Static Structural Analysis

1
Static Structural Analysis

• Chapter Four

2
Chapter Overview

• In this chapter, performing linear static
  structural analyses in Simulation will be
  covered
• Geometry and Elements
• Contact and Types of Supported Assemblies
• Environment, including Loads and Supports
• Solving Models
• Results and Postprocessing
• The capabilities described in this section are
  generally applicable to ANSYS DesignSpace Entra
  licenses and above.
• Some options discussed in this chapter may
  require more advanced licenses, but these are
  noted accordingly.
• Free vibration, harmonic, and nonlinear
  structural analyses are not discussed here but in
  their respective chapters.

3
Basics of Linear Static Analysis

• For a linear static structural analysis, the
  displacements x are solved for in the matrix
  equation belowThis results in certain
  assumptions related to the analysis
• K is essentially constant
• Linear elastic material behavior is assumed
• Small deflection theory is used
• Some nonlinear boundary conditions may be
  included
• F is statically applied
• No time-varying forces are considered
• No inertial effects (mass, damping) are included
• It is important to remember these assumptions
  related to linear static analysis. Nonlinear
  static and dynamic analyses are covered in later
  chapters.

4
A. Geometry

• In structural analyses, all types of bodies
  supported by Simulation may be used.
• For surface bodies, thickness must be supplied
  in the Details view of the Geometry branch.
• The cross-section and orientation of line bodies
  are defined within DesignModeler and are imported
  into Simulation automatically.
• For line bodies, only displacement results are
  available.

5
Point Mass

• A Point Mass is available under the Geometry
  branch to mimic weight not explicitly modeled
• A point mass is associated with surface(s) only
• The location can be defined by either
• (x, y, z) coordinates in any user-defined
  Coordinate System
• Selecting vertices/edges/surfaces to define
  location
• The weight/mass is supplied under Magnitude
• In a structural static analysis, the point mass
  is affected by Acceleration, Standard Earth
  Gravity, and Rotational Velocity. No other
  loads affect a point mass.
• The mass is connected to selected
  surfacesassuming no stiffness between them.
  This isnot a rigid-region assumption but similar
  to a distributed mass assumption.
• No rotational inertial terms are present.

6
Point Mass

• A point mass will be displayed as a round, grey
  sphere
• As noted previously, only inertial loads affect
  the point mass.
• This means that the only reason to use a point
  mass in a linear static analysis is to account
  for additional weight of a structure not modeled.
  Inertial loads must be present.
• No results are obtained for the Point Mass itself.

7
Material Properties

• The required structural material properties are
  Youngs Modulus and Poissons Ratio for linear
  static structural analyses
• Material input is under the Engineering Data
  branch, and material assignment is per part under
  the Geometry branch
• Mass density is required if any inertial loads
  are present
• Thermal expansion coefficient and thermal
  conductivity are required if any thermal loads
  are present
• Thermal loading not available with an ANSYS
  Structural license
• Negative thermal expansion coefficient may be
  input (shrinkage)
• Stress Limits are needed if a Stress Tool result
  is present
• Fatigue Properties are needed if Fatigue Tool
  result is present
• Requires Fatigue Module add-on license
• Specific loading and result tools will be
  discussed later

8
Material Properties

• Engineering Data view of sample material shown
  below

9
B. Assemblies Solid Body Contact

• When importing assemblies of solid parts, contact
  regions are automatically created between the
  solid bodies.
• Surface-to-surface contact allows non-matching
  meshes at boundaries between solid parts
• Tolerance controls under Contact branch allows
  the user to specify distance of auto contact
  detection via slider bar

10
Assemblies Solid Body Contact

• In Simulation, the concept of contact and target
  surfaces are used for each contact region.
• One side of the contact region is comprised of
  contact face(s), the other side of the region
  is made of target face(s).
• The integration points of the contact surfaces
  are restricted from penetrating through the
  target surfaces (within a given tolerance). The
  opposite is not true, however.
• When one side is the contact and the other side
  is the target, this is called asymmetric contact.
  On the other hand, if both sides are made to be
  contact target, this is called symmetric
  contact since neither side can penetrate the
  other.
• By default, Simulation uses symmetric contact
  for solid assemblies.
• For ANSYS Professional licenses and above, the
  user may change to asymmetric contact, as
  desired.

11
Assemblies Solid Body Contact

• Four contact types are available
• Bonded and No Separation contact are basically
  linear behavior and require only 1 iteration
• Frictionless and Rough contact are nonlinear and
  require multiple iterations. However, note that
  small deflection theory is still assumed.
• When using these options, an interface
  treatmentoption is available, set either as
  Actual Geometry(and Specified Offset) or
  Adjusted to Touch.The latter allows the user
  to have ANSYS close the gap to just touching
  position. This is availablefor ANSYS
  Professional and above.

12
Assemblies Solid Body Contact

• For the advanced user, some of the contact
  options can be modified
• Formulation can be changed from Pure Penalty to
  Augmented Lagrange, MPC, or Normal
  Lagrange.
• MPC is applicable to bonded contact only
• Augmented Lagrange is used in regular ANSYS
• The pure Penalty method can be thought of as
  adding very high stiffness between interface of
  parts, resulting in negligible relative movement
  between parts at the contact interface.
• MPC formulation writes constraint equations
  relating movement of parts at interface, so no
  relative movement occurs. This can be an
  attractive alternative to penalty method for
  bonded contact.

13
Assemblies Solid Body Contact

• Advanced options (continued)
• As explained in Chapter 3, the pinball region can
  be input and visualized
• The pinball region defines location of near-field
  open contact. Outside of the pinball region is
  far-field open contact.
• Originally, the pinball region was meant to more
  efficiently process contact searching, but this
  is also used for other purposes, such as bonded
  contact
• For bonded or no separation contact, if gap or
  penetration is smaller than pinball region, the
  gap/penetration is automatically excluded
• Other advanced contact options will be discussed
  in Chapter 11.

14
Assemblies Surface Body Contact

• For ANSYS Professional licenses and above, mixed
  assemblies of shells and solids are supported
• Allows for more complex modeling of assemblies,
  taking advantage of the benefits of shells, when
  applicable
• More contact options are exposed to the user
• Contact postprocessing is also available
  (discussed later)

15
Assemblies Surface Body Contact

• Edge contact is a subset of general contact
• For contact including shell faces or solid edges,
  only bonded or no separation behavior is allowed.
• For contact involving shell edges, only bonded
  behavior using MPC formulation is allowed.
• For MPC-based bonded contact, user can set the
  search direction (the way in which the
  multi-point constraints are written) as
  eitherthe target normal or pinball region.
• If a gap exists (as is often the case with shell
  assemblies), the pinball region can beused for
  the search direction to detect contact beyond a
  gap.

16
Assemblies Contact Summary

• A summary of contact types and options available
  in Simulation is presented in the table below
• This table is also in the Simulation online help.
  Please refer to this table to determine what
  options are available.
• Note that surface body faces can only participate
  in bonded or no separation contact. Surface body
  edges allow MPC-based bonded contact only.

17
Assemblies Spot Weld

• Spot welds provide a means of connecting shell
  assemblies at discrete points
• For ANSYS DesignSpace licenses, shell contact is
  not supported, so spotwelds are the only way to
  define a shell assembly.
• Spotweld definition is done in the CAD software.
  Currently, only DesignModeler and Unigraphics
  define spotwelds in a manner that Simulation
  supports.
• Spotwelds can also be created in Simulation
  manually, but only at discrete vertices.

18
C. Loads and Supports

• There are four types of structural loads
  available
• Inertial loads
• These loads act on the entire system
• Density is required for mass calculations
• These are only loads which act on defined Point
  Masses
• Structural Loads
• These are forces or moments acting on parts of
  the system
• Structural Supports
• These are constraints that prevent movement on
  certain regions
• Thermal Loads
• Structurally speaking, the thermal loads result
  in a temperature field, which causes thermal
  expansion on the model.

19
. . . Time Type

• A time type option is available at certain
  license levels.
• The default time type for loading is static
• Sequence and harmonic time types are
  available as options (harmonic analysis is
  covered in the Advanced WB training)
• Sequence loading allows a series of static time
  steps to be set up in advance and solved at once
• Sequenced results can be reviewed step by step

20
. . . Time Type

• Specify the desired number of sequence steps in
  the details of the Environment.
• Enter the value of the load for each step by
  first highlighting the desired step in the
  graphics window.
• The chart in the graphics window displays the
  variation of the load.

21
. . . Time Type

• The worksheet view provides a graphical
  representation of each loads sequence.
• Results of a sequenced simulation can be reviewed
  by highlighting the quantity of interest and
  picking the desired sequence from the graphics
  window.

22
Directional Loads

• For most loads/supports which have an
  orientation, the direction can be defined by
  components in any Coordinate System
• The Coordinate System (CS) has to be defined
  prior to specifying the loading. Only Cartesian
  coordinate systems may be used for
  loading/support orientation.
• In the Details view, change Define By to
  Components. Then, select the appropriate
  Cartesian CS from the pull-down menu.
• Specify x, y, and/or z components, which are
  relative to the selected Coordinate System
• Not all loads/supports support use of CS

23
Acceleration Gravity

• An acceleration can be defined on the system
• Acceleration acts on entire model in length/time2
  units.
• Users sometimes have confusion over notation of
  direction. If acceleration is applied to system
  suddenly, the inertia resists the change in
  acceleration, so the inertial forces are in the
  opposite direction to applied acceleration
• Acceleration can be defined by Components or
  Vector
• Standard Earth Gravity can also be applied as a
  load
• Value applied is 9.80665 m/s2 (in SI units)
• Standard Earth Gravity direction can only be
  defined along one of three World Coordinate
  System axes.
• Since Standard Earth Gravity is defined as an
  acceleration, define the direction as opposite to
  gravitational force, as noted above.

24
Rotational Velocity

• Rotational velocity is another inertial load
  available
• Entire model spins about an axis at a given rate
• Can be defined as a vector, using geometry for
  axis and magnitude of rotational velocity
• Can be defined by components, supplying origin
  and components in World Coordinate System
• Note that location of axis is very important
  since model spins around that axis.
• Default is to input rotational velocity in
  radians per second. Can be changed in Tools gt
  Control Panel gt Miscellaneous gt Angular Velocity
  to revolutions per minute (RPM) instead.

25
Forces and Pressures

• Pressure loading
• Pressures can only be applied to surfaces and
  always act normal to the surface
• Positive value acts into surface (i.e.,
  compressive)negative value acts outward from
  surface (i.e., suction)
• Units of pressure are in force per area
• Force loading
• Forces can be applied on vertices, edges, or
  surfaces.
• The force will be distributed on all entities.
  This means that if a force is applied to two
  identical surfaces, each surface will have half
  of the force applied. Units are
  masslength/time2
• A force is defined via vector and magnitude or by
  components (in user-defined Coordinate System)

26
Bearing Load

• Bearing Load (was called Bolt Load in prior
  releases)
• Bearing Loads are for cylindrical surfaces only.
  Radial component will be distributed on
  compressive side using projected area. Example
  of radial distribution shown below.Axial
  component is distributed evenly on cylinder.
• Use only one bearing load per cylindrical
  surface. If the cylindrical surface is split in
  two, however, be sure to select both halves of
  cylindrical surface when applying this load.
• Load is in units of force
• Bearing load can be defined via vector and
  magnitude or by components (in anyuser
  Coordinate System).

27
Moment Load

• Moment Load
• For solid bodies, a moment can be applied on any
  surface
• If multiple surfaces are selected, the moment
  load gets apportioned about those selected
  surfaces
• A vector and magnitude or components (in
  user-defined Coordinate System) can define the
  moment. The moment acts about the vector using
  the right-hand rule
• For surface bodies, a moment can also be applied
  to a vertex or edge with similar definition via
  vector or components as with a surface-based
  moment
• Units of moment are in Forcelength.

28
Remote Load

• Remote Load
• Allows the user to apply an offset force on a
  surface or edge of a surface body
• The user supplies the origin of the force (using
  vertices, a cylinder, or typing in (x, y, z)
  coordinates). A user-defined Coordinate System
  may be used to reference the location.
• The force can then be defined by vector and
  magnitude or by components (components for
  direction is in Global CS)
• This results in an equivalent force on the
  surface plus a moment caused by the moment arm
  of the offset force
• The force is distributed on the surfacebut
  includes the effect of the momentarm due to the
  offset of the force
• Units are in force (masslength/time2)

29
Supports (General)

• Fixed Support
• Constraints all degrees of freedom on vertex,
  edge, or surface
• For solid bodies, prevents translations in x, y,
  and z
• For surface and line bodies, prevents
  translations and rotations in x, y, and z
• Given Displacement
• Applies known displacement on vertex, edge, or
  surface
• Allows for imposed translational displacement in
  x, y, and z (in user-defined Coordinate System)
• Entering 0 means that the direction is
  constrained.
• Leaving the direction blank means that the entity
  is free to move in that direction

30
Supports (Solid Bodies)

• Frictionless Support
• Applies constraint in normal direction on
  surfaces
• For solid bodies, this support can be used to
  apply a symmetry plane boundary condition since
  symmetry plane is same as normal constraint
• Cylindrical Constraint
• Applied on cylindrical surfaces
• User can specify whether axial, radial, or
  tangential components are constrained
• Suitable for small-deflection (linear) analysis
  only

31
Supports (Solid Bodies)

• Compression Only Support
• Applies a compression-only constraint normal to
  any given surface. This prevents the surface to
  move in the positive normal direction only.
• A way to think of this support is to imagine a
  rigid structure which has the same shape of the
  selected surface. Note that the contacting
  (compressive) areas are not known beforehand.
• Can be used on a cylindrical surface to model a
  (referred to as Pinned Cylinder 7.1)
• Notice the example on the right,where the
  outline of the undeformed cylinder
  is shown. The compressive side
  retains the shapeof the original cylinder, but
  the tensile side is free to deform.
• This requires an iterative (nonlinear) solution.

32
Supports (Line/Surface Bodies)

• Simply Supported
• Can be applied on edge or vertex of surface or
  line bodies
• Prevents all translations but all rotations are
  free
• Fixed Rotation
• Can be applied on surface, edge, or vertex of
  surface or line bodies
• Constrains rotations but translations are free

33
Summary of Supports

• Supports and Contact Regions may both be thought
  of as being boundary conditions.
• Contact Regions provides a flexible boundary
  condition between two existing parts explicitly
  modeled
• Supports provide a rigid boundary condition
  between the modeled part an a rigid, immovable
  part not explicitly modeled
• If Part A, which is of interest, is connected to
  Part B, consider whether both parts need to be
  analyzed (with contact) or whether supports will
  suffice in providing the effect Part B has on
  Part A.
• In other words, is Part B rigid compared to
  Part A? If so, a support can be used and only
  Part A modeled. If not, one may need to model
  both Parts A and B with contact.

34
Thermal Loading

• Temperature causes thermal expansion in the model
• Thermal strains are calculated as
  followswhere a is the thermal expansion
  coefficient (CTE), Tref is the reference
  temperature at which thermal strains are zero, T
  is the applied temperature, and eth is the
  thermal strain.
• Thermal strains do not cause stress by
  themselves. It is the constraint, temperature
  gradient, or CTE mismatch that produce stress.
• CTE is defined in Engineering Data and has
  units of strain per temperature
• The reference temperature is defined in
  theEnvironment branch

35
Thermal Loading

• Thermal loads can be applied on the model
• Any temperature loading can be applied (see
  Chapter 6 on Thermal Analysis for details)
• Simulation will always perform a thermal solution
  first, then use the calculated temperature field
  as input when solving the structural solution.

36
D. Workshop 4.1

• Workshop 4.1 Linear Structural Analysis
• Goal
• A 5 part assembly representing an impeller type
  pump is analyzed with a 100N preload on the belt.

37
E. Solution Options

• Solution options can be set under the Solution
  branch
• The ANSYS database can be saved if SaveANSYS
  db is set
• Useful if you want to open a database in ANSYS
• Two solvers are available in Simulation
• The solver is automatically chosen, although
  someinformative messages may appear after
  solutionletting the user know what solver was
  used. Setdefault behavior under Tools gt
  Options gtSimulation Solution gt Solver Type
• The Direct solver is useful for models
  containingthin surface and line bodies. It is a
  robust solverand handles any situation.
• The Iterative solver is most efficient when
  solvinglarge, bulky solid bodies. It can handle
  large modelswell, although it is less efficient
  for beam/shells.

38
Solution Options

• Weak springs can be added to stabilize model
• If Program Controlled is set, Simulation tries
  to anticipate under-constrained models. If
  noFixed Support is present, it may add weak
  springsand provide an informative message
  letting the userknow that it has done so
• This can be set to On or Off. To set the
  defaultbehavior, go to Tools gt Options gt
  Simulation Solution gt Use Weak Springs.
• In some cases, the user expects the model to be
  inequilibrium and does not want to constrain all
  possible rigid-body modes. Weak springs will
  helpby preventing matrix singularity.
• It is good practice to constrain all possible
  rigid-bodymotion, however.

39
Solution Options

• Informative messages are also present
• The type of analysis is shown, such as Static
  Structural for the cases described in this
  section.
• If a nonlinear solution is required, it will be
  indicated as such. Recall that for some contact
  behavior and compression-only support, the
  solution becomes nonlinear. These type of
  solutions require multiple iterations and take
  longer than linear solutions.
• The solver working directory is where scratch
  files are saved during the solution of the matrix
  equation. By default, the TEMP directory of your
  Windows system environment variable is used,
  although this can be changed in Tools gt Options
  gt Simulation Solution gt Solver Working
  Directory. Sufficient free space must be on
  that partition.
• Any solver messages which appear after solution
  can be checked afterwards under Solver Messages

40
Solving the Model

• To solve the model, request results first
  (covered next) and click on the Solve button on
  the Standard Toolbar
• By default, two processors (if present) will be
  used for parallel processing. To set the number,
  use Tools gt Options gt Simulation Solution gt
  Number of Processors to Use
• Recall that if a Solution Information branch is
  requested, the contents of the Solution Output
  can be displayed.

41
F. Results and Postprocessing

• Various results are available for postprocessing
• Directional and total deformation
• Components, principal, or invariants of stresses
  and strains
• Contact output
• Requires ANSYS Professional and above
• Reaction forces
• In Simulation, results are usually requested
  before solving, but they can be requested
  afterwards, too.
• If you solve a model then request results
  afterwards, click on the Solve button ,
  and the results will be retrieved. A new
  solution is not required if that type of result
  has been requested previously (i.e., total
  deformation was requested previously but now
  direction deformation is added).

42
Plotting Results

• All of the contour and vector plots are usually
  shown on the deformed geometry. Use the Context
  Toolbar to change the scaling or display of
  results to desired settings.

43
Deformation

• The deformation of the model can be plotted
• Total deformation is a scalar quantity
• The x, y, and z components of deformation can be
  requested under Directional. Because there
  isdirection associated with the components, if
  aCoordinate System branch is present, users
  canrequest deformation in a given coordinate
  system.
• For example, it may be easier to interpret
  displacement for a cylindrical geometry in a
  radial direction by using a cylindrical
  coordinate system to display the result.
• Vector plots of deformation are available.Recall
  that wireframe mode is the easiestto view vector
  plots.

44
Deformation

• Deformation results are available for line,
  surface, and solid bodies
• Note that deformation results are associated
  with translational DOF only. Rotations
  associated with the DOF of line and surface
  bodies are not directly viewable
• Because deformation (displacements) are DOF which
  Simulation solves for, the convergence behavior
  is well-behaved when using the Convergence tool
• Vector deformation plots cannot useAlert or
  Convergence tools because they are vector
  quantities (x, y, z) rather than a unique
  quantity (x or y or z). Use Alert or Convergence
  tools on Total or Directional quantities
  instead.
• Total deformation is an invariant, so
  Coordinate Systems cannot be used on this
  result quantity. Also, Vector deformation is
  always shown in the world coordinate system.

45
Stresses and Strains

• Stresses and strains can be viewed
• Strains are actually elastic strains
• Stresses and (elastic) strains aretensors and
  have six components(x, y, z, xy, yz, xz) while
  thermal strains can be considered a vector with
  three components (x, y, z)
• For stresses and strains, components can be
  requested under Normal (x, y, z) and Shear
  (xy, yz, xz). For thermal strains, (x, y, z)
  components are under Thermal.
• Can request in different results coordinate
  systems
• Thermal strains not available with an ANSYS
  Structural license
• Only available for shell and solid bodies. Line
  bodies currently do not report any results except
  for deformation.
• Equivalent Plastic strain output is covered in
  Chapter 11

46
Stress Tools

• Safety Factors can be calculated based on any of
  4 failure theories
• Ductile Theories
• Maximum Equivalent Stress
• Maximum Shear Stress
• Brittle Theories
• Mohr-Coulomb Stress
• Maximum Tensile Stress
• Within each stress tool safety factor, safety
  margin and stress ratio can be plotted
• Note see appendix 4 and the Simulation
  documentation for more details

47
Contact Results

• Contact Results
• Contact results can be requested for selected
  bodies or surfaces which have contact elements.
• Contact elements in ANSYS use the concept
  ofcontact and target surfaces. Only contact
  surfacesreport contact results. MPC-based
  contact, the target surfaces of any contact, and
  edge-based contact do not report results. Line
  bodies do not support contact.
• If asymmetric or auto-asymmetric contact is used,
  then contact results will be reported on the
  contact surfaces only. The target surfaces
  will report zero values, if requested.
• If symmetric contact is used, then contact
  results will be reported on both surfaces. For
  values such as contact pressure, the actual
  contact pressure will be an average of both
  surfaces in contact.
• Contact results are first requested via a
  Contact Tool under the Solution branch.

48
Contact Results

• The user can specify contact output under
  Contact Tool
• The Worksheet view easily allows users to select
  which contact regions will be associated with the
  Contact Tool
• Results on contact or target sides (or both)
  can be selected from the spreadsheet (symmetric
  vs. asymmetric contact)
• Specific contact results chosen from Context
  Toolbar

49
Contact Results

• Types of Contact Results available
• Contact Pressure shows distribution of normal
  contact pressure
• Contact Penetration shows the resulting amount of
  penetration whereas contact Gap shows any gap
  (within pinball radius).
• Sliding Distance is the amount one surface has
  slid with respect to the other. Frictional
  Stress is tangential contact traction due to
  frictional effects.
• Contact Status provides information on whether
  the contact is established (closed state) or not
  touching (open state).
• For the open state, near-field means that it is
  within pinball region, far-field means that it
  is outside of pinball region.

Contour results are plotted with therest of the
model being translucentfor easier viewing.
50
Contact Forces

• If Reactions are requested for Contact Tool,
  forces and moments are reported for the requested
  contact regions
• Under the Worksheet tab, contact forces for all
  requested contact regions will be tabulated
• Under the Geometry tab, symbols will show
  direction of contact forces and moments.

51
Reaction Forces at Supports

• Reaction forces and moments are output for each
  support
• For each support, look under the Details view
  after solution. Reaction forces and moments are
  printed. X, y, and z components are with
  respect to the world coordinate system. Moments
  are reported at the centroid of the support.
• The reaction force for weak springs, if used, is
  under the Environment branch Details view
  after solution. The weak spring reaction forces
  should be small to ensure that the effect of
  weak springs is negligible.

52
Reaction Forces at Supports

• The Worksheet tab for Environment branch has
  a summary of reaction forces and moments
• If a support shares a vertex, edge, or surface
  with another support, contact pair, or load, the
  reported reaction forces may be incorrect. This
  is due to the fact that the underlying mesh will
  have multiple supports and/or loads applied to
  the same nodes. The solution will still be
  valid, but the reported values may not be
  accurate because of this.

53
Fatigue

• If the Fatigue Module add-on license is
  available, additional post-processing involving
  fatigue calculations is possible
• The Fatigue Tool provides stress-based fatigue
  calculations to aid the design engineer with
  evaluating the life of components in the system
• Constant or variable amplitude loading,
  proportional or non-proportional loading is
  possible

Damage Matrix at Critical Location
Contour of Safety Factor
54
G. Workshop 4.2 2D vs 3D Analysis

• Workshop 4.2 Comparing 2D and 3D Structural
  Analysis
• Comparing 2D and 3D structural analyses.
• Shown here are the 3D sector model and the 2D
  axisymmetric model.

Pressure Cap
Retaining Ring