship between load
  (F) and response (x) is not known beforehand
• No time-dependent effects are considered.
• It is important to remember these assumptions
  related to performing nonlinear static analyses
  in Simulation.

6
Newton-Raphson Method

• Nonlinear solutions require several iterations
• The actual relationship between load and
  displacement (shown with a yellow dotted line) is
  not known beforehand
• Consequently, a series of linear approximations
  with corrections is performed. This is a
  simplified explanation of the Newton-Raphson
  method (shown as solid red lines)
• In the Newton-Raphson Method, the totalload Fa
  is applied in iteration 1. The resultis x1.
  From the displacements, the internalforces F1
  can be calculated. If Fa ? F1, thenthe system
  is not in equilibrium. Hence,a new stiffness
  matrix (slope of red line) iscalculated based on
  the current conditions.The difference of Fa - F1
  is the out-of-balanceor residual forces. The
  residual forces mustbe small enough for the
  solution to converge.
• This process is repeated until Fa Fi. In this
  example, after iteration 4, the system achieves
  equilibrium and the solution is said to be
  converged.

7
Nonlinear Solution

• It is useful to understand how loads are managed
• Load steps are changes in general loading.
• Simulation usually solves all nonlinear models
  with one load step, but, in the case of
  Pretension Bolt Loads, this is done in two load
  steps. The bolt preload is applied first, then
  all other loads are applied next. These load
  steps can be thought of as Fa and Fb.
• Substeps apply the loads in an incremental
  fashion
• Because of the complex response, itmay be
  necessary to apply the loadincrementally. For
  example, Fa1 may benear 50 of the Fa load.
  After the loadfor Fa1 is converged, then the
  full Fa loadis applied. Fa has 2 substeps while
  Fbhas 3 substeps in this example
• Equilibrium iterations are the correctivesolution
  s to obtain a converged substep
• In the example on right, the iterations between
  the dotted white lines indicate equilibrium
  iterations.

8
Background on Nonlinear Analysis

• In Simulation, the following types of nonlinear
  static structural analyses are directly available
  via the GUI
• Large deflection effects
• Nonlinear contact (I.e. frictionless, frictional,
  no separation)
• Metal plasticity (Bi-linear or Multi-linear
  Isotropic Hardening).
• Many more advanced nonlinear features are not
  available directly in the Simulation interface.
• These items can be added with Command Objects
• Advanced Nonlinear material models (i.e. Creep,
  Hyperelasticity)
• Nonlinear solution options, element formulations,
  and advanced contact options
• Advanced time-history postprocessing

9
B. Nonlinear Analysis Setup

• The procedure for nonlinear static analysis is
  very similar to performing a linear static
  analysis, so not all steps will be covered in
  detail. The steps in yellow italics include
  options that are specific to nonlinear analyses.
• Attach Geometry
• Assign Material Properties (with metal
  plasticity, if applicable)
• This will be covered in detail in Section C
• Define Contact Options (if applicable)
• Define Mesh Controls (optional)
• Include Loads and Supports
• Request Results
• Set Nonlinear Solution Options
• Solve the Model
• Review Results

10
Geometry (Solid Bodies)

• Solid bodies are supported for large-deflection
  analyses with ANSYS Structural licenses and
  above.
• Advanced users can change the Brick Integration
  Scheme from Full to Reduced, which may be
  useful for large-deformation problems.

11
Geometry (Line/Surface Bodies)

• ANSYS Professional licenses and above support
  large-deformation analyses with surface or line
  bodies.
• Note that ANSYS Professional does not support a
  combination of line and surface bodies. ANSYS
  Structural and above must be used in these cases.

12
Solid Body Contact Options

• All of the contact options available in linear
  static analyses are also available for nonlinear,
  large-deflection analyses in ANSYS Structural
  licenses and above
• In general, face-to-face contact for solid bodies
  is the only type of contact which supports
  advanced nonlinear options
• Most other contact involving surface bodies or
  solid edges support bonded (and no separation)
  contact only

13
Meshing Controls

• 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, Simulation
  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 Ch. 3 from the
  Workbench Simulation -
• Intro course for some ways to detect andremedy
  mesh failures.

14
Loads and Supports

• Most loads and supports used in linear analyses
  may also be used in large-deflection analyses
• Thermal-stress analyses are supported for
  large-deflection analyses.
• See Chapter 6 of the Workbench Simulation Intro
  course on details of performing thermal analyses
• ANSYS Structural licenses do not support any
  thermal loads
• Recall that ANSYS Professional does not support
  large-deflection analyses for solid bodies
• Two unique items for loads and supports in
  large-deflection analyses will be covered next
• Orientation of loads for large-deflection
• Pretension Bolt Load

15
Load Orientation

• It is important to note the orientation of loads
  and its effect on the structure in
  large-deflection analyses

16
Pretension Bolt Load

• A Pretension Bolt Load is available in ANSYS
  Structural
• Pretension Bolt Load is applied on a single
  cylindrical surface
• Each load must be applied to only one set of
  cylindrical surface(s)
• For multiple loads, add separate Pretension Bolt
  Loads branches
• Usually, a preload value is input in the Details
  view
• If the torque is known, this can be converted to
  a preload force
• If known, an initial adjustment can be directly
  applied
• Internally, preloads are applied in two steps
• The preload value is applied first, which
  shortens the grip length
• The grip length is then fixed, and any other
  loads are then applied

17
Pretension Bolt Load

• A Pretension Bolt Load is useful to account for
  the effect of the preload in bolts, which is
  caused by their tightening
• The loss of preload and the effect the preload
  has on contact regions can be included in this
  manner, enabling for more complex simulation of
  real-world assemblies.
• Contact options for parts connected with
  fasteners should be set separately in the Contact
  branch. The Pretension Bolt Load only controls
  the load on the cylindrical surface representing
  the bolt.
• The adjustment or preload is applied in two
  steps.
• In real life, if the fastener is tightened, its
  grip length changes.
• Simulation mimics this the same way by first
  applying only the preload or adjustment. If the
  preload is defined, the adjustment (shortening of
  the grip length) is calculated. The given or
  calculated adjustment shortens the grip length of
  the bolt.
• All other external loads are then applied in the
  second load step, once the grip length is
  shortened.

18
Pretension Bolt Load

• In large-deflection analyses, the orientation of
  the Pretension Bolt Load is not updated
• The Pretension Bolt Load should not be applied on
  any part that undergoes large rotation
• The Pretension Bolt Load is applied in the center
  of the solid body containing the cylindrical
  surface
• Verify the mesh, and ensure that no constraints
  or bonded contact is present near the center of
  the bolt solid body. Otherwise, the preload
  may be overconstrained.
• The Adjustment and Working Load can be reviewed
• After the solution, in the Details view, the
  adjustment caused by the preload is shown.
  Also, the working load is provided, so the user
  can determine how much preload was lost.

The Adjustment and Working Load information is
also available in the Worksheet tab of the
Environment branch
19
C. Metal Plasticity

• What is plasticity?
• When a ductile material experiences stresses
  beyond the elastic limit, it will yield,
  acquiring large permanent deformations.
• Plasticity refers to the material response beyond
  yield.
• Plastic response is important for metal forming
  operations.
• Plasticity is also important as an
  energy-absorbing mechanism for structures in
  service.
• Materials that fail with little plastic
  deformation are said to be brittle.
• Ductile response is safer in many respects than
  is brittle response.
• This section will review some basics of
  plasticity by defining certain terminology.

20
Elasticity

• Review of Elasticity
• Before proceeding to a discussion on plasticity,
  it may be useful to review elasticity of metals.
• In elastic response, if the induced stresses are
  below the materials yield strength, the material
  can fully recover its original shape upon
  unloading.
• From a standpoint of metals, this behavior is due
  to the stretching but not breaking of chemical
  bonds between atoms. Because elasticity is due
  to this stretching of atomic bonds, it is fully
  recoverable. Moreover, these elastic strains
  tend to be small.
• Elastic behavior of metals is most commonly
  described by the stress-strain relationship of
  Hookes Law

21
Plasticity

• Review of Plasticity
• Plastic deformation results from slip between
  planes of atoms due to shear stresses (deviatoric
  stresses). This dislocation motion is
  essentially atoms in the crystal structure
  rearranging themselves to have new neighbors
• results in unrecoverable strains or permanent
  deformation after load is removed.
• slipping does not generally result in any
  volumetric strains (condition of
  incompressibility), unlike elasticity

22
Rate-Independent Plasticity

• Rate-Independent Plasticity
• If the material response is not dependent on the
  rate of loading or deformation, the material is
  said to be rate-independent.
• Most metals exhibit rate-independent behavior at
  low temperatures (lt 1/4 or 1/3 melting
  temperature) and low strain rates.
• Engineering vs. True Stress-Strain
• While engineering stress-strain can be used for
  small-strain analyses, true stress-strain must be
  used for plasticity, as they are more
  representative measures of the state of the
  material.

23
True Stress and Strain

• Engineering vs. True Stress-Strain (contd)
• If presented with engineering stress-strain data,
  one can convert these values to true
  stress-strain with the following approximations
• Up until twice the strain at which yielding
  occurs
• Up until the point at which necking
  occursNote that, only for stress conversion,
  the following is assumed
• Material is incompressible (acceptable
  approximation for large strains)
• Stress distribution across cross-section of
  specimen is assumed to be uniform.
• Beyond necking
• There is no conversion equation relating
  engineering to true stress-strain at necking.
  The instantaneous cross-section must be measured.

24
Yield Criterion (Yield Point)

• Yield Criterion
• The yield criteria is used to relate multiaxial
  stress state with the uniaxial case.
• Tensile testing on specimens provide uniaxial
  data, which can easily be plotted on
  one-dimensional stress-strain curves, such as
  those presented earlier in this section.
• The actual structure usually exhibits multiaxial
  stress state. The yield criterion provides a
  scalar invariant measure of the stress state of
  the material which can be compared with the
  uniaxial case.
• A common yield criterion is the von Mises yield
  criterion (also known as the octahedral shear
  stress or distortion energy criterion). The von
  Mises equivalent stress is defined as

25
Mises Yield Criterion

• If plotted in principal stress space, the von
  Mises yield surface is a cylinder.

Inside the yield surface, as noted earlier,
behavior is elastic. Note that the multiaxial
stress state can exist anywhere inside of the
cylinder. At the edge of the cylinder (circle),
yielding will occur. No stress state can exist
outside of the cylinder. Instead, hardening
rules will describe how the cylinder changes with
respect to yielding.
26
Hardening Rules

• Hardening Rules
• The hardening rule describes how the yield
  surface changes (size, center,shape) as the
  result of plastic deformation.
• The hardening rule determines when the material
  will yield again if the loading is continued or
  reversed.
• This is in contrast to elastic-perfectly-plastic
  materials which exhibit no hardening -- i.e., the
  yield surface remains fixed.

27
Isotropic Hardening

• Isotropic Hardening
• Isotropic hardening states that the yield surface
  expands uniformly during plastic flow. The term
  isotropic refers to the uniform dilatation of
  the yield surface and is different from an
  isotropic yield criterion (i.e., material
  orientation).

28
Isotropic Hardening

• Plotting the stress-strain curve enables an
  understanding of what occurs during a loading and
  reverse loading cycle

Note that the subsequent yield in compression is
equal to the highest stress attained during the
tensile phase. Isotropic hardening is often
used for large strain or proportional loading
simulations. It is usually not applicable cyclic
loading.
29
Stress-Strain Curve Representation

• Curve shapes
• Two different type of stress-strain curve
  representations are possible

30
Summary of Plasticity in Simulation

• In Simulation, metal plasticity can be included
  as part of the model. The following points
  should be remembered
• Metal plasticity deals with elastic and inelastic
  (permanent) deformation. Inelastic or plastic
  deformation occurs when the stress is higher than
  the yield strength. There will always be some
  recoverable strain (elastic strain) upon
  unloading.
• A stress-strain curve is based on scalar data,
  usually from a uniaxial test. A system may
  undergo a multiaxial stress state, so Simulation
  uses the Mises yield criterion to relate a
  multiaxial stress state with scalar test data.
  In this situation, true stress vs. strain data
  should be supplied.
• After yielding occurs, the yield point may
  increase due to strain hardening. This changes
  the yield surface, and the way in which it
  evolves in Simulation is determined by isotropic
  hardening assumption.
• The stress-strain curve can be represented by a
  bilinear or multilinear curve.

31
Material Properties

• Linear elastic material properties must be
  supplied
• The same requirements exist for linear static
  structural analyses, namely that Youngs Modulus
  and Poissons Ratio must be defined as a minimum.
• Metal plasticity is available as a nonlinear
  material model. This will be discussed next.
• Other nonlinear constitutive models may be added
  with the Preprocessing Command Builder
• However, note that only ANSYS Structural licenses
  and above support nonlinear material laws.
• ANSYS Professional supports large-deflection
  analyses of surface or line bodies, but it does
  not support any material nonlinearities

32
Metal Plasticity

• To add metal plasticity, first navigate to the
  specific part or parts under the geometry branch.
  In the Details window, highlight the material
  you wish to modify

33
Metal Plasticity

• Right side of the Engineering Data application
  shows the currently defined properties. Choose
  Add/Remove Properties to continue.

34
Metal Plasticity

• Select either Bilinear or Multilinear
  Isotropic Hardening under Nonlinear gt
  Plasticity.
• Multilinear representation usually provides a
  more accurate description of stress-strain curve
  than Bilinear.

35
Metal Plasticity

• To enter or modify the plasticity definition
  click either chart icons for the property.

• To return to the general material property
  display use the Close Curve icon.

36
Bilinear Stress-Strain

• The Bilinear Stress-Strain requires two input
  values
• The Yield Strength and Tangent Modulus is
  input in the Details view.

The yield strength is the value at which plastic
straining occurs. The tangent modulus is the
slope of the stress-strain curve after
yielding. As the name implies, the Bilinear
Stress-Strain provides a simple representation
of metal plasticity
37
Multilinear Stress-Strain

• The Multilinear Stress-Strain allows
  stress-strain input
• Right-click on the spreadsheet to add rows
• Input as many Strain and Stress values as needed
• The stress-strain plot will be displayed
  dynamically

The origin (0,0) should be the first point.
Also, ensure that the second point has the same
slope as the Youngs modulus. Simulation assumes
perfect plasticity (zero slope) beyond the
defined stress-strain values.
38
Large Deflection with Metal Plasticity

• Workshop 2A

39
D. Workshop 2A Metal Plasticity

• Goal
• Compare and contrast results using small
  deflection, large deflection and large deflection
  with metal plasticity on a model with identical
  loads and boundary conditions.
• Model Description
• 3D large deflection of spring plate
• Spring plate
• Ductile steel
• Loads and Boundary Conditions
• Fixed support
• 3 Mpa Pressure load at opposite end

40
Workshop 2A Metal Plasticity

• Steps to Follow
• Start an ANSYS Workbench session. Browse for and
  open Spring_ws01.wbdb project file.
• This project contains a Design Modeler (DM)
  geometry file Spring_ws01.agdb and a Simulation
  (S) file Spring_ws01.dsdb.
• Highlight the the Model, Small Deflection-Linear
  Matl (Spring_ws01.dsdb) file and open a
  Simulation Session.

41
Workshop 2A Metal Plasticity

• Review the contents of the model

Highlight geometry Solid branch and examine the
Details of Solid Window (lower left corner of
screen). Note we will start with a structure
steel and Nonlinear Material Effects off. The
boundary conditions and load (3Mpa Pressure) have
already been defined. Highlight the
Solution branch. Note We accept the default
settings, including Large Deflection Off
42
Workshop 2A Metal Plasticity

• Add a Solution Information Folder to the Solution
  Branch
• Run the Solution
• Solution, RMB SOLVE
• After solution run is complete, open the Solution
  Information folder and scroll to near the bottom
  of the output. As expected, this solves in one
  iteration.

43
Workshop 2A Metal Plasticity

• Review the displacement and stress results from
  this first run.

44
Workshop 2A Metal Plasticity

• Highlight the Small Deflection- Linear Matl
  Branch at the top of the Project Tree, and
  duplicate this Branch with RMBgt Duplicate.
• Change the new branch name to Large Deflection -
  Linear Matl
• Highlight Solution Branch and turn Large
  Deflection ON
• The Project tree should look as shown in figure
  to the right.
• Execute a Solve on this new Solution

45
Workshop 2A Metal Plasticity

• After solution run is complete, open the Solution
  Information folder and scroll to near the bottom
  of the output. Note the solution still solves in
  one substep, but 9 iterations were made on the
  stiffness matrix during the run to account for
  large deflection effects.
• Change Solution Output to Force Convergence to
  review the Newton-Raphson History.

46
Workshop 2A Metal Plasticity

• Review the large deflection analysis displacement
  and stress results and compare with the first
  run. Note Total Deformation is larger, but
  max equivalent stress is actually slightly lower
  and in a different location then the linear run.
• Extra Credit To better understand the
  differences, try post processing x and y
  deflections and equivalent strains separately for
  both runs. Note the dramatic increase in the y
  deflections especially and the different
  distributions of strain energies.

47
Workshop 2A Metal Plasticity

• Highlight the Large Deflection- Linear Matl
  Branch and duplicate this Branch with RMBgt
  Duplicate.
• Change the new branch name to Large
  Deflection-NonLinear Matl
• Add metal plasticity
• Highlight Geometry Solid branch
• Activate Nonlinear material effects (YES)
• RMB on Structural Steel
• Select Edit Structural Steel
• Select Add/Remove Properties
• Activate Bilinear Isotropic Hardening Plasticity
• OK

48
Workshop 2A Metal Plasticity

• Click on the ICON to the right of Bilinear
  Isotropic Hardening
• Define Yield Strength of 250Mpa and a Tangent
  Modulus of 10000Mpa.
• Select Close Curve

• Return to project tree and execute a solve on
  this latest Solution

49
Workshop 2A Metal Plasticity

• This last solution run can take up to two minutes
  depending on machine.
• Review the Solution Convergence History as
  before.
• It now takes 42 iterations in eight substeps,
  including two bisections.

50
Workshop 2A Metal Plasticity

• Review the displacement and stress results and
  compare with the large deflection run. Note
  Total Deformation is considerably larger and
  stresses come down due to the dramatic loss of
  stiffness as part goes plastic.

51
Workshop 2A Metal Plasticity

• Add Equivalent Plastic Strain to the solution
  branch for a better picture of where most of the
  yielding occurs.

52
E. Solving Nonlinear Models

• The solution options for nonlinear analyses are
  the same for linear analyses. However, for
  large-deflection problems, the user has an
  additional option of turning on Large
  Deflection
• Use of the Large Deflection option accounts for
  changes in the geometry during the course of the
  analysis.
• ANSYS Professional only supports large-deflection
  analyses for surface or line bodies.
• The Newton-Raphson method is employed in
  nonlinear solutions (see next slides)

53
Nonlinear Solution

• Simulation automates nonlinear solutions by
  automatically determining the number of load
  steps, substeps, and equilibrium iterations
• In this way, the user does not have to worry
  about these settings. However, as will be shown
  later, it is very useful to understand these
  concepts in dealing with nonlinear solutions
• During the course of the analysis, if Simulation
  has trouble converging, it will bisect the
  solution.
• This means that Simulation will apply the load in
  smaller increments (more substeps). This usually
  helps for difficult problems since the response
  will be easier to converge if a smaller load is
  applied. The final, total load will be solved
  for in the end.

54
Nonlinear Solution

• The number of load steps is usually set to 1
• If Pretension Bolt Loads are present, there will
  be 2 load steps
• For thermal-stress analyses, the thermal analysis
  is performed first as a separate analysis.
  Hence, this part is not considered a load step
  since it is a different type of analysis.
• The initial number of substeps is usually set to
  1
• If frictional contact with a Friction Coefficient
  ? 0.2 is present, this results in 5 initial
  substeps
• The max number of equilibrium iterations is
  usually around 20
• The type of contact will dictate the maximum
  number of equilibrium iterations
• If a substep cannot be converged within the
  specified number of equilibrium iterations,
  Simulation will bisect the solution. It will
  apply half of the current load and run
  equilibrium iterations again to converge.
  Usually, this is repeated until 10 of the load
  is applied. If the solution still does not
  converge, Simulation will stop and produce an
  error message.

55
Nonlinear Solution

• Auto Time Stepping specifications can be changed
  within Simulation in the Details of Solution
  Window
• Change Auto Time Stepping from Program
  Controlled to On
• Manually define the initial, minimum and maximum
  values.

56
Nonlinear Solution Output

• Nonlinear solution output from the ANSYS solver
  is requested with the Solution Information
  branch
• When requested, the Solution Information
  branchmay be used to display Solver Output or
  ForceConvergence progress, among a number of
  otheroptions from the pull-down menu
• The Update Interval allows users to specify (in
  seconds) how frequency this output is updated
• The Solver Output and Force Convergence
  provide details on the nonlinear solution
  progress.

57
Nonlinear Solver Output

• Nonlinear solutions, especially those dealing
  with frictionless or frictional contact, can be
  difficult to solve
• During the solution, it is useful to become
  familiar with reading the ANSYS solver output
• In the Solution Information branch, informative
  messages about the solution, solver, and contact
  settings are usually printed first when solution
  is initiated
• It may be useful to browse through the contact
  information (sample below) to ensure that initial
  gaps or initial penetration is not very large.
  If an initial gap is automatically closed, this
  will also be printed in the output.

58
Nonlinear Solver Output

• As the nonlinear solution progresses, the
  equilibrium iteration information is shown
  (sample below)
• Note that for each equilibrium iteration, the
  residual forces (FORCE CONVERGENCE VALUE) must be
  lower than the CRITERION
• Ideally, the residual or out-of-balance forces
  should be zero for a system to be in equilibrium.
  However, because of machine precision and
  practical concerns, Simulation determines a value
  small enough to result in negligible error. This
  value is the CRITERION, and the FORCE CONVERGENCE
  VALUE must be smaller than the CRITERION for the
  substep to be converged.
• In the example below, after 3 equilibrium
  iterations, the residual forces are lower than
  the criterion, so the solution is converged.
• Informative messages (such as convergence or
  bisection) are noted with gtgtgt and ltltlt in the
  output.

59
Nonlinear Solver Output

• By understanding how to read the solution output,
  potential problems can be detected early on
• In the contact output below, there are notes of
  initial penetration and initial gaps.
• One should always verify automatically-generated
  contact regions
• The improper specification of contact may cause
  convergence difficulties, so reading the contact
  output would be helpful in determining if any
  contact region is problematic
• Initial penetration/gaps are reported in active
  length units

60
Nonlinear Solver Output

• During the equilibrium iterations, reviewing the
  pattern of the residual forces will help
  determine if a solution is diverging
• In the example below, the residual forces (FORCE
  CONVERGENCE VALUE) initially decreases but then
  starts to increase dramatically. In this
  situation, the user can abort the solution and
  check his/her model to see what caused the high
  residual forces. Otherwise, Simulation may
  continue for several more iterations (and even
  bisect the solution) until it diverges, which
  would take longer.
• Some causes of high residual forces include
  excessively large loading (verify units), high
  contact stiffness (especially for thin,
  bending-dominated behavior), or high friction
  coefficient values.

61
Nonlinear Solver Output

• Warning and error messages will also be printed
  in the output
• When contact status changes abruptly, this is
  just a warning indicating that the contact
  elements enter or exit the pinball region
  drastically. This may be due to parts sliding or
  separating drastically if the load is too high.
  Simulation may automatically bisect the solution,
  if necessary.
• Element distortion messages are usually severe
  problems due to excessive loading or
  over-constraints. Bisection of the load is
  automatically performed, but sometimes corrective
  measures may need to be taken to fix the problem.

62
Nonlinear Force Convergence

• The Solver Output option shows detailed text
  information. If Solution Output is changed to
  Force Convergence, the force convergence
  behavior is shown graphically

63
Nonlinear Force Convergence

• 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.

64
Results Tracker

• Besides monitoring the out-of-balance forces, a
  Results Tracker is available from the Solution
  Information branch
• The Results Tracker enables users to monitor
  deformation at a vertex and/or contact region
  information during the solution.
• For Results Tracker gt Deformation, select a
  vertex of interest and specify whether x, y, or z
  deformation is to be monitored.
• For Results Tracker gt Contact, a pull-down menu
  enables users to select a contact region. Then,
  the quantity to track (such as number of
  contacting elements) can be displayed.

65
Results Tracker

• After the Results Tracker items are requested and
  solution initiated, users may track the
  deformation or contact results during the course
  of the solution.

66
Nonlinear Solution

• It is the users responsibility to determine
  whether or not large deformation effects are
  significant and need to be considered.
• Simulation has some basic checks after the
  solution, where if the deformation is large
  compared to the overall geometry size, the
  warning below will appear
• This, however, occurs for obvious, exaggerated
  cases. It does not mean that if the warning does
  not appear in a linear analysis that large
  deformation effects may not be significant.

67
Newton-Raphson Residuals

• As emphasized earlier, the Newton-Raphson method
  employs multiple iterations until force
  equilibrium is achieved. For debugging purposes,
  it may be useful to request the Newton-Raphson
  Residuals (i.e., residual forces) to see what
  locations have high residuals which may be the
  cause of force equilibrium not being satisfied.
• In the Solution Information details view, enter
  the number of equilibrium iterations to retrieve
  Newton-Raphson Residuals. For example, if 3 is
  entered, the residual forces from the last three
  iterations will be returned if the solution is
  aborted or does not converge.

68
Newton-Raphson Residuals

• After solution is stopped or fails to converge,
  residuals will be available under the Solution
  Information branch, as shown below.

69
F. Reviewing Results

• Requesting and reviewing results are similar to
  linear static structural analyses
• 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.
70
Reviewing Results - Equivalent Plastic Strain

• If plasticity is defined, equivalent plastic
  strain can be requested as output (example shown
  below)
• Total equivalent strain is the sum of equivalent
  elastic and equivalent plastic strain. Total
  equivalent strain is used to correlate to the
  stress-strain curve.

71
Reviewing Results

• Animations of nonlinear solutions linearly
  increase from zero to the final value
• The actual load history is not accounted for in
  the animation
• If Pretension Bolt Loads are present, only the
  second load step (externally applied loads after
  adjustment) is animated, as shown in the example
  below

This model has Pretension Bolt Loads applied on
the three bolts. Although the solution consisted
of two load steps simulating the assembly and
loading processes, only the final result is
animated. This final result is animated in a
linear fashion from zero to the final value. The
actual load history is not contained in the
animation (i.e., if multiple substeps were solved
for, they are not included in the animation)
72
Bolt Pretension with Contact

• Workshop 2B

73
G. Workshop 2B Goals

• Goal
• In this workshop our goal is to investigate the
  behavior of the pipe clamp assembly
  (Pipe_clamp.x_t) shown here. Specifically we
  wish to determine the crushing stress and
  deformation in a copper pipe section when the
  bolt in the clamp is torqued down.

74
. . . Workshop 2B Assumptions

• We will assume the material used for the pipe is
  a copper alloy while all other parts are steel.
• It is assumed the clamp is torqued to 1000 N when
  placed in service.
• Well assume the coefficient of friction between
  the clamp and pipe is 0.4. The other contact
  regions will be treated as either bonded or no
  separation as shown in the accompanying figures.

75
. . . Workshop 2B - Start Page

• From the launcher start Simulation.
• Choose Geometry gt From File . . . and browse
  to the file Pipe_clamp.x_t.
• When Workbench Simulation starts, close the
  Template menu by clicking the X in the corner
  of the window.

76
. . . Workshop 2B Preprocessing

• Change the working unit system to metric mm.
• Units gt Metric (mm, kg, MPa, C, s)
• Insert the material Copper Alloy from the
  material library.
• Highlight the Part 2 in the geometry branch
  (pipe).
• Click in the Material field and Import.

1.
2.
3.
77
. . . Workshop 2B Preprocessing

1. Select Copper Alloy material.

4.
78
. . . Workshop 2B Preprocessing

1. Expand the Contact branch and use the shift key
   to highlight all contact definitions.
2. In the details window change the Formulation to
   Augmented Lagrange.

5.
6.
79
. . . Workshop 2B Preprocessing

• Highlight the first contact branch. This is the
  definition for the pipe to clamp contact.
• In the detail for the definition change the Type
  to Frictional.
• Enter a value for Friction Coefficient of 0.4.

7.
8.
9.
80
. . . Workshop 2B Preprocessing

• Highlight the second contact branch. This is the
  definition for the bolt shaft to clamp hole
  contact.
• From the details window change the Type to No
  Separation.
• The remaining 2 contact regions will be modeled
  using the default bonded type of contact.

10.
11.
81
. . . Workshop 2B Preprocessing

• Create a local coordinate system along the pipes
  axis. Note, we will use the local coordinate
  system for post processing later.
• Highlight the Model branch.
• RMB gt Insert gt Coordinate Systems.
• Notice the result is a new branch Coordinate
  Systems appears in the tree. Also, the Global
  Coordinate System is automatically placed in the
  branch.

12.
13.
82
. . . Workshop 2B Preprocessing

• With the Coordinate system branch highlighted
• Select the inside surface of the cylinder.
• RMB gt Insert gt Coordinate System.

14.
15.
83
. . . Workshop 2B Preprocessing

1. From the detail for the new coordinate system
   change Type to Cylindrical.
2. Click to Change in the Z Direction field to
   change the systems orientation.
3. Select the inner surface of the pipe.
4. Apply in the detail window.

18.
19.
84
. . . Workshop 2B - Environment

1. Highlight the Environment branch.
2. Select one of the end surfaces of the pipe.
3. RMB gt Insert gt Fixed Support.

85
. . . Workshop 2B - Environment

1. Select the cylindrical face of the bolt part.
2. RMB gt Insert gt Bolt
3. In the detail for the pretension bolt load enter
   a Preload value of 1000.

23.
86
. . . Workshop 2B Solution Setup

1. Highlight the solution branch.
2. RMB gt Insert gt Stress gt Equivalent (von Mises).
3. RMB gt Insert gt Deformation gt Total.

87
. . . Workshop 2B Solution Setup

1. Switch to Body select mode.
2. Select the pipe part.

30.
88
. . . Workshop 2B Solution Setup

• RMB gt Insert gt Deformation gt Directional.
• From the detail for the Directional Deformation
  change to Coordinate System.
• Note we allowed the default name Coordinate
  System to be used when the local system was
  created. We could easily change the name to a
  more meaningful one.

32.
89
. . . Workshop 2B Solution Setup

• Switch to face select mode.
• Highlight the outer surface of the pipe.
• RMB gt Insert gt Contact Tool gt Pressure.
• Repeat steps 34 and 35 inserting contact
  Frictional Stress.
• Solve

34.
90
. . . Workshop 2B Solution Notes

• The solution for this workshop will take several
  minutes or more depending on the available
  hardware.
• The use of frictional contact triggers a
  nonlinear solution requiring equilibrium
  iterations. The solution progress can be viewed
  by inserting the Solution Information object.
• The use of the pretension bolt load also causes 2
  solutions to be run. The first applies the
  pretension load and locks it down. The second
  applies any remaining loads.

91
. . . Workshop 2B - Results

• Recall that the solution triggered the use of
  Weak Spring stabilization. To insure that the
  weak springs are not the result of rigid body
  motion, highlight the Environment branch and
  inspect the weak spring reaction forces.
• Here we can see that the reaction in the weak
  springs is of the order e-5, a negligible value.

92
. . . Workshop 2B - Results

• Highlighting and plotting the Total Deformation
  for the assembly shows the plot is not
  particularly useful for our goal (investigation
  of pipes behavior).
• The scoped result we placed in the solution
  branch will be more instructive.

93
. . . Workshop 2B - Results

• Highlight and plot the result Directional
  Deformation.
• In this case the result is scoped only to the
  pipe section. Also, since we employed a local
  cylindrical system at the pipe axis, the X
  direction here is displayed in the radial sense.

94
. . . Workshop 2B - Results

• Similarly, the behavior of the contact region can
  be view by highlighting the contact result
  objects. Again the use of scoped results allows
  a more intuitive plot of the quantity displayed.