Ansys material analise numéria FEA

Esta é uma pré-visualização de arquivo. Entre para ver o arquivo original

Click to edit Master title style
Click to edit Master subtitle style
Results Postprocessing
Chapter Eight
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
A. Viewing Results
When selecting a results branch, the Context toolbar displays ways of viewing results:
	All of these options except for “Convergence” will be discussed next. “Convergence” is covered in Section C.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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
Model shown is from a sample Pro/ENGINEER assembly.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Display Method
The “Geometry” button controls the contour display 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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Contour Settings
The “Contours” button controls the way in which contours are shown on the model
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Outline Display
The “Edges” button allows the user show the undeformed geometry or mesh
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Min/Max and Probe Tool
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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Animation Controls
The animation toolbar allows user to play, pause, and stop animations
The slider bar allows users to go through frame-by-frame
The “Export Animation File” enables saving animation as AVI 
Animations will generally range from min to max value in a linear fashion. On the other hand, for free vibration and harmonic analysis, the full range will be correctly animated (+/- max value).
Animation speed can be controlled via “View > Animation Speed”
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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 select that result branch and add an Alert
In the Details view, specify the criterion
A minimum or maximum value of that result branch can be used
Input the value which is used for the threshold
In the Outline tree, a green checkmark indicates that the criterion is satisfied. A red exclamation mark indicates that the criterion was not satisfied.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Manipulating the Legend
For exterior contour plots, the legend can be manipulated to show result distributions more clearly.
Select the legend with the left mouse
Drag white bars to change overall min/max values
Out-of-range values are purple (high) and brown (low)
Drag yellow bars to rescale legend
Drag grey bars to change intermediate ranges
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Manipulating the Legend
For Capped IsoSurface plots, the legend has additional features to manipulate the display
The middle long grey bar controls where the cutoff value is for capped plots
The striped areas show what values will not be displayed. To toggle, simple click on the colored areas on either side of the long grey bar
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Manipulating the Legend
The legend may also be changed by selecting the values and directly inputting a numerical value
Select the contour value, type in a new value, and [Enter]
To rescale internal bands, select white bars and move them. Internal bands automatically get rescaled evenly 
For example, when comparing two results, one may want to change the legend to be the same for both
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Vector Plots
Vector plots involve any vector 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)
Proportional Vectors
Equal Length Vectors
Vector Length Control
Element Aligned
Grid Aligned
Line Form
Solid Form
Vector Length Control
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Vector Plots
Examples
Solid Form, Grid Aligned
Line Form, Grid Aligned
Proportional Length
Equal Length
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
B. Scoping Results
Sometimes, limiting the display
of results is useful when postprocessing
Although one can rescale the legend to get a better idea of the result distribution on a certain part or surface, results 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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Scoping Surface/Part Results
Some examples of scoping results on surfaces/parts:
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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”
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
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.
Vector plots show the direction, so they cannot use coordinate systems.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
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). Nonlinear results should not be added together in a linear fashion, although Contact Tool results can be added.
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 does not require a re-solve.
Sheet1
		ANSYS License		Availability
		DesignSpace Entra
		DesignSpace
		Professional		x
		Structural		x
		Mechanical/Multiphysics		x
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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
Sheet1
		ANSYS License		Availability
		DesignSpace Entra
		DesignSpace
		Professional		x
		Structural		x
		Mechanical/Multiphysics		x
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Solution Combinations
For example, consider the case below of a sample model with two environments
Sheet1
		ANSYS License		Availability
		DesignSpace Entra
		DesignSpace
		Professional		x
		Structural		x
		Mechanical/Multiphysics		x
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Solution Combinations
Use of solution combinations allows the user to solve different environments, thereby considering the effect of different loads separately.
By using the Solution Combination branch, a linear combination of solutions can be solved for very quickly without having to perform another separate solution.
Multiple
Solution Combination branches may be added, as needed.
Sheet1
		ANSYS License		Availability
		DesignSpace Entra
		DesignSpace
		Professional		x
		Structural		x
		Mechanical/Multiphysics		x
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
F. Stress Singularities
In any finite-element analysis, one seeks to balance accuracy and computational cost. 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 since these are derived from the DOF solution
In some cases, however, 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. This section will discuss situations where derived solution quantities are artificially high.
In thermal analyses, since temperature is the main quantity of interest, the discussion in this section will focus on stresses instead, not heat flux.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Stress Singularities
In a linear static structural analysis, there are several sources which may cause artificially high stresses, two common ones which are listed below:
Stress singularities
Geometry discontinuities, such as reentrant corners (shown on right)
Point/edge loads and constraints
Overconstraints
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
Model shown is from a sample Mechanical Desktop assembly.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Stress Singularities
If the area of artificially high stresses is not an area of interest, one can usually scope results only on part(s) or surface(s) of interest instead
If the area of artificially high stresses is 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 since some form of these (albeit small) would exist in the actual system
Point loads and constraints should only be used on line bodies. For solid bodies, every load/constraint has a finite area on which it is applied, so these should be applied on areas rather than vertices
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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
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.
More information on error estimation is available in section 19.7 of the ANSYS Theory Reference.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
. . . Error Estimation
Error plot shows region where element mesh refinement may be necessary.
Error is plotted in terms of energy.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Convergence
To use this feature, simply select a result branch and select the “Convergence” button on the Context toolbar
A Convergence branch will appear below the result branch
In the Details view of the Convergence branch, select whether the max or min value will be converged upon and input the allowable change (as a percentage)
For “Type,” “Minimum” is available since some result quantities (e.g., directional deformation or minimum principal stress) may have negative values
For allowable change, default is 20%. However, 5% for displacement and temperatures and 10% for other quantities is a good starting point.
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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Convergence
After this is completed, when solving, Simulation will automatically refine the mesh and resolve
At least two iterations are required (initial solution and first refinement loop)
The “Max Refinement Loops” in the Solution branch details allows the user to set the max number of loops per solve to prevent Simulation from excessive refinement. Usually, 2 to 4 max loops should be more than enough. Default is 1 loop per solve.
The mesh will automatically be refined only in areas deemed necessary, based on error approximation techniques
The convergence results will be stored for review in the “Convergence” branch
If not converged within the specified percentage, a red exclamation mark will appear.
If converged within the limits, a green checkmark will be shown
The result branches will display only the last solution
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Convergence & Stress Singularities
As noted in the previous chapter, there are some causes for artificially high stresses
Stress singularities are theoretically infinite stress, so Simulation’s adaptive mesh refinement will indicate this
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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Convergence & Scoping 
Besides adding details to get rid of 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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Convergence & Scoping Example
For example, consider the simple part below.
The part below has some geometric discontinuities, where smoothers were not modeled to reduce model complexity
For a given set of loading conditions, if the user knew that the bottom of the part was failing, this may be a region of interest the user would focus on.
Model shown is from a sample Mechanical Desktop assembly.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Convergence & Scoping Example
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.
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.
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … 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
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
 … Convergence Summary
Using convergence controls helps to achieve a given level of accuracy.
Note that the “percent change” is related to the previous solution. This is not “percent error” since Simulation does not know beforehand what the ‘actual answer’ is.
Convergence controls provides a way to get an accurate answer based on the mathematical model. It does not compensate for inaccurate assumptions, however! Hence, if loads, supports, material properties, etc. are wrong, the solution will still be inaccurate.
Because use of convergence controls results in adaptive mesh refinement, each new iteration will take longer than the previous solution
Although adaptive meshing will put more nodes and elements only where needed, the mesh density will still increase
Scoping results helps to minimize mesh density by explicitly indicating to Simulation the areas of interest
March 29, 2005
Inventory #002215
8-*
ANSYS Workbench – Simulation
Training Manual
Results Postprocessing
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. 
 I. Workshop 8