Results Postprocessing

1
Results Postprocessing

• Chapter Eight

2
Chapter Overview

• In this chapter, aspects of reviewing results
  will be covered
• Viewing Results
• Scoping Results
• Exporting Results
• Coordinate Systems Directional Results
• Solution Combinations
• Stress Singularities
• Error Estimation
• Convergence
• The capabilities described in this section are
  applicable to all ANSYS licenses, except when
  noted otherwise

3
A. Viewing Results

• When selecting a results branch, the Context
  toolbar displays ways of viewing results

4
Displacement Scaling

• For structural analyses (static, modal,
  buckling), the deformed shape can be changed
• By default, the scaling is automatically
  exaggerated to visualize the structural response
  more clearly
• The user can change to undeformed or actual
  deformation

5
Legend Controls
6
Display Method

• The Geometry button controls the
  contourdisplay method. Four choices are
  possible

Exterior is the default display option and is
most commonly used. IsoSurfaces is useful to
display regions with the same contour
value. Capped IsoSurfaces will remove regions
of the model where the contour values are above
(or below) a specified value. Slice Planes
allow a user to cut through the model visually.
A capped slice plane is also available, as shown
on the left.
Model shown is from a sample Inventor assembly.
7
Contour Settings

• The Contours button controls the way inwhich
  contours are shown on the model

8
Outline Display

• The Edges button allows the user show
  theundeformed geometry or mesh

9
Slice Planes

• When in Slice Plane viewing mode, slice
  planescan be added and edited
• To add a slice plane, simply select the Draw
  Slice Plane icon, then click-drag with the left
  mouse across the Graphics window. The path
  created will define the slice plane.
• To edit a slice plane, select the Edit Planes
  icon. The defined planes will have a handle in
  the Graphics window.
• Drag the handle to move the slice plane
• Click on one side of the bar to show capped slice
  display
• Select the handle, then hit the Delete key to
  remove plane

10
Min/Max and Probe

• The min/max symbols can be removed by
  selectingthe Maximum and Minimum buttons
• Results can be queried on the model by selecting
  the Probe button
• Left-mouse click to add an annotation of the
  value being queried on the model.
• Use the Label button to select and
  delete unwanted annotations

11
. . . Probe Tool

• The Probe object (previous page) allows users to
  annotate a result at a particular location on a
  contour plot
• The Probe Tool allows you to scope a result
  object to a location and make that result
  parametric
• The Probe tool can be scoped to geometry or
  located using a coordinate system
• The orientation of the result item can be with
  respect to global or local coordinate systems

12
. . . Probe Tool

• Probe Tool example
• Local coordinate system defined as shown
• Probe tool located at local CS
• Stress results (all) requested

Local CS
Probe Tool
13
Animation Controls

• The animation toolbar allows user to play, pause,
  and stop animations
• Note animations are accessed via the tab at the
  bottom of the graphics screen

Note pause feature available during playback
14
Alerts

• Alerts are simple ways of check to see if a
  scalar result quantity satisfies a criterion
• Alerts can be used on most contour results except
  for vector results, Contact Tool results, and
  Shape Finder
• Simply highlight that result branch RMB and
  insert an Alert
• In the Details view, specify the criterion
• In the Outline tree, a green checkmark indicates
  that the criterion is satisfied. A red
  exclamation mark indicates that the criterion
  was not satisfied.

15
Manipulating the Legend

• For exterior contour plots, the legend can be
  manipulated to show result distributions more
  clearly.

Original Contour Legend
Modified Contour Legend
16
Manipulating the Legend

• Capped IsoSurfaces are manipulated by an
  independent controller
• Icons allow isosurface, top or bottom capped
  plots
• The striped areas of the legend show what values
  will not be displayed
• The cap threshold can be controlled via the
  slider or by typing the value directly

Capped/Top/Isosurface Display
Threshold Controls
17
Vector Plots

• Vector plots involve any result quantity with
  direction, such as deformation, principal
  stresses/strains, and heat flux
• Activate vectors for appropriate quantities using
  the vector graphics icon
• Once the vectors are visible their appearance can
  be modified using the vector display controls
  (see next slide for examples)

Vector Length Control
Vector Length Control
Proportional Vectors
Equal Length Vectors
Element Aligned
Grid Aligned
Line Form
Solid Form
18
Vector Plots

• Examples

Solid Form, Grid Aligned
Line Form, Grid Aligned
Proportional Length
Equal Length
19
Multiple Viewports

• Using multiple viewports is especially useful
  forpostprocessing, where more than one
  resultcan be viewed at the same time
• Useful to compare multiple results, such as
  results from different environments or multiple
  mode shapes

20
Default Settings

• Under Tools gt Options gt Simulation Graphics,
  the default graphics settings can be changed.
• This way, each user can make all results for new
  simulations be displayed to his/her preference

21
B. Scoping Results

• Sometimes, limiting the display of results is
  useful when postprocessing
• Scoping automatically scales the legend and only
  shows the applicable surface(s) or part(s),
  making result viewing easier
• Scoping results on edges produces a path plot,
  allowing users to see detailed results along
  selected edges
• Results scoping is very useful for convergence
  controls (discussed later in this chapter)
• When using Contact Tool, Simulation automatically
  scopes contact results to contact regions.
• Results scoping can be performed on any result
  item in the Solution branch for any type of
  geometric quantity

22
Scoping Surface/Part Results

• To scope contour results, simply do either of the
  following
• Select part(s) or surface(s), then request the
  result of interest
• Select the result item, then click on Geometry
  in the Details view. Select the part(s) or
  surface(s), then click on Apply
• When this is performed, the Details view of the
  result item will indicate that results will be
  shown only for the selected items.
• The displayed values will show non-selected
  surfaces/parts as translucent.

23
Scoping Surface/Part Results

• Some examples of scoping results on
  surfaces/parts

24
Scoping Edge Vertex Results

• Results can be scoped to a single edge
• Select a single edge for results scoping
• A path plot of the result mapped on the edge will
  be displayed
• In a similar manner, results can also be scoped
  to a single vertex. No contour results will be
  displayed since only a vertex is present, but the
  value will reported in the Details view for the
  selected vertex

25
Renaming Scoped Results

• For scoped results, it is often useful to
  automatically rename the result branch
• Right-click on the result branch and select
  Rename Based on Definition. The name will
  become more descriptive.

26
C. Exporting Results

• Tabular data from Simulation can be exported to
  Excel for further data manipulation
• To export Worksheet tab information, do the
  following
• Select the branch and click on the Worksheet tab
• Right-click the same branch and select Export
• This can be used for Geometry, Contact,
  Environment, Frequency Finder, Buckling, and
  Harmonic Worksheets
• To export Contour Results
• Right-click on the result branch of interest and
  select Export
• This can be used for any result item of interest
• Node numbers and result quantities will be
  exported
• Exporting large amounts of data can take some CPU
  time

27
Exporting Results

• Usually, for result items, the internal ANSYS
  node number and result quantity will be output as
  shown below.
• To include node locations, change this option
  under Tools menu gt Options gt Simulation Export

28
Exporting Results

• For principal stresses and strains, additional
  information of the orientation needs to be
  included when export to .XLS
• The generated Excel file will have 6 fields
• The first three correspond to the maximum, middle
  and minimum principal quantities (stresses or
  strains).
• The last three correspond to the ANSYS Euler
  angle sequence (CLOCAL command in ANSYS) required
  to produce a coordinate system whose X, Y and
  Z-axis are the directions of maximum, middle and
  minimum principal quantities, respectively. This
  Euler angle sequence is ThetaXY, ThetaYZ and
  ThetaZX and orients the principal coordinate
  system relative to the global system.

29
D. Coordinate Systems

• If coordinate systems are defined, a new item
  will be displayed in the Details view of
  directional results
• As shown below, one can select from defined
  coordinate systems. The selected coordinate
  system will define x-, y-, and z-axes
• Direction Deformation, Normal/Shear
  Stress/Strain, and Directional Heat Flux can use
  coordinate systems
• Principal stress/strain have their own angles
  associated with them
• Other result items are scalars, so there are no
  directions associated with it

30
Coordinate Systems

• For the model shown below, one localcylindrical
  coordinate system is defined
• Note that displaying Deformation in the
  x-direction in the global and local
  coordinatesystems will show different results.
• If the user wants to see what is the
  radialdisplacement at the larger hole, a local
  cylindrical coordinate system allows to visualize
  this type of displacement.

31
E. Solution Combinations

• For ANSYS Professional licenses and above, the
  Solution Combination branch can be added to the
  Model branch to provide combinations of existing
  Environment branches
• Solution combinations are only valid for linear
  static structural analyses
• Linear combinations are only valid if the
  analyses are linear (Chapter 4)
• Thermal-stress and other types of analyses are
  not supported
• The supports must be the same between
  Environments for the results to be valid. Only
  the loading can change to allow for solution
  combinations
• Solution combination calculations are very quick
  and do not require a re-solve

32
Solution Combinations

• To perform solution combinations, do the
  following
• Add a Solution Combination branch. The Worksheet
  view will appear
• In the Worksheet view, add Environments and a
  coefficient (multiplier). The solution
  combination will be the sum of the multiples of
  the various Environments selected.
• Request results from the Context toolbar. These
  results will reflect the sum of the products of
  the selected Environments

33
Solution Combinations

• For example, consider the case below of a sample
  model with two environments

34
F. Stress Singularities

• In most finite-element analyses as the mesh is
  refined one expects to get mathematically more
  precise results.
• Quantities directly solved for (degrees of
  freedom) such as displacements and temperatures,
  converge without problems
• Derived quantities, such as stresses, strains,
  and heat flux, should also converge as the mesh
  is refined, but not as fast or smooth as DOF
• In some cases derived quantities such as stresses
  and heat flux will not converge as the mesh is
  refined. These are situations where these values
  are artificially high

35
Stress Singularities

• In a linear static structural analysis, there are
  several sources which may cause artificially high
  stresses
• Stress singularities
• Geometry discontinuities, such as reentrant
  corners (shown on right)
• Point/edge loads and constraints
• Fixed supports and other constraints which
  prevent Poissons effect
• Fixed supports and other constraints which
  prevent thermal expansion
• In the above situations, refining the mesh at the
  artificially high stress area will keep
  increasing the stresses

Model shown is from a sample Mechanical Desktop
assembly.
36
Stress Singularities

• If the singularity is not in an area of interest
  one can usually scope results only on parts or
  surfaces of interest
• If the singularity is in the area of interest
  there are several ways to obtain more accurate
  stress results
• Stress singularities
• Model geometry with fillets or other details
  which do not cause geometric discontinuities
• Apply loads spread over areas rather than point
  loading
• Overconstraints
• A Fixed Support is an idealization, and modeling
  the constraint properly may be required (possibly
  including the geometry on which the part is
  connected)
• Although the above are some suggestions, these
  usually involve additional effort or more
  nodes/elements, so it is up to the user to review
  the results and understand if and why stresses
  may be artificially high.

37
G. Error Estimation

• You can insert an Error result based on stresses
  (structural), or heat flux (thermal) to help
  identify regions of high error (see example next
  page)
• These regions show where the model would benefit
  from a more refined mesh in order to get a more
  accurate answer
• Regions of high error also indicate where
  refinement will take place if convergence is used

38
. . . Error Estimation

• Error plot shows region where element mesh
  refinement may be necessary.
• Error is plotted in terms of energy.

39
H. Convergence

• As noted earlier, as the mesh is refined, the
  mathematical model becomes more accurate.
  However, there is computational cost associated
  with a finer mesh.
• Obtaining an optimal mesh requires the following
• Having criteria to determine if a mesh is
  adequate
• Investing more elements only where needed
• Performing these tasks manually is cumbersome and
  inexact
• The user would have to manually refine the mesh,
  resolve, and compare results with previous
  solutions.
• Simulation has convergence controls to automate
  adaptive mesh refinement to a user-specified
  level of accuracy

40
Convergence

• To use this feature, simply select a result item
  RMB and insert Convergence
• In the Details of the Convergence branch select
  the max or min value for convergence and
  allowable change (20 default)
• In the Details view of the Solution branch, input
  the max number of refinement loops per solve
• Input a reasonable value, such as 1 to 4, so that
  Simulation will not try to refine the mesh
  indefinitely.

41
Convergence

• Simulation will automatically refine the mesh and
  resolve
• At least two iterations are required (initial
  solution and first refinement loop)
• The Max Refinement Loops is used to specify the
  number of allowable iterations (2 to 4 max loops
  is usually sufficient)
• The mesh will automatically be refined only in
  areas deemed necessary based on error
  approximation techniques
• The convergence information is stored in the
  Convergence branch
• Not converged a red exclamation mark will appear
• Converged a green checkmark will be shown
• The result branches will display only the last
  solution

42
Convergence

• After the solution is complete, one can view the
  results and the last mesh
• Note that the mesh is refined only where needed,
  as shown in the example below
• The Convergence branch shows the trend for each
  refinement loop as well as the values and number
  of nodes and elements in the mesh

43
Convergence Stress Singularities

• As mentioned earlier there are some causes for
  artificially high stresses
• Stress singularities are theoretically infinite
  so Simulations adaptive mesh refinement will be
  affected
• By specifying a reasonable value for the Max
  Refinement Loops, this will allow the user to
  know quickly whether a stress singularity or
  other type of artificially high stress source is
  present

44
Convergence Scoping

• Besides adding details to remove stress
  singularities, one can also converge on scoped
  results
• If the artificially high stress region is not of
  interest, one can scope results on selected
  part(s) or surface(s) and add convergence
  controls to those results only
• This provides the user with control on where to
  perform mesh refinement
• This also allows the user to ignore areas of
  artificially high stresses which are not of
  interest

45
Convergence Scoping Example

• For example, consider the simple part below
• The part below contains geometric discontinuities
  as shown
• For a given set of loading conditions if the user
  knew that the bottom of the part was failing this
  may be the region of interest

Model shown is from a sample Mechanical Desktop
assembly.
46
Convergence Scoping Example
If convergence controls were simply added to the
entire model, the geometric discontinuity would
cause a stress singularity which increases
without bounds. The solution becomes very costly
by including the stress singularity.
On the other hand, convergence controls on scoped
results allows for adaptive refinement only in
user-specified locations, providing the user with
more control over the mesh and the adaptive
solution. In this way, the user can get accurate
stresses on the bottom surface of the part.
47
Results Not Used with Convergence

• Convergence cannot be used on the following
  result quantities
• Any type of vector result
• Contact Tool results
• Frequency Finder stress/strain results
• Buckling stress/strain results
• Harmonic analysis results
• Shape Finder results
• Fatigue Tool graph results

48
Convergence Summary

• Convergence Details
• the percent change is related to the previous
  solution. This is not percent error
• Convergence controls do not compensate for
  inaccurate assumptions
• Convergence controls trigger adaptive mesh
  refinement. Each solution will take longer than
  the previous one
• Scoping results which contain convergence
  controls helps to minimize mesh density by
  isolating the areas of interest

49
I. Workshop 8 Advanced Results Processing

• Workshop 8 Advanced Results Processing
• Goal
• Analyze the high pressure vent assembly shown
  below and then use some of the advanced
  postprocessing features to review the stress and
  deflection results.

50
(No Transcript)