1. Results Postprocessing
Chapter Eight
Results Postprocessing

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
August 26, 2005
Inventory #002265
8-2

3. A. Viewing Results
When selecting a results branch, the Context toolbar displays ways of viewing results:
Min/Max
Displacement Scaling
Display Method
Contour Settings
Outline Display
Slice Planes
Probe Tool
Legend Settings
Animation Controls
Export AVI
Vector Display Controls
August 26, 2005
Inventory #002265
8-3

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
No Displacement Scaling
Automatic Displacement Scaling
August 26, 2005
Inventory #002265
8-4

5. …Legend Controls Color/Position/Size Selectors Auto Select Reset
Enter maximum/minimum legend value or allow auto selection
Contour number selector
Auto Select Reset
Enter maximum/minimum range for contours
August 26, 2005
Inventory #002265
8-5

6. … Display Method
The “Geometry” button controls the contour display method. Four choices are possible:
Slice Planes
IsoSurfaces
Exterior
Capped IsoSurfaces
“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.
August 26, 2005
Inventory #002265
8-6
Model shown is from a sample Inventor assembly.

7. … Contour Settings
The “Contours” button controls the way in which contours are shown on the model
Solid Fill
Contour Bands
Smooth Contours
Isolines
August 26, 2005
Inventory #002265
8-7

8. Show Undeformed Wireframe
… Outline Display
The “Edges” button allows the user show the undeformed geometry or mesh
No Wireframe
Show Undeformed Wireframe
Show Undeformed Model
Show Elements
August 26, 2005
Inventory #002265
8-8

9. … Slice Planes
When in Slice Plane viewing mode, slice planes can 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
Move a slice plane by dragging handle
Handles of 3 defined slice planes
Click on one side of bar to cap view
August 26, 2005
Inventory #002265
8-9

10. … Min/Max and Probe
The min/max symbols can be removed by selecting the “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
August 26, 2005
Inventory #002265
8-10

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
August 26, 2005
Inventory #002265
8-11

12. . . . Probe Tool Probe Tool example:
Local coordinate system defined as shown
Probe tool located at local CS
Stress results (all) requested
August 26, 2005
Inventory #002265
8-12
Local CS
Probe Tool

13. Export video (avi) file Control resolution and speed
… 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
Start/Stop/Pause
Distributed animation interpolates results while results sets animates only solution points.
Export video (avi) file
Control resolution and speed
Note: pause feature available during playback
August 26, 2005
Inventory #002265
8-13

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.
August 26, 2005
Inventory #002265
8-14

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
August 26, 2005
Inventory #002265
8-15

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
August 26, 2005
Inventory #002265
8-16

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
Grid Aligned
Element Aligned
Line Form
Solid Form
August 26, 2005
Inventory #002265
8-17

18. … Vector Plots Examples Solid Form, Grid Aligned
Line Form, Grid Aligned
Proportional Length
Equal Length
August 26, 2005
Inventory #002265
8-18

19. … Multiple Viewports
Using multiple viewports is especially useful for postprocessing, where more than one result can be viewed at the same time
Useful to compare multiple results, such as results from different environments or multiple mode shapes
August 26, 2005
Inventory #002265
8-19

20. … Default Settings
Under “Tools > Options… > 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
August 26, 2005
Inventory #002265
8-20

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
August 26, 2005
Inventory #002265
8-21

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.
August 26, 2005
Inventory #002265
8-22

23. … Scoping Surface/Part Results
Some examples of scoping results on surfaces/parts:
Scoping results on a single part
Stress results on selected surfaces
Vector Principal Stresses on single part
August 26, 2005
Inventory #002265
8-23

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
August 26, 2005
Inventory #002265
8-24

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.
The result branch name is now more descriptive, indicating it is a scoped result on a given edge.
Renaming result branches is also useful for directional results, as it will change the name to the direction of the stress or deformation or heat flux.
August 26, 2005
Inventory #002265
8-25

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
August 26, 2005
Inventory #002265
8-26

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 > Options… > Simulation: Export”
August 26, 2005
Inventory #002265
8-27

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.
August 26, 2005
Inventory #002265
8-28

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
August 26, 2005
Inventory #002265
8-29

30. … Coordinate Systems
For the model shown below, one local cylindrical coordinate system is defined
Note that displaying Deformation in the x- direction in the global and local coordinate systems will show different results.
If the user wants to see what is the radial displacement at the larger hole, a local cylindrical coordinate system allows to visualize this type of displacement.
Deformation in Global X-Direction
Deformation in Local Cylindrical X-Direction
August 26, 2005
Inventory #002265
8-30

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
August 26, 2005
Inventory #002265
8-31

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
August 26, 2005
Inventory #002265
8-32

33. … Solution Combinations
For example, consider the case below of a sample model with two environments
“Environment”
“Environment 3”
Solution Combination Results
August 26, 2005
Inventory #002265
8-33

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
August 26, 2005
Inventory #002265
8-34

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 Poisson’s 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
August 26, 2005
Inventory #002265
8-35
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.
August 26, 2005
Inventory #002265
8-36

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
August 26, 2005
Inventory #002265
8-37

38. . . . Error Estimation
Error plot shows region where element mesh refinement may be necessary.
Error is plotted in terms of energy.
August 26, 2005
Inventory #002265
8-38

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
August 26, 2005
Inventory #002265
8-39

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.
August 26, 2005
Inventory #002265
8-40

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
August 26, 2005
Inventory #002265
8-41

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
August 26, 2005
Inventory #002265
8-42

43. … Convergence & Stress Singularities
As mentioned earlier there are some causes for artificially high stresses
Stress singularities are theoretically infinite so Simulation’s 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
In this case, it is clear that the stresses will increase without bound.
By examining the model, it was clear that a stress singularity existed, which explains why the stresses do not converge as it normally would.
August 26, 2005
Inventory #002265
8-43

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
August 26, 2005
Inventory #002265
8-44

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
Possible stress singularity
Region of interest
August 26, 2005
Inventory #002265
8-45
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.
August 26, 2005
Inventory #002265
8-46

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
August 26, 2005
Inventory #002265
8-47

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
August 26, 2005
Inventory #002265
8-48

49. I. 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.
August 26, 2005
Inventory #002265
8-49